Preface
Fundamental Geometrical
Principles 1
Fundamental Principles of
NC Programming 2
Positional Data 3
Motion commands 4
Path Action 5
Frames 6
Feedrate Control and
Spindle Motion 7
Tool offsets 8
Special functions 9
Arithmetic Parameters and
Program Jumps 10
Program section repetition 11
Tables 12
Appendix A
SINUMERIK
SINUMERIK
840D sl/840Di sl/840D/840Di/810D
Fundamentals
Programming Manual
11/2006
6FC5398-1BP10-2BA0
Valid for
Control
SINUMERIK 840D sl/840DE sl
SINUMERIK 840Di sl/840DiE sl
SINUMERIK 840D powerline/840DE powerline
SINUMERIK 840Di powerline/840DiE powerline
SINUMERIK 810D powerline/810DE powerline
Software Version
NCU Systemsoftware für 840D sl/840DE sl 1.4
NCU Systemsoftware für 840Di sl/DiE sl 1.0
NCU Systemsoftware für 840D/840DE 7.4
NCU Systemsoftware für 840Di/840DiE 3.3
NCU Systemsoftware für 810D/810DE 7.4
Safety Guidelines
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent
damage to property. The notices referring to your personal safety are highlighted in the manual by a safety alert
symbol, notices referring only to property damage have no safety alert symbol. These notices shown below are
graded according to the degree of danger.
Danger
indicates that death or severe personal injury will result if proper precautions are not taken.
Warning
indicates that death or severe personal injury may result if proper precautions are not taken.
Caution
with a safety alert symbol, indicates that minor personal injury can result if proper precautions are not taken.
Caution
without a safety alert symbol, indicates that property damage can result if proper precautions are not taken.
Notice
indicates that an unintended result or situation can occur if the corresponding information is not taken into
account.
If more than one degree of danger is present, the warning notice representing the highest degree of danger will
be used. A notice warning of injury to persons with a safety alert symbol may also include a warning relating to
property damage.
Qualified Personnel
The device/system may only be set up and used in conjunction with this documentation. Commissioning and
operation of a device/system may only be performed by qualified personnel. Within the context of the safety notes
in this documentation qualified persons are defined as persons who are authorized to commission, ground and
label devices, systems and circuits in accordance with established safety practices and standards.
Prescribed Usage
Note the following:
Warning
This device may only be used for the applications described in the catalog or the technical description and only in
connection with devices or components from other manufacturers which have been approved or recommended by
Siemens. Correct, reliable operation of the product requires proper transport, storage, positioning and assembly
as well as careful operation and maintenance.
Trademarks
All names identified by ® are registered trademarks of the Siemens AG. The remaining trademarks in this
publication may be trademarks whose use by third parties for their own purposes could violate the rights of the
owner.
Disclaimer of Liability
We have reviewed the contents of this publication to ensure consistency with the hardware and software
described. Since variance cannot be precluded entirely, we cannot guarantee full consistency. However, the
information in this publication is reviewed regularly and any necessary corrections are included in subsequent
editions.
Siemens AG
Automation and Drives
Postfach 48 48
90437 NÜRNBERG
GERMANY
Order No.: 6FC5398-1BP10-2BA0
Ⓟ 11/2006
Copyright © Siemens AG 2006.
Technical data subject to change
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 3
Preface
SINUMERIK® Documentation
The SINUMERIK documentation is organized in 3 parts:
• General Documentation
• User Documentation
• Manufacturer/service documentation
An overview of publications (updated monthly) indicating the language versions available
can be found on the Internet at:
http://www.siemens.com/motioncontrol
Select the menu items "Support" → "Technical Documentation" → "Overview of
Publications".
The Internet version of DOConCD (DOConWEB) is available at:
http://www.automation.siemens.com/doconweb
Information about training courses and FAQs (Frequently Asked Questions) can be found
at the following website:
http://www.siemens.com/motioncontrol under menu option "Support"
Target group
This publication is intended for:
• Programmers
• Project engineers
Benefits
With the programming manual, the target group can develop, write, test, and debug
programs and software user interfaces.
Preface
Fundamentals
4 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Standard scope
This Programming Guide describes the functionality afforded by standard functions.
Extensions or changes made by the machine tool manufacturer are documented by the
machine tool manufacturer.
Other functions not described in this documentation might be executable in the control. This
does not, however, represent an obligation to supply such functions with a new control or
when servicing.
Further, for the sake of simplicity, this documentation does not contain all detailed
information about all types of the product and cannot cover every conceivable case of
installation, operation or maintenance.
Technical Support
If you have any technical questions, please contact our hotline:
Europe/Africa Asia/Australia America
Phone +49 180 5050 222 +86 1064 719 990 +1 423 262 2522
Fax +49 180 5050 223 +86 1064 747 474 +1 423 262 2289
Internet http://www.siemens.com/automation/support-request
E-Mail mailto:adsupport@siemens.com
Note
Country telephone numbers for technical support are provided under the following Internet
address:
Enter http://www.siemens.com/automation/service&support
Questions about the manual
If you have any queries (suggestions, corrections) in relation to this documentation, please
fax or e-mail us:
Fax: +49 (0) 9131 / 98 - 63315
E-mail: mailto:docu.motioncontrol@siemens.com
Fax form: See the reply form at the end of this publication
SINUMERIK Internet address
http://www.siemens.com/sinumerik
Preface
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 5
EC declaration of conformity
The EC Declaration of Conformity for the EMC Directive can be found/obtained from:
• the internet:
http://www.ad.siemens.de/csinfo
under product/order no. 15257461
• the relevant branch office of the A&D MC group of Siemens AG.
Export version
The following functions are not available in the export version:
Function 810DE 840DE sl 840DE 840DiE sl 840DiE
Helical interpolation 2D+6
(Basic version, no options)
− − − − −
Milling machining package − − − − −
Five axis machining package − − − − −
Handling transformation package − − − − −
Multi-axis interpolation (> 4 interpolating axes) − − − − −
OA NCK compile cycles − − − − −
Clearance control 1D/3D in position-control cycle 1) − − − − −
Synchronized actions 1)
(Basic version, no options)
# # # # #
Master-value coupling and curve-table interpolation # # # # #
Sag compensation, multi-dimensional # # # # #
Synchronized actions, stage 2 1) − − # − #
Electronic gear 1) − − # − #
Electronic transfer − − # − #
# Restricted functionality
- Function not available
1) The restricted functions for the SINUMERIK 810DE powerline / SINUMERIK 840DE sl/
SINUMERIK 840DE powerline/SINUMERIK 840DiE sl/SINUMERIK 840DiE powerline export versions impose a limit
of "max. 4 interpolating axes".
Preface
Fundamentals
6 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Description
Fundamentals
This Programming Guide "Fundamentals" is intended for use by skilled machine operators
with the appropriate expertise in drilling, milling and turning operations. Simple programming
examples are used to explain the commands and statements which are also defined
according to DIN 66025.
Job planning
The Programming Guide "Job Planning" is intended for use by technicians with in-depth,
comprehensive programming knowledge. By virtue of a special programming language, the
SINUMERIK 840D sl/840Di sl/840D/840Di/810D control enables the user to program
complex workpiece programs (e.g., for free-form surfaces, channel coordination, etc.) and
greatly facilitates the programming of complicated operations.
The commands and statements described in this Programming Guide are not specific to one
particular technology.
They can be used for a variety of tasks, such as
• Turning, milling and grinding
• Cyclical machines (packaging, woodworking)
• Laser power controls.
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 7
Table of contents
Preface ...................................................................................................................................................... 3
1 Fundamental Geometrical Principles ....................................................................................................... 13
1.1 Description of workpiece points ...................................................................................................13
1.1.1 Workpiece coordinate systems....................................................................................................13
1.1.2 Definition of workpiece positions..................................................................................................14
1.1.3 Polar coordinates .........................................................................................................................17
1.1.4 Absolute dimensions....................................................................................................................17
1.1.5 Incremental dimension.................................................................................................................19
1.1.6 Plane designations.......................................................................................................................21
1.2 Position of zero points..................................................................................................................22
1.3 Position of coordinate systems ....................................................................................................24
1.3.1 Overview of various coordinate systems .....................................................................................24
1.3.2 Machine coordinate system .........................................................................................................25
1.3.3 Basic coordinate system ..............................................................................................................28
1.3.4 Workpiece coordinate system......................................................................................................30
1.3.5 Frame system ..............................................................................................................................31
1.3.6 Assignment of workpiece coordinate system to machine axes ...................................................33
1.3.7 Current workpiece coordinate system .........................................................................................34
1.4 Axes .............................................................................................................................................34
1.4.1 Main axes/Geometry axes ...........................................................................................................36
1.4.2 Special axes.................................................................................................................................37
1.4.3 Main spindle, master spindle .......................................................................................................37
1.4.4 Machine axes...............................................................................................................................37
1.4.5 Channel axes ...............................................................................................................................38
1.4.6 Path axes .....................................................................................................................................38
1.4.7 Positioning axes...........................................................................................................................38
1.4.8 Synchronized axes.......................................................................................................................39
1.4.9 Command axes............................................................................................................................40
1.4.10 PLC axes......................................................................................................................................40
1.4.11 Link axes......................................................................................................................................40
1.4.12 Lead link axes ..............................................................................................................................42
1.5 Coordinate systems and workpiece machining ...........................................................................44
2 Fundamental Principles of NC Programming........................................................................................... 47
2.1 Structure and contents of an NC program ...................................................................................47
2.2 Language elements of the programming language .....................................................................49
2.3 Programming a sample workpiece...............................................................................................69
2.4 First programming example for milling application ......................................................................70
2.5 Second programming example for milling application .................................................................71
2.6 Programming example for turning application .............................................................................74
Table of contents
Fundamentals
8 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3 Positional Data......................................................................................................................................... 77
3.1 General notes.............................................................................................................................. 77
3.1.1 Program dimensions ................................................................................................................... 77
3.2 Absolute/relative dimensions ...................................................................................................... 78
3.2.1 Absolute dimension (G90, X=AC)............................................................................................... 78
3.2.2 Incremental dimensions (G91, X=IC).......................................................................................... 82
3.3 Absolute dimension for rotary axes (DC, ACP, ACN)................................................................. 86
3.4 Dimensions inch/metric, (G70/G700, G71/G710) ....................................................................... 88
3.5 Special turning functions............................................................................................................. 91
3.5.1 Dimensions for radius, diameter in the channel (DIAMON/OF, DIAM90)................................... 91
3.5.2 Position of workpiece .................................................................................................................. 96
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA ........................................... 98
3.7 Selection of working plane (G17 to G19) .................................................................................. 104
3.8 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)......................................... 108
3.9 Working area limitation in WCS/SZS (WALCS0 ... WALCS10)................................................ 111
3.10 Reference point approach (G74) .............................................................................................. 114
4 Motion commands ................................................................................................................................. 115
4.1 General notes............................................................................................................................ 115
4.2 Travel commands with polar coordinates, polar angle, polar radius ........................................ 118
4.2.1 Defining the pole (G110, G111, G112) ..................................................................................... 118
4.2.2 Traversing commands with polar coordinates, (G0, G1, G2, G3 AP=..., RP=...) ..................... 121
4.3 Rapid traverse movement (G0, RTLION, RTLIOF) .................................................................. 125
4.4 Linear interpolation (G1) ........................................................................................................... 129
4.5 Circular interpolation types, (G2/G3, CIP, CT).......................................................................... 131
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...) ....................... 135
4.7 Circular interpolation with radius and end point (G2/G3, CR)................................................... 139
4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)........................................ 141
4.9 Circular interpolation with polar coordinates (G2/G3, AP=, RP=)............................................. 143
4.10 Circular interpolation with intermediate and end points (CIP)................................................... 145
4.11 Circular interpolation with tangential transition (CT) ................................................................. 147
4.12 Helical interpolation (G2/G3, TURN=)....................................................................................... 150
4.13 Involute interpolation (INVCW, INVCCW)................................................................................. 155
4.14 Contour definitions .................................................................................................................... 159
4.14.1 Straight line with angle (X2... ANG...) ....................................................................................... 159
4.14.2 Two straight lines (ANG1, X3... Z3... ANG2) ............................................................................ 160
4.14.3 Three straight lines (ANG1, X3... Z3... ANG2, X4... Z4...) ........................................................ 161
4.14.4 End point programming with angle ........................................................................................... 163
4.15 Thread cutting with constant lead (G33) ................................................................................... 164
4.15.1 Programmable run-in and run-out paths (DITS, DITE) ............................................................. 171
4.16 Linear progressive/degressive thread pitch change (G34, G35) .............................................. 173
4.17 Tapping without compensating chuck (G331, G332)................................................................ 175
Table of contents
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 9
4.18 Tapping with compensating chuck (G63) ..................................................................................179
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)..............................................181
4.19.1 Retraction for thread cutting (LFOF, LFON, LIFTFAST, DILF, ALF) .........................................181
4.19.2 Lifting on retraction (LFTXT, LFWP, LFPOS, POLF, POLFMASK; POLFMLIN).......................183
4.20 Approaching a fixed point (G75) ................................................................................................186
4.21 Travel to fixed stop (FXS, FXST, FXSW) ..................................................................................188
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)....................................................193
5 Path Action ............................................................................................................................................ 199
5.1 General notes.............................................................................................................................199
5.1.1 Programming path travel behavior.............................................................................................199
5.2 Exact stop (G60, G9, G601, G602, G603).................................................................................202
5.3 Continuous-path mode (G64, G641, G642, G643, G644).........................................................205
5.4 Acceleration behavior ................................................................................................................215
5.4.1 Acceleration response, BRISK, SOFT, DRIVE..........................................................................215
5.4.2 Influence of acceleration on following axes (VELOLIMA, ACCLIMA, JERKLIMA)....................217
5.4.3 Technology G group (DYNNORM, DYNPOS, DYNROUGH, DYNSEMIFIN, DYNFINISH)......219
5.5 Smoothing the path velocity.......................................................................................................220
5.6 Traversing with feedforward control, FFWON, FFWOF.............................................................222
5.7 Contour accuracy, CPRECON, CPRECOF ...............................................................................223
5.8 Dwell time, delay (G4, WRTPR) ................................................................................................224
5.9 Internal preprocessing stop........................................................................................................225
6 Frames ................................................................................................................................................ 227
6.1 General ......................................................................................................................................227
6.2 Frame instructions .....................................................................................................................229
6.3 Programmable zero offset..........................................................................................................232
6.3.1 Zero offset (TRANS, ATRANS)..................................................................................................232
6.3.2 Axial zero offset (G58, G59) ......................................................................................................237
6.4 Programmable rotation (ROT, AROT, RPL) ..............................................................................239
6.5 Programmable frame rotations with solid angles (ROTS, AROTS, CROTS) ............................251
6.6 Programmable scale factor (SCALE, ASCALE) ........................................................................252
6.7 Programmable mirroring (MIRROR, AMIRROR) .......................................................................256
6.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT).......................261
6.9 Deselect frame (G53, G153, SUPA, G500) ...............................................................................264
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF, CORROF) ..............................265
7 Feedrate Control and Spindle Motion .................................................................................................... 269
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)...............................................................269
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC) ...............................278
7.3 Position-controlled spindle operation (SPCON, SPCOF) ..........................................................281
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)...........................................................282
Table of contents
Fundamentals
10 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF) .................................. 290
7.6 Percentage feedrate override (OVR, OVRA)............................................................................ 293
7.7 Feedrate with handwheel override (FD, FDA) .......................................................................... 294
7.8 Percentage acceleration override (ACC option) ....................................................................... 298
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN)..................................... 300
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5).................................................. 302
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])................. 306
7.12 Constant grinding wheel peripheral speed (GWPSON, GWPSOF).......................................... 312
7.13 Programmable spindle speed limitation (G25, G26)................................................................. 313
7.14 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=.., SRA=..).................... 314
7.15 Blockwise feed (FB...) ............................................................................................................... 317
8 Tool offsets ............................................................................................................................................ 319
8.1 General notes............................................................................................................................ 319
8.1.1 Tool offsets................................................................................................................................ 319
8.1.2 Tool offsets in the control's offset memory ............................................................................... 320
8.2 List of tool types ........................................................................................................................ 324
8.3 Tool selection/tool call T............................................................................................................ 331
8.3.1 Tool change with T commands (turning)................................................................................... 331
8.3.2 Tool change with M06 (mill) ...................................................................................................... 332
8.4 Tool offset D.............................................................................................................................. 335
8.5 Tool selection T with tool management .................................................................................... 337
8.5.1 Turning machine with circular magazine (T selection).............................................................. 339
8.5.2 Milling machine with chain magazine (T selection)................................................................... 340
8.6 Tool offset call D with tool management ................................................................................... 341
8.6.1 Turning machine with circular magazine (D call) ...................................................................... 341
8.6.2 Milling machine with chain magazine (D call) ........................................................................... 342
8.7 Activating the active tool offset immediately ............................................................................. 343
8.8 Tool radius compensation (G40, G41, G42)............................................................................. 343
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)....................................... 355
8.10 Compensation at the outside corners (G450, G451) ................................................................ 362
8.11 Smooth approach and retraction............................................................................................... 367
8.11.1 Approach and retraction (G140 to G143, G147, G148, G247, G248, G347, G348, G340,
G341) ........................................................................................................................................ 367
8.11.2 Approach and retraction with enhanced retraction strategies (G460, G461, G462)................. 378
8.12 Collision monitoring (CDON, CDOF, CDOF2) .......................................................................... 382
8.13 2D tool compensation (CUT2D, CUT2DF)................................................................................ 386
8.14 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR)................. 389
8.15 Grinding-specific tool monitoring in parts programs (TMON, TMOF) ....................................... 392
8.16 Additive offsets.......................................................................................................................... 394
8.16.1 Select offsets (via DL numbers)................................................................................................395
8.16.2 Specify wear and setup values ($TC_SCPxy[t,d], $TC_ECPxy[t,d]) ........................................ 396
Table of contents
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 11
8.16.3 Delete additive offsets (DELDL).................................................................................................397
8.17 Special handling of tool offsets ..................................................................................................398
8.17.1 Mirroring of tool lengths .............................................................................................................400
8.17.2 Wear sign evaluation .................................................................................................................401
8.17.3 Coordinate system of the active machining operation
(TOWSTD/TOWMCS/TOWWCS/TOWBCS/TOWTCS/TOWKCS) ...........................................402
8.17.4 Tool length and plane change....................................................................................................405
8.18 Tools with a relevant cutting edge length ..................................................................................406
9 Special functions.................................................................................................................................... 409
9.1 Auxiliary function outputs ...........................................................................................................409
9.1.1 M functions.................................................................................................................................413
9.1.2 H functions .................................................................................................................................415
10 Arithmetic Parameters and Program Jumps .......................................................................................... 417
10.1 Arithmetic parameter (R)............................................................................................................417
10.2 Unconditional program jumps ....................................................................................................419
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC) .......................................421
11 Program section repetition..................................................................................................................... 425
11.1 Program section repetition.........................................................................................................425
12 Tables.................................................................................................................................................... 431
12.1 List of statements.......................................................................................................................431
12.2 List of addresses........................................................................................................................471
12.3 List of G functions/preparatory functions ...................................................................................479
12.4 List of predefined subprograms .................................................................................................494
12.4.1 Predefined subroutine calls........................................................................................................494
12.4.2 Predefined subroutine calls in motion-synchronous actions......................................................509
12.4.3 Predefined functions ..................................................................................................................510
12.4.4 Data types ..................................................................................................................................516
A Appendix................................................................................................................................................ 517
A.1 List of abbreviations ...................................................................................................................518
A.2 List of abbreviations ...................................................................................................................523
A.2.1 Correction sheet - fax template..................................................................................................523
A.2.2 Overview ....................................................................................................................................525
Glossary ................................................................................................................................................ 527
Index...................................................................................................................................................... 551
Table of contents
Fundamentals
12 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 13
Fundamental Geometrical Principles 1
1.1 Description of workpiece points
1.1.1 Workpiece coordinate systems
In order for the machine or control to operate with the specified positions, these data must be
entered in a reference system that corresponds to the direction of motion of the axis slides. A
coordinate system with the axes X, Y and Z is used for this purpose.
Milling:
;
;
<
<
=
=
r
r
r
:
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
14 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Turning:
=
=
;
;
<
r
r
r
:
<
DIN 66217 stipulates that machine tools must use right-handed, rectangular (Cartesian)
coordinate systems.
The workpiece zero (W) is the origin of the workpiece coordinate system. Sometimes it is
advisable or even necessary to work with negative positional data. Positions to the left of the
origin are prefixed by a negative sign (–).
1.1.2 Definition of workpiece positions
To specify a position, imagine that a ruler is placed along the coordinate axes. You can now
describe every point in the coordinate system by specifying the direction (X, Y and Z) and
three numerical values. The workpiece zero always has the coordinates X0, Y0, and Z0.
The infeed depth must also be described in milling operations.
One plane is sufficient to describe the contour on a lathe.
Workpiece positions in the working area
For the sake of simplicity, we will only use one plane of the coordinate system in this
example, i.e., the X/Y plane. Points P1 to P4 then have the following coordinates:
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 15
;
;
<
<
3
3
3
3
P1 corresponds to X100 Y50
P2 corresponds to X-50 Y100
P3 corresponds to X-105 Y-115
P4 corresponds to X70 Y-75
=
;
3
3 3
3
The workpiece positions are required only in one plane for turning.
Points P1 to P4 are defined by the following coordinates:
P1 corresponds to X25 Z-7.5
P2 corresponds to X40 Z-15
P3 corresponds to X40 Z-25
P4 corresponds to X60 Z-35
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
16 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning positions
Points P1 and P2 are defined by the following coordinates:
;
3
<
;
3
3
3
3
=
P1 corresponds to X-20 Y-20 Z23
P2 corresponds to X13 Y-13 Z27
Example:Positions for milling
To state the infeed depth, we need to specify a numerical value for the third coordinate
(Z in this case).
3
3
3
3
3
3
<
=
<
;
Points P1 to P3 are defined by the following coordinates:
P1 corresponds to X10 Y45 Z-5
P2 corresponds to X30 Y60 Z-20
P3 corresponds to X45 Y20 Z-15
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 17
1.1.3 Polar coordinates
The method used to date to specify points in the coordinate system is known as the
"Cartesian coordinate" method.
However, there is another way to specify coordinates, i.e., as so-called "polar coordinates".
The polar coordinate method is useful only if a workpiece or part of a workpiece has radius
and angle measurements. The point, on which the measurements are based, is called the
"pole".
Example of polar data
The points P1 and P2 can then be described, with reference to the pole, as follows:
;
<
3
3
¡
¡
3ROH
P1 corresponds to radius =100 plus angle =30°
P2 corresponds to radius =60 plus angle =75°
1.1.4 Absolute dimensions
With absolute dimensions, all the positional data refer to the currently valid zero point.
Applied to tool movement this means:
the position, to which the tool is to travel.
Example of milling
The positional parameters for points P1 to P3 in absolute dimensions referring to the zero
point are the following:
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
18 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
<
3
3
3
P1 corresponds to X20 Y35
P2 corresponds to X50 Y60
P3 corresponds to X70 Y20
Example of turning
The positions for points P1 to P4 in absolute dimensions are as follows with reference to the
zero point:
=
;
3
3 3
3
P1 corresponds to X25 Z-7.5
P2 corresponds to X40 Z-15
P3 corresponds to X40 Z-25
P4 corresponds to X60 Z-35
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 19
1.1.5 Incremental dimension
Production drawings are frequently encountered, however, where the dimensions refer not to
the origin, but to another point on the workpiece. In order to avoid having to convert such
dimensions, it is possible to specify them in incremental dimensions. Incremental dimensions
refer to the positional data for the previous point. Applied to tool movement this means:
The incremental dimensions describe the distance the tool is to travel.
Example of milling
The positional data for points P1 to P3 in incremental dimensions are:
;
<
3
3
3
P1 corresponds to X20 Y35 ;(with reference to the zero point)
P2 corresponds to X30 Y20 ;(with reference to P1)
P3 corresponds to X20 Y-35 ;(with reference to P2)
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
20 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning
The positions for points P1 to P4 in incremental dimensions are as follows:
=
;
3
3 3
3
G90 P1 corresponds to X25 Z-7.5 ;(with reference to the zero point)
G91 P2 corresponds to X15 Z-7.5 ;(with reference to P1)
G91 P3 corresponds to Z-10 ;(with reference to P2)
G91 P4 corresponds to X20 Z-10 ;(with reference to P3)
Note
When DIAMOF or DIAM90 is active, the path setpoint is programmed as a radius dimension
with G91.
Fundamental Geometrical Principles
1.1 Description of workpiece points
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 21
1.1.6 Plane designations
When programming, it is necessary to specify the working plane so that the control system
can calculate the tool offset values correctly. The plane is also relevant to certain types of
circular programming and polar coordinates.
A plane is defined by means of two coordinate axes.
Milling:
;
<
=
*
*
*
Turning:
*
*
<
;
=
*
The third coordinate axis is perpendicular to this plane and determines the infeed direction of
the tool (e.g., for 2D machining).
Fundamental Geometrical Principles
1.2 Position of zero points
Fundamentals
22 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Working planes
The working planes are specified as follows in the NC program with G17, G18 and G19:
Level
Designation
Infeed direction
X/Y G17 Z
Z/X G18 Y
Y/Z G19 X
1.2 Position of zero points
The various origins (zero points) and reference positions are defined on the NC machine.
They are reference points
• for the machine to approach and
• for programming the workpiece dimensions.
The diagrams show the zero points and reference points for drilling/milling machines and
turning machines.
Milling:
::
0
<
;
Fundamental Geometrical Principles
1.2 Position of zero points
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 23
Turning:
=
;
5
%
:
$
0
Reference points
They are:
M Machine zero
A Blocking point. Can coincide with the workpiece zero point
(only turning machines).
W Workpiece zero = Program zero
B Start point. Can be defined for each program.
Start point of the first tool for machining.
R Reference point. Position determined by cams and measuring
system. The distance to the machine zero M must be known, so
that the axis position can be set at this place exactly on this value
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
24 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.3 Position of coordinate systems
1.3.1 Overview of various coordinate systems
We distinguish between the following coordinate systems:
• The machine coordinate system with the machine zero M
• The basic coordinate system (this can also be the workpiece coordinate system W)
• The workpiece coordinate system with the workpiece zero W
• The current workpiece coordinate system with the current offset workpiece zero Wa
In cases where different machine coordinate systems are in use (e.g., 5-axis transformation),
an internal transformation function mirrors the machine kinematics on the coordinate system
currently selected for programming.
Note
The individual axis identifiers are explained in the section headed "Axis types".
Milling coordinate system:
=
P
;
P
<
P
=
Z
;
Z
<
Z
=
D
;
D
<
D
0
:
:D
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 25
Turning coordinate system:
:
0
;
=
<
1.3.2 Machine coordinate system
The machine coordinate system comprises all the physically existing machine axes.
Reference points and tool and pallet changing points (fixed machine points) are defined in
the machine coordinate system.
0
<P
;P
=P
Where the machine coordinate system is used for programming (this is possible with some
of the G functions), the physical axes of the machine are addressed directly. No allowance
is made for workpiece clamping.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
26 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Right-hand rule
The orientation of the coordinate system relative to the machine depends on the machine
type. The axis directions follow the so-called "three-finger rule" of the right hand (in
accordance with DIN 66217).
Seen from in front of the machine, the middle finger of the right hand points in the opposite
direction to the infeed of the main spindle. Therefore:
• the thumb points in the +X direction
• the index finger points in the +Y direction
• the middle finger points in the +Z direction
;
<
=
Determination from the right hand rule for different machine types
With different machine types the determination from the right hand rule can look different in
each case. The following are examples of machine coordinate systems for various
machines.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 27
=
<
;
&
&
;
=
<
;
<
%
%
<
;
=
$
$
=
%
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
28 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.3.3 Basic coordinate system
The basic coordinate system is a Cartesian coordinate system, which is mirrored by
kinematic transformation (for example, 5-axis transformation or by using Transmit with
peripheral surfaces) onto the machine coordinate system.
;
:=
;
<
=
<
%DVLFFRRUGLQDWHV\VWHP
IRUIURQWIDFH
:RUNSLHFH
FRRUGLQDWHV\VWHP
IRUSODQHRIURWDWLRQ
%DVLF
FRRUGLQDWHV\VWHP
IRUSHULSKHUDOVXUIDFH
If there is no kinematic transformation, the basic coordinate system differs from the machine
coordinate system only in terms of the axis designations.
The activation of a transformation can produce deviations in the parallel orientation of the
axes. The coordinate system does not have to be at a right angle.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 29
Further determinations
3URJUDPPDEOH)5$0(
'5)RIIVHW]HURRIIVHWH[WHUQDO
<0&6
0&
6
.LQHPDWLFWUDQVIRUPDWLRQ
%&6
:&6
<%&6 <:&6
;0&6
;%&6
;:&
6
%DVLFIUDPHEDVLFRIIVHW
%=6
<%=6
;%=6
**VHWWDEOH)5$0(6
6=6
<6=6
;6=6
0&6 0DFKLQH&RRUGLQDWH6\VWHP%&6 %DVLF&RRUGLQDWH6\VWHP
%=6 %DVLF=HUR6\VWHP 6=6 6HWWDEOH=HUR6\VWHP
:&6 :RUNSLHFH&RRUGLQDWH6\VWHP
Zero offsets, scaling, etc., are always executed in the basic coordinate system.
The coordinates also refer to the basic coordinate system when specifying the working field
limitation.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
30 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.3.4 Workpiece coordinate system
The geometry of a workpiece is described in the workpiece coordinate system. In other
words, the data in the NC program refer to the workpiece coordinate system.
=
;
<
The workpiece coordinate system is always a Cartesian coordinate system and assigned to
a specific workpiece.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 31
1.3.5 Frame system
The frame is a self-contained arithmetic rule that transforms one Cartesian coordinate
system into another Cartesian coordinate system.
;
<
;
<
= =
;
<
=
5RWDWLRQ
DURXQGWKH=D[LV
=HURRIIVHW
It is a spatial description of the workpiece coordinate system
The following components are available within a frame:
• Zero offset
• Rotate
• Mirroring
• Scaling
These components can be used individually or in any combination.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
32 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Mirroring of the Z axis
;
=
0:
=HURRIIVHW
;
=
0
:
=HURRIIVHW
Shifting and turning the workpiece coordinate system
One way of machining inclined contours is to use appropriate fixtures to align the workpiece
parallel to the machine axes.
<
;
=
<
;
=
... Another way is to generate a coordinate system, which is oriented to the workpiece. The
coordinate system can be moved and/or rotated with programmable frames.
This enables you to
• move the zero point to any position on the workpiece
• align the coordinate axes parallel to the desired working plane by rotation
• and thus machine surfaces clamped in inclined positions, produce drill holes at different
angles.
Fundamental Geometrical Principles
1.3 Position of coordinate systems
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 33
• Performing multi-side machining operations.
<
;
=
;
<
=
The conventions for the working plane and the tool offsets must be observed – in
accordance with the machine kinematics – for machining operations in inclined working
planes.
For further information, please see "Selection of working plane, G17 to G19".
1.3.6 Assignment of workpiece coordinate system to machine axes
The location of the workpiece coordinate system in relation to the basic coordinate system
(or machine coordinate system) is determined by settable frames.
=0 =%
<0 =%
;
0
;
%
=:
;
:
<0
0
*
The settable frames are activated in the NC program by means of commands such as G54.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
34 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.3.7 Current workpiece coordinate system
Sometimes it is advisable or necessary to reposition and to rotate, mirror and/or scale the
originally selected workpiece coordinate system within a program.
The programmable frames can be used to reposition (rotate, mirror and/or scale) the current
zero point at a suitable point in the workpiece coordinate system. You will thus obtain the
current workpiece coordinate system.
<%
;%
=%
<
<
;
;
=
=
)UDPH
)UDPH
:RUNSLHFH
FRRUGLQDWHV\VWHP
&XUUHQWZRUNSLHFH
FRRUGLQDWHV\VWHP
)UDPHVHWWDEOHRIIVHWDQGURWDWLRQ
)UDPHSURJUDPPDEOHRIIVHWDQGURWDWLRQ
Several zero offsets are possible in the same program.
1.4 Axes
A distinction is made between the following types of axes when programming:
• Machine axes
• Channel axes
• Geometry axes
• Special axes
• Path axes
• Synchronized axes
• Positioning axes
• Command axes (motion-synchronous actions)
• PLC axes
• Link axes
• Lead link axes
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 35
0DFKLQHD[HV
3RVLWLRQLQJD[HV
*HRPHWU\D[HV
6\QFKU
D[HV
3/&D[HV
&RPPDQG
D[HV
3RVLWLRQLQJ
D[HV
0DFKLQHD[HV
6SHFLDOD[HV
&KDQQHOD[HV
.LQHPDWLFWUDQVIRUPDWLRQ
*HRPHWU\D[HV
3DWKD[HV
Behavior of programmed axis types
Geometry, synchronized and positioning axes are programmed.
• Path axes traverse with feedrate F in accordance with the programmed travel commands.
• Synchronized axes traverse synchronously to path axes and take the same time to
traverse as all path axes.
• Positioning axes traverse asynchronously to all other axes. These traversing movements
take place independently of path and synchronized movements.
• Command axes traverse asynchronously to all other axes. These traversing movements
take place independently of path and synchronized movements.
• PLC axes are controlled by the PLC and can traverse asynchronously to all other axes.
The traversing movements take place independently of path and synchronized
movements.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
36 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.4.1 Main axes/Geometry axes
The main axes define a right-angled, right-handed coordinate system. Tool movements are
programmed in this coordinate system.
In NC technology, the main axes are called geometry axes. This term is also used in this
Programming Guide.
The "Switchable geometry axes" function (see Advanced) can be used to alter the geometry
axes grouping configured by machine data. Here any geometry axis can be replaced by a
channel axis defined as a synchronous special axis.
Axis identifier
For turning machines:
Geometry axes X and Z are used, and sometimes Y.
7RROV
5HYROYHUVZLYHO
D[LV
6SHFLDOVSLQGOH
6SHFLDOD[LV
7DLO
VWRFN
*HRPHWU\
D[HV
0DLQVSLQGOH
PDVWHUVSLQGOH
&D[LV
;
=
For milling machines:
Geometry axes X, Y and Z are used.
A maximum of three geometry axes are used for programming frames and the workpiece
geometry (contour).
The identifiers for geometry and channel axes may be the same, provided a reference is
possible.
Geometry axis and channel axis names can be the same in any channel so that the same
programs can be executed.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 37
1.4.2 Special axes
In contrast to the geometry axes, no geometrical relationship is defined between the special
axes.
Axis identifier
In a turning machine with revolver magazine, for example,
Turret position U, tailstock V
Application examples
Typical special axes are tool revolver axes, swivel table axes, swivel head axes, and loader
axes.
N10 G1 X100 Y20 Z30 A40 F300 ;Path axis movements
N20 POS[U]=10POS[X]=20 FA[U]=200 FA[X]=350 ;Positioning axis movements
N30 G1 X500 Y80 POS[U]=150FA[U]=300 F550 ;Path and positioning axis
N40 G74 X1=0 Z1=0 ;Approaching a reference point
1.4.3 Main spindle, master spindle
The machine kinematics determine, which spindle is the main spindle. This spindle is
declared the master spindle in the machine data. As a rule, the main spindle is declared the
master spindle. This assignment can be changed with the program command SETMS
(spindle number). By issuing SETMS without statement of the spindle number you can
switch back to the master spindle defined in the machine data. Special functions such as
thread cutting apply to the master spindle, see "Spindle speed S, spindle direction of rotation
M3, M4, M5".
Spindle identifier
Identifiers: S or S0
1.4.4 Machine axes
Machine axes are the axes physically existing on a machine. The movements of axes can
still be assigned by transformations (TRANSMIT, TRACYL, or TRAORI) to the machine
axes. If transformations are intended for the machine, different axis names must be
determined.
The machine axis names are programmed only in special cases, such as reference point or
fixed point approaching.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
38 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Axis identifier
The axis identifiers can be set in the machine data.
Standard identifiers:
X1, Y1, Z1, A1, B1, C1, U1, V1
There are also standard axis identifiers that can always be used:
AX1, AX2, ..., AXn
1.4.5 Channel axes
Channel axes are all axes, which traverse in a channel.
Axis identifier
Identifiers: X, Y, Z, A, B, C, U, V
1.4.6 Path axes
Path axes define the path and therefore the movement of the tool in space.
The programmed feed is active for this path. The axes involved in this path reach their
position at the same time. As a rule, these are the geometry axes.
However, default settings define, which axes are the path axes, and therefore determine the
velocity.
Path axes can be specified in the NC program with FGROUP, see "Path behavior".
1.4.7 Positioning axes
Positioning axes are interpolated separately, i.e., each positioning axis has its own axis
interpolator and its own feedrate. Positioning axes do not interpolate with the path axes.
Positioning axes are traversed by the NC program or the PLC. If an axis is to be traversed
simultaneously by the NC program and the PLC, an error message appears.
Typical positioning axes are:
• Loaders for moving workpieces to machine
• Loaders for moving workpieces away from machine
• Tool magazine/turret
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 39
Programming
A distinction is made between positioning axes with synchronization at the block end or over
several blocks.
Parameters
POS axes:
Block change occurs at the end of the block when all the path and positioning axes
programmed in this block have reached their programmed end point.
POSA axes:
The movement of these positioning axes can extend over several blocks.
POSP axes:
The movement of these positioning axes for approaching the end position takes place in
sections.
Note
Positioning axes become synchronized axes if they are traversed without the special
POS/POSA identifier.
Continuous-path mode (G64) for path axes is only possible if the positioning axes (POS)
reach their final position before the path axes.
Path axes that are programmed with POS/POSA are removed from the path axis grouping
for the duration of this block.
You will find further information on POS, POSA, and POSP in the section on "Traversing
positioning axes, POS, POSA, POSP".
1.4.8 Synchronized axes
Synchronized axes traverse synchronously to the path from the start position to the
programmed end position.
The feedrate programmed in F applies to all the path axes programmed in the block, but
does not apply to synchronized axes. Synchronized axes take the same time as the path
axes to traverse.
A synchronized axis can be a rotary axis, which is traversed synchronously to the path
interpolation.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
40 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.4.9 Command axes
Command axes are started from synchronized actions in response to an event (command).
They can be positioned, started, and stopped fully asynchronous to the parts program. An
axis cannot be moved from the parts program and from synchronized actions
simultaneously.
Command axes are interpolated separately, i.e., each command axis has its own axis
interpolator and its own feedrate.
References:/FBSY/, Synchronized Actions
1.4.10 PLC axes
PLC axes are traversed by the PLC via special function blocks in the basic program; their
movements can be asynchronous to all other axes. The traversing movements take place
independently of path and synchronized movements..
1.4.11 Link axes
Link axes are axes, which are physically connected to another NCU and whose position is
controlled from this NCU. Link axes can be assigned dynamically to channels of another
NCU. Link axes are not local axes from the perspective of a particular NCU.
&KDQQHO
&KDQQHO
/LQNPRGXOH+: /LQNPRGXOH+:
&KDQQHO
1&8 1&8
' '
/LQNFRPPXQLFDWLRQ
$
$
$
%
%
The axis container concept is used for the dynamic modification of the assignment to an
NCU. Axis substitution with GET and RELEASE from the parts program is not available for
link axes.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 41
Prerequisite
The participating NCUs, NCU1 and NCU2, must be connected by means of high-speed
communication via the link module.
References:
/PHD/Configuring Manual NCU; NCU 571-573.2 Link Module
The axis must be configured appropriately by machine data.
The link axis option must be installed.
Description
The position control is implemented on the NCU on which the axis is physically connected to
the drive. This NCU also contains the associated axis VDI interface. The position setpoints
for link axes are generated on another NCU and communicated via the NCU link.
The link communication must provide the means of interaction between the interpolators and
the position controller or PLC interface. The setpoints calculated by the interpolators must be
transported to the position control loop on the home NCU and, vice versa, the actual values
must be returned from there back to the interpolators.
For further information about link axes, please refer to
References: /FB2/Function Manual Extended Functions; Multiple Operator Panels and NCUs
(B3)
Axis container
An axis container is a circular buffer data structure, in which local axes and/or link axes are
assigned to channels. The entries in the circular buffer can be shifted cyclically.
In addition to the direct reference to local axes or link axes, the link axis configuration in the
logical machine axis image also allows references to axis containers. This type of reference
consists of:
• a container number and
• a slot (circular buffer location within the container)
The entry in a circular buffer location contains:
• a local axis or
• a link axis
Axis container entries contain local machine axes or link axes from the perspective of an
individual NCU. The entries in the logical machine axis image
MN_AXCONF_LOGIC_MACHAX_TAB of an individual NCU are fixed.
The axis container function is described in
References: /FB2/Function Manual Extended Functions; Multiple Operator Panels and
NCUs (B3)
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
42 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.4.12 Lead link axes
A leading link axis is one that is interpolated by one NCU and utilized by one or several other
NCUs as the master axis for controlling slave axes.
$
1&8
,QWHUSRODWRU
6HUYR
'
%
%
'
1&8
,QWHUSRODWRU
6HUYR
1&8OLQNPRGXOH
6HWSRLQWVIURP$
&KDQQHOFRQWURO
E\IROORZLQJ
D[LVD[HV
$FWXDOYDOXHV
IURP$
1&8Q
An axial position controller alarm is sent to all other NCUs, which are connected to the
affected axis via a leading link axis.
NCUs that are dependent on the leading link axis can utilize the following coupling
relationships with it:
• Master value (setpoint, actual master value, simulated master value)
• Coupled motion
• Tangential correction
• Electronic gear (ELG)
• Synchronous spindle
Programming
Master NCU:
Only the NCU, which is physically assigned to the master value axis can program travel
motions for this axis. The travel program must not contain any special functions or
operations.
NCUs of slave axes:
The travel program on the NCUs of the slave axes must not contain any travel commands for
the leading link axis (master value axis). Any violation of this rule triggers an alarm.
The leading link axis is addressed in the usual way via channel axis identifiers. The states of
the leading link axis can be accessed by means of selected system variables.
Fundamental Geometrical Principles
1.4 Axes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 43
Prerequisites
• The dependent NCUs, i.e., NCU1 to NCUn (n equals max. of 8), must be interconnected
via the link module for high-speed communication.
References:
/PHD/Configuring Manual NCU; NCU 571-573.2 Link Module
• The axis must be configured appropriately by machine data.
• The link axis option must be installed.
• The same interpolation cycle must be configured for all NCUs connected to the leading
link axis.
Restrictions
• A master axis, which is leading link axis cannot be a link axis, i.e., it cannot be operated
by NCUs other than its home NCU.
• A master axis, which is leading link axis cannot be a container axis, i.e., it cannot be
addressed alternately by different NCUs.
• A leading link axis cannot be the programmed leading axis in a gantry grouping.
• Couplings with leading link axes cannot be cascaded.
• Axis replacement can only be implemented within the home NCU of the leading link axis.
System variables:
The following system variables can be used in conjunction with the channel axis identifier of
the leading link axis:
• $AA_LEAD_SP; Simulated master value position
• SAA_LEAD_SV; Simulated master value velocity
If these system variables are updated by the home NCU of the master axis, the new values
are also transferred to any other NCUs, which wish to control slave axes as a function of this
master axis.
References: /FB2/Function Manual Extended Functions; Multiple Operator Panels and
NCUs (B3)
Fundamental Geometrical Principles
1.5 Coordinate systems and workpiece machining
Fundamentals
44 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
1.5 Coordinate systems and workpiece machining
The relationship between travel commands of the programmed axis movements from the
workpiece coordinates and the resulting machine movement is displayed.
How you can determine the distance traveled taking into account all shifts and corrections is
shown by reference to the path calculation.
Relationship between the travel commands from workpiece coordinates and the resulting machine
movements
Axis movement programmed in the workpiece coordinate system
$[LVPRYHPHQWSURJUDPPHGLQWKHZRUNSLHFHFRRUGLQDWHV\VWHP
'HVFULSWLRQRIWKH
ZRUNSLHFHJHRPHWU\YLDJHRPHWU\
D[HVHJ;<=
&RQWRXULQ&DUWHVLDQ
FRRUGLQDWHV\VWHP
RIWKHFKDQQHO%&6
7RROUDGLXVFRPSHQVDWLRQ
0RYHPHQWRI
WRRO]HUR
LQ%&6
7RROOHQJWKFRPSHQVDWLRQ
.LQHPDWLFWUDQVIRUPDWLRQLIDFWLYH
0RYHPHQWRIPDFKLQHD[HVRIFKDQQHODEF
5RWDU\D[HVIRU
D[LVWUDQVIRUPDWLRQ
5HPDLQLQJWUDYHUVLQJ
LQVWUXFWLRQV
YLDVRFDOOHGVSHFLDOD[HV
HJ&89
'HVFULSWLRQRIWRRO
RULHQWDWLRQE\PHDQVRI
RULHQWDWLRQYHFWRU(XOHUDQJOH
)UDPHFDOFXODWLRQ
2IIVHW75$16
5RWDWLRQ527
6FDOLQJ6&$/(
)UDPHFDOFXODWLRQ
2IIVHW
6FDOLQJ
Path calculation
The path calculation determines the distance to be traversed in a block, taking into account
all offsets and compensations.
In general:
Distance = setpoint - actual value + zero offset (ZO) + tool offset (TO)
Fundamental Geometrical Principles
1.5 Coordinate systems and workpiece machining
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 45
;
=
0:
=2
$EVROXWHSRVLWLRQ
:.
6HW
SRLQW
YDOXH
$EVROXWH
SRVLWLRQ
:.
6HW
SRLQW
9DOXH
7
If a new zero offset and a new tool offset are programmed in a new program block, the
following applies:
• With absolute dimensioning:
Distance = (absolute dimension P2 - absolute dimension P1) + (ZO P2 - ZO P1) +
(TO P2 - TO P1).
• With incremental dimensioning:
Distance = incremental dimension + (ZO P2 - ZO P1) + (TO P2 - TO P1).
193
193
$EVROXWHGLPHQVLRQVVHWSRLQWIRU3 :.3
'LVWDQFH
:.3
$EVROXWH
GLPHQVLRQV
VHWSRLQW
IRU3
0:3 3
0RWLRQ
$FWXDOYDOXH
$FWXDOYDOXH
Fundamental Geometrical Principles
1.5 Coordinate systems and workpiece machining
Fundamentals
46 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 47
Fundamental Principles of NC Programming 2
2.1 Structure and contents of an NC program
Note
DIN 66025 is the guideline for designing a parts program.
An (NC/part) program consists of a sequence of NC blocks (see table below). Each data
block represents one machining step. Instructions are written in the blocks in the form of
words. The last block in the execution sequence contains a special word for the end of
program: M2, M17 or. M30.
Set Word Word Word ... ;Comment
Set N10 G0 X20 ... ;1. Set
Set N20 G2 Z37 ... ;2. Set
Set N30 G91 ... ... ;...
Set N40 ... ... ...
Set N50 M30 ... ... ;End of program (last block)
Program names
Each program has a different name; the name can be chosen freely during program creation
(except for punch tape format), taking the following conditions into account:
• The first two characters must be letters (or a letter with an underscore character)
• other letters, digits
Example:
_MPF100 or
SHAFT or
SHAFT_2
Only the first 24 characters of a program identifier are displayed on the NC.
Fundamental Principles of NC Programming
2.1 Structure and contents of an NC program
Fundamentals
48 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Punch tape format
File names:
File names can contain the characters 0...9, A...Z, a...z or _ and must not exceed 24
characters in total.
File names must have a 3-character extension (_xxx).
Data in punch tape format can be generated externally or processed with an editor. A file
name of a file that is filed internally in the NC memory starts with "_N_".
A file in punch tape format is introduced with %<name>, "%" must be in the first column of
the first row.
Examples:
%_N_SHAFT123_MPF = part program SHAFT123
Or
%flange3_MPF = part program flange3
For further information on downloading, creating, and storing parts programs, please refer to:
Operating Manuals HMI Chapter "Operator area program"/"Operator area services"
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 49
2.2 Language elements of the programming language
Overview
The language elements of the programming language are determined by
• Character set with uppercase and lowercase letters and digits
• Words with addresses and sequence of digits
• Blocks and block format
• Block length with maximum possible number of characters
• Order of the words in a block with table of the addresses and their meaning
• Main blocks and subblocks
• Block number
• Addresses with table for important addresses and explanations
• Addresses effective modally or non-modally
• Addresses with axial extension with table of extended address notations
• Fixed addresses with table and statement of the meaning for default setting
• Fixed addresses with axis expansion with table and statement of the meaning for default
setting
• Adjustable addresses with statement of the adjustable address letters
• Predefined computing functions as well as arithmetic, comparative and logical operators
with corresponding value assignments.
• Identifiers such as variables, subroutines, keywords, DIN addresses and jump markers
Character set
The following characters are available for writing NC programs:
Uppercase characters
A, B, C, D, E, F, G, H, I, J, K, L, M, N,(O),P, Q, R, S, T, U, V, W, X, Y, Z
Please note:
Take care to differentiate between the letter "O" and the digit "0".
Lowercase letters
a, b, c, d, e, f, g, h, i, j, k, l, m, n, o, p, q, r, s, t, u, v, w, x, y, z
Note
No distinction is made between upper and lower case letters.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
50 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Digits
1, 2, 3, 4, 5, 6, 7, 8, 9
Special characters
% Program start character (used only for writing programs on an external PC)
( For bracketing parameters or expressions
) For bracketing parameters or expressions
[ For bracketing addresses or indexes
] For bracketing addresses or indexes
< Less than
> Greater than
: Main block, end of label, chain operator
= Assignment, part of equation
/ Division, block suppression
* Multiplication
+ Addition
- Subtraction, minus sign
" Double quotation marks, identifier for character string
' Single quotation marks, identifier for special numerical values: hexadecimal,
binary
$ System variable identifiers
_ Underscore, belonging to letters
? Reserved
! Reserved
. Decimal point
, Comma, parameter separator
; Comment start
& Format character, same effect as space character
LF End of block
Tab character Separator
space character Separator (blank)
Note
Non-printable special characters are treated like blanks.
Words
In the same way as our language, NC programs are made up of blocks and each block is
made up of words.
A word in the "NC language" consists of an address character and a digit or sequence of
digits representing an arithmetic value.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 51
$GGUHVV
1XPEHUVWULQJ
6HW
:RUG
$GGUHVV
$GGUHVV
1XPEHUVWULQJ
1XPEHUVWULQJ
; 6
*
:RUG :RUG
The address character of the word is usually a letter. The sequence of digits can contain a
sign and decimal point. The sign always appears between the address letter and the
sequence of digits. The positive sign (+) does not have to be specified.
Blocks and block format
An NC program consists of individual blocks. A block generally consists of (several) words.
A block should contain all the data required for performing an operation step and is
terminated with the character "LF" (LINE FEED = new line).
Note
The "LF" character does not have to be inserted manually, it is generated automatically when
you change lines.
Block length
A block can contain a maximum of 512 characters (including the comment and end-of-block
character "LF").
Note
Three blocks of up to 66 characters each are normally displayed in the current block display
on the screen. Comments are also displayed. Messages are displayed in a separate
message window.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
52 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Word sequence in blocks
In order to keep the block format as clear as possible, the words in a block should be
arranged as follows:
Example:
N10 G… X… Y… Z… F… S… T… D… M… H…
Address Meaning
N Address of block number
10 Block number
G Preparatory function
X,Y,Z Positional data
F Feed
S Spindle speed
T Tool
D Tool offset number
M Miscellaneous (i.e., special) function
H Auxiliary function
Note
Certain addresses can be used repeatedly within a block
(e.g., G…, M…, H…)
Main block/subblock
There are two types of blocks:
• Main blocks and
• subblocks
The main block must contain all the words necessary to start the operation sequence in the
program section beginning with the main block.
Note
Main blocks can be contained in both main programs and subroutines. The control does not
check whether a main block contains all the necessary information.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 53
Block number
Main blocks are identified by a main block number. A main block number comprises the
character ":" and a positive whole number (block number). The block number always
appears at the start of a block.
Note
Main block numbers must be unique within a program to achieve an unambiguous result
when searching.
Example:
:10 D2 F200 S900 M3
Subblocks are identified by a subblock number. A subblock number comprises the character
"N" and a positive whole number (block number). The block number always appears at the
start of a block.
Example:
N20 G1 X14 Y35
N30 X20 Y40
Note
Subblock numbers must be unique within a program in order to achieve an unambiguous
result when searching.
The order of the block numbers is arbitrary, however increasing block numbers are
recommended. You can also program NC blocks without block numbers.
Addresses
Addresses are fixed or settable identifiers for axes (X, Y, etc.), spindle speed (S), feedrate
(F), circle radius (CR), etc.
Example:
N10 X100
Important addresses
Address Meaning (default setting) Notes
A=DC(...)
A=ACP(...)
A=ACN(...)
Rotary axis variable
ADIS Rounding clearance for path functions fixed
B=DC(...)
B=ACP(...)
B=ACN(...)
Rotary axis variable
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
54 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
C=DC(...)
C=ACP(...)
C=ACN(...)
Rotary axis variable
CHR=... Chamfer the contour corner fixed
D... Cutting edge number fixed
F... Feed fixed
FA[axis]=... or
FA[spindle]=... or
[SPI(spindle)]=...
Axial feed
(only if spindle no. defined by variable)
fixed
G... Preparatory function fixed
H...
H=QU(...)
Auxiliary function
Auxiliary function without read stop
fixed
I... Interpolation parameters variable
J... Interpolation parameters variable
K... Interpolation parameters variable
L... Subroutine call fixed
M...
M=QU(...)
Miscellaneous (i.e., special) function
Miscellaneous fct. w/o read stop
fixed
N... Subblock fixed
OVR=... Path override fixed
P... Number of program passes fixed
POS[Axis]=... Position axis fixed
POSA[Axis]=... Positioning axis across block boundary fixed
SPOS=...
SPOS[n]=...
Spindle position fixed
SPOSA=...
SPOSA[n]=...
Spindle position across block boundary fixed
Q... Axis variable
R0=... to Rn=...
R...
Arithmetic parameter, n can be set via MD
(default 0-99)
- Axis
fixed
variable
RND Round the contour corner fixed
RNDM Round contour corner (modally) fixed
S... Spindle speed fixed
T... Tool number fixed
U... Axis variable
V... Axis variable
W... Axis variable
X...
X=AC(...)
X=IC(...)
Axis
" absolute
" incremental
variable
Y...
Y=AC(...)
Y=IC(...)
Axis variable
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 55
Z...
Z=AC(...)
Z=IC(...)
Axis variable
AR+=... Opening angle variable
AP=... Polar angle variable
CR=... Circle radius variable
RP=... Polar radius variable
:... Main block fixed
"fixed"
These address names are available for a specific function.
Machine manufacturer
"variable"
The machine manufacturer may assign another name to these addresses via machine data.
Modal/non-modal addresses
Modal addresses remain valid with the programmed value (in all subsequent blocks) until a
new value is programmed at the same address.
Non-modal addresses only apply in the block, in which they were programmed.
Example:
N10 G01 F500 X10
N20 X10 ;Feedrate remains operative until a new feed value is entered
Addresses with axial extension
In addresses with axial extension, an axis name is inserted in square brackets after the
address. The axis name assigns the axis.
Example:
FA[U]=400 ;Axis-specific feed for U axis
Extended addresses
Extended address notation enables a larger number of axes and spindles to be organized in
a system. An extended address is composed of a numeric extension or a variable identifier
enclosed in square brackets and an arithmetic expression with an "=" sign.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
56 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example:
X7 ;No "=" required, 7 is a value, but the "=" character can
;also be used here
X4=20 ;Axis X4 ("=" required)
CR=7.3 ;2 letters ("=" required)
S1=470 ;Speed for 1st spindle 470 rpm
M3=5 ;Spindle stop for 3rd spindle
The extended address notation is only permitted for the following direct addresses:
Address Meaning
X, Y, Z Axis addresses
I, J, K Interpolation parameters
S Spindle speed
SPOS,
SPOSA
Spindle position
M Miscellaneous functions
H Auxiliary functions
T Tool number
F Feed
In the case of extended address notation, the number (index) can be substituted by a
variable for addresses M, H and S and for SPOS and SPOSA. The variable identifier is
enclosed in square brackets.
Example:
S[SPINU]=470 ;Speed for the spindle, whose number is stored in the
;SPINU variables.
M[SPINU]=3 ;Clockwise rotation for the spindle, whose number is stored in the
;SPINU variables.
T[SPINU]=7 ;Selection of the tool for the spindle, whose number is stored in the
;SPINU variables.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 57
Fixed addresses
The following addresses are set permanently:
Address Meaning (default setting)
D Cutting edge number
F Feed
G Preparatory function
H Auxiliary function
L Subroutine call
M Miscellaneous (i.e., special) function
N Subblock
P Number of program runs
R Arithmetic variables
S Spindle speed
T Tool number
: Main block
Example for programming:
N10 G54 T9 D2
Fixed addresses with axis expansion
Address Meaning (default setting)
AX Axis value (variable axis programming)
ACC Axial acceleration
FA Axial feed
FDA Axis feed for handwheel override
FL Axial feed limit
IP Interpolation parameter (variable axis programming)
OVRA Axial override
PO Polynomial coefficient
POS Position axis
POSA Positioning axis across block boundary
Example:
N10 POS[X]=100
Explanation:
When programming with the axis expansion, the axis to be traversed is enclosed in square
brackets.
You will find a complete list of all fixed addresses in the Appendix.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
58 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Settable addresses
Addresses can be defined either as an address letter (with numerical extension if necessary)
or as freely selected identifiers.
Note
Variable addresses must be unique within the control, i.e., the same identifier name may not
be used for different address types.
A distinction is made between the following address types:
• Axis values and end points
• Interpolation parameters
• Feedrates
• Corner rounding criteria
• Measurement
• Axis, spindle behavior
• …
Variable address letters are:
A, B, C, E, I, J, K, Q, U, V, W, X, Y, Z
Note
The user can change the names of the variable addresses in the machine data.
Example:
X1, Y30, U2, I25, E25, E1=90, …
The numeric extension has one or two digits and is always positive.
Address identifiers:
The address notation can be expanded by adding extra letters.
Example:
CR ;e.g., for circle radius
XPOS
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 59
Operators/mathematical functions
Operators and
mathematical
functions
Meaning
+ Addition
- Subtraction
* Multiplication
/ Division
Notice: (type INT)/(type INT)=(type REAL); example: 3/4 = 0.75
DIV Division, for variable types INT and REAL
Notice: (type INT)DIV(type INT)=(type INT); example: 3 DIV 4 = 0
MOD Modulo division (only for type INT) produces remainder of INT division;
Example 3 MOD 4=3
: Chain operator (for FRAME variables)
Sin() Sine
COS() Cosine
TAN() Tangent
ASIN() Arcsine
ACOS() Arccosine
ATAN2() Arctangent2
SQRT() Square root
ABS() Absolute number
POT() 2. 2nd power (square)
TRUNC() Truncate to integer
ROUND() Round to integer
LN() Natural logarithm
EXP() Exponential function
MINVAL Smaller value, two variables
MAXVAL Higher value, two variables
BOUND Variable value that lies in the defined value range
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
60 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Comparison and logic operators
Comparison and logic
operators
Meaning
== Equal to
<> Not equal to
> Greater than
< Less than
>= Greater than or equal to
<= Less than or equal to
AND AND
OR OR
NOT Negation
XOR Exclusive OR
In arithmetic expressions, the execution order of all the operators can be specified by
parentheses, in order to override the normal priority rules.
value assignments
Values can be assigned to the addresses. The method of value assignment depends on the
type of address identifier.
An "=" sign must be inserted between the address identifier and the value if
• The address identifier comprises more than one letter,
• The value includes more than one constant.
The "="-sign can be omitted if the address identifier is a single letter and the value consists
of only one constant. Signs are allowed and separators are permitted after the address letter.
Example of value assignments
X10 ;Value assignment (10) to address X, "=" not required
X1=10 ;Value assignment (10) to address (X) with
;numeric extension (1), "=" required
FGROUP(X1, Y2) ;Axis names from passed parameters
AXDATA[X1] ;Axis name as an index when accessing axis data
AX[X1]=10 ;Indirect axis programming
X=10*(5+SIN(37.5)
)
;Value assignment by means of a numeric expression
;"=" required
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 61
Note
A numeric extension must always be followed by one of the special characters "=", "(", "[",
")", "]", ",", or an operator, in order to distinguish an address name with numeric extension
from an address letter with a value.
Names
Identifiers can also be used to describe words (in compliance with DIN 66025). The
identifiers have the same meaning as the words within an NC block. Identifiers must be
unique. The same identifier must not be used for different objects.
Identifiers can stand for:
• Variable
– System variable
– User variable
• Subroutine
• Keywords
• DIN addresses with several letters
• Jump markers
Design
The identifiers are composed of up to 32 characters. The following characters may be used:
• Letters
• Underscore symbols
• Digits
The first two characters must be letters or underscores, separators must not be programmed
between the individual characters (see the following pages).
Example:
CMIRROR, CDON
Note
Reserved keywords must not be used as identifiers. Separators are not permitted between
the individual characters.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
62 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
Number of characters for each identifier
• Program names: 24 characters
• Axis identifiers: 8 characters
• Variable identifiers: 31 characters
Rules for allocating identifiers
The following rules are provided in order to avoid identifier collisions:
• All identifiers beginning with "CYCLE" or "_" are reserved for SIEMENS cycles.
• All identifiers beginning with "CCS" are reserved for SIEMENS compile cycles.
• User compile cycles begin with "CC”.
• We recommend that users select identifier names, which either begin with "U" (User) or
contain the underscore symbol, because these are not used by the system, compile
cycles or SIEMENS cycles.
Further reserved identifiers
• The identifier "RL" is reserved for conventional turning machines.
• All identifiers beginning with "E_ " are reserved for EASY-STEP programming.
Variable identifiers
In variables used by the system, the first letter is replaced by the "$" character. This
character may not be used for user-defined variables.
Examples (see "List of system variables"):
$P_IFRAME, $P_F
Leading zeroes are ignored in variables with numeric extensions (i.e., R01 is interpreted as
R1). Separators are allowed before a numeric extension.
Array identifiers
The rules for elementary variables also apply to array identifiers. It is possible to address
arithmetic variables as arrays.
Example:
R[10]=…
Data types
A variable can contain a numeric value (or several) or a character (or several), e.g., an
address letter.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 63
The data type permitted for the variable is determined when the variable is defined. The data
type for system variables and predefined variables is fixed.
Elementary variable types/data types are:
Type Meaning Range of values
INT Integers with sign -2147483646 ... +2147483647
REAL Real numbers (fractions with decimal
point, LONG REAL to IEEE)
±(2,2*10-308 … 1,8*10+308)
BOOL Boolean values: TRUE (1) and
FALSE (0)
1, 0
CHAR ASCII character specified by the
code
0 … 255
STRING Character string, number of
characters in [...], maximum of 200
characters
Sequence of values with 0 ... 255
AXIS Axis names (axis addresses) only Any axis identifiers in the channel
FRAME Geometrical parameters for
translation, rotation, scaling, and
mirroring
Identical elementary types can be combined in arrays. Up to two-dimensional arrays are
possible.
Constants
Integer constants
Integer with or without sign, e.g., for assigning a value to an address
Examples:
X10.25 ;Assignment of the value +10.25 to address X
X -10.25 ;Assignment of the value –.25 to address X
X0.25 ;Assignment of the value +0.25 to address X
X.25 ;Assignment of the value +0.25 to address X without leading "0"
X=-.1EX-3 ;Assignment of the value –.1*10-3 to address X
Note
If, in an address, which permits decimal point input, more decimal places are specified than
actually provided for the address, then they are rounded to fit the number of places provided.
X0 cannot be replaced with X.
Example:
Do not replace G01 X0 with G01 X!
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
64 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Hexadecimal constants
Constants can also be interpreted in hexadecimal format. The letters "A" to "F" stand for the
digits 10 to 15.
Hexadecimal constants are enclosed in single quotation marks and start with the letter "H",
followed by the value in hexadecimal notation. Separators are allowed between the letters
and digits.
Example for machine data (see also "Job Planning Programming Guide"):
$MC_TOOL_MANAGEMENT_MASK='H3C7F' ;Assignment of hexadecimal values to
;machine data
The maximum number of characters is limited by the value range of the integer data type.
Binary constants
Constants can also be interpreted in binary format. In this case, only the digits "0" and "1"
are used.
Binary constants are enclosed in single quotation marks and start with the letter "B", followed
by the binary value. Separators are allowed between the digits.
Example for machine data (see also "Job Planning Programming Guide"):
$MN_AUXFU_GROUP_SPEC='B10000001' ;Assignment of binary constants to ;machine data
bit 0 and 7 are set
The maximum number of characters is limited by the value range of the integer data type.
Program section
A program section consists of a main block and several subblocks.
Examples:
:10 D2 F200 S900 M3
N20 G1 X14 Y35
N30 X20 Y40
N40 Y-10
...
N100 M30
Skipping blocks
Blocks, which are not to be executed in every program pass (e.g., execute a trial program
run), can be skipped.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 65
1
1
1
1
1
1
1
1
1
1
1
1
3URJUDPH[HFXWLRQ
Blocks, which are to be skipped are marked with an oblique "/" in front of the block number.
Several consecutive blocks can also be skipped. The statements in the skipped blocks are
not executed; the program continues with the next block, which is not skipped.
Example of skipping blocks
N10 ;Is executed
/N20 … ;Skipped
N30 … ;Is executed
/N40 … ;Skipped
N70 … ;Is executed
Up to 10 skip levels can be programmed. Only one skip level can be specified per NC block:
/ ... ;Block is skipped (1st skip level)
/0 ... ;Block is skipped (1st skip level)
/1 N010... ;Block is skipped (2nd skip level)
/2 N020... ;Block is skipped (3rd skip level)
...
/7 N100... ;Block is skipped (8th skip level)
/8 N080... ;Block is skipped (9th skip level)
/9 N090... ;Block is skipped (10th skip level)
Machine manufacturer
The number of skip levels that can be used depends on a display machine datum.
Block skipping of levels /0 to /9 is activated by an operator action (see /BA/ Operator's Guide
HMI Advanced Embedded, program control menu in Machine operating area) or by the
programmable controller.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
66 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
System and user variables can also be used in conditional jumps in order to control program
execution.
Jump destinations (labels)
Labels can be defined to jump within a program.
Label names are allocated with at least two and up to 32 characters (letters, digits,
underscore). The first two characters must be letters or underscores. The label name is
followed by a colon (":").
References:
/PGA/ Job Planning Programming Manual; Subroutines, Macros
Note
Labels must be unique within a program.
Labels always appear at the start of a block. If a program number exists, the label appears
immediately after the block number.
Comments
To make NC programs easier to understand for other users and programmers, it is advisable
to insert meaningful comments in the program.
Comments are appended to the end of a block and are separated from the program section
of the NC block by a semicolon (";").
Examples of comments
N10 G1 F100 X10 Y20 ;Comments to explain the NC block
Or
N10 ;Company G&S, order no. 12A71
N20 ;Program written by H. Müller, Dept. TV 4
;on November 21, 1994
N50 ;Section no. 12, housing for submersible pump type TP23A
Note
Comments are stored and appear in the current block display when the program is running.
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 67
Programming messages
Messages can be programmed to provide the user with information about the current
machining situation during program execution.
A message in an NC program is generated when the message text is typed after keyword
"MSG" in round parentheses "()" and double quotation marks.
A message can be deleted using "MSG ()".
Example of activating/deleting messages
N10 MSG ("Roughing the contour") ;Activate message
N20 X… Y…
N …
N90 MSG () ;Clear message from N10
Note
A message text can be up to 124 characters long and is displayed in two lines
(2*62 characters). Contents of variables can also be displayed in message texts.
Example of message texts
N10 R12=$AA_IW [X] ;Current position of the X axis in R12
N20 MSG (″Check position of X axis″<<R12<<)
N …
N90 MSG () ;Clear message from N20
Or
N20 MSG (″Check position of X axis″<<$AA_IW[X]<<)
Fundamental Principles of NC Programming
2.2 Language elements of the programming language
Fundamentals
68 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Setting alarms
You can also set alarms in addition to messages in an NC program. Alarms are displayed in
a separate field on the screen display. An alarm always goes hand in hand with a response
from the controller according to the alarm category.
Alarms are programmed by writing the keyword "SETAL" followed by the alarm number
enclosed in round brackets.
The valid range for alarm numbers is between 60,000 and 69,999, whereby 60,000 to 64,999
are reserved for SIEMENS cycles and 65,000 to 69,999 are available to the user.
Note
Alarms are always programmed in a separate block.
Example:
N100 SETAL (65000) ;Set alarm no. 65000
You will find a list of reactions associated with specific alarms in the Installation and Start-up
Guide.
The alarm text must be configured in the HMI.
Programmable cycle alarms
A character string containing up to 4 parameters can be specified in addition to the alarm
number for the predefined subroutine SETAL.
Programming
SETAL(<alarmnumber>, <string>)
Parameters
Variable user texts can be defined in these parameters. Predefined parameters with the
following meaning are also provided:
%1 = Channel number
%2 = Block number, label
%3 = Text index for cycle alarms
%4 = Additional alarm parameters
Fundamental Principles of NC Programming
2.3 Programming a sample workpiece
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 69
2.3 Programming a sample workpiece
The programming of the individual operation steps in the NC language generally represents
only a small proportion of the work in the development of an NC program.
Programming of the actual instructions should be preceded by the planning and preparation
of the operation steps. The more accurately you plan in advance how the NC program is to
be structured and organized, the faster and easier it will be to produce a complete program,
which is clear and free of errors.
Programming
Clearly structured programs are a particular advantage if you need to make changes at a
later date.
Since workpieces differ in shape and form, it is not advisable to create every program using
exactly the same method. There are certain methods, which have proven to be successful in
most instances. A sort of "checklist" can be found below.
Procedures
• Prepare the workpiece drawing
– define the workpiece zero
– Draw in the coordinate system
– Calculate any missing coordinates
• Define machining sequence
– Which tools are used when and to machine which type of contour?
– In what order are the individual elements of the workpiece machined?
– Which individual elements repeat (possibly rotated) and should therefore be included
in a subprogram?
– Can you use part contours or similar elements, which already exist in other
subprograms or subroutines?
Where is it advisable or necessary to perform zero offset, rotation, mirroring or scaling
(frame concept)?
Fundamental Principles of NC Programming
2.4 First programming example for milling application
Fundamentals
70 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
• Create a machining plan
Define all the machining processes in steps, e.g.:
– Rapid traverse motions for positioning
– Tool change
– Retract to tool change point
– Activate/deactivate spindle, coolant
– Call tool data
– Infeed
– Path override
– Approach contour
– Retraction from the contour
– etc.
• Translate the work steps into the programming language
– Enter each individual step in an NC block or blocks.
• Combine all the individual steps in a program
2.4 First programming example for milling application
Testing first programming steps on the NC
Please proceed on the NC as described below to verify the following programming example:
• Create a new parts program (name)
• Edit the parts program
• Select the parts program
• Activate single block
• Part-Program Start
References: See Operator's Guide
Note
Alarms can occur during program verification. These alarms have to be reset first.
Machine manufacturer
The machine data settings must be defined correctly before the program can run on the
machine.
References: /FB1/Function Manual Basic Functions; Axes, Coordinate Systems,.. (K2)
Fundamental Principles of NC Programming
2.5 Second programming example for milling application
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 71
Example
_MILL1_MPF
N10 MSG("THIS IS MY NC PROGRAM") ;MSG = Message output in an alarm line
:10 F200 S900 T1 D2 M3 ;Feed, spindle, tool,
;tool offset, spindle clockwise
N20 G0 X100 Y100 ;Rapid traverse to position
N30 G1 X150 ;Rectangle with feed, straight line in X
N40 Y120 ;Straight line in Y
N50 X100 ;Straight line in X
N60 Y100 ;Straight line in Y
N70 G0 X0 Y0 ;Return rapid traverse movement
N100 M30 ;End of block
2.5 Second programming example for milling application
Programming a sample workpiece
This programming example contains surface and side milling, as well as drilling.
• The workpiece is intended for machining on a vertical milling machine.
• The dimensions are in inches.
Machine manufacturer
The machine data settings must be defined correctly before the program can run on the
machine.
References: /FB1/Function Manual Basic Functions; Axes, Coordinate Systems,.. (K2)
Example
%_N_RAISED_BOSS_MPF
N005 MSG ("Traverse axes to tool change location")
N010 START01:SUPA G0 G70 Z0 D0
N015 SUPA X0 Y0
;********************Tool change********************
N020 MSG ("Tool change active")
N025 T1 M6 ;d = 3 inch face cutter
N030 MSG () ;Clears the message from block N020
N035 MSG ("Face milling Z=0 workpiece surface")
N040 G0 G54 X-2 Y.6 S800 M3 M8
N045 Z1 D1
N050 G1 Z0 F50
N055 X8 F25
N060 G0 Y3.5
N065 G1 X-2
Fundamental Principles of NC Programming
2.5 Second programming example for milling application
Fundamentals
72 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N070 SUPA G0 Z0 D0 M5 M9
;********************Tool change********************
N075 T2 M6 ;d = 1 inch facing tool
MSG ("Side machining")
N080 G0 X-1 Y.25 S1200 M3 M8
N085 Z1 D1
N090 G1 Z-.5 F50
N095 G42 X.5 F30
N100 X5.5 RNDM=-.375 ;Modal rounding. Radius=0.375
N105 Y3.625
N110 X.5
N115 Y.25
N120 X=IC(.375) RNDM=0 ;Needed for edge rounding
N125 G40 G0 Y-1 M5 M9 ;Rapid traverse to initial setting
N130 Z1
N135 X-1 Y0
N140 Z-.25
,********************Continue to use 1-inch mill****************
MSG ("Side Cut Top Boss")
N145 G01 G41 X1 Y2
N150 G2 X1.5476 Y3.375 CR=2
N155 G3 X4.4524 CR=3
N160 G2 Y.625 CR=2
N165 G3 X1.5476 CR=3
N170 G2 X1 Y2 CR=2
N175 G0 G40 X0
N180 SUPA G0 Z0 D0 M5 M9 ;Z approaches tool change position
N185 SUPA X0 Y0 ;X and Y to tool change position
;********************Tool change********************
N190 T3 M6 ;27/64 drill
MSG ("Drill 3 holes")
N195 G0 X1.75 Y2 S1500 M3 M8 ;Approach first drill hole
N200 Z1 D1
N205 MCALL CYCLE81 (1,0,.1,-.5,)
N207 X1.75 ;Drill first hole
N210 X3 ;Drill second hole
N215 X4.25 ;Drill third hole
N220 MCALL
N221 SUPA Z0 D0 M5 M9 ;Delete modal call. Z axis traverses to ;machine zero
N225 SUPA X0 Y0
MSG ()
N230 M30 ;End of program
Fundamental Principles of NC Programming
2.5 Second programming example for milling application
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 73
5
5
5
;'3
'LPHQVLRQVDUHLQLQFKHV
Dimension drawing of workpiece "The Raised Boss" (not to scale).
6LGHYLHZ
'LPHQVLRQVLQLQFKHV
Fundamental Principles of NC Programming
2.6 Programming example for turning application
Fundamentals
74 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
2.6 Programming example for turning application
Radius programming and tool radius compensation
The sample program contains radius programming and tool radius compensation.
Example
%_N_1001_MPF
N5 G0 G53 X280 Z380 D0 ;Start point
N10 TRANS X0 Z250 ;Zero offset
N15 LIMS=4000 ;Speed limitation (G96)
N20 G96 S250 M3 ;Select constant cutting speed
N25 G90 T1 D1 M8 ;Select tool and offset
N30 G0 G42 X-1.5 Z1 ;Activate tool with tool radius compensation
N35 G1 X0 Z0 F0.25
N40 G3 X16 Z-4 I0 K-10 ;Rotate radius 10
N45 G1 Z-12
N50 G2 X22 Z-15 CR=3 ;Rotate radius 3
N55 G1 X24
N60 G3 X30 Z-18 I0 K-3 ;Rotate radius 3
N65 G1 Z-20
N70 X35 Z-40
N75 Z-57
N80 G2 X41 Z-60 CR=3 ;Rotate radius 3
N85 G1 X46
N90 X52 Z-63
N95 G0 G40 G97 X100 Z50 M9 ;Deselect tool radius compensation and ;approach tool
change location
N100 T2 D2 ;Call up tool and select offset
N105 G96 S210 M3 ;Select constant cutting speed
N110 G0 G42 X50 Z-60 M8 ;Activate tool with tool radius compensation
N115 G1 Z-70 F0.12 ;Rotate diameter 50
N120 G2 X50 Z-80 I6.245 K-5 ;Rotate radius 8
N125 G0 G40 X100 Z50 M9 ;Retract tool and ;deselect tool radius compensation
N130 G0 G53 X280 Z380 D0 M5 ;Move to tool change location
N135 M30 ;Program end
Fundamental Principles of NC Programming
2.6 Programming example for turning application
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 75
r
5
5
5
5
5
=
;
Machine manufacturer
The MD settings must be defined correctly before the program can run on the machine.
References: /FB1/Function Manual Basic Functions; Axes, Coordinate Systems,.. (K2)
Fundamental Principles of NC Programming
2.6 Programming example for turning application
Fundamentals
76 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 77
Positional Data 3
3.1 General notes
3.1.1 Program dimensions
In this section you will find descriptions of the commands, with which you can directly
program dimensions taken from a drawing. This has the advantage that no extensive
calculations have to be made for NC programming.
Note
The commands described in this section stand in most cases at the start of a NC program.
The way, in which these functions are combined, is not intended to be a patent remedy. For
example, the choice of working plane may be made at another point in the NC program.
The real purpose of this and all the following sections is to illustrate the conventional
structure of an NC program.
Overview of typical dimensions
The basis of most NC programs is a drawing with concrete dimensions.
When implementing in a NC program, it is helpful to take over exactly the dimensions of a
workpiece drawing into the machining program. These can be:
• Absolute dimension, G90 modally effective applies for all axes in the block, up to
revocation by G91 in a following block.
• Absolute dimension, X=AC(value) only this value applies only for the stated axis and is
not influenced by G90/G91. This is possible for all axes and also for SPOS, SPOSA
spindle positionings, and interpolation parameters I, J, K.
• Absolute dimension, X=CC(value) directly approaching the position by the shortest route,
only this value applies only for the stated rotary axis and is not influenced by G90/G91.
Is also possible for SPOS, SPOSA spindle positionings.
• Absolute dimension, X=ACP(value) approaching the position in positive direction, only
this value is set for the rotary axis, the range of which is set in the machine datum to
0...< 360°.
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
78 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
• Absolute dimension, X=ACN(value) approaching the position in negative direction, only
this value is set for the rotary axis, the range of which is set in the machine datum to
0...< 360°.
• Incremental dimension, G91 modally effective applies for all axes in the block, until it is
revoked by G90 in a following block.
• Incremental dimension, X=IC(value) only this value applies exclusively for the stated axis
and is not influenced by G90/G91. This is possible for all axes and also for SPOS,
SPOSA spindle positionings, and interpolation parameters I, J, K.
• Inch dimension, G70 applies for all linear axes in the block, until revoked by G71 in a
following block.
• Metric dimension, G71 applies for all linear axes in the block, until revoked by G70 in a
following block.
• Inch dimension as for G70, but applies also for feedrate and length-related setting data.
• Metric dimension as for G71, but applies also for feedrate and length-related setting data.
• Diameter programming, DIAMON on
• Diameter programming, DIAMOF off
Diameter programming, DIAM90 for traversing blocks with G90. Radius programming for
traversing blocks with G91.
3.2 Absolute/relative dimensions
3.2.1 Absolute dimension (G90, X=AC)
Function
With the G90 command or the non-modal statement AC you determine the descriptive
system for approaching individual axes from setpoints in absolute dimensions.
You program where the tool should travel.
Programming
G90
Or
X=AC(...) Y=AC(...) Z=AC(...)
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 79
Parameters
G90 Absolute reference dimension
X Y Z Axis identifiers of the axes to be traversed
AC Absolute dimensions non-modally effective
Note
The command G90 is modal.
Generally G90 applies to all axes programmed in subsequent NC blocks.
Example of milling
The traverse paths are entered in absolute coordinates with reference to the workpiece zero.
For entering the circle center point coordinates I and J see circle interpolation G2/G3.
;
<
=
;
N10 G90 G0 X45 Y60 Z2 T1 S2000 M3 ;Absolute dimensioning, rapid traverse to
;XYZ, tool, spindle on
;clockwise
N20 G1 Z-5 F500 ;Tool infeed at feedrate
N30 G2 X20 Y35 I=AC(45) J=AC(35) ;Circle center point in absolute dimensions
N40 G0 Z2 ;Retracting
N50 M30 ;End of block
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
80 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning
The traverse paths are entered in absolute coordinates with reference to the workpiece zero.
For entering the circle center point coordinates I and J see circle interpolation G2/G3.
=
;
:
N5 T1 D1 S2000 M3 ;Tool, spindle on clockwise
N10 G0 G90 X11 Z1 ;Absolute dimensioning, rapid traverse
;to position XYZ
N20 G1 Z-15 F0.2 ;Tool infeed at feedrate
N30 G3 X11 Z-27 I=AC(-5) K=AC(-21) ;Circle center point in absolute dimensions
N40 G1 Z-40 ;Retracting
Description
The dimensions refer to the origin of the active coordinate system. You program the point to
which the tool is to travel, e.g., in the workpiece coordinate system.
Non-modal absolute dimensioning AC
When incremental dimension G91 is active, AC can be used to allow entry of absolute
dimensions for individual axes on a block-by-block basis.
Milling:
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 81
;
<
*
*
*
*
Turning:
=
;
*
*
*
*
Note
On conventional turning machines, it is standard practice to interpret incremental traversing
blocks in the transverse axis as radius values, while diameter dimensions are valid for
absolute coordinates. This conversion for G90 is performed using the commands DIAMON,
DIAMOF or DIAM90.
For dimensioning for diameter or radius, see circular interpolation G2/G3.
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
82 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.2.2 Incremental dimensions (G91, X=IC)
Function
With the G91 command or the non-modal statement IC, you determine the descriptive
system for approaching individual axes from setpoints in incremental dimensions.
You program how far the tool is to travel.
Programming
G91
Or
X=IC(...) Y=IC(...) Z=IC(...)
Parameters
G91 Relative incremental dimensioning
X Y Z Axis identifiers of the axes to be traversed
=IC Incremental dimensions non-modally effective
Example of milling
The dimensions refer to the last point approached.
The circle center point coordinates of the circle interpolation are stated non-modally in
absolute coordinates, since as default the circle center point is independent of G91.
For entering the circle center point coordinates I and J see circle interpolation G2/G3.
;
<
=
;
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 83
N10 G90 G0 X45 Y60 Z2 T1 S2000 M3 ;Absolute dimensioning, rapid traverse to XYZ, tool,
;spindle on clockwise
N20 G1 Z-5 F500 ;Tool infeed at feedrate
N30 G2 X20 Y35 I0 J-25) ;Circle center point in incremental dimensions
N40 G0 Z2 ;Retracting
N50 M30 ;End of block
Example of turning
The dimensions refer to the last point approached.
For entering the circle center point coordinates I and J see circle interpolation G2/G3.
=
;
:
N5 T1 D1 S2000 M3 ;Tool, spindle on clockwise
N10 G0 G90 X11 Z1 ;Absolute dimensioning, rapid traverse to
;position XYZ
N20 G1 Z-15 F0.2 ;Tool infeed at feedrate
N30 G3 X11 Z-27 I-8 K-6 ;Circle center point in incremental dimensions
N40 G1 Z-40 ;Retracting
N50 M30 ;End of block
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
84 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example without traversing through the active zero offset
• G54 contains an offset of 25 in X
• SD 42440: FRAME_OFFSET_INCR_PROG = 0
N10 G90 G0 G54 X100
N20 G1 G91 X10 ;Traverse X by 10 mm, the offset is
;not traversed
N30 G90 X50 ;Traverse to position X75, the offset
;is traversed
Description
The dimensions refer to the last point approached. You program how far the tool is to travel.
Non-modally effective incremental dimensioning IC
Using IC and with a predefined absolute G90 dimension the incremental dimensioning can
be set non-modally for individual axes.
Milling:
;
<
*
*
*
*
Positional Data
3.2 Absolute/relative dimensions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 85
Turning:
=
;
*
*
*
*
Note
On conventional turning machines it is standard practice to interpret incremental NC blocks
in the transverse axis as radius values, while diameter dimensions are valid for absolute
coordinates. This conversion for G91 is performed using the commands DIAMON, DIAMOF
or DIAM90.
For dimensioning for diameter or radius see circular interpolation G2/G3.
G91 extension
For applications such as scratching, it is necessary only to traverse the path programmed in
the incremental coordinates. The active zero offset or tool offset is not traversed. This can be
set separately using setting data.
Incremental dimensioning without traversing through the active tool offset
The active tool offset is not traversed if the setting datum
SD 42442: TOOL_OFFSET_INCR_PROG = 0.
Incremental dimensioning without traversing through the active zero offset
The active zero offset is not traversed if the setting datum
SD 42440: FRAME_OFFSET_INCR_PROG = 0
Positional Data
3.3 Absolute dimension for rotary axes (DC, ACP, ACN)
Fundamentals
86 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.3 Absolute dimension for rotary axes (DC, ACP, ACN)
With the above parameters you can define the desired approach strategy for positioning
rotary axes.
Programming
A=DC(…) B=DC(…) C=DC(…)
Or
A=ACP(…) B=ACP(…) C=ACP(…)
Or
A=ACP(…) B=ACP(…) C=ACP(…)
Parameters
A B C Axis identifier for rotary axis to be traversed
DC Absolute dimensions, approach position directly
ACP Absolute dimensions, approach position in positive direction
ACN Absolute dimensions, approach position in negative direction
Example of milling
Machining on a rotary table: The tool is stationary, the table rotates through 270° in
clockwise direction. to produce a circular groove.
=
;
;
<
r
Positional Data
3.3 Absolute dimension for rotary axes (DC, ACP, ACN)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 87
N10 SPOS=0 ;Spindle in position control
N20 G90 G0 X-20 Y0 Z2 T1 ;Absolute, infeed in rapid traverse
N30 G1 Z-5 F500 ;Lower at feedrate
N40 C=ACP(270) ;The table rotates through 270° in
;clockwise direction (positive), the tool
;mills a circular groove
N50 G0 Z2 M30 ;Lift, end of program
Absolute dimensioning with DC
The rotary axis travels to the position programmed in absolute coordinates along the shortest
direct path. The rotary axis traverses across an area of up to 180°.
Absolute dimensioning with ACP
The rotary axis travels to the position programmed in absolute coordinates in the positive
direction of axis rotation (counterclockwise).
Absolute dimensioning with ACN
The rotary axis travels to the positions programmed in absolute coordinates in the negative
direction of axis rotation (clockwise).
'&
$&3 $&1
0D[LPXP
7UDYHUVLQJUDQJH
Note
The traversing range must be set to between 0° and 360° in the machine data (modulo
method) for positioning with directional data (ACP, ACN). To traverse modulo rotary axes by
more than 360° in a block, G91 or IC must be programmed.
The positive direction of rotation (clockwise or counterclockwise) is set in the machine data.
All of the commands are non-modal.
Positional Data
3.4 Dimensions inch/metric, (G70/G700, G71/G710)
Fundamentals
88 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
You can also use DC, ACP and ACN for spindle positioning from zero speed.
Example: SPOS=DC(45)
3.4 Dimensions inch/metric, (G70/G700, G71/G710)
Function
Depending on the dimensions in the production drawing, you can program workpiece
geometries alternately in metric measurements and inches.
Programming
Call-up
G70 or G71
G700 or G710
Parameters
G70 Imperial measure (length [inches])
G71 Metric dimensions (length [mm])
G700 Imperial measure (length [inch]; feedrate [inch/min])
G710 Metric dimensions (length [mm]; feedrate F [mm/min])
G700/G710
The functionality of G70/G71 has been extended with G700/G710. In addition to the
geometrical parameters, the technological parameters, such as feed F, are interpreted
during parts program execution in the measuring system set in G700/G710.
The controller interprets all feedrates used with G700/G710 in the programmed measuring
system, unlike G70/G71.
The programmed feedrate value is modal and thus does not change automatically on
subsequent G70/G71/G700/G710 selections.
Positional Data
3.4 Dimensions inch/metric, (G70/G700, G71/G710)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 89
Example of milling
Change between metric and imperial input with basic setting metric (G70/G71).
;
<
*
* *
*
N10 G0 G90 X20 Y30 Z2 S2000 M3 T1 ;Basic setting metric
N20 G1 Z-5 F500 ;At feedrate in Z [mm/min]
N30 X90
N40 G70 X2.75 Y3.22 ;Enter destination positions in inches, G70
;is active until deselected by G71 or
;end of program
N50 X1.18 Y3.54
N60 G71 X 20 Y30 ;Enter positions in mm
N70 G0 Z2 M30 ;Retract in rapid traverse, end of program
Description
G70 or G71
You can instruct the control to convert the following geometrical dimensions (with necessary
deviations) into the measuring system not set and enter them directly:
Examples
• Positional data X, Y, Z, ...
• Interpolation point coordinates I1, J1, K1
Interpolation parameters I, J, K and circle radius
CR with circular-path programming
• Thread pitch (G34, G35)
• Programmable zero offset (TRANS)
• Polar radius RP
Positional Data
3.4 Dimensions inch/metric, (G70/G700, G71/G710)
Fundamentals
90 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
All other parameters such as feedrates, tool offsets or settable zero offsets are
interpreted (when using G70/G71) in the default measuring system
(MD 10240: SCALING_SYSTEM_IS_METRIC).
The representation of system variables and machine data is also independent of the
G70/G71 context.
If the feedrate in the G70/G71/G700/G710 context is to be activated, a new F value must be
programmed explicitly.
All length-related NC data, machine data and setting data for G700/G710 are always read
and written in the programmed context of G700/G710.
References:
/FB1/Function Manual Basic Functions; Speeds, Setpoint/Actual-Value System, Closed-Loop
Control (G2), "Metric/Inch Measuring System"
Synchronized actions
If positioning tasks are performed in synchronized actions and no G70/G71/G700/G710
command is programmed in the synchronized action itself, the G70/G71/G700/G710 context
active at the time of execution determines which measuring system is used.
References:
/PGA/Programming Manual Advanced; "Motion-Synchronous Actions"
/FBSY/Description of Functions, Synchronized Actions.
Positional Data
3.5 Special turning functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 91
3.5 Special turning functions
3.5.1 Dimensions for radius, diameter in the channel (DIAMON/OF, DIAM90)
Function
The free choice of diameter or radius dimensions allows you to program the dimensions
straight from the engineering drawing without conversion.
=
;
'
:
',$021
',$02)
'
=
;
5
5
:
After powerup of
• DIAMON, the dimensions for the specified transverse axis are given as a diameter value
independently of the type of travel (G90/G91).
• DIAM90, the dimensions are given as a diameter value (in the case of G90) or as a
radius value (in the case of G91) independently of the type of travel (G90/G91).
• DIAMON or DIAM90, the transverse-axis actual values will always be displayed as a
diameter. This also applies to reading of actual values in the workpiece coordinate
system with MEAS, MEAW, $P_EP[x] and $AA_IW[x].
Machine manufacturer
By means of machine data which is configurable by the machine manufacturer, geometry
axes can be enabled as transverse axes for channel-specific diameter programming.
Positional Data
3.5 Special turning functions
Fundamentals
92 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
Channel-specific modal switchover between diametral and radius programming
DIAMON
or
DIAMOF
or
DIAM90
Parameter
Diameter/radius modal Absolute dimensioning (G90) Incremental dimensioning
(G91)
DIAMON Diameter Diameter
DIAM90 Diameter Radius
Radius Radius
DIAMOF
(For default setting, see machine manufacturer)
Diameter values (DIAMON/DIAM90)
Diameter values apply to the following data:
• Actual-value display of transverse axis in the workpiece coordinate system
• JOG mode: Increments for incremental dimension and travel with handwheel
• Programming end positions,
interpolation parameters I, J, K (with G2/G3), if these are programmed absolutely with
AC. If I, J, K are programmed incrementally (IC), the radius is always calculated.
• Reading in of actual values into the workpiece coordinate system with
MEAS, MEAW, $P_EP[X], $AA_IW[X],
see /PGA/Programming Manual Advanced;
Special Motion Commands and Motion-Synchronous Actions
Example
N10 G0 X0 Z0 ;Approach starting point
N20 DIAMOF Diameter input off
N30 G1 X30 S2000 M03 F0.7 X axis = transverse axis; radius dimensions active
Traverse to radius position X30
N40 DIAMON ;All axes with $MA_BASE_FUNCTION_MASK
;diameter data active,
N50 G1 X70 Z-20 Traverse to diameter position X70 and
Z–20
N60 Z-30
N70 DIAM90 ;Diameter programming for absolute dimensions
and radius programming for incremental
dimensions
N80 G91 X10 Z-20 Incremental dimension
N90 G90 X10 Absolute dimensions
N100 M30 ; End of program
Positional Data
3.5 Special turning functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 93
Function
In addition to channel-specific diameter programming, there is also the axis-specific
diameter-programming function, which enables you to specify and display dimensions for
one or more axes as diameter values.
Dimensions can also be displayed simultaneously for several axes assigned to one channel.
After powerup of
• DIAMON[axis], the dimensions for the specified axis are given as a diameter value
independently of the type of travel (G90/G91 or AC/IC).
• DIAM90[axis], the dimensions for the specified axis are given as a diameter value (in the
case of G90/AC) or as a radius value (in the case of G91/IC) in accordance with the type
of travel (G90/G91 or AC/IC).
• DIAMON[axis] or DIAM90[axis], the transverse-axis actual values will always be
displayed as a diameter. This also applies to reading of actual values in the workpiece
coordinate system with MEAS, MEAW, $P_EP[x] and $AA_IW[x].
Machine manufacturer
By means of machine data which is configurable by the machine manufacturer, both axis-
specific modal diameter programming and action-based diameter programming can be
enabled. Please refer to the machine manufacturer's instructions.
Programming
Axis-specific modal diameter programming for several transverse axes in one channel
DIAMONA[axis]
or
DIAM90A[axis]
or
DIAMOFA[axis]
Channel-specific acceptance of diameter programming
DIAMCHANA[axis]
or
DIAMCHAN
Axis-specific action-based non-modal diametral/radius programming
Modal settings can be modified non-modally for specific axes by means of:
Diameter programming, non-modal, absolute or relative
DAC or DIC
or
Radius programming, non-modal, absolute or relative
RAC or RIC
Positional Data
3.5 Special turning functions
Fundamentals
94 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameter
Diametral/radius modal Absolute dimensioning (G90) Incremental dimensioning
(G91)
DIAMONA[axis] Diameter, axis-specific Diameter, axis-specific
DIAM90A[axis] Diameter, axis-specific Radius, axis-specific
Radius, axis-specific Radius, axis-specific
DIAMOFA[axis]
(For default setting, see machine manufacturer)
Axis The axis specified must have been assigned to the channel.
Permitted axis identifiers are as follows:
Geometry-/channel-axis name or machine-axis name.
Note: Rotary axes are not permitted to serve as transverse axes.
Accepting the channel-specific diameter programming
DIAMCHANA[axis] The specified axis adopts the diameter-programming channel
status.
DIAMCHAN All axes with the $MA_BASE_FUNCTION_MASK bit set for
diameter programming adopt the diametral-programming channel
status.
Axis-specific non-modal or action-based diameter programming
Specifies the dimension type as a diameter or radius value in the parts program and
synchronized actions. The modal status of diameter programming remains unchanged.
DAC Diameter programming, axis-spec., non-modal, absolute
DIC Diameter programming, axis-spec., non-modal, relative
RAC Radius programming, axis-specific, non-modal, absolute
RIC Radius programming, axis-specific, non-modal, relative
Diameter values (DIAMONA[AX]/DIAM90A[AX])
Diameter values apply to the following data:
• Actual-value display of transverse axis in the workpiece coordinate system
• JOG mode: Increments for incremental dimension and travel with handwheel
• Programming end positions,
interpolation parameters I, J, K (with G2/G3), if these are programmed absolutely with
AC.
If I, J, K are programmed incrementally (IC), the radius is always calculated.
• Reading in of actual values into workpiece coordinate system with
MEAS, MEAW, $P_EP[X], $AA_IW[X]
See /PGA/Programming Manual Advanced;
Special Motion Commands and Motion-Synchronous Actions
Note
Axis-specific acceptance of diameter programming in the other channel
Within the context of axis replacement, an additional transverse axis is accepted on the
basis of a GET request plus RELEASE [axis] with the diameter-programming status in the
other channel.
Example of axis-specific, modal diameter programming
Positional Data
3.5 Special turning functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 95
;X is the channel's transverse axis, axis-specific diameter programming is enabled
for Y:
N10 G0 X0 Z0 DIAMON ;Diameter programming for X active
N15 DIAMOF ;Channel-specific diameter programming deactivated
N20 DIAMONA[Y] ;Axis-specific diameter programming activated for Y
N25 X200 Y100 ;Radius programming active for X
N30 DIAMCHANA[Y] ;Y adopts the status of channel-specific ;diameter programming
;and becomes subject to this status
N35 X50 Y100 ;Radius programming active for X and Y
N40 DIAMON
N45 X50 Y100 ;Diameter programming active for X and Y
Example of axis-specific, non-modal diameter programming
;X is the channel's transverse axis, axis-specific diameter programming is enabled
for Y:
N10 DIAMON ;Diameter programming for X and Y active
N15 G0 G90 X20 Y40 DIAMONA[Y] ;Channel-specific diameter programming deactivated
N20 G01 X=RIC(5) ;X incremental dimension, radius, non-modal
N25 X=RAC(80) ;X absolute dimension, radius, non-modal
N30 WHEN $SAA_IM[Y]> 50 DO POS[X]=RIC(1) ;X is the command axis with incremental
;dimension (radius)
N40 WHEN $SAA_IM[Y]> 60 DO POS[X]=DAC(10) ;X is the command axis with absolute
;dimension (diameter)
N50 G4 F3
Description Channel-specific diameter programming DIAMCHANA[AX], DIAMCHAN
The DIAMCHANA[AX] or DIAMCHAN statement causes the specified axis or all the
transverse axes associated with axis-specific diameter programming to adopt the active
status of channel-specific diameter programming. These axes will subsequently be subject to
channel-specific diameter programming.
Axis-specific, non-modal/action-based diameter programming DAC, DIC, RAC, RIC
The statements define the dimension type non-modally in terms of either a radius or a
diameter value. The modal status of diameter programming, e.g., for display or system
variable purposes, remains unaffected by this.
These statements are permissible for any commands for which channel-specific diameter
programming is relevant:
• Axis position: X..., POS, POSA
• Oscillating: OSP1, OSP2, OSS, OSE, POSP
• Interpolation parameters: I, J, K
• Contour definition: Straight line with specified angle
• Rapid retraction: POLF[AX]
• Movement in tool direction: MOVT
• Smooth approach and retraction:
G140 to G143, G147, G148, G247, G248, G347, G348, G340, G341
Positional Data
3.5 Special turning functions
Fundamentals
96 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.5.2 Position of workpiece
Function
While the machine zero is fixed, you can choose the position for the workpiece zero on the
longitudinal axis. The workpiece zero is generally located on the front or rear side of the
workpiece.
:
0
**
0
:RUNSLHFH
0DFKLQH
:RUNSLHFH
]HUR
UHDU
:RUNSLHFH
]HUR
IURQW
:RUNSLHFH
:RUNSLHFH
:RUNSLHFH
0DFKLQH
;;
=
=
**RU75$16
;;
=
RU75$16
Zero points
Both the machine zero and the workpiece zero are positioned on the center of rotation. The
settable offset on the X axis is thus zero.
coordinate system
The dimensions for the transverse axis are generally specified as diameter measurements
(double path dimension as compared to other axes).
The geometry axis to be used as a transverse axis is defined in machine data.
Positional Data
3.5 Special turning functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 97
=
;
'
:
'
0
/RQJLWXGLQDOD[LV
7UDQVYHUVHD[LV
Parameters
G54 to G599 or TRANS Call for the position of the workpiece zero
M Machine zero
W Tool zero point
Z axis Longitudinal axis
X axis Transverse axis
The two mutually perpendicular geometry axes are usually designated as follows:
• Longitudinal axis= Z axis (abscissa)
• Transverse axis= X axis (ordinate)
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
98 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Function
The settable zero offset relates the workpiece zero on all axes to the origin of the basic
coordinate system.
It is, therefore, possible to call up cross-program zero points for different fixtures with a G
command.
Milling:
=
;
<
=
;
<
*
For turning, for example, the offset value for tightening the chuck is entered in G54.
Turning:
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 99
;
=
0:
*
Programming
Call-up
G54
Or
G55
Or
G56
Or
G57
Or
G505 … G599
Switching off
G53
Or
G500
Or
SUPA
Or
G153
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
100 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G54 to G57 Call the second to fifth settable zero offset/frame
G505 ...G599 Call the 6th to the 99th settable zero offset
G53 Non-modal deactivation of current settable zero offset and
programmable zero offset
G500 G500=zero frame, default setting,
(contains no offset, rotation, mirroring or scaling)
Deactivation of settable zero offsets/frames (G54 to G599) until the
next call.
Activation of the total basic frame ($P_ACTBFRAME).
G500 is not 0
Activation of first settable zero offset/frames ($P_UIFR[0]) and
Activation of total basic frame ($P_ACTBFRAME), or a modified basic
frame is activated.
SUPA Non-modal deactivation, including programmed offsets, handwheel
offsets (DRF), external zero offset and PRESET offset.
G153 Non-modal suppression of settable, programmable and total basic
frame
For more information please refer to Frame section.
Offset of the zero in the Cartesian coordinate system by frames such as
• Programmable zero offset, e.g., TRANS, ATRANS
• Programmable rotations, e.g., ROT, AROT
• Programmable scalings, e.g., SCALE, ASCALE
• Programmable mirrorings, e.g., MIRROR, AMIRROR
Example
In this example, three workpieces, arranged on a pallet according to the zero offset values
G54 to G56, are machined successively. The machining sequence is programmed in
subprogram L47.
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 101
<
;
*
*
*
<
0
;
0
<
;
<
;
75$16;0
N10 G0 G90 X10 Y10 F500 T1 ;Approach
N20 G54 S1000 M3 ;Call the first zero offset,
;spindle clockwise
N30 L47 ;Run program, in this case as a subprogram
N40 G55 G0 Z200 ;Call the second zero offset
;Z via obstacle
N50 L47 ;Run program as subprogram
N60 G56 ;Call third zero offset
N70 L47 ;Run program as subprogram
N80 G53 X200 Y300 M30 ;Suppress zero offset, ;end of program
Description
Setting the offset values
On the operator panel or universal interface, enter the following values in the internal control
zero offset table:
• Coordinates for the offset
• Angle for rotated clamping and
• Scale factors if necessary
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
102 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
<
;
<
2II FVHW
5RWDWH
6FDOLQJ
Switching on zero offset, G54 to G57
In the NC program, the zero offset is moved from the machine coordinate system to the
workpiece coordinate system by executing one of the four commands G54 to G57.
;
<
;
<
;
<
;
<
In the next NC block with a programmed movement, all of the positional parameters and thus
the tool movements refer to the workpiece zero, which is now valid.
Note
The 4 available zero offsets can be used, for example, for multiple machining operations, to
describe 4 workpiece clamping positions simultaneously and execute them in the program.
Positional Data
3.6 Zero offset frame, (G54 to G57, G505 to G599, G53, G500/SUPA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 103
Further settable zero offsets, G505 to G599
Command numbers G505 to G599 are available for this purpose. This enables you to create
up to 100 settable zero offsets in total, in addition to the 4 default zero offsets G54 to G57,
by using the machine data. They are stored in the zero point memory.
Deactivating a zero offset
Command G500 activates the first settable zero offset including basic offset, i.e., when zero
frame is selected as the default, the current settable zero offset is deactivated.
G53 suppresses the programmable and settable offset modally.
G153 has the same effect as G53 and also suppresses the total basic frame.
SUPA has the same effect as G153 and also suppresses the DRF offset, overlaid motions,
and external ZOs.
Note
The basic setting at program start, e.g., G54 or G500, can be set with machine data.
You will find more information on programmable zero offsets in the Frames section
"Programmable zero offset".
Positional Data
3.7 Selection of working plane (G17 to G19)
Fundamentals
104 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.7 Selection of working plane (G17 to G19)
Function
The specification of the working plane, in which the desired contour is to be machined also
defines the following functions:
• The plane for tool radius compensation.
• The infeed direction for tool length compensation depending on the tool type.
• The plane for circular interpolation.
=
<
;
,QIHHG
,QIHHG
,QIHHG
*
*
*
Programming
Call-up
G17
or
G18
or
G19
Parameter
G17 Working plane X/Y
Infeed direction Z Plane selection 1st - 2nd geometry axis
G18 Working plane Z/X
Infeed direction Y Plane selection 3rd - 1st geometry axis
G19 Working plane Y/Z
Infeed direction X Plane selection 2nd - 3rd geometry axis
Positional Data
3.7 Selection of working plane (G17 to G19)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 105
Note
In the default setting, G17 (X/Y plane) is defined for milling and G18 (Z/X plane) is defined
for turning.
When calling the tool path correction G41/G42 (see Section "Tool offsets"), the working
plane must be defined so that the controller can correct the tool length and radius.
Example of milling
The "conventional" approach with milling tool:
• Define working plane (G17 default setting for milling).
• Select tool type (T) and tool offset values (D).
• Switch on path correction (G41).
• Program traversing movements.
N10 G17 T5 D8 ;G17 Call the working plane, in this case: X/Y T,
;D tool call. Tool length compensation is
performed in the Z direction.
N20 G1 G41 X10 Y30 Z-5 F500 ;Radius compensation is performed in the X/Y
plane.
N30 G2 X22.5 Y40 I50 J40 ;Circular interpolation/tool radius compensation in
;the X/Y plane.
Positional Data
3.7 Selection of working plane (G17 to G19)
Fundamentals
106 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Description
It is advisable to define the working plane G17 to G19 at the beginning of the program. In the
default setting, the Z/X plane is preset for turning G18.
Turning:
*
*
<
;
=
*
For calculating the direction of rotation, the controller requires the specification of the
working plane, refer to circular interpolation G2/G3.
Machining on inclined planes
Rotate the coordinate system with ROT (see Section "Coordinate system offset") to position
the coordinate axes on the inclined surface. The working planes rotate accordingly.
Tool length compensation on inclined planes
As a general rule, the tool length compensation always refers to the fixed, non-rotated
working plane.
Positional Data
3.7 Selection of working plane (G17 to G19)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 107
Milling:
Note
The tool length components can be calculated according to the rotated working planes with
the functions for "Tool length compensation for orientable tools".
The offset plane is selected with CUT2D, CUT2DF. For further information on this and for the
description of the available calculation methods, refer to Section "Tool offsets"
The control provides convenient coordinate transformation functions for the spatial definition
of the working plane.
For further information, please refer to Section "Coordinate system offset".
Positional Data
3.8 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)
Fundamentals
108 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.8 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)
Function
G25/G26 limits the working area (working field, working space) in which the tool can traverse.
The areas outside the working area limitations defined with G25/G26 are inhibited for any
tool motion.
;
=
:RUNLQJDUHD
3URWHFWHG]RQH
:
0
The coordinates for the individual axes apply in the basic coordinate system:
=
<
*<
*<
*<
*;
*;
*=
*=
;
%DVLF
FRRUGLQDWH
&RQWURO
The working-area limitation for all validated axes must be programmed with the WALIMON
command. The WALIMOF command deactivates the working area limitation. WALIMON is the
default setting. Therefore, it only has to be programmed if the working area limitation has
been disabled beforehand.
Positional Data
3.8 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 109
Programming
G25 X…Y…Z… Programming in a separate NC block
Or
G26 X…Y…Z… Programming in a separate NC block
Or
WALIMON
Or
WALIMOF
Parameters
G25, X Y Z Lower working area limitation, value assignment in the channel axes
in the basic coordinate system
G26, X Y Z Upper working area limitation, value assignment in the channel axes
in the basic coordinate system
WALIMON Switch on working area limitation for all axes
WALIMOF Working area limitation switch-off for all axes
In addition to programming values using G25/G26, values can also be entered using
axis-specific setting data:
SD43420 $SA_WORKAREA_LIMIT_PLUS (Working-area limitation plus)
SD43430 $SA_WORKAREA_LIMIT_MINUS (Working-area limitation minus)
Activating and de-activating the working area limitation, parameterized using SD43420 and
SD43430, are carried-out for a specific direction using the axis-specific setting data that
becomes immediately effective:
SD43400 $SA_WORKAREA_PLUS_ENABLE (Working-area limitation active in the positive
direction)
SD43410 $SA_WORKAREA_MINUS_ENABLE (Working-area limitation active in the
negative direction)
Using the direction-specific activation/de-activation, it is possible to limit the working range
for an axis in just one direction.
Note
The programmed working area limitation, programmed with G25/G26, has priority and
overwrites the values entered in SD43420 and SD43430.
Note
G25/G26 can also be used to program limits for spindle speeds at the address S. For further
information, please refer to "Feed control and spindle motion".
Positional Data
3.8 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)
Fundamentals
110 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning
Using the working area limitation G25/26, the working area of a lathe is limited so that the
surrounding devices and equipment - such as revolver, measuring station etc. - are
protected against damage.
Default setting: WALIMON
;%
;
;
=%
:RUNLQJDUHD
3URWHFWHG]RQH
:
0
N10 G0 G90 F0.5 T1
N20 G25 X-80 Z30 ;Define the lower limit for
;the individual coordinate axes
N30 G26 X80 Z330 ;Define the upper limit
N40 L22 ;Cutting program
N50 G0 G90 Z102 T2 ;To tool change location
N60 X0
N70 WALIMOF ;Deactivate working area limitation
N80 G1 Z-2 F0.5 ;Drill
N90 G0 Z200 ;Back
N100 WALIMON ;Activate working area limitation
N110 X70 M30 ;End of program
Description
Reference point at the tool
When tool length compensation is active, the tip of the tool is monitored as reference point,
otherwise it is the toolholder reference point.
Consideration of the tool radius must be activated separately. This is done using channel-
specific machine data:
MD21020 $MC_WORKAREA_WITH_TOOL_RADIUS
If the tool reference point lies outside the working area defined by the working area limitation
or if this area is left, the program sequence is stopped.
Positional Data
3.9 Working area limitation in WCS/SZS (WALCS0 ... WALCS10)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 111
Note
If transformations are active, then tool data are taken into consideration (tool length and tool
radius) can deviate from the described behavior.
References:
/FB1/Function Manual, Basic Functions; Axis Monitoring, Protection Zones (A3),
Chapter: "Monitoring the working area limitation"
Programmable working area limitation, G25/G26
An upper (G26) and a lower (G25) working area limitation can be defined for each axis.
These values are effective immediately and remain effective for the corresponding MD
setting (→ MD10710 $MN_PROG_SD_RESET_SAVE_TAB) after RESET and after being
powered-up again.
Note
The CALCPOSI subroutine is described in the Job Planning Programming Manual Using this
subroutine before any traversing motion is made, it can be checked as to whether the
predicted path is moved through taking into account the working area limits and/or the
protection zones.
3.9 Working area limitation in WCS/SZS (WALCS0 ... WALCS10)
Function
In addition to the working area limitation with WALIMON (refer to "Working area limitation in
BCS") there is an additional working area limitation that is activated using the G commands
WALCS1 - WALCS10. Contrary to the working area limitation with WALIMON, the working area
here is not in the basis coordinate system, but is limited coordinate system-specific in the
workpiece coordinate system (WCS) or in the settable zero system (SZS).
Using the G commands WALCS1 - WALCS10, a data set (working area limitation group) is
selected under the up to 10 channel-specific data sets for the coordinate system-specific
working area limitations. A data set contains the limit values for all axes in the channel. The
limitations are defined by channel-specific system variables.
Application
The working area limitation with WALCS1 - WALCS10 ("Working area limitation in the
WCS/SZS") is mainly used for working area limitations for conventional lathes. They allow
the programmer, to use the defined "end stops" - when moving the axis "manually" to define
a working area limitation referred to the workpiece.
Positional Data
3.9 Working area limitation in WCS/SZS (WALCS0 ... WALCS10)
Fundamentals
112 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
The "working area limitation in the "WCS/SZS" is activated by selecting a working area
limitation group. G commands are used to make the selection:
WALCS1 Activating working area limitation group No. 1
...
WALCS10 Activating working area limitation group No. 10
The de-activation of the "working area limitation in the WCS/SZS" is realized using G
commands:
WALCS0 De-activating the active working area limitation group
Parameter
The working area limitations of the individual axes are set and the reference frame (WCS or
SZS), in which the working area limits are to be effective, activated with WALCS1 - WALCS10,
by writing to channel-specific system variables:
System variable Description
Setting the working area limits
$AC_WORKAREA_CS_PLUS_ENABLE [WALimNo, ax] Validity of the working area limitation in the positive axis
direction.
$AC_WORKAREA_CS_LIMIT_PLUS [WALimNo, ax] Working area limitation in the positive axis direction.
Only effective, if:
$AC_WORKAREA_CS_PLUS_ENABLE = TRUE
$AC_WORKAREA_CS_MINUS_ENABLE [WALimNo, ax] Validity of the working area limitation in the negative axis
direction.
$AC_WORKAREA_CS_LIMIT_MINUS [WALimNo, ax] Working area limitation in the negative axis direction.
Only effective, if:
$AC_WORKAREA_CS_PLUS_ENABLE = TRUE
Selecting the reference frame
Coordinate system to which the working area limitation
group is referred:
Value Description
1 Workpiece coordinate system (WCS)
$AC_WORKAREA_CS_COORD_SYSTEM [WALimNo]
3 Settable zero system (SZS)
<WALimNo>: Number of the working area limitation group.
<ax>: Channel axis name of the axis for which the value is valid.
Positional Data
3.9 Working area limitation in WCS/SZS (WALCS0 ... WALCS10)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 113
Example
3 axes are defined in the channel: X, Y and Z
A working area limitation group No. 2 is to be defined and then activated in which the axes
are to be limited in the WCS acc. to the following specifications:
• X axis in the plus direction: 10 mm
• X axis in the minus direction: No limitation
• Y axis in the plus direction: 34 mm
• Y axis in the minus direction: -25 mm
• Z axis in the plus direction: No limitation
• Z axis in the minus direction: -600 mm
...
N51 $AC_WORKAREA_CS_COORD_SYSTEM[2] = 1 ; The working area limitation of
working area limitation group 2
applies in the WCS.
N60 $AC_WORKAREA_CS_PLUS_ENABLE[2,X] = TRUE
N61 $AC_WORKAREA_CS_LIMIT_PLUS[2,X] = 10
N62 $AC_WORKAREA_CS_MINUS_ENABLE[2,X] = FALSE
N70 $AC_WORKAREA_CS_PLUS_ENABLE[2,Y] = TRUE
N73 $AC_WORKAREA_CS_LIMIT_PLUS[2,Y] = 34
N72 $AC_WORKAREA_CS_MINUS_ENABLE[2,Y] = TRUE
N73 $AC_WORKAREA_CS_LIMIT_MINUS[2,Y] = –25
N80 $AC_WORKAREA_CS_PLUS_ENABLE[2,Z] = FALSE
N82 $AC_WORKAREA_CS_MINUS_ENABLE[2,Z] = TRUE
N83 $AC_WORKAREA_CS_LIMIT_PLUS[2,Z] = –600
...
N90 WALCS2 ; Activating working area limitation
group No. 2.
...
Description
Effectivity
The working area limitation with WALCS1 - WALCS10 acts independently of the working area
limitation with WALIMON. If both functions are active, that limit becomes effective which the
axis motion first reaches.
Reference point at the tool
Taking into account the tool data (tool length and tool radius) and therefore the reference
point at the tool when monitoring the working area limitation corresponds to the behavior for
the working area limitation with WALIMON.
Positional Data
3.10 Reference point approach (G74)
Fundamentals
114 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
3.10 Reference point approach (G74)
Function
When the machine has been powered up (where incremental position measuring systems
are used), all of the axis slides must approach their reference mark. Only then can traversing
movements be programmed.
The reference point can be approached in the NC program with G74.
Programming
G74 X1=0 Y1=0 Z1=0 A1=0 … Programmed in a separate NC block
Parameter
G74 Reference point approach
X1=0 Y1=0 Y1=0…
A1=0 B1=0 C1=0…
The stated machine axis address
X1, Y1, Z1… Reference point approach for linear axes.
A1, B1, C1… Reference point approach for rotary axes.
Note
A transformation must not be programmed for an axis which is to approach the reference
point with G74.
The transformation is deactivated with command TRAFOOF.
Example
When the measurement system is changed, the reference point is approached and the
workpiece zero point is initialized.
N10 SPOS=0 ;Spindle in position control
N20 G74 X1=0 Y1=0 Z1=0 C1=0 ;Reference point approach for linear axes and
;rotary axes
N30 G54 ;Zero offset
N40 L47 ;Cutting program
N50 M30 ;End of program
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 115
Motion commands 4
4.1 General notes
In this section you will find a description of all the travel commands you can use to machine
workpiece contours.
These travel commands with the associated parameters enable you to program quite
different workpiece contours for milling and also for turning.
Travel commands for programmable workpiece contours
The programmed workpiece contours are composed of straight lines and circular arcs.
A helix can be produced by combining these two elements.
Executed in succession, these contour elements produce the workpiece contour.
A programming example is given for each travel command.
Programming more complex sequences of motions is also discussed. These are also
described with the possible variants or special cases.
The positional data contain all necessary geometric data serving for an unequivocal
representation of the positions in the corresponding coordinate systems. These are:
• Travel commands with specification of coordinates
• Rapid traverse movements to the end point
• Linear interpolation 3D surface processing
• Circular interpolation for full circles or circular arcs
• Helical interpolation
• Involute interpolation
• Thread cutting and tapping
• Interruptions both of approaching certain positions and traveling to these
• Special turning functions
• Chamfering or rounding off contour corners
Motion commands
4.1 General notes
Fundamentals
116 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Tool prepositioning
Before a machining process is started, you need to position the tool in such a way as to
avoid any damage to the tool or workpiece.
Start point - destination point
The traversing movement always runs from the last approached position to the programmed
destination position. This destination position is also the start position for the next travel
command.
Number of axis values
Depending on the control configuration, you can program motions for up to 8 axes in each
motion block. These may include path axes, synchronized axes, positioning axes, and
spindle oscillation mode.
Number of motion blocks in milling:
Motion commands
4.1 General notes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 117
Number of motion blocks in turning:
=
;
Caution
An axis address can only be programmed once in each block.
These commands can be programmed in Cartesian or polar coordinates. Synchronized
axes, positioning axes and oscillation mode.
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
118 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
4.2 Travel commands with polar coordinates, polar angle, polar radius
4.2.1 Defining the pole (G110, G111, G112)
Function
The dimensioning starting point is called a pole. The pole can be specified in either
Cartesian or polar coordinates (polar radius RP=... and polar angle AP=...). The
programming commands G110 to G112 are used to provide a unique definition of the
reference point for dimensions. Therefore, neither absolute nor incremental dimensioning
affects the system defined in the programming command.
Programming
G110 X… Y… Z… Pole parameter, with reference to the last approached position in
Cartesian coordinates
Or
G110 AP=… RP=… Pole parameter, with reference to the last approached pole in
polar coordinates
Or
G111 X… Y… Z… Pole parameter, absolute in workpiece coordinate system with
Cartesian coordinates
Or
G111 AP=… RP=… Pole parameter, absolute in workpiece coordinate system with
polar coordinates
Or
G112 X… Y… Z… Pole parameter, with reference to the last valid pole with
Cartesian coordinates
Or
G112 AP=… RP=… Pole parameter, with reference to the last valid pole with polar
coordinates
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 119
Parameters
G110 Polar programming relative to the last programmed setpoint position
G111 Polar programming relative to origin of current workpiece coordinate
system
G112 Polar programming relative to the last valid pole
X Y Z Coordinate identifiers of the axes to be traversed
AP= Polar angle, value range ±0…360°, angle refers to horizontal axis of
the working plane
RP= Polar radius in mm or inches always in absolute positive values.
Note
In the NC program you can switch non-modally between polar and Cartesian coordinates..
You come directly back into the Cartesian system by using the Cartesian coordinate
identifiers (X, Y, Z...). The defined pole is moreover retained up to program end.
Note
All the commands relating to pole input must be programmed in a separate NC block
If no pole is specified, the origin of the current coordinate system applies.
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
120 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of defining a pole with G110, G111, G112
The statement of the pole in Cartesian G110(X,Y), G111(X,Y) G112(X,Y) or polar
coordinates by stating G110, G111, G112 with polar angle AP= and polar radius RP=.
3ROH
3ROH
¡
*;
*<
*; *;
3ROH
¡
*<
*<
<
;
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 121
4.2.2 Traversing commands with polar coordinates, (G0, G1, G2, G3 AP=..., RP=...)
Function
The polar coordinate method is useful only if a workpiece or part of a workpiece has radius
and angle measurements. Polar coordinates can be used to program these dimensions
directly in accordance with the drawing.
If the dimensions of a workpiece, such as those in hole patterns, proceed from a central
point, then the dimensions are given in terms of angles and radii.
Q
P
r
r
r
r
r
<
;
Programming
G0 AP=… RP=…
Or
G1 AP=… RP=…
Or
G2 AP=… RP=…
Or
G3 AP=… RP=…
The new end position is defined relative to a pole, see defining the pole G110, G111, G112
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
122 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G0 Rapid traverse movement
G1 Linear interpolation
G2 Circular interpolation clockwise
G3 Circular interpolation counter-clockwise
AP= Polar angle, value range ±0…360°, the polar angle can be defined
both absolutely and incrementally.
RP= Polar radius in mm or inches always in absolute positive values.
=AC(...) Absolute dimensioning
=IC(...) Incremental dimensioning
Example of making a hole pattern
The positions of the holes are specified in polar coordinates.
Each hole is machined with the same production sequence: Predrilling, drilling to size,
reaming, etc. The machining sequence is filed in the subroutine.
<
;
r
r
r r
r
N10 G17 G54 ;Working plane X/Y, workpiece zero
N20 G111 X43 Y38 ;Define pole
N30 G0 RP=30 AP=18 Z5 ;Approach starting point, position in ;cylindrical
coordinates
N40 L10 ;Subprogram call
N50 G91 AP=72 ;Approach next position in rapid traverse, ;polar
angle in incremental dimensions, polar radius
;from block N30 is still stored and does not need
;to be specified
N60 L10 ;Subprogram call
N70 AP=IC(72) ;…
N80 L10 ;…
N90 AP=IC(72)
N100 L10 ;…
N110 AP=IC(72)
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 123
N120 L10 ;…
N130 G0 X300 Y200 Z100 M30 ;Retract tool, program end
N90 AP=IC(72)
N100 L10 ;…
Example of cylinder coordinates
The 3rd geometry axis, which lies perpendicular to the working plane, can also be specified
in Cartesian coordinates.
=
$3
53
This enables spatial parameters to be programmed in cylindrical coordinates.
Example: G17 G0 AP… RP… Z…
Traversing commands
The positions stated with polar coordinates can be approached with rapid traverse G0, linear
interpolation G1, circular interpolation clockwise G2 or counterclockwise G3.
Working plane
The polar coordinates are valid in the working plane selected with G17 to G19.
You must not program Cartesian coordinates, such as interpolation parameters or axis
addresses, for the selected working plane in NC blocks with polar end position coordinates.
Polar angle AP
When absolute dimensions are specified, the angular reference is based on the horizontal
axis of the working plane, e.g., X axis with G17. The positive direction of rotation is counter-
clockwise.
Motion commands
4.2 Travel commands with polar coordinates, polar angle, polar radius
Fundamentals
124 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
The polar angle can be defined both absolutely and incrementally.
When incremental coordinates are entered (AP=IC…), the last angle programmed is taken
as the reference. The polar angle is stored until a new pole is defined or the working plane is
changed.
If no pole is defined, then the origin of the current workpiece coordinate system is considered
as pole.
$3
$3
$3 ,&
r
r
;
<
Polar radius RP
The polar radius remains stored until a new value is input.
If the modally active polar radius is RP = 0
The polar radius is calculated from the distance between the starting point vector in the polar
plane and the active pole vector. The calculated polar radius is stored modally afterwards.
This applies irrespective of a selected pole definition such as G110, G111, G112. If both
points are programmed identically, this radius becomes 0 and alarm 14095 is generated.
If a pole angle AP is programmed with RP = 0
If the current block contains a polar angle AP rather than a polar radius RP and if there is a
difference between the current position and pole in workpiece coordinates, then this
difference is applied as the polar radius and stored modally. If the difference = 0, the pole
coordinates are specified again and the modal polar radius remains zero.
Motion commands
4.3 Rapid traverse movement (G0, RTLION, RTLIOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 125
4.3 Rapid traverse movement (G0, RTLION, RTLIOF)
Function
You can use the rapid traverse movements to position the tool rapidly, to travel round the
workpiece or to approach tool change locations.
Non-linear interpolation is activated using RTLIOF parts program commands; linear
interpolation is activated using RTLION.
Note
This function is not suitable for workpiece machining!
Programming
G0 X… Y… Z…
Or
G0 AP=…
Or
G0 RP=…
Or
RTLIOF
Or
RTLION
Parameters
G0 Rapid traverse movement
X Y Z End point in Cartesian coordinates
AP= End point in polar coordinates, in this case the polar angle
RP= End point in polar coordinates, in this case the polar radius
RTLIOF with G0 Nonlinear interpolation
(each path axis interpolates as a single axis)
RTLION with G0 Linear interpolation (path axes are interpolated together)
Note
G0 cannot be replaced with G.
G0 is modal.
Motion commands
4.3 Rapid traverse movement (G0, RTLION, RTLIOF)
Fundamentals
126 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of milling
;
<
1
1
Start positions or tool change points, retracting the tool, etc., are approached with G0.
N10 G90 S400 M3 ;Absolute dimensioning, spindle clockwise
N20 G0 X30 Y20 Z2 ;Approach start position
N30 G1 Z-5 F1000 ;Tool infeed
N40 X80 Y65 ;Travel on straight line
N50 G0 Z2
N60 G0 X-20 Y100 Z100 M30 ;Retract tool, program end
Example of turning
=
;
1
1
.
Motion commands
4.3 Rapid traverse movement (G0, RTLION, RTLIOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 127
N10 G90 S400 M3 ;Absolute dimensioning, spindle clockwise
N20 G0 X25 Z5 ;Approach start position
N30 G1 G94 Z0 F1000 ;Tool infeed
N40 G95 Z-7.5 F0.2
N50 X60 Z-35 ;Travel on straight line
N60 Z-50
N70 G0 X62
N80 G0 X80 Z20 M30 ;Retract tool, program end
Description
The tool movement programmed with G0 is executed at the highest possible speed (rapid
traverse). The rapid traverse speed is defined separately for each axis in machine data. If
the rapid traverse movement is executed simultaneously on several axes, the rapid traverse
speed is determined by the axis, which requires the most time for its section of the path.
3DWK
FRPSRQHQW=
3DWKFRPSRQHQW<
3DWKFRPSRQHQW;
3DWKRI
5DSLGWUDYHUVH
PRYHPHQW
<
;
=
Traversing path axes as positioning axes with G0
Path axes can travel in one of two different modes to execute movements in rapid traverse:
• Linear interpolation (behavior in earlier SW version):
The path axes are interpolated together.
• Non-linear interpolation:
Each pat axis is interpolated as an individual (positioning) axis independently of the other
axes involved in the rapid traverse movement.
With non-linear interpolation, the setting for the appropriate positioning axis BRISKA, SOFTA
or DRIVEA applies, with reference to the axial jerk.
Motion commands
4.3 Rapid traverse movement (G0, RTLION, RTLIOF)
Fundamentals
128 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Notice
Since a different contour can be traversed in nonlinear interpolation mode, synchronized
actions that refer to coordinates of the original path are not operative in some cases!
Linear interpolation applies in the following cases:
• With a G code combination including G0, which does not permit positioning movements
(e.g., G40/41/42).
• With a combination of G0 and G64
• When the compressor is active
• When a transformation is active
Example
G0 X0 Y10
G0 G40 X20 Y20
G0 G95 X100 Z100 m3 s100
Path POS[X]=0 POS[Y]=10 is traversed in path mode. No revolutional feedrate is active if
path POS[X]=100 POS[Z]=100 is traversed.
Settable block change time with G0
For single axis interpolations, a new movement end criterion
FINEA
Or
COARSEA
Or
IPOENDA
can already be set for block change inside the braking ramp.
Consecutive axes are handled in G0 like positioning axes.
With the combination of
• "Block change settable in the braking ramp of the single axis interpolation" and
• "Traversing path axes in rapid traverse movement as positioning axes with G0"
all axes can travel to their end point independently of one another. In this way, two
sequentially programmed X and Z axes are treated like positioning axes in conjunction with
G0.
The block change to axis Z can be initiated by axis X as a function of the braking ramp time
setting (100-0%). Axis Z starts to move while axis X is still in motion. Both axes approach
their end point independently of one another.
For further information, please refer to "Feed control and spindle motion".
Motion commands
4.4 Linear interpolation (G1)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 129
4.4 Linear interpolation (G1)
Function
With G1, the tool travels along straight lines that are parallel to the axis, inclined or in any
orientation in space. Linear interpolation permits machining of 3D surfaces, grooves, etc.
Milling:
Programming
G1 X… Y… Z … F…
Or
G1 AP=… RP=… F…
Parameters
G1 Linear interpolation with feedrate (linear interpolation)
X Y Z End point in Cartesian coordinates
AP= End point in polar coordinates, in this case the polar angle
RP= End point in polar coordinates, in this case the polar radius
F Feedrate in mm/min. The tool travels at feedrate F along a straight
line from the current starting point to the programmed destination
point. You can enter the destination point in Cartesian or polar
coordinates. The workpiece is machined along this path.
Example: G1 G94 X100 Y20 Z30 A40 F100
The end point on X, Y, Z is approached at a feedrate of 100 mm/min;
the rotary axis A is traversed as a synchronized axis, ensuring that all
four movements are completed at the same time.
Motion commands
4.4 Linear interpolation (G1)
Fundamentals
130 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
G1 is modal.
The spindle speed S and the direction of spindle rotation M3/M4 must be specified for
machining.
FGROUP can be used to define groups of axes, to which the path feed F applies. You will
find more information in the "Path behavior" section.
Example of milling
Machining of a groove: The tool travels from the starting point to the end point in the X/Y
direction. Infeed takes place simultaneously in the Z direction.
;=
<
<
N10 G17 S400 M3 ;Select working plane, spindle clockwise
N20 G0 X20 Y20 Z2 ;Approach start position
N30 G1 Z-2 F40 ;Tool infeed
N40 X80 Y80 Z-15 ;Travel along inclined
:straight line
N50 G0 Z100 M30 ;Retract to tool change point
Motion commands
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 131
Example of turning
<
;
;
;
<
;
=
N10 G17 S400 M3 ;Select working plane, spindle clockwise
N20 G0 X40 Y-6 Z2 ;Approach start position
N30 G1 Z-3 F40 ;Tool infeed
N40 X12 Y-20 ;Travel along inclined
;straight line
N50 G0 Z100 M30 ;Retract to tool change point
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Possibilities of programming circular movements
The control provides a range of different ways to program circular movements. This allows
you to implement almost any type of drawing dimension directly. The circular movement is
described by the:
• center point and end point in the absolute or incremental dimension (default)
• Radius and end point in Cartesian coordinates
• Opening angle and end point in Cartesian coordinates or center point under the
addresses
• Polar coordinates with the polar angle AP= and the polar radius RP=
• Intermediate and end point
• End point and tangent direction at the start point.
Motion commands
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Fundamentals
132 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
G2/G3 X… Y… Z…
I=AC(…) J=AC(…) K=AC(…) Absolute center point and end point with reference to the
workpiece zero
Or
G2/G3 X… Y… Z… I… J… K… Center point in incremental dimensions with reference to
the circle starting point
Or
G2/G3 X… Y… Z… CR=… Circle radius CR= and circle end position in Cartesian
coordinates X..., Y..., Z...
Or
G2/G3 X… Y… Z… AR=… Opening angle AR= end point in Cartesian coordinates
X..., Y..., Z...
Or
G2/G3 I… J… K… AR=… Opening angle AR= center point at addresses I...,
J..., K...
Or
G2/G3 AP=… RP=… Polar coordinates with the polar angle AP= and the polar
radius RP=
Or
CIP X… Y… Z… I1=AC(…)
J1=AC(…) K1=(AC…) The intermediate point at addresses I1=, J1=, K1=
Or
CT X… Y… Z… Circle through starting and end point and tangent
direction at starting point
Parameters
G2 Circular interpolation, CW
G3 Circular interpolation counterclockwise
CIP Circular interpolation through intermediate point
CT Circle with tangential transition defines the circle
X Y Z End point in Cartesian coordinates
I J K Circle center point in Cartesian coordinates in X, Y, Z direction
CR= Circle radius
AR= Opening angle
AP= End point in polar coordinates, in this case the polar angle
RP= End point in polar coordinates, in this case polar radius corresponding
to circle radius
I1= J1= K1= Intermediate points in Cartesian coordinates in X, Y, Z direction
Motion commands
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 133
Example of milling
The following program lines contain an example for each circular programming possibility.
The necessary dimensions are shown in the production drawing on the right.
;
,
-
<
r
N10 G0 G90 X133 Y44.48 S800 M3 ;Approach starting point
N20 G17 G1 Z-5 F1000 ;Tool infeed
N30 G2 X115 Y113.3 I-43 J25.52 ;Circle end point, center point in
;incremental dimensions
Or
N30 G2 X115 Y113.3 I=AC(90) J=AC(70) ;Circle end point, center point in
;absolute dimensions
Or
N30 G2 X115 Y113.3 CR=-50 ;Circle end point, circle radius
Or
N30 G2 AR=269.31 I-43 J25.52 ;Opening angle, center point in
;incremental dimensions
Or
N30 G2 AR=269.31 X115 Y113.3 ;Opening angle, circle end point
Or
N30 N30 CIP X80 Y120 Z-10 ;Circle end point and intermediate point:
I1= IC(-85.35)J1=IC(-35.35) K1=-6 ;Coordinates for all
;three geometry axes
N40 M30 ;End of program
Motion commands
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Fundamentals
134 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning
==
;;
r
r
N.. ...
N120 G0 X12 Z0
N125 G1 X40 Z-25 F0.2
N130 G3 X70 Y-75 I-3.335 K-29.25 ;Circle end point, center point in
;incremental dimensions
Or
N130 G3 X70 Y-75 I=AC(33.33) K=AC(-54.25) ;Circle end point, center point in
;absolute dimensions
Or
N130 G3 X70 Z-75 CR=30 ;Circle end point, circle radius
Or
N130 G3 X70 Z-75 AR=135.944 ;Opening angle, circle end point
Or
N130 G3 I-3.335 K-29.25 AR=135.944 ;Opening angle, center point in
;incremental dimensions
Or
N130 G3 I=AC(33.33) K=AC(-54.25)
AR=135.944
;Opening angle, center point in
;absolute dimensions
Or
N130 G111 X33.33 Z-54.25 ;Polar coordinates
N135 G3 RP=30 AP=142.326 ;Polar coordinates
Or
N130 CIP X70 Z-75 I1=93.33 K1=-54.25 ;Programming a circle with intermediate and
;end points
N140G1 Z-95
N.. ...
N40 M30 ;End of program
Motion commands
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 135
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=,
K=AC...)
Function
Circular interpolation enables machining of full circles or arcs.
The circular movement is described by:
• The end point in Cartesian coordinates X, Y, Z and
• the circle center point at addresses I, J, K.
If the circle is programmed with a center point but no end point, the result is a full circle.
Programming
G2/G3 X… Y… Z… I… J… K…
Or
G2/G3 X… Y… Z… I=AC(…) J=AC(…) K=(AC…)
Parameters
G2 Circular interpolation, CW
G3 Circular interpolation counterclockwise
X Y Z End point in Cartesian coordinates
I Coordinates of the circle center point in the X direction
J Coordinates of the circle center point in the Y direction
K Coordinates of the circle center point in the Z direction
=AC(…) Absolute dimensions (non-modal)
Motion commands
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...)
Fundamentals
136 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
G2 and G3 are modal.
The G90/G91 defaults for absolute or incremental dimensions are only valid for the circle
end point.
The center point coordinates I, J, K are normally entered in incremental dimensions with
reference to the circle starting point.
You program the absolute center point non-modally with reference to the workpiece zero
point with: I=AC(…), J=AC(…), K=AC(…). An interpolation parameter I, J, K with value 0 can
be omitted but the second associated parameter must always be specified.
Examples for milling
,
-
- $&
, $&
;
<
&LUFOH
HQGSRLQW
W
&LUFOH
VWDUWLQJSRLQW
Incremental dimension
N10 G0 X67.5 Y80.211
N20 G3 X17.203 Y38.029 I–.5 J–.211 F500
Absolute dimensions
N10 G0 X67.5 Y80.211
N20 G3 X17.203 Y38.029 I=AC(50) J=AC(50)
Motion commands
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 137
Examples for turning
=
;
Incremental dimension
N120 G0 X12 Z0
N125 G1 X40 Z-25 F0.2
N130 G3 X70 Z-75 I-3.335 K-29.25
N135 G1 Z-95
Absolute dimensions
N120 G0 X12 Z0
N125 G1 X40 Z-25 F0.2
N130 G3 X70 Z-75 I=AC(33.33) K=AC(-54.25)
N135 G1 Z-95
Motion commands
4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...)
Fundamentals
138 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Indication of working plane
=
;
<
*
*
*
The control needs the working plane parameter (G17 to G19) in order to calculate the
direction of rotation for the circle – G2 is clockwise or G3 is counterclockwise.
=
<
;
**
**
**
It is advisable to specify the working plane generally.
Exception:
You can also machine circles outside the selected working plane (not with arc angle and
helix parameters). In this case, the axis addresses that you specify as an end point
determine the circle plane.
Programmed feedrate
You can use FGROUP to specify, which axes are to be traversed with a programmed
feedrate. For more information please refer to the Path behavior section.
Motion commands
4.7 Circular interpolation with radius and end point (G2/G3, CR)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 139
4.7 Circular interpolation with radius and end point (G2/G3, CR)
The circular movement is described by the:
• Circle radius CR= and
• the end point in Cartesian coordinates X, Y, Z.
In addition to the circle radius, you must also specify the leading sign +/– to indicate whether
the traversing angle is to be greater than or less than 180°. A positive leading sign can be
omitted.
Note
There is no practical limitation on the maximum size of the programmable radius.
Programming
G2/G3 X… Y… Z… CR=
Or
G2/G3 I… J… K… CR=
Parameters
G2 Circular interpolation, CW
G3 Circular interpolation counterclockwise
X Y Z End point in Cartesian coordinates. These data depend on the motion
commands G90/G91 or ...=AC(...)/...=IC(..)
I J K Circle center point in Cartesian coordinates (in X, Y, Z direction)
The identifiers have the following meanings:
I: Coordinate of the circle center point in the X direction
J: Coordinate of the circle center point in the Y direction
K: Coordinate of the circle center point in the Z direction
CR= Circle radius
Here:
CR=+…: Angle less than or equal to 180°
CR=–…: Angle more than 180°
Note
You don't need to specify the center point with this procedure. Full circles (traversing angle
360°) cannot be programmed with CR=, but must be programmed using the circle end point
and interpolation parameters.
Example of milling
Programming a circle with radius and end point
Motion commands
4.7 Circular interpolation with radius and end point (G2/G3, CR)
Fundamentals
140 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N10 G0 X67.5 Y80.511
N20 G3 X17.203 Y38.029 CR=34.913 F500
;
<
&5
&5
&5
Example of turning
Programming a circle with radius and end point
N125 G1 X40 Z-25 F0.2
N130 G3 X70 Z-75 CR=30
N135 G1 Z-95
=
;
Motion commands
4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 141
4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)
The circular movement is described by:
• The opening angle AR = and
• the end point in Cartesian coordinates X, Y, Z or
• the circle center at addresses I, J, K
Programming
G2/G3 X… Y… Z… AR=
or
G2/G3 I… J… K… AR=
Parameter
G2 Circular interpolation, CW
G3 Circular interpolation, CCW
X Y Z End point in Cartesian coordinates
I J K Circle center in Cartesian coordinates (in X, Y, Z direction)
Key:
I: Coordinate of the circle center in the X direction
J: Coordinate of the circle center in the Y direction
K: Coordinate of the circle center in the Z direction
AR= Opening angle, range of values 0° to 360°
=AC(…) Absolute dimensioning (non-modal)
Note
Full circles (traversing angle 360°) cannot be programmed with AR=, but must be
programmed using the circle end position and interpolation parameters. The center point
coordinates I, J, K are normally entered in incremental dimensions with reference to the
circle starting point.
You program the absolute center point non-modally with reference to the workpiece zero
with: I=AC(…), J=AC(…), K=AC(…). An interpolation parameter I, J, K with value 0 can be
omitted but the second associated parameter must always be specified.
Motion commands
4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)
Fundamentals
142 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of milling
;
<
,
-
$SHUWXUHDQJOH
&LUFOH
VWDUWLQJSRLQW
¡
Programming a circle with opening angle and center point or end point
N10 G0 X67.5 Y80.211
N20 G3 X17.203 Y38.029 AR=140.134 F500
or
N20 G3 I–17.5 J–30.211 AR=140.134 F500
Example of turning
Z
X
54.25
54.25
25
25
95
95
Ø 33.33
Ø 33.33
30
30
Ø 40
Ø 40
1
4
2
.
3
2
6
°
Programming a circle with opening angle and center point or end point
N125 G1 X40 Z-25 F0.2
N130 G3 X70 Z-75 AR=135.944
Motion commands
4.9 Circular interpolation with polar coordinates (G2/G3, AP=, RP=)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 143
or
N130 G3 I-3.335 K-29.25 AR=135.944
or
N130 G3 I=AC(33.33) K=AC(-54.25) AR=135.944
N135 G1 Z-95
4.9 Circular interpolation with polar coordinates (G2/G3, AP=, RP=)
The circular movement is described by:
• The polar angle AP=
• and the polar radius RP=
The following rule applies:
The pole lies at the circle center.
The polar radius corresponds to the circle radius.
Programming
G2/G3 AP= RP=
Parameter
G2 Circular interpolation, CW
G3 Circular interpolation, CCW
X Y Z End point in Cartesian coordinates
AP= End point in polar coordinates, in this case the polar angle
RP= End point in polar coordinates, in this case polar radius corresponds
to circle radius
Motion commands
4.9 Circular interpolation with polar coordinates (G2/G3, AP=, RP=)
Fundamentals
144 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of milling
*
;
<
53
$
3
r
Programming a circle with polar coordinates
N10 G0 X67.5 Y80.211
N20 G111 X50 Y50
N30 G3 RP=34.913 AP=200.052 F500
Example of turning
Z
X
54.25
54.25
25
25
95
95
Ø 33.33
Ø 33.33
30
30
Ø 40
Ø 40
1
4
2
.
3
2
6
°
Programming a circle with polar coordinates
N125 G1 X40 Z-25 F0.2
N130 G111 X33.33 Z-54.25
N135 G3 RP=30 AP=142.326
N140 G1 Z-95
Motion commands
4.10 Circular interpolation with intermediate and end points (CIP)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 145
4.10 Circular interpolation with intermediate and end points (CIP)
You can use CIP to program arcs. These arcs can also be inclined in space. In this case,
you describe the intermediate and end points with three coordinates.
The circular movement is described by:
• The intermediate point at addresses I1=, J1=, K1= and
• the end point in Cartesian coordinates X, Y, Z.
;
<
,
-
<
.
=
,QWHUPHGLDWHSRLQW
The traversing direction is determined by the order of the starting point, intermediate point
and end point.
Programming
CIP X… Y… Z… I1=AC(…) J1=AC(…) K1=(AC…)
Parameters
CIP Circular interpolation through intermediate point
X Y Z End point in Cartesian coordinates. These data depend on the motion
commands G90/G91 or ...=AC(...)/...=IC(..)
I1= J1= K1= Circle center point in Cartesian coordinates (in X, Y, Z direction)
The identifiers have the following meanings:
I: Coordinate of the circle center point in the X direction
J: Coordinate of the circle center point in the Y direction
K: Coordinate of the circle center point in the Z direction
=AC(…) Absolute dimensions (non-modal)
=IC(...) Incremental dimensions (non-modal)
Motion commands
4.10 Circular interpolation with intermediate and end points (CIP)
Fundamentals
146 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
CIP is modal.
Input in absolute and incremental dimensions
The G90/G91 defaults for absolute or incremental dimensions are valid for the intermediate
and circle end points.
With G91, the circle starting point is used as the reference for the intermediate point and end
point.
Example of milling
;
=
<<
In order to machine an inclined circular groove, a circle is described by specifying the
intermediate point with 3 interpolation parameters, and the end point with 3 coordinates.
N10 G0 G90 X130 Y60 S800 M3 ;Approach starting point
N20 G17 G1 Z-2 F100 ;Tool infeed
N30 CIP X80 Y120 Z-10 ;Circle end point and intermediate point:
I1= IC(-85.35)J1=IC(-35.35) K1=-6 ;Coordinates for all three geometry axes
N40 M30 ;End of program
Motion commands
4.11 Circular interpolation with tangential transition (CT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 147
Example of turning
=
;
N125 G1 X40 Z-25 F0.2
N130 CIP X70 Z-75 I1=IC(26.665)
K1=IC(-29.25)
or
N130 CIP X70 Z-75 I1=93.33 K1=-54.25
N135 G1 Z-95
4.11 Circular interpolation with tangential transition (CT)
Function
The Tangential transition function is an expansion of the circle programming.
The circle is defined by
• the start and end point and
• the tangent direction at the start point.
The G code CT produces an arc that lies at a tangent to the contour element programmed
previously.
Motion commands
4.11 Circular interpolation with tangential transition (CT)
Fundamentals
148 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
$UF6(DWDWDQJHQWWRWKH
VWUDLJKWOLQH
6
(
/
/
/
6
(
&7
&7
&7
$UFVWKDWOLHDWDWDQJHQWGHSHQG
RQWKHSUHYLRXVFRQWRXUHOHPHQW
Determining the direction of the tangent
The direction of tangent at the start point of a CT block is determined from the end tangent of
the programmed contour of the previous block with a traversing movement.
Any number of blocks without traversing information may lie between this block and the
current block.
Programming
CT X… Y… Z…
Parameters
CT Circle with tangential transition
X Y Z End point in Cartesian coordinates
Note
CT is modal.
As a rule, the circle is uniquely defined by the direction of the tangent, as well as the start
and end points.
Motion commands
4.11 Circular interpolation with tangential transition (CT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 149
Example of milling
;
<
ZLWK75&
Milling a circular arc with CT following a straight line:
N10 G0 X0 Y0 Z0 G90 T1 D1
N20 G41 X30 Y30 G1 F1000 ;Activate tool radius compensation (TRC)
N30 CT X50 Y15 ;Program circle with tangential ;transition
N40 X60 Y-5
N50 G1 X70
N60 G0 G40 X80 Y0 Z20
N70 M30
Example of turning
=
;
Motion commands
4.12 Helical interpolation (G2/G3, TURN=)
Fundamentals
150 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N110 G1 X23.293 Z0 F10
N115 X40 Z-30 F0.2
N120 CT X58.146 Z-42 ;Program circle with tangential ;transition
N125 G1 X70
Description
In the case of splines, the tangential direction is defined by the straight line through the last
two points. This direction is generally not the same as the direction at the end point of the
spline with A and C splines with active ENAT or EAUTO.
The transition of B splines is always tangential, the tangent direction is defined as for A or C
splines and active ETAN.
Frame change
If a frame change takes place between the block defining the tangent and the CT block, the
tangent is also subjected to this change.
Limit case
If the extension of the start tangent runs through the end point, a straight line is produced
instead of a circle (limit case: circle with infinite radius). In this special case, TURN must
either not be programmed or the value must be TURN=0.
Note
When the values tend towards this limit case, circles with an unlimited radius are produced
and machining with TURN unequal 0 is generally aborted with an alarm due to violation of
the software limits.
Position of the circle plane
The position of the circle plane depends on the active plane (G17-G19).
If the tangent of the previous block does not lie in the active plane, its projection in the active
plane is used.
If the start and end points do not have the same position components perpendicular to the
active plane, a helix is produced instead of a circle.
4.12 Helical interpolation (G2/G3, TURN=)
Function
Helical interpolation (helix interpolation) can be used to manufacture threads and oil grooves,
for example.
Motion commands
4.12 Helical interpolation (G2/G3, TURN=)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 151
In helical interpolation, two movements are superimposed and executed in parallel:
• A horizontal circular movement, on which
• a vertical linear movement is superimposed.
Motion commands
4.12 Helical interpolation (G2/G3, TURN=)
Fundamentals
152 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
G2/G3 X… Y… Z… I… J… K… TURN=
Or
G2/G3 X… Y… Z… I… J… K… TURN=
Or
G2/G3 AR=… I… J… K… TURN=
Or
G2/G3 AR=… X… Y… Z… TURN=
Or
G2/G3 AP… RP=… TURN=
Parameters
G2 Travel on a circular path in clockwise direction
G3 Travel on a circular path in counterclockwise direction
X Y Z End point in Cartesian coordinates
I J K Circle center point in Cartesian coordinates
AR Opening angle
TURN= Number of additional circle passes within the range 0 to 999
AP= Polar angle
RP= Polar radius
Note
G2 and G3 are modal.
The circular movement is performed on the axes specified by the working plane.
Motion commands
4.12 Helical interpolation (G2/G3, TURN=)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 153
Example
;
=
<<
N10 G17 G0 X27.5 Y32.99 Z3 ;Approach start position
N20 G1 Z-5 F50 ;Tool infeed
N30 G3 X20 Y5 Z-20 I=AC(20)
J=AC (20) TURN=2
;Helix with following parameters: Execute ;2 full
circles from start position,
;then approach end point
N40 M30 ;End of program
Sequence of motions
1. Approach starting point
2. With TURN= execute the full circles programmed
3. Approach circle end position, e.g., as part rotation
4. Execute steps 2 and 3 across the infeed depth.
The pitch, with which the helix is to be machined is calculated from the number of full circles
plus the programmed circle end position (executed across the infeed depth).
Motion commands
4.12 Helical interpolation (G2/G3, TURN=)
Fundamentals
154 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
6WDUWSRLQW
VW)XOOFLUFOH
QG)XOOFLUFOH
UG)XOOFLUFOH
(QGSRLQWDV
SDUWLDOURWDWLRQ
7DUJHWSRLQW
Programming the end point for helical interpolation
Please refer to circular interpolation for a detailed description of the interpolation parameters.
Programmed feedrate
For helical interpolation, it is advisable to specify a programmed feedrate override (CFC).
You can use FGROUP to specify, which axes are to be traversed with a programmed
feedrate. For more information please refer to the Path behavior section.
Motion commands
4.13 Involute interpolation (INVCW, INVCCW)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 155
4.13 Involute interpolation (INVCW, INVCCW)
Function
The involute of the circle is a curve traced out from the end point on a "piece of string"
unwinding from the curve. Involute interpolation allows trajectories along an involute. It takes
place in the plane, in which the base circle is defined. Start and end points outside this plane
result in superimposition on a curve in space, analogous to helical interpolation with circles.
;
<
;< 0;<
5
ȬȬ
%DVHFLUFOH
6WDUWSRLQW
(QGSRLQW
When paths perpendicular to the active plane are also programmed, it is possible to traverse
an involute in space (comparable to helical interpolation with circles).
Programming
INVCW X... Y... Z... I... J... K... CR=...
Or
INVCCW X... Y... Z... I... J... K... CR=...
Or
INVCW I... J... K... CR=... AR=...
Or
INVCCW I... J... K... CR=... AR=...
Motion commands
4.13 Involute interpolation (INVCW, INVCCW)
Fundamentals
156 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
INVCW Travel on an involute in clockwise direction
INVCCW Travel on an involute path in counterclockwise direction
X Y Z End point in Cartesian coordinates
I J K Center point of base circle in Cartesian coordinates
CR= Radius of base circle
AR= Opening angle (angle of rotation)
Supplementary condition
Both the start point and the end point must be outside the area of the base circle of the
involute (circle with radius CR around the center point determined by I, J and K). If this
condition is not fulfilled, an alarm is generated and the program run aborted.
Note
For more information about machine data and supplementary conditions that are relevant to
involute interpolation, please see References: /FB1/, A2 section "Settings for involute
interpolation".
Example of counterclockwise involute and back as clockwise involute
Counterclockwise involute according to programming method 1 from start to end point and
back again (clockwise involute)
; <
1VWDUWSRLQW
1HQGSRLQW
; <
5
1
1
<
;
N10 G1 X10 Y0 F5000 ;Approach start position
N15 G17 ;Select X/Y plane
Motion commands
4.13 Involute interpolation (INVCW, INVCCW)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 157
N20 INVCCW X32.77 Y32.77 CR=5 I-10 J0 ;E. counterclockwise, end point, radius,
;center point relative to start point
N30 INVCW X10 Y0 CR=5 I-32.77 J-32.77 ;Start point is end point from N20
;End point is start point from N20,
;radius, center point relative to new
;start point is equal to previous
;center point
...
Example of counterclockwise involute with end point over angle of rotation
Specification of end point via angle of rotation
; <
$5
5
<
;
6WDUWLQJ
SRLQW
N10 G1 X10 Y0 F5000 ;Approach start position
N15 G17 ;Select X/Y plane
N20 INVCCW CR=5 I-10 J0 AR=360 ;Counterclockwise involute, away from base
;circle (pos. angle setting) with
;one full rotation
...
Description
Programming methods
1. Direct programming of the end point with X, Y or X, Y, Z
2. Programming of the angle of rotation between the start and end vectors with AR=angle
(cf. also programming of the arc angle when programming circles). If the angle of rotation
is positive (AR > 0), the path on the involute moves away from the base circle; with a
negative angle of rotation (AR < 0), the path on the involute moves towards the base
circle. The maximum angle of rotation for AR < 0 is restricted by the fact that the end
point must always lie outside the base circle.
Motion commands
4.13 Involute interpolation (INVCW, INVCCW)
Fundamentals
158 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
$5
(QGSRLQWV
6WDUWSRLQW
Options 1. and 2. are mutually exclusive. Only one of these notations may be used each
block.
Further information
There are further options when the angle of rotation is programmed with AR. Two different
involutes can be implemented (see diagram) by specifying the radius and center point of the
base circle as well as the start point and direction of rotation (INVCW/INVCCW). The
selected path must be defined unambiguously by the sign of the angle.
The two involutes defined by the start point and the base circle are shown in the diagram
above. In this case, end point 1 is approached when AR > 0 is programmed and end point
2 when AR < 0 is programmed.
Accuracy
If the programmed end point does not lie exactly on the involute defined by the start point
and base circle, interpolation takes place between the two involutes defined by the start or
end point (see diagram). The maximum deviation of the end point is determined by a
machine data. If the programmed end point deviates more in the radial direction than the MD
setting, an alarm is generated and the program run aborted.
56WDUWSRLQW
%DVHFLUFOH 0D[
GHYLDWLRQ
(QGSRLQW
Motion commands
4.14 Contour definitions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 159
4.14 Contour definitions
4.14.1 Straight line with angle (X2... ANG...)
Function
The end point is defined through specification of
• the angle ANG and
• one of the two coordinates X2 or Z2.
;=
;=
=
;
$1*
Programming
X2… ANG…
Parameters
X2 or Z2 End point in Cartesian coordinates X or Z
ANG Angle
Machine manufacturer
The names for angle (ANG), radius (RND) and chamfer (CHR) can be set in MD, see
/FBFA/FB ISO Dialects.
Motion commands
4.14 Contour definitions
Fundamentals
160 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example
N10 X5 Z70 F1000 G18 ;Approach start position
N20 X88.8 ANG=110 or (Z39.5 ANG=110) ;Straight line with specified angle
N30 ...
4.14.2 Two straight lines (ANG1, X3... Z3... ANG2)
Function
The intersection of the two straight lines can be designed as a corner, curve or chamfer. The
end point of the first of the two straight lines can be programmed by defining the coordinates
or specifying the angle.
$1*
;
=
;=
;=
$1*
;=
$1*
;
=
;=
;=
$1*
;=
&DQDOVREHUDGLXV&DQDOVREHUDGLXV
RUFKDPIHU
RU&+5RU&+5
Programming
ANG1…
X3… Z3… ANG2…
Or
X1… Z1…
X3… Z3…
Motion commands
4.14 Contour definitions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 161
Parameters
ANG1= Angle of the first straight line
ANG2= Angle of the second straight line
CHR Chamfer
X1, Z1= Start coordinates
X2, Z2= Intersection of the two straight lines
X3=, Z3= End point of the second straight line
Machine manufacturer
The names for angle (ANG), radius (RND) and chamfer (CHR) can be set in MD, see
/FBFA/FB ISO Dialects.
Example
N10 X10 Z80 F1000 G18 ;Approach start position
N20 ANG1=148.65 CHR=5.5 ;Straight line with specified angle and chamfer
N30 X85 Z40 ANG2=100 ;Straight line with specified angle and end point
N40 ...
4.14.3 Three straight lines (ANG1, X3... Z3... ANG2, X4... Z4...)
Function
The intersection of the straight lines can be designed as a corner, a curve, or a chamfer. The
end point of the third straight line must always be programmed as Cartesian.
$1*
=
;=
;=
$1*
;=
;= $1*
;;
=
;=
;=
$1*
;=
;=
&DQDOVREHUDGLXV&DQDOVREHUDGLXV
RUFKDPIHU
RU51'RU51'
RU&+5RU&+5
Motion commands
4.14 Contour definitions
Fundamentals
162 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
ANG1…
X3… Z3… ANG2…
X4… Z4…
Or
X2… Z2…
X3… Z3…
X4… Z4…
Parameters
ANG, ANG2= Angle of the first/second straight line relative to the abscissa
CHR Chamfer
RND Rounding
X1, Z1 Start coordinates of the first straight line
X2, Z2 End point coordinates of the first straight line or starting point of the
second straight line.
X3, Z3 End point coordinates of the second straight line or starting point of
the third straight line
X4=, Z4= Endpoint coordinates of the third straight line
Machine manufacturer
The names for angle (ANG), radius (RND) and chamfer (CHR) can be set in MD, see
/FBFA/FB ISO Dialects.
Example
N10 X10 Z100 F1000 G18 ;Approach start position
N20 ANG1=140 CHR=7.5 ;Straight line with specified angle and chamfer
N30 X80 Z70 ANG2=95.824 RND=10 Straight line on intersection with specified angle
and ;rounding
N40 X70 Z50 ;Straight line on end point
Motion commands
4.14 Contour definitions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 163
4.14.4 End point programming with angle
Function
If the address letter A appears in an NC block, either none, one or both of the axes in the
active plane may also be programmed.
Number of programmed axes
• If none of the axes in the active plane is programmed, the block is either the first or
second block of a contour consisting of two blocks.
If it is the second block in this type of contour, it indicates that the start and end points in
the active plane are identical. The contour then comprises at most a motion perpendicular
to the active plane.
• If exactly one axis in the active plane is programmed, then it is either a single straight
line, whose end point is uniquely defined by the angle and programmed Cartesian
coordinate, or it is the second block in a contour definition comprising two blocks. In the
latter case, the missing coordinate is set to match the last reached (modal) position.
• If two axes are programmed in the current plane, it is the second block of a contour that
consists of two blocks. If the current block was not preceded by a block with angle
programming and no programmed axes in the current plane, the block in question is not
permissible.
Angle A must only be programmed for linear or spline interpolation.
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
164 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
4.15 Thread cutting with constant lead (G33)
Function
With G33 three types of thread
• Cylinder thread
• Face thread
• Taper thread
can be produced with single or multiple threads as right-hand or left-hand thread.
Thread chains
By programming several G33 blocks consecutively, you can align several sets of threads in a
sequence. With G64 continuous-path mode, the blocks are interconnected in a look ahead
velocity control so that no speed jumps are produced.
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 165
=
;
QG6HW
ZLWK*
UG6HW
ZLWK*
VW6HW
ZLWK*
Right-hand/left-hand threads
Right-hand or left-hand threads are set according to the spindle direction:
M3: Clockwise
M4: CCW rotation
Programming
Cylinder thread
G33 Z… K … SF=…
Face thread
G33 X… I… SF=…
Taper thread
G33 X… Z… K… SF=…
Or
G33 X… Z… I… SF=…
Parameters
G33 Thread cutting with constant speed
X Y Z End point in Cartesian coordinates
I Thread lead in X direction
J Thread lead in Y direction
K Thread lead in Z direction
Z Longitudinal axis
X Transverse axis
Z... K... The thread length and thread lead for cylinder threads
X... I... Thread diameter and thread lead for face threads
I... K... The dominant direction share for tape thread in X or Z
K (taper thread) Lead angle <45°, thread lead in longitudinal direction
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
166 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
I (taper thread) Lead angle >45°, thread lead in transverse direction
I... or K... I or K can be stated at thread lead = 45°
SF= Starting point offset, only needed for multiple threads
Example of double cylinder thread with start point offset
Machining a double cylindrical thread in offset steps with starting point offset 180°.
=
;
6WDUWSRLQW¡
6WDUWSRLQW¡
É
N10 G1 G54 X99 Z10 S500 F100 M3 ;Zero offset, approach
;start point, spindle on
N20 G33 Z-100 K4 ;Cylindrical thread: end point in Z
N30 G0 X102
N40 G0 Z10
N50 G1 X99
;Retract to starting position
N60 G33 Z-100 K4 SF=180 ;2. cut: Starting point offset 180°
N70 G0 X110 ;Retract tool
N80 G0 Z10 ;End of program
N90 M30
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 167
Example of taper thread with angle less than 45°
Machining a taper thread
;
=
N10 G1 X50 Z0 S500 F100 M3 ;Approach starting point, activate spindle
N20 G33 X110 Z-60 K4 ;Taper thread: End point on Z and X,
;lead K in Z direction, since angle < 45°
N30 G0 Z0 M30 ;Retraction, end of program
Requirements
Equipment required: speed-controlled spindle with position measurement system.
Operating principle
The control calculates the required feedrate from the programmed spindle speed and the
thread lead. The turning tool traverses across the length of the thread in the longitudinal
and/or facing direction at this feedrate. The feedrate F is not considered for G33, the
limitation to maximum axis speed (rapid traverse) is monitored by the control.
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
168 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
)HHG
/HDG
6SLQGOHVSHHG
Cylinder thread
A cylinder thread is described by the thread length and thread lead.
The thread length is entered in absolute or incremental dimensions with one of the Cartesian
coordinates X, Y, or Z. The Z direction is preferred on turning machines. Allowance must
also be made for the run-in and run-out paths, across which the feed is accelerated or
decelerated.
The thread lead is entered at addresses I, J, K, on turning machines preferentially with K.
=
;
=
.
5XQLQSDWK
5XQRXWSDWK
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 169
Face thread
The face thread is described by
• Thread diameter, preferentially in X direction and
• Thread lead, preferentially with I.
Otherwise, the procedure is the same as for cylindrical threads.
,
;
/HDG
'LDPHWHU
Taper thread
The taper thread is described by the end point in the longitudinal and facing direction (taper
contour) and the thread lead.
The taper contour is entered in Cartesian coordinates X, Y, Z in absolute or incremental
dimensions - preferentially in the X and Z direction for machining on turning machines.
Allowance must also be made for the run-in and run-out paths, across which the feed is
accelerated or decelerated.
The parameter for the lead is based on the taper angle (calculated from the longitudinal axis
lead angle <45° to the outside of the taper lead angle >45°).
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
170 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
!r ,
;
=
r
.
;
=
Start point offset SF - production of multi-turn threads
Threads with offset cuts are programmed by specifying starting point offsets in the G33
block.
The start point offset is specified as an absolute angle position at address SF=. The
associated setting data is changed accordingly.
Example: SF=45
Meaning: Start offset 45°
Value range: 0.0000 to 359.999 degrees
;
=
6WDUWSRLQW
RIIVHWLQ¡
6WDUWDQJOH
IRUWKUHDG
VHWWLQJGDWD
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 171
Note
If no starting point offset is specified, the "starting angle for thread" defined in the setting
data is used.
4.15.1 Programmable run-in and run-out paths (DITS, DITE)
Function
The commands DITS (Displacement Thread Start) and DITE (Displacement Thread End)
can be used to define the path ramp for acceleration and deceleration, in order to modify the
feedrate if the tool run-in and run-out paths are too short:
• Run-in path too short:
The band at the thread run-in provides insufficient space for the tool start ramp - a shorter
ramp must therefore be defined with DITS.
• Run-out path too short
The band at the thread run-out provides insufficient space for the tool deceleration ramp,
giving rise to danger of collision between the workpiece and the tool edge.
A shorter tool deceleration ramp can be defined with DITE; however, a collision can still
occur.
Remedy: Program a shorter thread, reduce the spindle speed.
5XQLQUXQRXWSDWK
GHSHQGLQJRQGLUHFWLRQRI
PDFKLQLQJ
;
=
Programming
DITS=value
DITE=value
Motion commands
4.15 Thread cutting with constant lead (G33)
Fundamentals
172 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
DITS Thread run-in path
DITE Thread run-out path
Value Specification of the run-in and run-out path: -1.0,...n
Note
Only paths, and not positions, are programmed with DITS and DITE.
Machine manufacturer
The DITS and DITE commands are related to the setting data SD 42010:
THREAD_RAMP_DISP[0,1], in which the programmed paths are written. If no run-
in/deceleration path is programmed before or in the first thread block, the value is
determined by the setting in SD 42010, see:
References: /FB1/Function Manual Basic Functions; Feedrates (V1)
Example
N...
N40 G90 G0 Z100 X10 SOFT M3 S500
N50 G33 Z50 K5 SF=180 DITS=1 DITE=3 ;Start of corner rounding with Z=53
N60 G0 X20
Description
If the run-in and/or run-out path is very short, the acceleration of the thread axis is higher
than the configured value. This causes an acceleration overload on the axis.
In this case, alarm 22280 "Programmed run-in path too short" is output for the thread run-in
(if configured in MD 11411: ENABLE_ALARM_MASK). The alarm is purely for information
and has no effect on parts program execution.
MD 10710: PROG_SD_RESET_SAVE_TAB is used to set the value written by the parts
program into the corresponding setting data on RESET. The values are therefore retained
after power off/on.
Motion commands
4.16 Linear progressive/degressive thread pitch change (G34, G35)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 173
Note
DITE acts at the end of the thread as an approximate distance. This achieves a smooth
change in the axis movement.
When a block containing command DITS and/or DITE is loaded to the interpolator, the path
programmed in DITS is transferred to SD 42010: THREAD_RAMP_DISP[0] and the path
programmed in DITE to SD 42010 THREAD_RAMP_DISP[1].
The programmed run-in path is handled according to the current setting (inches, metric).
4.16 Linear progressive/degressive thread pitch change (G34, G35)
Function
You can use the functions G34/G35 to produce self-cutting threads.
Both the functions G34 and G35 offer the functionality of G33, but provide the additional
option of programming a pitch change under F.
Programming
G34 X… Y… Z… I… J… K… F…
Or
G34 X… Y… Z… I… J… K… SF=…
Or
G35 X… Y… Z… I… J… K… F…
Or
G35 X… Y… Z… I… J… K… SF=…
Parameters
G34 Progressive change in thread lead (tapping with linear pitch increase)
G35 Degressive change in thread lead (tapping with linear pitch decrease)
X Y Z End point in Cartesian coordinates
I Thread pitch in X direction
J Thread lead in Y direction
K Thread lead in Z direction
Motion commands
4.16 Linear progressive/degressive thread pitch change (G34, G35)
Fundamentals
174 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
F Thread lead change (in mm/rev2)
If you already know the initial and final lead of a thread, you can
calculate the lead change to be programmed according to the
following equation:
|k2e - k2a|
F = ------------- [mm/rev2]
2*IG
The identifiers have the following meanings:
Ke: thread lead of axis target point coordinate in [mm/rev]
Ka: initial thread pitch (progr. under I, J, and K) in [mm/rev]
IG: Thread length in [mm]
SF= Starting point offset, only needed for multiple threads
Example of lead decrease
N1608 M3 S10 ;Spindle speed
N1609 G0 G64 Z40 X216 ;Approach start point and thread
N1610 G33 Z0 K100 SF=R14 ;With constant pitch 100 mm/rev
N1611 G35 Z-200 K100 F17.045455 ;Lead decrease 17.0454 mm/rev2
;lead at block end 50 mm/rev
N1612 G33 Z-240 K50 ;Traverse thread block without jerk
N1613 G0 X218 ;
N1614 G0 Z40 ;
N1615 M17 ;
Motion commands
4.17 Tapping without compensating chuck (G331, G332)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 175
4.17 Tapping without compensating chuck (G331, G332)
Function
With G331/G332 you can rigid tap a thread.
The spindle prepared for tapping can make the following movements in position-controlled
operation with distance measuring system:
• G331 Tapping with thread lead in tapping direction up to end point
• G332 retraction movement with the same lead as G331
=
;
.
Right-hand/left-hand threads
Right-hand or left-hand threads are defined in axis mode by the sign qualifying the lead:
• Positive lead, clockwise (same as M3)
• Negative lead, counterclockwise (same as M4)
The desired speed is also programmed at address S.
Programming
G331 X… Y… Z… I… J… K…
Or
G332 X… Y… Z… I… J… K…
Motion commands
4.17 Tapping without compensating chuck (G331, G332)
Fundamentals
176 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G331 Tapping. Tapping is described by the drilling depth (end point of the
thread) and the lead.
G332 Tapping retraction. This movement is described with the same lead as
the G331 movement. The reversal in the direction of the spindle is
performed automatically.
X Y Z Drilling depth (end point) in a Cartesian coordinate Drilling in
X direction, thread lead I
Y direction, thread lead J
Z direction, thread lead K
I Thread pitch in X direction
J Thread lead in Y direction
K Thread lead in Z direction
Value range of lead:
±0.001 to 2000.00 mm/revolution
Note
Both functions G331/G332 are modal.
After G332 (retraction), the next thread can be tapped with G331.
Equipment required: position-controlled spindle with position measurement system.
The spindle must be prepared for tapping with SPOS/SPOSA. It does not work in axis
operation, but as position-controlled spindle, see section Feed control and spindle movement
"Position-controlled spindle operation"
Note
Machine manufacturer
A second gear-stage data record can be preset for two additional configurable switching
thresholds (maximum speed and minimum speed) via axis-specific machine data (this record
can differ from the first gear-stage data record and the speed switching thresholds in the two
records are regarded as completely separate). Please see the machine manufacturer’s
specifications for further details.
Outputting the programmed drilling speed in the current gear stage
The programmed drilling speed, e.g., S800, is output in the current gear stage and, where
necessary, is limited to the maximum speed of the gear stage. No automatic gear-stage
change is possible following an SPOS operation. In order for an automatic M40-gear-stage
change to be performed, the spindle must be in speed-control mode.
The appropriate gear stage for M40 is determined on the basis of the first gear-stage data
record.
Motion commands
4.17 Tapping without compensating chuck (G331, G332)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 177
N05 M40 S500 ;Gear stage 1 is engaged, as S500 (for example) is within
the range
; 20 to 1,028 rpm.
....
N55 SPOS=0 ;Position tool
N60 G331 Z-10 K5 S800 ;Produce thread, spindle speed is 800 rpm ;gear stage 1
Note
If gear stage 2 is selected at a spindle speed of 800 rpm, then the switching thresholds for
the maximum and minimum speed must be configured in the relevant machine data, see
examples below.
Using the second gear-stage data record for specifying two switching thresholds
The switching thresholds of the second gear-stage data record for the maximum and
minimum speed are evaluated modally for G331/G332 and when programming an S-value
for the active master spindle. Automatic M40-gear-stage change must be active.
The gear stage as determined in the manner described above is compared with the active
gear stage. If they are found to be different, a gear-stage change is performed.
N05 M40 S500 ;Gear stage 1 is selected
....
N50 G331 S800 ;Master spindle with 2nd gear-stage data record: ;Gear
stage 2 is selected
N55 SPOS=0 ;Align spindle
N60 G331 Z-10 K5 ;Modal tapping with G331, no ;reprogramming necessary
;spindle accelerated on basis of second data record
Motion commands
4.17 Tapping without compensating chuck (G331, G332)
Fundamentals
178 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
If no speed programmed, gear stage is monitored
If no speed is programmed with G331, then the speed and gear stage last programmed will
be used to produce the thread.
In this case, monitoring is performed to check that the programmed speed is within the
speed range defined by the maximum and minimum speed thresholds for the active gear
stage. Otherwise, alarm 16748 is signaled.
N05 M40 S800 ;Gear stage 1 is selected, the
;first gear-stage data record is active.
....
N55 SPOS=0
N60 G331 Z-10 K5 ;Spindle speed S800 with 2nd gear-stage data record is
;monitored. Gear stage 2 should be active;
;alarm 16748 is signaled
No gear-stage change can be performed, gear stage is monitored.
If the spindle speed is programmed in the G331 data record as well as the geometry, the
gear stage cannot be changed, as this would prevent the necessary path motion of the
spindle and infeed axis/axes from being achieved.
As in the example above, the speed and gear stage are monitored in the G331 data record.
Where necessary, alarm 16748 can be signaled.
N05 M40 S500 ;Gear stage 1 is selected
....
N55 SPOS=0
N60 G331 Z-10 K5 S800 ;No gear-stage change possible,
;spindle speed S800 with 2nd gear-stage data record is
;monitored. Gear stage 2 should be active;
;alarm 16748 is signaled
Motion commands
4.18 Tapping with compensating chuck (G63)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 179
4.18 Tapping with compensating chuck (G63)
Function
You can use G63 to tap threads with compensating chuck. The following are programmed:
• Drilling depth in Cartesian coordinates
• Spindle speed and spindle direction
• Feed
The chuck compensates for any deviations occurring in the path.
;
=
Retraction movement
Also programmed with G63, but with the reverse direction of spindle rotation.
Programming
G63 X… Y… Z…
Motion commands
4.18 Tapping with compensating chuck (G63)
Fundamentals
180 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G63 Tapping with compensating chuck.
X Y Z Drilling depth (end point) in a Cartesian coordinate
Note
G63 is non-modal.
The last programmed interpolation command G0, G1, G2, etc., is reactivated after a block
with programmed G63.
Feedrate
Note
The programmed feed must match the ratio of the speed to the thread lead of the tap.
Thumb rule:
Feed F in mm/min = spindle speed S
in rpm x thread lead in mm/rev
Both the feed and the spindle speed override switch are set to 100% with G63.
Example 1
N10 SPOS[n]=0 ;Prepare tapping
N20 G0 X0 Y0 Z2 ;Approach starting point
N30 G331 Z-50 K-4 S200 ;Tapping, drilling depth 50, lead K
;negative = direction of spindle rotation
counterclockwise
N40 G332 Z3 K-4 ;Retract, automatic reversal of direction
N50 G1 F1000 X100 Y100 Z100 S300 M3 ;Spindle reverts to operation in spindle mode
N60 M30 ;End of program
Motion commands
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 181
Example 2
In this example, an M5 thread is to be drilled. The lead of an M5 thread is 0.8 (specified in
table).
With a selected speed of 200 rpm, the feed F is 160 mm/min.
N10 G1 X0 Y0 Z2 S200 F1000 M3 ;Approach starting point, activate spindle
N20 G63 Z-50 F160 ;Tap, drilling depth 50
N30 G63 Z3 M4 ;Retract, programmed reversal of direction
N40 M30 ;End of program
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
4.19.1 Retraction for thread cutting (LFOF, LFON, LIFTFAST, DILF, ALF)
Function
The function produces a nondestructive interruption with thread cutting (G33). The function
cannot be used with tapping (G331/G332). With mixed use of both functions, the response
can be parameterized for NC Stop/NC Reset via the machine data. If tapping was
interrupted, then there are several possibilities of programming the fast retraction to a certain
lift position. Both the length of the retraction path and the retraction direction can be defined
as target position.
Programming
LFON
Or
LFOF
Where
LIFTFAST= (if enabled as option)
Or
DILF=
Or
ALF=
Motion commands
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
Fundamentals
182 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
LFON Enable fast retraction for thread cutting (G33)
LFOF Disable fast retraction for thread cutting (G33)
LIFTFAST Fast retraction option acts with LFON in every retraction direction
DILF Determine retraction path (length)
ALF Define retraction direction for plane to be executed (LFTXT)
Note
LFON or LFOF can always be programmed, they are evaluated only during thread cutting
(G33).
Example of enabling fast retraction in tapping
N55 M3 S500 G90 G18 ;Active machining plane
... ;Approach start position
N65 MSG ("thread cutting") ;Tool infeed
MM_THREAD:
N67 $AC_LIFTFAST=0 ;Reset before beginning of
;thread
N68 G0 Z5
N68 X10
N70 G33 Z30 K5 LFON DILF=10 LFWP ALF=3 ;Enable fast retraction for thread ;cutting
Retraction path =10mm, retraction plane Z/X (due to G18)
Retraction direction -X (with ALF=3; retraction direction +X)
N71 G33 Z55 X15 K5
N72 G1 ;Deselect thread cutting
N69 IF $AC_LIFTFAST GOTOB MM_THREAD ;If thread cutting was ;interrupted
N90 MSG ("")
...
N70 M30
Motion commands
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 183
Example of deactivating fast retraction before tapping.
N55 M3 S500 G90 G0 X0 Z0
...
N87 MSG ("tapping")
N88 LFOF ;Deactivate fast retraction before ;tapping.
N89 CYCLE... ;Tapping cycle with G33
N90 MSG ("")
...
N99 M30
Trigger criteria for retraction
• Fast inputs, programmable with SETINT LIFTFAST (if LIFTFAST option is enabled)
• NC Stop/NC Reset
If fast retraction is enabled with LFON, it is active for every movement
Retraction path (DILF)
The retraction path can be defined in the machine data or by programming. After NC Reset,
the value in MD 21200: LIFTFAST_DIST is still active.
Retraction direction (ALF)
The retraction direction is controlled in conjunction with ALF with keywords LFTXT, LFWP
and LFPOS . With LFTXT, the retraction is defined in the tool direction for ALF=1. LFTXT
(tangential lifting in tool direction) is set as default. See "Lifting in retraction with LFTXT,
LFWP, LFPOS, POLF, POLFMADK and POLFMLIN".
4.19.2 Lifting on retraction (LFTXT, LFWP, LFPOS, POLF, POLFMASK; POLFMLIN)
Function
With the LFTXT, LFWP, LFPOS; POLF commands you can selectively program on lifting the
retraction processing from the lift movement up to the lift position. The following are
programmed:
• Retraction direction from the path tangent or the active working plane
• Retraction direction toward position programmed
• Absolute retraction position
In this case, the axis relation of the programmed path or the linear retracting movement is
not always guaranteed for a certain period of time. The linear relation cannot always be
produced according to the dynamic behavior of all participating axes up to reaching the lift
Motion commands
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
Fundamentals
184 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
position. Axes can be enabled for independent retraction to axis position and to axis position
with linear relation.
Programming
LFTXT
Or
LFWP
Or
LFPOS
Or
POLF[geo axis name | machine axis name]=
Or
POLFMASK(axisname1, axisname2, etc.)
Or
POLFMLIN
Parameters
LFTXT Retraction direction on lifting from the path tangent, default
LFWP Retraction direction from the active working plane G17, G18, G19
LFPOS Retraction direction toward position programmed with POLF
POLF Absolute retraction position of axis, incl. incremental with IC (value)
POLF is modal.
POLFMASK Enable for axes for independent retraction to absolute position
POLFMLIN Enable for axes for retraction to absolute position in linear
relationship. See also /FB3/Function Manual Special Functions;
Coupled Axes and ESR (M3)
X, Y, Z Geometry axes in POLF are interpreted as position in the tool
coordinate system (TCS).
X1, Y1, Z1 Machine axes in POLF are interpreted as position in the machine
coordinate system (MCS).
Motion commands
4.19 Stop with thread cutting (LFOF, LFON, LFTXT, LFWP, LFPOS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 185
Example
Here, the path interpolation of X is suppressed in the event of a stop and a motion executed
to position POLF[X] at maximum velocity instead. The motion of the other axes continues to
be determined by the programmed contour or the thread lead and spindle speed.
N10 G0 G90 X200 Z0 S200 M3
N20 G0 G90 X170
N22 POLF[X]=210 LFPOS
N23 POLFMASK(X) ;Activate (enable)
;rapid lift of
;the axis X
N25 G33 X100 I10 LFON
N30 X135 Z-45 K10
N40 X155 Z-128 K10
N50 X145 Z-168 K10
N55 X210 I10
N60 G0 Z0 LFOF
N70 POLFMASK() ;Block retraction for all axes
M30
Description
The retraction direction in connection with ALF is controlled using the following keywords:
• LFTXT
The plane in which the fast retraction is executed is calculated from the path tangent and
the tool direction (default setting).
• LFWP
The plane in which the fast retraction is executed is the active working plane.
• LFPOS
Retraction of the axis declared with POLFMASK to the absolute axis position
programmed with POLF. See also NC-controlled retraction in /FB3/Function Manual
Special Functions; Coupled Axes and ESR (M3).
ALF has no influence on the retraction direction on several axes or on several axes in
linear relation.
The direction is programmed as before in discrete steps of 45 degrees with ALF in the plane
of the retraction motion. With LFTXT, the retraction is defined in the tool direction for ALF=1.
With LFWP the direction in the working plane is derived from the following assignment:
• G17: X/Y plane
ALF=1 Retraction in X direction
ALF=3 Retraction in Y direction
• G18: Z/X plane
ALF=1 Retraction in Z direction
ALF=3 Retraction in X direction
Motion commands
4.20 Approaching a fixed point (G75)
Fundamentals
186 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
• G19: Y/Z plane
ALF=1 Retraction in Y direction
ALF=3 Retraction in Z direction
Retraction velocity
Retraction with maximum axis velocity.
Can be configured via machine data.
The maximum permissible acceleration/jerk values are used for traversing; they are
configured via the machine data.
Note
POLF with POLFMASK/POLFMLIN are not restricted to thread cutting applications. See
/FB3/Function Manual Special Functions; Coupled Axes and ESR (M3).
4.20 Approaching a fixed point (G75)
Function
G75 can be used to approach fixed points, such as tool change locations, loading points,
pallet changing points, etc.
The positions of the individual points are specified in the machine coordinate system and
stored in the machine parameters.
You can approach these positions from any NC program, irrespective of the current tool or
workpiece position.
Programming
G75 FP= X1=0 Y1=0 Z1=0 U1=0 …
Parameters
G75 Fixed point approach
The fixed point approach is described by a fixed point and axes, which
are to be traversed to the fixed point FP.
FP= Number of fixed point to be approached
Number of the fixed point FP=...
If no fixed point number is specified, fixed point 1 is automatically
approached.
Motion commands
4.20 Approaching a fixed point (G75)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 187
X1= Y1= Z1= Machine axes to be traversed to the fixed point
Machine axis addresses X1, Y1 ...
Here, you specify with value 0 the axes, with which the point is to be
approached simultaneously. Each axis traverses at the maximum
axial velocity.
Note
Two fixed point positions per machine axis can be specified in the machine parameters.
G75 is non-modal.
G75 "Approach fixed point" applies all offset values (DRF, external ZO and overlaid motion).
The fixed point corresponds to the actual value in the MCS.
Changes to the DRF and external zero offset while the G75 block is being preprocessed and
executed in the main run are not applied. You should prevent this problem by programming
STOPPRE in front of the G75 block.
Kinematic transformation must be deselected before fixed point approach is performed.
Example
The tool change location is a fixed point, which is defined in the machine data.
This point can be approached in any NC program with G75.
N10 G75 FP=2 X1=0 Y1=0 Z1=0 ;Retract from fixed point 2 on X, Y and Z,
;e.g., for tool change
N20 G75 X1=0 ;Approach fixed point X1
N30 M30 ;End of program
Motion commands
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Fundamentals
188 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Function
The "travel to fixed stop" (FXS = Fixed Stop) function can be used to build defined forces for
clamping workpieces, such as those required for tailstocks, quills and grippers. The function
can also be used for the approach of mechanical reference points.
3URJUDPPHG
(QGSRVLWLRQ
)L[HGVWRS
0RQLWRULQJZLQGRZ
6WDUWSRVLWLRQ
$FWXDOSRVLWLRQDIWHU
7UDYHOWRIL[HGVWRS
With sufficiently reduced torque, it is also possible to perform simple measurement
operations without connecting a probe. The "travel to fixed stop" function can be
implemented for axes as well as for spindles with axis-traversing capability.
Programming
FXS [axis]=…
FXST [axis]=…
FXSW [axis]=…
Motion commands
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 189
Parameters
FXS Select/deselect "travel to fixed stop" function
= select; 0 = deselect
FXST Setting clamping torque
Specification in % of maximum drive torque, parameter optional
FXSW Window width for fixed stop monitoring in mm, inches or degrees;
parameter optional
[axis] Machine axis name
Machine axes (X1, Y1, Z1, etc.) are programmed.
(See machine manufacturer's specifications).
Note
The commands are modal. Addresses FXST and FXSW are optional: If no parameter is
specified, the last programmed value or the value set in the relevant machine data applies.
Example of activating travel to fixed stop FXS=1
The movement to the destination point can be described as a path or positioning axis
movement. With positioning axes, the function can be performed across block boundaries.
Travel to fixed stop can be performed simultaneously for several axes and parallel to the
movement of other axes. The fixed stop must be located between the start and end
positions.
X250 Y100 F100 FXS[X1]=1 FXST[X1]=12.3 FXSW[X1]=2
Meaning:
Axis X1 travels with feed F100 (parameter optional) to destination position X=250 mm.
The clamping torque is 12.3% of the maximum drive torque. Monitoring is performed in a 2
mm wide window.
Caution
It is not permissible to program a new position for any axis/spindle for the "Travel to fixed
stop" function has already been activated
Spindles must be switched to position-controlled mode before the function is selected.
Motion commands
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Fundamentals
190 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of deactivating travel to fixed end stop FXS=0
Deselection of the function triggers a preprocessing stop.
Traversing movements may and should be programmed in a block with FXS=0:
X200 Y400 G01 G94 F2000 FXS[X1] = 0
Meaning:
Axis X1 is retracted from the fixed stop to position X= 200 mm.
All other parameters are optional.
Caution
The traversing movement to the retraction position must move away from the fixed stop,
otherwise damage to the stop or to the machine may result.
The block change takes place when the retraction position has been reached. If no retraction
position is specified, the block change takes place immediately the torque limit has been
deactivated.
Example of clamping torque FXST, monitoring window FXSW
Any programmed torque limitation FXST is effective from the block start, i.e., the fixed stop is
also approached at a reduced torque. FXST and FXSW can be programmed or changed at
any time in the parts program:
FXST[X1] = 34.57
FXST[X1]=34.57 FXSW[X1]=5
FXSW[X1] = 5
The changes take effect before traversing movements in the same block.
Programming of a new fixed stop monitoring window causes a change not only in the
window width but also in the reference point for the center of the window if the axis has
moved prior to reprogramming. The actual position of the machine axis when the window is
changed is the new window center point.
Caution
The window must be selected such that only a breakaway from the fixed stop causes the
fixed stop monitoring to respond.
Description
The limit stop alarm can be suppressed from the parts program where necessary. This is
done by masking the alarm in a machine data and then activating this MD by means of
NEWCONF.
Motion commands
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 191
The "Travel to fixed stop" commands can be called from synchronized actions/technology
cycles. They can be activated without initiation of a motion, the torque is limited
instantaneously. As soon as the axis is moved via a setpoint, the limit stop monitor is
activated.
Rise ramp
A rise ramp for the new torque limit can be defined by machine data to prevent any abrupt
changes to the torque limit setting (e.g., insertion of a quill).
Link and container axes
Travel to fixed stop is also permitted for
• Link axes
• Container axes
The status of the assigned machine axis is unaffected by container switches.
References: /FB2/Function Manual Extended Functions; Multiple Operator Panels and
NCUs. (B3)
This also applies to modal torque limiting with FOCON (see "travel with limited
torque/force").
Activation from synchronized actions
Example:
If the anticipated event ($R1) occurs and travel to fixed stop is not already operative, then
FXS must be activated for axis Y. The torque must correspond to 10% of the rated torque
value. The width of the monitoring window is set to the default.
N10 IDS=1 WHENEVER (($R1=1) AND ($AA_FXS[Y]==0)) DO $R1=0 FXS[Y]=1
FXST[Y]=10
The normal parts program must ensure that $R1 is set at the desired point in time.
Deactivation from synchronized actions
Example:
If an anticipated event ($R3) has occurred and the status "Limit stop contacted" (system
variable $AA_FXS) is reached, then FXS must be deselected.
N13 IDS=4 WHENEVER (($R3==1) AND ($AA_FXS[Y]==1)) DO FXS[Y]=0 FA[Y]=1000
POS[Y]=0
Fixed stop reached
When the fixed stop has been reached:
• The distance-to-go is deleted and the position setpoint is manipulated,
• The drive torque increases to the programmed limit value FXSW and then remains
constant,
• Fixed stop monitoring is activated within the specified window width.
Motion commands
4.21 Travel to fixed stop (FXS, FXST, FXSW)
Fundamentals
192 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Combinability
Note
"Measure and delete distance-to-go" ("MEAS" command) and "Travel to fixed stop" cannot
be programmed in the same block.
Exception: One function acts on a path axis and the other on a positioning axis or both act
on positioning axes.
Contour monitoring
Contour monitoring is not performed while "Travel to fixed stop" is active.
Positioning axes
With "Travel to fixed stop" with POSA axes, the block change takes place independently of
the fixed stop movement.
Restrictions
Travel to fixed stop cannot be programmed
• for hanging axes (exception: possible on 840D with SIMODRIVE 611 digital),
• for gantry axes,
• for concurrent positioning axes, which are controlled exclusively by the PLC (FXS must
be selected from the NC program).
• If the torque limit is reduced too far, the axis will not be able to follow the specified
setpoint; the position controller then goes to the limit and the contour deviation increases.
In this operating state, an increase in the torque limit may result in sudden, jerky
movements.
To ensure that the axis can follow the setpoint, check the contour deviation to make sure
it is not greater than the deviation with an unlimited torque.
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 193
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Function
You can insert the following elements at a contour corner:
• Chamfer or
• Rounding
If you wish to round several contour corners sequentially by the same method, use
command RNDM "Modal rounding". This address is for inserting a rounding between linear
and circle contours after each traversing block. This is, for example, for deburring sharp
workpiece edges.
You can program the feedrate for the chamfer/rounding with FRC (non-modal) or FRCM
(modal).
If FRC/FRCM is not programmed, then the normal path feedrate F is applicable.
Programming
CHF=…
Or
CHR=…
Or
RND=…
Or
RNDM=…
Or
FRC=…
Or
FRCM=…
Parameters
CHF=… Chamfer the contour corner
Value = Length of the chamfer (unit of measurement according to G70/G71)
CHR=… Chamfer the contour corner
Programming the chamfer in the original direction of movement.
Value = width of chamfer in direction of motion (unit of measurement as
above)
RND=… Round the contour corner
Value = Radius of the rounding (unit of measurement according to G70/G71)
RNDM=… Modal rounding: Rounding several consecutive contour corners in the same
way.
Value = Radius of the roundings (unit of measurement according to
G70/G71)
Rounding is deactivated with RNDM=0.
FRC=… Non-modal feedrate for chamfer/rounding
Value = feedrate in mm/min (G94) or mm/rev (G95); FRC > 0
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
194 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
FRCM=… Modal feedrate for chamfer/rounding
Value = feedrate in mm/min (G94) or mm/rev (G95)
=0: The feedrate programmed under F for the chamfer/rounding is active.
Feed FRC (non-modal), FRCM (modal)
To optimize surface quality, it is possible to program a separate feedrate for the
chamfer/rounding contour elements. FRC is non-modal and FRCM is modal, see examples.
Example of chamfer, CHF/CHR
For the chamfer insert another linear part, the chamfer, between the linear and the circle
contours in any combination. The following two options are available:
N30 G1 X… Z… F… CHR=2
N40 G1 X… Z…
or
N30 G1 X… Z… F… CHF=2(cos α ·2)
N40 G1 X… Z…
;
=
*
*
&KDPIHU
HJ*
&+5
&+)
˞
%LVHFWRU
The chamfer is inserted after the block, in which it is programmed. The chamfer is always in
the plane activated with G17 to G19.
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 195
Example of rounding, RND
A circle contour element can be inserted with tangential link between the linear and the circle
contours in any combination.
N30 G1 X… Z… F… RND=2
51'
;
=
*
*
5RXQGLQJ
HJ*
The rounding is always in the plane activated with G17 to G19. The above figure shows the
rounding between two straight lines.
Here, the figure shows the rounding between a straight line and a circle.
N30 G1 X… Z… F… RND=2
N40 G3 X… Z… I… K…
51'
;
=
*
*
HJ*
5RXQGLQJ
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
196 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of modal rounding, RNDM
Deburring sharp workpiece edges:
N30 G1 X… Z… F… RNDM=2 ;modal rounding 2 mm
N40...
N120 RNDM=0 ;deactivate modal rounding
Example of chamfer CHF, rounding FRCM of the following block
MD CHFRND_MODE_MASK Bit0 = 0: Accept technology from following block (default)
N10 G0 X0 Y0 G17 F100 G94
N20 G1 X10 CHF=2 ;Chamfer N20-N30 with F=100 mm/min
N30 Y10 CHF=4 ;Chamfer N30-N40 with FRC=200 mm/min
N40 X20 CHF=3 FRC=200 ;Chamfer N40-N60 with FRCM=50 mm/min
N50 RNDM=2 FRCM=50
N60 Y20 ;Modal rounding N60-N70
;with FRCM=50 mm/min
N70 X30 ;Modal rounding N70-N80
;with FRCM=50 mm/min
N80 Y30 CHF=3 FRC=100 ;Chamfer N80-N90 with FRC=50 mm/min (modal)
N90 X40 ;Modal rounding N90-N100
;with F=100 mm/min (deselect FRCM)
N100 Y40 FRCM=0 ;Modal rounding N100-N120
;with G95 FRC=1 mm/rev
N110 S1000 M3
N120 X50 G95 F3 FRC=1
...
M02
Example of chamfer CHF, rounding FRCM of the previous block
MD CHFRND_MODE_MASK Bit0 = 1: Accept technology from preceding block
(recommended)
N10 G0 X0 Y0 G17 F100 G94
N20 G1 X10 CHF=2 ;Chamfer N20-N30 with F=100 mm/min
N30 Y10 CHF=4 FRC=120 ;Chamfer N30-N40 with FRC=120 mm/min
N40 X20 CHF=3 FRC=200 ;Chamfer N40-N60 with FRCM=200 mm/min
N50 RNDM=2 FRCM=50
N60 Y20 ;Modal rounding N60-N70
;with FRCM=50 mm/min
N70 X30 ;Modal rounding N70-N80
;with FRCM=50 mm/min
N80 Y30 CHF=3 FRC=100 ;Chamfer N80-N90 with FRC=100 mm/min
(modal)
N90 X40 ;Modal rounding N90-N100
;with FRCM=50 mm/min
N100 Y40 FRCM=0 ;Modal rounding N100-N120
;at F=100 mm/min
N110 S1000 M3
N120 X50 CHF=4 G95 F3 FRC=1 ;Chamfer N120-N130 with G95 FRC=1 mm/rev
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 197
N130 Y50 ;Modal rounding N130-N140
;at F=3 mm/rev
N140 X60
...
M02
Description
Note
Chamfer/rounding
If the programmed values for chamfer (CHF/CHR) or rounding (RND/RNDM) are too large
for the associated contour elements, then the chamfer or rounding are automatically reduced
to a suitable value.
No chamfer/rounding is inserted, if
No straight or circle contour is available in the plane,
A movement is taking place outside the plane,
A plane change is taking place, or
The number of blocks - which is specified in the machine data - not containing information for
traversing (e.g., only command output), is exceeded.
Note
FRC/FRCM
FRC/FRCM has no effect if a chamfer is being machined with G0; the command can be
programmed according to the F value without error message.
The reference to the blocks, in which chamfer and rounding are programmed and to the
technology is set in machine data.
FRC is operative only if a chamfer/rounding is programmed in the same block or if RNDM
has been activated.
FRC overwrites the F or FRCM value in the current block.
The feedrate programmed under FRC must be greater than zero.
FRCM=0 activates the feed programmed in F for the chamfer/rounding.
If FRCM is programmed, the FRCM value must be reprogrammed, analogous to F, on
changeover G94<->95, etc. If only a new F value is programmed, and if FRCM > 0 before
the feed type changes, error message 10860 (no feed programmed) will be activated.
Motion commands
4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM)
Fundamentals
198 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 199
Path Action 5
5.1 General notes
5.1.1 Programming path travel behavior
In this section you will find descriptions of commands, with which you can adapt the travel
behavior at the block boundaries optimally for special requirements. For instance, you can
position axes quickly enough or correspondingly reduce path contours over several blocks
taking into account an acceleration limit and the overload factor of the axes. Greater
inaccuracies of the path contour occur with increasing speed.
Path commands are programmed with the associated parameters.
Basic description
On change of the movement direction in the continuous-path mode contour transitions are
smoothed in that programmed positions are not approached exactly. In this way corners can
be moved round with as constant as possible speed or transitions can be optimized with
additional commands. With the exact stop function, machining operations can be
implemented as precisely as possible with inclusion of additional accuracy criteria. The
control determines the velocity control with look ahead automatically for several blocks in
advance.
For axes acceleration processes can be activated both conservatively for the mechanical
system or time-optimized. Both path axes and positioning axes, geo axes and following
axes, which can also change according to program run depending on the relevant blocks or
the momentary processing are discussed. The type of feedforward control and which path
axes should be operated with feedforward control can also be determined. In machining
without feedforward control the maximum permissible contour error can be specified.
A dwell time or a block with implicit preprocessing stop can be generated between two
blocks of the NC machining.
A programming example is given for each typical travel command.
Path Action
5.1 General notes
Fundamentals
200 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Functions for optimizing travel behavior at block boundaries
The travel behavior at the block boundaries can be optimized with the following functions:
• Setting exact stop to be modally and non-modally effective
• Defining exact stop with additional exact stop windows
• Continuous-path mode with constant speed
• Continuous-path mode with statement of the type of corner rounding
• Continuous-path mode with predictive speed control
• Activating acceleration and speed behavior of axes
• Influencing acceleration of slave axes as a percentage
• Smoothing path velocity
• Travel with feedforward control for increasing path accuracy
• Activate programmable contour accuracy
• Activating programmable dwell time
Path Action
5.1 General notes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 201
Overview of the various velocity controls
1*
1
1*
1
1*
1
1*
1
1*
1
1*
1
1*
1
=
;
1 1 1 1 1 1 1
1 1 1 1 1 1 1
W
W
)
)
)
)
W
1 1 1 1 1 1 1
W
*62)7
*%5,6.
**QRZDLWWLPH
* * ZDLWWLPHZLWK*
&RQWRXUFXUYH
9SDWK SDWKYHORFLW\
9SDWK
9SDWK
5DSLGWUDYHUVH
9SDWK
Path Action
5.2 Exact stop (G60, G9, G601, G602, G603)
Fundamentals
202 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
5.2 Exact stop (G60, G9, G601, G602, G603)
Function
The exact positioning stop functions are used to machine sharp outside corners or to finish
inside corners to size.
With the exact stop criteria exact stop window fine and exact stop window coarse, you
determine how accurately the corner point is approached and when the change to the next
block takes place. At interpolation end you can initiate the block change at the block end
when the control has calculated a set speed of zero for the axes involved.
Programming
G60
Or
G9
Or
G601
Or
G602
Or
G603
Parameters
G60 Exact stop, modal
G9 Exact stop, non-modal
G601 Step enable if positioning window fine reached
G602 Step enable if positioning window coarse reached
G603 Step enable if setpoint (end of interpolation) reached
Exact stops fine and coarse can be defined for each axis in machine data. The velocity up to
reaching the accurate destination position at the end of the block is decelerated to zero.
Note
G601, G602 and G603 are only effective if G60 or G9 are active.
Path Action
5.2 Exact stop (G60, G9, G601, G602, G603)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 203
Example
N5 G602 ;Exact stop window coarse
N10 G0 G60 Z... ;Exact stop, modal
N20 X... Z... ;G60 continues to act
...
N50 G1 G601 ;Exact stop window fine
N80 G64 Z... ;Switching over to continuous-path mode
...
N100 G0 G9 :Exact stop acts only in this block
N111 ... ;Again continuous-path mode
Description
Exact stop, G60, G9
G9 generates the exact stop in the current block. G60 generates the exact stop in the current
block and all subsequent blocks.
Continuous-path-mode functions G64 or G641 are used to deactivate G60.
G601/G602
*
*
%ORFNVWHSHQDEOH
The movement is decelerated and stopped briefly at the corner point.
Note
Set the exact stop limits no tighter than you require. The tighter the limits, the longer it takes
to position and approach the target position.
End of interpolation, G603
Path Action
5.2 Exact stop (G60, G9, G601, G602, G603)
Fundamentals
204 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
The block change is initiated when the control has calculated a set velocity of zero for the
axes involved. At this point, the actual value lags behind by a proportionate factor depending
on the dynamic response of the axes and the path velocity. The workpiece corners can now
be rounded.
3URJUDPPHGSDWK
7UDYHUVHG
SDWK
ZLWK)
7UDYHUVHG
SDWK
ZLWK)
))
Command outputs
In all three cases, the following applies:
The auxiliary functions programmed in the NC block are enabled after the end of the
movement.
%ORFNFKDQJH
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 205
Note
Machine manufacturer
A machine data item can be set for specific channels which determines that default exact
stop criteria, which deviate from the programmed criteria, will be applied automatically.
These are given priority over the programmed criteria in some cases. Criteria for G0 and the
other G commands in the 1st G-code group can be stored separately, see
/FB1/Function Manual Basic Functions; Continuous-Path Mode, Exact Stop and
Look Ahead (B1).
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Function
In continuous-path mode, the contour is machined with a constant path velocity. The uniform
velocity also establishes better cutting conditions, improves the surface quality and reduces
the machining time.
Note
Continuous-path mode is interrupted by blocks which trigger a preprocessing stop implicitly
(e.g. access to particular status data of machine ($A...)). The corresponding situation applies
for the auxiliary function outputs.
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
206 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
Notice
In continuous-path mode, the programmed contour transitions are not approached exactly.
If a rounding movement initiated by G641, G642, G643, G644 is interrupted, the corner point
of the original contour will be used for subsequent repositioning (REPOS), rather than the
interruption point.
Sharp corners can be produced with G60 or G9.
G64
Or
G641 ADIS=…
Or
G641 ADISPOS=…
Or
G642 ADIS=…
Or
G642 ADISPOS=…
Or
G643 ADIS=…
Or
G643 ADISPOS=…
Or
G644
Note
G644 is not available with an active kinematic transformation. The system switches internally
to G642.
During continuous-path mode, a message is output from the parts program (even in the form
of an executable block), if MSG is programmed with the second call parameter = 1.
MSG("Text", 1)
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 207
Parameters
G64 Continuous-path mode
G641 Continuous-path mode with programmable transition rounding
G642 Corner rounding with axial tolerance, with modal activated
G643 Block-internal corner rounding
G644 Corner rounding with greatest possible dynamic response
ADIS=... Rounding clearance for path functions G1, G2, G3, etc.
ADISPOS=... Rounding clearance for rapid traverse G0
MSG Continue displaying message until next message is queued
"text" STRING-type character string
2. Parameter = 1 Executable block is generated explicitly for MSG. If the MSG procedure is
programmed without the 2nd parameter, the message "Text" is output with
the next executable block.
Corner rounding with ADIS and ADISPOS
Note
Rounding cannot be used as a substitute for smoothing (RND). The user should not make
any assumptions with respect to the appearance of the contour within the rounding area. The
type of rounding can depend on dynamic conditions, e.g., on the tool path velocity. Rounding
on the contour is therefore only practical with small ADISvalues. RND must be used if a
defined contour is to be followed at the corner without exception.
ADISPOS is used between G0 blocks. This enables the axis movement to be smoothed
substantially and the traversing time to be reduced during positioning.
If ADIS/ADISPOS is not programmed, a value of zero applies and the traversing behavior
therefore corresponds to G64. The rounding clearance is automatically reduced (by up to
36%) for short traversing distances.
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
208 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example
With this workpiece, the two outside corners at the groove are approached exactly. All other
machining takes place in continuous-path mode.
;
<
=
<
([DFWVWRS
)LQH
N05DIAMOF ;Radius as dimension
N10 G17 T1 G41 G0 X10 Y10 Z2 S300 M3 ;Approach starting position, activate
;spindle, path compensation
N20 G1 Z-7 F8000 ;Tool infeed
N30 G641 ADIS=0.5 ;Contour transitions are smoothed
N40 Y40
N50 X60 Y70 G60 G601 ;Approach exact position with exact stop
;fine
N60 Y50
N70 X80
N80 Y70
N90 G641 ADIS=0.5 X100 Y40 ;Contour transitions are smoothed
N100 X80 Y 10
N110 X10
N120 G40 G0 X-20 ;Deactivate path compensation
N130 Z10 M30 ;Retract tool, end of program
Note
An example of rounding with G643, also refer to to:
References:
/PGA/ Job Planning Programming Manual; special movement commands,
Chapter "Settable path reference (SPATH, UPATH)"
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 209
Continuous-path mode, G64
In continuous-path mode, the tool travels across tangential contour transitions with as
constant a path velocity as possible (no deceleration at block boundaries). Look Ahead
deceleration takes place before corners (G9) and blocks with exact stop ("Look Ahead", see
following pages).
Corners are also traversed at a constant velocity. In order to minimize the contour error, the
velocity is reduced according to an acceleration limit and an overload factor.
Reference:
/FB1/ Function Manual Basic Functions; Continuous Path Mode, Exact Stop and
Look Ahead (B1)
9HORFLW\
UDWH
Note
The overload factor can be set in the MD32310. The extent of smoothing of the contour
transitions depends on the feedrate and the overload factor. With G641, you can specify the
desired rounding area explicitly.
Smoothing cannot and should not replace the functions for defined smoothing (RND, RNDM,
ASPLINE, BSPLINE, CSPLINE).
Continuous-path mode with programmable transition rounding, G641
With G641, the control inserts transition elements at contour transitions. With ADIS=… or
ADISPOS=…, you can specify the extent, to which the corners are rounded. The effect of
G641 is similar to RNDM; however, it is not restricted to the axes of the working plane.
Example: N10 G641 ADIS=0.5 G1 X... Y...
The rounding block must begin 0.5 mm before the programmed end of block at the earliest
and must be finished 0.5 mm after the end of the block. This setting remains modal.
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
210 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G641 also operates with "Look Ahead" predictive velocity control. Corner rounding blocks
with a high degree of curvature are approached at reduced velocity.
PD[PP 3URJUDPPHG
FRQWRXUHQG
$',6$',6326
PD[PP
Continuous-path mode G64/G641 over several blocks
The following points should be noted in order to prevent an undesired stop in the path motion
(relief cutting):
• Auxiliary function outputs trigger a stop (exception: high-speed auxiliary functions and
auxiliary functions during movements).
• Intermediate blocks, which contain only comments, calculation blocks or subroutine calls
do not affect the movement.
Extensions of corner rounding
If FGROUP does not contain all the path axes, there is often a step change in the velocity at
block boundaries for those axes excluded from FGROUP; the control limits this change in
velocity to the permissible values set in MD32300 $MA_MAX_AX_ACCEL and MD32310
$MA_MAX_ACCEL_OVL_FACTOR. This braking operation can be avoided through the
application of a rounding function, which "smoothes" the specific positional interrelationship
between the path axes.
Corner rounding with G641
You can activate a modal corner rounding action by programming G641 and specifying a
rounding radius with ADIS (or ADISPOS in rapid traverse). Within this radius about the block
change point, the control is free to ignore the path construct and replace it with a dynamically
optimized path. Disadvantage:Only one ADIS value is available for all axes.
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 211
Corner rounding with axial precision using G642
G642 activates corner rounding with modal axial tolerances. Smoothing is not made within a
defined ADIS range, but the axial tolerances, defined with MD33100
$MA_COMPRESS_POS_TOL are maintained. Otherwise, the mode of operation is identical
to G641.
With G642, the rounding travel is determined on the basis of the shortest rounding travel of
all axes. This value is taken into account when generating a rounding block.
Block-internal corner rounding with G643
The maximum deviations from the precise contour when smoothing with G643 are defined
for each axis using machine data MD33100 $MA_COMPRESS_POS_TOL[...]. G643 is not
used to generate a separate rounding block, but axisspecific blockinternal rounding
movements are inserted. In the case of G643, the rounding travel of each axis may be
different .
Corner rounding with contour tolerance in G642 and G643
The expansions described below refine the response with G642 and G643 and rounding with
contour tolerance is introduced. When rounding with G642 and G643, the maximum
permissible deviations of each axis are normally specified.
MD20480 $MC_SMOOTHING_MODE can be used to configure rounding with G642 and
G643 so that instead of the axis-specific tolerances, a contour tolerance and an orientation
tolerance can be specified. In this case, the tolerance of the contour and of the orientation is
set using two independent setting data, programmed in the NC, so that setting data can be
specified differently for each block transition.
Setting data
SD42465 $SC_SMOOTH_CONTUR_TOL
This setting data is used to define the maximum tolerance for the contour when rounding.
SD42466 $SC_SMOOTH_ORI_TOL
This setting data is used to define the maximum tolerance for the contour when rounding for
the tool orientation (angle deviation).
This data is only effective if an orientation transformation is active. Very different
specifications for the contour tolerance and the tolerance of the tool orientation can only
have effect with G643.
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
212 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Corner rounding with greatest possible dynamic response in G644
Rounding with maximum possible speed is activated with G644 and configured with
MD20480 $MC_SMOOTHING_MODE in the thousands place:
Value Meaning
0 Specifying the maximum axial deviation using MD33100 $MA_COMPRESS_POS_TOL
1 Specify the maximum rounding travel by programming ADIS=... or ADISPOS=...
2 Specify the maximum possible frequencies for each axis in the rounding area using
MD32440 $MA_LOOKAH_FREQUENCY. The rounding area is defined such that no
frequencies in excess of the specified maximum can occur while the rounding motion is in
progress.
3 When rounding with G644, neither the tolerance nor the rounding distance are monitored.
Each axis traverses around a corner with the maximum possible dynamic response.
With SOFT, both the maximum acceleration and the maximum jerk of each axis is
maintained.
With the BRISK command, the jerk is not limited; instead, each axis travels at the maximum
possible acceleration.
Reference:
/FB1/ Function Manual Basic Functions; Continuous Path Mode, Exact Stop and Look Ahead
(B1)
No rounding block/no rounding movement
Command outputs
Auxiliary functions, which are enabled after the end of the movement or before the next
movement interrupt continuous-path mode.
Positioning axes
Positioning axes always traverse according to the exact stop principle, positioning window
fine (as for G601). If an NC block has to wait for positioning axes, continuous-path mode is
interrupted on the path axes.
No corner rounding is performed in the following situations:
• Movement is stopped between the two blocks. This occurs when ...
– The following block contains an auxiliary function output before the movement.
– The following block does not contain a path movement.
– An axis is traversed for the first time as a path axis for the following block when it was
previously a positioning axis.
– An axis is traversed for the first time as a positioning axis for the following block when
it was previously a path axis.
– Before tapping, the following block uses G33 as preparatory function and the previous
block does not.
– A change is made between BRISK and SOFT.
– Axes involved in the transformation are not completely assigned to the path motion
(e.g., for oscillation, positioning axes).
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 213
• The rounding block would slow down parts program processing. This occurs when ...
– A rounding block is inserted between very short blocks. Since each block requires at
least one interpolation cycle, the added intermediate block would double the
machining time.
– A block transition G64 (continuous-path mode without corner rounding) can be
traversed without a reduction in velocity. Rounding would increase the machining time.
This means that the value of the permitted overload factor (MD32310
$MA_MAX_ACCEL_OVL_FACTOR) affects whether a block transition is rounded or
not. The overload factor is only taken into account when corner rounding in
conjunction G641/G642. The overload factor is ignored in corner rounding with G643.
– This behavior can also be set for G641 and G642 by setting MD20490
$MC_IGNORE_OVL_FACTOR_FOR_ADIS is set to TRUE.
• Rounding is not parameterized. This occurs when...
– forG641 in G0 blocks ADISPOS== 0 (default!).
– for G641 in non-G0 blocks ADIS== 0 (default!).
– for G641 on transition from G0 and non-G0 or non-G0 and G0 respectively, the smaller
value from ADISPOS and ADIS applies.
– forG642/G643, all axis-specific tolerances are zero.
• Block does not contain traversing motion (zero block).
Normally, the interpreter eliminates zero blocks. However, if synchronous actions are
active, this zero block is included and also executed. In so doing, an exact stop is initiated
corresponding to the active programming. This allows the synchronous action to also
switch.
Blocks without traversing motion can also be generated using program jumps.
– Examples of zero blocks:
N1000 G91 X0 Y0 Z0
...
N10 G90 G64 X100 Y100 Z100
N15 Z100
...
Path Action
5.3 Continuous-path mode (G64, G641, G642, G643, G644)
Fundamentals
214 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Look Ahead speed control
In continuous-path mode with G64 or G641, the control automatically detects the velocity
control in advance for several NC blocks. This enables acceleration and deceleration across
multiple blocks with almost tangential transitions.
Look Ahead is particularly suitable for the machining of movement sequences comprising
short traverse paths with high path feedrates.
The number of NC blocks included in the Look Ahead calculation can be defined in machine
data.
;
Y
1 1 1 1 1 1 1 1 1
9HORFLW\SDWWHUQ
ZLWK**
*ZLWK/RRN$KHDG
3URJUDPPHG
)HHG
**
HJ*ZLWKLQVXIILFLHQW
/RRN$KHDG
Note
Look Ahead across more than one block is an option.
Continuous-path mode in rapid traverse G0
One of the functions G60/G9 or G64/G641 must also be specified for rapid traverse.
Otherwise, the default in the machine data is used.
By setting MD 20490: IGNORE_OVL_FACTOR_FOR_ADIS results in block transitions being
smoothed irrespective of the programmed overload factor.
Path Action
5.4 Acceleration behavior
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 215
5.4 Acceleration behavior
5.4.1 Acceleration response, BRISK, SOFT, DRIVE
Function
BRISK, BRISKA: The axis slides travel with maximum acceleration until the feedrate is
reached. BRISK enables time-optimized machining, but with jumps in the acceleration curve.
SOFT, SOFTA: The axis slides travel with constant acceleration until the feedrate is
reached. SOFT acceleration enables higher path accuracy and less wear and tear on the
machine.
DRIVE, DRIVEA: The axis slides traverse at the maximum acceleration rate up to the
velocity limit set in the machine data. The acceleration rate is then reduced according to
machine data until the feedrate is reached. This function allows the acceleration
characteristic to be optimally adapted to a specific motor characteristic, for example, for
stepper motor applications.
Programming
BRISK
BRISKA (axis1,axis2,…)
or
SOFT
SOFTA(axis,axis2,…)
or
DRIVE
DRIVEA(axis1,axis2,…)
Parameter
BRISK Abrupt acceleration of path axes
BRISKA (axis1,axis2,…) Switch on stepped axis acceleration for the programmed axes
SOFT Jerk-limiting acceleration of path axes
SOFTA(axis,axis2,…) Switch on jerk-limiting axis acceleration for the programmed axes
DRIVE Reduction of acceleration above a velocity for path axes that can
be set in $MA_ACCEL_REDUCTION_SPEED_POINT (only
applicable for FM-NC)
DRIVEA(axis1,axis2,…) Reduction of acceleration above a velocity for programmed axes
that can be set in $MA_ACCEL_REDUCTION_SPEED_POINT
(only applicable for FM-NC)
Path Action
5.4 Acceleration behavior
Fundamentals
216 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
(axis1,axis2,…) The acceleration pattern set in machine data $MA_POS_AND
JOG_JERK_ENABLE or $MA_ACCEL_TYPE_DRIVE is active for
the programmed axes.
Note
A change between BRISK and SOFT causes a stop at the block transition. The acceleration
pattern for the path axes can be defined in machine data.
Apart from the path-related jerk limitation that is effective in the MDA and AUTO modes,
there is the axis-related jerk limitation that can influence positioning axes and traversing axes
in JOG mode.
Example of BRISK and SOFT
N10 G1 X… Y… F900 SOFT
N20 BRISKA(AX5,AX6)
%5,6.
WLPH
RSWLPL]HG
62)7
SURWHFWLQJWKH
PHFKDQLFDO
V\VWHP
6HWSRLQW
3DWKYHORFLW\
7LPH
Path Action
5.4 Acceleration behavior
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 217
Example of DRIVE, DRIVEA
N05 DRIVE
N10 G1 X… Y… F1000
N20 DRIVEA (AX4, AX6)
3DWKYHORFLW\
7LPH
/LPLWRI
FRQVWDQW
DFFHOHUDWLRQ
6HWSRLQW
5.4.2 Influence of acceleration on following axes (VELOLIMA, ACCLIMA, JERKLIMA)
Function
The axis couplings described in the Programming Guide, Advanced: Tangential correction,
coupled-motion axes, master value coupling, and electronic gear have the property of
moving following axes/spindles as a function of one or more leading axes/spindles.
The commands for correction of limitation for the dynamic response of the following axis can
be issued from the parts program or from synchronous actions. The commands for
correction of limitations of the following axis can already be given while axis coupling is
active.
Programming
VELOLIMA[AX4]=75 75% of the maximum axial velocity stored in the machine data
ACCLIMA[AX4]=50 50% of the maximum axial acceleration stored in the machine data
JERKLIMA[AX4]=50 50% of the maximum jerk on path motion stored in the machine data
Path Action
5.4 Acceleration behavior
Fundamentals
218 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
VELOLIMA[Ax], Change to limit for maximum velocity for following axis
ACCLIMA[Ax], Change to limit for maximum acceleration for following axis
JERKLIMA[Ax], Change to limit for maximum jerk for following axis
Note
JERLIMA[ax] is not available for all types of connection. Details about the function are
described in:
References:
/FB3/Function Manual Special Functions; Coupled Axes and ESR (M3)
/FB2/Function Manual Extended Functions; Synchronous Spindle (S3)
Example of electronic gear
Axis 4 is coupled to axis X via an electronic gear coupling. The acceleration capability of the
following axis is limited to 70% of maximum acceleration. The maximum permissible velocity
is limited to 50% of maximum velocity. After successful activation of the coupling, the
maximum permissible velocity is set to 100% again.
N120 ACCLIMA[AX4]=70 ;Reduced maximum acceleration
N130 VELOLIMA[AX4]=50 ;Reduced maximum velocity
...
N150 EGON(AX4, "FINE", X, 1, 2) ;Activation of the EG coupling
...
N200 VELOLIMA[AX4]=100 ;Full maximum velocity
Example of influencing master value coupling by static synchronized action
Axis 4 is coupled to X by master value coupling. The acceleration response is limited to 80%
by static synchronized action 2 from position 100.
N120 IDS=2 WHENEVER $AA_IM[AX4] > 100
DO ACCLIMA[AX4]=80
;Synchronized action
N130 LEADON(AX4, X, 2) ;Master value coupling on
Path Action
5.4 Acceleration behavior
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 219
5.4.3 Technology G group (DYNNORM, DYNPOS, DYNROUGH, DYNSEMIFIN,
DYNFINISH)
Function
Using the "Technology" G group, the appropriate dynamic response can be activated for five
varying technological machining steps.
Machine manufacturer
Dynamic values and G codes can be configured and are, therefore, dependent on machine
data settings.
References: /FB3/, B1, "Continuous-path mode"
Programming
DYNNORM
Or
DYNPOS
Or
DYNROUGH
Or
DYNSEMIFIN
Or
DYNFINISH
Parameters
DYNNORM Standard dynamic response, as previously (index n=0)
DYNPOS Dynamic response for positioning mode, tapping (index n=1)
DYNROUGH Dynamic response for roughing (index n=2)
DYNSEMIFIN Dynamic response for finishing (index n=3)
DYNFINISH Dynamic response for smooth-finishing (index n=4)
Write or read specific field element
$MA...[n, X] Machine data with field element, which affects dynamic response
[<n>, <X>] Field element with field device n and axis address X
n = 0 to 4 Range of values corresponds to Technology G group.
Note
The dynamic values are already active in the block, in which the associated G code is
programmed. Machining is not stopped.
Path Action
5.5 Smoothing the path velocity
Fundamentals
220 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example
Dynamic values by technology group G code
DYNNORM G1 X10 ;Initial setting
DYNPOS G1 X10 Y20 Z30 F… ;Positioning mode, tapping
DYNROUGH G1 X10 Y20 Z30 F10000 ;Roughing
DYNSEMIFIN G1 X10 Y20 Z30 F2000 ;Finishing
DYNFINISH G1 X10 Y20 Z30 F1000 ;Smooth-finishing
Write or read specific field element
Maximum acceleration for roughing, axis X
R1=$MA_MAX_AX_ACCEL[2, X] ;Read
$MA_MAX_AX_ACCEL[2, X]=5 ;Write
5.5 Smoothing the path velocity
Function
A smoother path velocity profile can be achieved with the "Path velocity smoothing" function,
which allows special, configurable, machine data and the character of the parts program to
be taken into account.
The velocity control function utilizes the specified axial dynamic response. If the programmed
feedrate cannot be achieved, the path velocity is brought to the parameterized axial limit
values and the limit values of the path (velocity, acceleration, jerk). This can lead to repeated
braking and acceleration on the path.
Note
Machine manufacturer
The user can control the path velocity as appropriate for the configurable machine data by
making use of the program properties.
References: Functional description /FB1/; B1; "Smoothing the path velocity"
Path Action
5.5 Smoothing the path velocity
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 221
Parameter
Machine manufacturer
Limit values that can be configured in relation to (specially) adjustable parameters of the
parts program, using machine data:
• lengthening the machining time
The machining time of the part program is specified as percentage. The actual
lengthening is according to the worst case of all acceleration processes inside the part
program and can even be zero.
• Input of the natural frequencies of the operated axes
Only acceleration processes that lead to clear excitation of machine axes should be
removed.
• Taking the programmed feedrate into account.
In this case the smoothing factor is observed especially exactly if the override is set to
100%.
Note
Variations in path velocity due to the input of a new feedrate are not changed either. This
remains the responsibility of the programmer of the subprogram.
Note
If a short acceleration takes place during a machining function with high path velocity,
and is thus followed almost immediately by braking, the reduction in the machining time is
only minimal. Acceleration of this kind can, however, have undesirable effects if, for
example, it results in machine resonance.
Path Action
5.6 Traversing with feedforward control, FFWON, FFWOF
Fundamentals
222 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
5.6 Traversing with feedforward control, FFWON, FFWOF
Function
Using feedforward control the velocity-dependent overtravel in path traversing is reduced to
zero. Traversing with feedforward control permits higher path accuracy and thus improved
machining results.
Programming
FFWON
Or
FFWOF
Parameters
FFWON Activate feedforward control
FFWOF Deactivate feedforward control
Note:The type of feedforward control and the path axes to which feedforward is to be applied
are determined via machine data.
Default: Velocity-dependent feedforward control
Option: Acceleration-dependent feedforward control (not possible with 810D)
Example
N10 FFWON
N20 G1 X… Y… F900 SOFT
Path Action
5.7 Contour accuracy, CPRECON, CPRECOF
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 223
5.7 Contour accuracy, CPRECON, CPRECOF
Function
In machining operations without feedforward control (FFWON), errors may occur on curved
contours as a result of velocity-related differences between setpoint and actual positions.
The programmable contour accuracy function CPRECON makes it possible to store a
maximum permissible contour violation in the NC program which must never be overshot.
The magnitude of the contour violation is specified with setting data $SC_CONTPREC.
The Look Ahead function allows the entire path to be traversed with the programmed contour
accuracy.
Programming
CPRECON
or
CPRECOF
Parameter
CPRECON Activate programmable contour accuracy
CPRECOF Deactivate programmable contour accuracy
Note
A minimum velocity can be defined via the setting datum $SC_MINFEED, which is not
undershot, and the same value can also be written directly out from the parts program via
the system variable $SC_CONTPREC.
On the basis of the value of the contour violation $SC_CONTPREC and the servo gain factor
(velocity/following error ratio) of the geometry axes concerned, the control calculates the
maximum path velocity at which the contour violation produced by the overtravel does not
exceed the minimum value stored in the setting data.
Example
N10 X0 Y0 G0
N20 CPRECON ;Activate contour accuracy
N30 F10000 G1 G64 X100 ;Machine contour at 10 m/min in continuous-path mode
N40 G3 Y20 J10 ;Automatic feed limitation in circular block
N50 X0 ;Feed without limitation to 10 m/min
Path Action
5.8 Dwell time, delay (G4, WRTPR)
Fundamentals
224 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
5.8 Dwell time, delay (G4, WRTPR)
Function
You can use G4 to interrupt workpiece machining between two NC blocks for the
programmed length of time, e.g., for relief cutting.
The WRTPR command does not generate an executable block in continuous-path mode.
Thus, it can be used to delay the machining job without interrupting continuous-path mode.
Programming
G4 F…
Or
G4 S…
Write string-type statement with next block in main run:
WRTPR(string, parameter) if parameter = 0 or not specified.
Programming in a separate NC block
Parameters
G4 Activate dwell time, G4 interrupts the continuous-path mode
F… Time specified in seconds
S… Time specified in revolutions of the master spindle
WRTPR Either append a job in continuous-path mode to the next executable block
or execute it immediately.
Parameter = 0 Write to log with next executable block (following a delay). This is the
default response so there is no need for parameterization. Continuous-path
mode functions as normal.
Path Action
5.9 Internal preprocessing stop
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 225
Parameter = 1 Write to log immediately. A main-run block is generated, which affects the
response in continuous-path mode.
Note
The words with F... and S... are used for time specifications only in the block with G4.
Any previously programmed feed F and spindle speed S remain valid.
Example
N10 G1 F200 Z-5 S300 M3 ;Feed F; spindle speed S
N20 G4 F3 ;Dwell time 3 s
N30 X40 Y10
N40 G4 S30 ;Dwelling 30 revolutions of the spindle, corresponds
;at S=300 rpm and 100% speed override to:
;t=0.1 min
N40 X... ;Feed and spindle speed remain effective
5.9 Internal preprocessing stop
Function
The control generates an internal preprocessing stop on access to machine status data
($A...). If a command, which implicitly causes a preprocessing stop, is read in a following
block, this block is not executed until all other blocks, which have already been preprocessed
and stored, have been executed. The preceding block is halted in exact stop (as with G9).
Programming
Machine status data ($A...) are generated internally by the control.
Parameters
Status data of the machine ($A...).
Path Action
5.9 Internal preprocessing stop
Fundamentals
226 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example
Machining should be stopped in block N50.
N40 POSA[X]=100
N50 IF $AA_IM[X]==R100 GOTOF
MARKE1
;Access to machine status data ($A...), the ;control generates
an internal preprocessing stop.
N60 G0 Y100
N70 WAITP(X)
N80 LABEL1:
N40 X... ;Feed and spindle speed remain effective
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 227
Frames 6
6.1 General
Function
Frames are used to describe the position of a destination coordinate system by specifying
coordinates or angles starting from the current workpiece coordinate system.
;
<
;
<
= =
5RWDWLRQ
DURXQGWKH=
D[LV
;0
<0
=0
=HURRIIVHW
Possible frames:
• Basic frame (basic offset)
• Settable frames (G54...G599)
• Programmable frames
Programming
Frame is the conventional term for a geometrical expression that describes an arithmetic
rule, such as translation, rotation and scaling or mirroring.
Frames
6.1 General
Fundamentals
228 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Param eters
Machine manufacturer
Settable frames (G54...G57, G505... G599): See machine manufacturer's specifications.
Frame components for the programmer
A frame can consist of the following arithmetic rules:
• Zero point offset, TRANS, ATRANS
• Rotation, ROT, AROT
• Scale, SCALE, ASCALE
• Mirroring, MIRROR, AMIRROR
These frames can be used individually or in any combination.
Example of frame components in milling
75$16$75$16
6&$/($6&$/(
0,5525$0,5525
527
$527
<
;
<
;
<
;
<
;
Frames
6.2 Frame instructions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 229
Example of frame components in turning
75$16$75$16
6&$/($6&$/( 0,5525$0,5525
527
$527
;
=
;
=
;
=
;
=
6.2 Frame instructions
Function
For the possible frames the position of one of the target coordinate systems is defined:
• Basic frame (basic offset)
• Settable frames (G54...G599)
• Programmable frames
In addition to these frames, you can program replacing and additive statements or generate
frames as well as frame rotations for tool orientation. Certain set frames or superposed
movements and transformations can also be deselected.
Basic frame (basic offset)
The basic frame describes the coordinate transformation from the Basic Coordinate System
(BCS) to the Basic Zero System (BZS) and has the same effect as for settable frames.
Settable statements
Settable statements are the zero offsets, which can be called from any NC program with the
commands G54 to G599. The offset values are predefined by the user and stored in the zero
offset memory on the control. This is used to define the Workpiece Coordinate System
(WCS).
Programmable instructions
Programmable instructions (TRANS, ROT, etc.) are valid in the current NC program and
refer to the settable instructions. The programmable frame is used to define the Workpiece
Coordinate System (WCS).
Frames
6.2 Frame instructions
Fundamentals
230 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
TRANS X… Y… Z… or ATRANS X… Y… Z… or
G58 X… Y… Z… A… or G59 X… Y… Z… A… or
ROT X… Y… Z… or ROT RPL=… or AROTX… Y… Z… or AROT RPL=… or
ROTS X... Y... or AROTS X... Y... or CROTS X... Y... or
SCALE X… Y… Z… or ASCALE X… Y… Z… or
MIRROR X0 Y0 Z0 or AMIRROR X0 Y0 Z0 or
TOFRAME or TOFRAMEZ or TOFRAMEY or TOFRAMEX or
TOROTOF or TOROT or TOROTZ or TOROTY or TOROTX or
PAROT or PAROTOF or
CORROF(axis,string[axis,string]) or CORROF(axis,string) or
CORROF(axis) or CORROF()
Caution
The above frame instructions are programmed in separate NC blocks and executed in the
programmed order.
TRANS, ROT, SCALE and MIRROR instructions.
Substituting instructions
TRANS, ROT, SCALE and MIRROR are substituting instructions.
75$16$75$16
6&$/($6&$/(
0,5525$0,5525
527
$527
<
;
<
;
<
;
<
;
Frames
6.2 Frame instructions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 231
Note
This means that each of these instructions cancels all other previously programmed frame
instructions.
The last called settable zero offset G54 to G599 is used as the reference.
Additive instructions
ATRANS, AROT, ASCALE and AMIRROR are additive instructions. The currently set zero
point or the last workpiece zero to be programmed with frame instructions is used as the
reference. The above instructions are added to existing frames.
Note
Additive statements are frequently used in subroutines. The basic functions defined in the
main program are not lost after the end of the subroutine if the subroutine has been
programmed with the SAVE attribute.
75$16
$75$16
References:
/PGA/Programming Manual Advanced; "Subroutines, Macros"
Frames
6.3 Programmable zero offset
Fundamentals
232 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
6.3 Programmable zero offset
6.3.1 Zero offset (TRANS, ATRANS)
Function
TRANS/ATRANS can be used to program translations for all path and positioning axes in the
direction of the specified axis. This allows you to work with different zero points, for example
when performing recurring machining processes at different workpiece positions.
Milling:
=0
=
<0
<
;0
;
*
75$16
Frames
6.3 Programmable zero offset
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 233
Turning:
;
=
0
:
*
75$16
Deactivate programmable zero offset:
For all axes: TRANS (without axis parameter)
Programming
TRANS X… Y… Z… (substituting instruction programmed in a separate NC block)
Or
ATRANS X… Y… Z… (additive instruction programmed in a separate NC block)
Parameters
TRANS Absolute zero offset, with reference to the currently valid workpiece zero
set with G54 to G599
ATRANS as TRANS, but with additive zero offset
X Y Z Offset value in the direction of the specified geometry axis
Frames
6.3 Programmable zero offset
Fundamentals
234 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of milling
With this workpiece, the illustrated shapes recur several times in the same program.
The machining sequence for this shape is stored in a subprogram.
You use the translation to set only those workpiece zeroes and then call up the subprogram.
<
;
<0
;0
<
;
<
;
*
N10 G1 G54 ;Working plane X/Y, workpiece zero
N20 G0 X0 Y0 Z2 ;Approach starting point
N30 TRANS X10 Y10 ;Absolute offset
N40 L10 ;Subprogram call
N50 TRANS X50 Y10 ;Absolute offset
N60 L10 ;Subprogram call
N70 M30 ;End of program
Frames
6.3 Programmable zero offset
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 235
Example of turning
;
=
0:
N.. ...
N10 TRANS X0 Z150 ;Absolute offset
N15 L20 ;Subprogram call
N20 TRANS X0 Z140 (or ATRANS Z-10) ;Absolute offset
N25 L20 ;Subprogram call
N30 TRANS X0 Z130 (or ATRANS Z-10) ;Absolute offset
N35 L20 ;Subprogram call
N.. ...
Substituting instruction, TRANS X Y Z
Translation through the offset values programmed in the specified axis directions (path,
synchronized axes and positioning axes). The last specified settable zero offset (G54 to
G599) is used as a reference.
Note
The TRANS command cancels all frame components of the previously activated
programmable frame.
Frames
6.3 Programmable zero offset
Fundamentals
236 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
75$16
75$16
Note
You can use ATRANS to program a translation, which is to be added to existing frames.
Additive instruction, ATRANS X Y Z
Translation through the offset values programmed in the specified axis directions. The
currently set or last programmed zero point is used as the reference.
75$16
$75$16
Frames
6.3 Programmable zero offset
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 237
Note
Previously programmed frames are canceled. The settable zero offset remains programmed.
6.3.2 Axial zero offset (G58, G59)
Function
G58 and G59 allow translation components of the programmable zero offset (frame) to be
replaced for specific axes. The translation function comprises:
• absolute component (G58, coarse offset)
• additive component (G59, fine offset)
Machine manufacturer
These functions can only be used if the fine offset is configured via machine datum MD
24000:. FRAME_ADD_COMPONENTS=1. If G58 or G59 is used without a configured fine
offset, alarm "18312 channel %1 block %2 frame: Fine offset not configured" is output.
=0
=
<0
<
;0
;
*
7UDQVODWLRQ
DEVROXWHWUDQVODWLRQ
*
75$16
DGGLWLYHWUD
*
$75$16
Programming
G58 X… Y… Z… A… (substituting instruction programmed in separate NC block)
Or
G59 X… Y… Z… A… (substituting instruction programmed in separate NC block)
Frames
6.3 Programmable zero offset
Fundamentals
238 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G58 Replaces the absolute translation component of the programmable zero
offset for the specified axis, but the programmed additive offset remains
valid, (in relation to the workpiece zero set with G54 to G599)
G59 Replaces the absolute translation component of the programmable zero
offset for the specified axis, but the programmed absolute offset remains
valid
X Y Z Offset value in the direction of the specified geometry axis
Example
N...
N50 TRANS X10 Y10 Z10 ;Absolute translation component X10 Y10 Z10
N60 ATRANS X5 Y5 ;Additive translation component X5 Y5
= total offset X15 Y15 Z10
N70 G58 X20 ;Absolute translation component X20 + addit. X5 Y5
= total offset X25 Y15 Z10
N80 G59 X10 Y10 ;Additive translation component X10 Y10 + absolute X20 Y 10
= total offset X30 Y20 Z10
N...
Description
The absolute translation component is modified by the following commands:
• TRANS
• G58
• CTRANS
• CFINE
• $P_PFRAME[X,TR]
The additive translation component is modified by the following commands:
• ATRANS
• G59
• CTRANS
• CFINE
• $P_PFRAME[X,FI]
The table below describes the effect of various program commands on the absolute and
additive offsets.
Effect of the additive/absolute offset:
command Coarse or
absolute offset
Fine or additive
offset
Comment
TRANS X10 10 unchanged Absolute offset for X
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 239
G58 X10 10 unchanged Overwrites absolute offset for X
$P_PFRAME[X,TR] = 10 10 unchanged Progr. offset in X
ATRANS X10 unchanged Fine (old) + 10 Additive offset for X
G59 X10 unchanged 10 Overwriting additive offset for X
$P_PFRAME[X,FI] = 10 unchanged 10 Progr. fine offset in X
CTRANS(X,10) 10 0 Offset for X
CTRANS() 0 0 Deselection of offset (including fine
offset component)
CFINE(X,10) 0 10 fine offset in X
6.4 Programmable rotation (ROT, AROT, RPL)
Function
ROT/AROT can be used to rotate the workpiece coordinate system around each of the
geometry axes X, Y, Z or through an angle RPL in the selected working plane G17 to G19
(or around the perpendicular infeed axis). This allows inclined surfaces or several workpiece
sides to be machined in one setting.
Programming
ROT X… Y… Z… Substituting instruction for rotation in space
Or
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
240 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
ROT RPL=… Substituting instruction for rotation in the plane
Or
AROTX… Y… Z… Additive instruction for rotation in space
Or
AROT RPL=… Additive instruction for rotation in the plane
Each instruction must be programmed in a separate NC block.
Parameters
ROT, Absolute rotation with reference to the currently valid workpiece zero set
with G54 to G599
RPL, Rotation in the plane: Angle, through which the coordinate system is
rotated (plane set with G17-G19). The order, in which the rotation should
be performed can be defined via machine data. RPY notation is the default
setting (= roll, pitch, yaw) with Z,Y,X
AROT, Additive rotation with reference to the currently valid set or programmed
zero point
X Y Z Rotation in space: geometry axes, around which the rotation takes place
Example: Rotation in the plane
;
<
r r
5
With this workpiece, the illustrated shapes recur several times in the same program.
Rotations have to be performed in addition to the translation, because the shapes are not
arranged parallel to the axes.
N10 G17 G54 ;Working plane X/Y, workpiece zero
N20 TRANS X20 Y10 ;Absolute offset
N30 L10 ;Subprogram call
N40 TRANS X55 Y35 ;Absolute offset
N50 AROT RPL=45 ;Rotation of the coordinate system through 45°
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 241
N60 L10 ;Subprogram call
N70 TRANS X20 Y40 ;Absolute offset
; (cancels all previous offsets)
N80 AROT RPL=60 ;Additive rotation through 60°
N90 L10 ;Subprogram call
N100 G0 X100 Y100 ;Retraction
N110 M30 ;End of program
Example: Rotation in space
In this example, paraxial and inclined workpiece surfaces are to be machined in one setting.
Requirement: The tool must be aligned perpendicular to the inclined surface in the rotated Z
direction.
;
=
r
;
<
U
N10 G17 G54 ;Working plane X/Y, workpiece zero
N20 TRANS X10 Y10 ;Absolute offset
N30 L10 ;Subprogram call
N40 ATRANS X35 ;Additive offset
N50 AROT Y30 ;Rotation through the Y axis
N60 ATRANS X5 ;Additive offset
N70 L10 ;Subprogram call
N80 G0 X300 Y100 M30 ;Retraction, end of program
Example of multi-side machining
In this example, identical shapes on two perpendicular workpiece surfaces are machined by
using subprograms. The setup of the infeed direction, working plane and zero point in the
new coordinate system on the right-hand workpiece surface matches that of the top surface.
The conditions required for subprogram execution apply as before: Working plane G17,
coordinate plane X/Y, infeed direction Z.
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
242 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
=
=
;
;
<
<
*
*
N10 G17 G54 ;Working plane X/Y, workpiece zero
N20 L10 ;Subprogram call
N30 TRANS X100 Z-100 ;Absolute offset
=
;
<
=
;
<
N40 AROT Y90 ;Rotation of the coordinate system through Y
Z
X
Y
Z
X
Y
AROT Y90
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 243
N50 AROT Z90 ;Rotation of the coordinate system through Z
Z
X
Y
Z
X
Y
AROT Z90
N60 L10 ;Subprogram call
N70 G0 X300 Y100 M30 ;Retraction, end of program
Rotation in the plane
The coordinate system is
• rotated in the plane selected with G17 to G19.
Substituting statement, ROT RPL or additive statement, AROT RPL
• current plane, about which there is rotation with RPL= programmed rotation angle.
Note
See "Rotation in space" for more information.
=
;
<
*
*
*
=
;
<
=
*
*
*
527
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
244 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Plane change
Warning
If you program a change of plane (G17 to G19) after a rotation, the angles of rotation
programmed for the axes are retained and continue to apply in the new working plane. It is
therefore advisable to deactivate the rotation before a change of plane.
Deactivate rotation
For all axes: ROT (without axis parameter)
Caution
In both cases, all frame components of the previously programmed frame are reset.
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 245
Substituting statement, ROT X Y Z
The coordinate system is rotated through the programmed angle around the specified axes.
The center of rotation is the last specified settable zero offset (G54 to G599).
Caution
The ROT command cancels all frame components of the previously activated programmable
frame.
;
<
Note
A new rotation based on existing frames is programmed with AROT.
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
246 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Additive statement, AROT X Y Z
Rotation through the angle values programmed in the axis direction parameters. The center
of rotation is the currently set or last programmed zero point.
$527
527
<
;
Note
For both statements, please note the order and direction of rotation, in which the rotations
are performed (see next page)!
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 247
Direction of rotation
The following is defined as the positive direction of rotation: The view in the direction of the
positive coordinate axis and clockwise rotation.
=
<
;
Order of rotation
You can rotate up to three geometry axes simultaneously in one NC block.
The order of the RPY notation or Euler angle, through which the rotations are performed can
be defined in machine data.
MD 10600: FRAME_ANGLE_INPUT_MODE =
• RPY notation (RPY notation is the default setting)
• Euler angles
After that, the sequence Z, Y, X of the rotation is defined as follows:
Rotation around the 3rd geometry axis (Z)
Rotation around the 2nd geometry axis (Y)
Rotation around the 1st geometry axis (X)
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
248 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Z
Y
0
1
2
X
This order applies if the geometry axes are programmed in a single block. It also applies
irrespective of the input sequence. If only two axes are to be rotated, the parameter for the
3rd axis (value zero) can be omitted.
Value range with RPY angle
The angles are defined uniquely only within the following value ranges:
Rotation around 1st geometry axis: -180° ≤ X ≤ +180°
Rotation around 2nd geometry axis: -90° ≤ Y ≤ +90°
Rotation around 3rd geometry axis: -180° ≤ Z ≤ +180°
All possible rotations can be represented with this value range. Values outside the range are
normalized by the control into the above range during writing and reading. This value range
applies to all frame variables.
Examples of reading back in RPY
$P_UIFR[1] = CROT(X, 10, Y, 90, Z, 40)
returns on reading back
$P_UIFR[1] = CROT(X, 0, Y, 90, Z, 30)
$P_UIFR[1] = CROT(X, 190, Y, 0, Z, -200)
returns on reading back
$P_UIFR[1] = CROT(X, -170, Y, 0, Z, 160)
When frame rotation components are read and written, the value range limits must be
observed to ensure that the same results are obtained for read or write, or repeat write
operations
.
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 249
Value range with Euler angle
The angles are defined uniquely only within the following value ranges:
Rotation around 1st geometry axis: 0° ≤ X ≤ +180°
Rotation around 2nd geometry axis: -180° ≤ Y ≤ +180°
Rotation around 3rd geometry axis: -180° ≤ Z ≤ +180°
All possible rotations can be represented with this value range. Values outside the range are
normalized by the control into the above range. This value range applies to all frame
variables.
Caution
To ensure the angles written are read back unambiguously, it is necessary to observe the
defined value ranges.
Note
If you want to define the order of the rotations individually, program the desired rotation
successively for each axis with AROT.
References:
/FB1/Function Manual Basic Functions; Axes, Coordinate Systems, Frames (K2)
The working plane also rotates
The working plane defined with G17, G18 or G19 rotates with the spatial rotation.
Example: Working plane G17 X/Y, the workpiece coordinate system is positioned on the top
surface of the workpiece. Translation and rotation is used to move the coordinate system to
one of the side surfaces. Working plane G17 also rotates. This feature can be used to
program plane destination positions in X/Y coordinates and the infeed in the Z direction.
Frames
6.4 Programmable rotation (ROT, AROT, RPL)
Fundamentals
250 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
=
=
;
;
<
<
*
*
Requirement:
The tool must be positioned perpendicular to the working plane. The positive direction of the
infeed axis points in the direction of the toolholder. Specifying CUT2DF activates the tool
radius compensation in the rotated plane. For more information please refer to Section
"2D Tool Compensation, CUT2D CUT2DF".
Frames
6.5 Programmable frame rotations with solid angles (ROTS, AROTS, CROTS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 251
6.5 Programmable frame rotations with solid angles (ROTS, AROTS,
CROTS)
Function
Orientations in space can be specified by means of frame rotations with solid angles ROTS,
AROTS, CROTS. Programming commands ROTS and AROTS behave analogously to ROT
and AROT.
Programming
When programming the solid angles X and Y the new X-axis lies in the old ZX plane.
ROTS X... Y...
Or
AROTS X... Y...
Or
CROTS X... Y...
When programming solid angles Z and X the new Z-axis lies in the old YZ plane.
ROTS Z... X...
Or
AROTS Z... X...
Or
CROTS Z... X...
When programming the solid angles Y and Z the new Y-axis lies in the old XY plane.
ROTS Y... Z...
Or
AROTS Y... Z...
Or
CROTS Y... Z...
Frames
6.6 Programmable scale factor (SCALE, ASCALE)
Fundamentals
252 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
ROTS, Frame rotations with solid angles for spatial orientation of a plane
absolute, referred to the currently valid frame with set workpiece zero for
G54 to G599.
AROTS, Frame rotations with solid angles for spatial orientation of a plane
additive, referred to the currently valid frame with set or programmed zero
point.
CROTS, Frame rotations with solid angles for spatial orientation of a plane,
referred to the valid frame in the data management with rotation in the
specified axes.
X Y Z A maximum of two solid angles may be specified.
RPL Rotation in the plane: Angle through which the coordinate system is
rotated (plane set with G17-G19).
6.6 Programmable scale factor (SCALE, ASCALE)
Function
With SCALE/ASCALE you can program scale factors for all path, synchronized axes and
positioning axes in the direction of the axis specified in each case. This enables the size of a
shape to be changed. You can thus program taking similar geometrical shapes or different
shrinkages into account.
Programming
SCALE X… Y… Z… (substituting instruction programmed in a separate NC block)
Or
ASCALE X… Y… Z… (additive instruction programmed in a separate NC block)
Parameters
SCALE, Absolute enlargement/reduction with reference to the currently valid
coordinate system set with G54 to G599
ASCALE, Additive enlargement/reduction with reference to the currently valid set or
programmed coordinate system
X Y Z Scale factor in the direction of the specified geometry axis
Deactivate scaling factor
For all axes: SCALE (without axis parameter). All frame components of the previously
programmed frame are reset.
Example of milling
With this workpiece, the two pockets occur twice, but in different sizes and at different angles
to each other. The machining sequence is stored in a subprogram.
Frames
6.6 Programmable scale factor (SCALE, ASCALE)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 253
Use zero offset and rotation to set each of the workpiece zeroes, reduce the contour with a
scale and then call the subprogram up again.
;
<
r
N10 G17 G54 ;Working plane X/Y, workpiece zero
N20 TRANS X15 Y15 ;Absolute offset
N30 L10 ;Machine large pocket
N40 TRANS X40 Y20 ;Absolute offset
N50 AROT RPL=35 ;Rotation in the plane through 35°
N60 ASCALE X0.7 Y0.7 ;Scale factor for the small pocket
N70 L10 ;Machine small pocket
N80G0 X300 Y100 M30 ;Retraction, end of program
Substituting instruction, SCALE X Y Z
You can specify an individual scale factor for each axis, by which the shape is to be reduced
or enlarged. The scale refers to the workpiece coordinate system set with G54 to G57.
Notice
The SCALE command cancels all frame components of the previously activated
programmable frame.
Frames
6.6 Programmable scale factor (SCALE, ASCALE)
Fundamentals
254 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
=
<
Additive instruction, ASCALE X Y Z
You can program scale changes, which are to be added to existing frames by using the
ASCALE command. In this case, the last valid scale factor is multiplied by the new one.
The currently set or last programmed coordinate system is used as the reference for the
scale change.
AROT
TRANS
ASCALE
Note
If you program an offset with ATRANS after SCALE, the offset values are also scaled.
Frames
6.6 Programmable scale factor (SCALE, ASCALE)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 255
Caution
Please take great care when using different scale factors! Example: Circular interpolations
can only be scaled using identical factors. You can, however, use different scale factors to
program distorted circles, for example.
Frames
6.7 Programmable mirroring (MIRROR, AMIRROR)
Fundamentals
256 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
6.7 Programmable mirroring (MIRROR, AMIRROR)
Function
MIRROR/AMIRROR can be used to mirror workpiece shapes on coordinate axes. All
traversing movements, which are programmed after the mirror call, e.g., in the subprogram,
are executed in the mirror image.
Programming
MIRROR X0 Y0 Z0 (substituting instruction programmed in a separate NC block)
Or
AMIRROR X0 Y0 Z0 (additive instruction programmed in a separate NC block)
Parameters
MIRROR Absolute mirror image with reference to the currently valid coordinate
system set with G54 to G599
AMIRROR Additive mirror image with reference to the currently valid set or
programmed coordinate system
X Y Z Geometry axis whose direction is to be changed. The value specified
here can be chosen freely, e.g., X0 Y0 Z0.
Example of mirroring milling
Program the contour shown here once as a subprogram and generate the three other
contours with a mirror operation. The workpiece zero is located at the center of the contours.
;
;
;
<
<
<
;
<
N10 G17 G54 ;Working plane X/Y, workpiece zero
Frames
6.7 Programmable mirroring (MIRROR, AMIRROR)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 257
N20 L10 ;Machine first contour, top right
N30 MIRROR X0 ;Mirror X axis (the direction is changed in X)
N40 L10 ;Machine second contour, top left
N50 AMIRROR Y0 ;Mirror Y axis (the direction is changed in Y)
N60 L10 ;Machine third contour, bottom left
N70 MIRROR Y0 ;MIRROR cancels previous frames. Mirror Y axis (the direction is
;changed in Y)
N80 L10 ;Machine fourth contour, bottom right
N90 MIRROR ;Deactivate mirroring
N100 G0 X300 Y100 M30 ;Retraction, end of program
Example of rotating mirroring
The actual machining is stored as a subprogram and the execution at the respective spindles
is done by means of mirrorings and offsets.
=
:
=
0
:
0
;;
6SLQGOH 6SLQGOH
N10 TRANS X0 Z140 ;Zero offset to W
N.. ... ;Machine first side with spindle 1
N30 TRANS X0 Z600 ;Zero offset to spindle 2
N40 AMIRROR Z0 ;Mirroring of the Z axis
N50 ATRANS Z120 ;Zero offset to W1
N.. ... ;Machine second side with spindle 2
Substituting instruction, MIRROR X Y Z
The mirror is programmed by means of an axial change of direction in the selected working
plane.
Frames
6.7 Programmable mirroring (MIRROR, AMIRROR)
Fundamentals
258 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example: Working plane G17 X/Y
The mirror (on the Y axis) requires a change of direction on X and is subsequently
programmed with MIRROR X0. The contour is then mirrored on the opposite side of the
mirror axis Y.
;
<
0,5525;
0,5525<
The mirror image refers to the coordinate axes set with G54 to G57.
Caution
The MIRROR command cancels all previously set programmable frames.
Additive instruction, AMIRROR X Y Z
A mirror image, which is to be added to an existing transformation, is programmed with
AMIRROR. The currently set or last programmed coordinate system is used as the
reference.
Frames
6.7 Programmable mirroring (MIRROR, AMIRROR)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 259
75$16
$0,5525
Deactivate mirroring
For all axes: MIRROR (without axis parameter)
All frame components of the previously programmed frame are reset.
Note
The mirror command causes the control to automatically change the path compensation
commands (G41/G42 or G42/G41) according to the new machining direction.
;
<
*
0,5525;
*
**
The same applies to the direction of circle rotation (G2/G3 or G3/G2).
Frames
6.7 Programmable mirroring (MIRROR, AMIRROR)
Fundamentals
260 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
If you program an additive rotation with AROT after MIRROR, you may have to work with
reversed directions of rotation (positive/negative or negative/positive). Mirrors on the
geometry axes are converted automatically by the control into rotations and, where
appropriate, mirrors on the mirror axis specified in the machine data. This also applies to
settable zero offsets.
Machine manufacturer
• You can set the axis, around which mirroring is performed, via machine data MD.
MD 10610 = 0: Mirroring is performed in relation to the programmed axis (negation of
values).
MD 10610 = 1 or 2 or 3: Depending on the data setting, mirroring is performed in relation
to a specific reference axis (1=X axis; 2=Y axis; 3=Z axis) and rotations of two other
geometry axes.
• MD10612 MIRROR_TOGGLE = 0 can be used to define that the programmed values are
always evaluated. A value of 0, i.e., MIRROR X0, deactivates the mirroring of the axis,
and values not equal to 0 cause the axis to be mirrored if it is not already mirrored.
Frames
6.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 261
6.8 Frame generation according to tool orientation (TOFRAME, TOROT,
PAROT)
Function
TOFRAME generates a rectangular frame whose Z axis coincides with the current tool
orientation. You can use this function to retract the tool after a tool breakage in a 5-axis
program without collision, simply by retracting the Z axis. The resulting frame describing the
orientation is written in the system variable for the programmable frame $P_PFRAME.
Only the rotation component is overwritten with TOROT in the programmed frame. All other
components remain unchanged.
PAROT aligns the workpiece on the workpiece coordinate system (WCS).
Machine manufacturer
The position of the two axes X and Y can be defined in MD21110:
X_AXES_IN_OLD_X_Z_PLANE where X is rotated about Z into the existing X-Z plane.
=
;
*HQHUDWHG
)UDPH
7RROUHWUDFWLRQ
DORQJ=D[LV
<%DVH
=
;
<%DVH
%DVH
%DVH
¡
=
;
<
0RGLILHGLQ0';LVDJDLQ
ORFDWHGLQWKHSUHYLRXV;=SODQH
Frames
6.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT)
Fundamentals
262 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
TOFRAME Frame rotation in tool direction
Or
TOFRAMEZ or TOFRAMEY or
TOFRAMEX Z/Y/X axis parallel to tool orientation
Or
TOROTOF Frame rotation in tool direction OFF
Or frame rotation on with
TOROT or TOROTZ or TOROTY
or TOROTX
Z/Y/X axis parallel to tool orientation
Or
PAROT Align workpiece coordinate system (WCS) on workpiece
Or
PAROTOF Deactivate workpiece-related frame rotation
Parameters
TOFRAME Frame rotation in tool direction
The new frame, whose Z axis is pointing in the tool direction, is
applicable after the block containing TOFRAME. TOROTOF
deactivates the frame rotation in tool direction.
TOFRAMEZ
TOFRAMEY
TOFRAMEX
Z axis parallel to tool orientation
Y axis parallel to tool orientation
X axis parallel to tool orientation
TOROTOF Frame rotation in tool direction OFF
TOROT Frame rotation ON Z axis parallel to tool orientation. The rotation
defined by TOROT is the same as that defined with TOFRAME.
TOROTZ
TOROTY
TOROTX
Frame rotation ON Z axis parallel to tool orientation
Frame rotation ON Y axis parallel to tool orientation
Frame rotation ON X axis parallel to tool orientation
PAROT Align workpiece coordinate system (WCS) on workpiece.
Translations, scaling and mirroring in the active frame remain valid.
The workpiece-related frame rotation activated with PAROT is
deactivated with PAROTOF.
PAROTOF Deactivate workpiece-related frame rotation
Milling with working plane G17
TOFRAME or TOROT defines frames whose Z axes point in the tool direction. This definition
is tailored to milling operations, for which working plane G17 X/Y of the 1st – 2nd geometry
axis is typically active.
Turning with working plane G18 or G19
Frames
6.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 263
Turning operations in particular, and active G18 or G19 in general, require frames, with
which the tool is aligned in the X or Y axis. A frame of this type can be defined with G codes
• TOFRAMEX TOROTX
• TOFRAMEY TOROTY
• TOFRAMEZ
TOROTZ. This functionality of TOFRAME and TOFRAMEZ or TOROT and TOROTZ is
identical in each case.
Example of TOFRAME
N100 G0 G53 X100 Z100 D0
N120 TOFRAME
N140 G91 Z20 ;Frame TOFRAME is included, all programmed geometry axis
;movements
;refer to TOFRAME
N160 X50
...
Milling with working plane G17
TOFRAME or TOROT defines frames whose Z axes point in the tool direction. This definition
is tailored to milling operations, for which working plane G17 X/Y of the 1st – 2nd geometry
axis is typically active.
Turning with working plane G18 or G19
Turning operations in particular, and active G18 or G19 in general, require frames, with
which the tool is aligned in the X or Y axis. A frame of this type can be defined with G codes
• TOFRAMEX TOROTX
• TOFRAMEY TOROTY
• TOFRAMEZ
TOROTZ. This functionality of TOFRAME and TOFRAMEZ or TOROT and TOROTZ is
identical in each case.
Assigning axis direction
If one of the G codes TOFRAMEX, TOFRAMEY, TOROTX, TOROTY is programmed
instead of TOFRAME(Z) or TOROT(Z), the axis directions are assigned as shown in the
table below:
TOFRAME (Z),
TOROT (Z)
TOFRAMEY,
TOROTY
TOFRAMEX,
TOROTX
Z Y X Tool direction (applicate)
X Z Y Secondary axis (abscissa)
Frames
6.9 Deselect frame (G53, G153, SUPA, G500)
Fundamentals
264 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Y X Z Secondary axis (ordinate)
Note
After tool orientation has been programmed with TOFRAME, all the programmed geometry
axis movements refer to the frame generated by this programming.
Note
Separate system frame for TOFRAME or TOROT
The frames resulting from TOFRAME or TOROT can be written in a separate system frame
$P_TOOLFRAME.
This can be done by setting bit 3 in machine data MD 28082: MM_SYSTEM_FRAME_MASK.
The programmable frame remains unchanged. Differences occur when the programmable
frame is processed further elsewhere.
Note
NC command TOROT ensures consistent programming with active orientable tool carriers
for each kinematic type. Just as in the situation for rotatable toolholders, PAROT can be
used to activate a rotation of the work table. This defines a frame, which changes the
position of the workpiece coordinate system in such a way that no compensatory movement
is performed on the machine. Language command PAROT is not rejected if no orientable
toolholder is active.
References: For further explanations about machines with orientable toolholder, see:
/PGA/Programming Manual Advanced; "Tool Orientation"
/FB1/Function Manual Basic Functions; Tool Offset (W1),
"Orientable Toolholders"
6.9 Deselect frame (G53, G153, SUPA, G500)
Function
When executing certain processes, such as approaching the tool change location or initial
setting, various frame components must be defined and suppressed at different times. Set
frames can either be deactivated modally or suppressed non-modally.
The programmable frames are cleared by specifying the TRANS, ROT, SCALE, MIRROR
component without an axis.
Frames
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF, CORROF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 265
Deactivate coordinate transformation
A distinction must be made here between non-modal suppression and modal deactivation.
Programming
G53
Or
G153
Or
SUPA
Or
G500
Parameters
Non-modal suppression:
G53 Deactivation of all programmable and settable frames
G153 Deactivation of all programmable, settable and basic frames
SUPA Deactivation of all programmable, settable frames, DRF handwheel offsets,
external zero offsets and preset offset
Modal deactivation:
G500 Deactivation of all settable frames if G500 does not contain a value
Deleting FRAMES:
TRANS, ROT, SCALE,
MIRROR
Programming without specifying the axis → clearing the programmable
frames
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF,
CORROF)
Function
DRFOF can be used to deactivate all active axes of the channel for DRF handwheel offsets.
Frames
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF, CORROF)
Fundamentals
266 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
For instance, if a particular axis with an overlaid motion or a position offset interpolates, the
instruction CORRROF can be used to deactivate either the DRF offsets or the position offset
for this axis. The axis is not traversed.
Programming
DRFOF
Or
CORROF(axis,string[axis,string])
Or
CORROF(axis,string)
Or
CORROF(axis)
Or
CORROF()
Parameters
Modal deactivation:
DRFOF Deactivation (deselection) of DRF handwheel offsets for all active axes in
the channel
CORROF(axis,DRF[AXIS
,AA_OFF])
Deactivation (deselection) of axial DRF offsets and the position offset for
individual axes as a result of $AA_OFF
CORROF(axis) All active overlaid motions are deselected
Axis Axis identifiers (for channel, geometry or machine axis)
String == DRF DRF offset of axis is deselected
String == AA_OFF Position offset of axis is deselected due to $AA_OFF
The following expansions are possible:
String == ETRANS An active zero offset is deselected
String == FTOCOF, Acts like FTOCOF (deactivate online tool offset)
Example of axial DRF deselection
A DRF offset is generated in the X axis by DRF handwheel traversal. No DRF offsets are
operative for any other axes in the channel.
N10 CORROF(X,"DRF") acts like DRFOF( )
A DRF offset is generated in the X and Y axes by DRF handwheel traversal. No DRF offsets
are operative for any other axes in the channel.
N10 CORROF(X,"DRF") ;Only the DRF offset of the X axis is deselected, the
;X axis does not move
;The DRF offset of the Y axis is ;retained
;Both offsets would have been deselected with
;DRFOF()
Frames
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF, CORROF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 267
Example of axial DRF deselection and $AA_OFF deselection
A DRF offset is generated in the X axis by DRF handwheel traversal. No DRF offsets are
operative for any other axes in the channel.
N10 WHEN TRUE DO $AA_OFF[X] = 10
G4 F5
;A position offset == 10 is ;interpolated for the X axis
N70 CORROF(X,"DRF",X,"AA_OFF") ;Only the DRF offset of the X axis is ;deselected,
the X axis does not move
;The DRF offset of the Y axis is ;retained
Example of deselecting AA_OFF
A position offset of the X axis is deselected with: CORROF(X,"AA_OFF") with $AA_OFF[X] =
0 and added to the current position of the X axis.
The following programming example shows the relevant programming commands for the X
axis that was previously interpolated with a position offset of 10:
N10 WHEN TRUE DO $AA_OFF[X] = 10
G4 F5
;A position offset == 10 is ;interpolated for the X axis
N80 CORROF(X,"AA_OFF") ;Delete position offset of X axis
;the X axis does not move
Description
CORROF
A preprocessing stop is initiated and the position component of the deselected overlaid
motion (DRF offset or position offset) is transferred to the position in the basic coordinate
system. Since no axis is traversed, the value of $AA_IM[axis] does not change. Owing to the
deselected overlaid motion, only the value of system variable $AA_IW[axis] is altered.
After the position offset, e.g., for one axis, has been deselected by
$AA_OFF, the system variable
$AA_OFF_VAL of this axis is zero.
Setting bit 2 of MD 36750: AA_OFF_MODE to "1" when $AA_OFF is changed enables
interpolation of the position offset as an overlaid motion in JOG mode.
Frames
6.10 Deselect DRF (handwheel) offsets, overlaid motions (DRFOF, CORROF)
Fundamentals
268 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
CORROF is possible only from the parts program, not via synchronized actions.
Alarm 21660 is output if a synchronized action is active when the position offset is
deselected via parts program command CORROF(axis,"AA_OFF"). $AA_OFF is deselected
simultaneously and not set again. If the synchronized action becomes active later in the
block after CORROF, $AA_OFF remains set and a position offset is interpolated.
If a CORROF command has been programmed for an axis and this axis is active in a
different channel, then an axis replacement sends the axis to the other channel with machine
data 30552: AUTO_GET_TYPE = 0. This causes the DRF offset and any other position
offset to be deselected.
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 269
Feedrate Control and Spindle Motion 7
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Function
You can use the above commands to set the feedrates in the NC program for all axes
participating in the machining sequence.
;
<
)
0RYHPHQWRQ<
0RYHPHQWRQ;
The path feedrate is generally composed of the individual speed components of all geometry
axes participating in the movement and refers to the center point of the cutter or the tip of the
turning tool.
The following feedrate types can be programmed:
• Path feedrate with G commands G93, G94, G95 on axes participating in movement
• Feedrate F for path axes
• Feedrate F for synchronized axes
• Feedrate F applies to all axes programmed under FGROUP
• Feedrate for synchronized-/path axes with limit speed FL
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
270 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
The inverse-time feedrate 1/min G93 is not implemented for 802D.
Programming
G93 or G94 or G95
F…
or
FGROUP (X, Y, Z, A, B, …)
Or
FL[axis]=…
or
FGREF[axis name]=reference radius
Parameters
G93 Inverse-time feedrate 1/rpm
G94 Feedrate in mm/min or inches/min or in deg/min
G95 Feedrate in mm/rev or inches/rev with reference to the speed of the master
spindle – generally the cutting spindle or the main spindle on the turning
machine
F… Feedrate value in unit defined by G93, G94, G95
FGROUP Feedrate value F valid for all axes specified in FGROUP
FL Limit speed for synchronized/path axes; the unit set with G94 applies
(max. rapid traverse) One FL value can be programmed per axis. The axis
identifiers of the basic coordinate system must be used (channel axes or
geometry axes).
FGREF Effective radius (reference radius) for the rotary axes entered in FGROUP
Axis Channel axis or geometry axes or orientation axes
X Y Z Movement of the specified geometry axis
A B C Axis identifier for rotary axis to be traversed
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 271
Example of operating principle of FGROUP
The following example illustrates the effect of FGROUP on the path and the path feedrate.
The variable $AC_TIME contains the time from the start of the block in seconds. It can only
be used in synchronized actions. See /FBSY/, Synchronized Actions.
N100 G0 X0 A0
N110 FGROUP(X,A)
N120 G91 G1 G710 F100 ;Feedrate=100 mm/min or 100 deg/min
N130 DO $R1=$AC_TIME
N140 X10 ;Feedrate=100 mm/min, path dist.=10 mm, R1=approx. 6 s
N150 DO $R2=$AC_TIME
N160 X10 A10 ;Feedrate=100 mm/min, path dist.=14.14 mm, R2=approx. 8 s
N170 DO $R3=$AC_TIME
N180 A10 ;Feedrate=100 degrees/min, path dist.=10 degrees, R3=approx. 6 s
N190 DO $R4=$AC_TIME
N200 X0.001 A10 ;Feedrate=100 mm/min, path dist.=10 mm, R4=approx. 6 s
N210 G700 F100 ;Feedrate=2540 mm/min or 100 degrees/min
N220 DO $R5=$AC_TIME
N230 X10 ;Feedrate=2540 mm/min, path dist.=254 mm, R5=approx. 6 s
N240 DO $R6=$AC_TIME
N250 X10 A10 ;Feedrate=2540 mm/min, path dist.=254.2 mm, R6=approx. 6 s
N260 DO $R7=$AC_TIME
N270 A10 ;Feedrate=100 degrees/min, path dist.=10 degrees, R7=approx. 6 s
N280 DO $R8=$AC_TIME
N290 X0.001 A10 ;Feedrate=2540 mm/min, path dist.=10 mm, R8=approx. 0.288 s
N300 FGREF[A]=360/(2*$PI) ;1 degree=1 inch above the effective radius
N310 DO $R9=$AC_TIME
N320 X0.001 A10 ;Feedrate=2540 mm/min, path dist.=254 mm, R9=approx. 6 s
N330 M30
Example of traversing synchronized axes with limit speed FL
The path velocity of the path axes is reduced if the synchronized axis reaches the limit
speed.
Example, Z is a synchronized axis:
N10 G0 X0 Y0
N20 FGROUP(X)
N30 G1 X1000 Y1000 G94 F1000 FL[Y]=500
N40 Z-50
One FL value can be programmed per axis. The axis identifiers of the basic coordinate
system must be used (channel axes or geometry axes).
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
272 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of helical interpolation
Path axes X and Y traverse with the programmed feedrate, the infeed axis Z is a
synchronized axis.
;
<
=
<
N10 G17 G94 G1 Z0 F500 ;Tool infeed
N20 X10 Y20 ;Approach start position
N25 FGROUP(X, Y) ;Axes X/Y are path axes, Z is a
;synchronized axis
N30 G2 X10 Y20 Z-15 I15 J0 F1000
FL[Z]=200
;On the circular path, the feedrate is1000 mm/min.
;Traversing in the Z direction is synchronized.
...
N100 FL[Z]=$MA_AX_VELO_LIMIT[0,Z] ;The limit velocity is deselected
;when the velocity
;value is read from the MD.
N110 M30 ;End of program
Feedrate G93, G94, G95
All of the commands are modal. If the G feedrate command is switched between G93, G94
or G95, the path feedrate must be reprogrammed. The feedrate can also be specified in
deg/rev when machining with rotary axes.
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 273
Feedrate F for path axes
The feedrate is specified with address F. Depending on the default setting in the machine
data, the units of measurement specified with the G commands are either in mm or inch.
One F value can be programmed per NC block. The unit for the feedrate is defined in one of
the above G commands. The feed F acts only on path axes and remains active until a new
feedrate is programmed. Separators are permitted after address F.
Example: F100 or F 100 or F.5 or F=2*FEED
Feedrate for synchronized axes
The feedrate F programmed at address F applies to all the path axes programmed in the
block, but not to synchronized axes. The synchronized axes are controlled such that they
require the same time for their path as the path axes, and all axes reach their end point at
the same time.
Traverse synchronized axes with limit speed FL
With this command, synchronized/path axes are traversed at their limit speed FL.
Traverse synchronized axes with path velocity F, FGROUP
With FGROUP, you define whether a path axis is to be traversed with path feed or as a
synchronized axis. In helical interpolation, for example, you can define that only two
geometry axes, X and Y, are to be traversed at the programmed feedrate. The infeed axis Z
is the synchronized axis in this case.
Example: N10 FGROUP(X, Y)
Change FGROUP
1. By reprogramming another FGROUP statement.
Example: FGROUP(X, Y, Z)
2. With FGROUP () without axis parameter
Afterwards, the initial setting in the machine data applies – the geometry axes again traverse
in the path axis grouping.
Note
You must program channel axis names with FGROUP.
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
274 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Caution
The FGREF evaluation also works if only rotary axes are programmed in the block. The
normal F value interpretation as degree/min applies in this case only if the radius reference
corresponds to the FGREF default, when
G71/G710: FGREF[A]=57.296
G70/G700: FGREF[A]=57.296/25.4
Units of measurement and calculation
Machine manufacturer
See machine manufacturer's specifications.
Units of measurement for feedrate F
You can use the following G commands to define the units of measurement for the feed
input. Feedrate functions are not affected by G70/G71.
Note
With G700/G710, feedrate values F are interpreted as geometrical parameters in the
measuring system set by G function (G700: [inch/min]; G710: [mm/min]).
Feedrate G93
Unit 1/rpm. The inverse-time feedrate specifies the time required to execute the motion
commands in a block.
Example: N10 G93 G01 X100 F2 means: the programmed path is traversed in 0.5 min.
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 275
;
<
*;)
PLQ
Note
If the path lengths vary greatly from block to block, a new F value should be specified in
each block with G93. The feedrate can also be specified in deg/rev when machining with
rotary axes.
Unit of measurement for synchronized axes with limit speed FL
The unit of measurement set for F by G command (G70/G71) also applies to FL. If FL is not
programmed, rapid traverse velocity is used. FL is deselected by assignment to MD
$MA_AX_VELO_LIMIT.
Unit of measurement for rotary and linear axes
For linear and rotary axes, which are combined with FGROUP and traverse a path together,
the feed is interpreted in the unit of measurement of the linear axes. Depending on the
default for G94/G95: mm/min or inch/min and mm/rev or inch/rev.
The tangential velocity of the rotary axis in mm/min or inch/min is calculated according to the
following formula:
F[mm/min] = F'[degrees/min] * π * D[mm]/360[degrees]
F: Tangential velocity
F': Angular velocity
π: Circle constant
D: Diameter
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
276 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
D
F
F'
Traverse rotary axes with path velocity F, FGREF
For machining operations, in which the tool or the workpiece or both are moved by a rotary
axis, the effective machining feedrate is to be interpreted as a path feed in the usual way by
reference to the F value. This requires the specification of an effective radius (reference
radius) FGREF for each of the rotary axes involved.
The unit of the reference radius depends on the G70/G71/G700/G710 setting.
All axes involved must be included in the FGROUP command, as before, in order to be
evaluated in the calculation of the path feed.
In order to ensure compatibility with the behavior with no FGREF programming, the factor 1
degree = 1mm is activated on system powerup and RESET. This corresponds to a reference
radius of FGREF=360 mm/(2π)=57.296 mm.
Note
This default setting is independent of the active basic system MD 10240:
SCALING_SYSTEM_IS_METRIC and of the currently active inch/metric G code.
Special situations: With the following programming:
N100 FGROUP(X,Y,Z,A)
N110 G1 G91 A10 F100
N120 G1 G91 A10 X0.0001 F100
the F value programmed in N110 is evaluated as a rotary axis feedrate in deg/min, while the
feedrate weighting in N120 is either 100 inch/min or 100 mm/min depending on the currently
active inch/metric setting.
Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 277
Path reference factors for orientation axes with FGREF
With orientation axes the mode of operation of the FGREF[ ] factors is dependent on
whether the change in the orientation of the tool is implemented by rotary axis or vector
interpolation.
In the case of rotary axis interpolation, the relevant FGREF factors of the orientation axes
are calculated, as for rotary axes, individually as reference radius for the axis paths.
In the case of vector interpolation, an effective FGREF factor, which is calculated as the
geometric mean value of the individual FGREF factors, is applied.
FGREF[eff] = n-te root of:[(FGREF[A] * FGREF[B]...)]
They are:
A: Axis identifier of 1st orientation axis
B: Axis identifier of 2nd orientation axis
C: Axis identifier of 3rd orientation axis Number of orientation axes
Example: There are two orientation axes for a standard 5-axis transformation, and the
effective factor is thus the root of the product of the two axial factors:
FGREF[eff] = square root of:[(FGREF[A] * FGREF[B])]
Note
With the effective factor for orientation axes FGREF, it is therefore possible to define a
reference point on the tool, to which the programmed path feedrate refers.
Feedrate Control and Spindle Motion
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC)
Fundamentals
278 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP,
WAITMC)
Function
Positioning axes are traversed independently of the path axes at a separate, axis-specific
feedrate. There are no interpolation commands. With the POS/POSA/POSP commands, the
positioning axes are traversed and the sequence of motions coordinated at the same time.
The following are typical examples of positioning axes: pallet feed equipment, gauging
stations or similar.
WAITP enables you to identify a position in the NC program where the program is to wait
until an axis programmed with POSA in a previous NC block has reached its end position.
With WAITMO, the next NC block is loaded immediately when the wait marker is received.
Programming
POS[axis]=...
Or
POSA [axis]=…
Or
POSP [axis]=(…,…,…)
Or
FA [axis]=...
Or
WAITP (axis)=… (programming must be written in a separate NC block)
Or
WAITMC(marker)=…
Parameters
POS [axis]= Position the axis; the next NC block is not enabled until the position has
been reached
POSA [axis]= Position the axis; the next NC block is enabled, even if the position has
not been reached
POSP [axis]=(,,) Approach end position in sections. The first value indicates the end
position; the second the length of the section. Approaching the end
position is defined in the third value with 0 or 1
FA[axis]= Feedrate for the positioning axis, up to 5 per NC block
WAITP (axis) Waiting for end of travel of axis. With WAITP, an axis can be made
available for traversing as a reciprocating axis or as a concurrent
positioning axis (by PLC).
WAITMC (marker) During the braking ramp, WAIITMC loads the next NC block
immediately when the WAIT marker is received.
Feedrate Control and Spindle Motion
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 279
Axis Channel axes or geometry axes
Marker, , An axis is only decelerated if the marker has not yet been reached or if
a different search criterion prevents the block change.
Example of traveling with POSA[…]=
On accessing status data of the machine ($A...), the control generates an internal
preprocessing stop
,
processing is halted until all blocks, which have already been
preprocessed and, have been executed in full.
N40 POSA[X]=100
N50 IF $AA_IM[X]==R100 GOTOF LABEL1 ;Access to machine status data
N60 G0 Y100
N70 WAITP(X)
N80 LABEL1:
N...
Example of waiting for end of travel with WAITP(...)
Pallet feed equipment
Axis U: Pallet store, transporting the pallet to the working area
Axis V: Transfer line to a measuring station, where sampling controls are carried out:
N10 FA[U]=100 FA[V]=100 ;Axis-specific feedrate functions for ;each
positioning axis U and V
N20 POSA[V]=90 POSA[U]=100 G0 X50 Y70 ;Traverse positioning and path axes
N50 WAITP(U) ;Execution of the program is only
;continued when axis U has reached the
;end position programmed in N20.
N60 …
Feedrate Control and Spindle Motion
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC)
Fundamentals
280 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Traveling with POSA[…]=
The axis indicated in square brackets is traversed to the end position. The block step enable
or program execution is not affected by POSA. The movement to the end position can be
performed during execution of subsequent NC blocks.
Caution
Internal preprocessing stop
If a command, which implicitly causes a preprocessing stop, is read in a following block, this
block is not executed until all other blocks, which are already preprocessed and stored have
been executed. The preceding block is halted in exact stop (as with G9).
Traveling with POS[…]=
The next block is only executed when all axes programmed under POS have reached their
end positions.
Traveling with POSP[...]=
POSP is deployed especially for programming oscillating motions, see
/PGA/Programming Manual Advanced; "Asynchronous Oscillation"
Wait for end of travel with WAITP(...)
After WAITP, assignment of the axis to the NC program is no longer valid; this applies until
the axis is programmed again. This axis can then be operated as a positioning axis through
the PLC, or as a reciprocating axis from the NC program/PLC or HMI.
Block change in the braking ramp with IPOBRKA and WAITMC(...)
An axis is only decelerated if the marker has not yet been reached or if a different search
criterion prevents the block change. After a WAITMC, the axes start immediately if no other
search criterion prevents block change.
Feedrate Control and Spindle Motion
7.3 Position-controlled spindle operation (SPCON, SPCOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 281
7.3 Position-controlled spindle operation (SPCON, SPCOF)
Function
In some cases, position-controlled operation of the spindle may be advisable, e.g., in
conjunction with large-pitch thread cutting with G33, higher quality can be achieved.
Note
The command requires up to three interpolation cycles.
Programming
SPCON or SPCON(n) Activate position control
or
SPCOF or SPCOF(n) Deactivate position control, switch to speed control
or
SPCON(n, m, 0) Activate position control for multiple spindles in a block
or
SPCOF(n, m, 0) Deactivate position control for multiple spindles in a block
Parameter
SPCON
SPCON(n)
Switch master spindle or spindle number n from speed control to
position control
SPCOF
SPCOF(n)
Switch master spindle or spindle number n back from position control to
speed control
SPCON
SPCON(n, m, 0)
Several spindles with number n can be switched from speed control to
position control in one block
SPCOF
SPCOF(n, m, 0)
Several spindles with number n can be switched back from position
control to speed control in one block
n
m
Integers from 1 ... n of spindle number
Integers from 1 ... m of master spindle
Note
SPCON has modal action and remains valid until SPCOF.
The speed is specified with S... M3, M4 and M5 apply in respect of the directions of rotation
and spindle stop.
With synchronized spindle setpoint value linkage, the master spindle must be operated in
position-control mode.
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
282 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Function
With SPOS, M19 and SPOSA, you can position spindles at specific angular positions, e.g.,
during tool change. In order to synchronize spindle movements, WAITS can be used to wait
until the spindle position is reached.
$QJOHSRVLWLRQ
The spindle can also be operated as a path axis, synchronized axis or positioning axis at the
address defined in the machine data. When the axis identifier is specified, the spindle is in
axis mode. M70 switches the spindle directly to axis mode.
Switching off
SPOS, M19 and SPOSA effect a temporary switchover to position-controlled operation until
the next M3 or M4 or M5 or M41 to M45. If the position control was activated with SPCON
prior to SPOS, then this remains active until SPCOF is issued.
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 283
Programming
SPOS=… or SPOS[n]=…
Or
M19 or M[n]=19
Or
SPOSA=… or SPOSA[n]=…
Or
M70 or Mn=7
Or
FINEA=… or FINEA[n]=…
Or
COARSEA=… or COARSEA[n]=…
Or
IPOENDA=… or IPOENDA[n]=…
Or
IPOBRKA=… or IPOBRKA(axis[,REAL]) (programmed in a separate NC block)
Or
WAITS or WAITS(n,m) (programmed in a separate NC block)
Parameters
SPOS=
SPOS[n]=
Position master spindle (SPOS or SPOS[0]) or spindle number n
(SPOS[n]); the next NC block is not enabled until the position has
been reached.
M19
M[n]=19
Position master spindle (M19 or M[0]=19) or spindle number n
(M[n]=19); the next NC block is not enabled until the position has
been reached.
SPOSA=
SPOSA[n]=
Position master spindle (SPOSA or SPOSA[0]) or spindle with number
n (SPOSA[n]); the next NC block is enabled, even if the position has
not been reached.
M70
Mn=70
Switch over master spindle (M70) or spindle number n (Mn=70) to
axis operation. No defined position is approached. The NC block is
enabled after the switchover has been performed.
FINEA=
FINEA[Sn]=
Motion end when "Exact stop fine" reached
End of positioning for specified spindle Sn
COARSEA=
COARSEA[Sn]=
Motion end when "Exact stop coarse" reached
End of positioning for specified spindle Sn
IPOENDA=
IPOENDA[Sn]=
End of motion when “IPO stop” is reached
End of positioning for specified spindle Sn
IPOBRKA=
IPOBRKA(axis[,Real])=
End of motion criterion from moment of application of braking ramp at
100% down to end of braking ramp at 0% and identical to IPOENDA.
IPOBKRA must be programmed in round parenthesis "()".
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
284 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
WAITS
WAITS(n,m)
Wait for spindle position to be reached, spindle stop after M5, spindle
speed after M3/M4
WAITS applies to the master spindle, WAITS( ..., ...) for the specified
spindle numbers
n
m
Sn
Integers from 1 ... n of spindle number
Integers from 1 ... m of master spindle
nth Spindle number, 0 to max. spindle number
Axis
Real
Channel identifier
Percentage specification 100-0% referred to the braking ramp for
block changes. If no % is specified, the current value of the setting
data is applied.
Specify spindle position
The spindle position is specified in degrees. Three spindle positions are possible for each
NC block. If nothing is specified, traversing automatically takes place as for DC. With
incremental dimensioning IC (INC), spindle positioning can take place over several
revolutions.
AC(…) Absolute dimension, value range AC: 0…359.9999 degrees
IC(…) Absolute dimension, value range IC: 0…±99 999.999 degrees
DC(…) Approach absolute value directly
ACN(…) Absolute dimension, approach in negative direction
ACP(…) Absolute dimension, approach in positive direction
Example of positioning spindle with negative direction of rotation
Position spindle 2 at 250° in negative direction of rotation.
N10 SPOSA[2]=ACN(250) ;The spindle decelerates if necessary and accelerates in the
;opposite direction to the positioning
;movement
'&
$&
r
r
;
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 285
Example, spindle positioning in the axis mode
...
N10 M3 S500
...
N90 SPOS[2]=0 or ;Position control on, spindle 2 positioned to 0, axis mode
;can be used in the next block.
M2=70 ;Spindle 2 is switched to axis mode
N100 X50 C180 ;Spindle 2 (C axis) is traversed with linear interpolation
;synchronous to X.
N110 Z20 SPOS[2]=90 ;Spindle 2 is positioned to 90 degrees.
Example of drilling cross holes in turned part
Cross holes are to be drilled in this turned part. The running drive spindle (master spindle) is
stopped at zero degrees and then successively turned through 90°, stopped and so on.
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
286 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
=
; ;
....
N110 S2=1000 M2=3 ;Switch on cross drilling attachment
N120 SPOSA=DC(0) ;Position main spindle directly at 0°,
;the program will advance to the next block immediately
N125 G0 X34 Z-35 ;Switch on the drill while the spindle is being positioned
N130 WAITS ;Wait until the main spindle reaches its position
N135 G1 G94 X10 F250 ;Feedrate in mm/min (G96 is suitable only for the multi-edge turning
;tool and synchronous spindle, but not for power tools on the cross
;slide)
N140G0 X34
N145 SPOS=IC(90) ;The spindle is positioned through 90° with read halt in a
;positive direction
N150 G1 X10
N155 G0 X34
N160 SPOS=AC(180) ;The spindle is positioned at 180° with respect to the
;spindle zero point
N165 G1 X10
N170 G0 X34
N175 SPOS=IC(90) ;The spindle turns in
;a positive direction through 90° from the absolute 180° position,
;ending up in the absolute 270° position.
N180 G1 X10
N185 G0 X50
...
Requirements
The spindle must be capable of operation in position-control mode.
Position with SPOSA=, SPOSA[n]=
The block step enable or program execution is not affected by SPOSA. The spindle
positioning can be performed during execution of subsequent NC blocks. The program
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 287
moves onto the next block if all the functions (except for spindle) programmed in the current
block have reached their block end criterion. The spindle positioning operation may be
programmed over several blocks (see WAITS).
Notice
If a command, which implicitly causes a preprocessing stop, is read in a following block,
execution of this block is delayed until all positioning spindles are stationary.
Positioning with SPOS=, SPOS[n]= and positioning with M19=, M19[n]=
The block step enabling condition is fulfilled when all functions programmed in the block
have reached their block end criterion (e.g., all auxiliary functions acknowledged by the PLC,
all axes have reached end point) and the spindle has reached the programmed position.
Speed of the movements
The speed or delay response for positioning is stored in the machine data and can be
programmed.
Specify spindle position
As the commands G90/G91 have no effect here, the corresponding units of measurements
such as AC, IC, ACN, ACP explicitly apply. If nothing is specified, traversing automatically
takes place as for DC.
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
288 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
End of positioning
Programmable by means of the following commands: FINEA [Sn], COARSEA [Sn],
IPOENDA [Sn].
Settable block change time
For single axis interpolation mode, a new end of motion can be set in addition to the existing
end of motion criteria based on FINEA, COARSEA, IPOENDA.The new criterion can be set
within the braking ramp (100-0%) using IPOBRKA.
The program advances to the next block if the end of motion criteria for all spindles or axes
programmed in the current block plus the block change criterion for path interpolation are
fulfilled. Example:
N10 POS[X]=100
N20 IPOBRKA(X,100)
N30 POS[X]=200
N40 POS[X]=250
N50 POS[X]=0
N60 X10 F100
N70 M30
Block changes if the X axis has reached position 100 and exact stop fine. Activate block
change criterion IPOBRKA braking ramp. Block change commences as soon as the X axis
starts to decelerate. The X axis does not brake at position 200, but moves on to position 250;
as soon as the X axis starts to brake, the block changes. The X axis brakes and returns to
position 0, the block is changed at position 0 and exact stop fine.
Synchronizing spindle motions WAITS, WAITS(n,m)
WAITS can be used to identify a point at which the NC program waits until one or more
spindles programmed with SPOSA in a previous NC block have reached their positions.
Example: The block waits until spindles 2 and 3 have reached the positions specified in
block N10.
N10 SPOSA[2]=180 SPOSA[3]=0
N20…N30
N40 WAITS(2,3)
WAITS can be used after M5 to wait until the spindle(s) has(have) stopped. WAITS can be
used after M3/M4 to wait until the spindle(s) has(have) reached the specified speed/direction
of rotation.
Note
If the spindle has not yet been synchronized with synchronization marks, the positive
direction of rotation is taken from the machine data (state on delivery).
Position spindle from rotation (M3/M4)
When M3 or M4 is active, the spindle comes to a standstill at the programmed value.
Feedrate Control and Spindle Motion
7.4 Positioning spindles (SPOS, M19 and SPOSA, WAITS)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 289
'& $&
'& $&
'LUHFWLRQRIURWDWLRQ
3URJUDPPHG
DQJOH
3URJUDPPHG
DQJOH
'LUHFWLRQRIURWDWLRQ
There is no difference between DC and AC dimensioning. In both cases, rotation continues
in the direction selected by M3/M4 until the absolute end position is reached. With ACN and
ACP, deceleration takes place if necessary, and the appropriate approach direction is
followed. With IC, the spindle rotates additionally to the specified value starting at the current
spindle position.
When M3 or M4 is active, the spindle decelerates if necessary, and accelerates in the
programmed direction of rotation.
Position a spindle from standstill (M5)
The exact programmed distance is traversed from standstill (M5).
Feedrate Control and Spindle Motion
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF)
Fundamentals
290 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF)
Function
Positioning axes, such as workpiece transport systems, tool turrets and end supports, are
traversed independently of the path and synchronized axes. A separate feedrate is therefore
defined for each positioning axis. Example: FA[A1]=500.
FPRAON can be used to axially activate the revolutional feedrate for positioning axes and
spindles, and FPRAOF can be used to deactivate the respective axis again.
Programming
FA [axis]=...
FA[SPI(spindle)]=… or FA[S…]=…
or
FPR (rotary axis ) or FPR(SPI(spindle)) or FPR(S…)
Or
FPRAON (axis, rotary axis)
Or
FPRAON(axis,SPI(spindle)) or FPRAON(axis,S…)
or
FPRAON(SPI(spindle),rotary axis) or FPRAON(S…,rotary axis)
or
FPRAON(SPI(spindle),SPI(spindle)) or FPRAON(S…,S…)
or
FPRAOF(axis,SPI(spindle),…) or FPRAOF(axis,S…,…)
Parameters
FA[axis] Feedrate for the specified positioning axis in mm/min or inch/min or
deg/min
FA[SPI(spindle)]
FA[S…]
Positioning velocity (axial feed)
for the specified spindles in deg/min.
FPR Identification of the rotary axis or spindle whose revolutional feedrate
programmed in G95 is to be used as the basis for the revolutional
feedrate of the path and synchronized axes.
FPRAON Activate revolutional feedrate for positioning axes and spindles axially.
The first command identifies the positioning axis/spindle that is to be
traversed at a revolutional feedrate. The second command identifies
the rotary axis/spindle from which the feedrate must be derived.
FPRAOF Deactivate revolutional feedrate. Specification of axis or spindle that is
to stop traversing at a revolutional feedrate.
Feedrate Control and Spindle Motion
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 291
SPI Converts the spindle number into an axis identifier; the transfer
parameter must contain a valid spindle number. SPI is used for the
indirect definition of a spindle number.
Axis Positioning axes or geometry axes
Range of values …999 999.999 mm/min, degree/min
…39 999.9999 inch/min
Note
The programmed feedrate FA[...] is modal.
Up to 5 feeds for positioning axes or spindles can be programmed in each NC block.
Example of synchronous spindle link
With synchronous spindle link, the positioning speed of the following spindle can be
programmed independently of the master spindle – for example, for positioning operations.
Example: FA[S2]=100
The spindle identifiers SPI(...) and S... are identical in terms of function.
Example of calculating the derived feedrate FPR
The derived feedrate is calculated according to the following formula:
Derived feedrate = programmed feedrate * Absolute master feedrate
Example: Path axes X, Y must be traversed at the revolutional feedrate derived from rotary
axis A:
N40 FPR(A)
N50 G95 X50 Y50 F500
Feedrate FA[…]
The feedrate is always G94. When G70/G71 is active, the unit of measurement is
metric/inches according to the default setting in the machine data. G700/G710 can be used
to modify the unit of measurement in the program.
Notice
If no FA is programmed, the value defined in the machine data applies.
Feedrate Control and Spindle Motion
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF)
Fundamentals
292 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Feedrate FPR[...]
As an extension of the G95 command (revolutional feedrate referring to the master spindle),
FPR allows the revolutional feedrate to be derived from any chosen spindle or rotary axis.
G95 FPR(...) is valid for path and synchronized axes.
If the rotary axis/spindle specified in the FPR command is operating on position control, then
the setpoint linkage is active. Otherwise the actual-value linkage is effective.
Feedrate FPRAON(…,…), FPRAOF(…,…)
The FPRAON command makes it possible to derive the revolutional feedrate for specific
positioning axes and spindles from the current feedrate of another rotary axis or spindle.
The first command identifies the axis/spindle that must be traversed at a revolutional
feedrate. The second command identifies the rotary axis/spindle that is to supply the
feedrate. The command need not be specified a second time. If it is not, the feedrate is
derived from the master spindle.
The revolutional feedrate can be deactivated for one or several axes/spindles simultaneously
with the FPRAOF command. The feedrate is calculated in the same way as for FPR(...).
Examples: The revolutional feedrate for master spindle 1 must be derived from spindle 2.
N30 FPRAON(S1,S2)
N40 SPOS=150
N50 FPRAOF(S1)
The revolutional feedrate for positioning axis X must be derived from the master spindle. The
positioning axis is traversing at 500 mm/revolution of the master spindle.
N30 FPRAON(X)
N40 POS[X]=50 FA[X]=500
N50 FPRAOF(S1)
Feedrate Control and Spindle Motion
7.6 Percentage feedrate override (OVR, OVRA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 293
7.6 Percentage feedrate override (OVR, OVRA)
Function
You can use the programmable feedrate override to change the velocity of path axes,
positioning axes, and spindles via a command in the NC program.
Programming
OVR=…
or
OVRA[axis]=…
or
OVRA[SPI(spindle)]=… or OVRA[S…]=…
Parameter
OVR Feedrate change in percent for path feedrate F
OVRA Feedrate change in percent for positioning feedrate FA or for spindle
speed S
SPI Converts the spindle number into an axis identifier; the transfer
parameter must contain a valid spindle number. The spindle
identifiers SPI(...) and S... are identical in terms of function.
Axis Positioning axes or geometry axes
Range of values …200%, integers; with path and rapid traverse override, the
maximum velocities set in the machine data are not overshot.
Example of programmed feed rate change
The programmed feedrate change refers to or is combined with the feedrate override set on
the machine control panel.
Example:
Set feedrate override 80%
Programmed feedrate override OVR=50
The programmed path feedrate F1000 is changed to F400 (1000 * 0.8 * 0.5).
N10 OVR=25 OVRA[A1]=70 ;Path feedrate 25%, Positioning feedrate for A1 70%.
N20 OVRA[SPI(1)]=35 ;Speed for spindle 1 35%.
or
N20 OVRA[S1]=35
Feedrate Control and Spindle Motion
7.7 Feedrate with handwheel override (FD, FDA)
Fundamentals
294 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.7 Feedrate with handwheel override (FD, FDA)
Function
With these functions, you can use the handwheel to traverse path and positioning axes
(position parameter) or change the axis velocities (speed override) during program
execution. The handwheel override is frequently used for grinding operations.
Notice
Only speed override can be used for path axes. The path feedrate F and the handwheel
override FD may not be programmed in the same NC block.
Programming
FD=…
Or
FDA[axis]=0 or FDA[axis]=…
Or
FDA[axis]=...
Parameters
FD=… Handwheel travel for path axes with feedrate override
FDA[axis]=0 Handwheel travel for positioning axes according to position parameter
FDA[axis]=... Handwheel travel for positioning axes with feedrate override
Axis Positioning axes or geometry axes
The handwheel override function is non-modal. The function is deactivated in the next NC
block and the NC program continues to be executed.
Feedrate Control and Spindle Motion
7.7 Feedrate with handwheel override (FD, FDA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 295
Example
Path specification: The grinding wheel oscillating in the Z direction is moved to the workpiece
in the X direction using the handwheel.
=
;
The operator can then adjust the position of the tool until the spark generation is constant.
When "Delete distance-to-go" is activated, the program goes to the next NC block and
machining continues in NC mode.
Requirements
A handwheel must be assigned to the axes to be traversed for the handwheel override
function. For the precise approach see HMI Operator's Guide. The number of handwheel
pulses per graduated position is defined in machine data.
Traverse path axes with handwheel override, FD
The following preconditions apply to handwheel overrides for path axes:
in the NC block with the programmed handwheel override
• a G1, G2 or G3 motion command must be active,
• exact stop G60 must be switched on, and
• the path feedrate must be specified with G94 mm/min or inch/min.
Feed override
The feed override acts only on the programmed feed, not on the travel movement generated
by the handwheel (except if feed override = 0).
Example:
N10 G1 X… Y… F500…
N50 X… Y… FD=700
Feedrate Control and Spindle Motion
7.7 Feedrate with handwheel override (FD, FDA)
Fundamentals
296 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
The feedrate is accelerated to 700 mm/min in block N50. The path velocity can be increased
or reduced according to the direction of rotation on the handwheel.
Note
It is not possible to traverse in the opposite direction.
Handwheel travel with path default for positioning axes, FDA[axis]=0
In NC blocks with programmed FDA[axis]=0, the feed is set to zero in order that the program
does not generate any travel movement. The programmed travel movement to the target
position is now controlled exclusively by the operator rotating the handwheel.
Example: N20 POS[V]=90 FDA[V]=0
The automatic travel movement is stopped in block N20. The operator can now move the
axis manually using the handwheel.
Direction of movement, travel velocity
The axes accurately follow the path set by the handwheel in the direction of the leading sign.
Depending on the direction of rotation, you can travel forwards or backwards – the faster you
turn the handwheel, the higher the travel velocity.
Traversing range
The traversing range is limited by the starting position and the end point programmed with
the positioning command.
Feedrate Control and Spindle Motion
7.7 Feedrate with handwheel override (FD, FDA)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 297
Handwheel travel with velocity overlay, FDA[axis]=...
In NC blocks with programmed FDA[...], the feedrate from the last programmed FA value is
accelerated or decelerated to the value programmed under FDA. Starting from the current
feedrate FDA, you can turn the handwheel to accelerate the programmed movement to the
target position or delay it to zero. The values defined in the machine data are used for the
maximum velocity.
Example:
N10 POS[U]=10 FDA[U]=100
POSA[V]=20 FDA[V]=150
Note
With velocity override of path axes, you always control the path velocity with the handwheel
of the 1st geometry axis.
Traversing range
The traversing range is limited by the starting position and the programmed end point.
Manual override in automatic mode
The manual override function in automatic mode for POS/A axes has two different effects
that are analogous to Jog functions.
1. Path override: FDA [ax] = 0
The axis does not move. Handwheel impulses received for each IPO cycle are traversed
directionally and path-specifically. When the target position is achieved, the axis
decelerates.
2. Velocity override FDA [ax] > 0
The axis approaches the target position at the programmed axis speed. This enables
target position to be reached even without handwheel impulses. Pulses received for each
IPO cycle are converted to an accumulative change in the existing velocity. Impulses in
the traversing direction increase the velocity. Velocity is limited to the maximum axis
velocity MAX_AX_VELO. Impulses away from the traversing direction decrease the
velocity. The minimum velocity is 0.
Feedrate Control and Spindle Motion
7.8 Percentage acceleration override (ACC option)
Fundamentals
298 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.8 Percentage acceleration override (ACC option)
Function
In critical program sections, it may be necessary to limit the acceleration to below the
maximum values, e.g., to prevent mechanical vibrations from occurring.
You can use the programmable acceleration override to change the acceleration for each
path axis or spindle via a command in the NC program. The limit is effective for all types of
interpolation. The values defined in the machine data determine the 100% acceleration.
Programming
ACC[axis]=...
Or deactivate
ACC[axis]=100, program start, reset
Or
ACC[SPI(spindle)]=… or ACC(S…)
Parameters
ACC Change in acceleration in percent for the specified path axis or
change in speed for the specified spindle.
Range of values: 1..200%, integers
SPI Converts the spindle number into an axis identifier; the transfer
parameter must contain a valid spindle number. The spindle identifiers
SPI(...) and S... are identical in terms of function.
Axis Channel axis name of the path axis, e.g., with X
Note
Please note that the maximum permissible values of the machine manufacturer can be
exceeded with a higher acceleration rate.
Feedrate Control and Spindle Motion
7.8 Percentage acceleration override (ACC option)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 299
Example
N50 ACC[X]=80
Meaning: Traverse the axis slide in the X direction with only 80% acceleration.
N60 ACC[SPI(1)]=50
Or
ACC[S1]=50
Meaning: Accelerate or decelerate spindle 1 with only 50% of the maximum acceleration.
The spindle identifiers SPI(...) and S... are identical in terms of function.
Acceleration override programmed with ACC
The acceleration override programmed with ACC[] is always taken into consideration on
output in system variable $AA_ACC. Readout in the parts program and in synchronized
actions takes place at different times in the NC processing run.
In the part program
The value described in the parts program is only considered in the system variables
$AA_ACC as described in the parts program, if ACC was not changed in the meantime by a
synchronized action.
In synchronized actions
The following thus applies: the value written to the synchronized action is only considered in
the system variables $AA_ACC as written to the synchronized action if ACC was not
changed in the meantime by a parts program.
The defined acceleration can also be changed via synchronized actions. See /FBSY/,
Synchronized Actions.
Example: N100 EVERY $A_IN[1] DO POS[X]=50 FA[X]=2000 ACC[X]=140
The current acceleration value can be called with the system variables $AA_ACC[<axis>].
Machine data can be used to determine whether the ACC value last set should apply on
RESET/parts program end or whether it should be set to 100%.
Feedrate Control and Spindle Motion
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN)
Fundamentals
300 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN)
Function
The programmed feedrate initially refers to the cutter center path when the G41/G42
override is activated for the cutter radius (cf. chapter "Frames").
When you mill a circle – the same applies to polynomial and spline interpolation – the extent
of the change in feedrate at the cutter edge is such that it can have a considerable effect on
the quality of the machined part.
Example: you are milling a small external radius with a large tool. The path that the outside
of the cutter needs to cover is much longer than the path along the contour.
7RROSDWK
&RQWRXU
You therefore work with a very small feedrate on the contour. In order to avoid effects like
this, you should regulate the feedrate for curved contours accordingly.
Programming
CFTCP Constant feedrate on cutter center-point path, deactivate feedrate override
Or
CFC Constant feedrate only on contour
Or
CFIN Constant feedrate only on inside radii, no increment at outer radii
Feedrate Control and Spindle Motion
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 301
Parameters
CFTCP Constant feedrate on cutter center-point path.
The control keeps the feedrate constant, feed overrides are
deactivated.
CFC Constant feed at contour (tool edge).
This function is set as the default.
CFIN Constant feed at tool edge for concave contours only, otherwise on
the cutter center path. The feedrate velocity is reduced at inside radii.
Example of milling
In this example, the contour is first machined with a CFC-compensated feed. During
finishing, the cutting base is additionally machined with CFIN. This prevents the cutting base
from being damaged at outside radii by too high a feedrate.
;
<
N10 G17 G54 G64 T1 M6
N20 S3000 M3 CFC F500 G41
N30 G0 X-10
N40 Y0 Z-10 ;Infeed to first cutting depth
N50 CONTOUR1 ;Subroutine call
N40 CFIN Z-25 ;Infeed to second cutting depth
N50 CONTOUR1 ;Subroutine call
N60 Y120
N70 X200 M30
Feedrate Control and Spindle Motion
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5)
Fundamentals
302 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Constant feedrate on contour with CFC
UDWH
UDWH
UHGXFHG
LQFUHDVHG
The feedrate is reduced for inside radii and increased for outside radii. This ensures a
constant speed at the tool edge and thus at the contour.
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5)
Function
The functions described are used to
• switch the spindle on
• specify the required direction of spindle rotation, and
• define the counterspindle or an actuated tool as the master spindle, e.g., on turning
machines.
The following programming commands are valid for the master spindle: G95, G96/G961,
G97/G971, G33, G331 (see also Chapter "Main spindle, master spindle").
Machine manufacturer
Definition as master spindle is also possible via machine data (default).
Feedrate Control and Spindle Motion
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 303
Programming
M3 or M1=3
or
M4 or M1=4
or
M5 or M1=5
S…
Or
Sn=…
Or
SETMS(n) or SETMS
Parameters
M1=3 M1=4 M1=5 Spindle rotation clockwise/counterclockwise, spindle stop for spindle
1. Other spindles are defined according to M2=… M3=…
M3 Direction of spindle rotation clockwise for master spindle
M4 Direction of spindle rotation counterclockwise for master spindle
M5 Spindle stop for master spindle
S… Spindle speed in rpm for the master spindle
Sn…= Spindle speed in rpm for spindle n
SETMS(n) Set spindle specified in n as master spindle
SETMS Reset to the master spindle defined in machine data
Spindle speed S
The speed specified with S… or S0=… applies to the master spindle. You specify the
corresponding number for additional spindles: =…, S2=…
Note
Three S values can be programmed per NC block.
Example of master spindle with work spindle
S1 is the master spindle, S2 is the second spindle. The part is to be machined from two
sides. To do this, it is necessary to divide the operations into steps. After the cut-off point,
the synchronizing device (S2) takes over machining of the workpiece after the cut off. To do
this, this spindle S2 is defined as the master spindle to which G95 then applies.
Feedrate Control and Spindle Motion
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5)
Fundamentals
304 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
6
6
6
N10 S300 M3 ;Speed and direction of rotation
;for drive spindle = preset master spindle
N20…N90 ;Machining of right side of workpiece
N100 SETMS(2) ;S2 is now master spindle
N110 S400 G95 F… ;Speed for new master spindle
N120…N150 ;Machining of left side of workpiece
N160 SETMS ;Switch back to master spindle S1
Preset M commands, M3, M4, M5
In a block with axis commands, the above mentioned functions are activated before the axis
movements commence (basic settings on the control).
Example:
N10 G1 F500 X70 Y20 S270 M3 ;The spindle powers up to 270 rpm, then
;the movements are executed in X and Y.
N100 G0 Z150 M5 ;Spindle stop before retraction motion in Z
Note
Machine data can be used to set when axis movements should be executed; either once the
spindle has powered up to the setpoint speed, or immediately after the programmed
switching operations have been traversed.
Working with multiple spindles
5 spindles – master spindle plus 4 additional spindles – can be available in one channel at
the same time.
Feedrate Control and Spindle Motion
7.10 Spindle speed (S), direction of spindle rotation (M3, M4, M5)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 305
One of the spindles is defined in machine data as the master spindle. Special functions apply
to this spindle, such as thread cutting, tapping, revolutional feed, dwell time. The numbers
must be specified with the speed and the direction of rotation/spindle stop for the other
spindles, e.g., for a second spindle and actuated tool.
Example:
N10 S300 M3 S2=780 M2=4 ;Master spindle 300 rpm, U/min, clockwise,
;2nd spindle 780 rpm, counterclockwise
Deactivate SETMS
By issuing SETMS without spindle parameter you can switchback to the master spindle
defined in the machine data.
Programmable switchover of master spindle, SETMS(n)
You can define any spindle as the master spindle with a command in the NC program.
Example:
N10 SETMS (2) ;SETMS must be located in a separate block,
;spindle 2 is now the master spindle
Note
The speed specified with S and M3, M4, M5 now apply.
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
306 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS,
SCC[AX])
Function
When G96/G961 is active, the spindle speed – depending on the respective workpiece
diameter – is modified in order that the cutting rate S in m/min or ft/min remains constant at
the tool edge.
6SLQGOHVSHHG
5HGXFH
&RQVWDQW
FXWWLQJUDWH
6SLQGOHVSHHG
LQFUHDVHG
This increases the uniformity and thus the surface quality of turned parts, and also protects
the tool.
The constant cutting rate, activated with G96/G961/G962 can be cancelled again with
G97/G971/G972 with the active feed type (G94 linear feed or G95 revolutional feedrate).
Using G973 a constant cutting rate (G96) is de-selected without speed limiting being
activated as is the case for G97.
If any of the G96/G961/G962 functions are active, SCC[axis] can be used to assign any
geometry axis as a reference axis. If the reference axis changes, which will in turn affect the
TCP (tool-center-point) reference position for the constant cutting rate, the resulting spindle
speed will be attained via the set braking or acceleration ramp.
The command LIMS specifies a maximum spindle speed limitation for the master spindle.
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 307
Programming
Activate
G96 or G96 S…
Deactivate
G97
or
G973 without activating spindle speed limiting
Activate/deactivate
G961 or G971 with feed type as for G94
or
G962 or G972 with feed type, either as for G94 or as for G95
Speed limitation of the master spindle in a block
LIMS=value or LIMS[1]=value up to LIMS[4]=value in one block
LIMS can be expanded for machines with selectable master spindles by adding four
limitations in the parts program for each of these master spindles. The speed limitation
programmed with G26 or specified via setting data cannot be exceeded with LIMS and
activates an alarm if not observed.
Assignment of the specified axis as a reference axis
SCC[AX] can be programmed together with G96/G961/G962 or in isolation.
Note
The reference axis for G96/G961/G962 must be a geometry axis assigned to the channel at
the time when SCC[AX] is programmed. SCC[AX] can also be programmed when any of the
G96/G961/G962 functions are active.
Parameters
G96 Activate constant cutting rate with feedrate type as with G95
(revolutional feedrate in relation to a master spindle).
G961= Activate constant cutting rate with feedrate type as with G94 (linear
feedrate in relation to a linear/rotary axis).
G962= Activate constant cutting rate with feedrate type as with G94 or G95.
S... Cutting rate in m/min, always applies to master spindle Range of
values.
Range of values The range of values for the cutting rate S can be between 0.1 m/min
... 9999 9999.9 m/min. The precision can be set in the machine data.
Note:At G70/G700: cutting rate is in feet/min.
G97 Deactivate constant cutting rate with feedrate type as with G95
(revolutional feedrate in relation to a master spindle).
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
308 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G971= Deactivate constant cutting rate with feedrate type as with G94 (linear
feedrate in relation to a linear/rotary axis).
G972= Deactivate constant cutting rate with feedrate type as with G94 or
G95.
G973= Deactivate constant cutting rate without activating speed limiting.
LIMS= The speed limitation is active if G96, G961 and G97 are active for the
master spindle (LIMS does not work with G971). LIMS applies to the
master spindle.
LIMS[1 to 4]=value Limitations of differing values can be programmed for up to four
spindles within one block. Unless expansion is specified, LIMS will
only remain effective for one master spindle.
SCC[axis] Selective assignment of specified axis to G96/G961/G962
Value Spindle speed limitation in RPM
Axis A reference axis is permitted to take the form of a geometry, channel
or machine axis, otherwise alarm 14850 will be signaled.
Example of speed limitation for the master spindle
N10 SETMS (3)
N20 G96 S100 LIMS=2500 ;Speed limitation at 2500 rpm
or
N60 G96 G90 X0 Z10 F8 S100
LIMS=444
;Max. speed of the master spindle is 444 rpm
Example of speed limitation for up to four spindles
Speed limitations are defined for spindle 1 (supposed master spindle) and spindles 2, 3 and
4:
N10 LIMS=300 LIMS[2]=450 LIMS[3]=800 LIMS[4]=1500
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 309
Example Y-axis assignment for face cutting with X axis
N10 G18 LIMS=3000 T1 D1 ;Speed limitation at 3000 rpm
N20 G0 X100 Z200
N30 Z100
N40 G96 S20 M3 ;Constant cutting rate 20 m/min, is
;dependent on X axis.
N50 G0 X80
N60 G01 F1.2 X34 ;Face cutting in X at 1.2 mm/rev
N70 G0 G94 X100
N80 Z80
N100 T2 D1
N110 G96 S40 SCC[Y]
...
;Y axis is assigned to G96 and G96 is activated, can be achieved
in a
;single block. Constant cutting rate
;S40 m/min is dependent on Y axis.
N140 Y30
N150 G01 F1.2 Y=27 ;Grooving in Y, feedrate F 1.2 mm/rev
N160 G97 ;Constant cutting rate OFF
N170 G0 Y100
Adjust feedrate F
When G96 is active, G95 feedrate is automatically activated in mm/rev.
Caution
If G95 was not already active, you must specify a new feedrate F when you call G96 (e.g.,
convert F value from mm/min to mm/rev).
Activate constant cutting rate, G96/G961
When G96/G961is first selected in the parts program, a constant cutting rate must be
entered in m/min or ft/min; when the command is reselected, a new cutting rate may be
entered.
Upper speed limit LIMS
If you machine a workpiece that varies greatly in diameter, it is advisable to specify a speed
limit for the spindle. This prevents excessively high speeds with small diameters. LIMS
functions as a speed limiter with G96/G961 and G97.
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
310 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
/,06
Note
On loading the block into the main run, all programmed values are transferred into the
setting data.
Deactivate constant cutting rate, G97/G971/G973
After G97/G971, the control interprets an S word as a spindle speed in rpm again. If you do
not specify a new spindle speed, the last speed set by G96/G961 is retained.
• The G96/G961 function can also be deactivated with G94 or G95. In this case, the last
programmed speed S is used for further machining operations.
• G97 can be programmed without G96 beforehand. The function then has the same effect
as G95; LIMS can also be programmed.
• With G961 and G971, the constant cutting rate can be activated/deactivated.
• Using G973, the constant cutting rate can be deactivated without activating a spindle
speed limitation.
Note
The transverse axis must be defined in machine data.
Feedrate Control and Spindle Motion
7.11 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC[AX])
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 311
Rapid traverse G0
With rapid traverse G0, there is no change in speed. Exception: if the contour is approached
in rapid traverse and the next NC block contains a G1, G2, G3 … path command, the speed
is adjusted in the G0 approach block for the next path command.
Axis replacement of the assigned channel axis
The reference axis property for G96/G961/G962 is always assigned to a geometry axis. In
the event of an axis replacement involving the assigned channel axis, the reference axis
property for G96/G961/G962 is retained in the old channel.
A geo-axis replacement will not affect how the geometry axis is assigned to the constant
cutting rate. If the TCP reference position for G96/G961/G962 is affected by a geo-axis
replacement, the spindle will attain the new speed via a ramp.
If no new channel axis is assigned as a result of a geo-axis replacement, e.g., GEOAX(0, X),
the spindle speed will be frozen in accordance with G97.
Examples of GEOAX geo-axis replacement with reference-axis assignments using SCC
Example 1
N05 G95 F0.1
N10 GEOAX(1, X1) ;Channel axis X1 becomes first geo axis
N20 SCC[X] ;First geo axis (X) becomes reference axis for G96/G961/G962
N30 GEOAX(1, X2) ;Channel axis X2 becomes first geo axis
N40 G96 M3 S20 ;Reference axis for G96 is channel axis X2
Example 2
N05 G95 F0.1
N10 GEOAX(1, X1) ;Channel axis X1 becomes first geo axis
N20 SCC[X1] ;X1 and implicitly first geo axis (X) becomes reference axis
;for G96/G961/G962
N30 GEOAX(1, X2) ;Channel axis X2 becomes first geo axis
N40 G96 M3 S20 ;Reference axis for G96 is X2 or X, no alarm
Example 3
N05 G95 F0.1
N10 GEOAX(1, X2) ;Channel axis X2 becomes first geo axis
N20 SCC[X1] ;X1 is not a geo axis, compensation-block alarm 14850
Example 4
N05 G0 Z50
N10 X35 Y30
N15 SCC[X] ;Reference axis for G96/G961/G962 is X
N20 G96 M3 S20 ;Constant cutting rate at 10 mm/min ON
N25 G1 F1.5 X20 ;Face cutting in X at 1.5 mm/rev
N30 G0 Z51
N35 SCC[Y] ;Reference axis for G96 is Y, reduction in spindle speed (Y30)
N40 G1 F1.2 Y25 ;Face cutting in Y at 1.2 mm/rev
References
/FB1/Function Manual Basic Functions; Transverse Axes (P1) and Feedrates (V1).
Feedrate Control and Spindle Motion
7.12 Constant grinding wheel peripheral speed (GWPSON, GWPSOF)
Fundamentals
312 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7.12 Constant grinding wheel peripheral speed (GWPSON, GWPSOF)
Function
With the function "Constant grinding wheel peripheral speed" (=GWPS), you can set the
grinding wheel speed such that, taking account of the current radius, the grinding wheel
peripheral speed remains constant.
Programming
GWPSON(T No.)
Or
GWPSOF(T No.)
S...
S1…
Parameters
GWPSON(T No.) Select constant grinding wheel peripheral speed (GWPS)
It is only necessary to specify the T number if the tool with this T number is
not active.
GWPSOF(T No.) Deselect GWPS; it is only necessary to specify the T number if the tool
with this T number is not active.
S…
S1…
Program GWPS
S…: PWGS for master spindle; S1…: PWGS for spindle 1
GWPS Peripheral speed value in m/s or ft/s
The GWPS can only be selected for grinding tools (types 400-499).
Example of grinding tools with constant grinding wheel peripheral speed
A constant grinding wheel peripheral speed is to be used for grinding tools T1 and T5.
T1 is the active tool.
N20 T1 D1 ;Select T1 and D1
N25 S1=1000 M1=3 ;1000 rpm for spindle 1
N30 S2=1500 M2=3 ;1500 rpm for spindle 2
…
N40 GWPSON ;Selection of GWPS for active tool
N45 S1 = 60 ;Set GWPS for active tool to 60 m/s
…
N50 GWPSON(5) ;GWPS selection for tool 5 (2nd spindle)
N55 S2 = 40 ;Set GWPS for spindle 2 to 40 m/s
…
N60 GWPSOF ;Deactivate GWPS for active tool
N65 GWPSOF(5) ;Switch off GWPS for tool 5 (spindle 2)
Feedrate Control and Spindle Motion
7.13 Programmable spindle speed limitation (G25, G26)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 313
Tool-specific parameters
In order to activate the function "Constant peripheral speed", the tool-specific grinding data
$TC_TPG1, $TC_TPG8 and $TC_TPG9 must be set accordingly. When the GWPS function
is active, even online offset values (= wear parameters; cf. "Grinding-specific tool monitoring
in the parts program TMON, TMOF" or PUTFTOC, PUTFTOCF) must be taken into account
when changing speed.
Select GWPS: GWPSON, program GWPS
After selecting the GWPS with GWPSON, each subsequent S value for this spindle is
interpreted as a grinding wheel peripheral speed.
Selection of grinding wheel peripheral speed with GWPSON does not cause the automatic
activation of tool length compensation or tool monitoring.
The GWPS can be active for several spindles on a channel with different tool numbers.
If GWPS is to be selected for a new tool on a spindle where GWPS is already active, the
active GWPS must first be deselected with GWPSOF.
Deactivate GWPS GWPSOF
When GWPS is deselected with GWPSOF, the last speed to be calculated remains valid as
the setpoint.
GWPS programming is reset at the end of the parts program or on RESET.
Query active GWPS $P_GWPS[spindle no.]
This system variable can be used to query from the parts program whether the GWPS is
active for a specific spindle.
TRUE: GWPS active.
FALSE: GWPS is inactive.
7.13 Programmable spindle speed limitation (G25, G26)
Function
You can use a command in the NC program to change the minimum and maximum spindle
speeds defined in the machine data and setting data. It is possible to program spindle speed
limitations for all spindles on the channel.
Programming
G25 S… S1=… S2=…
Or
G26 S… S1=… S2=…
A maximum of three spindle speed limitations can be programmed for each block.
Feedrate Control and Spindle Motion
7.14 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=.., SRA=..)
Fundamentals
314 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
G25 Lower spindle speed limitation
G26 Upper spindle speed limitation
S S1 S2=…=… Minimum or maximum spindle speed
Range of values Value assignment for the spindle speed can be between
rpm ... 9999 9999.9 rpm.
Caution
A spindle speed limitation programmed with G25 or G26 overwrites the speed limitations in
the setting data and thus remains stored after the end of the program.
Examples
N10 G26 S1400 S2=350 S3=600 ;Upper speed limitation for master spindle,
;spindle 2 and spindle 3
Maximum possible spindle speed limitations within a block
LIMS[1]=500 LIMS[2]=600
LIMS[3]=700 LIMS[3]=800
;Master spindle speed limitations
;Maximum for 4 spindles within a block
G25 S1=1 S2=2 S3=3
G26 S1=1000 S2=2000 S3=3000
; Lower and upper speed limit
;Maximum of 3 spindle limitations within a block
7.14 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=..,
SRA=..)
Function
The "Several feedrates in one block" function can be used independent of external analog
and/or digital inputs to activate
• Different feedrates of an NC block,
• dwell time, and
• Retraction
in synchronism with the movement.
The HW input signals are combined in one input byte.
Feedrate Control and Spindle Motion
7.14 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=.., SRA=..)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 315
Programming
F2= to F7= Multiple path motions in 1 block
ST=
SR=
Or
FMA[2,x]= to FMA[7,x]=Multiple axial motions in 1 block
STA=
SRA=
Parameters
F2=... to F7=...== In addition to the path feed, you can program up to 6 further feedrates
in the block; non-modal
ST=... Dwell time (for grinding technology: sparking-out time); non modal
SR=... Return path; non modal. The unit for the retraction path refers to the
current valid unit of measurement (mm or inch).
FMA[2,x]=... to
FMA[7,x]=...
In addition to the path feed, you can program up to 6 further feedrates
per axis in the block; non modal
STA=... Axial dwell time (for grinding technology: sparking-out time); non-
modal
SRA=... Axial return path; non-modal
FA, FMA and F value
The axial feedrate (FA or FMA value) or path feedrate (F value) corresponds to 100%
feedrate. You can use this function to realize feedrates that are smaller than or equal to the
axial feedrate or the path feedrate.
Note
If feedrates, dwell time or return path are programmed for an axis on account of an external
input, this axis must in this block must not be programmed as POSA axis (positioning axis
over multiple blocks).
Look Ahead is also active for multiple feedrates in one block. In this way, the current
feedrate is restricted by the Look Ahead value.
Feedrate Control and Spindle Motion
7.14 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=.., SRA=..)
Fundamentals
316 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of programming path motion
The path feed is programmed under the address F and remains valid until an input signal is
present. The numerical expansion indicates the bit number of the input that activates the
feedrate when changed:
F7=1000 ;7 corresponds to input bit 7
F2=20 ;2 corresponds to input bit 2
ST=1 ;Dwell time (s) input bit 1
SR=0.5 ;Return path (mm) input bit 0
Example of programming axial motion
The axial path feed is programmed under the address FA and remains valid until an input
signal is present.
FMA[7,x]= to FMA[2,x]= can be used to program up to 6 further feeds per axis in the block.
The first expression in the square brackets indicates the bit number of the input; the second
the axis for which the feedrate is to apply
FMA[3, x]=1000 ;Axial feedrate with the value 1000 for X axis, 3
;corresponds to input bit 3
Example of axial dwell time and return path
Dwell time and return path are programmed under the following additional addresses:
STA[x]=... ;Axial dwell time (s) input bit 1
SRA[x]=... ;Axial return path (mm) input bit 0
If input bit 1 is activated for the dwell time or bit 0 for the return path, the distance to go for
the path axes or the relevant single axes is deleted and the dwell time or return started.
Example of several operations in one block
N20 T1 D1 F500 G0 X100 ;Initial setting
N25 G1 X105 F=20 F7=5
F3=2.5 F2=0.5 ST=1.5 SR=
0.5
;Normal feedrate with F, roughing with F7, finishing with
;F3, smooth-finishing with F2, dwell time 1.5 s
;return path 0.5 mm
N30 ...
…
Feedrate Control and Spindle Motion
7.15 Blockwise feed (FB...)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 317
7.15 Blockwise feed (FB...)
Function
You can use the function "Non-modal feedrate" to define a separate feedrate for a single
block.
The address FB is used to define the feedrate only for the current block. After this block, the
previously active modal feedrate is active.
Programming
FB=<Wert> Feed motion only in one block
Parameter
FB=...= Instead of the modal feedrate active in the previous block, you can
program a separate feedrate for this block; in the block that follows,
the previously active modal feedrate applies.
<WERT> The programmed value of FB=<Wert> must be greater than zero.
Feed value
The address FB is used to define the feedrate only for the current block. After this block, the
previously active modal feedrate is active.
The feedrate is interpreted according to the active feedrate type:
• G94: feedrate in mm/min or degrees/min
• G95: feedrate in mm/rev or inch/rev
• G96: Constant cutting rate
References: /FB1/Function Manual Basic Functions; Feedrates (V1)
Note
If no traversing motion is programmed in the block (e.g., computation block), the FB has no
effect.
If no explicit feed for chamfering/rounding is programmed, then the value of FB also applies
for any contour element chamfering/rounding in this block.
Feedrate interpolations FLIN, FCUB, etc., are also possible without restriction.
Simultaneous programming of FB and FD (handwheel travel with feed overlay) or F (modal
path feedrate) is not possible.
Example
Feedrate Control and Spindle Motion
7.15 Blockwise feed (FB...)
Fundamentals
318 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N10 G0 X0 Y0 G17 F100
G94
;Initial setting
N20 G1 X10 ;Feedrate 100 mm/min
N30 X20 FB=80 ;Feedrate 80 mm/min
N40 X30 ;Feedrate is 100 mm/min again
N50 ...
…
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 319
Tool offsets 8
8.1 General notes
8.1.1 Tool offsets
When writing a program, it is not necessary to specify the cutter diameter, the tool point
direction of the turning tool (left/right-handed turning tools) or tool length.
You program the workpiece dimensions directly, for example, following the production
drawing.
When machining a workpiece, the tool paths are controlled according to the tool geometry
such that the programmed contour can be machined using any tool.
7RROSDWK
&RQWRXU
The control corrects the traverse path
You enter the tool data separately in the tool table on the control.
All you need to do is call the required tool with its offset data in the program.
Tool offsets
8.1 General notes
Fundamentals
320 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
&RUUHFWHG
7RROSDWK
3URJUDPPHGFRQWRXU
During program execution, the control fetches the offset data from the tool files and corrects
the tool path individually for different tools.
Enter tool offsets into the offset memory
In the offset memory enter the following:
• Geometric dimensions based on wear: length, radius.
• Tool type with the tool parameters for drill, milling tool and grinding, turning or special
tools
• Length of cutting edge
8.1.2 Tool offsets in the control's offset memory
Which tool offsets are stored in the control's offset memory?
In the offset memory enter the following:
• Geometrical dimensions: length, radius.
Tool offsets
8.1 General notes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 321
5DGLXV
/HQJWK
)
They consist of several components (geometry, wear). The control computes the
components to a certain dimension (e.g., overall length 1, total radius). The respective
overall dimension becomes active when the offset memory is activated.
The way in which these values are computed in the axes is determined by the tool type and
the current plane G17, G18, G19.
• Tool type
The type determines which geometry data are needed and how they are calculated (drill or
milling tool or turning tool).
• Cutting-edge position
Tool parameters
The following section "List of tool types" describes the individual tool parameters on the
display. The relevant tool parameters must be entered in the entry fields with "DP...".
Notice
Values that have been entered once in the offset memory are included in the processing for
each tool called.
Tool offsets
8.1 General notes
Fundamentals
322 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
/
/
)
3 7RROWLS
6 &XWWLQJHGJHFHQWHU
5 5DGLXV
3
6
5
Any tool parameters that are not required must be set to "zero".
Description
Tool length compensation
This value compensates for the differences in length between the tools used.
The tool length is the distance between the toolholder reference point and the tip of the tool.
FF
F
F
This length is measured and entered in the control together with definable wear values. From
this data, the control calculates the traversing movements in the infeed direction.
Tool offsets
8.1 General notes
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 323
Note
The compensation value of the tool length depends on the spatial orientation of the tool. See
also chapter "Tool orientation and tool length compensation" for more information.
Tool radius compensation
The contour and tool path are not identical. The cutter or tool nose radius center must travel
along a path that is equidistant from the contour. To do this, the programmed tool center
point path is displaced by an amount that depends on the radius and the direction of
machining and such that the tool nose travels exactly along the desired contour.
The control fetches the required radii during program execution and calculates the tool path
from these values.
(TXLGLVWDQWSDWK
(TXLGLVWDQWSDWK
Notice
The tool radius compensation acts according to default setting CUT2D or CUT2DF. You will
find more information later in this chapter.
Tool offsets
8.2 List of tool types
Fundamentals
324 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.2 List of tool types
Codings of tool types
The individually coded tool types are divided up into the following groups depending on the
technology used:
1. Group with type 1xy milling tools
2. Group with type 2xy drills
3. Group with type 3xy reserved
4. Group with type 4xy grinding tools
5. Group with type 5xy turning tools
6. Group with type 6xy reserved
7. Group with type 7xy special tools such as slotting saw
Codings of tool types for milling tools
Group with type 1xy (milling tool):
100 Milling tool according to CLDATA
110 Ball end mill (cylindrical die sinker)
111 Ball end mill (tapered die sinker)
120 End mill (without corner rounding)
121 End mill (with corner rounding)
130 Angle head cutter (without corner rounding)
131 Angle head cutter (with corner rounding)
140 Face milling
145 Thread cutter
150 Side mill
151 Saw
155 Bevel cutter (without corner rounding)
156 Bevel cutter (with corner rounding)
157 Conical die milling cutter
160 Drill and thread milling cutter
Tool offsets
8.2 List of tool types
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 325
))
(QWULHVLQ
7RROSDUDPHWHUV
'3
'3
'3
*HRPHWU\OHQJWK
*HRPHWU\UDGLXV
$GDSWHUOHQJWK
:HDUYDOXHV
DV
UHTXLUHG
6HWUHPDLQLQJ
YDOXHVWR
'3 [\
*
*
*
/HQJWKLQ=
5DGLXVLQ;<
/HQJWKLQ<
5DGLXVLQ=;
/HQJWKPP;
5DGLXVLQ<=
)¥7RROKROGHU
5HIHUHQFHSRLQW
)5HIHUHQFHSRLQWDGDSWHUZLWKWRROLQVHUWHG
WRROKROGHUUHIHUHQFHSRLQW
(IIHFW
/HQJWK
/HQJWK7RWDO
/HQJWK$GDSWHU
$IL[HGDVVLJQPHQWLVSRVVLEOHIRU***
HJOHQJWK ;OHQJWK =OHQJWK <VHH)%:7RROFRPSHQV
;
<
=
=
;
<
<
=
;
:HDUYDOXHVDFFWR
UHTXLUHPHQWV
6HWUHPDLQLQJ
YDOXHVWR
(IIHFW
*
*
*
/HQJWKLQ<
/HQJWKLQ;
/HQJWKLQ=
5DGLXV75&LQ=;
/HQJWKPP;
/HQJWKLQ=
/HQJWKLQ<
5DGLXV75&LQ<=
/HQJWKPP=
/HQJWKFP<
/HQJWKLQ;
5DGLXV75&LQ;<
(QWULHVLQ
7RROSDUDPHWHUV
'3
'3
'3
'3
'3
'3
[\
*HRPHWU\OHQJWK
*HRPHWU\UDGLXV
%DVHOHQJWK
%DVHOHQJWK
%DVHOHQJWK
)
)
7RROEDVH
GLPHQVLRQ
/HQJWK
7RROEDVH
GLPHQVLRQ
/HQJWK
7RROEDVH
GLPHQVLRQ
/HQJWK
)¥7RROKROGHUUHIHUHQFHSRLQW
)7RROKROGHUUHIHUHQFHSRLQW
5DGLXV
$IL[HGDVVLJQPHQWLVSRVVLEOHIRU***
HJOHQJWK ;OHQJWK <OHQJWK =VHH)%:7RROFRPSHQVDWLRQ
Tool offsets
8.2 List of tool types
Fundamentals
326 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Coding of tool types for drills
Group type 2xy (drills):
200 Twist drill
205 Drill
210 Boring bar
220 Center drill
230 Countersink
231 Counterbore
240 Regular thread tap
241 Fine thread tap
242 Whitworth-thread tap
250 Reamer
)
(QWULHVLQ
7RROSDUDPHWHUV
'3
'3
[\
/HQJWK
:HDUYDOXHV
DV
UHTXLUHG
6HWUHPDLQLQJ
YDOXHVWR
* /HQJWKPP=
/HQJWKLQ<
/HQJWKPP;
*
*
)7RROKROGHU
5HIHUHQFHSRLQW
/HQJWK
(IIHFW
Tool offsets
8.2 List of tool types
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 327
Coding of tool types for grinding tools
Group type 4xy (grinding tools):
400 Surface grinding wheel
401 Surface grinding wheel with monitoring
402 Surface grinding wheel without monitoring without toolbase dimension (TOOLMAN)
403 Surface grinding wheel with monitoring/without tool base dimension
for grinding wheel surface speed (GWPS)
410 Facing wheel
411 Facing wheel (TOOLMAN) with monitoring
412 Facing wheel (TOOLMAN) without monitoring
413 Facing wheel with monitoring/without tool base dimension for
grinding wheel surface speed (GWPS)
490 Dresser
)
)
(QWULHVLQ
7RROSDUDPHWHUV
'3
'3
'3
'3
/HQJWK
/HQJWK
5DGLXV
73*
73*
73*
73*
73*
73*
73*
73*
73*
6SLQGOHQXPEHU
&KDLQLQJUXOH
0LQLPXPZKHHOUDGLXV
0LQLPXPZKHHOZLGWK
&XUUHQWZKHHOZLGWK
0D[LPXPVSHHG
$QJOHRIWKHLQFOLQHGZKHHO
3DUDPHWHUQRIRUUDGLXVFDOFXODWLRQ
:HDUYDOXHV
DV
UHTXLUHG
6HWUHPDLQLQJ
YDOXHVWR
(IIHFW
*
*
*
/HQJWKLQ<
/HQJWKLQ;
5DGLXVLQ;<
/HQJWKLQ;
/HQJWKLQ=
5DGLXVLQ=;
/HQJWKLQ=
/HQJWKLQ<
5DGLXVLQ<=
)7RROKROGHUUHIHUHQFHSRLQW
5DGLXV
*HRPHWU\
/HQJWK
%DVHOHQJWK
%DVH
/HQJWK
*HRPHWU\
/HQJWK
wÁ
'3
3RVLWLRQ
7RROQRVHSRVLWLRQ
0D[SHULSKHUDOVSHHG
Tool offsets
8.2 List of tool types
Fundamentals
328 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Coding of tool types for turning tools
Group type 5xy (turning tools):
500 Roughing tool
510 Finishing tool
520 Plunge cutter
530 Parting tool
540 Threading tool
550 Mushroom tool/form tool (TOOLMAN)
560 Rotary drill (ECOCUT)
580 Probe with cutting edge position parameter
=
;
)56
3
7XUQLQJWRRO
HJ*=;SODQH
)7RROKROGHUUHIHUHQFHSRLQW
/HQJWK=
7RROWLS3
WRROHGJH 'Q
/HQJWK;
6SRVLWLRQRIWRROQRVHFHQWHU
5UDGLXVRIWRROQRVH
WRROUDGLXV
Tool offsets
8.2 List of tool types
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 329
=
;
3
=
;
3 6
(QWULHVLQ
7RROSDUDPHWHUV
'3
'3
'3
'3
'3
[\
/HQJWK
/HQJWK
5DGLXV
(IIHFW
*
*
*
/HQJWKLQ<
/HQJWKLQ;
/HQJWKPP;
/HQJWKLQ=
/HQJWKPP=
/HQJWKFP<
:HDUYDOXHV
DV
UHTXLUHG
6HWUHPDLQLQJ
YDOXHVWR
7KHWRROSDUDPHWHU'3VSHFLILHVWKHOHQJWKRIWKHWRROQRVH
3RVLWLRQYDOXHWRSRVVLEOH
7RROQRVHSRVLWLRQ'3
1RWH
3DUDPHWHUVOHQJWKOHQJWKUHIHUWRWKH
SRLQWZLWKWRROQRVHSRVLWLRQEXWWR6
6 3ZLWK
Chaining rule
The tool length offsets
• Geometry,
• Wear and
• Tool base dimension
can be chained for the left and right wheel correction in each case, i.e., if the length offsets
for the left tool edge are altered, the values for the right edge are automatically entered and
vice versa. For more information see
/FB2/Function Manual Extended Functions; Grinding (W4)
Coding of tool types for special tools
Group type 7xy (special tools):
700 Slotting saw
710 3D probe
711 Edge probe
730 Stop
Tool offsets
8.2 List of tool types
Fundamentals
330 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Slotting saw
Group with type:
700 Slotting saw
(QWULHVLQ
7RROSDUDPHWHUV
'3%DVHOHQJWK
'3%DVHOHQJWK
'3*HRPHWU\GLDPHWHU
'3*HRPHWU\]HURZLGWK
'3*HRPHWU\RYHUVKRRW
:HDUYDOXHV
DV
UHTXLUHG
6HWUHPDLQLQJ
YDOXHVWR
(IIHFW
6ORWZLGWKE
7RROEDVHGLPHQVLRQ
/HQJWK
([FHVVGLP
N
7RROEDVHGLPHQVLRQ
/HQJWK
'LDPHWHUG
*+DOIGLDPHWHU/LQ;3ODQHVHOHFWLRQ
([FHVVGLPLQ/<VWQGD[LV;<
6DZEODGHLQ5;<
*+DOIGLDPHWHU/LQ<3ODQHVHOHFWLRQ
([FHVVGLPLQ/;VWQGD[LV;=
6DZEODGHLQ5=;
*+DOIGLDPHWHU/LQ=3ODQHVHOHFWLRQ
([FHVVGLPLQ/=VWQGD[LV<=
6DZEODGHLQ5<=
Note
You will find a description of the tool-type parameters on the control's help screens and in:
References: /FB1/Function Manual Basic Functions; Tool Offset (W1)
Tool offsets
8.3 Tool selection/tool call T
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 331
8.3 Tool selection/tool call T
8.3.1 Tool change with T commands (turning)
Function
A direct tool change takes place when the T word is programmed.
Tool selection without tool management
Free selection of D No. (flat D No.) relative to cutting edges
Tabulated D No.: D1 ... D8
Tool selection with tool management
Free selection of D No. (flat D No.) relative to cutting edges
Fixed assignment of D No. to the cutting edges
Programming
Tx or T=x or Ty=X
Or
T0=
Parameters
Tx or T=x or Ty=x Tool selection with T No. including tool change
(active tool), tool offset is active
x x stands for T No.: 0-32000
T0= Tool deselection
Number of tools: 1200
(depending on the machine manufacturer's configuration)
Machine manufacturer
The effect of the T number call is defined in machine data. See machine manufacturer's
configuration.
Important
It is important to ensure that the machine data for "Error response for programmed tool
change" is expanded by bit 7.
• With the currently valid default setting
, a check is performed immediately to ascertain whether the NC kernel is aware of the
tool number. If not, an alarm is triggered immediately.
• A response that deviates from this (default setting for previous software versions) can be
brought into line with bit 7.
The programmed tool number will only be checked following D-selection. If the NC kernel
is unaware of the tool number, an alarm is set during D-selection. This response is
Tool offsets
8.3 Tool selection/tool call T
Fundamentals
332 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
desirable if, for example, tool programming is also intended to achieve positioning and
the tool data is not necessarily available (circular magazine).
8.3.2 Tool change with M06 (mill)
Function
Tool selection takes place when the T word is programmed.
1. Tool selection without tool management
• Free selection of D No. (flat D No.) relative to cutting edges
7 >GLJLW@
' ' ' '
• Tabulated D No.: D1 ... D8
7 ' ' ' '
7'
7'
7 ' ' '
7 ' '
' '
7 ' '
2. Tool selection with tool management
• Free selection of D No. (flat D No.) relative to cutting edges
• Fixed assignment of D No. to the cutting edges
The tool only becomes active with M06 (incl. corresponding D No.).
Tool offsets
8.3 Tool selection/tool call T
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 333
Programming
Tx or T=x or Ty=X
or
T0=
or
M06F2=... to F7=...
Parameter
Tx or T=x or Ty=x Tool selection with T no.
x x stands for T no.: 0-32000
T0= Tool deselection
M06 Tool change, then tool T... and tool offset D are active
Number of tools: 1200
(depending on the machine manufacturer's configuration)
Machine manufacturer
The effect of the T number call is defined in machine data. Please refer to the machine
manufacturer's configuration.
Explanation
The free selection of the D No., "Flat D numbers", is used when tool management is done
outside the NC. In this case, the D numbers are created with the corresponding tool
compensation blocks without assignment to tools.
T can continue to be programmed in the parts program. However, this T has no reference to
the programmed D number.
Example:
Circular magazine with 12 locations and 12 single-edge tools.
Tool offsets
8.3 Tool selection/tool call T
Fundamentals
334 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7'
7'
7'
7'
Machine manufacturer
T can or cannot be programmed in the parts program, depending on the setting in MD
18102.
Creating a new D number
Creating a new D number with the associated tool compensation blocks is performed exactly
as for the normal D number via tool parameters $TC_DP1 to $TC_DP25. The T number
need not be entered any more.
Machine manufacturer
The type of D number management is defined in the machine data. There are two settings
available for programming D numbers in the "flat D number structure":
• Flat D number structure with direct programming
• Flat D number structure with indirect programming
Tool offsets
8.4 Tool offset D
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 335
8.4 Tool offset D
Function
It is possible to assign between 1 and 8 (12) tool noses per tool with different tool offset
blocks to a specific tool. This allows you to define various tool noses for one tool, which you
can call as required in the NC program. Different offset values could be used, for example,
for the left and right tool nose of a grooving tool.
N40...
D6 Z-5
N30 G1
D1 X10
Z
X
N20 G0
N10 T2
X35 Z-20
-5
-20
10
When D is called, the tool length offset for a specific tool nose is activated. If D0 is
programmed, the offsets for the tool are ineffective.
Tool length offsets take immediate effect when the D number is programmed. If no D word is
programmed, the default setting from the machine data is valid for tool change. A tool radius
offset must also be activated by G41/G42.
Programming
D...
or
D0=
Tool offsets
8.4 Tool offset D
Fundamentals
336 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameter
Dx Tool offset number:
Without WZV 1... 8 or with WZV 1...12
x x stands for the D No.: 0-32000
D0= Tool offset deselection, no offsets active.
D0 is preset by default after control is powered up.
Note
If you do not enter a D number, you will be working without a tool offset.
Machine manufacturer
Machine manufacturer default setting (e.g., D1, which means no D programming) is
activated/selected by means of tool change (M06) D1. The tools are activated with T
programming (see machine manufacturer's specifications).
The offset is applied with the first programmed traverse of the respective length offset axis.
Caution
The modified values only become active the next time the T or D number is programmed.
The required D number must always be programmed before the tool length offset can be
selected. The tool length offset is also effective if set in the machine data.
Example of turning
Tool change with T command
N10 T1 D1 ;Tool T1 is changed and activated with ;associated D1
N11 G0 X... Z... ;The length offsets are traversed
N50 T4 D2 ;Load tool T4, D2 from T4 is active
...
N70 G0 Z... D1 ;Other cutting edge D1 is activated for tool T4
Tool offsets
8.5 Tool selection T with tool management
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 337
8.5 Tool selection T with tool management
Function
Tool selection T with tool management is illustrated in the sample magazine with 1 to 20
locations.
Initial conditions when calling the tool
Note
When calling the tool, the
1. tool offset values stored under a D number must be activated.
2. The appropriate working plane (system setting: G18) must be programmed. This ensures
that the length compensation is assigned to the correct axis.
Machine manufacturer
Tool management: See machine manufacturer's configuration.
Important
It is important to ensure that the machine data for "Error response for programmed tool
change" is expanded by bit 7.
Tool magazine
If the selected magazine location in a tool magazine is not occupied, the tool command has
the same effect as T0. Selecting the empty magazine location can be used to position the
empty location.
Sample magazine with 1 to 20 locations
A magazine has locations 1 to 20:
Location 1 occupied by drilling tool, duplo no.=1, T15, disabled
Location 2 is not occupied
Location 3 is occupied by drilling tool, duplo no.=2, T10, enabled
Location 4 is occupied by drilling tool, duplo no.=3, T1, active
Locations 5 to 20 are not occupied
Tool offsets
8.5 Tool selection T with tool management
Fundamentals
338 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming N10 T1 or T=1:
1. Magazine location 1 is scrutinized and the tool identifier is ascertained.
2. This tool is locked and therefore cannot be used.
3. A tool search for T="drill" is initiated in accordance with the search method set.
Exception: "Find the active tool; or else, select the one with the next highest duplo
number".
4. "Drill" tool with duplo number 3 (in magazine location 4) is identified as the tool that can
be used.
This completes the tool selection process and the tool change is initiated:
5. If the "Select the first available tool from the group" search method is employed, the
sequence must first be defined within the tool group being loaded.
Group T10 is loaded, as T15 is locked.
6. On completion of tool search strategy "Take the first tool with status "active" from group",
T1 is loaded.
Tool offsets
8.5 Tool selection T with tool management
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 339
8.5.1 Turning machine with circular magazine (T selection)
Function
The tools must be assigned unique names and numbers for identification purposes. Below it
will be demonstrated how to uniquely define the parameters for the tool management option
on a turning machine with circular magazine.
Machine manufacturer
Tool management: See machine manufacturer's configuration.
Programming
The following sequence usually applies:
T = location
Or
T = identifier
D... Tool offset number: 1...32000 (max., see machine manufacturer's specifications)
Parameters
T = location or identifier
T2 = identifier
Location or identifier, T triggers the tool change.
Extended address, tool for spindle 2
T0 Magazine location not occupied
D = offset 1 to n (n ≤ 32000)
If the relative D No. structure with internal reference to the
associated tools is used, replacement tool management and
monitoring function are possible.
D0 no offsets active!
Tool offsets
8.5 Tool selection T with tool management
Fundamentals
340 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.5.2 Milling machine with chain magazine (T selection)
Function
The tools must be assigned unique names and numbers for identification purposes. Below it
will be demonstrated how to uniquely define the parameters for the tool management option
on a milling machine with chain magazine.
Machine manufacturer
Tool management: Please refer to the machine manufacturer's configuration.
Programming
The following sequence usually applies:
T = identifier or
T = number
M06 triggers the tool change
D = offset Tool edge number 1 to n (n ≤ 12)
Tool selection
With integrated tool management (within the NC)
Relative D no. structure With internal reference made to the associated tools
(e.g., tool management and monitoring function)
Without integrated tool management (external to NC)
Flat D no. structure Without internal reference made to the associated tools
Selection
• With integrated tool management (inside NC)
relative D no. structure with internal reference to the associated tools
(e.g., replacement tool management and monitoring function possible)
• Without integrated tool management (outside NC)
flat D no. structure without internal reference to associated tools.
Tool offsets
8.6 Tool offset call D with tool management
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 341
Note
When calling the tool, the
1. tool offset values stored under a D number must be activated.
2. The appropriate working plane (system setting: G17) must be programmed. This
ensures that the length compensation is assigned to the correct axis.
If the selected magazine location in a tool magazine is not occupied, the tool command
has the same effect as T0. Selecting the empty magazine location can be used to
position the empty location.
Machine manufacturer
Tool management: See machine manufacturer's configuration.
Tool magazine
If the selected magazine location in a tool magazine is not occupied, the tool command has
the same effect as T0. Selecting the empty magazine location can be used to position the
empty location.
8.6 Tool offset call D with tool management
8.6.1 Turning machine with circular magazine (D call)
Programming
The following programming sequence usually applies:
T = location
Or
T = identifier T triggers the tool change
D... Tool offset number: 1...32000 (max., see machine manufacturer's specifications)
D0: no offsets active!
Direct, absolute programming
Programming is performed with the D number structure. The compensation blocks to be
used are called directly via their D number.
Assignment of the D number to a specific tool does not take place in the NC kernel.
Machine manufacturer
Direct programming is defined by machine data.
Tool offsets
8.6 Tool offset call D with tool management
Fundamentals
342 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of turning machine with circular magazine
$MC_TOOL_CHANGE_MODE=0 ;MD20270 CUTTING_EDGE_DEFAULT = 1
...
D92 ;Traverse with tool offsets from D92
...
T17 ;Select T17, traverse with tool offsets from D92
...
D16 ;Traverse with tool offsets from D16
...
D32000 ;Traverse with tool offsets from D32000
...
T29000500 ;Select T29000500, ;traverse with tool offsets from D32000
...
D1 ;Traverse with tool offsets from D1
8.6.2 Milling machine with chain magazine (D call)
Function
It is possible to assign between 1 and 12 tool noses with different tool compensation blocks
to a specific tool. When D is called, the tool length compensation for a specific tool nose is
activated. When D0 is programmed, offsets for the tool are ineffective. If no D word is
programmed, the default setting from the machine data is valid for tool change.
Tool length compensations take immediate effect when the D number is programmed.
A tool radius offset must also be activated by G41/G42.
Machine manufacturer
Tool management: Please refer to the machine manufacturer's instructions.
Programming
The following sequence usually applies:
T = identifier or
T = number
M06 triggers the tool change
D = offset Tool edge number 1 to n (n ≤ 12)
Tool selection
With integrated tool management (within the NC)
Tool offsets
8.7 Activating the active tool offset immediately
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 343
Relative D no. structure With internal reference made to the associated tools
(e.g., tool management and monitoring function)
Without integrated tool management (external to NC)
Flat D no. structure Without internal reference made to the associated tools
Selection
• With integrated tool management (inside NC)
relative D no. structure with internal reference to the associated tools
(e.g., replacement tool management and monitoring function possible)
• Without integrated tool management (outside NC)
flat D no. structure without internal reference to associated tools
Machine manufacturer
Tool management: See machine manufacturer's specifications.
8.7 Activating the active tool offset immediately
Function
MD $MM_ACTIVATE_SEL_USER_DATA can be used to define that the active tool offset
can be activated immediately if the parts program is in "stop" mode. See
/FB1/Function Manual Basic Functions; Axes, Coordinate Systems, Frames (K2)
Danger
The offset is applied the next time the parts program is started.
8.8 Tool radius compensation (G40, G41, G42)
Function
When tool radius compensation is active, the control automatically calculates the equidistant
tool paths for different tools.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
344 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
(TXLGLVWDQWSDWK
(TXLGLVWDQWSDWK
You can generate equidistant paths with OFFN, e.g., for rough-finishing.
Programming
G40
Or
G41
Or
G42
or
OFFN=
Parameters
G40 Deactivate tool radius compensation.
G41 Activate tool radius compensation; tool operates in machining
direction to the left of the contour.
G42 Activate tool radius compensation, tool operates in machining
direction to the right of the contour.
OFFN= Allowance on the programmed contour (normal contour offset).
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 345
Example 1 milling
;
<
1
1
&RPSHQVDWLRQ
RQ<
&RPSHQVDWLRQ
RQ;
N10 G0 X50 T1 D1
N20 G1 G41 Y50 F200
N30 Y100
Only tool length compensation is activated in block N10. X50 is approached without
compensation.
In block N20, the radius compensation is activated, point X50/Y50 is approached with
compensation.
Example 2 milling
The "conventional" approach:
Call tool, load tool, activate working plane and tool radius compensation.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
346 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
<
=
<
N10 G0 Z100 ;Retract to tool change point
N20 G17 T1 M6 ;Change tool
N30 G0 X0 Y0 Z1 M3 S300 D1 ;Call tool offset values, ;select length compensation
N40 Z-7 F500 ;Tool infeed
N50 G41 X20 Y20 ;Activate tool radius compensation, tool
;operates on left-hand side of contour
N60 Y40 ;Mill contour
N70 X40 Y70
N80 X80 Y50
N90 Y20
N100 X20
N110 G40 G0 Z100 M30 ;Retract tool, end of program
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 347
Example 1 turning
Z
X
Ø 20
Ø 100
20
20 1
N20 T1 D1
N30 G0 X100 Z20
N40 G42 X20 Z1
N50 G1 Z-20 F0.2
Only tool length compensation is activated in block N20. X100 Z20 is approached without
compensation in block N30.
In block N40, the radius compensation is activated, point X20/Z1 is approached with
compensation.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
348 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example 2 turning
r
5
5
5
5
5
=
;
%_N_1001_MPF ;Program name
N5 G0 G53 X280 Z380 D0 ;Start point
N10 TRANS X0 Z250 ;Zero offset
N15 LIMS=4000 ;Speed limitation (G96)
N20 G96 S250 M3 ;Select constant feed
N25 G90 T1 D1 M8 ;Select tool and offset
N30 G0 G42 X-1.5 Z1 ;Activate tool with tool radius compensation
N35 G1 X0 Z0 F0.25
N40 G3 X16 Z-4 I0 K-10 ;Rotate radius 10
N45 G1 Z-12
N50 G2 X22 Z-15 CR=3 ;Rotate radius 3
N55 G1 X24
N60 G3 X30 Z-18 I0 K-3 ;Rotate radius 3
N65 G1 Z-20
N70 X35 Z-40
N75 Z-57
N80 G2 X41 Z-60 CR=3 ;Rotate radius 3
N85 G1 X46
N90 X52 Z-63
N95 G0 G40 G97 X100 Z50 M9 ;Deselect tool radius compensation and ;approach tool
change location
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 349
N100 T2 D2 ;Call up tool and select offset
N105 G96 S210 M3 ;Select constant cutting speed
N110 G0 G42 X50 Z-60 M8 ;Activate tool with tool radius compensation
N115 G1 Z-70 F0.12 ;Rotate diameter 50
N120 G2 X50 Z-80 I6.245 K-5 ;Rotate radius 8
N125 G0 G40 X100 Z50 M9 ;Retract tool and ;deselect tool radius compensation
N130 G0 G53 X280 Z380 D0 M5 ;Move to tool change location
N135 M30 ;Program end
Description
The control requires the following information in order to calculate the tool paths:
• Tool no. T/edge no. D
• Direction of machining G41, G42
• Working plane G17 to G19
Tool no. T/edge no. D
Where appropriate, a tool offset number D is also required. The distance between the tool
path and the workpiece contour is calculated from the cutter and tool edge radii and the tool
point direction parameters.
G42
G42
G41
G41
G41
With flat D number structure it is only necessary to program the D number.
Direction of machining G41, G42
From this information, the control detects the direction, in which the tool path is to be
displaced.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
350 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
A negative offset value is the same as a change of offset side (G41, G42).
You can generate equidistant paths with OFFN, e.g., for rough-finishing.
Working plane G17 toG19
From this information, the control detects the plane and therefore the axis directions for
compensation.
= ;
<
/HQJWK
/HQJWK
5DGLXV
5DGLXV
5DGLXV
Example of milling cutters
N10 G17 G41 …
The tool radius compensation is performed in the X/Y plane, the tool length compensation is
performed in the Z direction.
Note
On 2-axis machines, the tool radius compensation is only possible in "real" planes, in
general with G18 (see tool length compensation table).
Tool length compensation
The wear parameter assigned to the diameter axis on tool selection can be defined as the
diameter value (MD). This assignment is not automatically altered when the plane is
subsequently changed.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 351
To do this, the tool must be selected again after the plane has been changed.
Turning:
/HQJWK
/HQJWK
/HQJWK
5DGLXV
5DGLXV
/HQJWK ;
<
=
Using NORM and KONT you can determine the tool path for activation/deactivation of
compensation mode (see chapter "Contour approach and retraction", NORM, KONT, G450,
G451).
Caution
Activation/deactivation of tool radius compensation
A travel command must be programmed with G0 or G1 in an NC block with G40, G41 or
G42. This travel command must specify at least one axis in the selected working plane.
If you only specify one axis on activation, the last position on the second axis is added
automatically and traversed with both axes.
The two axes must be active as GEOAX in the channel. This can be achieved by
programming them with GEOAX.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
352 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Intersection
Select intersection with SD 42496: CUTCOM_CLSD_CONT
FALSE:
If two intersections appear on the inside when offsetting an (virtually) closed contour, which
consists of two circle blocks following on from one another, or from one circle block and one
linear block, the intersection positioned closest to the end of block on the first partial contour
is selected, in accordance with standard procedure.
A contour is deemed to be (virtually) closed if the distance between the starting point of the
first block and the end point of the second block is less than 10% of the effective
compensation radius, but not more than 1000 path increments (equals 1 mm with three
decimal places).
TRUE:
In the same situation as described above, the intersection positioned on the first partial
contour closer to the block start is selected.
Changing the direction of compensation
G41/G42, G42/G41 can be programmed without an intermediate G40.
Changing the working plane
It is not possible to change the working plane G17 to G19 when G41/G42 is active.
G41
G42
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 353
Changing the offset number D
The offset number D can be changed in compensation mode.
A modified tool radius is active with effect from the block, in which the new D number is
programmed.
Caution
The radius change or compensation movement is performed across the entire block and only
reaches the new equidistance at the programmed end point.
1&EORFNZLWKPRGLILHGUDGLXVFRUUHFWLRQ
7UDYHUVHSDWK
3URJUDPPHGSDWK
With linear movements, the tool travels along an inclined path between the starting point and
end point; with circular interpolation spiral movements are produced.
Changing the tool radius
This can be achieved, for example, using system variables. The execution is the same as for
changes in the D number.
Caution
The modified values only take effect the next time T or D is programmed. The change only
applies with effect from the next block.
Tool offsets
8.8 Tool radius compensation (G40, G41, G42)
Fundamentals
354 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
Compensation mode
Compensation mode may only be interrupted by a certain number of consecutive blocks or
M commands, which do not contain any travel commands or positional parameters in the
compensation plane: Standard 3.
Machine manufacturer
The number of consecutive blocks or M commands can be set in machine data 20250 (see
machine manufacturer).
Note
A block with a path distance of zero also counts as an interruption!
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 355
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Function
You can use these functions to adapt the approach and retraction paths, for example,
according to the desired contour or shape of the blanks.
Only G1 blocks are permitted as original approach/retraction blocks for the two functions
KONTC and KONTT. The control replaces these by polynomials for the relevant
approach/retraction path.
Programming
NORM
Or
KONT
Or
KONTC
Or
KONTT
Parameters
NORM The tool travels directly in a straight line and is positioned
perpendicular to the contour point
KONT The tool traverses the contour point according to the programmed
corner behavior G450 or G451.
KONTC Tool reaches/leaves contour point with continuous curvature.
Continuous curvature includes continuous tangent. See below. With
continuous curvature means at constant acceleration.
KONTT Tool reaches/leaves contour point along continuous tangent.
Generally, continuous tangent is not continuous acceleration.
KONTC
The contour point is approached/exited with a continuous curvature. No acceleration step
change occurs at the contour point. The path from the starting point to the contour point is
interpolated as a polynomial.
KONTT
The contour point is approached/exited along a continuous tangent. An acceleration step
change might occur at the contour point. The path from the starting point to the contour point
is interpolated as a polynomial.
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
356 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of KONTC
The full circle is approached beginning at the circle center point. The direction and curvature
radius of the approach circle at the block end point are identical to the values of the next
circle. Infeed takes place in the Z direction in both approach/retraction blocks
simultaneously. The adjacent diagram shows the vertical projection of the path.
The associated NC program segment is as follows:
$TC_DP1[1.1]= 121 ;Milling tool
$TC_DP6[1.1]=10 ;Radius 10 mm
N10 G1 X0 Y0 Z60 G64 T1 D1
F10000
N20 G41 KONTC X70 Y0 Z0 ;Approach
N30 G2 I-70 ;Full circle
N40 G40 G1 X0 Y0 Z60 ;Retract
N50 M30
3D representation: At the same time the curvature is adjusted to the circular path of the full
circle, the axes moves from Z60 to the plane of circle Z0.
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 357
Direct approach to perpendicular position, G41, G42, NORM
The tool travels in a straight line directly to the contour and is positioned perpendicular to the
path tangent at the starting point.
Selection of the approach point
When NORM is active, the tool travels directly to the compensated starting position
irrespective of the approach angle programmed for the travel movement (see diagram).
*
&RUUHFWHG
7RROSDWK
&RUUHFWHG
7RROSDWK
7DQJHQW
5DGLXV
*
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
358 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Deactivate compensation mode, G40, NORM
The tool is positioned perpendicular to the last compensated path end point and then travels
directly in a straight line to the next uncompensated position, e.g., to the tool change
location.
Choosing the retraction point
When NORM is active, the tool travels directly to the uncompensated position irrespective of
the approach angle programmed for the travel movement (see diagram).
*
*
5DGLXV
7DQJHQW
Warning
The following applies to approach and retraction movements:
You should make allowance for the modified angles of travel when programming in order to
avoid collisions.
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 359
Travel round contour at starting point, G41, G42, KONT
Two cases are distinguished here:
1. Starting point lies in front of the contour
The approach strategy is the same as with NORM.
The path tangent at the starting point serves as a dividing line between the front and rear of
the contour.
6WDUWSRLQW
%HKLQGFRQWRXU
,QIURQWRIFRQWRXU
3DWKWDQJHQW
1. Starting point lies behind the contour
The tool travels round the starting point either along a circular path or over the intersection of
the equidistant paths depending on the programmed corner behavior G450/G451.
The commands G450/G451 apply to the transition from the current block to the next block.
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
360 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G450
G450 G451
G451
Generation of the approach path
In both cases (G450/G451), the following approach path is generated:
A straight line is drawn from the uncompensated approach point. This line is a tangent to a
circle with circle radius = tool radius. The center point of the circle is on the starting point.
$SSURDFKSRLQW
$SSURDFKSDWK
6WDUWSRLQW
7RROUDGLXV
Tool offsets
8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 361
Deactivate compensation mode, G40, KONT
If the retraction point is located in front of the contour, the same retraction movement as for
NORM applies.
If the retraction point is located behind the contour, the retraction movement is the reverse of
the approach movement.
Precondition for KONTC and KONTT
The two functions KONTC and KONTT are available only if polynomial interpolation is
enabled in the control.
Description of KONTC and KONTT
The continuity conditions are observed in all three axes. It is therefore permissible to
program a path component perpendicular to the offset plane simultaneously.
Exception:
KONTT and KONTC are not available in the 3D variants of the tool radius compensation
(CUT3DC, CUT3DCC, CUT3DF).
If they are programmed, the control switches internally to NORM without an error message.
Difference between KONTC and KONTT
This diagram shows the differences in approach/retract behavior between KONTT and
KONTC. A circle with a radius of 20 mm about the center point at X0 Y-40 is compensated
with a tool with an external radius of 20 mm. The tool center point therefore moves along a
circular path with radius 40 mm. The end point of the approach blocks is at X40 Y30. The
transition between the circular block and the retraction block is at the zero point. Due to the
extended continuity of curvature associated with KONTC, the retraction block first executes a
movement with a negative Y component. This will often be undesired. This response does
not occur with the KONTT retraction block. However, with this block, an acceleration step
change occurs at the block transition.
Tool offsets
8.10 Compensation at the outside corners (G450, G451)
Fundamentals
362 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
If the KONTT or KONTC block is the approach block rather than the retraction block, the
contour is exactly the same, but machined in the opposite direction.
8.10 Compensation at the outside corners (G450, G451)
Function
G450/G451 defines the following:
On the one hand, the approach path for active KONT and the approach point behind the
contour (see section "Contour approach and retraction").
On the other hand, the corrected tool path when traveling around outside corners.
Programming
G450 DISC=…
Or
G451
Parameters
G450 Transition circle: the tool travels around workpiece corners on a
circular path with tool radius
DISC= Flexible programming of the approach and retraction instruction. In
steps of 1 from DISC=0 circle to DISC=100 intersection
G451 Intersection, the tool backs off from the workpiece corner
DISC=... is effective only when G450 is called, but can be programmed in a preceding block
without G450. Both commands are modal.
Tool offsets
8.10 Compensation at the outside corners (G450, G451)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 363
Example
In this example a transition radius is added to all outside corners (progr. in block N30). This
prevents the tool from having to stop and free cut when changing direction.
;
<
=
<
N10 G17 T1 G0 X35 Y0 Z0 F500 ;Start conditions
N20 G1 Z-5 ;Tool infeed
N30 G41 KONT G450 X10 Y10 ;Activate compensation mode
N40 Y60
N50 X50 Y30
N60 X10 Y10
;Cut contour
N80 G40 X-20 Y50 ;Deactivate compensation mode, retract on ;transition circle
N90 G0 Y100
N100 X200 M30
Tool offsets
8.10 Compensation at the outside corners (G450, G451)
Fundamentals
364 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Corner behavior, transition circle, G41, G42, G450
The tool center point travels around the workpiece corner across an arc with tool radius.
At intermediate point P*, the control executes instructions such as infeed movements or
switching functions. These instructions are programmed in blocks inserted between the two
blocks forming the corner.
G450
P*
The transition circle belongs to the next travel command with respect to the data.
Tool offsets
8.10 Compensation at the outside corners (G450, G451)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 365
Corner behavior, selectable transitions G41, G42, G450 DISC=…
DISC distorts the transition circle, thus creating sharp contour corners.
The values have the following meanings:
DISC=0 transition circle
DISC=100 intersection of the equidistant paths (theoretical value)
',6&
',6&
DISC is programmed in steps of 1.
When DISC values greater than 0 are specified, intermediate circles are shown with a
magnified height – the result is transition ellipses or parabolas or hyperbolas.
An upper limit can be defined in machine data – generally DISC=50.
Tool offsets
8.10 Compensation at the outside corners (G450, G451)
Fundamentals
366 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Path action, depending on DISC values and contour angle
Depending on the angle of the contour that is traversed, with acute contour angles and high
DISC values the tool is lifted off the contour at the corners. With angles of 120° and more,
the contour is traversed evenly (see adjacent table).
',6&
',6&
65
57RROUDGLXV67UDYHUVHRYHUVKRRW
651RUPDOL]HGRYHUVKRRW
LQUHODWLRQWRWRROUDGLXV
&RQWRXUDQJOHGHJUHHV
Corner behavior, intersection, G41, G42, G451
The tool approaches the intersection of the two equidistants, which lie in the distance
between the tool radius and the programmed contour. G451 applies only to circles and
straight lines.
At intermediate point P*, the control executes instructions such as infeed movements or
switching functions. These instructions are programmed in blocks inserted between the two
blocks forming the corner.
*
3
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 367
Note
Superfluous non-cutting tool paths can result from liftoff movements at acute contour angles.
A parameter can be used in the machine data to define automatic switchover to transition
circle in such cases.
8.11 Smooth approach and retraction
8.11.1 Approach and retraction (G140 to G143, G147, G148, G247, G248, G347, G348,
G340, G341)
Function
The soft approach and retraction function (SAR) is used to achieve a tangential approach to
the start point of a contour, regardless of the position of the start point.
*
',65
*
3URJU&RQWRXU
*
The function is mainly used in conjunction with the tool radius offset, but is not mandatory.
The approach and retraction motion consists of a maximum of 4 sub-movements:
• Start point of the movement P0
• Intermediate points P1, P2 und P3
• End point P4
Points P0, P3 und P4 are always defined. Intermediate points P1 and P2 can be omitted,
according to the parameters defined and the geometrical conditions.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
368 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
G140
Or
G141 to G143
Or
G147, G148
Or
G247, G248
Or
G347, G348
Or
G340, G341
Or
DISR=..., DISCL=..., FAD=...
Parameters
G140 Approach and retraction direction independent of the current
compensation side (basic setting)
G141 Approach from the left or retraction to the left
G142 Approach from the right or retraction to the right
G143 Approach and retraction direction depends on the relative position of
the start and end point with respect to the tangent direction
G147 Approach with a straight line
G148 Retraction with a straight line
G247 Approach with a quadrant
G248 Retraction with a quadrant
G347 Approach with a semicircle
G348 Retraction with a semicircle
G340 Approach and retraction in space (basic setting)
G341 Approach and retraction in the plane
DISR Approach and retraction with straight line (G147/G148)
Distance from the mill edge to the start point of the contour
Approach and retraction with circles (G247, G347/G248, G348)
Radius of the tool center point path
Caution: In the case of REPOS with a semicircle, DISR is the
diameter of the circle
DISCL DISCL=... Distance from the end point of the
fast infeed motion to the machining plane
DISCL=AC(...) Specifies the absolute position of the end point of the
fast infeed motion
FAD Speed of the slow infeed motion
FAD=... the programmed value applies according to the
G code of group 15 (feedrate; G93, G94, etc.)
FAD=PM(...) the programmed value is interpreted as a linear feedrate
(as G94), independently of the active G code, group 15
FAD=PR(...) the programmed value is interpreted as a revolutional
feedrate (as G95), independently of the active G code, group 15.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 369
Example
3UHW
3DSS3UHW
3DSS
3UHW
7RROFHQWHUSDWK
7RRO
+HOL[
6HPLFLUFOH
3DSS 3UHW
&RQWRXU
\
[
• Smooth approach (block N20 activated)
• Approach motion with quadrant (G247)
• Approach direction not programmed, G140 is operative, i.e., TRC is active (G41)
• Contour offset OFFN=5 (N10)
• Current tool radius=10; thus the effective offset radius for TRC=15, the radius of the SAR
contour=25, so that the radius of the tool center point path is then DISR=10.
• The end point of the circle is obtained from N30, since only the Z position is programmed
in N20
• Infeed movement
– From Z20 to Z7 (DISCL=AC(7)) with rapid traverse
– Then on to Z0 with FAD=200
– Approach circle in X-Y plane and following blocks with F1500 (in order for this speed
to become active in the following blocks, the G0 active in N30 must be overwritten by
G1, otherwise the contour would continue to be machined with G0)
• Smooth retraction (block N60 active)
• Retraction motion with quadrant (G248) and helix (G340)
• FAD not programmed, since irrelevant for G340
• Z=2 in the start point; Z=8 in the end point, since DISCL=6
• When DISR=5, the radius of SAR contour=20; that of the tool center point path=5
Retraction motions from Z8 to Z20 and the motion parallel to X-Y plane to X70 Y0
$TC_DP1[1.1]= 120 ;Tool definition T1/D1
$TC_DP6[1.1]=10 ;Radius
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
370 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
N10 G0 X0 Y0 Z20 G64 D1 T1 OFFN = 5 ;(P0app)
N20 G41 G247 G341 Z0
DISCL = AC(7) DISR = 10 F1500 FAD=200
;Approach (P3app)
N30 G1 X30 Y-10 ;(P4app)
N40 X40 Z2
N50 X50 ;(P4ret)
N60 G248 G340 X70 Y0 Z20 DISCL = 6
DISR = 5 G40 F10000
;Retract (P3ret)
N70 X80 Y0 ;(P0ret)
N80 M30
Selecting the approach and retraction contour
The appropriate G command can be used
• to approach or retract with a straight line (G147, G148),
• a quadrant (G247, G248) or
• a semicircle (G347, G348).
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 371
3
3IRUDSSURDFKUHWXUQZLWK
DVWUDLJKWOLQH*
3 &RQWRXU
',65
$SSURDFKDQGUHWUDFWLRQVKRZQZLWKLQWHUPHGLDWH
SRLQW3ZLWKVLPXOWDQHRXVDFWLYDWLRQRIWRROUDGLXV
FRPSHQVDWLRQ
3
3IRUDSSURDFKUHWXUQZLWK
4XDGUDQW*
3 &RQWRXU
3
3IRUDSSURDFKUHWXUQZLWK
6HPLFLUFOH*
3 &RQWRXU
',65
',65
7RROFHQWHUSDWK
7RRO
7RRO
7RROFHQWHUSDWK
7RRO
7RROFHQWHUSDWK
Selecting the approach and retraction direction
Use the tool radius compensation (G140, basic setting) to determine the approach and
retraction direction with positive tool radius:
• G41 active → approach from left
• G42 active → approach from right
G141, G142 and G143 provide further approach options.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
372 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Description
The G codes are only significant when the approach contour is a quadrant or a semicircle.
Motion steps between start point and end point (G340 and G341)
The approach characteristic from P0 to P4 is shown in the adjacent image.
3
0DFKLQLQJSODQH
',6&/ ',6&/
* *
3
3
3
3
3
3
33
,QIHHGPRYHPHQW
6WUDLJKWOLQHFLUFOH
RUKHOL[
6WUDLJKW
RUFLUFOH
$SSURDFKPRYHPHQWGHSHQGLQJRQ**
3
In cases which include the position of the active plane G17 to G19 (circular plane, helical
axis, infeed motion perpendicular to the active plane), any active rotating FRAME is taken
into account.
Length of the approach straight line or radius for approach circles (DISR)(see figure when
selecting approach/retraction contour)
• Approach/retract with straight line
DISR specifies the distance of the cutter edge from the starting point of the contour, i.e.,
the length of the straight line when TRC is active is the sum of the tool radius and the
programmed value of DISR. The tool radius is only taken into account if it is positive.
The resultant line length must be positive, i.e., negative values for DISR are allowed
provided that the absolute value of DISR is less than the tool radius.
• Approach/retraction with circles
DISR indicates the radius of the tool center point path. If TRC is activated, a circle is
produced with a radius that results in the tool center point path with the programmed
radius.
Distance of the point from the machining plane (DISCL) (see figure when selecting
approach/retraction contour)
If the position of point P2 is to be specified by an absolute reference on the axis
perpendicular to the circle plane, the value must be programmed in the form DISCL=AC(...).
The following applies for DISCL=0:
• With G340: The whole of the approach motion now only consists of two blocks (P1, P2
and P3 are combined). The approach contour is formed by P1 to P4.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 373
• With G341: The whole approach contour consists of three blocks (P2 and P3 are
combined). If P0 and P4 are on the same plane, only two blocks result (infeed movement
from P1 to P3 is omitted).
• The point defined by DISCL is monitored to ensure that it is located between P1 and P3,
i.e., the sign must be identical for the component perpendicular to the machining plane in
all motions that possess such a component.
• On detection of a direction reversal, a tolerance defined by the machine data
SAR_CLEARANCE_TOLERANCE is permitted.
Programming the end point P4 for approach or P0 for retraction
The end point is generally programmed with X... Y... Z...
• Programming during approach
– P4 in SAR block
– P4 is defined by the end point of the next traversing block.
Other blocks can be inserted between the SAR block and the next traversing block
without moving the geometry axes.
Example:
$TC_DP1[1.1]= 120 ;Milling tool T1/D1
$TC_DP6[1.1]=7 ;Tool with 7 mm radius
N10 G90 G0 X0 Y0 Z30 D1 T1
N20 X10
N30 G41 G147 DISCL=3 DISR=13 Z=0
F1000
N40 G1 X40 Y-10
N50 G1 X50
...
...
N30/N40 can be replaced by:
1.
N30 G41 G147 DISCL=3 DISR=13 X40
Y-10 Z0 F1000
Or
2.
N30 G41 G147 DISCL=3 DISR=13
F1000
N40 G1 X40 Y-10 Z0
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
374 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
<
',65
3
=
=
0DFKLQLQJXSWRWKLV
SRLQWZLWK*R
FRQWLQXLQJZLWK*
)
&RQWRXU
]
• Programming during retraction
– For an SAR block without programmed geometry axis,
the contour ends in P2. The position in the axes that form the machining plane are
obtained from the retraction contour. The axis component perpendicular to this is
defined by DISCL. If DISCL=0, movement runs fully in the plane.
– If only the axis is programmed perpendicular to the machining plane in the SAR block,
the contour ends in P1. The position of the other axes is obtained as described
previously. If the SAR block is also the deactivation block of the TRC, an additional
path is inserted from P1 to P0, so that there is no movement at the end of the contour
when the TRC is deactivated.
– If only one axis on the machining plane is programmed, the missing 2nd axis is
modally added from its last position in the previous block.
– For an SAR block without programmed geometry axis, the contour ends in P2. The
position in the axes that form the machining plane are obtained from the retraction
contour. The axis component perpendicular to this is defined by DISCL. If DISCL=0,
movement runs fully in the plane.
– If only the axis is programmed perpendicular to the machining plane in the SAR block,
the contour ends in P1. The position of the other axes is obtained as described
previously. If the SAR block is also the deactivation block of the TRC, an additional
path is inserted from P1 to P0, so that there is no movement at the end of the contour
when the TRC is deactivated.
– If only one axis on the machining plane is programmed, the missing 2nd axis is
modally added from its last position in the previous block.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 375
3
&RQWRXUSUHFHGLQJEORFN
3
3
7RRO
7RROFHQWHUSDWK
)ROORZLQJEORFN
ZLWKRXWFRPSHQVDWLRQ
6$5EORFN
**
5HWUDFWLRQZLWK6$5DQGVLPXOWDQHRXV
GHDFWLYDWLRQRI75&
Approach and retraction velocities
• Velocity of the previous block (G0):
All motions from 0 up to P2 are executed at this velocity, i.e., the motion parallel to the
machining plane and the part of the infeed motion up to the safety clearance.
• Programming with FAD:
Specify the feedrate for
– G341: infeed movement perpendicular to the machining plane from P2 to P3
– G340: from point P2 or P3 to P4
If FAD is not programmed, this part of the contour is also traversed at the modally
active speed of the previous block, if no F word is programmed in the SAR block.
• Programmed feedrate F:
This feedrate value is effective as of 3 or P2 if FAD is not programmed. If no F word is
programmed in the SAR block, the speed of the previous block is active.
Example:
$TC_DP1[1.1]= 120 ;Milling tool T1/D1
$TC_DP6[1.1]=7 ;Tool with 7 mm radius
N10 G90 G0 X0 Y0 Z20 D1 T1
N20 G41 G341 G247 DISCL=AC(5)
DISR=13
FAD 500 X40 Y-10 Z=0 F200
N30 X50
N40 X60
...
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
376 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
;
<
;
=
*
)
*
) )
3 3
3
3
3
During retraction, the rolls of the modally active feedrate from the previous block and the
programmed feedrate value in the SAR block are changed round, i.e., the actual retraction
contour is traversed with the old feedrate value and a new speed programmed with the F
word applies from P2 up to P0.
1RYHORFLW\
SURJUDPPHG
2QO\)
SURJUDPPHG
2QO\)$'
SURJUDPPHG
)DQG)$'
SURJUDPPHG
3 3 33 3
5DSLGWUDYHUVHLI*LVDFWLYHRWKHUZLVHZLWK
ROGQHZ)ZRUG
9HORFLW\RIWKHSUHYLRXVEORFN
ROG)ZRUG
,QIHHGYHORFLW\SURJUDPPHGZLWK)$'
1HZPRGDOYHORFLW\SURJUDPPHG
9HORFLW\
9HORFLWLHVLQWKH6$5VXEEORFNV
RQUHWUDFWLRQZLWK*
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 377
9HORFLWLHVLQWKH6$5VXEEORFNV
RQUHWUDFWLRQZLWK*
1HZPRGDOYHORFLW\SURJUDPPHG
9HORFLW\
,QIHHGYHORFLW\SURJUDPPHGZLWK)$'
9HORFLW\RIWKHSUHYLRXVEORFN
ROG)ZRUG
5DSLGWUDYHUVHLI*LVDFWLYHRWKHUZLVHZLWK
ROGQHZ)ZRUG
333
33
)DQG)$'
SURJUDPPHG
2QO\)$'
SURJUDPPHG
2QO\)
SURJUDPPHG
1RYHORFLW\
SURJUDPPHG
1RYHORFLW\
SURJUDPPHG
2QO\)
SURJUDPPHG
2QO\)$'
SURJUDPPHG
)DQG)$'
SURJUDPPHG
3 3 3 3 3
5DSLGWUDYHUVHLI*LVDFWLYH
RWKHUZLVHZLWKROGQHZ)ZRUG
9HORFLW\RIWKHSUHYLRXVEORFN
ROG)ZRUG
,QIHHGYHORFLW\5HWUDFWLRQVSHHG
1HZPRGDOYHORFLW\SURJUDPPHG
9HORFLW\
9HORFLWLHVLQWKH6$5VXEEORFNV
RQUHWUDFWLRQ
Reading positions
Points P3 and P4 can be read in the WCS as a system variable during approach.
• $P_APR: reading P
• 3 (initial point)
• $P_AEP: reading P
• 4 (contour starting point)
• $P_APDV: read whether $P_APR and $P_AEP contain valid data
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
378 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.11.2 Approach and retraction with enhanced retraction strategies (G460, G461, G462)
Function
In certain special geometrical situations, enhanced approach and retraction strategies,
compared with the previous implementation with activated collision monitoring for approach
and retraction block, are required in order to activate or deactivate tool radius compensation.
For instance, collision monitoring can lead to a section of the contour not being fully
machined. See following image.
&HQWHUSRLQWSDWKZLWK
WRROUDGLXVFRPSHQVDWLRQ
3URJUDPPHG
&RQWRXU
7RROUDGLXV
1
1 <
;
1
Retraction behavior with G460
Programming
G460
Or
G461
or
G462
Parameters
G460 As before (activation of collision monitoring for approach and
retraction block)
G461 Insertion of a circle in the TRC block, if no intersection point is
possible, whose center point is at the end point of the uncorrected
block and whose radius is equal to the tool radius.
Auxiliary circuit is used to machine around the contour end point (i.e.
up to the end of the countour) up to the intersection.
G462 Insertion of a straight line in the TRC block if no intersection point is
possible; the block is extended by its end tangent (default setting)
Machining is done up to the extension of the last contour element (i.e.
up to just before the contour end).
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 379
Further information
The approach behavior is symmetrical to the retraction behavior.
The approach/retraction behavior is determined by the state of the G command in the
approach/retraction block. The approach behavior can therefore be set independently of the
retraction behavior.
Example of retraction behavior with G460
The following example describes only the situation for deactivation of tool radius
compensation. The behavior for approach is the same.
G42 D1 T1 ;Tool radius 20mm
...
G1 X110 Y0
N10 X0
N20 Y10
N30 G40 X50 Y50
Example of approach with G461
N10 $TC_DP1[1,1]=120 ;Tool type: milling tool
N20 $TC_DP6[1,1]=10 ;Tool radius
N30 X0 Y0 F10000 T1 D1
N40 Y20
N50 G42 X50 Y5 G461
N60 Y0 F600
N70 X30
N80 X20 Y-5
N90 X0 Y0 G40
N100 M30
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
380 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G461
If no intersection is possible between the last TRC block and a preceding block, the offset
curve of this block is extended with a circle whose center point lies at the end point of the
uncorrected block and whose radius is equal to the tool radius.
The control attempts to cut this circle with one of the preceding blocks.
&HQWHUSRLQWSDWKZLWK
WRROUDGLXVFRPSHQVDWLRQ
3URJUDPPHG
&RQWRXU
$X[LOLDU\FXUYH
1
1 <
;
1
Retraction behavior with G461 (see example)
Collision monitoring CDON, CDOF
If CDOF is active (see section Collision monitoring, CDON, CDOF), the search is aborted
when an intersection is found, i.e., the system does not check whether further intersections
with previous blocks exist.
If CDON is active, the search continues for further intersections after the first intersection is
found.
An intersection point, which is found in this way, is the new end point of a preceding block
and the start point of the deactivation block. The inserted circle is used exclusively to
calculate the intersection and does not produce a traversing movement.
Note
If no intersection is found, alarm 10751 (collision danger) is output.
Tool offsets
8.11 Smooth approach and retraction
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 381
G462
If no intersection is possible between the last TRC block and a preceding block, a straight
line is inserted, on retraction with G462 (initial setting), at the end point of the last block with
tool radius compensation (the block is extended by its end tangent).
The search for the intersection is then identical to the procedure for G461.
&HQWHUSRLQWSDWKZLWK
WRROUDGLXVFRPSHQ
VDWLRQ
3URJUDPPHG
&RQWRXU
$X[LOLDU\
FXUYH
1
1 <
;
1
Retraction behavior with G462 (see example)
With G462, the corner generated by N10 and N20 in the example program is not machined
to the full extent actually possible with the tool used. However, this behavior may be
necessary if the part contour (as distinct from the programmed contour), to the left of N20 in
the example, is not permitted to be violated even with y values greater than 10 mm.
Corner behavior with KONT
If KONT is active (travel round contour at start or end point), the behavior differs according to
whether the end point is in front of or behind the contour.
• End point in front of contour
If the end point is in front of the contour, the retraction behavior is the same as with
NORM. This property does not change even if the last contour block for G451 is extended
with a straight line or a circle.Additional circumnavigation strategies to avoid a contour
violation in the vicinity of the contour end point are therefore not required.
• Endpoint behind the contour
If the end point is behind the contour, a circle or straight line is always inserted depending
on G450/G451. In this case, G460-462 has no effect. If the last traversing block in this
situation has no intersection with a preceding block, an intersection with the inserted
contour element or with the straight line of the end point of the bypass circle to the
programmed endpoint can result.
If the inserted contour element is a circle (G450), and this forms an interface with the
preceding block, this is equal to the interface that would occur with NORM and G461. In
general, however, a remaining section of the circle still has to be traversed. For the linear
part of the retraction block, no further calculation of intersection is required.
In the second case, if no interface of the inserted contour element with the preceding
blocks is found, the intersection between the retraction straight line and a preceding block
is traversed.
Therefore, a behavior that deviates from G460 can only occur with active G461 or G462
either if NORM is active or the behavior with KONT is geometrically identical to that with
NORM.
Tool offsets
8.12 Collision monitoring (CDON, CDOF, CDOF2)
Fundamentals
382 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.12 Collision monitoring (CDON, CDOF, CDOF2)
Function
When CDON (Collision Detection ON) and tool radius compensation are active, the control
monitors the tool paths with Look Ahead contour calculation. This Look Ahead function
allows possible collisions to be detected in advance and permits the control to actively avoid
them.
When collision detection is off (CDOF), a search is made at inside corners in the previous
traversing block (and if necessary in blocks further back) for a common intersection point for
the current block. If no intersection is found with this method, an error is generated.
Programming
CDON
Or
CDOF
Or
CDOF2
Parameters
CDON Activate bottleneck detection
CDOF Deactivate bottleneck detection
CDOF2 Determine tool offset direction from adjacent block parts.
CDOF2 is active only for 3D circumferential milling.
Tool offsets
8.12 Collision monitoring (CDON, CDOF, CDOF2)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 383
CDOF helps prevent the incorrect detection of bottlenecks, e.g., due to missing information,
which is not available in the NC program.
Machine manufacturer
The number of NC blocks monitored can be defined in the machine data (see machine
manufacturer).
Example of milling on the center-point path with standard tools
The NC program defines the center-point path of a standard tool. The contour for a tool
currently in use results in an undersize, which is shown on an unrealistically large scale
solely to illustrate the geometric conditions. The following description is based on the simple
assumption that the control can only "see" three blocks.
1
1
1
3
3
1
3DUWFRQWRXU
&RPSHQ
VDWLQJ
PRYHPHQW
8QGHUVL]H
6WDQGDUG
VL]H
2IIVHWSRLQWLQ
6WDUWSRLQWRI
1
2IIVHWSRLQWLQHQGSRLQWRI1
3URJUDPPHG
RULJLQDOSDWK
VWDQGDUGWRRO
&RPSHQVDWLQJPRYHPHQWLQDEVHQFHRIVWDUWSRLQW
&RUUHFWHG
VHWSRLQWSDWK
RIIVHWFXUYH
Since an intersection exists only between the offset curves of the two blocks N10 and N40,
the two blocks N20 and N30 would have to be omitted. In this instance, the control is still not
aware of block N40 if N10 must be processed subsequently. Only a single block can
therefore be omitted.
When CDOF2 is active, the compensatory motion shown in the diagram is executed and not
halted. In this situation, an active CDOF or CDON would generate an alarm.
Identifying critical machining situations
The following are some examples of critical machining situations, which can be detected by
the control and compensated for by modifying the tool paths.
In order to prevent program stops, you should always select the tool with the widest radius
from all of the tools used when testing the program.
In each of the following examples a tool with too wide a radius was selected for machining
the contour.
Tool offsets
8.12 Collision monitoring (CDON, CDOF, CDOF2)
Fundamentals
384 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Bottleneck detection
3URJUDPPHGFRQWRXU
7RROSDWK
Since the tool radius selected is too wide to machine this inside contour, the "bottleneck" is
bypassed.
An alarm is output.
Contour path shorter than tool radius
3URJUDPPHGFRQWRXU
7RROSDWK
The tool travels round the workpiece corner on a transition circle and then continues to
follow the programmed contour exactly.
Tool offsets
8.12 Collision monitoring (CDON, CDOF, CDOF2)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 385
Tool radius too wide for inside machining
3URJUDPPHG
&RQWRXU
7RROSDWK
In such cases, the contours are machined only to the extent possible without damaging the
contour..
Tool offsets
8.13 2D tool compensation (CUT2D, CUT2DF)
Fundamentals
386 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.13 2D tool compensation (CUT2D, CUT2DF)
Function
With CUT2D or CUT2DF you define how the tool radius compensation is to act or to be
interpreted when machining in inclined planes.
Tool length compensation
The tool length compensation generally always refers to the fixed, non-rotated working
plane.
2D tool radius compensation with contour tools
The tool radius compensation for contour tools is used for automatic cutting-edge selection
in the case of non-axially symmetrical tools that can be used for piece-by-piece machining of
individual contour segments.
Programming
CUT2D
Or
CUT2DF
2D tool radius compensation for contour tools is activated if either of the two machining
directions G41 or G42 is programmed with CUT2D or CUT2DF.
Note
If tool radius compensation is not activated, a contour tool will behave like a standard tool
with only the first cutting edge.
Parameters
CUT2D Activate 2 1/2 D radius compensation (default)
CUT2DF Activate 2 1/2 D radius compensation, tool radius compensation
relative to the current frame or to inclined planes
CUT2D is used when the orientation of the tool cannot be changed and the workpiece is
rotated for machining on inclined surfaces.
CUT2D is generally the standard setting and does not, therefore, have to be specified
explicitly.
Cutting-edge selection with contour tools
Up to a maximum of 12 cutting edges can be assigned to each contour tool in any order.
Machine manufacturer
Tool offsets
8.13 2D tool compensation (CUT2D, CUT2DF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 387
The valid tool types for non-axially symmetrical tools and the maximum number of cutting
edges (Dn = D1 to D12) are defined by the machine manufacturer via machine data. Please
contact the machine manufacturer if not all of the 12 cutting edges are available.
References:
/FB1/Function Manual Basic Functions; Tool Offset (W1)
Tool radius compensation, CUT2D
As for many applications, tool length compensation and tool radius compensation are
calculated in the fixed working plane specified with G17 to G19.
;
;
==
Example of G17 (X/Y plane):
Tool radius compensation is active in the non-rotated X/Y plane, tool length compensation in
the Z direction.
Tool offset values
For machining on inclined surfaces, the tool compensation values have to be defined
accordingly, or be calculated using the functions for "Tool length compensation for orientable
tools". For more information on this calculation method, see chapter "Tool orientation and
tool length compensation".
Tool offsets
8.13 2D tool compensation (CUT2D, CUT2DF)
Fundamentals
388 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Tool radius compensation, CUT2DF
In this case, it is possible to arrange the tool orientation perpendicular to the inclined working
plane on the machine.
;
;
==
If a frame containing a rotation is programmed, the compensation plane is also rotated with
CUT2DF. The tool radius compensation is calculated in the rotated machining plane.
Note
The tool length compensation continues to be active relative to the non-rotated working
plane.
Definition of contour tools, CUT2D, CUT2DF
A contour tool is defined by the number of cutting edges (on the basis of D nos) associated
with a T no. The first cutting edge of a contour tool is the cutting edge that is selected when
the tool is activated. If, for example, D5 is activated on T3 D5, then it is this cutting edge and
the subsequent cutting edges that define the contour tool either partially or as a whole. The
previous cutting edges will be ignored.
References:
/FB1/Function Manual Basic Function; Tool Offset (W1)
Tool offsets
8.14 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 389
8.14 Tool length compensation for orientable toolholders (TCARR,
TCOABS, TCOFR)
Function
When the spatial orientation of the tool changes, its tool length components also change.
;
;
==
,
,
,
After a reset, e.g., through manual setting or change of the toolholder with a fixed spatial
orientation, the tool length components also have to be determined again. This is performed
using the TCOABS and TCOFR path commands.
For a tool holder of an active frame that can be orientated, when selecting the tool with
TCOFRZ, TCOFRY, and TCOFRX, it is possible to define the direction in which the tool
should point.
Programming
TCARR=[m]
or
TCOABS
or
TCOFR
or
TCOFRZ, TCOFRY, TCOFRX
Parameter
TCARR=[m] Request toolholder with the number "m"
TCOABS Determine tool length components from the orientation of the current
toolholder
Tool offsets
8.14 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR)
Fundamentals
390 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
TCOFR Determine tool length components from the orientation of the active
frame
TCOFRZ Orientable toolholder from active frame with a tool pointing in the Z
direction
TCOFRY Orientable toolholder from active frame with a tool pointing in the Y
direction
TCOFRX Orientable toolholder from active frame with a tool pointing in the X
direction
Determine tool length compensation from the orientation of the toolholder, TCOABS
TCOABS calculates the tool length compensation from the current orientation angles of the
toolholder; stored in system variables $TC_CARR13 and $TC_CARR14.
For a definition of toolholder kinematics with system variables, see
References: /PGA/Job Planning Programming Manual; Tool Offsets,
"Toolholder Kinematics".
In order to make a new calculation of the tool length compensation when frames are
changed, the tool has to be selected again.
Tool direction from active frame
It is possible to set the orientating toolholder such that command
• TCOFR or TCOFRZ points in Z direction.
• TCOFRY points in Y direction.
• TCOFRX points in X direction.
If there is a switchover between TCOFR and TCOABS, the tool length compensation is
calculated again.
Request toolholder, TCARR
With TCARR, the toolholder number m is requested with its geometry data (offset memory).
With m=0, the active toolholder is deselected.
The geometry data of the toolholder only become active after a tool is called. The selected
tool remains active after a toolholder change has taken place.
The current geometry data for the toolholder can also be defined in the parts program via the
corresponding system variables.
Tool offsets
8.14 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 391
Recalculation of tool length compensation, TCOABS with frame change
In order to make a new calculation of the tool length compensation when frames are
changed, the tool has to be selected again.
Note
The tool orientation must be manually adapted to the active frame.
When the tool length compensation is calculated, the angle of rotation of the toolholder is
calculated in an intermediate step. With toolholders with two rotary axes, there are generally
two sets of rotation angles, which can be used to adapt the tool orientation to the active
frame; therefore, the rotation angle values stored in the system variables must at least
correspond approximately to the mechanically set rotation angles.
Note
Tool orientation
It is not possible for the control to check whether the rotation angles calculated by means of
the frame orientation are settable on the machine.
If the rotary axes of the toolholder are arranged such that the tool orientation calculated by
means of the frame orientation cannot be reached, then an alarm is output.
The combination of tool precision compensation and the functions for tool length
compensation on movable toolholders is not permissible. If both functions are called
simultaneously, an error message is issued.
The TOFRAME function allows a frame to be defined on the basis of the direction of
orientation of the selected toolholder. For more information please refer to chapter "Frames".
When orientation transformation is active (3, 4 or 5-axis transformation), it is possible to
select a toolholder with an orientation deviating from the zero position without causing output
of an alarm.
Transfer parameter from standard and measuring cycles
For the transfer parameter of standard and measuring cycles, the following defined value
ranges apply.
For angular value, the value range is defined as follows:
• Rotation around 1st geometry axis: -180 degrees to +180 degrees
• Rotation around 2nd geometry axis: -90 degrees to +90 degrees
• Rotation around 3rd geometry axis: -180 degrees to +180 degrees
Reference:
/PG/ Fundamentals Programming Manual; Frames, Chapter "Programmable rotation (ROT,
AROT, RPL)"
Tool offsets
8.15 Grinding-specific tool monitoring in parts programs (TMON, TMOF)
Fundamentals
392 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
When transferring angular values to a standard or measuring cycle, the following should be
carefully observed:
Values less than the calculation resolution of the NC should be rounded-off to zero!
The calculation resolution of the NC for angular positions is defined in the machine data:
MD10210 $MN_INT_INCR_PER_DEG
8.15 Grinding-specific tool monitoring in parts programs (TMON, TMOF)
Function
The command TMON is used to activate geometry and speed monitoring for grinding tools
(types 400-499) in the NC parts program. Monitoring remains active until it is deactivated in
the parts program with TMOF.
Machine manufacturer
See machine manufacturer's specifications
Programming
TMON (T no.)
Or
TMOF (T no.)
Tool offsets
8.15 Grinding-specific tool monitoring in parts programs (TMON, TMOF)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 393
Parameters
TMON (T no.) Activate tool monitoring
TMOF (T no.) Deselect tool monitoring
T No. = 0: Deactivate monitoring for all
tools
It is only necessary to
specify the T number if the
tool with this
T number is not active.
Assignment of tool-specific parameters
Further tool-specific parameters can be set up in the machine data and assigned by the
user.
Parameters Meaning Data type
Tool-specific parameters
$TC_TPG1 Spindle number Integer
$TC_TPG2 Chaining rule
The parameters are automatically kept
identical for the left and right side of the
wheel.
Integer
$TC_TPG3 Minimum wheel radius Real
$TC_TPG4 Minimum wheel width Real
$TC_TPG5 Current wheel width Real
$TC_TPG6 Maximum speed Real
$TC_TPG7 Maximum peripheral speed Real
$TC_TPG8 Angle of inclined wheel Real
$TC_TPG9 Parameter number for radius calculation Integer
Requirements
You can only activate tool monitoring if the tool-specific grinding data $TC_TPG1 to
$TC_TPG9 are set, see
/FB1/Function Manual Basic Functions; Tool Offset (W1).
According to the machine data settings, tool monitoring for the grinding tools (types 400-499)
can be automatically activated when the tool selection is activated.
Only one monitoring routine can be active at any one time for each spindle.
Geometry monitoring
The current wheel radius and the current width are monitored.
The set speed is monitored against the speed limitation cyclically with allowance for the
spindle override.
The speed limit is the smaller value resulting from a comparison of the maximum speed with
the speed calculated from the maximum wheel peripheral speed and the current wheel
radius.
Working without a T or D number
In the machine data, a default T and D number
Tool offsets
8.16 Additive offsets
Fundamentals
394 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
• T number, and
• D number can be set,
that do not have to be reprogrammed and are effective after Power ON/Reset.
Example
All machining is performed with the same grinding wheel.
Machine data can be set to keep the current tool active after Reset; see
/PGA/Programming Manual Advanced; Free D-Number Assignment, Cutting Edge Numbers.
8.16 Additive offsets
Function
Additive offsets are essentially process offsets which can be programmed during machining.
They refer to the geometrical data of a tool edge and are thus components of the tool edge
data.
The data of an additive offset are addressed via a DL number (DL: location-dependent;
offsets relative to relevant location) and enter tool offset via parameter display in the
Parameter area.
References: /BAD, BEM/ "Operator's Guide HMI Advanced, HMI Embedded" chapter
"Parameters"
Tool offsets
8.16 Additive offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 395
8.16.1 Select offsets (via DL numbers)
Function
Setup value:
The setup value is defined optionally by the machine manufacturer in MD.
Same tool edge:
The same tool edge is used for 2 bearing seats (see example). Compensation can be made
for a location-dependent measurement error occurring as a result of machining forces, etc.
=
;
'
''/
Location 1Location 2
Fine offset:
Location-dependent allowances can be made for over/under-dimensioning.
Parameters
Machine data are used to activate and define the number of additive offsets. Please refer to
the machine manufacturer's instructions.
Example
N110 T7 D7 ;The tool turret is positioned at location 7
;D7 and DL=1 are activated and traversed in the next block
N120 G0 X10 Z1 ;N120
N130 G1 Z-6
N140 G0 DL=2 Z-14 ;DL=2 is activated in addition to D7 and traversed
;in the next block
N150 G1 Z-21
N160 G0 X200 Z200 ;Approach tool change point
...
Tool offsets
8.16 Additive offsets
Fundamentals
396 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.16.2 Specify wear and setup values ($TC_SCPxy[t,d], $TC_ECPxy[t,d])
Function
Wear and setup values can be read and written via system variables and the corresponding
OPI services.
The logic is based on the logic of the corresponding system variables for tools and tool
noses.
Programming
$TC_SCPxy [t,d] Wear values
or
$TC_ECPxy [t,d] Setup values
Parameter
$TC_SCPxy Wear values are assigned to the corresponding geometry parameters
via xy, where x is the number of the wear value and y is the reference
to the geometry parameter.
$TC_ECPxy Setup values are assigned to the corresponding geometry parameters
via xy, where x is the number of the setup value and y is the reference
to the geometry parameter.
t T number of the tool
d D number of the tool nose
Note
The defined wear and setup values are added to the geometry parameters and the other
offset parameters (D numbers).
Example
The wear value of length 1 is set to the value 1.0 for the tool nose (D number d) of the
tool (t).
Parameter: $TC_DP3 (length 1, with turning tools)
Wear values: $TC_SCP13 to $TC_SCP63
Setup values: $TC_ECP13 to $TC_ECP63
$TC_SCP43 [t, d] = 1.0
Tool offsets
8.16 Additive offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 397
8.16.3 Delete additive offsets (DELDL)
Function
DELDL is used to delete the additive offsets for the tool edge of a tool (in order to release
memory). Both the defined wear values and the setup values are deleted.
Programming
status = DELDL [t,d]
Parameters
DELDL [t,d] All additive offsets of the tool edge with D number d of tool t are deleted
DELDL[t] All additive offsets of all tool edges of tool t are deleted
DELDL All additive offsets of the tool edges of all tools of the TO- unit are
deleted (for the channel, in which the command is programmed)
status 0: Offsets have been successfully deleted.
–: Offsets have not been deleted (if the parameter settings specify
exactly one tool edge), or not deleted completely (if the parameter
settings identify several tool edges).
Note
The wear and setup values of active tools cannot be deleted (behave similar to deletion of D
or tool data).
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
398 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.17 Special handling of tool offsets
Function
Setting data SD 42900 - SD 42960 can be used to control the evaluation of the sign for tool
length and wear.
The same applies to the behavior of the wear components when mirroring geometry axes or
changing the machining plane, and also to temperature compensation in tool direction.
Parameter
Where reference is made below to wear values, this means in each case the sum of the
actual wear values ($TC_DP12 to $TC_DP20) and the total offsets with the wear ($SCPX3
to $SCPX11) and setup values ($ECPX3 to $ECPX11).
For more details on total offsets, see:
References: /FBW/Description of Functions, Tool Management
SD42900
MIRROR_TOOL_LENGTH
Mirroring of tool-length components and components of the tool base
dimension
D42910 MIRROR_TOOL_WEAR Mirroring of wear values of the tool-length components
SD42920 WEAR_SIGN_CUTPOS Sign evaluation of the wear components depending on the tool point
direction
SD42930 WEAR_SIGN Inverts the sign of the wear dimensions
SD42935 WEAR_TRANSFORM Transformation of wear values
SD42940
TOOL_LENGTH_CONST
Assignment of tool-length components to geometry axes
SD42950 TOOL_LENGTH_TYPE Assignment of the tool-length components independent of tool type
SD42960 TOOL_TEMP_COMP Temperature compensation value in tool direction. Also operative
when tool orientation is programmed.
References:
/PGA/Programming Manual, Advanced, "Tool Offsets"
/FB1/Function Manual Basic Functions; Tool Offset (W1)
Description
Activation of modified setting data
When the setting data described above are modified, the tool components are not
reevaluated until the next time a tool edge is selected. If a tool is already active and the data
of this tool are to be reevaluated, the tool must be selected again.
The same applies in the event that the resulting tool length is modified due to a change in
the mirroring status of an axis. The tool must be selected again after the mirror command, in
order to activate the modified tool-length components.
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 399
Orientable toolholders and new setting data
Setting data SD 42900-42940 have no effect on the components of an active orientable
toolholder. However, the calculation with an orientable toolholder always allows for a tool
with its total resulting length (tool length + wear + tool base dimension). All modifications
initiated by the setting data are included in the calculation of the resulting total length; i.e.,
vectors of the orientable toolholder are independent of the machining plane.
Note
When orientable toolholders are used, it is frequently practical to define all tools for a non-
mirrored basic system, even those which are only used for mirrored machining. When
machining with mirrored axes, the toolholder is then rotated such that the actual position of
the tool is described correctly. All tool-length components then automatically act in the
correct direction, dispensing with the need for control of individual component evaluation via
setting data, depending on the mirroring status of individual axes.
Further application options
The use of orientable toolholder functionality can also be useful if there is no physical option
of turning tools on the machine, even though tools with different orientations are permanently
installed. Tool dimensioning can then be performed uniformly in a basic orientation, where
the dimensions relevant for machining are calculated according to the rotations of a virtual
toolholder.
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
400 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.17.1 Mirroring of tool lengths
Function
Set setting data SD 42900 MIRROR_TOOL_LENGTH and SD 42910
MIRROR_TOOL_WEAR not equal to zero can be used to mirror tool length components and
components of the tool base dimensions with wear values of the corresponding axes.
=
:
=
0
:
;
0
:&6
'ZLWK6/
;
:&6
'ZLWK6/
'
Parameters
SD 42900 MIRROR_TOOL_LENGTH
Setting data not equal to zero:
The tool length components ($TC_DP3, $TC_DP4 and $TC_DP5) and the components of
the tool base dimensions ($TC_DP21, $TC_DP22 and $TC_DP23), whose associated axes
are mirrored, are also mirrored – through sign inversion.
The wear values are not mirrored. If these are also to be mirrored, setting data
$SC_MIRROR_TOOL_WEAR must be enabled.
SD 42910 MIRROR_TOOL_WEAR
Setting data not equal to zero:
The wear values of the tool length components, whose associated axes are mirrored, are
also mirrored - by sign inversion.
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 401
8.17.2 Wear sign evaluation
Function
Set setting data SD 42920 WEAR_SIGN_CUTPOS und SD 42930 WEAR_SIGN not equal to
zero can be used to invert the sign evaluation of the wear components.
Parameters
SD 42920 WEAR_SIGN_CUTPOS
Setting data not equal to zero:
In the case of tools with a relevant tool point direction (turning and grinding tools, tool types
400), the sign evaluation of the wear components depends on the tool point direction in the
machining plane. This setting data has no effect with tool types, which do not have a relevant
tool point direction.
In the following table, the dimensions whose sign is inverted by SD 42920 (not equal to 0)
are marked with an X:
Length of cutting edge Length 1 Length 2
1
2 X
3 X X
4 X
5
6
7 X
8 X
9
Note
The sign settings of SD 42920 and 42910 are independent. For example, if the sign of a
dimensional parameter is changed by both setting data, the resulting sign is unchanged.
SD 42930 WEAR_SIGN
Setting data not equal to zero:
the sign of all wear dimensions is inverted. This affects both the tool length and other
variables such as tool radius, rounding radius, etc.
If a positive wear dimension is entered, the tool becomes "shorter" and "thinner", see chapter
"Tool offsets, Special handling, Activation of changed setting data".
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
402 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.17.3 Coordinate system of the active machining operation
(TOWSTD/TOWMCS/TOWWCS/TOWBCS/TOWTCS/TOWKCS)
Function
Depending on the kinematics of the machine or the availability of an orientable toolholder,
the wear values measured in one of these coordinate systems are converted or transformed
to a suitable coordinate system.
Programming
TOWSTD
Or
TOWMCS
Or
TOWWCS
Or
TOWBCS
Or
TOWTCS
Or
TOWKCS
Parameters
Coordinate systems of active machining operation
The following coordinate systems can produce tool length offsets that can be used to
incorporate the tool length component "wear" into an active tool via the corresponding G
code of Group 56.
1. Machine coordinate system (MCS)
2. Basic coordinate system (BCS)
3. Workpiece coordinate system (WCS)
4. Tool coordinate system (TCS)
5. Tool coordinate system of kinematic transformation (KCS)
TOWSTD Initial setting value for offsets in tool length wear value
TOWMCS Offsets in tool length in MCS
TOWWCS Offsets in tool length in WCS
TOWBCS Offsets in tool length in BCS
TOWTCS Offsets of tool length at toolholder reference point (orientable
toolholder)
TOWKCS Offsets of tool length at tool head (kinematic transformation)
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 403
Description
The most important distinguishing features are shown in the following table:
G code Wear value Active orientable toolholder
TOWSTD Initial value, tool length Wear values are subject to rotation
TOWMCS Wear value in MCS. TOWMCS is
identical to TOWSTD if no orientable
toolholder is active.
Only the vector of the resultant tool
length rotates. Wear is ignored
TOWWCS The wear value is converted to the
MCS in the WCS
The tool vector is calculated as with
TOWMCS, i.e., the wear value is
ignored
TOWBCS The wear value is converted to the
MCS in the BCS
The tool vector is calculated as with
TOWMCS, i.e., the wear value is
ignored
TOWTCS The wear value is converted to the
MCS in the tool coordinate system
The tool vector is calculated as with
TOWMCS, i.e., the wear value is
ignored
TOWWCS, TOWBCS, TOWTCS: The wear vector is added to the tool vector.
Linear transformation
The tool length can be defined meaningfully in the MCS only if the MCS is generated by
linear transformation from the BCS.
Non-linear transformation
If, for example, a non-linear transformation is active with TRANSMIT, the BCS is
automatically applied when the MCS is specified as the chosen coordinate system.
No kinematic transformation and no orientable toolholder
If neither a kinematic transformation nor an orientable toolholder is active, then all the other
four coordinate systems (except for the WCS) are combined. It is then only the WCS, which
is different to the other systems. Since only tool lengths need to be evaluated, translations
between the coordinate systems are irrelevant.
References
For further information about tool offsets, please see:
/FB1/Function Manual Basic Functions; Tool Offset (W1)
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
404 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Inclusion of wear values in calculation
The setting data SD 42935 WEAR_TRANSFORM defines, which of the following three wear
components
1. Wear
2. Total offsets fine
3. Total offsets coarse
are to be made subject to a rotation by way of an adapter transformation or orientable
toolholder if one of the following G codes is active.
• TOWSTD Initial setting
for offsets in tool length
• TOWMCS Wear values
in the machine coordinate system (MCS)
• TOWWCS Wear values
in workpiece coordinate system (WCS)
• TOWBCS Wear values (BCS)
in basic coordinate system
• TOWTCS Wear values in tool coordinate system at the toolholder (T toolholder reference)
• TOWKCS Wear values in coordinate system of tool head with kinematic transformation
Note
Evaluation of individual wear components (assignment to geometry axes, sign evaluation)
is influenced by the
Active plane
Adapter transformation and
- The following setting data:
SD 42910: MIRROW_TOOL_WEAR
SD 42920: WEAR_SIGN_CUTPOS
SD 42930: WEAR_SIGN
SD 42940: TOOL_LENGTH_CONST
SD 42950: TOOL_LENGTH_TYPE
Tool offsets
8.17 Special handling of tool offsets
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 405
8.17.4 Tool length and plane change
Function
With the set setting data SD 42940 TOOL_LENGTH_CONST not equal to zero, you can
assign tool length components such as length, wear and base dimension to the geometry
axes for turning and grinding tools at a plane change.
Parameters
SD 42940 TOOL_LENGTH_CONST
Setting data not equal to zero:
The assignment between the tool length components (length, wear and tool base dimension)
and the geometry axes is not modified when the machining plane is changed (G17-19).
The following table shows the assignment between the tool length components and the
geometry axes for turning and grinding tools (tool types 400 to 599):
Table of Contents Length 1 Length 2 Length 3
17 Y X Z
*) X Z Y
19 Z Y X
-17 X Y Z
-18 Z X Y
-19 Y Z X
*) Each value not equal to 0 which is not equal to one of the six listed values is evaluated as
value 18.
The following table shows the assignment between the tool length components and the
geometry axes for all other tools (tool types < 400 or > 599):
Machining plane Length 1 Length 2 Length 3
*) Z Y X
18 Y X Z
19 X Z Y
-17 Z X Y
-18 Y Z X
-19 X Y Z
*) Each value not equal to 0 which is not equal to one of the six listed values is evaluated as
value 17.
Further information
The representation in the tables assumes that the geometry axes to 3 are labeled X, Y, Z.
The axis order and not the axis identifier determines the assignment between an offset
and an axis.
Tool offsets
8.18 Tools with a relevant cutting edge length
Fundamentals
406 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
8.18 Tools with a relevant cutting edge length
Function
In the case of tools with a relevant tool point direction (turning and grinding tools – tool types
400–599; see chapter "Sign evaluation wear"), a change from G40 to G41/G42 or vice-versa
is treated as a tool change. If a transformation is active (e.g., TRANSMIT), this leads to a
preprocessing stop (decoding stop) and hence possibly to deviations from the intended part
contour.
This original functionality changes with regard to:
1. Preprocessing stop on TRANSMIT
2. Calculation of intersection points at approach and retraction with KONT
3. Tool change with active tool radius compensation
4. Tool radius compensation with variable tool orientation at transformation
Description
This original functionality was changed as follows:
• A change from G40 to G41/G42 and vice-versa is no longer treated as a tool change.
Therefore, a preprocessing stop no longer occurs with TRANSMIT.
• The straight line between the tool edge center points at the block start and block end is
used to calculate intersection points with the approach and retraction block. The
difference between the tool edge reference point and the tool edge center point is
superimposed on this movement.
On approach and retraction with KONT (tool circumnavigates the contour point, see
above subsection "Contour approach and retraction"), superimposition takes place in the
linear part block of the approach or retraction motion. The geometric conditions are
therefore identical for tools with and without a relevant tool point direction. Differences
from the previous behavior occur only in relatively rare situations where the approach or
retraction block does not intersect with an adjacent motion block, see diagram below.
Tool offsets
8.18 Tools with a relevant cutting edge length
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 407
/DVWSRVLWLRQRIFXWWLQJHGJHFHQWHUSRLQW
RQWKHFRQWRXU6:DQGKLJKHU
3URJUDPPHGUHWUDFWLRQEORFN
%ORFNZLWKRXW
LQWHUVHFWLRQZLWK
SUHYLRXVEORFN
7RROHGJHUHIHUHQFHSRLQW
&XWWLQJHGJHFHQWHUSRLQW
7RROHQGSRVLWLRQ
7RROHGJHUHIHUHQFHSRLQW
&HQWHUSRLQWSDWK
/DVWSRVLWLRQRIFXWWLQJHGJHFHQWHUSRLQW
• In circle blocks and in motion blocks containing rational polynomials with a denominator
degree > 4, it is not permitted to change a tool with active tool radius compensation in
cases where the distance between the tool edge center point and the tool edge reference
point changes. With other types of interpolation, it is now possible to change when a
transformation is active (e.g., TRANSMIT).
• For tool radius compensation with variable tool orientation, the transformation from the
tool edge reference point to the tool edge center point can no longer be performed by
means of a simple zero offset. Tools with a relevant tool point direction are therefore not
permitted for 3D peripheral milling (an alarm is output).
Note
The subject is irrelevant with respect to face milling as only defined tool types without
relevant tool point direction are permitted for this operation anyway. (A tool with a type,
which has not been explicitly approved, is treated as a ball end mill with the specified
radius. A tool point direction parameter is ignored).
Tool offsets
8.18 Tools with a relevant cutting edge length
Fundamentals
408 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 409
Special functions 9
9.1 Auxiliary function outputs
Function
The auxiliary function output sends information to the PLC indicating when the NC program
needs the PLC to perform specific switching operations on the machine tool. The auxiliary
functions are output, together with their parameters, to the PLC interface. The values and
signals must be processed by the PLC user program.
Function outputs
The following functions can be downloaded to the programmable controller:
• Select tool T
• Tool compensation D,DL
• Feed F/FA
• Spindle speed S
• H functions
• M functions
For the above-mentioned functions it is possible to define whether they are to be transferred
during the machining sequence, and which reactions are to be activated.
For each function group or individual function, machine data define whether the output is
initiated
• Before the traversing movement,
• With the traversing movement, or
• After the traversing movement
.
The PLC can be programmed to acknowledge auxiliary function outputs in various ways.
Special functions
9.1 Auxiliary function outputs
Fundamentals
410 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Programming
Letter[address extension]=Value
The letters, which can be used for auxiliary functions, are:
M
Or
S
Or
H
Or
T
Or
D
Or
DL
Or
F
Parameters
In the following table you will find information about the meaning and value ranges for the
address extension and the value in auxiliary function outputs. The maximum number of
auxiliary functions of the same type per block is also specified.
Overview of auxiliary functions, programming
Functi
on
Address extension
(integer)
Value Explanation Number
per
block
Meaning Area Area Type Meaning
- implicit
0
0 - 99 INT Function The address extension is
0 for the value range
between 00 and 99. M0,
M1, M2, M17, M30 must
be used without an
address extension.
5
Spindle
no.
1 - 12 1 - 99 Function M3, M4, M5, M19, M70
with address extension
spindle no., e.g., M5 for
spindle 2: M2=5. Master
spindle is used if no
spindle is specified.
M
Any 0 - 99 100- (max.
INT value)
Function User M function
S Spindle
no.
1 - 12 0-±3.4028
ex 38
REAL Spindle
speed
Without spindle no. for
master spindle
3
Special functions
9.1 Auxiliary function outputs
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 411
H Any 0 - 99 ±(max.
INT value)
±3.4028
ex 38
INT
REAL
Any Functions have no effect
in the NCK; only to be
implemented on the PLC
3
T Spindle
no.
(for active
tool
manage
ment)
1 - 12 0 - 32000
(or tool
names
with active
tool
managem
ent)
INT Tool
selection
Tool names are not
passed to the PLC
interface.
1
D 0 - 9 INT Tool offset
selection
D0 selection,
default D1
1
DL Location-
depende
nt offset
1 - 6 ±3.4028
ex 38
REAL See tool fine
offset
selection
/FBW/
Refers to previously
selected D number
1
F Path
feedrate
0 0.001 -
999
999,999
Path
feedrates
(FA) Axis No. 1 - 31 0.001 -
999
999,999
REAL
Axis
feedrates
6
The highest number for a type specified in the table must not be exceeded.
Example
M=QU(…)
H=QU(…)
N10 H=QU(735) ;High-speed output for H735
N10 G1 F300 X10 Y20 G64
N20 X8 Y90 M=QU(7)
M7 was programmed as a high-speed output, so continuous-path mode (G64) is not
interrupted.
Note
You should only use this function in individual cases, because it can affect the time
synchronization as a result of interaction with other function outputs.
Special functions
9.1 Auxiliary function outputs
Fundamentals
412 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Description
Number of function outputs per NC block
Up to 10 function outputs can be programmed in one NC block. Auxiliary functions can also
be output from the action component of synchronized actions. See /FBSY/.
Grouping
The functions described can be grouped together. Group assignment is predefined for some
M commands. The acknowledgment behavior can be defined by the grouping.
Acknowledgements, high-speed function outputs, QU
Functions, which have not been programmed as high-speed outputs, can be defined as high-
speed outputs for individual outputs with the keyword QU. Program execution continues
without waiting for the acknowledgment of the miscellaneous function (the program waits for
the transport acknowledgment). This helps avoid unnecessary hold points and interruptions
to traversing movements.
Machine manufacturer
The appropriate MD must be set for "high-speed function outputs", see FB1/Function Manual
Basic Functions; Auxiliary Function Output to PLC (H2).
Function outputs for travel commands
Time is needed to transfer information and wait for a corresponding response, and this has
an impact on the travel movements.
High-speed acknowledgment without block change delay
Block change behavior can be influenced by machine data. When the "without block change
delay" setting is selected, the system response with respect to high-speed auxiliary functions
is as follows:
Auxiliary function
output
Response
Before the movement The block transition between blocks with highspeed auxiliary functions
occurs without interruption and without a reduction in velocity. The
auxiliary function output takes place in the first interpolation cycle of the
block. The following block is executed with no acknowledgment delay.
During the movement The block transition between blocks with highspeed auxiliary functions
occurs without interruption and without a reduction in velocity. The
auxiliary function output takes place during the block. The following block
is executed with no acknowledgment delay.
After the movement The movement stops at the end of the block. The auxiliary function output
takes place at the end of the block. The following block is executed with
no acknowledgment delay.
Special functions
9.1 Auxiliary function outputs
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 413
Caution
Function outputs in continuous-path mode
Function outputs before the traversing movements interrupt continuous-path mode
(G64/G641) and generate an exact stop for the previous block.
Function outputs after the traversing movements interrupt continuous-path mode
(G64/G641) and generate an exact stop for the current block.
Important:A wait for an outstanding acknowledgment signal from the PLC can also cause an
interruption to continuous-path mode, e.g., M instruction sequences in blocks with extremely
short path lengths.
9.1.1 M functions
Function
M functions can trigger, for example, switching operations such as "Coolant ON/OFF" and
other operations on the machine. Permanent functions have already been assigned to some
of the M functions by the control manufacturer (see list of predefined M functions).
Programming
M... Possible values. 0 to 9999 9999 (max. INT value), integer
Parameters
List of predefined M functions
M0* Programmed stop 1
M1* Optional stop
M2* End of main program with return to beginning of program
M30* End of program, same effect as M2
M17* End of subprogram
M3 Spindle clockwise
M4 Spindle counterclockwise
M5 Spindle stop
M6 Tool change (default setting)
M70 Spindle is switched to axis mode
M40 Automatic gear change
M41 Gear stage 1
M42 Gear stage 2
M43 Gear stage 3
M44 Gear stage 4
M45 Gear stage 5
Special functions
9.1 Auxiliary function outputs
Fundamentals
414 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Notice
Extended address notation cannot be used for the functions marked with *.
The commands M0, M1, M2, M17 and M30 are always initiated after the traversing
movement.
Machine manufacturer
All free M function numbers can be assigned by the machine manufacturer, e.g., with
switching functions for controlling clamping fixtures or for activating/deactivating other
machine functions, etc.
See machine manufacturer's specifications.
Example
N10 S...
N20 X... M3 ;M function in the block with axis movement,
;spindle accelerates before the X axis
;movement
N180 M789 M1767 M100 M102 M376 ;Max. of 5 M functions in the block
Predefined M commands
Certain important M functions for program execution are supplied as standard with the
control:
Programmed stop, M0
Machining stops in the NC block with M0. You can now, for example, remove swarf,
remeasure, etc.
Programmed stop 1 - optional stop, M1
M1 can be set with
• HMI/dialog "Program Control" or
• the VDI interface.
Program execution on the NC is stopped at each of the programmed blocks.
Programmed stop 2 - an auxiliary function associated with M1 with stop in program
execution
Programmed halt 2 can be set via HMI/dialog "Program control" and permits technological
processes to be interrupted at any time when the part has finished machining. It therefore
allows the operator to intervene in the production process in order to remove chips, for
example.
Special functions
9.1 Auxiliary function outputs
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 415
End of program, M2, M17, M30
A program is terminated with M2, M17 or M30 and reset to the beginning of the program. If
the main program is called from another program (as a subprogram), M2/M30 has the same
effect as M17 and vice versa, i.e., M17 has the same effect in the main program as M2/M30.
Spindle functions, M3, M4, M5, M19, M70
The extended address notation with spindle number is used for all spindle functions.
Example: M2=3 means CW spindle rotation for the second spindle. If no address extension
is programmed, the function applies to the master spindle.
9.1.2 H functions
Function
H functions are used to transfer information to the PLC (programmable logic controller), in
order to activate specific switching operations. H functions are REAL values.
Up to three H functions can be programmed in one NC block.
Machine manufacturer
The meaning of the functions is determined by the manufacturer.
Programming
N10 G0 X20 Y50 H3=–11.3
Special functions
9.1 Auxiliary function outputs
Fundamentals
416 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 417
Arithmetic Parameters and Program Jumps 10
10.1 Arithmetic parameter (R)
Function
The arithmetic parameters are used, for example, if an NC program is not only to be valid for
values assigned once, or if you need to calculate values. The required values can be set or
calculated by the control during program execution. Another possibility consists of setting the
arithmetic parameter values by operator inputs. If values have been assigned to the
arithmetic parameters, they can be assigned to other variable-setting NC addresses in the
program.
Programming
Rn=...
Parameters
R Arithmetic variables
n Number of the arithmetic parameter, n= 0 to max. See machine data or
machine manufacturer for max.; default setting: max = 0-99
Range of values ±(0.000 0001 ... 9999 9999) (8 decimal places and leading sign and
decimal point) can be assigned to the arithmetic parameters.
Machine manufacturer
The number of R parameters is set in the machine data, or see specifications of machine
manufacturer.
Example of R parameters
N10 R1= R1+1 ;The new R1 is calculated from the
;old R1 plus 1
N20 R1=R2+R3 R4=R5-R6 R7=R8* R9 R10=R11/R12
N30 R13=SIN(25.3) ;R13 equals sine of 25.3 degrees
N40 R14=R1*R2+R3 ;Multiplication or division takes precedence
over addition or subtraction
;R14=(R1*R2)+R3
N50 R14=R3+R2*R1 ;Result, the same as block N40
N60 R15=SQRT(R1*R1+R2*R2) ;Meaning: R15=square root of ;R12+R22
Arithmetic Parameters and Program Jumps
10.1 Arithmetic parameter (R)
Fundamentals
418 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example of assignment of axis values
N10 G1 G91 X=R1 Z=R2 F300
N20 Z=R3
N30 X=-R4
N40 Z=-R5
...
Value assignment
You can assign values in the following range to the arithmetic parameters:
±(0.000 0001 ... 9999 9999) (8 decimal places and sign and decimal point)
• The decimal point can be omitted for integer values.
• A plus sign can always be omitted.
Example:
R0=3.5678 R1=-37.3 R2=2 R3=-7
R4=-45678.1234
It is possible to assign an extended numerical range by using exponential notation:
Example:
± (10-300 ... 10+300)
The value of the exponent is written after the EX characters; maximum total number of
characters: 10 (including signs and decimal point)
Range of values for EX: -300 to +300
Example:
R0=-0.1EX-5 ;Meaning: R0 = -0.000 001
R1=1.874EX8 ;Meaning: R1 = 187 400 000
Note
There can be several assignments in one block incl. assignments of arithmetic expressions.
Value assignment must be in a separate block.
Assignments to other addresses
The flexibility of an NC program comes down to being able to assign these arithmetic
parameters or expressions with arithmetic parameters to other NC addresses. Values,
arithmetic expressions and arithmetic parameters can be assigned to all addresses;
Exception: addresses N, G, and L.
Arithmetic Parameters and Program Jumps
10.2 Unconditional program jumps
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 419
When assigning, write the character " = " after the address character. It is also possible to
have an assignment with a minus sign. A separate block is required for assignments to axis
addresses (traversing instructions).
Example:
N10 G0 X=R2 ;Assignment to the X axis
Arithmetic operations and functions
When operators/arithmetic functions are used, it is necessary to use conventional
mathematical notation. Machining priorities are set by parentheses. Otherwise, multiplication
and division take precedence over addition and subtraction. Degrees are used for the
trigonometrical functions.
10.2 Unconditional program jumps
Function
By default, main programs, subprograms, cycles and interrupt routines execute the blocks in
the sequence in which they were programmed. Program jumps can be used to modify this
sequence.
Programming
GOTOB <destination>
GOTOF <destination>
GOTO/GOTOC <destination variable>
Parameter
GOTOB "Jump instruction" with backward jump destination (towards beginning
of program)
GOTOF Jump instruction with forward jump destination (towards end of
program)
GOTO Jump instruction with forward, then backward destination search (first
towards end of program and then towards beginning of program)
GOTOC Suppress Alarm 14080 "Branch destination not found". Jump instruction
with forward, then backward destination search (first towards end of
program and then towards beginning of program)
<destination> Branch destination parameters for label, block number, or string
variable
Label Destination for a jump instruction
Label: Labeling of branch destination within the program
Block number Branch destination as main block or subblock number (e.g., 200, N300)
String variable Variable of type string containing a label or block number
Arithmetic Parameters and Program Jumps
10.2 Unconditional program jumps
Fundamentals
420 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example
Axis U: Pallet storage, transporting the pallet to the working area
Axis V: Transfer line to a measuring station, where sampling controls are carried out:
N10 …
N20 GOTOF LABEL_0 ;Jump forward to LABEL_0
N30 …
N40 LABEL_1: R1=R2+R3 ;Branch destination LABEL_1
N50 …
N60 LABEL_0: ;Branch destination LABEL_0
N70 …
N80 GOTOB LABEL_1 ;Jump backwards to LABEL_1
N90 …
Description
Jump destinations with user-defined names can be programmed in a routine. The command
GOTOF or GOTOB can be used to branch to a jump destination from any other point within
the same program. The program then resumes execution at the instruction immediately
following the jump destination.
Destination not found
If the destination is not found, program execution is terminated with Alarm 14080
"Destination not found". Command GOTOC suppresses this alarm. Program execution is
resumed at the line following the GOTOC command.
Destination backward
Jump with label
Label_1: ;destination
....
GOTOB Label_1
Jump forward
Jump with block number
GOTOF N100
....
N100 ;destination
Arithmetic Parameters and Program Jumps
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 421
Indirect jumps
Jump to block number
N5 R10=100
N10 GOTOF "N"<<R10 ;jump to block whose number is in R10
N90
N100 ;destination
N110
Jump to labels
DEF STRING[20] DESTINATION
DESTINATION = "label2" ;jump with variable jump destination
GOTOF DESTINATION
Label1: T="Drill1"
....
Label2: T="drill2" ;destination
Further information
The unconditional jump must be programmed in a separate block.
• In programs with unconditional jumps, the end of program M2/M30
does not have to appear at the end of the program.
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC)
Function
Jump conditions can be formulated using IF statements. The jump to the programmed jump
destination is only performed if the jump condition is fulfilled.
Programming
IF expression GOTOB <destination>
Or
IF expression GOTOF <destination>
Or
IF expression GOTO/GOTOC <destination
Arithmetic Parameters and Program Jumps
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC)
Fundamentals
422 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Parameters
IF Keyword for condition
GOTOB "Jump statement" with backward jump destination (towards beginning of
program)
GOTOF Jump statement with forward jump destination (toward program end)
GOTO Jump statement with destination search first forward then backward
(first toward end of program and then toward beginning of program)
GOTOC Suppress Alarm 14080 "Destination not found". Jump instruction with
destination search first forward then backward (first toward end of
program and then toward beginning of program)
<destination> Branch destination parameters for label, block number, or string
variable
Label Destination for a jump command
Label: Labeling of destination within the program
Block number Jump destination as main block or subblock number (e.g., 200, N300)
String variable Variable of type string containing a label or block number
Comparison and logical operands
The jump condition can be programmed with any comparison or logic operation (result:
TRUE or FALSE). The program jump is executed if the result of the operation is TRUE.
The jump destination can only be a block with a label or block number that appears within
the program.
Note
Several conditional jumps can be formulated in the same block.
== Equal to
<> Not equal to
> Greater than
< Less than
>= Greater than or equal to
<= Less than or equal to
Note
For more information, see
/PGA/Programming Manual Advanced; "Flexible NC Programming".
Arithmetic Parameters and Program Jumps
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC)
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 423
Example
N40 R1=30 R2=60 R3=10 R4=11 R5=50 R6=20 ;Assignment of initial values
N41 MA1: G0 X=R2*COS(R1)+R5 ->
-> Y=R2*SIN(R1)+R6
;Calculation and assignment to ;axis
address
N42 R1=R1+R3 R4=R4-1 ;Specification of variable
N43 IF R4>0 GOTOB MA1 ;Jump statement with label
N44 M30 ;End of program
Arithmetic Parameters and Program Jumps
10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC)
Fundamentals
424 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 425
Program section repetition 11
11.1 Program section repetition
Function
Program section repetition allows you to repeat existing program sections within a program
in any order. The block or program sections to be repeated are identified by labels.
For more information on labels, please see:
Fundamentals of NC Programming, "Language Elements of Programming Language"
References: /PGA/Job Planning Programming Manual; Flexible NC Programming,
"CASE Statement" and "Control Structures"
Programming repeat block
LABEL: xxx
yyy
REPEATB LABEL P=n
Zzz
The program line identified by a label is repeated P=n times. If P is not specified, the
program section is repeated exactly once. After the last repetition, the program is continued
at the line zzz following the REPEATB line.
The block identified by the label can appear before or after the REPEATB statement. The
search initially commences toward the start of the program. If the label is not found in this
direction, the search continues toward the end of the program.
Programming repeat area starting at label
LABEL: xxx
yyy
REPEAT LABEL P=n
zzz
The program section between the label with any name and the REPEAT statement is
repeated P=n times. If the block with the label contains further statements, these are
executed again on each repetition. If P is not specified, the program section is repeated
exactly once. After the last repetition, the program is continued at the line zzz following the
REPEAT line.
Program section repetition
11.1 Program section repetition
Fundamentals
426 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Note
The label must appear before the REPEAT statement. The search is performed toward the
start of the program only.
Programming repeat area between two labels
START_LABEL: xxx
ooo
END_LABEL: yyy
ppp
REPEAT START_LABEL END_LABEL P=n
zzz
The area between the two labels is repeated P=n times. User-defined names can be
assigned to the labels. The first line of the repetition contains the start label, the last line
contains the end label. If the line containing the start or end label contains further
statements, these are executed again on each run. If P is not specified, the program section
is repeated once. After the last repetition, the program is continued at the line zzz following
the REPEAT line.
Note
The program section to be repeated can appear before or after the REPEAT statement. The
search initially commences toward the start of the program. If the start label is not found in
this direction, the search resumes from the REPEAT statement toward the end of the
program.
It is not possible to nest the REPEAT statement with the two labels within parentheses. If the
start label is found before the REPEAT statement and the end label is not reached before
the REPEAT statement, the repetition is performed on the section between the start label
and the REPEAT statement.
Programming repeat an area between a label and the end label
LABEL: xxx
ooo
ENDLABEL: yyy
REPEAT LABEL P=n
zzz
ENDLABEL is a predefined label with a fixed name. ENDLABEL marks the end of a program
section and can be used multiple times in the program. The block marked by ENDLABEL
can contain further statements.
Program section repetition
11.1 Program section repetition
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 427
The area between a label and the following ENDLABEL is repeated P=n times. Any name
can be used to define the start label. If the block with the start label or ENDLABEL contains
further statements, these are executed on each repetition.
Note
If no ENDLABEL is found between the start label and the block with the REPEAT call, the
loop ends before the REPEAT line. The construct therefore has the same effect as described
above in "repeat area from label".
If P is not specified, the program section is repeated once.
After the last repetition, the program is continued at the line zzz following the REPEAT line.
Parameters
LABEL: Jump destination; the name of the jump destination is followed by a
colon
REPEAT Repeat (repeat several lines)
REPEATB Repeat block (repeat one line only)
Example of repetition of positions
N10 POSITION1: X10 Y20
N20 POSITION2: CYCLE(0,,9,8) ;Position cycle
N30 ...
N40 REPEATB POSITION1 P=5 ;Execute BLOCK N10 five times
N50 REPEATB POSITION2 ;Execute block N20 once
N60 ...
N70 M30
Example 5 squares with increasing width are to be produced
N5 R10=15
N10 Begin: R10=R10+1 ;Width
N20 Z=10-R10
N30 G1 X=R10 F200
N40 Y=R10
N50 X=-R10
N60 Y=-R10
N70 Z=10+R10
N80 REPEAT BEGIN P=4 ;Execute area from N10 to N70 four times
N90 Z10
N100 M30
Program section repetition
11.1 Program section repetition
Fundamentals
428 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example repeat program section from BEGIN to END
N5 R10=15
N10 Begin: R10=R10+1 ;Width
N20 Z=10-R10
N30 G1 X=R10 F200
N40 Y=R10
N50 X=-R10
N60 Y=-R10
N70 END:Z=10
N80 Z10
N90 CYCLE(10,20,30)
N100 REPEAT BEGIN END P=3 ;Execute area from N10 to N70 three times
N110 Z10
N120 M30
Example of ENDLABEL
N10 G1 F300 Z-10
N20 BEGIN1:
N30 X10
N40 Y10
N50 BEGIN2:
N60 X20
N70 Y30
N80 ENDLABEL: Z10
N90 X0 Y0 Z0
N100 Z-10
N110 BEGIN3: X20
N120 Y30
N130 REPEAT BEGIN3 P=3 ;Execute area from N110 to N120 three times
N140 REPEAT BEGIN2 P=2 ;Execute area from N50 to N80 twice
N150 M100
N160 REPEAT BEGIN1 P=2 ;Execute area from N20 to N80 twice
N170 Z10
N180 X0 Y0
N190 M30
Example of milling: Machine drill position with different technologies
N10 CENTER DRILL() ;Load center drill
N20 POS_1: ;Drilling positions 1
N30 X1 Y1
N40 X2
N50 Y2
N60 X3 Y3
N70 ENDLABEL:
N80 POS_2: ;Drilling positions 2
N90 X10 Y5
N100 X9 Y-5
Program section repetition
11.1 Program section repetition
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 429
N110 X3 Y3
N120 ENDLABEL:
N130 DRILL() ;Change drill and drilling cycle
N140 THREAD(6) ;Load tap M6 and ;threading cycle
N150 REPEAT POS_1 ;Repeat program section once from ;POS_1
up to ENDLABEL
N160 DRILL() ;Change drill and drilling cycle
N170 THREAD(8) ;Load tap M8 and ;threading cycle
N180 REPEAT POS_2 ;Repeat program section once from ;POS_2
up to ENDLABEL
N190 M30
Supplementary conditions
• Program section repetitions can be nested. Each call uses a subprogram level.
• If M17 or RET is programmed during processing of a program section repetition, the
repetition is aborted. The program is resumed at the block following the REPEAT line.
• In the actual program display, the program section repetition is displayed as a separate
subprogram level.
• If the level is canceled during the program section repetition, the program resumes at the
point after the program section repetition call.
Example:
N5 R10=15
N10 Begin: R10=R10+1 ;Width
N20 Z=10-R10
N30 G1 X=R10 F200
N40 Y=R10 ;Level cancellation
N50 X=-R10
N60 Y=-R10
N70 END: Z10
N80 Z10
N90 CYCLE(10,20,30)
N100 REPEAT BEGIN END P=3
N120 Z10 ;Resume program processing
N130 M30
• Control structures and program section repetitions can be used in combination. There
should be no overlap between the two, however. A program section repetition should
appear within a control structure branch or a control structure should appear within a
program section repetition.
• If jumps and program section repetitions are mixed, the blocks are executed purely
sequentially. For example, if a jump is performed from a program section repetition,
processing continues until the programmed end of the program section is found.
Program section repetition
11.1 Program section repetition
Fundamentals
430 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Example:
N10 G1 F300 Z-10
N20 BEGIN1:
N30 X=10
N40 Y=10
N50 GOTOF BEGIN2
N60 ENDLABEL:
N70 BEGIN2:
N80 X20
N90 Y30
N100 ENDLABEL: Z10
N110 X0 Y0 Z0
N120 Z-10
N130 REPEAT BEGIN1 P=2
N140 Z10
N150 X0 Y0
N160 M30
Note
Program section repetition is activated by programming.
The REPEAT instruction should be placed behind the traveling blocks.
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 431
Tables 12
12.1 List of statements
Legend:
1 Default setting at beginning of program (factory settings of the control, if nothing else programmed)
2 The groups are numbered according to the table in section "List of G functions/preparatory functions".
3 Absolute end points: modal (m);
incremental end points: non-modal (n);
otherwise: modal/non-modal depending on syntax of G function
4 As circle center points, IPO parameters act incrementally. They can be programmed in absolute mode with AC. The
address modification is ignored when the parameters have other meanings (e.g., thread pitch).
5 The keyword is not valid for SINUMERIK 810D.
5 The keyword is not valid for SINUMERIK 810D/NCU571.
7 The keyword is not valid for SINUMERIK FM-NC.
8 The OEM can add two extra interpolation types. The names can be changed by the OEM.
9 Extended address notation cannot be used for these functions.
Name Meaning Value Description,
comment
Syntax m/s3Group 2
: Block number - main
block (see N)
0 ...
99 999 999
integers only,
without signs
Special
identification of
blocks, instead
of N... ;this
block should
contain all
statements
required for a
complete
subsequent
machining
section.
e.g.,20
A Axis Real m/n
A2 5 Tool orientation: Euler
angles
Real s
Tables
12.1 List of statements
Fundamentals
432 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
A3 5 Tool orientation: Direction-
vector component
Real s
A4 5 Tool orientation for start of
block
Real s
A5 5 Tool orientation for end of
block:
Normal-vector component
real s
ABS Absolute value real
AC Input of absolute
dimensions
0, ...,
359.9999°
X=AC(100) s
ACC 5 Axial acceleration Real, without
sign
m
ACCLIMA 5 Reduction or overshoot of
maximum axial
acceleration
0, ..., 200 Valid range is
1% to 200%.
ACCLIMA[X]= ...[%] m
ACN Absolute dimensions for
rotary axes, approach
position in negative
direction
A=ACN(...) B=ACN(...)
C=ACN(...)
s
ACOS Arc cosine
(trigon. function)
real
ACP Absolute dimensions for
rotary axes, approach
position in positive
direction
A=ACP(...) B=ACP(...)
C=ACP(...)
s
ADIS Rounding clearance for
path functions G1, G2,
G3, ...
Real, without
sign
m
ADISPOS Rounding clearance for
rapid traverse G0
Real, without
sign
m
ADISPOSA Size of the tolerance
window for IPOBRKA
Integer, real ADISPOSA=... or
ADISPOSA(<axis>[,RE
AL])
m
ALF Angle tilt fast
Integer,
without sign
m
AMIRROR Programmable mirroring
(additive mirror)
AMIRROR X0 Y0
Z0AMIRROR
; separate block
s 3
AND Logical AND
ANG Contour angle real s
AP Angle polar 0, ..., ± 360° m/n
APR Read/display access
protection
(access protection read)
Integer,
without sign
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 433
Name Meaning Value Description,
comment
Syntax m/s3Group 2
APW Write access protection
(access protection write)
Integer,
without sign
AR Opening angle
(angle circular)
0, ..., 360° m/n
AROT Programmable rotation
(additive rotation)
Rotation
about:
1st geometry
axis:
-180°... +180°
2nd geometry
axis:
-90°... +90°
3rd geometry
axis:
-180°... +180°
AROT X... Y... Z...
AROT RPL=
;separate block
s 3
AROTS Programmable frame rotations with solid
angles (additive rotation)
AROTS X... Y...
AROTS Z... X...
AROTS Y... Z...
AROTS RPL=
;separate block
s 3
SL Macro definition String
ASCALE Programmable scaling
(additive scale)
ASCALE X... Y... Z...
;separate block
s 3
ASPLINE Akima spline m 1
ATAN2 Arc tangent 2 real
ATRANS Additive programmable offset
(additive translation)
ATRANS X... Y... Z...
;separate block
s 3
AX Variable axis identifier Real m/n
AXCSWAP Advance container axis AXCSWAP(CTn,
CTn+1,...)
25
AXCTSWE Advance container axis AXCTSWE(CTi) 25
AXIS Data type: Axis identifier Name of file
can be added
AXNAME Converts the input string
to an axis name (get
axname)
String An alarm is
generated if the
input string
does not
contain a valid
axis name.
AXSTRING Converts the spindle-
number string (get string)
String Name of file
can be added
AXSTRING[ SPI(n) ]
AXTOCHAN Request axis for a specific channel.
Possible from NC program and
synchronized action.
AXTOCHAN(axis,
channel number[,axis,
channel number[,…]])
B Axis real m/n
B_AND Bit AND
B_OR Bit OR
B_NOT Bit negation
Tables
12.1 List of statements
Fundamentals
434 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
B_XOR Bit exclusive OR
B2 5 Tool orientation:
Euler angles
Real s
B3 5 Tool orientation:
Direction-vector
component
Real s
B4 5 Tool orientation for start of
block
Real s
B5 5 Tool orientation for end of
block: Normal-vector
component
Real s
BAUTO Definition of first spline segment by the
following 3 points
(begin not a knot)
m 19
BLSYNC Processing of interrupt routine is only to
start with the next block change
BNAT1 Natural transition to first spline block
(begin natural)
m 19
BOOL Data type: Boolean value TRUE/FALSE or
1/0
BOUND Tests whether the value
falls within the defined
value range. If the values
are equal, the test value is
returned.
real Var1 : Varmin
Var2: Varmax
Var3: Varcheck
RetVar =
BRISK1 Fast non-smoothed path acceleration m 21
BRISKA Switch on brisk path acceleration for the
programmed axes
BSPLINE B-spline m 1
BTAN Tangential transition to first spline block
(begin tangential)
m 19
C Axis real m/n
C2 5 Tool orientation: Euler
angles
Real s
C3 5 Tool orientation:
Direction-vector
component
Real s
C4 5 Tool orientation for start of
block
Real s
C5 5 Tool orientation for end of
block; normal vector
component
Real s
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 435
Name Meaning Value Description,
comment
Syntax m/s3Group 2
CAC Absolute approach of position
(coded position: absolute coordinate)
Coded value is
table index;
table value is
approached.
CACN Absolute approach in negative direction of
value stored in table
(coded position absolute negative)
Permissible for
the
programming of
rotary axes as
positioning
axes.
CACP Absolute approach in positive direction of
value stored in table
(coded position absolute positive)
CALCDAT Calculate radius and
center point or circle from
3 or 4 points
(calculate circle data)
VAR Real [3] The points must
be different.
CALL Indirect subprogram call CALL PROGVAR
CALLPATH Programmable search path for
subprogram calls
A path can be
programmed to
the existing
NCK file system
with
CALLPATH.
CALLPATH
(/_N_WKS_DIR/_N_MY
WPD/
subprogram_identifier_
SPF)
CANCEL Cancel modal
synchronized action
INT Cancel
with specified
ID.
Without
parameters:
All modal
synchronized
actions are
deselected.
CASE Conditional program branch
CDC Direct approach of position
(coded position: direct coordinate)
See CAC.
CDOF 1 Collision detection OFF
m 23
CDON Collision detection ON
m 23
CDOF2 Collision detection OFF
For CUT3DC
only
m 23
CFC 1 Constant feed at contour
m 16
Tables
12.1 List of statements
Fundamentals
436 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
CFIN Constant feed at internal radius only, not
at external radius
m 16
CFTCP Constant feed in tool-center- point (center-
point path)
m 16
CHAN Specify validity range for data Once per
channel
CHANDATA Set channel number for
channel data access
INT Only
permissible in
the initialization
module.
CHAR Data type: ASCII
character
0, ..., 255
CHECKSUM Forms the checksum over
a an array as a fixed-
length STRING
Max. length
32
Returns string
of 16 hex digits.
ERROR=
CHECKSUM
CHF
CHR
Chamfer;
value = length of chamfer
Chamfer;
value = width of chamfer
in direction of movement
(chamfer)
Real, w/o
signs
s
CHKDNO Check for unique D numbers
CIC Incremental approach of position
(coded position: incremental coordinate)
See CAC.
CIP Circular interpolation through intermediate
point
CIP X... Y... Z...
I1=... J1=... K1=...
m 1
CLEARM Reset one/several
markers for channel
coordination
INT,
1 - n
Does not
influence
machining in
own channel.
CLRINT Deselect interrupt: INT Parameter:
Interrupt
number
CMIRROR Mirror on a coordinate
axis
FRAME
COARSEA Motion end when "Exact stop coarse"
reached
COARSEA=... or
COARSEA[n]=...
m
COMPOF1,6 Compressor OFF m 30
COMPON6 Compressor ON m 30
COMPCURV Compressor ON: Polynomials with
constant curvature
m 30
COMPCAD Compressor ON: Optimized surface quality
CAD program
m 30
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 437
Name Meaning Value Description,
comment
Syntax m/s3Group 2
CONTDCON Tabular contour decoding ON
CONTPRON Activate contour preparation
(contour preparation ON)
COS Cosine
(trigon. function)
real
COUPDEF Definition ELG
group/synchronous
spindle group
(couple definition)
String Block change
(software)
response:
NOC: no block-
change control
FINE/COARSE:
block change
on
"synchronism
fine/coarse"
IPOSTOP:
block change in
setpoint-
dependent
termination of
overlaid
movement.
COUPDEF(FS, ...)
COUPDEL Delete ELG group (couple delete) COUPDEL(FS,LS)
COUPOF ELG group/synchronous spindle pair OFF
(couple OFF)
COUPOF(FS,LS,
POSFS,POSLS)
COUPOFS Deactivating ELG group/synchronized
spindle pair with stop of following spindle
COUPOFS(FS,LS,POS
FS)
COUPON ELG group/synchronous spindle pair ON
(couple ON)
COUPON(FS,LS,
POSFS)
COUPONC Transfer activation of ELG
group/synchronized spindle pair with
previous programming
COUPONC(FS,LS)
COUPRES Reset ELG group
(couple reset)
Programmed
values invalid;
machine data
values valid.
COUPRES(FS,LS)
CP Path movement (continuous path) m 49
CPRECOF1,6 Programmable contour precision OFF m 39
CPRECON 6 Programmable contour precision ON
m 39
CPROT Channel-specific protection zone ON/OFF
CPROTDEF Channel specific protection area definition
CR Circle radius Real, without
sign
s
CROT Rotation of the current
coordinate system.
FRAME Max. parameter
count: 6
Tables
12.1 List of statements
Fundamentals
438 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
CROTS Programmable frame rotations with solid
angles (rotation in the specified axes)
CROTS X... Y...
CROTS Z... X...
CROTS Y... Z...
CROTS RPL=
;separate block
s
CSCALE Scale factor for multiple
axes.
FRAME Max. parameter
count:
2 * axis
countmax
CSPLINE Cubic spline m 1
CT Circle with tangential transition CT X... Y.... Z... m 1
CTAB Define following axis
position according to
leading axis position from
curve table
real If parameter 4/5
not
programmed:
Standard
scaling
CTABDEF Table definition ON
CTABDEL Clear curve table
CTABEND Table definition OFF
CTABEXISTS Checks the curve table with number n Parameter n
CTABFNO Number of curve tables still possible in the
memory
memType
CTABFPOL Number of polynomials still possible in the
memory
memType
CTABFSEG Number of curve segments still possible in
the memory
memType
CTABID Returns table number of the nth curve
table
parameter n
and memType
CTABINV Define leading axis
position according to
following axis position
from curve table
real See CTAB.
CTABIS
LOCK
Returns the lock state of the curve table
with number n
Parameter n
CTABLOCK Set lock against deletion and overwriting Parameters n,
m, and
memType.
CTABMEMTYP Returns the memory in which curve table
number n is created.
Parameter n
CTABMPOL Max. number of polynomials still possible
in the memory
memType
CTABMSEG Max. number of curve segments still
possible in the memory
memType
CTABNO Number of defined curve tables
irrespective of mem. type
No parameters.
CTABNOMEM Number of defined curve tables in SRAM
or DRAM memory.
memType
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 439
Name Meaning Value Description,
comment
Syntax m/s3Group 2
CTABPERIOD Returns the table periodicity with number n Parameter n
CTABPOL Number of polynomials already used in the
memory
memType
CTABPOLID Number of the curve polynomials used by
the curve table with number n
Parameter n
CTABSEG Number of curve segments already used
in the memory
memType
CTABSEGID Number of the curve segments used by
the curve table with number n
Parameter n
CTABSEV Returns the final value of the following axis
of a segment of the curve table
Segment is
determined by
LW.
R10 = CTABSEV(LW,
n, degree, Faxis, Laxis)
CTABSSV Returns the initial value of the following
axis of a segment of the curve table
Segment is
determined by
LW.
R10 = CTABSSV(LW,
n, degree, Faxis, Laxis)
CTABTEP Returns the value of the leading axis at
curve table end.
Master value at
end of curve
table
R10 = CTABTEP(n,
degree, Laxis)
CTABTEV Returns the value of the the following axis
at curve table end
Following value
at end of curve
table.
R10 = CTABTEV(n,
degree, Faxis)
CTABTMAX Returns the maximum value of the
following axis of the curve table
Following value
of the curve
table.
R10 = CTABTMAX(n,
Faxis)
CTABTMIN Returns the minimum value of the
following axis of the curve table
Following value
of the curve
table.
R10 = CTABTMIN(n,
Faxis)
CTABTSP Returns the value of the leading axis at
curve table start
Master value at
start of curve
table.
R10 = CTABTSP(n,
degree, Laxis)
CTABTSV Returns the value of the following axis at
curve table start
Following value
at start of curve
table.
R10 = CTABTSV(n,
degree, Faxis)
CTABUNLOCK Cancel locking against deletion and
overwriting
Parameters n,
m, and
memType
CTRANS Zero offset for multiple
axes
FRAME Max. 8 axes.
CUT2D 1 2D cutter compensation type 2-
dimensional
m 22
CUT2DF 2D cutter compensation type 2-
dimensional frame. The cutter
compensation acts relative to the current
frame (inclined plane).
m 22
CUT3DC 5 3D cutter compensation type 3-
dimensional circumference milling
m 22
CUT3DCC 5 3D cutter compensation type 3-
dimensional circumference milling with
limitation surfaces
m 22
Tables
12.1 List of statements
Fundamentals
440 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
CUT3DCCD 5 3D cutter compensation type 3-
dimensional circumference milling with
limitation surfaces with differential tool
m 22
CUT3DF 5 3D cutter compensation type 3-
dimensional face milling
m 22
CUT3DFF 5 3D cutter compensation type 3-
dimensional face milling with constant tool
orientation dependent on the current frame
m 22
CUT3DFS 5 3D cutter compensation type 3-
dimensional face milling with constant tool
orientation independent of the current
frame
m 22
CUTCONOF1 Constant radius compensation OFF m 40
CUTCONON Constant radius compensation ON m 40
D Tool offset number 1, ..., 32 000 Contains
offset data for a
particular tool
T...
; D0 → offset
values for a tool
D...
DAC Absolute, non-modal,
axis-specific diameter
programming
Diameter
programming
DAC(50) s
DC Absolute dimensions for
rotary axes, approach
position directly
A=DC(...) B=DC(...)
C=DC(...)
SPOS=DC(...)
s
DEF Variable definition Integer,
without sign
DEFAULT Branch in CASE branch Jump to if
expression
does not fulfill
any of the
specified
values.
DELAYFSTON Define start of a stop delay range
(DELAY feed stop ON)
Implied if
G331/G332
active.
m
DELAYFSTOF Define end of a stop delay range (DELAY
feed stop OFF)
m
DELDTG Delete distance-to-go
DELETE Delete the specified file. The file name can
be specified with path and file identifier.
Can delete all
files.
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 441
Name Meaning Value Description,
comment
Syntax m/s3Group 2
DELT Delete tool Duplo number
can be omitted.
DIACYCOFA Axis-specific, modal diametral
programming: OFF in cycles
Radius
programming,
last active
G code
DIACYCOFA[axis] m
DIAM90 Diameter programming for G90, radius
programming for G91
m 29
DIAM90A Axis-specific, modal diameter
programming for G90 and AC, radius
programming for G91 and IC
m
DIAMCHAN Acceptance of all axes from MD axis
functions in diameter-programming
channel status
Accept
diameter
programming
from MD.
DIAMCHAN
DIAMCHANA Acceptance of the diameter-programming
channel status
Channel status DIAMCHANA[axis]
DIAMCYCOF Radius programming for G90/G91: ON.
The G code of this group that was last
active remains active for display
Radius
programming,
last active
G code
m 29
DIAMOF1 Diameter programming: OFF
(Diameter programming OFF)
For default setting, see machine
manufacturer.
Radius
programming
for G90/G91
m 29
DIAMOFA Axis-specific, modal diameter
programming: ON
For default setting, see machine
manufacturer.
Radius progr.
for G90/G91
and AC, IC.
DIAMOFA[axis] m
DIAMON Diameter programming: ON
(Diameter programming ON)
Diameter
programming
for G90/G91.
m 29
DIAMONA Axis-specific, modal diameter
programming: ON
For activation, see machine manufacturer.
Diameter
programming
for G90/G91
and AC, IC.
DIAMONA[axis] m
DIC Relative, non-modal, axis-specific
diameter programming
Diameter
programming.
DIC(50) s
DILF Length for lift fast m
DISABLE Interrupt OFF
DISC Transition circle overshoot
- radius compensation
0, ..., 100 m
DISPLOF Suppress current block display
(display OFF)
DISPR Distance for repositioning Real, without
sign
s
Tables
12.1 List of statements
Fundamentals
442 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
DISR Distance for repositioning Real, without
sign
s
DITE Thread run-out path Real m
DITS Thread run-in path Real m
DIV Integer division
DL Total tool offset INT m
DRFOF Deactivate the handwheel offsets (DRF) m
DRIVE7, 9 Velocity-dependent path acceleration m 21
DRIVEA Switch on bent acceleration characteristic
curve for the programmed axes
DYNFINISH Dynamic for smooth-finishing DYNFINISH G1 X10
Y20 Z30 F1000
m 59
DYNNORM Standard dynamic, as previously DYNNORM G1 X10 m 59
DYNPOS Dynamics for positioning mode, tapping DYNPOS G1 X10 Y20
Z30 F...
m 59
DYNROUGH Dynamic for roughing DYNROUGH G1 X10
Y20 Z30 F10000
m 59
DYNSEMIFIN Dynamic for finishing
Technology
G group
DYNSEMIFIN G1 X10
Y20 Z30 F2000
m 59
EAUTO Definition of last spline segment by the last
3 points
(end not a knot)
m 20
EGDEF Definition of an electronic gear
(electronic gear define)
For 1 following
axis with
up to 5 leading
axes
EGDEL Delete coupling definition for the following
axis
(electronic gear delete)
Stops the
preprocessing.
EGOFC Switch off electronic gear continuously
(electronic gear OFF continuous)
EGOFS Switch off electronic gear selectively
(electronic gear OFF selective)
EGON Switch on electronic gear
(Electronic gear ON)
Without
synchronization
.
EGONSYN Switch on electronic gear
(electronic gear ON synchronized)
With
synchronization
.
EGONSYNE Switch on electronic gear, stating
approach mode
(electronic gear ON synchronized)
With
synchronization
.
ELSE Program branch, if IF condition not fulfilled
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 443
Name Meaning Value Description,
comment
Syntax m/s3Group 2
ENABLE Interrupt ON
ENAT 1, 7 Natural transition to next traversing block
(end natural)
m 20
ENDFOR End line of FOR counter loop
ENDIF End line of IF branch
ENDLOOP End line of endless program loop LOOP
ENDPROC End line of program with start line PROC
ENDWHILE End line of WHILE loop
ETAN Tangential transition to next traversing
block at spline end (end tangential)
m 20
EVERY Execute synchronized action if condition
changes from FALSE to TRUE
EXECSTRING Transfer of a string variable with the part
program line to run
Indirect part
program line
EXECSTRING(MFCT1
<< M4711)
EXECTAB Execute an element from a motion table
(execute table)
EXECUTE Program execution ON Return from the
reference-point
edit mode or
after building a
protection area
to normal
program
processing.
EXP Exponential function (ex) real
EXTCALL Execute external subprogram Reload program
from HMI in
"Execution from
external
source" mode.
EXTERN Broadcast a subprogram with parameter
passing
F Feed value
(in conjunction with G4
the dwell time is also
programmed in F)
0.001, ...,
99999.999
Path veloc.
of a
tool/workpiece;
unit: mm/min or
mm/revolution
depending on
G94 or G95
F=100 G1 ...
Tables
12.1 List of statements
Fundamentals
444 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
FA Axial feed
(feed axial)
0.001, ...,
999999.999
mm/min,
degrees/min;
0.001, ...,
39999.9999
inch/min
FA[X]=100 m
FAD Infeed feed for smooth
approach and retraction
(feed approach/depart)
Real, without
sign
FALSE Logical constant: Incorrect BOOL Can be
replaced with
integer constant
0.
FCTDEF Define polynomial function Is evaluated in
SYNFCT or
PUTFTOCF.
FCUB 6 Feedrate variable according to cubic spline
(feed cubic)
Acts on feed
with G93 and
G94.
m 37
FD Path feed for handwheel
override
(feed DRF)
Real, w/o
signs
s
FDA Axial feed for handwheel
override
(feed DRF axial)
Real, w/o
signs
s
FENDNORM Corner deceleration OFF m 57
FFWOF 1 Feedforward control OFF (feed forward
OFF)
m 24
FFWON Feedforward control ON (feed forward ON) m 24
FGREF Reference radius of rotary axis or path
reference factors of orientation axes
(vector interpolation)
Reference size
effective value
m
FGROUP Definition of axis/axes with path feed F applies to all
axes specified
under
FGROUP.
FGROUP (axis1,
[axis2], ...)
FIFOCTRL Control of preprocessing buffer m 4
FIFOLEN Programmable preprocessing depth
FILEDATE Delivers date when file
was last accessed and
written.
STRING,
length 8
Format is
"dd.mm.yy".
FILEINFO Delivers sum of
FILEDATE, FILESIZE,
FILESTAT and FILETIME
STRING,
length 32
Format "rwxsd
nnnnnnnn dd.
hh:mm:ss"
FILESIZE Delivers current file size Type: INT In BYTES.
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 445
Name Meaning Value Description,
comment
Syntax m/s3Group 2
FILESTAT Delivers file status of
rights for read, write,
execute, display, delete
(rwxsd).
STRING,
length 5
Format is
"rwxsd".
FILETIME Delivers time when file
was last accessed and
written
STRING,
length 8
Format is
"dd:mm:yy".
FINEA Motion end when "Exact stop fine"
reached
FINEA=... or
FINEA[n]=...
m
FL Speed limit for
synchronized axes
(feed limit)
Real, without
sign
The unit set
with G93, G94,
G95 is
applicable
(max. rapid
traverse).
FL[axis] =… m
FLIN 6 Feed linear variable (feed linear) Acts on feed
with G93 and
G94.
m 37
FMA Feed multiple axial
Real, without
sign
m
FNORM 1,6 Feed normal to DIN 66025
m 37
FOCOF Deactivate travel with limited
moment/force
m
FOCON Activate travel with limited moment/force m
FOR Counter loop with fixed number of passes
FP Fixed point: Number of
fixed point to be
approached
Integer,
without sign
G75 FP=1 s
FPO Feed characteristic
programmed via a
polynomial
(feed polynomial)
real Quadratic,
cubic
polynomial
coefficient
FPR Identification for rotary
axis
0.001, ...,
999999.999
FPR (rotary axis)
FPRAOF Deactivate revolutional
feedrate
FPRAON Activate revolutional
feedrate
Tables
12.1 List of statements
Fundamentals
446 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
FRAME Data type to define the coordinate system Contains for
each geometry
axis:
Offset, rotation,
angle of shear,
scaling,
mirroring;
For each
special axis:
offset, scaling,
mirroring
FRC Feed for radius and
chamfer
s
FRCM Feed for radius and
chamfer, modal
m
FTOC Change fine tool offset As a function of
a 3rd-order
polynomial
defined with
FCTDEF.
FTOCOF 1,6 Online fine tool offset OFF m 33
FTOCON 6 Online fine tool offset ON m 33
FXS Travel to fixed stop ON Integer,
without sign
1 = select,
0 = deselect
m
FXST Torque limit for travel to
fixed stop
(fixed stop torque)
% parameter
optional
m
FXSW Monitoring window for
travel to fixed stop
(fixed stop window)
mm, inch or
degrees
parameter
optional
G G function (preparatory
function)
The G functions are
divided into G groups.
Only one G function of a
group can be
programmed in a block.
A G function can be either
modal (until it is canceled
by another function of the
same group) or only
effective for the block in
which it is programmed
(non-modal).
Only
specified,
integer values
G...
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 447
Name Meaning Value Description,
comment
Syntax m/s3Group 2
G0 Linear interpolation with rapid traverse
(rapid traverse motion)
G0 X... Z... m 1
G1 1 Linear interpolation with feedrate (linear
interpolation)
G1 X... Z... F... m 1
G2 Circular interpolation clockwise G2 X... Z... I... K... F...
;Center point and end
point
G2 X... Z... CR=... F...
;radius and end point
G2 AR=... I... K... F...
;opening angle and
;center point
G2 AR=... X... Z... F.
;opening angle and
;end point
m 1
G3 Circular interpolation counter-clockwise
Motion
commands
G3 ...; otherwise as for
G2
m 1
G4 Dwell time preset Special motion G4 F... ; dwell time in
seconds
or
G4 S... ; dwell time in
spindle revolutions.
; separate block
s 2
G5 Oblique plunge-cut grinding Oblique plunge-
cutting
s 2
G7 Compensatory motion during oblique
plunge-cut grinding
Start position s 2
G9 Exact stop - deceleration s 11
G17 1 Selection of working plane X/Y Infeed direction
Z
m 6
G18 Selection of working plane Z/X Infeed direction
Y
m 6
G19 Selection of working plane Y/Z Infeed direction
X
m 6
G25 Lower working area limitation G25 X... Y... Z...
;separate block
s 3
G26 Upper working area limitation
Value
assignment in
channel axes. G26 X... Y... Z...
;separate block
s 3
G33 Thread interpolation with
constant pitch
0.001, ...,
2000.00
mm/rev
Motion
command
G33 Z... K... SF=...
; cylindrical thread
G33 X... I... SF=...
; face thread
G33 Z... X... K... SF=...
; taper thread
(path longer in Z axis
than in X axis)
G33 Z... X... I... SF=...
; taper thread
(path longer in X axis
than in Z axis)
m 1
Tables
12.1 List of statements
Fundamentals
448 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
G34 Linear progressive speed change
[mm/rev2]
Motion
command
G34 X... Y... Z... I... J...
K... F...
m 1
G35 Linear degressive speed change [mm/rev2] Motion
command
G35 X... Y... Z... I... J...
K... F...
m 1
G40 1 Tool radius compensation OFF m 7
G41 Tool radius compensation left of contour m 7
G42 Tool radius compensation right of contour m 7
G53 Suppression of current zero offset (non-
modal)
Incl.
programmed
offsets
s 9
G54 1st settable zero offset m 8
G55 2. Settable work offset m 8
G56 3. Settable work offset m 8
G57 4. Settable work offset m 8
G58 Axial programmable zero offset, absolute s 3
G59 Axial programmable zero offset, additive s 3
G60 1 Exact stop - deceleration m 10
G62 Corner deceleration at inside corners
when tool radius offset is active (G41,
G42)
Together with
continuous-path
mode only
G62 Z... G1 m 57
G63 Tapping with compensating chuck G63 Z... G1 s 2
G64 Exact stop - continuous-path mode m 10
G70 Dimension in inches (lengths) m 13
G71 1 Metric dimension (lengths) m 13
G74 Reference point approach G74 X... Z...
;separate block
s 2
G75 Fixed point approach Machine axes G75 FP=.. X1=... Z1=...
;separate block
s 2
G90 1 Absolute dimensions G90 X... Y... Z...(...)
Y=AC(...) or
X=AC Z=AC(...)
m
n
14
G91 Incremental dimension input G91 X... Y... Z... or
X=IC(...) Y=IC(...)
Z=IC(...)
m
n
14
G93 Inverse-time feedrate 1/rpm Execution of a
block: Time
G93 G01 X... F... m 15
G94 1 Linear feedrate F in mm/min or inch/min
and °/min
m 15
G95 Revolutional feedrate F in mm/rev or
inches/rev
m 15
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 449
Name Meaning Value Description,
comment
Syntax m/s3Group 2
G96 Constant cutting speed (as for G95) ON G96 S... LIMS=... F... m 15
G97 Constant cutting speed (as for G95) OFF m 15
G110 Pole programming relative to the last
programmed setpoint position
G110 X... Y... Z... s 3
G111 Polar programming relative to origin of
current workpiece coordinate system
G110 X... Y... Z... s 3
G112 Pole programming relative to the last valid
pole
G110 X... Y... Z... s 3
G140 1 SAR approach direction defined by
G41/G42
m 43
G141 SAR approach direction to left of contour m 43
G142 SAR approach direction to right of contour m 43
G143 SAR approach direction tangent-
dependent
m 43
G147 Soft approach with straight line s 2
G148 Soft retraction with straight line s 2
G153 Suppress current frames including base
frame
Incl. system
frame.
s 9
G247 Soft approach with quadrant s 2
G248 Soft retraction with quadrant s 2
G290 Switch to SINUMERIK mode ON m 47
G291 Switch to ISO2/3 mode ON m 47
G331 Tapping m 1
G332 Retraction (tapping)
±0.001, ...,
2000.00
mm/rev
Motion
commands m 1
G340 1 Spatial approach block (depth and in plane
(helix))
Effective during
soft
approach/retrac
tion
m 44
G341 Initial infeed on perpendicular axis (z),
then approach in plane
Effective during
soft
approach/retrac
tion
m 44
G347 Soft approach with semicircle s 2
G348 Soft retraction with semicircle s 2
G450 1 Transition circle Corner behavior
with tool radius
compensation
m 18
G451 Intersection of equidistances m 18
G460 1 Collision monitoring for approach and
retraction block ON
m 48
G461 Extend border block with arc
if ...
m 48
G462 Extend border block with line if ...
... no
intersection in
TRC block m 48
G500 1 Deactivation of all settable frames if G500
does not contain a value
m 8
Tables
12.1 List of statements
Fundamentals
450 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
G505 ...G599 5 ... 99. Settable zero offset m 8
G601 1 Block change at exact stop fine m 12
G602 Block change at exact stop coarse m 12
G603 Block change at IPO - end of block m 12
G641 Exact stop - continuous-path mode G641 AIDS=... m 10
G642 Corner rounding with axial precision
Only effective:
- with act. G60
or
- with G9 with
programmable
transition
rounding m 10
G643 Block-internal corner rounding m 10
G644 Corner rounding with specified axis
dynamics
m 10
G621 Corner deceleration at all corners Together with
continuous-path
mode only
G621 AIDS=... m 57
G700 Dimensions in inches and inch/min
(lengths + velocities + system variable)
m 13
G710 1 Metric dimension in mm and mm/min
(lengths + velocities + system variable)
m 13
G8101, ..., G819 G group reserved for the OEM
31
G8201, ..., G829 G group reserved for the OEM
32
G931 Feedrate specified by travel time Travel time m 15
G942 Freeze linear feedrate and constant cutting
rate or spindle speed
m 15
G952 Freeze revolutional feedrate and constant
cutting rate or spindle speed
m 15
G961 Constant cutting rate and linear feed Feed type as
for G94.
G961 S... LIMS=... F... m 15
G962 Linear or revolutional feedrate and
constant cutting rate
m 15
G971 Freeze spindle speed and linear feed Feed type as
for G94.
m 15
G972 Freeze linear or revolutional feedrate and
constant spindle speed
m 15
G973 Revolutional feedrate without spindle
speed limitation
G97 without
LIMS for ISO
mode
m 15
GEOAX Assign new channel axes to geometry
axes 1 - 3.
Without
parameter:
MD settings
effective.
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 451
Name Meaning Value Description,
comment
Syntax m/s3Group 2
GET Assign machine axis/axes Axis must be
released in the
other channel
with RELEASE.
GETD Assign machine axis/axes directly See GET.
GETACTT Get active tool from a group of tools with
the same name.
GETSELT Get selected T number.
GETT50 Get T number for tool name
GOTO Jump statement first forward then
backward (direction initially to end of
program and then to start of program)
GOTO (label, block no.)
Labels must exist in the
subprogram.
GOTOF Jump forwards (toward the end of the
program)
GOTOF (Label, block
no.)
GOTOB Jump backwards (toward the start of the
program)
Can be applied
in part program
and technology
cycles.
GOTOB (Label, block
no.)
GOTOC Suppress alarm 14080 "Destination not
found".
See GOTO.
GWPSOF Deselect constant grinding wheel
peripheral speed (GWPS).
GWPSOF(T No.) s
GWPSON Select constant grinding wheel peripheral
speed (GWPS)
GWPSON(T No.) s
H... Auxiliary function output to
the PLC
Real/INT
progr.:
REAL:
0 ...+/- 3.4028
exp38
INT:
-2147483646
...
+2147483647
Display:
±
999,999,999.9
999
Can be
set for each MD
(machine
manufacturer).
H100 or H2=100
I 4 Interpolation parameters Real s
I1 Intermediate point
coordinate
Real s
IC Incremental dimensioning 0, ...,
±99999.999°
X=IC(10) s
ICYCOF All blocks of a technology cycle are
processed in one IPO cycle following
ICYCOF.
Within the
program level
only.
ICYCON Each block of a technology cycle is
processed in a separate IPO cycle
following ICYCON.
Within the
program level
only.
IDS Identification of static synchronized actions
Tables
12.1 List of statements
Fundamentals
452 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
IF Introduction of a conditional jump in the
part program/technology cycle
Structure: IF-
ELSE-ENDIF
IF (condition)
INCCW Travel on a circle involute
in CCW direction with
interpolation of involute by
G17/G18/G19
Real m 1
INCW Travel on a circle involute
in CW direction with
interpolation of involute by
G17/G18/G19
Real
End point:
Center point:
Radius with
CR > 0:
Angle of
rotation in
degrees
between start
and end vectors
INCW/INCCW X... Y...
Z...
INCW/INCCW I... J...
K...
INCW/INCCW CR=...
AR...
Direct programming:
INCW/INCCW I... J...
K... CR=... AR=...
m 1
INDEX Define index of character
in input string
0, ...,
INT
String:
1st parameter,
character:
2nd parameter
INIT Select module for execution in a channel Channel
numbers
1-10 or $MC
_CHAN_
NAME
INIT(1,1,2) or
INIT(CH_X, CH_Y)
INT Data type: Integer with
sign
- (231-1), ...,
231-1
INTERSEC Calculate intersection
between two contour
elements and specify
TRUE intersection status
in ISPOINT
VAR REAL [2] ISPOINT error
status: BOOL
FALSE
ISPOINTS=
INTERSEC
(TABNAME1[n1],
TABNAME2[n2],
ISTCOORD, MODE)
IP Variable interpolation
parameter
real
IPOBRKA Motion criterion from braking ramp
activation
Braking ramp at
100% to 0%.
IPOBRKA=.. or
IPOBRKA(<axis>[,REA
L])
m
IPOENDA End of motion when “IPO stop” is reached IPOENDA=.. or
IPOENDA[n]..
m
IPTRLOCK Freeze start of the untraceable program
section at next machine function block.
Freeze interrupt
pointer.
m
IPTRUNLOCK Set end of untraceable program section at
current block at time of interruption.
Set interrupt
pointer.
m
ISAXIS Check if geometry axis 1
specified as parameter
BOOL
ISD Insertion depth
real m
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 453
Name Meaning Value Description,
comment
Syntax m/s3Group 2
ISFILE Check whether the file
exists in the NCK user
memory.
BOOL Returns results
of type BOOL.
RESULT=ISFILE("Testfi
le") IF
(RESULT==FALSE)
ISNUMBER Check whether the input
string can be converted to
a number.
BOOL Convert input
string to a
number.
ISPOINTS Possible intersections
calculated by ISTAB
between two contours on
the current plane.
INT Machining type
MODE
(optional).
STATE=ISPOINTS
(KTAB1[n1],
KTAB2[n2], ISTAB,
[MODE])
ISVAR Check whether the
transfer parameter
contains a variable known
in the NC
BOOL Machine data,
setting data and
variables such
as GUDs
J 4 Interpolation parameters Real s
J1 Intermediate point
coordinate
real s
JERKA Activate acceleration response set via MD
for programmed axes
JERKLIMA5 Reduction or overshoot of
maximum jerk (jerk axial)
1, ..., 200 Valid range is
1 to 200%
JERKLIMA[X]= ...[%] m
K 4 Interpolation parameters Real s
K1 Intermediate point
coordinate
Real s
KONT Travel round contour on tool offset m 17
KONTC Approach/retract with continuous-
curvature
polynomial.
m 17
KONTT Approach/retract with continuous-tangent
polynomial.
m 17
L Subroutine number Integer, up to
7 places
L10 s
LEAD 5 Lead angle real m
LEADOF Master value coupling OFF (lead off)
LEADON Master value coupling ON (lead on)
LFOF 1 Interrupt thread cutting OFF m 41
LFON Interrupt thread cutting ON m 41
LFPOS Axial retraction to a position m 46
LFTXT 1 Tangential tool direction on retraction m 46
LFWP Non-tangential tool direction on retraction m 46
Tables
12.1 List of statements
Fundamentals
454 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
LIFTFAST Rapid lift before interrupt routine call
LIMS Spindle speed limitation
with G96/G961 and G97
(limit spindle speed)
0.001, ...,
99 999. 999
m
LN Natural logarithm real
LOCK Disable synchronized action with ID
(stop technology cycle)
LOG (Common) logarithm real
LOOP Introduction of an endless loop Structure:
LOOP-
ENDLOOP
M... Switching operations INT
Display:
0, ...,
999 999 999
Program:
0,...,
2147483647
Up to 5
unassigned
M functions can
be assigned by
the machine
manufacturer.
M0 9 Programmed stop
M1 9 Optional stop
M2 9 End of main program with return to
beginning of program
M3 Direction of spindle rotation clockwise for
master spindle
M4 Direction of spindle rotation
counterclockwise for master spindle
M5 Spindle stop for master spindle
M6 Tool change
M17 9 End of subroutine
M19 For SSL accumulated spindle
programming
M30 9 End of program, same effect as M2
M40 Automatic gear change
M41... M45 Gear stage 1, ..., 5
M70 Transition to axis mode
MASLDEF Define master/slave axis grouping.
MASLDEL Uncouple master/slave axis grouping and
clear grouping definition.
MASLOF Disable a temporary coupling
MASLOFS Deactivate a temporary coupling with
automatic slave axis stop.
MASLON Enable a temporary coupling
MAXVAL Larger value of two
variables (arithm.
function)
real If values are the
same, the same
value is
returned.
ValMax =
MAXVAL(Var1, Var2)
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 455
Name Meaning Value Description,
comment
Syntax m/s3Group 2
MCALL Modal subprogram call Without
subprogram
name:
Deselection
MEAC Continuous measurement
without deleting distance-
to-go
Integer,
without sign
s
MEAFRAME Frame calculation from
measuring points
FRAME
MEAS Measure with touch-
trigger probe
Integer,
without sign
s
MEASA Measurement with
deletion of distance-to-go
s
MEAW Measure with touch-
trigger probe without
deleting distance-to-go
Integer,
without sign
s
MEAWA Measurement without
deletion of distance-to-go
s
MI Access to frame data: Mirroring MI
MINDEX Define index of
character in input
string
0, ...,
INT
String:
1st parameter,
character:
2nd parameter
MINVAL Smaller value of two
variables (arithm.
function)
real If values are the
same, the same
value is
returned.
ValMin =
MINVAL(Var1, Var2)
MIRROR Programmable Mirroring MIRROR X0 Y0 Z0
;separate block
s 3
MMC Call the dialog
window interactively
from the part
program on the HMI.
STRING
MOD Modulo division.
MOV Start positioning axis
(start moving
positioning axis).
real
MSG Programmable messages MSG("message") m
N Block number - subblock 0, ...,
9999 9999
integers only,
without signs
Can be used for
assigning a
number to a
block; located
at beginning of
block.
e.g., N20
Tables
12.1 List of statements
Fundamentals
456 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
NCK Specify validity range for data Once per NCK
NEWCONF Accept modified machine data.
Corresponds to set machine data active.
Also possible
via HMI.
NEWT Create new tool Duplo number
can be omitted.
NORM 1 Standard setting in starting point and end
point with tool offset
m 17
NOT Logical NOT (negation)
NPROT Machine-specific protection zone ON/OFF
NPROTDEF Machine-specific protection area definition
(NCK-specific protection area definition)
NUMBER Convert input string to
number
real
OEMIPO16,8 OEM interpolation 1 m 1
OEMIPO26,8 OEM interpolation 2 m 1
OF Keyword in CASE branch
OFFN Allowance on the programmed contour OFFN=5
OMA1 6 OEM address 1 Real m
OMA2 6 OEM address 2 Real m
OMA3 6 OEM address 3 Real m
OMA4 6 OEM address 4 Real m
OMA5 6 OEM address 5 Real m
OFFN Offset - normal real m
OR Logical OR
ORIC 1,6 Orientation changes at outside corners are
superimposed on the circle block to be
inserted
(orientation change continuously)
m 27
ORID 6 Orientation changes are performed before
the circle block
(orientation change discontinuously)
m 27
ORIAXPOS Orientation angle via virtual orientation
axes with rotary axis positions
m 50
ORIEULER Orientation angle via Euler angle m 50
ORIAXES Linear interpolation of machine axes or
orientation axes
m 51
ORICONCW Interpolation on a circular peripheral
surface in CW direction
m 51
ORICONCCW Interpolation on a circular peripheral
surface in CCW direction
Final
orientation:
Vector
specification
A3, B3, C3, or
Euler/RPY
angle A2, B2,
C2
Additional
Parameter settings as
follows:
Direction vectors
normalized A6=0 B6=0
C6=1
Opening angle
implemented as travel
angle with
SLOT=...
m 51
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 457
Name Meaning Value Description,
comment
Syntax m/s3Group 2
ORICONIO Interpolation on a circular peripheral
surface with intermediate orientation
setting
m 51
ORICONTO Interpolation on circular peripheral surface
in tangential transition (final orientation)
m 51
ORICURVE Interpolation of orientation with
specification of motion of two contact
points of tool
m 51
ORIPLANE Interpolation in a plane
(corresponds to ORIVECT),
large-radius circular interpolation
specifications:
Rotational
vectors
A6, B6, C6
Opening angle
of cone in
degrees:
0 < SLOT < 180
Intermediate
vectors:
A7, B7, C7
Tool contact
point:
XH, YH, ZH
SLOT=+... at ≤ 180
degrees
SLOT= -... at ≥ 180
degrees
Intermediate orientation
normalized
A7=0 B7=0 C7=1
m 51
ORIPATH Tool orientation in relation to path Handling
transformation
package (see
/FB3/TE4).
m 51
ORIPATHS Tool orientation in relation to path, blips in
the orientation characteristic are smoothed
Relative to the
path as a
whole.
m 51
ORIROTA Angle of rotation to an absolute direction
of rotation.
m 54
ORIROTC Tangential rotational vector in relation to
path tangent
Relative to path
tangent.
m 54
ORIROTR Angle of rotation relative to the plane
between the start and end orientation.
m 54
ORIROTT Angle of rotation relative to the change in
the orientation vector.
m 54
ORIRPY Orientation angle via RPY angle (XYZ) Rotational
sequence XYZ
m 50
ORIRPY2 Orientation angle via RPY angle (ZYX) Rotational
sequence ZYX
m 50
ORIS 5 Orientation modification
(orientation smoothing
factor)
real Relative to the
path.
m
ORIVECT Large-radius circular interpolation
(identical to ORIPLANE)
m 51
ORIVIRT1 Orientation angle via virtual orientation
axes (definition 1)
m 50
ORIVIRT2 Orientation angle via virtual orientation
axes (definition 1)
m 50
ORIMKS 6 Tool orientation in the machine coordinate
system
m 25
ORIRESET Initial setting of tool orientation with up to 3
orientation axes
Parameter
optional (REAL)
ORIRESET(A,B,C)
Tables
12.1 List of statements
Fundamentals
458 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
ORIWKS 1,6 Tool orientation in the workpiece
coordinate system
m 25
OS Oscillation on/off Integer,
without sign
OSB Oscillating: Start point m
OSC 6 Continuous tool orientation smoothing m 34
OSCILL Axis assignment for
oscillation-
activate oscillation
Axis: 1 - 3
infeed axes
m
OSCTRL Oscillation control options Integer,
without sign
m
OSD 6 Rounding of tool orientation by specifying
rounding length with SD
Block-internal m 34
OSE Oscillating: End point m
OSNSC Oscillating: Number of
spark-out cycles
(oscillating: number spark-
out cycles)
m
OSOF 1,6 Tool-orientation smoothing OFF m 34
OSP1 Oscillating: Left reversal
point
(oscillating: position 1)
Real m
OSP2 Oscillating: Right reversal
point
(oscillating: position 2)
Real m
OSS 6 Tool-orientation smoothing at end of block m 34
OSSE 6 Tool-orientation smoothing at start and
end of block
m 34
OST 6 Rounding of tool orientation by specifying
angle tolerance in degrees with SD
(maximum deviation from programmed
orientation characteristic)
Block-internal m 34
OST1 Oscillating: Stopping point
in left reversal point
Real m
OST2 Oscillating: Stopping point
in right reversal point
Real m
OVR Speed override 1, ..., 200% m
OVRA Axial speed override 1, ..., 200% m
P Number of subprogram
cycles
1, ..., 9999,
integers w/o
signs
e.g., L781 P...
; separate block
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 459
Name Meaning Value Description,
comment
Syntax m/s3Group 2
PCALL Call subprograms with the absolute path
and parameter transfer
No absolute
path. Behavior
as for CALL.
PAROT Align workpiece coordinate system on
workpiece
m 52
PAROTOF Deactivate workpiece-related frame
rotation
m 52
PDELAYOF 6 Punch with delay OFF
m 36
PDELAYON 1.6 Punch with delay ON
m 36
PL Parameter interval length Real, without
sign
s
PM Per minute Feed per
minute.
PO Polynomial Real, without
sign
s
POLF LIFTFAST position Real, without
sign
Geometry axis
in WCS,
otherwise MCS.
POLF[Y]=10 target
position of retracting
axis
m
POLFA Start retract position of
single axes with
$AA_ESR_TRIGGER
For single axes. POLFA(AX1, 1, 20.0) m
POLFMASK Enable axes for retraction
without a connection
between the axes
Selected axes POLFMASK(AX1, AX2,
...)
m
POLFMLIN Enable axes for retraction
with a linear connection
between the axes
Selected axes POLFMIN(AX1, AX2,
...)
m
POLY 5 Polynomial interpolation m 1
POLYPATH 5 Polynomial interpolation can be selected
for the AXIS or VECT axis groups
POLYPATH ("AXES")
POLYPATH ("VECT")
m 1
PON 6 Punch ON m 35
PONS 6 Punch ON in IPO cycle (punch ON slow) m 35
POS Axis positioning POS[X]=20
POSA Position axis across block
boundary
POSA[Y]=20
POSP Positioning in part
sections (oscillation)
(position axis in parts)
Real: end
position, part
length;
Integer: option
POT Square
(arithmetic function)
real
PR Per revolution Revolutional feedrate
Tables
12.1 List of statements
Fundamentals
460 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
PRESETON Sets the actual value for programmed
axes
One axis
identifier is
programmed at
a time, with its
respective
value in the
next parameter.
Up to 8 axes
possible.
PRESETON(X,10,Y,
4.5)
PRIO Keyword for setting the priority for interrupt
processing
PROC First instruction in a program Block number - PROC -
identifier
PTP Point to point motion
(point to point)
synchronous
axis
m 49
PTPG0 Point to point motion only with G0,
otherwise CP
synchronous
axis
m 49
PUTFTOC Fine tool offset for parallel dressing
(continuous dressing)
(put fine tool correction)
Channel
numbers 1 - 10
or $MC
_CHAN_NAME
PUTFTOC(1,1,2) or
PUTFTOC(CH_name)
PUTFTOCF Fine tool offset depending on a function
defined with FCtDEF for parallel dressing
(continuous dressing)
(put fine tool correction function
dependant)
Channel
numbers 1 - 10
or $MC
_CHAN_NAME
PUTFTOCF(1,1,2) or
PUTFTOCF(CH_name)
PW Point weight
Real, without
sign
s
QECLRNOF Quadrant error compensation learning
OFF
QECLRNON Quadrant error compensation learning ON
QU Fast additional (auxiliary) function output
R... Arithmetic parameters
also as settable address
identifier and with numerical
extension
±
0.0000001,
...,
9999 9999
Number of R
parameters that
can be set by
MD
R10=3
;R parameter
assignment
X=R10 ;axis
valueR[R10]=6
;indirect prog.
RAC Absolute, non-modal, axis-specific radius
programming
Radius
programming
RAC(50) s
RDISABLE Read-in disable
READ Reads one or more lines in the specified
file and stores the information read in the
array.
The information
is available as
STRING.
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 461
Name Meaning Value Description,
comment
Syntax m/s3Group 2
READAL Read alarm Alarms are
searched
according to
ascending
numbers
REAL Data type: floating point
variable with sign (real
numbers)
Correspond
s to the 64-
bit floating
point format
of the
processor
REDEF Setting for machine data, NC language
elements and system variables, specifying
the user groups they are displayed for
RELEASE Release machine axes Multiple axes
can be
programmed.
REP Keyword for initialization of all elements of
an array with the same value
REP(value)
or
DO ARRAY[n,m]=REP(
)
REPEAT Repeat a program loop Until (UNTIL) a
condition is
fulfilled.
REPEATB Repeat a program line nnn times
REPOSA Repositioning linear all axes
s 2
REPOSH Repositioning semi circle
s 2
REPOSHA Repositioning all axes; geometry axes
semicircle
(repositioning semicircle all axes)
s 2
REPOSL Repositioning linear
s 2
REPOSQ Repositioning quarter circle
s 2
REPOSQA Repositioning linear all axes; geometry
axes quarter circle
(repositioning quarter circle all axes)
s 2
RESET Reset technology cycle One or several
IDs can be
programmed.
Tables
12.1 List of statements
Fundamentals
462 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
RET End of subroutine Use in place of
M17 – without
function output
to PLC.
RET
RIC Relative, non-modal, axis-specific radius
programming
Radius
programming
RIC(50) s
RINDEX Define index of character
in input string
0, ...,
INT
String:
1st parameter,
character:
2nd parameter
RMB Repositioning at beginning of block
(repos mode begin of block)
m 26
RME Repositioning at end of block
(repos mode end of block)
m 26
RMI 1 Repositioning at interruption point
(repos mode interrupt)
m 26
RMN Reapproach to nearest path point
(repos mode end of nearest orbital block)
m 26
RND Round the contour corner Real, without
sign
RND=... s
RNDM Modal rounding Real, without
sign
RNDM=...
RNDM=0: disable
modal rounding
m
ROT Programmable rotation Rotation
around
1st geometry
axis:
-180°... +180°
2nd geometry
axis:
-90° ... +90°
3rd geometry
axis:
-180°... +180°
ROT X... Y... Z...
ROT RPL=
;separate block
s 3
ROTS Programmable frame rotations with solid
angles (rotation)
ROTS X… Y…
ROTS Z… X...
ROTS Y... Z...
ROTS RPL=
;separate block
s 3
ROUND Round decimal places real
RP Polar radius real m/n
RPL Rotation in the plane Real, without
sign
s
RT Parameter for access to frame data:
Rotation
RTLION G0 with linear interpolation m 55
RTLIOF G0 without linear interpolation (single-axis
interpolation)
m 55
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 463
Name Meaning Value Description,
comment
Syntax m/s3Group 2
S Spindle speed or
(with G4, G96/G961)
other meaning
REAL
Display:
±999 999
999.9999
Program:
±3.4028 ex38
Spindle speed
in rpm
G4: Dwell time
in spindle
revolutions
G96/G961:
Cutting rate in
m/min.
S...: Speed for master
spindle
S1...: Speed for spindle
1
m/n
SAVE Attribute for saving information at
subprogram calls
The following
are saved: All
modal G
functions and
the current
frame.
SBLOF Suppress single block
(single block OFF)
The following
blocks are
executed in
single block like
a block.
SBLON Clear single block suppression
(single block ON)
SC Parameter for access to frame data:
Scaling (scale)
SCALE Programmable scaling
(scale)
SCALE X... Y... Z...
;separate block
s 3
SCC Selective assignment of transverse axis to
G96/G961/G962. Axis identifiers may take
the form of geo, channel or machine axes.
Also with
constant cutting
rate
SCC[axis]
SD Spline degree
Integer,
without sign
s
SEFORM Structuring instruction in Step editor to
generate the step view for HMI Advanced
Evaluated in
Step editor.
SEFORM
(<section_name>,
<level>, <icon> )
SET Keyword for initialization of all elements of
an array with listed values
SET(value, value, ...) or
DO ARRAY[n,m]=SET(
)
SETAL Set alarm
SETDNO Set D number of tool (T) and its cutting
edge to "new".
SETINT Define which interrupt routine is to be
activated when an NCK input is present
Edge 0 → 1
is analyzed.
SETMS Reset to the master spindle defined in
machine data
SETMS(n) Set spindle n as master spindle
SETPIECE Set piece number for all tools assigned to
the spindle.
Without spindle
number:
applies to
master spindle.
Tables
12.1 List of statements
Fundamentals
464 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
SF Starting point offset for
thread cutting
(spline offset)
0.0000,...,
359.999°
m
SIN Sine (trigon. function) real
SOFT Soft smoothed path acceleration m 21
SOFTA Switch on soft axis acceleration for the
programmed axes
SON 6 Nibbling ON (stroke ON) m 35
SONS 6 Nibbling ON in IPO cycle (stroke ON slow) m 35
SPATH 1 Path reference for FGROUP axes is arc
length
m 45
SPCOF Switch master spindle or spindle(s) from
position control to speed control
SPCOF
SPCOF(n)
m
SPCON Switch master spindle or spindle(s) from
speed control to position control
SPCON
SPCON (n)
m
SPIF1 1,6 Fast NCK inputs/outputs for
punching/nibbling byte 1
(stroke/punch interface 1)
m 38
SPIF2 6 Fast NCK inputs/outputs for
punching/nibbling byte 2
(stroke/punch interface 2)
m 38
SPLINE-PATH Define spline grouping Max. 8 axes.
SPOF 1,6 Stroke OFF, punching, nibbling OFF
m 35
SPN 6 Number of path sections
per block
(stroke/punch number)
Integer s
SPP 6 Length of path section
(stroke/punch path)
Integer m
SPOS Spindle position SPOS=10 or
SPOS[n]=10
m
SPOSA Spindle position across
block boundaries
SPOSA=5 or
SPOSA[n]=5
m
SQRT Square root
(arithmetic function)
real
SR Sparking-out retraction
path
for synchronized action
Real, without
sign
s
SRA Sparking-out retraction
path with external input
axial
for synchronized action
SRA[Y]=0.2 m
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 465
Name Meaning Value Description,
comment
Syntax m/s3Group 2
ST Sparking-out time
for synchronized action
Real, without
sign
s
STA Sparking-out time axial
for synchronized action
m
START Start selected programs simultaneously in
several channels from current program
Ineffective for
the local
channel.
START(1,1,2) or
START(CH_X, CH_Y)
$MC _CHAN_NAME
STARTFIFO1 Execute; simultaneously fill preprocessing
memory
m 4
STAT Position of joints Integer s
STOPFIFO Stop machining; fill preprocessing memory
until STARTFIFO is detected, FIFO full or
end of program
m 4
STOPRE Stop preprocessing until all prepared
blocks are executed in main run
STOPREOF Stop preprocessing OFF
STRING Data type: Character
string
Max. 200
characters
STRINGIS Checks the present scope
of NC language and NC
cycle names, user
variables, macros and
label names belonging
especially to this
command to establish
whether these exist, are
valid, defined or active.
INT The return
value results
are
000
not known 100
programmable
2XX recognized
as present
STRINGIS
(STRING,name)=
Digit-coded
return value
STRLEN Define string length INT
SUBSTR Define index of character
in input string
real String: 1st
parameter,
character: 2nd
parameter
SUPA Suppression of current zero offset,
including programmed offsets, system
frames, handwheel offsets (DRF), external
zero offset and overlaid motion
s 9
SYNFCT Evaluation of a polynomial
as a function of a
condition in the motion-
synchronous action
VAR REAL
Tables
12.1 List of statements
Fundamentals
466 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
SYNR The variable is read synchronously, i.e., at
execution time
(synchronous read)
SYNRW The variable is read and written
synchronously, i.e., at execution time
(synchronous read-write)
SYNW The variable is written synchronously, i.e.,
at execution time
(synchronous write)
T Call tool
(only change if specified
in machine data;
otherwise M6 command
necessary)
1, ..., 32 000 Call using T-no.
or tool identifier.
For example, T3 or
T=3,
e.g., T="DRILL"
TAN Tangent (trigon. function) real
TANG Determine tangent for the follow-up from
both specified leading axes
TANGOF Tangent follow-up mode OFF
TANGON Tangent follow-up mode ON
TCARR Request toolholder
(number "m")
Integer m=0: deselect
active
toolholder
TCARR=1
TCOABS 1 Determine tool length components from
the orientation of the current toolholder
m 42
TCOFR Determine tool length components from
the orientation of the active frame
Necessary after
reset, e.g.,
through manual
setting m 42
TCOFRX Determine tool orientation of an active
frame on selection of tool, tool points in X
direction
Tool
perpendicular to
inclined surface
m 42
TCOFRY Determine tool orientation of an active
frame on selection of tool, tool points in Y
direction
Tool
perpendicular to
inclined surface
m 42
TCOFRZ Determine tool orientation of an active
frame on selection of tool, tool points in Z
direction
Tool
perpendicular to
inclined surface
m 42
THETA Angle of rotation THETA is
always
perpendicular to
the current tool
orientation.
THETA=Value
THETA=AC
THETA=IC
Polynomial for THETA
PO[THT]=(…)
s
TILT 5 Tilt angle real TILT=Value m
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 467
Name Meaning Value Description,
comment
Syntax m/s3Group 2
TMOF Deselect tool monitoring T-no. required
only when the
tool with this
number is not
active.
TMOF (T no.)
TMON Activate tool monitoring T No. = 0:
Deactivate
monitoring for
all tools
TMON (T no.)
TO Defines the end value in a FOR counter
loop
TOFFOF Deactivate on-line tool offset
TOFFON Activate online tool length offset
(Tool offset ON)
Specify a 3D
offset direction.
TOFFON (Z, 25) with
offset direction Z,
offset value 25
TOFRAME Set current programmable frame to tool
coordinate system
m 53
TOFRAMEX X axis parallel to tool direction, secondary
axis Y, Z
m 53
TOFRAMEY Y axis parallel to tool direction, secondary
axis Z, X
m 53
TOFRAMEZ Z axis parallel to tool direction, secondary
axis X, Y
Frame rotation
in tool direction.
m 53
TOLOWER Convert letters of the string into lowercase
TOROTOF Frame rotations in tool direction OFF m 53
TOROT Z axis parallel to tool orientation m 53
TOROTX X axis parallel to tool orientation m 53
TOROTY Y axis parallel to tool orientation m 53
TOROTZ Z axis parallel to tool orientation
Frame rotations
EIN
Rotary
component of
the
programmable
frame
m 53
TOUPPER Convert letters of the string into uppercase
TOWSTD Initial setting value for offsets in tool length m 56
TOWBCS Wear values in basic coordinate system
(BCS)
m 56
TOWKCS Wear values in the coordinate system of
the tool head for kinetic transformation
(differs from MCS by tool rotation)
m 56
TOWMCS Wear data in the machine coordinate
system (MCS)
Inclusion of tool
wear
m 56
Tables
12.1 List of statements
Fundamentals
468 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
TOWTCS Wear values in the tool coordinate system
(tool carrier ref. point T at the tool holder)
m 56
TOWWCS Wear values in workpiece coordinate
system (WCS)
m 56
TRAANG Transformation inclined axis Several
transformations
can be set for
each channel.
TRACEOF Circularity test: Transfer of values OFF
TRACEON Circularity test: Transfer of values ON
TRACON Transformation concatenated
TRACYL Cylinder: Peripheral surface
transformation
See TRAANG.
TRAFOOF Deactivate transformation TRAFOOF( )
TRAILOF Asynchronous coupled motion of axes
OFF
(trailing OFF)
TRAILON Asynchronous coupled motion of axes ON
(trailing ON)
TRANS Programmable offset (translation) TRANS X... Y... Z...
;separate block
s 3
TRANSMIT Polar transformation See TRAANG.
TRAORI 4-axis, 5-axis transformation, generic
transformation
(transformation oriented)
Activates the
specified
orientation
transformation.
Generic transformation
TRAORI(1,X,Y,Z)
TRUE Logical constant: True BOOL Can be
replaced
with integer
constant 1.
TRUNC Truncate decimal places real
TU Axis angle Integer TU=2 s
TURN Number of turns for helix 0, ..., 999 s
UNLOCK Enable synchronized action with ID
(continue technology cycle)
UNTIL Condition for end of REPEAT loop
UPATH Path reference for
FGROUP axes is curve
parameter
m 45
VAR Keyword: Type of parameter passing With VAR: Call
by reference
Tables
12.1 List of statements
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 469
Name Meaning Value Description,
comment
Syntax m/s3Group 2
VELOLIMA5 Reduction or overshoot of
maximum axial velocity
1, ..., 200 Valid range is
1 to 200%
VELOLIMA[X]= ...[%] m
WAITC Wait until coupling block change criterion
for axes/spindles is fulfilled (wait for couple
condition)
Up to 2
axes/spindles
can be
programmed.
WAITC(1,1,2)
WAITE Wait for end of program on another
channel.
Channel
numbers 1 - 10
or $MC
_CHAN_NAME
WAITE(1,1,2) or
WAITE(CH_X, CH_Y)
WAITM Wait for marker in specified channel;
terminate previous block with exact stop.
Channel
numbers 1 - 10
or $MC
_CHAN_NAME
WAITM(1,1,2) or
WAITM(CH_X, CH_Y)
WAITMC Wait for marker in specified channel; exact
stop only if the other channels have not
yet reached the marker.
Channel
numbers 1 - 10
or $MC
_CHAN_NAME
WAITMC(1,1,2) or
WAITMC(CH_X, CH_Y)
WAITP Wait for end of traversing WAITP(X)
; separate block
WAITS Waiting to reach spindle position WAITS (main spindle)
WAITS (n,n,n)
WALCS0 WORK working-area limitation deselected m 60
WALCS1 WORK working-area-limitation group 1
active
m 60
WALCS2 WORK working-area-limitation group 2
active
m 60
WALCS3 WORK working-area-limitation group 3
active
m 60
WALCS4 WORK working-area-limitation group 4
active
m 60
WALCS5 WORK working-area-limitation group 5
active
m 60
WALCS6 WORK working-area-limitation group 6
active
m 60
WALCS7 WORK working-area-limitation group 7
active
m 60
WALCS8 WORK working-area-limitation group 8
active
m 60
WALCS9 WORK working-area-limitation group 9
active
m 60
WALCS10 WORK-working-area-limitation group 10
active
m 60
WALIMOF BCS working area limitation OFF
; separate block m 28
WALIMON1 BCS working area limitation ON
; separate block m 28
Tables
12.1 List of statements
Fundamentals
470 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Name Meaning Value Description,
comment
Syntax m/s3 Group 2
WHILE Start of WHILE program loop End:
ENDWHILE
WRITE Write block in file system.
Appends a block to the end of the
specified file.
The blocks are
inserted after
M30.
X Axis real m/n
XOR Logical exclusive OR
Y Axis real m/n
Z Axis real m/n
Legend:
1 Default setting at beginning of program (factory settings of the control, if nothing else programmed)
2 The groups are numbered according to the table in section "List of G functions/preparatory functions".
3 Absolute end points: modal (m);
incremental end points: non-modal (n);
otherwise: modal/non-modal depending on syntax of G function
4 As circle center points, IPO parameters act incrementally. They can be programmed in absolute mode with AC. The
address modification is ignored when the parameters have other meanings (e.g., thread pitch).
5 The keyword is not valid for SINUMERIK 810D.
5 The keyword is not valid for SINUMERIK 810D/NCU571.
7 The keyword is not valid for SINUMERIK FM-NC.
8 The OEM can add two extra interpolation types. The names can be changed by the OEM.
9 Extended address notation cannot be used for these functions.
Tables
12.2 List of addresses
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 471
12.2 List of addresses
List of addresses
The list of addresses consists of
• Address letters
• Fixed addresses
• Fixed addresses with axis expansion
• Settable addresses
Address letters
Available address letters
Letter Meaning Numeric
extension
A Variable address identifier x
B Variable address identifier x
C Variable address identifier x
D Selection/deselection of tool length compensation, tool cutting edge
E Variable address identifier
F Feedrate
dwell time in seconds
x
G G function
H H function x
I Variable address identifier x
J Variable address identifier x
K Variable address identifier x
L Subprograms, subprogram call
M M function x
N Subblock number
O Unassigned
P Number of program runs
Q Variable address identifier x
R Variable identifier (arithmetic parameter)/variable address identifier without numerical
Expansion
x
S Spindle value
dwell time in spindle revolutions
x
x
T Tool number x
V Variable address identifier x
V Variable address identifier x
W Variable address identifier x
X Variable address identifier x
Y Variable address identifier x
Tables
12.2 List of addresses
Fundamentals
472 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Z Variable address identifier x
% Start character and separator for file transfer
: Main block number
/ Skip identifier
Available fixed addresses
Address
identifier
Address type Modal/
non-
modal
G70/
G71
G700/
G710
G90/
G91
IC AC DC,
ACN,
ACP
CIC,
CAC,
CDC,
CACN,
CACP
Qu Data type
L Subprogram
no.
n Integer without
sign
P Number of
subprogram
passes
n Integer without
sign
N Block number n Integer without
sign
G G function See
list of
G
functio
ns
Integer without
sign
F Feed, dwell
time
m, n x x Real without
sign
OVR Override m Real without
sign
S Spindle, dwell
time
m, n x Real without
sign
SPOS Spindle
position
m x x x Real
SPOSA Spindle
position
beyond block
limits
m x x x Real
T Tool number m x Integer without
sign
D Offset number m x Integer without
sign
M, H, Auxiliary
functions
n x M: Integer
without sign
H: Real
Tables
12.2 List of addresses
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 473
Fixed addresses with axis expansion
Address
identifier
Address type Modal/
non-
modal
G70/
G71
G700/
G710
G90/
G91
IC AC DC,
ACN,
ACP
CIC,
CAC,
CDC,
CACN,
CACP
Qu Data type
AX: Axis Variable axis
identifier
*) x x x x x x Real
IP:
Interpolatio
n parameter
Variable
interpolation
parameter
n x x x x x Real
POS:
Positioning
axis
Positioning
axis
m x x x x x x x Real
POSA:
Positioning
axis above
end of block
Positioning
axis across
block
boundaries
m x x x x x x x Real
POSP:
Positioning
axis in parts
Positioning
axis in parts
(oscillation)
m x x x x x x Real: End
position/real:
partial length
integer: Option
PO:
Polynomial
1)
Polynomial
coefficient
n x x Real without
sign
1 - 8 times
FA: Feed
axial
Axial feedrate m x x Real without
sign
FL: Feed
limit
Axial feed
limit
m x Real without
sign
OVRA:
Override
Axial override m x Real without
sign
ACC 2):
Axial
acceleration
Axial
acceleration
m Real without
sign
FMA:
Feedrate
multiple
axial
Synchronous
feedrate axial
m x Real without
sign
STW:
Sparking-
out time
axial
Sparking out
time axial
m Real without
sign
SRA:
Sparking-
out retract
Retraction
path on
external input
axial
m x x Real without
sign
OS:
Oscillating
ON/OFF
Oscillation
ON/OFF
m Integer without
sign
Tables
12.2 List of addresses
Fundamentals
474 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
OST1:
Oscillating
time 1
Stopping time
at left reversal
point
(oscillation)
m Real
OST2:
Oscillating
time 2
Stopping time
at right
reversal point
(oscillation)
m Real
OSP1:
Oscillating
position 1
Left reversal
point
(oscillation)
m x x x x x x Real
OSP2:
Oscillating
position 2
Right reversal
point
(oscillation)
m x x x x x x Real
OSB:
Oscillating
start
position m x x x x x x Real
OSE:
Oscillating
end position
Oscillation
end position
m x x x x x x Real
OSNSC:
Oscillating:
number
spark-out
cycles
Number of
spark-out
cycles
(oscillation)
m Integer without
sign
OSCTRL:
Oscillating
control
Oscillation
control
options
m Integer without
sign: set
options, integer
without sign:
reset options
OSCILL:
Oscillating
Axis
assignment
for oscillation
activate
oscillation
m Axis: 1 - 3
infeed axes
FDA:
Feedrate
DRF axial
Axis feedrate
for handwheel
override
n x Real without
sign
FGREF Reference
radius
m x x Real without
sign
POLF LIFTFAST
position
m x x Real without
sign
FXS:
Fixed stop
Travel to fixed
stop ON
m Integer without
sign
FXST:
Fixed stop
torque
Torque limit
for travel to
fixed stop
m Real
Tables
12.2 List of addresses
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 475
FXSW:
Fixed stop
window
Monitoring
window for
travel to fixed
stop
m Real
In these addresses, an axis or an expression of axis type is specified in square brackets.
The data type in the above column shows the type of value assigned.
*) Absolute end points: modal, incremental end points: non-modal, otherwise modal/non-
modal depending on syntax of G function.
1) The vocabulary word is not valid for SINUMERIK FM-NC.
2) The vocabulary word is not valid for SINUMERIK FM-NC/810D
Settable addresses
Address
identifier
Address
type
Modal/
non-
modal
G70/
G71
G700/
G710
G90/
G91
IC AC DC,
ACN,
ACP
CIC,
CAC,
CDC,
CACN,
CACP
Qu Max.
numb
er
Data type
Axis values and end points
X, Y, Z, A, B,
C
Axis *) x x x x x x 8 Real
AP: Angle
polar
Polar angle m/n* x x x 1 Real
RP: Polar
radius
Polar radius m/n* x x x x x 1 Real without
sign
Tool orientation
A2, B2, C2 1) Euler angle
or RPY
angle
n 3 Real
A3, B3, C3 1) Direction
vector
component
n
3 Real
A4, B4, C4 for
block
beginning 1)
Normal
vector
component
s 3 Real
A5, B5, C5 for
end of block 1)
Normal
vector
component
n 3 Real
A6, B6, C6
standardized
vector 1)
Direction
vector
component
s 3 Real
A7, B7, C7
standardized
vector 1)
Intermediat
e
orientation
component
s 3 Real
LEAD:
Lead angle 1)
Lead angle m 1 Real
Tables
12.2 List of addresses
Fundamentals
476 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
THETA: third
degree of
freedom Tool
orientation1)
Angle of
rotation,
rotation
about the
tool
direction
s x x x 1 Real
TILT:
Tilt angle 1)
Tilt angle m 1 Real
ORIS:1)
Orientation
Smoothing
factor
Orientation
change
(referring to
the path)
m 1 Real
Interpolation parameters
I, J, K**
I1, J1, K1
Interpolatio
n parameter
Intermediat
e point
coordinate
n
n
x
x
x
x
x
x**
x
x**
x
3 Real
Real
RPL:
Rotation
plane
Rotation in
the plane
n 1 Real
CR:
Circle radius
Circle
radius
n x x 1 Real without
sign
AR:
Angle circular
Opening
angle
1 Real without
sign
TURN Number of
turns for
helix
n 1 Integer
without sign
PL:
Parameter
interval length
Parameter
interval
length
n 1 Real without
sign
PW: Point weight n 1 Real without
sign
SD: Spline degree n 1 Integer
without sign
TU: Turn Turn m Integer Int
STAT: State State m Integer
without sign
SF:
Spindle offset
Starting
point offset
for thread
cutting
m 1 Real
DISR:
Distance for
repositioning
Distance for
repositionin
g
n x x 1 Real without
sign
Tables
12.2 List of addresses
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 477
DISPR:
Distance path
for
repositioning
Repos path
difference
n x x 1 Real without
sign
ALF:
Angle lift fast
Fast
retraction
angle
m 1 Integer
without sign
DILF:
Distance lift
fast
Fast
retraction
length
m x x 1 Real
FP Fixed point:
Number of
fixed point
to approach
n 1 Integer
without sign
RNDM:
Round modal
Modal
rounding
m x x 1 Real without
sign
RND:
Round
Non-modal
rounding
n x x 1 Real without
sign
CHF:
Chamfer
Chamfer
non-modal
n x x 1 Real without
sign
CHR:
Chamfer
Chamfer in
initial
direction of
motion
n x x 1 Real without
sign
ANG: Angle Contour
angle
n 1 Real
ISD:
Insertion
depth
Insertion
depth
m x x 1 Real
DISC:
Distance
Transition
circle
overshoot
tool offset
m x x 1 Real without
sign
OFFN Offset
contour -
normal
m x x 1 Real
DITS Thread run-
in path
m x x 1 Real
DITE Thread run-
out path
m x x 1 Real
Nibbling/punching
SPN:
Stroke/Punch
Number 2)
Number of
path
sections per
block
n 1 INT
SPP:
Stroke/Punch
Path 2)
Length of a
path section
m 1 Real
Tables
12.2 List of addresses
Fundamentals
478 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Grinding
ST:
Sparking-out
time
Sparking-
out time
n 1 Real without
sign
SR:
Sparking-out
retract path
Return path n x x 1 Real without
sign
Approximate positioning criteria
ADIS Rounding
clearance
m x x 1 Real without
sign
ADISPOS Rounding
clearance
for rapid
traverse
m x x 1 Real without
sign
Measurement
MEAS:
Measure
Measure
with touch-
trigger
probe
n 1 Integer
without sign
MEAW:
Measure
without
deleting
distance-to-go
Measure
without
deleting
distance-to-
go
n 1 Integer
without sign
Axis, spindle behavior
LIMS:
Limit spindle
speed
Spindle
speed
limitation
m 1 Real without
sign
Feedrates
FAD
Speed of
the slow
infeed
motion
n x 1 Real without
sign
FD:
Feed DRF
Path feed
for
handwheel
override
n x 1 Real without
sign
FRC Feed for
radius and
chamfer
n x Real without
sign
FRCM Feed for
radius and
chamfer,
modal
m x Real without
sign
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 479
OEM addresses
OMA1: OEM
address 1 2)
OEM
address 1
m x x x 1 Real
OMA2: OEM
address 2 2)
OEM
address 2
m x x x 1 Real
OMA3: OEM
address 3 2)
OEM
address 3
m x x x 1 Real
OMA4: OEM
address 4 2)
OEM
address 4
m x x x 1 Real
OMA5: OEM
address 5 2)
OEM
address 5
m x x x 1 Real
*) Absolute end points: modal, incremental end points: non-modal, otherwise modal/non-
modal depending on syntax of G function.
**)As circle center points, IPO parameters act incrementally. They can be programmed in
absolute mode with AC. The address modification is ignored when the parameters have
other meanings (e.g., thread pitch).
1) The vocabulary word is not valid for SINUMERIK FM-NC/810D.
2) The vocabulary word is not valid for SINUMERIK FM-NC/810D/NCU571.
12.3 List of G functions/preparatory functions
List of G functions/preparatory functions
In the list of G functions/motion commands you will find all available G codes according to
the appropriate functional groups.
Legend for describing the G groups
No.: internal number for, e.g., PLC interface
X: No. for GCODE_RESET_VALUES not permitted
m: modal or n: non-modal
Def.: Siemens AG (SAG) default setting, M: Milling: T: Turning or other conventions
MM.: Default setting, please see machine manufacturer's instructions
Group 1: Modally valid motion commands
Name No. Meaning X m/n SAG MM
G0 1. Rapid traverse m
G1 2. Linear interpolation (linear interpolation) m Def.
G2 3. Circular interpolation clockwise m
G3 4. Circular interpolation counter-clockwise m
CIP 5. Circle through points: Circular interpolation through intermediate point m
ASPLINE 6. Akima spline m
BSPLINE 7. B-spline m
CSPLINE 8. Cubic spline m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
480 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
POLY 9. Polynomial: Polynomial interpolation m
G33 10. Thread cutting with constant lead m
G331 11. Tapping m
G332 12. Retraction (tapping) m
OEMIPO1
##
13. Reserved m
OEMIPO2
##
14. Reserved m
CT 15. Circle with tangential transition m
G34 16. Increase in thread pitch (progressive change) m
G35 17. Decrease in thread pitch (degressive change) m
INVCW 18. Involute interpolation in CW direction m
INVCCW 19. Involute interpolation in CCW direction m
If no function from the group is programmed with modal G functions, the default setting
(which can be changed in the machine data) applies: $MC_GCODE_RESET_VALUES
## The keyword is not valid for SINUMERIK 810D/NCU571.
Group 2: Non-modally valid motions, dwell time
Name No. Meaning X m/n SAG MM
G4 1. Dwell time preset X n
G63 2. Tapping without synchronization X n
G74 3. Reference point approach with synchronization X n
G75 4. Fixed point approach X n
REPOSL 5. Repositioning linear: Linear repositioning X n
REPOSQ 6. Repositioning quadrant: Repositioning in a quadrant X n
REPOSH 7. Repositioning semicircle: Repositioning in semicircle X n
REPOSA 8. Repositioning linear all axis: Linear repositioning with all axes X n
REPOSQA 9. Repositioning quadrant all axes: Linear repositioning with all axes,
geometry axes in quadrant
X n
REPOSHA 10. Repositioning semicircle all axes: Repositioning with all axes; geometry
axes in semicircle
X n
G147 11. Soft approach with straight line X n
G247 12. Soft approach with quadrant X n
G347 13. Soft approach with semicircle X n
G148 14. Soft retraction with straight line X n
G248 15. Soft retraction with quadrant X n
G348 16. Soft retraction with semicircle X n
G05 17. Oblique plunge-cut grinding X n
G07 18. Compensatory motion during oblique plunge-cut grinding X n
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 481
Group 3: Programmable frame, working area limitation and pole programming
Name No. Meaning X m/n SAG MM
TRANS 1. TRANSLATION: translation, programmable X n
ROT 2. ROTATION: rotation, programmable X n
SCALE 3. SCALE: scaling, programming X n
MIRROR 4. MIRROR: Programmable mirroring X n
ATRANS 5. Additive TRANSLATION: additive translation, programming X n
AROT 6. Additive ROTATION: rotation, programmable X n
ASCALE 7. Additive SCALE: scaling, programming X n
AMIRROR 8. Additive MIRROR: Programmable mirroring X n
9. Unassigned
G25 10. Minimum working area limitation/spindle speed limitation X n
G26 11. Maximum working area limitation/spindle speed limitation X n
G110 12. Pole programming relative to the last programmed setpoint position X n
G111 13. Polar programming relative to origin of current workpiece coordinate
system
X n
G112 14. Pole programming relative to the last valid pole X n
G58 15. Programmable offset, absolute axial substitution X n
G59 16. Programmable offset, additive axial substitution X n
ROTS 17. Rotation with solid angles X n
AROTS 18. Additive rotation with solid angles X n
Group 4: FIFO
Name No. Meaning X m/n SAG MM
STARTFIFO 1. Start FIFO
Execute and simultaneously fill preprocessing memory
m Def.
STOPFIFO 2. STOP FIFO,
Stop machining; fill preprocessing memory until STARTFIFO is detected,
FIFO full or end of program
m
FIFOCTRL 3. FIFO CTRL,
Preprocessing memory control
m
Group 6: Plane selection
Name No. Meaning X m/n SAG MM
G17 1. Plane selection 1st - 2nd geometry axis m Def.
G18 2. Plane selection 3rd - 1st geometry axis m
G19 3. Plane selection 2nd - 3rd geometry axis m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
482 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Group 7: Tool radius compensation
Name No. Meaning X m/n SAG MM
G40 1. No tool radius compensation m Def.
G41 2. Tool radius compensation left of contour X m
G42 3. Tool radius compensation right of contour X m
Group 8: Settable zero offset
Name No. Meaning X m/n SAG MM
G500 1. Deactivate all settable G54-G57 frames if G500 does not contain a value m Def.
G54 2. Settable zero offset m
G55 3. Settable zero offset m
G56 4. Settable zero offset m
G57 5. Settable zero offset m
G505 6. Settable zero offset m
G5xx n+1 nth settable zero offset m
G599 100. Settable zero offset m
The G functions of this group activate a settable user frame $P_UIFR[ ].
G54 corresponds to frame $P_UIFR[1], G505 corresponds to frame $P_UIFR[5].
The number of settable user frames and, therefore, the number of G functions in this group
can be configured in the machine data $MC_MM_NUM_USER_FRAMES.
Group 9: Frame suppression
Name No. Meaning X m/n SAG MM
G53 1. Suppression of current frames:
Programmable frame including
system frame for TOROT and TOFRAME and
active settable frame G54 ... G599.
X n
SUPA 2. Suppression as for G153 and including
system frames for actual-value setting, scratching, zero offset external,
PAROT including handwheel offsets (DRF), [zero offset external],
overlaid motion
X n
G153 3. Suppression as for G53 and
including all channel-specific and/or NCU-global basic frame
X n
Group 10: Exact stop - continuous-path mode
Name No. Meaning X m/n SAG MM
G60 1. Velocity reduction, exact positioning m Def.
G64 2. Continuous-path mode m
G641 3. Continuous-path mode (G64) with programmable rounding distance m
G642 4. Corner rounding with axial precision m
G643 5. Block-internal axial corner rounding m
G644 6. Corner rounding with specified axis dynamics m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 483
Group 11: Exact stop, non-modal
Name No. Meaning X m/n SAG MM
G9 1. Velocity reduction, exact positioning X n
Group 12: Block change criteria at exact stop (G60/G09)
Name No. Meaning X m/n SAG MM
G601 1. Block change at exact stop fine m Def.
G602 2. Block change at exact stop coarse m
G603 3. Block change at IPO - end of block m
Group 13: Workpiece measuring inch/metric
Name No. Meaning X m/n SAG MM
G70 1. Input system inches (lengths) m
G71 2. Input system metric (lengths) m Def.
G700 3. Input system in inches; inch/min
(lengths + velocity + system variable)
m
G710 4. Input system, metric; mm; mm/min
(lengths + velocity + system variable)
m
Group 14: Workpiece measuring absolute/incremental
Name No. Meaning X m/n SAG MM
G90 1. Absolute dimensions m Def.
G91 2. Incremental dimension input m
Group 15: Feed type
Name No. Meaning X m/n SAG MM
G93 1. Inverse-time feedrate 1/rpm m
G94 2. Linear feed mm/min, inch/min m Def.
G95 3. Revolutional feedrate in mm/rev, inch/rev m
G96 4. Constant cutting speed (type of feed as for G95) ON m
G97 5. Constant cutting speed (type of feed as for G95) OFF m
G931 6. Feedrate specified by travel time, deactivate constant path velocity m
G961 7. Constant cutting speed (type of feed as for G94) ON m
G971 8. Constant cutting speed (type of feed as for G94) OFF m
G942 9. Freeze linear feedrate and constant cutting rate or spindle speed m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
484 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G952 10. Freeze revolutional feedrate and const. cutting rate or spindle speed m
G962 11. Linear or revolutional feedrate and constant cutting rate m
G972 12. Freeze linear or revolutional feedrate and constant spindle speed m
G973 13 Revolutional feedrate without spindle speed limiting
(G97 without LIMS for ISO mode
m
G963 Reserved m
Group 16: Feedrate override on inside and outside curvature
Name No. Meaning X m/n SAG MM
CFC 1. Constant feed at contour
m Def.
CFTCP 2. Constant feed in tool center point
(center-point path)
m
CFIN 3. Constant feed at internal radius, acceleration at external radius
m
Group 17: Approach and retraction response, tool offset
Name No. Meaning X m/n SAG MM
NORM 1. Normal position at start and end points m Def.
KONT 2. Travel around contour at start and end points m
KONTT 3. Insert polynominal with constant tangent (approach/retract) m
KONTC 4. Insert polynominal with constant curvature (approach/retract) m
Group 18: Corner behavior, tool offset
Name No. Meaning X m/n SAG MM
G450 1. Transition circle
(tool travels round workpiece corners on a circular path)
m Def.
G451 2. Intersection of equidistant paths
(tool backs off from the workpiece corner)
m
Group 19: Curve transition at beginning of spline
Name No. Meaning X m/n SAG MM
BNAT 1. Begin natural: natural transition to first spline block m Def.
BTAN 2. Begin tangential: tangential transition to first spline block m
BAUTO 3. Begin not a node: (no node) Start is determined by the position of the
1st point
m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 485
Group 20: Curve transition at end of spline
Name No. Meaning X m/n SAG MM
ENAT 1. End natural: natural transition to next traversing block m Def.
ETAN 2. End tangential: tangential transition to next traversing block at spline
begin
m
EAUTO 3. Begin not a node: (no node) End is determined by the position of the last
point
m
Group 21: Acceleration profile
Name No. Meaning X m/n SAG MM
BRISK 1. Fast non-smoothed path acceleration m Def.
SOFT 2. Soft smoothed path acceleration m
DRIVE 3. Velocity-dependent path acceleration m
Group 22: Tool offset types
Name No. Meaning X m/n SAG MM
CUT2D 1. Cutter compensation type 2-dimensional 2 1/2D tool offset determined by
G17 – G19
m Def.
CUT2DF 2. Cutter compensation type 2-dimensional frame – relative: 2 1/2D tool
offset determined by frame
The tool offset is effective in relation to the current frame
(inclined plane)
m
CUT3DC # 3. Cutter compensation type 3-dimensional circumference: 3D tool
compensation circumference milling
m
CUT3DF # 4. Cutter compensation type 3-dimensional face: 3D tool offset with
inconstant tool orientation
m
CUT3DFS # 5. Cutter compensation type 3-dimensional face: 3D tool offset face milling
with constant tool orientation independent of active frame
m
CUT3DFF # 6. Cutter compensation type 3-dimensional face frame: 3D tool offset face
milling with constant tool orientation dependent on active frame
m
CUT3DCC # 7. Cutter compensation type 3-dimensional circumference: 3D tool offset
circumferential milling with limitation surfaces
m
CUT3DCCD # 8. Cutter compensation type 3-dimensional circumference: 3D tool offset
circumferential milling with limitation surfaces with differential tool
m
# The keyword is not valid for SINUMERIK 810D/NCU571.
Tables
12.3 List of G functions/preparatory functions
Fundamentals
486 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Group 23: Collision monitoring at inside contours
Name No. Meaning X m/n SAG MM
CDOF 1. Collision detection OFF: Collision monitoring OFF m Def.
CDON 2. Collision detection ON: Collision monitoring ON m
CDOF2 3. Collision detection OFF: Collision monitoring OFF
(currently only for CUT3DC)
m
Group 24: Feedforward control
Name No. Meaning X m/n SAG MM
FFWOF 1. Feed forward OFF: Feedforward control OFF m Def.
FFWON 2. Feed forward OFF: Feed forward control ON m
Group 25: Tool orientation reference
Name No. Meaning X m/n SAG MM
ORIWKS # 1. Tool orientation in workpiece coordinate system: Tool orientation in
workpiece coordinate system (WCS)
m Def.
ORIMKS # 2. Tool orientation in machine coordinate system: Tool orientation in
machine coordinate system (MCS)
m
# The keyword is not valid for SINUMERIK 810D/NCU571.
Group 26: Repositioning point for REPOS
Name No. Meaning X m/n SAG MM
RMB 1. REPOS mode beginning of block: Reapproach to start of block position m
RMI 2. REPOS – Mode interrupt: Reapproach to interruption point m Def.
RME 3. REPOS mode end of block: Repositioning to end-of-block position m
RMN 4. REPOS mode end of nearest orbital block: Reapproach to nearest path
point
m
Group 27: Tool offset for change in orientation at outside corners
Name No. Meaning X m/n SAG MM
ORIC # 1. Orientation change continuously: Orientation changes at outside corners
are superimposed on the circle block to be inserted
m Def.
ORID # 2. Orientation change discontinuously: Orientation changes are performed
before the circle block
m
# The keyword is not valid for SINUMERIK 810D/NCU571.
Group 28: Working area limitation ON/OFF
Name No. Meaning X m/n SAG MM
WALIMON 1. Working area limitation ON: Working area limitation ON m Def.
WALIMOF 2. Working area limitation OFF: Working area limitation OFF m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 487
Group 29: Radius - diameter
Name No. Meaning X m/n SAG MM
DIAMOF 1. Diameter programming OFF: Diameter programming OFF; radius
programming for G90/G91
m Def.
DIAMON 2. Diameter programming ON: Diameter programming ON for G90/G91 m
DIAM90 3. Diameter programming G90: Diameter programming for G90; radius
programming for G91
m
DIAMCYCOF 4. Diameter programming OFF: Radius programming for G90/G91: ON. The
G-code of this group that was last active remains active for display
m
Group 30: Compressor ON/OFF
Name No. Meaning X m/n SAG MM
COMPOF # 1. Compressor OFF m Def.
COMPON # 2. Compressor ON m
COMPCURV
#
3. Compressor ON: Polynomials with constant curvature m
COMPCAD # 4. Compressor ON: Optimized surface quality CAD program m
Group 31: OEM - G group
Name No. Meaning X m/n SAG MM
G810 # 1. OEM - G function Def.
G811 # 2. OEM - G function
G812 # 3. OEM - G function
G813 # 4. OEM - G function
G814 # 5. OEM - G function
G815 # 6. OEM - G function
G816 # 7. OEM - G function
G817 # 8. OEM - G function
G818 # 9. OEM - G function
G819 # 10. OEM - G function
Two G groups are reserved for the OEM. This enables the OEM to program functions that
can be customized.
# The keyword is not valid for SINUMERIK 810D/NCU571.
Group 32: OEM - G group
Name No. Meaning X m/n SAG MM
G820 # 1. OEM - G function Def.
G821 # 2. OEM - G function
G822 # 3. OEM - G function
G823 # 4. OEM - G function
Tables
12.3 List of G functions/preparatory functions
Fundamentals
488 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
G824 # 5. OEM - G function
G825 # 6. OEM - G function
G826 # 7. OEM - G function
G827 # 8. OEM - G function
G828 # 9. OEM - G function
G829 # 10. OEM - G function
Two G groups are reserved for the OEM. This enables the OEM to program functions that
can be customized.
Group 33: Settable fine tool offset
Name No. Meaning X m/n SAG MM
FTOCOF # 1. Fine tool offset compensation OFF: Online fine tool offset OFF m Def.
FTOCON # 2. Fine tool offset compensation ON: Online fine tool offset ON X m
Group 34: Smoothing, tool orientation
Name No. Meaning X m/n SAG MM
OSOF # 1. Tool orientation smoothing OFF m Def.
OSC # 2. Continuous tool orientation smoothing m
OSS # 3. Tool orientation smoothing at end of block m
OSSE # 4. Tool orientation smoothing at start and end of block m
OSD # 5 Block-internal rounding with specification of path length m
OST # 6 Block-internal rounding with specification of angle tolerance m
Group 35: Punching and nibbling
Name No. Meaning X m/n SAG MM
SPOF# 1. Stroke/punch OFF: Stroke OFF, nibbling, punching OFF m Def.
SON # 2. Stroke ON: Nibbling ON m
PON # 3. Punch ON: Punching ON m
SONS # 4. Stroke ON slow: Nibbling ON in IPO cycle X m
PONS # 5. Punch ON slow: Punching ON in IPO cycle X m
Group 36: Punching with delay
Name No. Meaning X m/n SAG MM
PDELAYON
#
1. Punch with delay ON: Punching with delay ON m Def.
PDELAYOF
#
2. Punch with delay OFF: Punching with delay OFF m
# The keyword is not valid for SINUMERIK 810D/NCU571.
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 489
Group 37: Feed profile
Name No. Meaning X m/n SAG MM
FNORM # 1. Feed normal: Feed normal (as per DIN 66025) m Def.
FLIN # 2. Feed linear: Feed linear variable m
FCUB # 3. Feed cubic: Feedrate variable according to cubic spline m
Group 38: Assignment of high-speed inputs/outputs for punching/nibbling
Name No. Meaning X m/n SAG MM
SPIF1 # 1. Stroke/punch interface 1: fast NCK inputs/outputs for punching/nibbling
byte 1
m Def.
SPIF2 # 2. Stroke/punch interface 2: fast NCK inputs/outputs for punching/nibbling
byte 2
m
Group 39: Programmable contour accuracy
Name No. Meaning X m/n SAG MM
CPRECOF 1. Contour precision OFF: Programmable contour precision OFF m Def.
CPRECON 2. Contour precision ON: Programmable contour precision ON m
#The keyword is not valid for SINUMERIK NCU571.
Group 40: Tool radius compensation constant
Name No. Meaning X m/n SAG MM
CUTCONOF 1. Constant radius compensation OFF m Def.
CUTCONON 2. Constant radius compensation ON m
Group 41: Interrupt thread cutting
Name No. Meaning X m/n SAG MM
LFOF 1. Interrupt thread cutting OFF m Def.
LFON 2. Interrupt thread cutting ON m
Group 42: Toolholder
Name No. Meaning X m/n SAG MM
TCOABS 1. Tool Carrier Orientation Absolute: Toolholder orientation absolute m Def.
TCOFR 2. Toolholder orientation frame alignment of tool on
Z axis
m
TCOFRZ 3. Orientable toolholder frame-related (tool on Z axis) m
TCOFRY 4. Orientable toolholder frame-related (tool on Y axis) m
TCOFRX 5. Orientable toolholder frame-related (tool on X axis) m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
490 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Group 43: SAR approach direction
Name No. Meaning X m/n SAG MM
G140 1. SAR approach direction defined by G41/G42 m Def.
G141 2. SAR approach direction to left of contour m
G142 3. SAR approach direction to right of contour m
G143 4. SAR approach direction tangent-dependent m
Group 44: SAR path segmentation
Name No. Meaning X m/n SAG MM
G340 1. Spatial approach block (depth and in plane (helix)) m Def.
G341 2. Initial infeed on perpendicular axis (z), then approach in plane m
Group 45: Path reference for FGROUP axes:
Name No. Meaning X m/n SAG MM
SPATH 1. Path reference for FGROUP axes is arc length m Def.
UPATH 2. Path reference for FGROUP axes is curve parameter m
Group 46: Plane definition for rapid lift:
Name No. Meaning X m/n SAG MM
LFTXT 1. Tangential tool direction on retraction m Def.
LFWP 2. Non-tangential tool direction on retraction m
LFPOS 3. Axial retraction to a position m
Group 47: Mode switchover for external NC code
Name No. Meaning X m/n SAG MM
G290 1. Switchover to SINUMERIK mode
(activate SINUMERIK language mode)
m Def.
G291 2. Switchover to ISO 2/3 mode (activate ISO language mode) m
Group 48: Approach and retraction response, TRC
Name No. Meaning X m/n SAG MM
G460 1. Collision monitoring for approach and retraction block ON m Def.
G461 2. If no intersection in TRC block, extend border block with arc m
G462 3. If no intersection in TRC block, extend border block with straight line m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 491
Group 49: Point to point motion
Name No. Meaning X m/n SAG MM
CP 1. continuous path; path motion m Def.
PTP 2. point to point; point to point motion (synchronized axis motion) m
PTPG0 3. point to point; point to point motion only with G0, otherwise path motion
CP
m
Group 50: Orientation programming
Name No. Meaning X m/n SAG MM
ORIEULER 1. Orientation angle via Euler angle m Def.
ORIRPY 2. Orientation angle via RPY angle (rotation sequence XYZ) m
ORIVIRT1 3. Orientation angle via virtual orientation axes (definition 1) m
ORIVIRT2 4. Orientation angle via virtual orientation axes (definition 2) m
ORIAXPOS 5. Orientation angle via virtual orientation axes with rotary axis positions m
ORIRPY2 6. Orientation angle via RPY angle (rotation sequence ZYX) m
Group 51: Orientation interpolation
Name No. Meaning X m/n SAG MM
ORIVECT 1. Large-radius circular interpolation (identical to ORIPLANE) m Def.
ORIAXES 2. Linear interpolation of machine axes or orientation axes m
ORIPATH 3. Tool orientation trajectory referred to path m
ORIPLANE 4. Interpolation in plane (identical to ORIVECT) m
ORICONCW 5. Interpolation on a peripheral surface of the cone in clockwise direction m
ORICONCCW 6. Interpolation on a conical peripheral surface in CCW direction m
ORICONIO 7. Interpolation on a conical peripheral surface with intermediate
orientation setting
m
ORICONTO 8. Interpolation on a peripheral surface of the cone with tangential
transition
m
ORICURVE 9. Interpolation with additional space curve for orientation m
ORIPATHS 10. Tool orientation in relation to path, blips in the orientation characteristic
are smoothed
m
Group 52: Workpiece-oriented WCS
Name No. Meaning X m/n SAG MM
PAROTOF 1. Deactivate workpiece-related frame rotation m Def.
PAROT 2. Align workpiece coordinate system (WCS) on workpiece m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
492 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Group 53: Frame rotations in tool direction
Name No. Meaning X m/n SAG MM
TOROTOF 1. Frame rotation in tool direction OFF m Def.
TOROT 2. Frame rotation ON Z axis parallel to tool orientation m
TOROTZ 3. Frame rotation ON Z axis parallel to tool orientation m
TOROTY 4. Frame rotation ON Y axis parallel to tool orientation m
TOROTX 5. Frame rotation ON X axis parallel to tool orientation m
TOFRAME 6. Frame rotation in tool direction Z axis parallel to tool orientation m
TOFRAMEZ 7. Frame rotation in tool direction Z axis parallel to tool orientation m
TOFRAMEY 8. Frame rotation in tool direction Y axis parallel to tool orientation m
TOFRAMEX 9. Frame rotation in tool direction X axis parallel to tool orientation m
Group 54: Rotation of the rotational vector
Name No. Meaning X m/n SAG MM
ORIROTA 1. Orientation Rotation Absolute Rotation absolute m Def.
ORIROTR 2. Orientation Rotation Relative relative rotational vector m
ORIROTT 3. Orientation Rotation Tangential tangential rotational vector in relation to
change in orientation
m
ORIROTC 4. Orientation Rotation Tangential tangential rotational vector in relation to
path tangent
m
Group 55: Rapid traverse with/without linear interpolation
Name No. Meaning X m/n SAG MM
RTLION 1. Rapid traverse (G0) with linear interpolation ON: G0 with linear
interpolation
m Def.
RTLIOF 2. Rapid traverse (G0) with linear interpolation OFF: G0 without linear
interpolation (single-axis interpolation)
m
Tables
12.3 List of G functions/preparatory functions
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 493
Group 56: Inclusion of tool wear
Name No. Meaning X m/n SAG MM
TOWSTD 1. Tool wear default initial setting value for offsets in tool length m Def.
TOWMCS 2. Tool WearCoard MCS: Wear values in machine coordinate system
(MCS)
m
TOWWCS 3. Tool WearCoard WCS: Wear values in workpiece coordinate system
(WCS)
m
TOWBCS 4. Tool WearCoard BCS: Wear values in basic coordinate system (MCS) m
TOWTCS 5. Tool WearCoard TCS: Wear values in the tool coordinate system (tool
carrier ref. point T at the tool holder)
m
TOWKCS 6. Wear values in the coordinate system of the tool head for kinetic
transformation (differs from
MCS by tool rotation)
m
Group 57: Automatic corner override
Name No. Meaning X m/n SAG MM
FENDNORM 1. Corner deceleration deactivated m Def.
G62 2. Corner deceleration at inside corners when tool radius offset is active m
G621 3. Corner deceleration at all corners m
Group 58: Reserved for retracting from software end position
Name No. Meaning X m/n SAG MM
RELIEVEON 1. Retracting from software limit switch ON m
RELIEVEOF 2. Retracting from software limit switch OFF m Def.
Group 59: Technology G groups
Name No. Meaning X m/n SAG MM
DYNNORM 1. Standard dynamic, as previously m Def.
DYNPOS 2. Positioning mode, tapping m
DYNROUGH 3. Roughing m
DYNSEMIFIN 4. Finishing m
DYNFINISH 5. Smooth-finishing m
Group 60: Working-area limitations
Name No. Meaning X m/n SAG MM
WALCS0 1. WCS working area limitation deselected m Def.
WALCS1 2. WORK-working-area-limitation group 1 active m
WALCS2 3. WORK-working-area-limitation group 2 active m
WALCS3 4 WCS working area limitation group 3 active m
Tables
12.4 List of predefined subprograms
Fundamentals
494 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
WALCS4 5 WCS working area limitation group 4 active m
WALCS5 6 WCS working area limitation group 5 active m
WALCS6 7 WCS working area limitation group 6 active m
WALCS7 8 WCS working area limitation group 7 active m
WALCS8 9 WCS working area limitation group 8 active m
WALCS9 10 WCS working area limitation group 9 active m
WALCS10 11 WCS working area limitation group 10 active m
12.4 List of predefined subprograms
12.4.1 Predefined subroutine calls
List of predefined subroutines
The list of predefined subroutines contains all available subroutines grouped according to
function.
Some control functions are activated with subroutine call syntax.
1. Coordinate system
Keyword/
function
identifier
1st parameter 2nd parameter 3rd-15th
parameter
4th-16th
parameter
Explanation
PRESETON AXIS*:
Axis identifier
Machine axis
REAL:
Preset offset
G700/G7100
context
3.-15.
Parameter as
1 ...
4.-16.
parameter
as 2 ...
Sets the actual value for programmed
axes.
One axis identifier is programmed at a
time, with its respective value in the
next parameter.
PRESETON can be used to program
preset offsets for up to 8 axes.
DRFOF Deletes the DRF offset for all axes
assigned to the channel.
*) As a general rule, geometry or special axis identifiers can also be used instead of the
machine axis identifier, as long as the reference is unambiguous.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 495
Predefined subroutine calls
2. Axis groupings
1st-8th
parameter
Explanation
FGROUP Channel axis
identifiers
Variable F value reference: defines the axes to which the path feed refers.
Maximum axis number: 8
The default setting for the F value reference is activated with FGROUP ( ) without
parameters.
1st-8th
parameter
2nd-9th
parameter
Explanation
SPLINEPATH INT: Spline
group (must be
1)
AXIS:
Geometry or
special axis
identifier
Definition of the spline group
Maximum number of axes: 8
BRISKA AXIS Switch on brisk axis acceleration for the programmed axes
SOFTA AXIS Switch on jerk limited axis acceleration for programmed axes
DRIVEA ### AXIS Switch on knee-shaped acceleration characteristic for programmed
axes
JERKA AXIS The acceleration behavior set in machine data
$MA_AX_JERK_ENABLE is active for the programmed axes.
# The keyword is not valid for SINUMERIK 810D/NCU571.
## The keyword is not valid for SINUMERIK 810D.
### The keyword is only valid for SINUMERIK FM-NC.
3. Coupled motion
Keyword/
subroutine
identifier
1st parameter 2nd
param.
3rd
param.
4th
param.
5th
param.
6th
param.
Explanation
TANG AXIS: Axis
name
Following axis
AXIS:
Leading
axis 1
AXIS:
Leading
axis 2
REAL:
Coupling
factor
CHAR:
Option:
"B":
follow-up
in basic
coordinat
e system
"W":
follow-up
in work-
piece
coord.
system
CHAR
Optimizat
ion:
"S"
default"P
"
autom.
with
rounding
travel,
angle
tolerance
Preparatory statement for the
definition of a tangential
follow-up: The tangent for the
follow-up is determined by
the two master axes
specified. The coupling factor
specifies the relationship
between a change in the
angle of tangent and the
following axis. It is usually 1.
Optimization: See PGA
TANGON AXIS: Axis
name
Following axis
REAL:
Offset
Angle
REAL:
Round
-ing
travel
REAL:
Angle
toleranc
e
Tangential follow-up mode
ON:
par. 3, 4 with TANG Par. 6 =
"P"
Tables
12.4 List of predefined subprograms
Fundamentals
496 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
TANGOF AXIS: Axis
name
Following axis
Tangential follow-up mode
OFF
TLIFT AXIS: Following
axis
REAL:
Lift-off
path
REAL:
Factor
Tangential lift: tangential
follow-up mode, stop at
contour end
rotary axis lift-off possible
TRAILON AXIS: Following
axis
AXIS:
Master
axis
REAL:
Coupling
factor
Trailing ON: Asynchronous
coupled motion ON
TRAILOF AXIS: Following
axis
AXIS:
Master
axis
Trailing OFF: Asynchronous
coupled motion OFF
6. Revolutional feedrate
Keyword/
function
identifier
1st parameter 2nd parameter Explanation
FPRAON AXIS: Axis, for which
revolutional feedrate is
deactivated
AXIS: Axis/spindle from
which the revolutional
feedrate is derived.
If no axis has been
programmed, the
revolutional feedrate is
derived from the master
spindle.
Feedrate per revolution axial ON: Axial
revolutional feedrate ON
FPRAOF AXIS: Axis for which
revolutional feedrate is
deactivated
Feedrate per revolution axial OFF: Axial
revolutional feedrate OFF
The revolutional feedrate can be deactivated for
several axes at once. You can program as
many axes as are permitted in a block.
FPR AXIS: Axis/spindle from
which the revolutional
feedrate is derived.
If no axis has been
programmed, the
revolutional feedrate is
derived from the master
spindle.
Feedrate per revolution: selection of a rotary
axis or spindle from which the revolutional
feedrate of the path is derived if G95 is
programmed.
If no axis/spindle has been programmed, the
revolutional feedrate is derived from the master
spindle.
The setting made with FPR is modal.
It is also possible to program a spindle instead of an axis: FPR(S1) or FPR(SPI(1))
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 497
7. Transformations
Keyword/
function
identifier
1st parameter 2nd parameter Explanation
TRACYL REAL: Working
diameter
INT: Number
of
transformation
Cylinder: Peripheral surface transformation
Several transformations can be set per channel. The transformation
number specifies which transformation is to be activated. If the
second parameter is omitted, the transformation group defined in
the MD is activated.
TRANSMIT INT: Number of
transformation
Transmit: Polar transformation
Several transformations can be set per channel. The transformation
number specifies which transformation is to be activated. If the
parameter is omitted, the transformation group defined in the MD is
activated.
TRAANG REAL: Angle INT: Number
of
transformation
Transformation inclined axis:
Several transformations can be set per channel. The transformation
number specifies which transformation is to be activated. If the
second parameter is omitted, the transformation group defined in
the MD is activated. If no angle programmed:
TRAANG ( ,2) or TRAANG, the last angle applies modally.
TRAORI INT: Number of
transformation
Transformation oriented: 4, 5-axis transformation
Several transformations can be set per channel. The transformation
number specifies which transformation is to be activated.
TRACON INT: Number of
transformation
REAL: Further
parameters,
MD-dependent
Transformation concentrated: Cascaded transformation; the
meaning of the parameters depends on the type of cascading.
TRAFOOF Deactivate transformation
For each transformation type, there is one command for one transformation per channel. If
there are several transformations of the same transformation type per channel, the
transformation can be selected with the corresponding command and parameters. It is
possible to deselect the transformation by a transformation change or an explicit deselection.
8. Spindles
Keyword/
subroutine
identifier
1st parameter 2nd parameter
and others
Explanation
SPCON INT: Spindle
number
INT: Spindle
number
Spindle position control ON: Switch to position-controlled spindle
operation
SPCOF INT: Spindle
number
INT: Spindle
number
Spindle position control OFF: Switch to speed-controlled spindle
operation
SETMS INT: Spindle
number
Set master spindle: Declaration of spindle as master spindle for
current channel.
With SETMS( ), the machine-data default applies automatically
without any need for parameterization.
Tables
12.4 List of predefined subprograms
Fundamentals
498 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
9. Grinding
Keyword/
subroutine
identifier
1st parameter Explanation
GWPSON INT: Spindle
number
Grinding wheel peripheral speed ON: Constant grinding wheel peripheral speed ON
If the spindle number is not programmed, then grinding wheel peripheral speed is
selected for the spindle of the active tool.
GWPSOF INT: Spindle
number
Grinding wheel peripheral speed OFF. Constant grinding wheel peripheral speed
OFF.
If the spindle number is not programmed, grinding wheel peripheral speed is
deselected for the spindle of the active tool.
TMON INT: Spindle
number
Tool monitoring ON:
If no T number is programmed, monitoring is activated for the active tool.
TMOF INT: T number Tool monitoring OFF:
If no T number is programmed, monitoring is deactivated for the active tool.
10. Stock removal
Keyword/
subroutine
identifier
1st parameter 2nd parameter 3rd
parameter
4th
parameter
Explanation
CONTPRON REAL [ , 11]:
Contour table
CHAR: Stock
removal
method
"L":
Longitudinal
turning:
External mach.
"P": Face
turning:
External mach.
"N": Face
turning: Internal
machining
"G":
Longitudinal
turning: Internal
machining
INT: Number
of relief cuts
INT: Status
of
calculation:
0:
unchanged
1:
Calculation
forwards
and
backwards
Contour preparation on: Activate
reference-point editing.
The contour programs or NC blocks
which are called in the following steps
are divided into individual movements
and stored in the contour table.
The number of relief cuts is returned.
CONTDCON REAL [ , 6]:
Contour table
INT:
0: in
programmed
direction
Contour decoding
The blocks for a contour are stored in a
named table with one table line per
block and coded to save memory.
EXECUTE INT: Error
status
EXECUTE: Activate program
execution.
This switches back to normal program
execution from reference-point-editing
mode or after setting up a protection
zone.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 499
11. Execute table
Keyword/
subroutine
identifier
1st parameter Explanation
EXECTAB REAL [ 11]:
Element from
motion table
Execute table: Execute an element from a motion table.
12. Protection zones
Keyword/
function
identifier
1st parameter 2nd parameter 3rd parameter 4th parameter 5th parameter Explanation
CPROTDEF INT: Number of
protection zone
BOOL:
TRUE:
Tool-oriented
protection zone
INT:
0: 4. U.G.
Parameters not
evaluated
1: 4. Parameter
evaluated
2: 5. Parameter
evaluated
3: 4. U. 5.
Parameter
evaluated
REAL: Limit in
plus direction
REAL: Limit in
minus direction
Channel-
specific
protection
area
definition:
Definition of
a channel-
specific
protection
zone
NPROTDEF INT: Number of
protection zone
BOOL:
TRUE:
Tool-oriented
protection zone
INT:
0: 4. U. 5.
parameters not
evaluated
1: 4. Parameter
evaluated
2: 5. Parameter
evaluated
3: 4. U. 5.
parameter
evaluated
REAL: Limit in
plus direction
REAL: Limit in
minus direction
NCK-
specific
protection
area
definition:
Definition of
a machine-
specific
protection
zone
Tables
12.4 List of predefined subprograms
Fundamentals
500 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
CPROT INT: Number of
protection zone
INT: Option
0: Protection
zone OFF
1: Preactivate
protection zone
2: Protection
zone ON
3: Preactivate
protection zone
with conditional
stop, only with
protection zones
active.
REAL: Offset of
protection zone
in 1st geometry
axis
REAL: Offset of
protection zone
in 2nd geometry
axis
REAL: Offset of
protection zone
in 3rd geometry
axis
Channel-
specific
protection
zone
ON/OFF
NPROT INT: Number of
protection zone
INT: Option
0: Protection
zone OFF
1: Preactivate
protection zone
2: Protection
zone ON
3: Preactivate
protection zone
with conditional
stop, only with
protection zones
active
REAL: Offset of
protection zone
in 1st geometry
axis
REAL: Offset of
protection zone
in 2nd geometry
axis
REAL: Offset of
protection zone
in 3rd geometry
axis
Machine-
specific
protection
zone
ON/OFF
EXECUTE VAR INT: Error
status
EXECUTE: Activate program execution. This switches back to normal program
execution from reference point editing mode or after setting up a protection zone.
13. Preprocessing/single block
STOPRE Stop processing: Preprocessing stop until all prepared blocks are executed in main
run
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 501
14. Interrupts
Keyword/
function
identifier
1st parameter Explanation
ENABLE # INT: Number of
interrupt input
Activate interrupt: Activates the interrupt routine assigned to the hardware input with
the specified number. An interrupt is enabled after the SETINT statement.
DISABLE # INT: Number of
interrupt input
Deactivate interrupt: Deactivates the interrupt routine assigned to the hardware input
with the specified number. Fast retraction is not executed. The assignment between
the hardware input and the interrupt routine made with SETINT remains valid and can
be reactivated with ENABLE.
CLRINT # INT: Number of
interrupt input
Select interrupt: Cancel the assignment of interrupt routines and attributes to an
interrupt input. The interrupt routine is deactivated and no reaction occurs when the
interrupt is generated.
#The keyword is not valid for SINUMERIK 810D.
15. Motion synchronization
CANCEL INT: Number of
synchronized
action
Aborts the modal motion-synchronous action with the specified ID
16. Function definition
1st parameter 2nd parameter 3rd parameter 4th-7th
parameter
Explanation
FCTDEF INT: Function
number
REAL: Lower
limit value
REAL: Upper
limit value
REAL:
Coefficients a0
– a3
Define polynomial. This is
evaluated in SYFCT or
PUTFTOCF.
17. Communication
Keyword/su
broutine
identifier
1st
parameter
2nd parameter Explanation
MMC # STRING:
Command
CHAR:
Acknowledgement mode**
"N": Without acknowledgment
"S": Synchronous acknowledgment
"A": Asynchronous acknowledgment
MMC command: Command ON
MMC command interpreter for the configuration of
windows via NC program
see /AM/IM1 Start-Up Functions for the MMC
#)The keyword is not valid for SINUMERIK 810D.
**)Acknowledgement mode:
Commands are acknowledged on request from the executing component (channel, NC,
etc.).
Without acknowledgement: Program execution is continued when the command has been
transmitted. The sender is not informed if the command cannot be executed successfully.
Tables
12.4 List of predefined subprograms
Fundamentals
502 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
18. Program coordination
Keyword/su
broutine
identifier
1st
parameter
2nd
parameter
3rd
parameter
4th
parameter
5th
param
eter
6th-8th
param
eter
Explanation
INIT # INT:
Channel
numbers
1 - 10
or STRING:
Channel
name
$MC_CHAN
_NAME
STRING:
path
CHAR:
acknowledg
ement
mode**
Selection of a module for
execution in a channel.
1 : 1st channel;
2 : 2. channel.
As an alternative to the channel
number, the channel name
defined in $MC_CHAN_NAME
can also be used.
START # INT:
Channel
numbers
1 - 10
or STRING:
Channel
name
$MC_CHAN
_NAME
Starts selected programs
simultaneously on multiple
channels from running program.
The command has no effect on
the existing channel.
1 : 1st channel;
2 : 2nd channel or channel
name defined in
$MC_CHAN_NAME.
WAITE # INT: or
channel
numbers
1 - 10
STRING:
Channel
name
$MC_CHAN
_NAME
Wait for end of program: Waits
until end of program in another
channel (number or name).
WAITM # INT: Marker
number
0-9
INT:
Channel
numbers
1 - 10
or STRING:
Channel
name
$MC_CHAN
_NAME
Wait: Wait for a marker to be
reached in other channels. The
program waits until the WAITM
with the relevant marker has
been reached in the other
channel. The number of the
own channel can also be
specified.
WAITMC # INT: Marker
number
0-9
INT:
Channel
numbers
1 - 10
or STRING:
Channel
name
$MC_CHAN
_NAME
Wait: Waits conditionally for a
marker to be reached in other
channels. The program waits
until the WAITMC with the
relevant marker has been
reached in the other channel.
Exact stop only if the other
channels have not yet reached
the marker.
WAITP AXIS: Axis
identifier
AXIS: Axis
identifier
AXIS: Axis
identifier
AXIS: Axis
identifier
AXIS:
Axis
ident-
ifier
AXIS:
Axis
ident-
ifier
Wait for positioning axis: Wait
for positioning axes to reach
their programmed endpoint.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 503
WAITS INT: Spindle
number
INT: Spindle
number
INT: Spindle
number
INT: Spindle
number
INT:
Spindl
e
numbe
r
Wait for positioning spindle:
Wait until programmed spindles
previously programmed with
SPOSA reach their
programmed endpoint.
RET End of subroutine with no
function output to the PLC.
GET # AXIS AXIS AXIS AXIS AXIS AXIS Assign machine axis
GETD# AXIS AXIS AXIS AXIS AXIS AXIS Assign machine axis directly
RELEASE # AXIS AXIS AXIS AXIS AXIS AXIS Release machine axis
PUTFTOC # REAL:
Offset value
INT:
Parameter
number
INT:
Channel
number or
STRING:
Channel
name
$MC_CHAN
_NAME
INT: Spindle
number
Put fine tool correction: Fine
tool compensation
PUTFTOCF
#
INT:
No. of
function
The number
used here
must be
specified in
FCTDEF.
VAR REAL:
Reference
value *)
INT:
Parameter
number
INT:
Channel
numbers
1 - 10
or STRING:
Channel
name
$MC_CHAN
_NAME
INT:
Spindl
e
numbe
r
Put fine tool correction function
dependent:
Change online tool
compensation according to a
function defined with FCTDEF
(max. 3rd degree polynomial).
The SPI function can also be used to program a spindle instead of an axis: GET(SPI(1))
#)The keyword is not valid for SINUMERIK FM-NC/NCU571.
**) Acknowledgment mode:
Commands are acknowledged on request from the executing component (channel, NC,
etc.).
Without acknowledgement: Program execution is continued when the command has been
transmitted. The executing component is not informed if the command cannot be executed
successfully. Acknowledgment mode "N" or "n".
Synchronous acknowledgement: The program execution is paused until the receiving
component acknowledges the command. If the acknowledgement is positive, the next
command is executed.
If the acknowledgement is negative an error is output.
Acknowledgement "S", "s" or to be omitted.
For some commands, the acknowledgement response is predefined, for others it is
programmable.
The acknowledgement response for program-coordination commands is always
synchronous.
If the acknowledgement mode is not specified, synchronous acknowledgement is the default
response.
Tables
12.4 List of predefined subprograms
Fundamentals
504 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
19. Data access
1st
parameter
Explanation
CHANDATA INT:
Channel
number
Set channel number for channel data access (only permitted in initialization block);
the subsequent accesses refer to the channel set with CHANDATA.
20. Messages
1st
parameter
2nd
parameter
Explanation
MSG STRING:
STRING:
signal
INT:
Continuous-
path-mode
call
parameter
Message modal: The message is active until the next message is queued.
If the 2nd parameter = 1 is programmed, e.g., MSG(Text, 1), the message will
even be output as an executable block in continuous-path mode.
22. Alarms
1st
parameter
2nd
parameter
Explanation
SETAL INT: Alarm
number
(cycle
alarms)
STRING:
Character
string
Set alarm: Sets alarm. A character string with up to 4 parameters can be
specified in addition to the alarm number.
The following predefined parameters are available:
%1 = channel number
%2 = block number, label
%3 = text index for cycle alarms
%4 = additional alarm parameters
23. Compensation
Keyword/su
broutine
identifier
1st
parameter-
4th
parameter
Explanation
QECLRNO
N
AXIS: Axis
number
Quadrant error compensation learning ON Quadrant error compensation
learning ON
QECLRNOF Quadrant error compensation learning OFF: Quadrant error compensation
learning OFF
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 505
24. Tool management
1st parameter 2nd parameter 3rd
parameter
Explanation
DELT STRING[32]: Tool
designation
INT: Duplo
number
Delete tool. Duplo number can be
omitted.
GETSELT VAR INT:
T number (return
value)
INT: Spindle
number
Get selected T number. If no spindle
number is specified, the command
for the master spindle applies.
SETPIECE INT: Count INT: Spindle
number
Takes account of set piece number
for all tools assigned to the spindle.
If no spindle number is specified, the
command for the master spindle
applies.
SETDNO INT: Tool number T INT: Tool
edge no.
INT: D No. Set D no. of tool (T) and its tool
edge to new
DZERO Set D numbers of all tools of the TO
unit assigned to the channel to
invalid
DELDL INT: Tool number T INT: D No. Delete all additive offsets of the tool
edge (or of a tool if D is not
specified)
SETMTH INT: Tool-holder
no.
Set toolholder no.
POSM INT: Location no.
for positioning
INT: No. of the
magazine to
be moved
INT:
Location
number of
the internal
magazine
INT:
Magazine
number of
the internal
magazine
Position magazine
SETTIA VAR INT:
Status=result of
operation (return
value)
INT: Magazine
number
INT: Wear
grouping no.
Deactivate tool from wear group
SETTA VAR INT:
Status=result of
operation (return
value)
INT: Magazine
number
INT: Wear
grouping no.
Activate tool from wear group
RESETMON VAR INT:
Status=result of
operation (return
value)
INT: Internal T
no.
INT: D no. of
tool
Set actual value of tool to setpoint
#) The keyword is not valid for SINUMERIK FM-NC.
Tables
12.4 List of predefined subprograms
Fundamentals
506 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
25. Synchronous spindle
1st para-
meter
2nd
para-
meter
3rd para-
meter
4th para-
meter
5th parameter
Block change behavior
6th
parameter
Explanation
COUPDEF
#
AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
REAL:
Numerat
or
transfor
mation
ratio (FA)
or (FS)
REAL:
Denomin
ator
transfor
mation
ratio (LA)
or (LS)
STRING[8]: Block change behavior:
"NOC": no block change control,
block change is enabled
immediately, "FINE": block change
on "synchronism fine", "COARSE":
block change on synchronism
coarse and "IPOSTOP": block
change in setpoint-dependent
termination of overlaid movement. If
the block change behavior is not
specified, the set behavior is
applicable and there is no change.
STRING[2]:
"DV":
Setpoint
coupling
"AV":
Actual-
value
coupling
Couple
definition:
definition of
synchronized
spindle grouping
COUPDEL # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
Couple delete:
Delete
synchronous
spindle group
COUPOF # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
The block change is enabled
immediately.
Fastest possible
deactivation of
synchronous
operation.
COUPOF # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
REAL:
POSFS
Block change is not enabled until
this position has been crossed.
Deselection of
synchronous
operation after
deactivation
position POSFS
has been
crossed
COUPOF # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
REAL:
POSFS
REAL:
POSLS
Block change is not enabled until
both programmed positions have
been crossed. Range of
POSFS, POSLS: 0 ... 359.999
degrees.
Deselection of
synchronous
operation after
the two
deactivation
positions
POSFS and
POSLS have
been crossed.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 507
COUPOFS
# AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
Block change performed as quickly
as possible with immediate block
change.
Deactivation of
couple with
following-spindle
stop.
COUPOFS
#
AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
REAL:
POSFS
After the programmed deactivation
position that refers to the machine
coordinate system has been
crossed, the block change is not
enabled until the deactivation
positions POSFS have been
crossed.
Value range 0 ... 359.999 degrees.
Only deactivated
after
programmed
following-axis
deactivation
position has
been crossed.
COUPON # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
The block change is enabled
immediately.
Fastest possible
activation of
synchronous
operation with
any angular
reference
between the
leading and
following
spindles.
COUPON # AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
REAL:P
OSFS
The block change is enabled
according to the defined setting.
Range of POSFS: 0 ... 359.999
degrees.
Activation with a
defined angular
offset
POSFSbetween
the following and
leading spindles.
This offset is
referred to the
zero degrees
position of the
leading spindle
in a positive
direction of
rotation.
COUPONC
#
AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
An offset
position
cannot
be
program
med.
Acceptance of
activation with
previously
programmed
M3 S.. or M4 S...
Immediate
acceptance of
rotational speed
difference.
Tables
12.4 List of predefined subprograms
Fundamentals
508 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
COUPRES
#
AXIS:
Followin
g axis or
following
spindle
(FS)
AXIS:
Leadin
g axis
or
leading
spindle
(LS)
Couple reset:
Reset
synchronous
spindle group.
The pro-
grammed values
become invalid.
The machine
data values are
valid.
For synchronous spindles, the axis parameters are programmed with SPI(1) or S1.
26. Structure statements in the STEP editor (editor-based program support)
1st parameter 2nd parameter 3rd parameter Explanation
SEFORM STRING[128]:
section name
INT: level STRING[128]:
icon
Current section name for STEP
editor
#) The keyword is not valid for SINUMERIK 810 D.
Keyword/su
broutine
identifier
1st
parameter
2nd
parameter
3rd
parameter
4th
parameter
Explanation
COUPON # AXIS:
Following
axis
AXIS:
Master axis
REAL:
Activation
position of
following
axis
Couple on:
Activate ELG group/synchronous spindle pair. If
no activation positions are specified, the couple is
activated as quickly as possible (ramp). If an
activation position is specified for the following
axis and spindle, this refers absolutely or
incrementally to the master axis or spindle.
Parameters 4 and 5 only have to be programmed
if the 3rd parameter is specified.
COUPOF # AXIS:
Following
axis
AXIS:
Master axis
REAL:
Deactivation
position of
following
axis
(absolute)
REAL:
Deactivation
position of
master axis
(absolute)
Couple OFF:
Deactivate ELG group/synchronous spindle pair.
The couple parameters are retained. If positions
are specified, the couple is only canceled when all
the specified positions have been overtraveled.
The following spindle continues to revolve at the
last speed programmed before deactivation of the
couple.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 509
WAITC # AXIS: Axis/
spindle
STRING[8]:
Block
change
criterion
AXIS: Axis/
spindle
STRING[8]:
Block
change
criterion
Wait for couple condition:
Wait until couple block change criterion for the
axes/spindles is fulfilled.
Up to 2 axes/spindles can be programmed.
Block change criterion:
"NOC": no block change control, block change is
enabled immediately,
"FINE": block change on "synchronism fine",
"COARSE": block change on synchronism coarse
and
"IPOSTOP": Block change in setpoint-dependent
termination of overlaid movement.
If the block change behavior is not specified, the
set behavior is applicable and there is no change.
AXCTSWE AXIS:
Axis/spindle
Advance container axis
#)The keyword is not valid for SINUMERIK 810D.
12.4.2 Predefined subroutine calls in motion-synchronous actions
Predefined subroutine calls in motion-synchronous actions
27. Synchronous procedures
Keyword/
function
identifier
1st parameter 2nd parameter 3rd parameter
to
5th parameter
Explanation
STOPREOF Stop preparation OFF:
A synchronized action with a STOPREOF
command causes a preprocessing stop after the
next output block (= block for the main run). The
preprocessing stop is canceled with the end of the
output block or when the STOPREOF condition is
fulfilled. All synchronized action instructions with the
STOPREOF command are therefore interpreted as
having been executed.
RDISABLE Read-in disable Read-in disable
DELDTG AXIS: Axis for
axial delete
distance-to-go
(optional). If the
axis is omitted,
delete distance-
to-go is
triggered for the
path distance
Delete distance-to-go:
A synchronized action with the DELDTG command
causes a preprocessing stop after the next output
block (= block for the main run). The preprocessing
stop is canceled with the end of the output block or
when the first DELDTG condition is fulfilled. The
axial distance to the destination point on an axial
delete distance-to-go is stored in $AA_DELT[axis];
the distance-to-go is stored in $AC_DELT.
Tables
12.4 List of predefined subprograms
Fundamentals
510 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
SYNFCT INT: Number of
polynomial
function
defined with
FCTDEF.
VAR REAL:
Reference
variable*)
VAR REAL:
input variable**)
If the condition in the motion synchronous action is
fulfilled, the polynomial determined by the first
expression is evaluated at the input variable. The
upper and lower range of the value is limited and
the input variable is assigned.
FTOC INT: Number of
polynomial
function defined
with FCTDEF
VAR REAL:
input variable**)
INT: Length 1,
2, 3
INT: Channel
number
INT: Spindle
number
Modify tool fine compensation according to a
function defined with FCTDEF (polynomial no
higher than 3rd degree).
The number used here must be specified in
FCTDEF.
*) Only special system variables are permissible as result variables. These are described in
the Programming Guide Advanced in the section on "Write main run variable".
**) Only special system variables are permissible as input variables. These variables are
described in the Programming Guide Advanced in the list of system variables.
12.4.3 Predefined functions
Predefined functions
Predefined functions are invoked by means of a function call. Function calls return a value.
They can be included as an operand in an expression.
1. Coordinate system
Keyword/
function
identifier
Result 1st parameter 2nd parameter Explanation
CTRANS FRAME AXIS REAL: Offset 3. - 15.
Parameter
as 1 ...
4. - 16.
Parameter
as 2 ...
Translation: Zero offset
for multiple axes.
One axis identifier is
programmed at a time,
with its respective value
in the next parameter.
CTRANS can be used to
program offset for up to
8 axes.
CROT FRAME AXIS REAL:
Rotation
3./5.
Parameter
as 1 ...
4./6.
Parameter
as 2 ...
Rotation: Rotation of the
current coordinate
system.
Maximum number of
parameters: 6 (one axis
identifier and one value
per geometry axis)
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 511
CSCALE FRAME AXIS REAL: Scale
factor
3. - 15.
Parameter
as 1 ...
4. - 16.
Parameter
as 2 ...
Scale: Scale factor for
multiple axes.
Maximum number of
parameters is 2*
maximum number of
axes (axis identifier and
value).
One axis identifier is
programmed at a time,
with its respective value
in the next parameter.
CSCALE can be used to
program scale factors
for up to 8 axes.
CMIRROR FRAME AXIS 2. - 8.
Parameter
as 1 ...
Mirror: Mirror on a
coordinate axis
MEAFRAME FRAME 2-dim. REAL
array
2-dim. REAL
array
3. Parameter:
REAL
variables
Frame calculation from 3
measuring points in
space
Frame functions CTRANS, CSCALE, CROT and CMIRROR are used to generate frame
expressions.
2. Geometry functions
Keyword/
function
identifier
Result 1st parameter 2nd parameter 3rd parameter Explanation
CALCDAT BOOL:
Error status
VAR REAL [,2]:
Table with input
points (abscissa
and ordinate for
points 1, 2, 3,
etc.)
INT: Number of
input points for
calculation
(3 or 4)
VAR REAL [3]:
Result:
Abscissa,
ordinate and
radius of
calculated
circle center
point
CALCDAT: Calculate circle data
Calculates radius and center
point of a circle from 3 or 4 points
(according to parameter 1), which
must lie on a circle. The points
must be different.
Tables
12.4 List of predefined subprograms
Fundamentals
512 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Names Result 1st parameter 2nd parameter 3rd parameter 4th parameter 5th
parameter
6th
parameter
CALCPOSI INT:
Status
0 OK
-1 DLIMIT
neg.
-2 Trans.
n.def.
1 SW limit
2 Working
area
3 Prot. zone
See PGA for
more
REAL:
Starting
position in
WCS
[0] Abscissa
[1] Ordinate
[2] Applicate
REAL:
Increment:
Path definition
[0] Abscissa
[1] Ordinate
[2] Applicate
referred to
starting
position
REAL:
Minimum
clearances of
limits to be
observed
[0] Abscissa
[1] Ordinate
[2] Applicate
[3] Lin.
machine
Axis
[4] Rot. Axis
REAL:
Return value
possible incr.
path if path
from parameter
3 cannot be
fully traversed
without
violating limit
BOOL:
0:
Evaluation
G code
group 13
(inch/metr.)
1:
Reference
to basic
control
system,
independen
t of active
G codes
group 13
bin
encoded
to be
monitored
1 SW limits
2 working
area
4 active
protection
zone
8 preactive
protection
zone
Explanation:
CALCPOSI
CALCPOSI is for checking whether, starting from a defined starting point, the geometry
axes can traverse a defined path without violating the axis limits (software limits), working
area limitations, or protection zones. If the defined path cannot be traversed without
violating limits, the maximum permissible value is returned.
INTERSEC BOOL:
Error status
VAR REAL [11]:
First contour
element
VAR REAL [11]:
Second contour
element
VAR REAL [2]:
Result vector:
Intersection
coordinate,
abscissa and
ordinate
Intersection: Calculation of
intersection
The intersection between two
contour elements is calculated.
The intersection coordinates
are return values. The error
status indicates whether an
intersection was found.
3. Axis functions
Result 1st parameter 2nd parameter Explanation
AXNAME AXIS:
Axis identifier
STRING [ ]:
Input string
AXNAME: Get axis identifier
Converts the input string to an axis identifier. An
alarm is generated if the input string does not
contain a valid axis identifier.
AXTOSPI INT:
Spindle
number
AXIS:
Axis identifier
AXTOSPI: Convert axis to spindle
Converts an axis identifier into a spindle number.
An alarm is set if the transfer parameter does not
contain a valid axis identifier.
SPI AXIS:
Axis identifier
INT:
Spindle number
SPI: Convert spindle to axis
Converts a spindle number to an axis identifier. An
alarm is generated if the passed parameter does
not contain a valid spindle number.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 513
ISAXIS BOOL
TRUE:
Axis exists:
Otherwise:
FALSE
INT:
Number of the
geometry axis
(1 to 3)
Check whether the geometry axis 1 to 3 specified
as parameter exists in accordance with
$MC_AXCONF_GEOAX_ASSIGN_TAB.
AXSTRING STRING AXIS Convert axis identifier into string.
4. Tool management
Result 1st parameter 2nd parameter Explanation
NEWT # INT:
T number
STRING [32]:
Tool name
INT: Duplo
number
Create new tool (prepare tool data). The duplo
number can be omitted.
GETT # INT:
T number
STRING [32]:
Tool name
INT: Duplo
number
Get T number for tool identifier
GETACTT # INT:
Status
INT:
T number
STRING[32]:
Tool name
Get active tool from a group of tools with the same
name
TOOLENV INT:
Status
STRING:
Name
Save a tool environment in SRAM with the
specified name
DELTOOLENV INT:
Status
STRING:
Name
Delete a tool environment in SRAM with the
specified name. All tool environments if no name
specified.
GETTENV INT:
Status
STRING:
Name
INT:
Number = [0]
Number = [1]
Number = [2]
Reading:
T number,
D number,
DL number
from a tool environment with the specified name
#) The keyword is not valid for SINUMERIK FM-NC.
Result 1st par. 2nd par. 3rd par. 4th par. 5th par. 6th par. Explanation
GETTCOR INT:
Status
REAL:
Length
[11]
STRING:
Compon
ents:
Coordi-
nate
system
STRING:
Tool
environm
ent/
" "
INT:
Int. T
number
INT:
D
number
INT:
DL
number
Read tool lengths and tool
length components from tool
environment or current
environment
Details: See /FB1/ Function
Manual Basic Functions; (W1)
Result 1st par. 2nd par. 3rd par. 4th par. 5th par. 6th par. 7th par. 8th par. 9th par.
SETTCOR INT:
Status
REAL:
Offset
vector
[0-3]
STRING:
Compo-
nent(s)
INT:
Compon
ent(s) to
be offset
INT:
Type of
write
operation
INT:
Index of
geo. axis
STRING:
Name of
tool
environm
ent
INT:
Int. T
number
INT:
D
number
INT:
DL
number
Tables
12.4 List of predefined subprograms
Fundamentals
514 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Explanation Changing tool components whilst observing all marginal conditions that are included in the evaluation of the
individual components. Details: See Function Manual Basic Functions; (W1)
Result 1st parameter 2nd parameter 3rd parameter Explanation
LENTOAX INT:
Status
INT:
Axis index
[0-2]
REAL:
L1, L2, L3 for
abscissa,
ordinate,
applicate
[3], [3] Matrix
STRING:
Coordinate
system for the
assignment
The function provides information
about the assignment of the tool
lengths L1, L2, L3 of the active
tools to abscissa, ordinate,
applicate. The assignment to the
geometry axes is affected by
frames and the active plane (G17
- 19). Details: See Function
Manual Basic Functions; (W1)
5. Arithmetic
Result 1st parameter 2nd parameter Explanation
SIN REAL REAL Sine
ASIN REAL REAL Arcsine
COS REAL REAL Cosine
ACOS REAL REAL Arccosine
TAN REAL REAL Tangent
ATAN2 REAL REAL REAL Arctangent 2
SQRT REAL REAL Square root
ABS REAL REAL Generate absolute value
POT REAL REAL Square
TRUNC REAL REAL Truncate decimal places
ROUND REAL REAL Round decimal places
LN REAL REAL Natural logarithm
EXP REAL REAL Exponential function ex
MINVAL REAL REAL REAL Determines the smaller value of two variables
MAXVAL REAL REAL REAL Determines the larger value of two variables
Result 1st parameter 2nd parameter 3rd parameter Explanation
BOUND REAL: Check
status
REAL:
Minimum
REAL:
Maximum
REAL: Check
variable
Checks whether the variable
value lies within the defined
min/max value range
Explanation The arithmetic functions can also be programmed in synchronized actions. Arithmetic functions are
calculated and evaluated in the main run. Synchronized action parameter $AC_PARAM[n] can also be
used for calculations and as buffer memory.
Tables
12.4 List of predefined subprograms
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 515
6. String functions
Result 1st parameter 2nd parameter
to
3rd parameter
Explanation
ISNUMBER BOOL STRING Check whether the input string can be converted to
a number.
Result is TRUE if conversion is possible.
ISVAR BOOL STRING Check whether the transfer parameter contains a
variable known in the NC. (Machine data, setting
data, system variable, general variables such as
GUDs
Result is TRUE if all the following checks produce
positive results according to the (STRING) transfer
parameter:
– The identifier exists
– It is a 1- or 2-dimensional
array
– An array index is allowed.
For axial variables, the axis names are accepted as
an index but not checked.
NUMBER REAL STRING Convert the input string into a number.
TOUPPER STRING STRING Convert all alphabetic characters in the input string
to upper case.
TOLOWER STRING STRING Convert all alphabetic characters in the input string
to lower case.
STRLEN INT STRING The result is the length of the input string up to the
end of the string (0).
INDEX INT STRING CHAR Find the character (2nd parameter) in the input
string (1st parameter). The reply gives the place, at
which the character was first found. The search is
from left to right.
The 1st character in the string has the index 0.
RINDEX INT STRING CHAR Find the character (2nd parameter) in the input
string (1st parameter). The reply gives the place, at
which the character was first found. The search is
from right to left.
The 1st character in the string has the index 0.
MINDEX INT STRING STRING Find one of the characters specified in the 2nd
parameter in the input string (1st parameter). The
place where one of the characters was first found is
output. The search is from left to right. The first
character in the string has the index 0.
SUBSTR STRING STRING INT Returns the substring of the input string (1st
parameter), defined by the start character (2nd
parameter) and number of characters (3rd
parameter).
Example:
SUBSTR("Hello world",1,5) returns "Hello world"
Tables
12.4 List of predefined subprograms
Fundamentals
516 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
12.4.4 Data types
Data types
Data types
Type Comment Value range
INT Integers with sign -2147483646 ... +2147483647
REAL Real numbers (fractions with decimal point, LONG
REAL to IEEE)
±(2,2*10-308 … 1,8*10+308)
BOOL Truth values TRUE (1) and FALSE (0) 1, 0
CHAR ASCII character specified by the code 0 ... 255
STRING Character string, number of characters in [...],
maximum of 200 characters
Sequence of values with 0 ... 255
AXIS Axis names (axis addresses) only Any axis identifiers in the channel
FRAME Geometrical parameters for translation, rotation,
scaling, and mirroring
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 517
Appendix A
Appendix
A.1 List of abbreviations
Fundamentals
518 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
A.1 List of abbreviations
A Output
AS Automation system
ASCII American Standard Code for Information Interchange: American coding standard for
the exchange of information
ASIC Application Specific Integrated Circuit: User switching circuit
ASUB Asynchronous subroutine
AuxF Auxiliary function
AV Job planning
BA Operating mode
BB Ready to run
BCD Binary Coded Decimals: Decimal numbers encoded In binary code
BCS Basic Coordinate System
BIN Binary files (Binary Files)
BIOS Basic Input Output System
BOT Boot files: Boot files for SIMODRIVE 611 digital
BP Basic program
C Bus Communication bus
CAD Computer-Aided Design
CAM Computer-Aided Manufacturing
CNC Computerized Numerical Control: Computerized numerical control
COM Communication
COR Coordinate rotation
CP Communications Processor
CPU Central Processing Unit: Central processing unit
CR Carriage Return
CRC Cutter radius compensation
CRT Cathode Ray Tube picture tube
CSB Central Service Board: PLC module
CSF Function plan (PLC programming method)
CTS Clear To Send: Signal from serial data interfaces
CUTOM Cutter radius compensation: Tool radius compensation
DAC Digital-to-Analog Converter
DB Data block in the PLC
DBB Data block byte in the PLC
DBW Data block word in the PLC
DBX Data block bit in the PLC
DC Direct Control: Movement of the rotary axis via the shortest path to the absolute
position within one revolution
DCD Data Carrier Detect
DDE Dynamic Data Exchange
DIN Deutsche Industrie Norm (German Industry Standard)
Appendix
A.1 List of abbreviations
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 519
DIO Data Input/Output: Data transfer display
DIR Directory: Directory
DLL Dynamic Link Library
DOE Data transmission equipment
DOS Disk Operating System
DPM Dual-Port Memory
DPR Dual-Port RAM
DRAM Dynamic Random Access Memory
DRF Differential Resolver Function: Differential resolver function (DRF)
DRY Dry Run: Dry run feedrate
DSB Decoding Single Block: Decoding single block
DTE Data Terminal Equipment
DW Data word
E Input
EIA code Special punched tape code, number of holes per character always odd
ENC Encoder: Actual value encoder
EPROM Erasable Programmable Read Only Memory
Error Error from printer
FB Function block
FBS Slimline screen
FC Function Call: Function block in the PLC
FDB Product database
FDD Floppy Disk Drive
FDD Feed Drive
FEPROM Flash-EPROM: Read and write memory
FIFO First In First Out: Memory that works without address specification and whose data
are read in the same order in which they were stored.
FIPO Fine InterPOlator
FM Function Module
FM-NC Function module – numerical control
FPU Floating Point Unit Floating Point Unit
FRA Frame block
FRAME Data record (frame)
FST Feed Stop: Feed stop
GUD Global User Data: Global user data
HD Hard Disk Hard disk
HEX Abbreviation for hexadecimal number
HHU Handheld unit
HMI Human Machine Interface
HMI Human Machine Interface: Operator functionality of SINUMERIK for operation,
programming and simulation.
HMS High-resolution Measuring System
HW Hardware
I/O Input/Output
Appendix
A.1 List of abbreviations
Fundamentals
520 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
I/R Infeed/regenerative-feedback unit (power supply) of the SIMODRIVE 611digital
IBN Startup
IF Drive module pulse enable
IK (GD) Implicit communication (global data)
IKA Interpolative Compensation: Interpolatory compensation
IM Interface Module Interconnection module
IMR Interface Module Receive: Interconnection module for receiving data
IMS Interface Module Send: Interconnection module for sending data
INC Increment: Increment
INI Initializing Data: Initializing data
IPO Interpolator
IS Interface signal
ISA Industry Standard Architecture
ISO International Standardization Organization
ISO code Special punched tape code, number of holes per character always even
JOG Jogging: Setup mode
K1 .. K4 Channel 1 to channel 4
KUE Speed ratio
Kv Servo gain factor
LAD Ladder diagram (PLC programming method)
LCD Liquid Crystal Display: Liquid crystal display
LEC Leadscrew error compensation
LED Light-Emitting Diode: Light emitting diode
LF Line Feed
LR Position controller
LUD Local User Data
MB Megabyte
MC Measuring circuit
MCP Machine control panel
MCS Machine coordinate system
MD Machine data
MDI Manual Data Automatic: Manual input
MLFB Machine-readable product designation
Mode group Mode group
MPF Main Program File: NC parts program (main program)
MPI Multiport Interface Multiport Interface
MS Microsoft (software manufacturer)
MSD Main Spindle Drive
NC Numerical Control: Numerical Control
NCK Numerical Control Kernel: NC kernel with block preparation, traversing range, etc.
NCU Numerical Control Unit: Hardware unit of the NCK
NRK Name for the operating system of the NCK
NURBS Non-Uniform Rational B-Spline
Appendix
A.1 List of abbreviations
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 521
OB Organization block in the PLC
OEM Original Equipment Manufacturer
OP Operator Panel
OP Operator Panel: Operating setup
OPI Operator Panel Interface
OPI Operator Panel Interface: Interface for connection to the operator panel
OPT Options: Options
OSI Open Systems Interconnection: Standard for computer communications
P bus Peripheral Bus
PC Personal Computer
PCIN Name of the SW for data exchange with the control
PCMCIA Personal Computer Memory Card International Association: Standard for plug-in
memory cards
PCU PC Unit: PC box (computer unit)
PG Programming device
PLC Programmable Logic Control: Interface control
PLC Programmable Logic Controller
PMS Position measuring system
POS Positioning
RAM Random Access Memory: Program memory that can be read and written to
REF Reference point approach function
REPOS Reposition function
RISC Reduced Instruction Set Computer: Type of processor with small instruction set and
ability to process instructions at high speed
ROV Rapid override: Input correction
RPA R-Parameter Active: Memory area on the NCK for R parameter numbers
RPY Roll Pitch Yaw: Rotation type of a coordinate system
RS-232-C Serial interface (definition of the exchange lines between DTE and DCE)
RTS Request To Send: RTS, control signal of serial data interfaces
SBL Single Block: Single block
SD Setting Data
SDB System Data Block
SEA Setting Data Active: Identifier (file type) for setting data
SFB System Function Block
SFC System Function Call
SK Softkey
SKP SKiP: Skip block
SM Stepper Motor
SPF Sub Routine File: Subroutine
SR Subroutine
SRAM Static RAM (non-volatile)
SSI Serial Synchronous Interface: Synchronous serial interface
STL Statement list
SW Software
Appendix
A.1 List of abbreviations
Fundamentals
522 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
SYF System Files System files
T Tool
TC Tool change
TEA Testing Data Active: Identifier for machine data
TLC Tool length compensation
TNRC Tool Nose Radius Compensation
TO Tool Offset: Tool offset
TO Tool offset
TOA Tool Offset Active: Identifier (file type) for tool offsets
TRANSMIT TRANSform Milling Into Turning: Coordinate conversion on turning machine for
milling operations
TRC Tool Radius Compensation
UFR User Frame: Work offset
UI User interface
WCS Workpiece coordinate system
WOP Workshop-oriented Programming
WPD Workpiece Directory: Workpiece directory
ZO Work offset
ZOA Zero Offset Active: Identifier (file type) for zero offset data
µC Micro Controller
Appendix
A.2 List of abbreviations
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 523
A.2 List of abbreviations
A.2.1 Correction sheet - fax template
Should you come across any printing errors when reading this publication, please notify us
on this sheet. Suggestions for improvement are also welcome.
Appendix
A.2 List of abbreviations
Fundamentals
524 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
7R
6,(0(16$*
$'0&06
3RVWIDFK
'(UODQJHQ
)D['RFXPHQWDWLRQ
PDLOWRGRFXPRWLRQFRQWURO#VLHPHQVFRP
ZZZVLHPHQVFRPDXWRPDWLRQVHUYLFHVXSSRUW
)URP
1DPH
&RPSDQ\'HSW
6WUHHW
=LSFRGH 7RZQ
3KRQH
)D[
6XJJHVWLRQVDQGRUFRUUHFWLRQV
Appendix
A.2 List of abbreviations
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 525
A.2.2 Overview
*HQHUDO'RFXPHQWDWLRQ
6,180(5,.
%URFKXUH
2YHUYLHZRI6,180(5,.'VO'LVO'RFXPHQWDWLRQ
6,180(5,.
'VO
'LVO
&DWDORJ1&
6,1$0,&6
6
&DWDORJ
'6HUYR&RQWURO
8VHU'RFXPHQWDWLRQ
6,180(5,.
'VO
2SHUDWLQJ0DQXDO
B+0,VO
ಥ+0,(PEHGGHG
ಥ6KRS0LOO
ಥ6KRS7XUQ
6,180(5,.
'VO
'
'LVO
'L
'
2SHUDWLQJ0DQXDO
ಥ+0,$GYDQFHG
ಥ3URJUDPPLQJ
FRPSDFW
6,180(5,.
'VO
'
'LVO
'L
'
3URJUDPPLQJ0DQXDO
ಥ)XQGDPHQWDOV
ಥ$GYDQFHG
ಥ3URJUDPPLQJFRPSDFW
ಥ/LVWV6\VWHP9DULDEOHV
ಥ,627XUQLQJ0LOOLQJ
0DQXIDFWXUHU6HUYLFH'RFXPHQWDWLRQ
6,180(5,.
'VO
0DQXDO
1&8
6,180(5,.
'VO
'LVO
0DQXDO
2SHUDWRU
&RPSRQHQWV
6,180(5,.
'VO
&RPPLVVLRQLQJ
0DQXDO&1&
ಥ1&.3/&'ULYH
ಥ+0,VO
ಥ+0,(PEHGGHG
ಥ+0,$GYDQFHG
ಥ6KRS0LOO
ಥ6KRS7XUQ
0DQXIDFWXUHU6HUYLFH'RFXPHQWDWLRQ
6,180(5,.
'VO
'
'LVO
'L
'
)XQFWLRQ0DQXDO
ಥ%DVLF0DFKLQH
ಥ([WHQGHG)XQFWLRQV
ಥ6SHFLDO)XQFWLRQV
6,180(5,.
'VO
'
'LVO
'L
'
)XQFWLRQ0DQXDO
ಥ6\QFKURQL]HG$FWLRQV
ಥ,VR'LDOHFWV
6,1$0,&6
6
)XQFWLRQ0DQXDO
'ULYH)XQFWLRQV
6,180(5,.
'VO
'
'LVO
'L
'
3URJUDPPLQJ0DQXDO
ಥ&\FOHV
ಥ0HDVXULQJ&\FOHV
6,180(5,.
'VO
'LVO
'LDJQRVWLFV0DQXDO
6,180(5,.
'LVO
&RPPLVVLRQLQJ
0DQXDO
6,180(5,.
'VO
'LVO
3DUDPHWHU0DQXDO
ಥ3DUW
ಥ3DUW
6,180(5,.
'VO
)XQFWLRQ0DQXDO
6DIHW\,QWHJUDWHG
6,180(5,.
'VO
'
'LVO
'L
'
(0&*XLGHOLQHV
(OHFWURQLF'RFXPHQWDWLRQ
6,180(5,.
6,1$0,&6
0RWRUV
'2&21&'
'2&21:(% 7KHVHGRFXPHQWVDUHDPLQLPXPUHTXLUHPHQW
Appendix
A.2 List of abbreviations
Fundamentals
526 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
*HQHUDO'RFXPHQWDWLRQ
6,180(5,.
%URFKXUH
2YHUYLHZIR6,180(5,.''L''RFXPHQWDWLRQ
6,180(5,.
'
'L
'
&DWDORJ1&
6DIHW\,QWHJUDWHG
6DIHW\,QWHJUDWHG
$SSOLFDWLRQ0DQXDO
8VHU'RFXPHQWDWLRQ
6,180(5,.
'
'L
'
2SHUDWLQJ0DQXDO
ಥ+0,(PEHGGHG
ಥ6KRS0LOO
ಥ6KRS7XUQ
ಥ+7
6,180(5,.
'VO
'
'LVO
'L
'
2SHUDWLQJ0DQXDO
ಥ+0,$GYDQFHG
ಥ3URJUDPPLQJ
FRPSDFW
6,180(5,.
'VO
'
'LVO
'L
'
3URJUDPPLQJ0DQXDO
ಥ)XQGDPHQWDOV
ಥ$GYDQFHG
ಥ3URJUDPPLQJFRPSDFW
ಥ/LVWV6\VWHP9DULDEOHV
ಥ,627XUQLQJ0LOOLQJ
0DQXIDFWXUHU6HUYLFH'RFXPHQWDWLRQ
6,180(5,.
'
'
&RQILJXULQJ+:
ಥ'
ಥ'
6,180(5,.
'
'L
'
0DQXDO
2SHUDWRU
&RPSRQHQWV
6,180(5,.
'
'L
'
)XQFWLRQ0DQXDO
ಥ6KRS0LOO
ಥ6KRS7XUQ
0DQXIDFWXUHU6HUYLFH'RFXPHQWDWLRQ
6,180(5,.
'VO
'
'LVO
'L
'
)XQFWLRQ0DQXDO
ಥ%DVLF0DFKLQH
ಥ([WHQGHG)XQFWLRQV
ಥ6SHFLDO)XQFWLRQV
ಥ6\QFKURQL]HG$FWLRQV
ಥ,VR'LDOHFWV
ಥ(0&*XLGHOLQHV
6,180(5,.
'
'L
'
)XQFWLRQ0DQXDO
ಥ'ULYH)XQFWLRQV
ಥ7RRO0DQDJHPHQW
ಥ+\GUDXOLFV0RGXOH
ಥ$QDORJ0RGXOH
6,180(5,.
'
'L
'
)XQFWLRQ0DQXDO
ಥ5HPRWH'LDJQRVLV
ಥ#(YHQW
6,180(5,.
'VO
'
'LVO
'L
'
3URJUDPPLQJ0DQXDO
ಥ&\FOHV
ಥ0HDVXULQJ&\FOHV
6,180(5,.
'
'L
'
'LDJQRVWLFV0DQXDO
6,180(5,.
'L
&RPPLVVLRQLQJ
0DQXDO
6,180(5,.
'
'L
'
3DUDPHWHU0DQXDO
ಥ3DUW
ಥ3DUW
6,180(5,.
'
)XQFWLRQ0DQXDO
6DIHW\,QWHJUDWHG
6,180(5,.
'
'
0&,6
ಥ&RPSXWHU/LQN
ಥ7RRO'DWD,QIR6\V
ಥ1&'DWDPDQDJHP
ಥ1&'DWD7UDQVIHU
ಥ7RRO'DWD&RPPXQ
(OHFWURQLF'RFXPHQWDWLRQ
6,180(5,.
6,02'5,9(
0RWRUV
'2&21&'
'2&21:(% 7KHVHGRFXPHQWVDUHDPLQLPXPUHTXLUHPHQW
6,180(5,.
'L
6\VWHP2YHUYLHZ
6,180(5,.
'
'
&RQILJXULQJ
ಥ2SHUDWRU,QWHUIDFH
23
ಥ+0,(PEHGGHG
6,180(5,.
'
'L
'
&RPPLVVLRQLQJ0DQXDO
ಥ''
ಥ+0,
ಥ%DVHVRIWZDUH
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 527
Glossary
Absolute dimensions
A destination for an axis movement is defined by a dimension that refers to the origin of the
currently active coordinate system. See -> incremental dimension.
Acceleration with jerk limitation
In order to optimize the acceleration response of the machine whilst simultaneously
protecting the mechanical components, it is possible to switch over in the machining program
between abrupt acceleration and continuous (jerk-free) acceleration.
Address
An address is the identifier for a certain operand or operand range, e.g. input, output etc.
Analog input/output module
Analog input/output modules are signal formers for analog process signals.
Analog input modules convert analog measured values into digital values which can be
processed in the CPU.
Analog output modules convert digital values into analog output signals.
Approach machine fixed-point
Approach motion towards one of the predefined -> fixed machine points.
Archiving
Reading out data and/or directories to an external memory device.
A-Spline
The Akima-Spline runs under a continuous tangent through the programmed interpolation
points (3rd order polynomial).
Asynchronous subroutine
A parts program which can be started asynchronously to (independently of) the current
program status by an interrupt signal (e.g. "rapid NC input" signal).
Glossary
Fundamentals
528 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Automatic
Operating mode of the control (block sequence operation according to DIN): Operating Mode
in NC systems in which a -> parts program is selected and continuously executed.
Auxiliary functions
Auxiliary functions can be used to transfer -> parameters to the -> PLC in -> parts programs,
where they trigger reactions which are defined by the machine manufacturer.
Axes
In accordance with their functional scope, the CNC axes are subdivided into:
• Axes: interpolating path axes
• Auxiliary axes: non-interpolating feed and positioning axes with an axis-specific feed rate.
Auxiliary axes are not involved in the actual machining, and include for example tool
feeders and tool magazines.
Axis address
See -> axis identifier
Axis identifier
Axes are labeled in accordance with DIN 66217 (for a clockwise orthogonal -> coordinate
system) with the letters X,Y, Z.
-> Rotary axes which rotate around are labeled with the letters A, B, C. Additional axes
parallel to the above can be identified with further address letters.
Axis name
See -> axis identifier
B spline
With the B-Spline, the programmed positions are not interpolation points, as they are just
"control points" instead. The generated curve only runs near to the control points, not directly
through them (optional 1st, 2nd or 3rd order polynomials).
Backlash compensation
Compensation for mechanical machine backlash, e.g. backlash on reversal for feed screws.
Backlash compensation can be entered separately for each axis.
Backup
Saving the memory contents to an external memory device.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 529
Backup battery
The backup battery ensures that the → user program in the → CPU is stored so that it is safe
from power failure and so that specified data areas and bit memory, timers and counters are
stored retentively.
Back-up memory
The backup memory enables buffering of memory areas of the -> CPU without a buffer
battery. Buffering can be performed for a configurable number of times, counters, markers
and data bytes.
Basic axis
Axis whose setpoint or actual value position forms the basis of the calculation of a
compensation value.
Basic Coordinate System
Cartesian coordinate system which is mapped by transformation onto the machine
coordinate system.
In the -> parts program, the programmer uses the axis names of the basic coordinate
system. The basic coordinate system exists in parallel to the -> machine coordinate system
when no -> transformation is active. The difference between the systems relates to the axis
identifiers.
Baud rate
Rate of data transfer (Bit/s).
Blank
Workpiece as it is before it is machined.
Block
"Block" is the term given to any files required for creating and processing programs.
Block search
For debugging purposes or following a program abort, the "Block search" function can be
used to select any location in the part program at which the program is to be started or
resumed.
Booting
Loading the system program after power on.
Glossary
Fundamentals
530 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Bus connector
A bus connector is an S7-300 accessory part which is supplied together with the -> I/O
modules. The bus connector expands the -> S7-300 bus from the -> CPU or an I/O module
to the neighboring I/O module.
C axis
Axis around which the tool spindle describes a controlled rotational and positioning
movement.
C spline
The C-spline is the most well-known and widely used spline. The transitions at the
interpolation points are continuous, both tangentially and in terms of curvature. 3rd order
polynomials are used.
Channel
A channel is characterized by its ability to execute a -> parts program independently of other
channels. A channel exclusively controls the axes and spindles assigned to it. Parts
programs run on various channels can be coordinated by -> synchronization.
Channel structure
The channel structure enables the -> programs of the individual channels to be executed
simultaneously and asynchronously.
Circular interpolation
The -> tool is required to travel in a circle between defined points on the contour at a
specified feedrate while machining the workpiece.
CNC
See -> NC
COM
Component of the NC control for the implementation and coordination of communication.
Compensation axis
Axis with a setpoint or actual value modified by the compensation value
Compensation table
Table containing interpolation points. It provides the compensation values of the
compensation axis for selected positions on the basic axis.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 531
Compensation value
Difference between the axis position measured by the position sensor and the desired,
programmed axis position.
Connecting cables
Connecting cables are pre-assembled or user-assembled 2-wire cables with a connector at
each end. This connecting cable connects the → CPU to a → programming device or to other
CPUs by means of a → multi-point interface (MPI).
Continuous-path mode
The purpose of continuous-path mode is to prevent excessive deceleration of the -> path
axes at the part program block boundaries (in terms of the control, machine and other
properties of the operation and the user) and to effect the transition to the next block at as
uniform a path speed as possible.
Contour
Outline of the -> workpiece
Contour monitoring
The following error is monitored within a defined tolerance band to ensure contour precision.
An impermissibly high following error might be caused by a drive overload, for example. In
this case an alarm is triggered and the axes are stopped.
coordinate system
See -> Machine Coordinate System, -> Workpiece Coordinate System
CPU
Central Processor Unit, see -> Programmable Logic Controller
Data Block
1. Data unit of the -> PLC, which the -> HIGHSTEP programs can access.
2. Data unit of the -> NC: Data blocks contain data definitions for global user data. These
data can be initialized directly when they are defined.
Data transmission program PCIN
PCIN is an auxiliary program which is used to send and receive CNC user data via the serial
interface, such as e.g. parts programs, tool offsets etc. The PCIN program can be executed
under MS-DOS on standard industrial PCs.
Glossary
Fundamentals
532 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Data word
A data unit, two bytes in size, within a -> data block.
Diagnosis
1. Control operating area
2. The control has both a self-diagnostics program and testing aids for service. Status,
alarm and service indicators.
Digital input/output module
Digital modules are signal formers for binary process signals.
Dimensions in metric units and inches
Position and gradient values can be entered in the machining program in inches. The control
can be set to a basic system regardless of the programmed measuring system (G70/G71).
DRF
Differential Resolver Function: An NC function which generates an incremental zero offset in
automatic mode in conjunction with an electronic handwheel.
Drive
The SINUMERIK 840D control system is connected to the SIMODRIVE 611 digital converter
system by means of a high-speed digital parallel bus.
Dynamic feedforward control
Inaccuracies in the → contour due to following errors can be virtually eliminated using
dynamic, acceleration-dependent feedforward control. This results in excellent machining
accuracy, even at high → path velocities. Feedforward control can be selected and
deselected on an axis-specific basis via the → part program.
Editor
The editor is used to create, modify, add to, compress, and insert programs/texts/program
blocks.
Electronic handwheel
The electronic handwheels can be used to simultaneously traverse selected axes manually.
The meaning of the lines on the handwheels is defined by the external zero offset increment
weighting.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 533
Exact stop
With a programmed exact stop instruction, the position stated in a block is approached
precisely and very slowly, if necessary. In order to reduce the approach time, -> exact stop
limits are defined for rapid traverse and feed.
Exact stop limit
When all path axes reach their exact stop limits, the control responds as if it had reached its
destination point precisely. The -> part program continues execution at the next block.
External zero offset
Zero offset specified by the -> PLC.
Fast retraction from contour
When an interrupt occurs, a motion can be initiated via the CNC machining program,
enabling the tool to be quickly retracted from the workpiece contour that is currently being
machined. The retraction angle and the distance retracted can also be parameterized. After
fast retraction, an interrupt routine can also be executed (SINUMERIK 840D).
Feed override
The programmed velocity is overridden by the current velocity setting made via the
→ machine control panel or by the → PLC (0% to 200%). The feedrate can also be corrected
by a programmable percentage factor (1-200%) in the machining program.
Finished-part contour
Contour of the finished workpiece. See -> blank.
Fixed machine point
A point defined uniquely by the machine tool, e.g. the reference point.
Fixed-point approach
Machine tools can approach fixed points such as a tool change point, loading point, pallet
change point, etc. in a defined way. The coordinates of these points are stored in the control.
Where possible, the control moves these axes in -> rapid traverse.
Frame
A frame is an arithmetic rule that transforms one Cartesian coordinate system into another
Cartesian coordinate system. A frame contains the components -> zero offset, -> rotation, ->
scaling, -> mirroring.
Glossary
Fundamentals
534 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Geometry
Description of a -> workpiece in the -> workpiece coordinate system.
geometry axis
Geometry axes are used to describe a 2- or 3-dimensional range in the workpiece coordinate
system.
Global main program/subroutine
Every global main program/subroutine can only appear once under its own name in the
directory, and it is not possible to have the same program name in different directories with
different contents as a global program.
Ground
Ground is taken as the total of all linked inactive parts of a device which will not become live
with a dangerous contact voltage even in the event of a malfunction.
Helical interpolation
The helical interpolation function is ideal for machining internal and external threads using
form milling cutters and for milling lubrication grooves.
The helix comprises two movements:
• Circular movement in one plane
• A linear movement perpendicular to this plane
High-level CNC language
The high-level language offers: -> User-defined variable, -> System variable, -> Macro
technique.
High-speed digital inputs/outputs
The digital inputs can be used for example to start fast CNC program routines (interrupt
routines). The digital CNC outputs can be used to trigger fast, program-controlled switching
functions (SINUMERIK 840D).
HIGHSTEP
Summary of the programming options for the -> PLC in the AS300/AS400 system.
Inch measuring system
Measuring system, which defines distances in inches and fractions of inches.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 535
Inclined surface machining
Drilling and milling operations on workpiece surfaces that do not lie in the coordinate planes
of the machine can be performed easily using the function "inclined-surface machining".
Increment
Travel path length specification based on number of increments. The number of increments
can be stored as → setting data or selected by means of a suitably labeled key (i.e., 10, 100,
1000, 10000).
Incremental dimension
Also incremental dimension: A destination for axis traversal is defined by a distance to be
covered and a direction referenced to a point already reached. See -> Absolute dimension.
Initialization block
Initialization blocks are special -> program blocks. They contain value assignments that are
performed before program execution. The primary purpose of initialization blocks is to
initialize predefined data or global user data.
Initialization files
It is possible to create an initialization file for each -> workpiece. Various variable
assignments which are intended to apply specifically to one workpiece can be stored in this
file.
Intermediate blocks
Motions with selected → tool offset (G41/G42) may be interrupted by a limited number of
intermediate blocks (blocks without axis motions in the offset plane), whereby the tool offset
can still be correctly compensated for. The permissible number of intermediate blocks which
the control reads ahead can be set in system parameters.
Interpolator
Logical unit of the -> NCK which determines intermediate values for the movements to be
traversed on the individual axes on the basis of destination positions specified in the parts
program.
Interpolatory compensation
The interpolatory compensation allows manufacturing related Leadscrew Error
Compensation and Measuring System Error Compensation (LEC, MSEC).
Glossary
Fundamentals
536 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
interrupt routine
Interrupt routines are special -> subroutines which can be started on the basis of events
(external signals) in the machining process. A parts program block which is currently being
worked through is interrupted and the position of the axes at the point of interruption is
automatically saved.
Interrupts
All alarms and -> messages are output on the operator panel in plain text with the date and
time and a symbol indicating the cancel criterion. The display is divided into alarms and
messages.
1. Alarms and messages in the part program:
Alarms and messages can be displayed in plain text directly from the part program.
2. Alarms and messages from PLC
Alarms and messages for the machine can be displayed in plain text from the PLC
program. No additional function block packages are required to do this.
Inverse-time feed
With SINUMERIK 840D, the time required for the path of a block to be traversed can be
programmed for the axis motion instead of the feed velocity (G93).
Jog
Control operating mode (setup mode): In JOG mode, it is possible to set up the machine.
Individual axes and spindles can be moved in this mode using the direction keys. Other
functions available in JOG mode are -> reference point approach, -> repositioning and ->
preset (setting an actual value).
Key switch
The key switch on the → machine control panel has 4 positions that are assigned functions
by the operating system of the control. The key switch has three different colored keys that
can be removed in the specified positions.
Keywords
Words with specified notation that have a defined meaning in the programming language for
→ part programs.
Kv
Servo gain factor, a control variable in a control loop.
Leadscrew error compensation
Compensation for the mechanical inaccuracies of a leadscrew participating in the feed. The
control uses stored deviation values for the compensation.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 537
Limit speed
Maximum/minimum (spindle) speed: The maximum speed of a spindle may be limited by
values defined in the machine data, the -> PLC or -> setting data.
Linear axis
The linear axis is an axis which, in contrast to a rotary axis, describes a straight line.
Linear interpolation
The tool travels along a straight line to the destination point while machining the workpiece.
Load memory
For the CPU 314 of the -> PLC, the load memory is equal to the -> Work memory .
Look ahead
With the look ahead function, a configurable number of traversing blocks is read in advance
in order to calculate the optimum machining velocity.
Machine
Control operating area
Machine axes
Axes which exist physically on the machine tool.
Machine control panel
An operator panel on a machine tool with operating elements such as keys, rotary switches
etc. and simple indicators such as LEDs. It is used to control the machine tool directly via the
PLC.
Machine coordinate system
System of coordinates based on the axes of the machine tool.
Machine zero
A fixed point on the machine tool, which can be referenced by all (derived) measuring
systems.
Glossary
Fundamentals
538 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Machining channel
Via a channel structure, parallel sequences of movements, such as positioning a loading
gantry during machining, can shorten unproductive times. Here, a CNC channel must be
regarded as a separate CNC control system with decoding, block preparation and
interpolation.
Macro techniques
Grouping of a set of instructions under a single identifier. The identifier in the program refers
to the grouped set of instructions.
Main block
A block prefixed by ":" containing all the parameters required to start execution of a -> parts
program.
Main program
Parts program identified by a number or identifier in which further main programs,
subroutines or -> cycles may be called.
Mains
The term "network" describes the connection of several S7-300 and other terminal devices,
e.g. a programming device, via -> interconnecting cables. A data exchange takes place over
the network between the connected devices.
MDI
Control operating mode: Manual Data Automatic. In MDA mode, it is possible to enter
individual program blocks or sequences of blocks without reference to a main program or
subroutine and to then execute them immediately via the NC start key.
Messages
All messages programmed in the parts program and -> alarms recognized by the system are
output on the operator panel in plain text with the date and time and a symbol indicating the
cancel criterion. The display is divided into alarms and messages.
Metric system
Standardized measuring system: for lengths in millimeters (mm), meters (m), etc.
Mirroring
Mirroring reverses the signs of the coordinate values of a contour, with respect to an axis. It
is possible to mirror with respect to more than one axis at a time.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 539
Mode group
At any one time, all axes/spindles are assigned to just one channel. Each channel is
assigned to a mode group. The same -> mode is always assigned to the channels in a mode
group.
Multipoint interface
The multipoint interface (MPI) is a 9-pole Sub-D interface. A configurable number of devices
can be connected to a multipoint interface and then communicate with each other.
• Programming devices
• Operator control and monitoring equipment
• Further automation systems
The parameter block "Multipoint Interface MPI" of the CPU contains the -> parameters which
define the properties of the multipoint interface.
Name of identifier
The words according to DIN 66025 are supplemented by the identifiers (names) for variables
(computer variable, system variable, user variable), for subroutines, for keywords and words
with several address letters. In terms of the block format, these supplements have the same
significance as the words. Identifiers must be unique. The same identifier must not be used
for different objects.
NC
Numerical Control: NC control incorporates all the components of the of the machine tool
control system: -> NCK, -> PLC, HMI, -> COM.
Note
CNC (Computerized Numerical Control) is a more accurate term for the SINUMERIK 840D
controls. MARS and Merkur controls.
NCK
Numerical Control Kernel: Component of the NC control which executes -> parts programs
and essentially coordinates the movements on the machine tool.
NRK
Numeric Robotic Kernel (operating system of the -> NCK)
Glossary
Fundamentals
540 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
NURBS
Internal motion control and path interpolation are performed using NURBS (non-uniform
rational B-splines). This provides a uniform internal method for all interpolations in the control
(SINUMERIK 840D).
OEM
For machine manufacturers who manufacture their own user interface or wish to integrate
their own technology-specific functions in the control, free space has been left for individual
solutions (OEM applications) for SINUMERIK 840D.
Offset memory
Data range in the control in which the tool offset data are stored.
Operating mode
An operating concept on a SINUMERIK control. The operating modes -> Jog, -> MDA and ->
Automatic are defined.
Oriented spindle stop
Stops the workpiece spindle with a specified orientation angle, e.g. to perform an additional
machining operation at a specific position.
Oriented tool retraction
RETTOOL: If machining is interrupted (because of tool breakage, for example), a program
command can be used retract the tool with a defined orientation by a defined path.
Overall reset
In the event of an overall reset, the following memories of the → CPU are deleted:
• -→ RAM
• Read/write area of → load memory
• → System memory
• → Backup memory
Override
Manual or programmable control feature which enables the user to override programmed
feedrates or speeds in order to adapt them to a specific workpiece or material.
Part program block
Part of a → part program that is demarcated by a line feed. There are two types: → main
blocks and → subblocks.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 541
Part program management
Part program management can be organized by → workpieces. The size of the user memory
determines the number of programs and the amount of data that can be managed. Each file
(programs and data) can be given a name consisting of a maximum of 24 alphanumeric
characters.
Path axis
Path axes are all the machining axes in the -> channel which are controlled by the ->
interpolator so that they start, accelerate, stop and reach their end positions simultaneously.
Path feed
Path feed acts on -> path axes. It represents the geometrical sum of the feeds on the
participating -> geometry axes.
Path velocity
The maximum programmable path velocity depends on the input resolution. For example,
with a resolution of 0.1 mm the maximum programmable path velocity is 1000 m/min.
Peripheral module
I/O modules represent the link between the CPU and the process.
I/O modules are:
• → Digital input/output modules
• → Analog input/output modules
• → Simulator modules
PLC
Programmable Logic Control: → Speicherprogrammierbare Steuerung. → Programmable
logic control. Component of → NC: Programmable controller for processing the control logic
of the machine tool.
PLC program memory
SINUMERIK 840D: The PLC user program, the user data and the basic PLC program are
stored together in the PLC user memory.
PLC Programming
The PLC is programmed using the STEP 7 software. The STEP 7 programming software is
based on the WINDOWS standard operating system and contains the STEP 5 programming
functions with innovative enhancements.
Glossary
Fundamentals
542 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Polar coordinates
A coordinate system, which defines the position of a point on a plane in terms of its distance
from the origin and the angle formed by the radius vector with a defined axis.
Polynomial interpolation
Polynomial interpolation enables a wide variety of curve characteristics to be generated,
such as straight line, parabolic, exponential functions (SINUMERIK 840D).
Positioning axis
Axis that performs an auxiliary movement on a machine tool (e.g., tool magazine, pallet
transport). Positioning axes are axes that do not interpolate using → path axes.
Pre-coincidence
Block change occurs already when the path distance approaches an amount equal to a
specifiable delta of the end position.
Program block
Program blocks contain the main program and subprograms of → part programs.
Programmable frames
Programmable → frames enable dynamic definition of new coordinate system output points
while the part program is being executed. A distinction is made between absolute definition
using a new frame and additive definition with reference to an existing starting point.
Programmable Logic Controller
Programmable logic controllers (PLC) are electronic controls, the function of which is stored
as a program in the control unit. This means that the layout and wiring of the device do not
depend on the function of the control. The programmable logic controller has the same
structure as a computer; it consists of a CPU (central module) with memory, input/output
modules and an internal bus system. The peripherals and the programming language are
matched to the requirements of the control technology.
Programmable working area limitation
Limitation of the motion space of the tool to a space defined by programmed limitations.
Programming key
Character and character strings that have a defined meaning in the programming language
for → part programs.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 543
Protection zone
Three-dimensional zone within the → working area into which the tool tip must not pass.
Quadrant error compensation
Contour errors at quadrant transitions, which arise as a result of changing friction conditions
on the guideways, can be almost entirely eliminated with the quadrant error compensation.
Parameterization of the quadrant error compensation is performed by means of a circuit test.
R parameters
Arithmetic parameter that can be set or queried by the programmer of the → part program for
any purpose in the program.
Rapid traverse
The highest speed of an axis. It is used for example to move the tool from rest position to the
-> workpiece contour or retract the tool from the contour.
Reference point
Machine tool position that the measuring system of the → machine axes references.
Rotary axis
Rotary axes apply a workpiece or tool rotation to a defined angular position.
Rotation
Component of a → frame that defines a rotation of the coordinate system around a particular
angle.
Rounding axis
Rounding axes rotate a workpiece or tool to an angular position corresponding to an
indexing grid. When a grid index is reached, the rounding axis is "in position".
Safety Functions
The control is equipped with permanently active monitoring functions that detect faults in the
→ CNC, the → PLC and the machine in a timely manner so that damage to the workpiece,
tool or machine is largely prevented. In the event of a fault, the machining operation is
interrupted and the drives stopped. The cause of the malfunction is logged and output as an
alarm. At the same time, the PLC is notified that a CNC alarm has been triggered.
Scaling
Component of a → frame that implements axis-specific scale modifications.
Glossary
Fundamentals
544 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Scan cycle
Protected subprogram for implementing a repetitious machining operation on the
→ workpiece.
Selecting
Series of instructions to the NC that act in concert to produce a particular → workpiece.
Likewise, this term applies to execution of a particular machining operation on a given → raw
part.
Serial V.24 interface
For data input/output, the PCU 20 has one serial V.24 interface (RS232) while the
PCU 50/70 has two V.24 interfaces. Machining programs and manufacturer and user data
can be loaded and saved via these interfaces.
Services
Control operating area
Setting data
Data, which communicates the properties of the machine tool to the NC control, as defined
by the system software.
Softkey
A key, whose name appears on an area of the screen. The choice of soft keys displayed is
dynamically adapted to the operating situation. The freely assignable function keys (soft
keys) are assigned defined functions in the software.
Software limit switches
Software limit switches limit the traversing range of an axis and prevent an abrupt stop of the
slide at the hardware limit switch. Two value pairs can be specified for each axis and
activated separately by means of the → PLC.
Spline interpolation
With spline interpolation, the controller can generate a smooth curve characteristic from only
a few specified interpolation points of a set contour.
SRT
Speed ratio
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 545
Standard cycles
Standard cycles are provided for machining operations, which are frequently repeated:
• Cycles for drilling/milling applications
• for turning technology
The available cycles are listed in the "Cycle support" menu in the "Program" operating area.
Once the desired machining cycle has been selected, the parameters required for assigning
values are displayed in plain text.
Subblock
Block prefixed by "N" containing information for a machining step such as position data.
Subprogram
Sequence of statements of a → part program that can be called repeatedly with different
defining parameters. The subprogram is called from a main program. Every subprogram can
be protected against unauthorized read-out and display. → Cycles are a form of subprogram.
Synchronization
Statements in → part programs for coordination of sequences in different → channels at
certain machining points
Synchronized actions
1. Auxiliary function output
During workpiece machining, technological functions (→ auxiliary functions) can be output
from the CNC program to the PLC. For example, these auxiliary functions are used to
control additional equipment for the machine tool, such as quills, grabbers, clamping
chucks, etc.
2. Fast auxiliary function output
For time-critical switching functions, the acknowledgement times for the → auxiliary
functions can be minimized and unnecessary hold points in the machining process
avoided.
Synchronized axes
Synchronized axes take the same time to traverse their path as the geometry axes take for
their path.
System memory
The system memory is a memory in the CPU in which the following data are stored:
• Data required by the operating system
• The operands times, counters, markers
Glossary
Fundamentals
546 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
System variables
A variable that exists without any input from the programmer of a → part program. It is
defined by a data type and the variable name preceded by the character $. See → User-
defined variable.
TappingRigid
This function allows threads to be tapped without a compensating chuck. By using the
method whereby the spindle, as a rotary axis, and the drilling axis interpolate, threads can be
cut to a precise final drilling depth (e.g. for blind hole threads) (requirement: spindles in axis
operation).
Text editor
See → Editor
TOA area
The TOA area includes all tool and magazine data. By default, this area coincides with the
→ channel area with regard to the reach of the data. However, machine data can be used to
specify that multiple channels share one → TOA unit, so that common tool management data
is then available to these channels.
TOA unit
Each → TOA area can have more than one TOA unit. The number of possible TOA units is
limited by the maximum number of active → channels. A TOA unit includes exactly one tool
data block and one magazine data block. In addition, a TOA unit can also contain a
toolholder data block (optional).
Tool
Active part on the machine tool that implements machining (e.g., turning tool, milling tool,
drill, LASER beam, etc.).
Tool nose radius compensation
Contour programming assumes that the tool is pointed. Because this is not actually the case
in practice, the curvature radius of the tool used must be communicated to the control which
then takes it into account. The curvature center is maintained equidistantly around the
contour, offset by the curvature radius.
Tool offset
Consideration of the tool dimensions in calculating the path.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 547
Tool radius compensation
To directly program a desired → workpiece contour, the control must traverse an equidistant
path to the programmed contour taking into account the radius of the tool that is being used
(G41/G42).
Transformation
Additive or absolute work offset of an axis.
Traversing range
The maximum permissible travel range for linear axes is ± 9 decades. The absolute value
depends on the selected input and position control resolution and the unit of measurement
(inch or metric).
User interface
The user interface (UI) is the display medium for a CNC control in the form of a screen. It is
laid out with horizontal and vertical softkeys.
User memory
All program and data, such as part programs, subroutines, comments, tool compensations,
and work offsets/frames, as well as channel- and program user data can be stored in the
shared CNC user memory.
User program
User programs for the S7-300 automation systems are created using the programming
language STEP 7. The user program has a modular layout and consists of individual blocks.
The basic block types are:
code modules: these blocks contain the STEP 7 commands.
Data blocks: these blocks contain the constants and variables for the STEP 7 program.
User-defined variable
The user can declare user-defined variables for any use in the -> parts program or data
block (global user data). A definition contains a data type specification and the variable
name. See -> system variable.
Variable definition
A variable definition includes the specification of a data type and a variable name. The
variable names can be used to access the value of the variables.
Glossary
Fundamentals
548 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Velocity control
In order to be able to achieve an acceptable traversing velocity on very short traverse
movements within a single block, predictive velocity control can be set over several blocks (-
> look ahead).
Work offset
Specification of a new reference point for a coordinate system through reference to an
existing zero point and a -> frame.
1. Adjustable
SINUMERIK 840D: A configurable number of adjustable zero offsets is available for each
CNC axis. The offsets which can be selected via G functions are effective on an
alternating basis.
2. External
In addition to all the offsets which define the position of the workpiece zero point, an
external zero offset can be overlaid by means of the handwheel (DRF offset) or from the
PLC.
3. Programmable
Zero offsets are programmable for all path and positioning axes with the TRANS
command.
Working area
Three-dimensional zone into which the tool tip can be moved on account of the physical
design of the machine tool. See -> protection zone.
Working area limitation
With the aid of the working area limitation, the traversing range of the axes can be further
restricted in addition to the limit switches. One value pair per axis may be used to describe
the protected working area.
Working memory
The working area is a RAM area in the -> CPU which is accessed by the processor to
access the user program during program execution.
Workpiece
Part to be made/machined by the machine tool.
Workpiece contour
Set contour of the → workpiece to be created or machined.
Glossary
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 549
Workpiece coordinate system
The workpiece coordinate system has its starting point in the → workpiece zero. In machining
operations programmed in the workpiece coordinate system, the dimensions and directions
refer to this system.
Workpiece zero
The workpiece zero is the starting point for the → workpiece coordinate system. It is defined
in terms of distances to the → machine zero.
Glossary
Fundamentals
550 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 551
Index
A
a fixed point, 186
Absolute dimensioning, 78
Absolute dimensions, 17
AC, 79, 80, 122, 284
ACC, 298
Acceleration
Pattern, 215
ACCLIMA, 218
ACN, 87, 284
ACP, 87, 284
additive offsets
Delete, 397
Additive offsets
select, 394
Address
Arithmetic parameter R, 54
Auxiliary function (H), 54
Circle radius CR, 55
Interpolation parameter I, 54
Interpolation parameter J, 54
Interpolation parameter K, 54
Miscellaneous function M, 54
Number of program runs P, 54
Opening angle AC, 55
Polar angle AP, 55
Polar radius RP, 55
Preparatory function G, 54
Subblock N, 54
Subroutine call L, 54
Address letters, 471
Address of block number N, 52
Addresses, 53
Extended addresses, 55
Fixed addresses, 57, 472
Fixed addresses with axis expansion, 57
Modal/non-modal addresses, 55
Settable addresses, 58
Value assignments, 60
with axial extension, 55
ADIS, 206
ADISPOS, 206
Alarm
-number, 68
-text, 68
ALF, 182, 185
AMIRROR, 231, 256
ANG, 432
ANG1, 161
ANG2, 161, 162
AP, 119, 122, 124, 132, 143, 152
Approach and retraction velocities, 375
Approach point/angle, 357
Approach, retraction paths, 355
AR, 141, 152, 156
Arithmetic parameter R, 54, 417
Arithmetic parameters
n, 417
R..., 417
Value assigments, possible range, 418
Value assignments to G, 418
Value assignments to L, 418
Value assignments to N, 418
AROT, 228, 231, 240
AROTS, 252
ASCALE, 228, 231, 252
ATRANS, 231, 233, 238
Auxiliary function (H), 52, 54
Auxiliary function outputs
Overview of auxiliary functions, 410
Transfer functions to the PLC, 409
Axial DRF deselection, 266
Axial DRF deselection and $AA_OFF deselection, 267
Axis
Q, 54
V, 54
W, 54
X, 54
Y, 54
Z, 55
Axis identifiers X, Y, Z, 79, 82
Axis types
Channel axes, 38
Machine axes, 37
Main spindle, 37
Path axes, 38
Positioning axes, 38
Index
Fundamentals
552 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Special axes, 37
Synchronized axes, 39
B
Basic Coordinate System, 28
Blank, 355
Block format
D address, 52
F address, 52
G address, 52
H address, 52
M address, 52
N address, 52
S address, 52
T address, 52
X address, 52
Y address, 52
Z address, 52
Block number, 52, 53, 419, 422
Blocks, 51
Block format, 51
Block length, 51
Block number, 53
Comments, 66
Main block/subblock, 52
Skip block/blocks, 64
Word sequence in blocks, 52
Bottleneck detection, 384
Branch destination, 419
BRISK, 215
BRISKA, 215
C
CALCPOSI, 111, 512
CDOF, 382
CDOF2, 382
CDON, 382
CFC, 154, 301
CFIN, 301
CFTCP, 301
Chamfer, 193
Chamfer the contour corner, 193
Change of direction, 363
Channel axes, 38
Character set, 49
CHF, 193
CHR, 193
CIP, 132, 145
Circle
Circle radius CR, 53
Circle radius CR, 55
Circular interpolation
Center-point coordinates I, 79
Circular interpolation
Center point coordinates J, 79
Circular interpolation
Indication of working plane, 138
Circular interpolation
Helical interpolation, 150
Circular magazine, 337
Circular-path programming
With center and end points, 131, 135
With interpolation and end points, 131, 145
With opening angle and center point, 131, 141
With polar angle and polar radius, 131
With polar coordinates, 143
With radius and end point, 131, 139
With tangential transition, 131
Clamping torque FXST, 190
COARSEA, 283
Collision detection, 382
Determine from adjacent block parts, 383
Collision Detection ON (CDON)/OFF (CDOF), 382
Collisions, 358
Command axes, 40
Comments, 66
Compensation plane, 388
Constant
cutting rate, 306
Grinding wheel peripheral speed, 312
Constant cutting rate
Activate, 309
Axis replacement of assigned channel axis, 311
Preserve, 310
Upper speed limitation, 309
Constants, 63
Binary constants, 64
Hexadecimal constants, 64
Integer constants, 63
Continuous-path mode, 203, 205, 209
For positioning axes, 212
In rapid traverse G0, 214
Look ahead, 214
with programmable transition rounding, 207
With programmable transitional grinding, 209
Contour
Approach, retract, 355
damage, 385
point, 355
Roughing, 67
Contour accuracy, programmable, 223
Index
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 553
Coordinate systems, 13
Absolute dimensions, 17
Basic Coordinate System, 28
Incremental dimension, 19
Machine coordinate system, 25
Overview, 24
Plane designations, 21
Polar coordinates, 17
Workpiece coordinate system, 30
Coordinate systems and workpiece machining, 44
Coordinate systems of active machining operation, 402
Corner behavior
Intersection, 366
Transition circle, 364
Corner rounding
Extensions, 210
On the contour, 207
With contour tolerance in G642 and G643, 211
With G641, 210
with G642, 211
With G643, 211
With greatest possible dynamic response in
G644, 212
CORROF, 266, 267
CPRECOF, 223
CPRECON, 223
CR, 89, 156
CROTS, 252
CT, 132, 148
CUT2D, 107, 323, 386, 389
CUT2DF, 107, 323, 386, 389
Cylinder thread, 168
Cylindrical coordinates, 123
D
D, 336, 339
D number, 341
D0, 336, 339
DAC, 94
Data types, 62
Constants, 63
DC, 87, 284
Deactivate compensation mode
G40, 358
G40, KONT, 361
Definition of workpiece positions, 14
DELDL, 397
Deselect frame, 265
destination, 422
DIAM90, 92
DIAM90A[axis], 94
DIAMCHANA, 94
Diameter programming
Action-based, non-modally, 93
Axis-specific acceptance, 94
Axis-specific, modal and action-based, 93
Axis-specific, non-modal or action-based, 94
Channel-specific acceptance, 93, 94
DIAMOF, 92
DIAMOFA[axis], 94
DIAMON, 92
DIAMONA[axis], 94
DIC, 94
DILF, 182
Dimensions, 88
Absolute dimensioning, 80
Circular-path programming CR, 89
Incremental dimensioning, 82
Interpolation parameters I, J, K, 89
Interpolation point coordinates I1, J1, K1, 89
Metric/inch, G70/G71, 88
Metric/inch, G700/G710, 88
Positional data X, Y, Z, 89
Rotary axes and spindles, 86
Dimensions as a diameter value (G90/AC) or a radius
value (G91/IC) for the specified axis, 93
Dimensions in the channel
Diametral or radius programming, 91
Dimensions independently of G90/G91 or AC/IC for the
specified axis, 93
Dimensions, axis-specific
Diametral or radius programming, 93
DISC, 362
DISC=..., 365
DISCL, 368
DISR, 368
Distance
data X, Y, Z, ..., 52
function G, 52
DITE, 172
DITS, 172
DL, 395
DL number, 395
DRFOF, 266
DRIVE, 215
DRIVEA, 215
Dwell time, 224
Dwell time G4
Feedrate F, 224
Spindle speed S, 224
DYNFINISH, 219
DYNNORM, 219
DYNPOS, 219
Index
Fundamentals
554 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
DYNROUGH, 219
DYNSEMIFIN, 219
E
End of block LF, 50
End of program, M2, M17, M30, 47, 415
EX, 418
Exact stop
Command output, 204
End of interpolation, 204
Positioning window, 203
Extended address
Auxiliary function H, 56
Feedrate F, 56
Miscellaneous function M, 56
Spindle speed S, 56
Tool number T, 56
F
F, 270
FA, 54, 278, 290
Face thread, 169
FAD, 368
FALSE, 63
FB, 317
FD, 294
FDA, 294
Feed, 269
-Axial feed: FA, 54
Example of optimization, 301
for path axes, F, 273
for positioning axes, 290
for synchronized axes, F, 273
FPRAON, FPRAOFF, 292
Metric/inch units of measurement, 274
Modal, 194
Optimization for curved path sections, CFTCP,
CFC, CFIN, 300
Override, 295
Programmed, 194
Traverse rotary axes with path velocity F, 276
Unit of measurement for rotary and linear axes, 275
Unit of measurement for synchronized axes with
limit speed FL, 275
with handwheel override, FD, FDA, 294
Feedforward control, 222
Feedrate
FPRAON, FPRAOFF, 290
G95 FPR(…), 292
Metric/inch units of measurement, 291
Feedrate F, 52, 54
Feedrate non-modal, 193
Feedrate override, percentage, OVR,OVRA, 293
Feedrate values in one block, 314
FFWOF, 222
FFWON, 222
FGREF, 270
FGROUP, 270
FINEA, 283
Fixed addresses with axis expansion
Interpolation parameter IP, 57
Fixed stop, 188
Clamping torque, 190
Monitoring window, 190
Traversing to fixed stop, 189
FL, 270
Flat D number structure, 333
FMA, 445
FP, 186
FPR, 290
FPRAOF, 290
FPRAON, 290
Frame generation according to tool orientation,
TOFRAME, TOROT, PAROT, 261
Frame instructions
Programmable Mirroring, 256
Programmable zero offset, 233, 238
Rotation, programmable, 239
Scale factor, programmable, 253
Settable and programmable statements, 229
Substituting instructions, 230
Frame rotation in tool direction, 262
Frame rotation in working direction
G18, 262, 263
G18 or G19, 263
Frame statements
Additive instructions, 231
Frame system, 31, 227
FRC, 193, 444, 446
FRCM, 193, 194, 446
Function outputs
For travel commands, 412
In continuous-path mode, 413
FXS, 188
FXST, 188
FXSW, 188
G
G function list, 479
G0, 122, 125, 207, 214
Index
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 555
G1, 126, 127, 129
G110, 119
G111, 119
G112, 119
G140, 368
G141, 368
G142, 368
G143, 368
G147, 368
G148, 368
G153, 100, 265
G17, 104, 105, 321, 350, 387
G18, 104, 321, 350
G19, 104, 321, 350, 387
G2, 92, 94, 132, 135, 139, 141, 143, 152
G247, 368
G248, 368
G25, 109, 314
G26, 109, 314
G3, 92, 94, 132, 135, 139, 141, 143, 152
G33, 165
G33 I, J, K, 165
G331, 175, 176
G331 I, J, K, 175
G332, 175, 176
G332 I, J, K, 175
G34, 173
G34, G35, 89
G340, 368
G341, 368
G347, 368
G348, 368
G35, 173
G4, 224
G40, 344, 358
G41, 105, 335, 342, 344, 357
G42, 105, 335, 342, 344, 357
G450, 355, 362
G451, 355, 362
G460, 378
G461, 378
G462, 378
G500, 100, 265
G505 ...G599, 100
G505 to G599, 103
G53, 100, 265
G54, 100
G55, 100
G56, 100
G57, 100
G58, 237
G59, 237
G60, 202
G601, 202, 212
G602, 202
G603, 202
G63, 179, 180
G64, 164, 203, 207
G64,G641, 413
G641, 207
G641 ADIS, 206
G641 ADISPOS, 206
G642, 207
G642 ADIS, 206
G642 ADISPOS, 206
G643, 207
G643 ADIS, 206
G643 ADISPOS, 206
G644, 207
G70, 88, 89
G700, 88
G71, 88, 89
G710, 88
G74, 114
G75, 186
G9, 202
G90, 79, 80, 84, 136
G91, 82, 85, 87, 136
G93, 270
G94, 270
G95, 270
G96, 307
G961, 307
G962, 307
G97, 307
G971, 308
G973, 308
Geometry axes, 36
Switchable, 36
Geometry/speed monitoring, 392
GOTO, 419, 422
GOTOB, 419, 422
GOTOC, 419, 422
GOTOF, 419, 422
Grinding wheel peripheral speed, 312
Grinding wheel peripheral speed, constant, 312
Grinding-specific tool monitoring, 392
GWPS, 312, 313, 327
GWPSOF, 312
GWPSON, 312
H
H functions, 415
Index
Fundamentals
556 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
High-speed function outputs, QU, 412
Halt at cycle end, 414
Handwheel jogging
with path default, 296
with velocity overlay, 297
Handwheel override, 294
Helical interpolation
Programming the end point, 153
Sequence of motions, 158
Helix interpolation, 150
High-speed function outputs, QU, 412
I
I, 89, 173
I1, 89
IC, 82, 84, 87, 122, 284
Identifier
for character string, 50
Identifier for special numerical values, 50
Identifier for system variables, 50
IF, 422
Incremental dimension, 19
Incremental dimensioning, 82, 85
Infeed movement, 364
Inside contour, 384
Internal preprocessing stop, 225, 280
Interpolation parameter IP, 57
Interpolation parameters I, J, K, 54, 56
INVCCW, 156
INVCW, 156
IPOBRKA, 283
IPOENDA, 283
J
J, 89, 173
J1, 89
Jerk limitation, 216, 217
JERKA, 216
JERKLIMA, 218
Jump destinations, 66
Jump instruction, 419
Jump statement, 422
K
K, 89, 173
K1, 89
KONT, 355, 362
KONTC, 355
KONTT, 355
L
Label, 419, 422
Length of cutting edge
relevant, 406
LF, 50
LFOF, 182
LFON, 182
LFPOS, 184, 185
LFTXT, 183, 184, 185
LFWP, 183, 184, 185
LIFTFAST, 182, 183
LIMS, 308
LINE FEED, 51
Linear
Degressive change in thread pitch, 173
Progressive change in thread pitch, 173
Linear interpolation, 127, 129
Linear interpolation G1
Feedrate F, 129
List
of predefined subroutines, 494
of preparatory functions (G functions), 479
Look ahead, 214
M
M functions, 413
End of program, M2, M17, M30, 415
Optional stop, 414
Programmed stop, MO, 414
M instruction sequence, 413
M..., 413
M0, 413
M1, 303, 413
M17, 413
M19, 283
M2, 413
M3, 165, 282, 303, 413
M30, 413
M4, 165, 282, 303, 413
M40, 413
M41, 282, 413
M42, 413
M43, 413
M44, 413
M45, 282, 413
M5, 282, 303, 413
M6, 333, 413
Index
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 557
M7, 411
M70, 283, 413
Machine axes, 37
Machine coordinate system, 25
Main axes, 36
Main block, 52, 55
Main spindle, 37
Master spindle, 37
MEAS, 92, 94
MEAW, 92, 94
Messages, 67
MIRROR, 228, 230, 256
Miscellaneous function M, 52, 54
Modal feedrate, 194
Modal rounding, 193
Monitoring window FXSW, 190
Motion commands, 115
Number of axis values, 116
Programming motion commands, 115
Start point - destination point, 116
MSG, 67
Multiple feedrate values in one block, 314
N
Names, 61
Array identifiers, 62
Identifier, 62
Variable identifiers, 62
NC program, 47
Non-cutting tool path, 367
Non-linear interpolation, 127
Non-modal feedrate, 193
NORM, 355, 357, 361
O
OFFN, 344
Offset memory, 390
Opening angle AC, 55
Operators, 59, 60
ORIPATH, 457
ORIPATHS, 457
Overview
Coordinate systems, 24
Dimensions, 77
Frame components, 228
Language elements, 49
Positional data for geometrical settings, 115
Programmable path action at block boundaries, 200
Tool types, 324
Types of feedrate, 269
OVR, 54, 293
OVRA, 293
P
Parameterizing cycle alarms, 68
PAROT, 262
PAROTOF, 262
Path action, depending on DISC values, 366
Path axes
traverse with handwheel override, 295
Path axes, 38
Path override OVR, 54
Path tangent, 359
Plane designations, 21
PLC axes, 40, 42
PM, 368
Polar
-angle AP, 55
Radius RP, 55
Polar coordinates, 17, 121
Cylindrical coordinates, 123
Define pole, 118, 120
Polar angle AP, 123
Polar radius RP, 124
Working plane, 123
Polar radius RP = 0, 124
POLF, 184
POLFMASK, 184
POLFMLIN, 184
POS, 54, 278, 292
POSA, 54, 278
Position-controlled spindle operation, 281
Position-controlled spindles, position
Position a spindle from standstill, 289
Position spindle from rotation, 282
Positioning axes, 38
traverse, 278
Positioning axis POS, 54
POSP, 278
PR, 368
Preparatory function G, 54
Preprocessing stop, 280
Program
-identifiers, 47
Programming messages, 67
Setting alarms, 68
Program jumps, conditional, 421
Program jumps, unconditional, 419
Program passes, number P, 54
Program section, 64
Index
Fundamentals
558 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Program section repetition, 425
Programmable contour accuracy, 223
Programmable frame rotations with solid angles, 251
Programmable mirroring, MIRROR, AMIRROR, 256
Programmable scale factor, SCALE, ASCALE, 252
Programmable zero offset
G58, G59, 237
TRANS, ATRANS, 232
Programmed feedrate, 194
Programmed rotation in the plane, 243
Programmed stop, M0, 414
Programming commands
List, 431, 470
Programming language
Addresses, 53
Blocks, 51
Character set, 49
Data types, 62
Names, 61
Variable identifier, 55
Words, 50
Programming the end point, 373
PUTFTOC, 313
PUTFTOCF, 313
Q
QU, 412
R
RAC, 94
Radius programming
Action-based, non-modally, 93
Range of values, 63
Rapid traverse movement, 125
Reading positions, 377
Reference point approach, 114
REPEAT, 427
REPEATB, 427
Retraction direction, 183
Retraction path, 183
Retraction velocity, 186
RIC, 94
RND, 193
RNDM, 193
ROT, 106, 228, 230, 240
Rotary axis A, B, C, 53, 86, 270
Rotation, programmable
Direction of rotation, 247
in space, 245
Plane change, 244
ROT, AROT, 239
ROTS, 252
Round the contour corner, 193
Rounding, 193
Modal, 193
RP, 89, 119, 122, 132, 143, 152
RPL, 240
RTLIOF, 125
RTLION, 125
Run-in and run-out paths, programmable, 171
S
S, 303, 307, 312
S1, 303, 312, 314
S2, 303, 314
SCALE, 228, 230, 252
SCC[axis], 308
Select/deselect travel to fixed stop, 189
SETAL, 68
SETMS, 303
Settable block change time with G0, 128
Settable zero offsets, 98
Setting alarms, 68
Setting clamping torque, 189
Setup value, 396
SF, 166, 174
SIEMENS cycles, 68
Skip block
Ten skip levels, 65
Skip levels, 65
Smooth approach and retraction, 367
SOFT, 215
SOFTA, 215
SPCOF, 281
SPCON, 281
Special axes, 37
Special characters, 50
:, 50
=, 50
LF, 50
Speed S, 52
SPI, 291
SPIF1, 464
SPIF2, 464
Spindle, 302
Define master spindle, SETMS(n), 305
Master spindle with work spindle, 303
-position SPOS, SPOSA, 56
speed S, 53
Speed S, 54, 56
Index
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0 559
Speed, direction of rotation and stop, 281
Spindle rotation directions, 302
Spindle speed before/after axis movements, 304
Spindle speed S, 303
Spindle position across block boundary SPOSA, 54
Spindle position SPOS, 54
Spindle speed limitation, 314, 315, 317
Spindle speed S, 54
Spindles
Position-controlled spindle operation, 281
Positioning is axis operation, 282
Working with multiple spindles, 304
SPINU, 56
SPOS, 54, 88, 176, 283, 292
SPOS, SPOSA, 56
SPOSA, 54, 176, 283, 284
SR, 464
SRA, 464
ST, 465
STA, 465
Start point offset SF, 170
Statements
List, 431, 470
Straight line with angle, 159
String variable, 419, 422
Subblock N, 54
Subroutine
-call L, 54
Subroutine list, 494
SUPA, 100, 265
Synchronized axes, 39
T
T0, 331, 333
Taper thread, 169
Tapping
Rigid tapping, 175
with compensating chuck, 179
Without compensating chuck, right-hand/left-hand
threads, 175
Tapping G63
Rule of thumb for feedrate F, 180
Spindle speed S, 180
TCARR, 389
TCOABS, 389
TCOFR, 390
TCOFRX, 390
TCOFRY, 390
TCOFRZ, 390
Technology G group, 219
Thread chains, 164
Thread cutting, 164, 167, 181
Cylinder thread, 168
Right-hand/left-hand threads, 165
Start point offset, 170
Taper thread, 169
Thread chains, 164
with constant lead, 164, 167
with linearly progressive/degressive speed
change, 173
Thread cutting G33
Feedrate F, 167
TMOF, 393
TMON, 393
TOFRAME, 262
TOFRAMEX, 262
TOFRAMEY, 262
TOFRAMEZ, 262
Tool
-number T, 54
Offset number D, 52
Tool change point, 358
Tool edge number D, 54
Tool edge reference point, 406
Tool length
component, 389
offset, 389
Offset from toolholder orientation, TCOABS, 390
Tool monitoring
Deactivate, 393
Selection/deselection, 393
Tool offset
Coordinate system for wear values, 402
CUT2D, CUT2DF, 386
CUT2D, CUT2DF with contour tools, 386
Cutting-edge selection with contour tools, 386
Tool Offset
Activate immediately, 343
Tool offsets
Compensation at outside corners, 362
Contour, approach, retract, 355
Smooth approach and retraction (SAR), 367
Tool radius compensation, 323
Tool radius compensation, 343, 398
Change of the direction of compensation, 352
Changing the offset number D, 353
Corner behavior, 365
Corner behavior, intersection, 366
Corner behavior, selectable transitions, 365
Corner behavior, transition circle, 364
CUT2D, 387
CUT2DF, 388
Tool T, 52, 54
Index
Fundamentals
560 Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Tool types, 324, 392
Drill, 326
Grinding tools, 327
Milling tools, 324
Slotting saw, 330
Special tools, 329
Turning tools, 328
Toolholder, 389
Request, TCARR, 390
Toolholder with orientation capability
Tool direction from active frame, 390
Tool orientation with frame change, TCOABS, 391
Tools with a relevant tool point direction, 406
TOROT, 262
TOROTOF, 262
TOROTX, 262
TOROTY, 262
TOROTZ, 262
TOWBCS, 402, 403
TOWKCS, 402
TOWMCS, 402, 403
TOWSTD, 402, 403
TOWTCS, 402, 403
TOWWCS, 402, 403
TRAFOOF, 114
TRANS, 89, 228, 230, 233, 238
Transition
circle, 364, 384
ellipsis/parabola/hyperbola, 365
radius, 363
Transition current/next block, 359
Transverse axis
Always display actual values as a diameter, 93
Always display actual values as a diameter., 91
Channel-specific diameter dimensions (G90) or
radius dimensions (G91), 91
Channel-specific diameter dimensions
independently of G90/G91, 91
coordinate system, 96
Zero points, 96
Traversing path axes as positioning axes with G0, 127
Traversing with feedforward control, 222
TRUE, 63
TURN, 152
Turning Functions
Axis-specific dimensions for the specified axis, 93
Chamfer, rounding, 194
Channel-specific dimensions for transverse axis, 91
V
Variable identifier, 55
Velocity controls, 201
VELOLIMA, 218
W
WAITMC, 278
WAITP, 278
WAITS, 284, 288
WALCS0, 112
WALCS1-10, 112
WALIMOF, 109
WALIMON, 109
Wear value, 396
Window width for fixed stop monitoring, 189
Words, 50
Working area limitation
in BCS, 108
in WCS/SZS, 111
Reference points on the tool, 110
working area limitation, 109
Working plane, G17 to G19, 104
Workpiece coordinate system, 30
Align on workpiece, 262
X
X, 89, 104, 105
X1, 114, 187
X2, 159
X3, 161
X4, 162
Y
Y, 89, 104, 105
Y1, 114, 187
Z
Z, 89, 104, 105
Z1, 161
Z2, 161
Z3, 161
Z4, 162
Zero frame, 100
Zero offset
Activating the zero offset, 102
Deactivating a zero offset, 103
G54 to G599, 98
Setting the offset values, 101
Zero points, 22
