Siemens SINUMERIK 840D sl Owner's manual


SINUMERIK
SINUMERIK 840D sl / 828D
Fundamentals
Programming Manual
Validfor
Controlsystem
SINUMERIK840Dsl/840DEsl
SINUMERIK828D
Software  Version
CNC-Software 4.4
09/2011
6FC5398-1BP40-2BA0
Preface
Fundamental Geometrical
Principles 1
Fundamental Principles of
NC Programming 2
Creating an NC program 3
Tool change 4
Tool offsets 5
Spindle motion 6
Feed control 7
Geometry settings 8
Motion commands 9
Tool radius compensation 10
Path action 11
Coordinate transformations
(frames) 12
Auxiliary function outputs 13
Supplementary commands 14
Other information 15
Tables 16
Appendix A

Legal information- Warning notice system
Legal information
Warning notice system
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.
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 product/system described in this documentation may be operated only by personnel qualified for the specific
task in accordance with the relevant documentation for the specific task, in particular its warning notices and safety
instructions. Qualified personnel are those who, based on their training and experience, are capable of identifying
risks and avoiding potential hazards when working with these products/systems.
Proper use of Siemens products
Note the following:
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.
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.
WARNING
Siemens products may only be used for the applications described in the catalog and in the relevant technical
documentation. If products and components from other manufacturers are used, these must be recommended or
approved by Siemens. Proper transport, storage, installation, assembly, commissioning, operation and
maintenance are required to ensure that the products operate safely and without any problems. The permissible
ambient conditions must be adhered to. The information in the relevant documentation must be observed.
Siemens AG
Industry Sector
Postfach 48 48
90026 NÜRNBERG
GERMANY
Order number:6FC5398-1BP40-2BA0
Ⓟ 01.2011
Copyright © SiemensAG 2011.
Technical data subject to change

Fundamentals
Programming Manual 09/2011, 6FC5398-1BP40-2BA0 3
Preface
SINUMERIK documentation
The SINUMERIK documentation is organized in the following categories:
• General documentation
• User documentation
• Manufacturer/service documentation
Additional information
You can find information on the following topics at www.siemens.com/motioncontrol/docu:
• Ordering documentation/overview of documentation
• Additional links to download documents
• Using documentation online (find and search in manuals/information)
Please send any questions about the technical documentation (e.g. suggestions for
improvement, corrections) to the following address:
[e-mail]
My Documentation Manager (MDM)
Under the following link you will find information to individually compile OEM-specific machine
documentation based on the Siemens content:
www.siemens.com/mdm
Training
For information about the range of training courses, refer under:
• www.siemens.com/sitrain
SITRAIN - Siemens training for products, systems and solutions in automation technology
• www.siemens.com/sinutrain
SinuTrain - training software for SINUMERIK
FAQs
You can find Frequently Asked Questions in the Service&Support pages under Product
Support. http://support.automation.siemens.com

Preface
Fundamentals
4Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
SINUMERIK
You can find information on SINUMERIK under the following link:
www.siemens.com/sinumerik
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.
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
You will find telephone numbers for other countries for technical support in the Internet under
http://www.siemens.com/automation/service&support

Preface
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 5
Information on structure and contents
"Fundamentals" and "Advanced" Programming Manual
The description of the NC programming is divided into two manuals:
1. Fundamentals
This "Fundamentals" Programming Manual 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.
2. Job planning
The Programming Manual "Advanced" is intended for use by technicians with in-depth,
comprehensive programming knowledge. By virtue of a special programming language,
the SINUMERIK control enables the user to program complex workpiece programs (e.g.
for free-form surfaces, channel coordination, ...) and makes programming of complicated
operations easy for technologists.
Availability of the described NC language elements
All NC language elements described in the manual are available for the SINUMERIK 840Dsl.
The availability regarding SINUMERIK828D can be found in table"Operations: Availability for
SINUMERIK 828D [Page 489]".

Preface
Fundamentals
6Programming Manual, 09/2011, 6FC5398-1BP40-2BA0

Fundamentals
Programming Manual 09/2011, 6FC5398-1BP40-2BA0 7
Table of contents
Preface.........................................................................................................................................................3
1 Fundamental Geometrical Principles ........................................................................................................13
1.1 Workpiece positions .................................................................................................................. 13
1.1.1 Workpiece coordinate systems .................................................................................................. 13
1.1.2 Cartesian coordinates ................................................................................................................ 14
1.1.3 Polar coordinates ....................................................................................................................... 17
1.1.4 Absolute dimensions ................................................................................................................. 18
1.1.5 Incremental dimension .............................................................................................................. 20
1.2 Working planes.......................................................................................................................... 22
1.3 Zero points and reference points............................................................................................... 23
1.4 Coordinate systems................................................................................................................... 25
1.4.1 Machine coordinate system (MCS) ........................................................................................... 25
1.4.2 Basic coordinate system (BCS) ................................................................................................. 28
1.4.3 Basic zero system (BZS) ........................................................................................................... 30
1.4.4 Settable zero system (SZS) ....................................................................................................... 31
1.4.5 Workpiece coordinate system (WCS) ........................................................................................32
1.4.6 What is the relationship between the various coordinate systems? .......................................... 32
2 Fundamental Principles of NC Programming ............................................................................................33
2.1 Name of an NC program ........................................................................................................... 33
2.2 Structure and contents of an NC program................................................................................. 35
2.2.1 Blocks and block components ................................................................................................... 35
2.2.2 Block rules ................................................................................................................................. 37
2.2.3 Value assignments .................................................................................................................... 38
2.2.4 Comments ................................................................................................................................. 39
2.2.5 Skipping blocks .......................................................................................................................... 40
3 Creating an NC program ...........................................................................................................................43
3.1 Basic procedure......................................................................................................................... 43
3.2 Available characters .................................................................................................................. 45
3.3 Program header......................................................................................................................... 47
3.4 Program examples .................................................................................................................... 49
3.4.1 Example 1: First programming steps ......................................................................................... 49
3.4.2 Example 2: NC program for turning ........................................................................................... 50
3.4.3 Example 3: NC program for milling ............................................................................................ 52
4 Tool change ..............................................................................................................................................55
4.1 Tool change without tool management...................................................................................... 56
4.1.1 Tool change with T command ................................................................................................... 56
4.1.2 Tool change with M6 ................................................................................................................. 57
4.2 Tool change with tool management (option) ............................................................................. 59
4.2.1 Tool change with T command with active tool management (option) ........................................ 59

Table of contents
Fundamentals
8 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
4.2.2 Tool change with M6 with active tool management (option) ...................................................... 62
4.3 Behavior with faulty T programming .......................................................................................... 64
5 Tool offsets ................................................................................................................................................65
5.1 General information about the tool offsets................................................................................. 65
5.2 Tool length compensation.......................................................................................................... 66
5.3 Tool radius compensation.......................................................................................................... 67
5.4 Tool compensation memory ...................................................................................................... 68
5.5 Tool types .................................................................................................................................. 70
5.5.1 General information about the tool types ................................................................................... 70
5.5.2 Milling tools ................................................................................................................................ 71
5.5.3 Drills ........................................................................................................................................... 73
5.5.4 Grinding tools ............................................................................................................................. 74
5.5.5 Turning tools .............................................................................................................................. 75
5.5.6 Special tools .............................................................................................................................. 77
5.5.7 Chaining rule .............................................................................................................................. 78
5.6 Tool offset call (D)...................................................................................................................... 79
5.7 Change in the tool offset data.................................................................................................... 82
5.8 Programmable tool offset (TOFFL, TOFF, TOFFR) .................................................................. 83
6 Spindle motion ..........................................................................................................................................89
6.1 Spindle speed (S), direction of spindle rotation (M3, M4, M5)................................................... 89
6.2 Cutting rate (SVC) ..................................................................................................................... 93
6.3 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC)....................... 100
6.4 Constant grinding wheel peripheral speed (GWPSON, GWPSOF)......................................... 106
6.5 Programmable spindle speed limitation (G25, G26)................................................................ 108
7 Feed control ............................................................................................................................................109
7.1 Feedrate (G93, G94, G95, F, FGROUP, FL, FGREF)............................................................. 109
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC) ............................. 118
7.3 Position-controlled spindle operation (SPCON, SPCOF) ........................................................ 122
7.4 Positioning spindles (SPOS, SPOSA, M19, M70, WAITS)...................................................... 123
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF) ................................. 133
7.6 Programmable feedrate override (OVR, OVRRAP, OVRA) .................................................... 137
7.7 Programmable acceleration override (ACC) (option)............................................................... 139
7.8 Feedrate with handwheel override (FD, FDA) ......................................................................... 141
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN).................................... 145
7.10 Several feedrate values in one block (F, ST, SR, FMA, STA, SRA)........................................ 148
7.11 Non-modal feedrate (FB)......................................................................................................... 151
7.12 Tooth feedrate (G95 FZ).......................................................................................................... 152

Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 9
Table of contents
8 Geometry settings ...................................................................................................................................159
8.1 Settable work offset (G54 to G57, G505 to G599, G53, G500, SUPA, G153) ........................ 159
8.2 Selection of the working plane (G17/G18/G19)....................................................................... 165
8.3 Dimensions.............................................................................................................................. 168
8.3.1 Absolute dimensions (G90, AC) .............................................................................................. 168
8.3.2 Incremental dimensions (G91, IC) ........................................................................................... 171
8.3.3 Absolute and incremental dimensions for turning and milling (G90/G91) ............................... 174
8.3.4 Absolute dimension for rotary axes (DC, ACP, ACN) .............................................................. 175
8.3.5 Inch or metric dimensions (G70/G700, G71/G710) ................................................................. 177
8.3.6 Channel-specific diameter/radius programming (DIAMON, DIAM90, DIAMOF,
DIAMCYCOF) .......................................................................................................................... 180
8.3.7 Axis-specific diameter/radius programming (DIAMONA, DIAM90A, DIAMOFA,
DIACYCOFA, DIAMCHANA, DIAMCHAN, DAC, DIC, RAC, RIC) .......................................... 183
8.4 Position of workpiece for turning ............................................................................................. 188
9 Motion commands ...................................................................................................................................191
9.1 General information about the travel commands..................................................................... 191
9.2 Travel commands with Cartesian coordinates (G0, G1, G2, G3, X..., Y..., Z...) ...................... 193
9.3 Travel commands with polar coordinates ................................................................................ 195
9.3.1 Reference point of the polar coordinates (G110, G111, G112) ............................................... 195
9.3.2 Travel commands with polar coordinates (G0, G1, G2, G3, AP, RP) ...................................... 197
9.4 Rapid traverse movement (G0, RTLION, RTLIOF) ................................................................. 201
9.5 Linear interpolation (G1).......................................................................................................... 206
9.6 Circular interpolation................................................................................................................ 209
9.6.1 Circular interpolation types (G2/G3, ...) ................................................................................... 209
9.6.2 Circular interpolation with center point and end point (G2/G3, X... Y... Z..., I... J... K...) ......... 212
9.6.3 Circular interpolation with radius and end point (G2/G3, X... Y... Z.../ I... J... K..., CR) ........... 216
9.6.4 Circular interpolation with opening angle and center point (G2/G3, X... Y... Z.../
I... J... K..., AR) ........................................................................................................................ 218
9.6.5 Circular interpolation with polar coordinates (G2/G3, AP, RP) ................................................ 220
9.6.6 Circular interpolation with intermediate point and end point (CIP, X... Y... Z...,
I1... J1... K1...) ......................................................................................................................... 222
9.6.7 Circular interpolation with tangential transition (CT, X... Y... Z...) ............................................ 225
9.7 Helical interpolation (G2/G3, TURN) ....................................................................................... 229
9.8 Involute interpolation (INVCW, INVCCW) ............................................................................... 232
9.9 Contour definitions................................................................................................................... 237
9.9.1 General information about contour definitions ......................................................................... 237
9.9.2 Contour definitions: One straight line (ANG) ........................................................................... 238
9.9.3 Contour definitions: Two straight lines (ANG) ......................................................................... 240
9.9.4 Contour definitions: Three straight line (ANG) ......................................................................... 244
9.9.5 Contour definitions: End point programming with angle .......................................................... 247
9.10 Thread cutting with constant lead (G33).................................................................................. 248
9.10.1 Thread cutting with constant lead (G33, SF) ........................................................................... 248
9.10.2 Programmable run-in and run-out paths (DITS, DITE) ............................................................ 256
9.11 Thread cutting with increasing or decreasing lead (G34, G35) ............................................... 258

Table of contents
Fundamentals
10 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
9.12 Tapping without compensating chuck (G331, G332)............................................................... 260
9.13 Tapping with compensating chuck (G63) ................................................................................ 265
9.14 Fast retraction for thread cutting (LFON, LFOF, DILF, ALF, LFTXT, LFWP, LFPOS,
POLF, POLFMASK, POLFMLIN)............................................................................................. 267
9.15 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM) .................................................. 271
10 Tool radius compensation .......................................................................................................................277
10.1 Tool radius compensation (G40, G41, G42, OFFN)................................................................ 277
10.2 Contour approach and retraction (NORM, KONT, KONTC, KONTT)...................................... 287
10.3 Compensation at the outside corners (G450, G451, DISC) .................................................... 294
10.4 Smooth approach and retraction ............................................................................................. 298
10.4.1 Approach and retraction (G140 to G143, G147, G148, G247, G248, G347, G348,
G340, G341, DISR, DISCL, FAD, PM, PR) ............................................................................. 298
10.4.2 Approach and retraction with enhanced retraction strategies (G460, G461, G462) ................ 309
10.5 Collision monitoring (CDON, CDOF, CDOF2)......................................................................... 313
10.6 2D tool compensation (CUT2D, CUT2DF) .............................................................................. 317
10.7 Keep tool radius compensation constant (CUTCONON, CUTCONOF) .................................. 320
10.8 Tools with a relevant cutting edge position.............................................................................. 323
11 Path action ..............................................................................................................................................325
11.1 Exact stop (G60, G9, G601, G602, G603)............................................................................... 325
11.2 Continuous-path mode (G64, G641, G642, G643, G644, G645, ADIS, ADISPOS)................ 328
12 Coordinate transformations (frames) ......................................................................................................337
12.1 Frames..................................................................................................................................... 337
12.2 Frame instructions ................................................................................................................... 339
12.3 Programmable zero offset ....................................................................................................... 343
12.3.1 Zero offset (TRANS, ATRANS) ............................................................................................... 343
12.3.2 Axial zero offset (G58, G59) .................................................................................................... 347
12.4 Programmable rotation (ROT, AROT, RPL) ............................................................................ 350
12.5 Programmable frame rotations with solid angles (ROTS, AROTS, CROTS) .......................... 360
12.6 Programmable scale factor (SCALE, ASCALE) ...................................................................... 362
12.7 Programmable mirroring (MIRROR, AMIRROR) ..................................................................... 365
12.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT) ..................... 370
12.9 Deselect frame (G53, G153, SUPA, G500)............................................................................. 373
12.10 Deselecting overlaid movements (DRFOF, CORROF) ........................................................... 374
13 Auxiliary function outputs ........................................................................................................................377
13.1 M functions .............................................................................................................................. 381

Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 11
Table of contents
14 Supplementary commands .....................................................................................................................385
14.1 Messages (MSG)..................................................................................................................... 385
14.2 Writing string in OPI variable (WRTPR) .................................................................................. 387
14.3 Working area limitation ............................................................................................................ 388
14.3.1 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF) ........................................ 388
14.3.2 Working area limitation in WCS/SZS (WALCS0 ... WALCS10) ............................................... 392
14.4 Reference point approach (G74) ............................................................................................. 395
14.5 Fixed-point approach (G75, G751).......................................................................................... 396
14.6 Travel to fixed stop (FXS, FXST, FXSW) ................................................................................ 401
14.7 Acceleration behavior .............................................................................................................. 406
14.7.1 Acceleration mode (BRISK, BRISKA, SOFT, SOFTA, DRIVE, DRIVEA) ............................... 406
14.7.2 Influence of acceleration on following axes (VELOLIMA, ACCLIMA, JERKLIMA) .................. 409
14.7.3 Activation of technology-specific dynamic values (DYNNORM, DYNPOS, DYNROUGH,
DYNSEMIFIN, DYNFINISH) .................................................................................................... 411
14.8 Traversing with feedforward control, FFWON, FFWOF .......................................................... 413
14.9 Contour accuracy, CPRECON, CPRECOF............................................................................. 414
14.10 Dwell time (G4)........................................................................................................................ 415
14.11 Internal preprocessing stop ..................................................................................................... 417
15 Other information ....................................................................................................................................419
15.1 Axes......................................................................................................................................... 419
15.1.1 Main axes/Geometry axes ....................................................................................................... 421
15.1.2 Special axes ............................................................................................................................ 422
15.1.3 Main spindle, master spindle ................................................................................................... 422
15.1.4 Machine axes .......................................................................................................................... 423
15.1.5 Channel axes ........................................................................................................................... 423
15.1.6 Path axes ................................................................................................................................. 423
15.1.7 Positioning axes ...................................................................................................................... 424
15.1.8 Synchronized axes .................................................................................................................. 425
15.1.9 Command axes ....................................................................................................................... 425
15.1.10 PLC axes ................................................................................................................................. 425
15.1.11 Link axes ................................................................................................................................. 426
15.1.12 Lead link axes .......................................................................................................................... 428
15.2 From travel command to machine movement ......................................................................... 430
15.3 Path calculation ....................................................................................................................... 431
15.4 Addresses................................................................................................................................ 432
15.5 Identifiers ................................................................................................................................. 436
15.6 Constants ................................................................................................................................ 438

Table of contents
Fundamentals
12 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
16 Tables .....................................................................................................................................................441
16.1 Operations ............................................................................................................................... 441
16.2 Operations: Availability for SINUMERIK 828D ........................................................................ 489
16.3 Addresses................................................................................................................................ 511
16.4 G function groups .................................................................................................................... 520
16.5 Predefined subroutine calls ..................................................................................................... 536
16.6 Predefined subroutine calls in motion-synchronous actions.................................................... 551
16.7 Predefined functions................................................................................................................ 552
16.8 Currently set language in the HMI ........................................................................................... 557
A Appendix .................................................................................................................................................559
A.1 List of abbreviations................................................................................................................. 559
A.2 Documentation overview ......................................................................................................... 564
Glossary...................................................................................................................................................567

Fundamentals
Programming Manual 09/2011, 6FC5398-1BP40-2BA0 13
1
Fundamental Geometrical Principles
1.1 Workpiece positions
1.1.1 Workpiece coordinate systems
In order that the machine or the control can work with the positions specified in the NC
program, these specifications have to be made in a reference system that can be transferred
to the directions of motion of the machine axes. A coordinate system with the axes X, Y and Z
is used for this purpose.
DIN 66217 stipulates that machine tools must use clockwise, right-angled (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 position specifications. For
this reason, positions that are to the left of the zero point are assigned a negative sign ("-").
Figure 1-1 Workpiece coordinate system for
turning
Figure 1-2 Workpiece coordinate system for
milling
=
= ;
;
<
r
r
r:
<
;
; <
<
=
=
r
r
r
:

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
14 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
1.1.2 Cartesian coordinates
The axes in the coordinate system are assigned dimensions. In this way, it is possible to
clearly describe every point in the coordinate system and therefore every workpiece position
through the direction (X, Y and Z) and three numerical values The workpiece zero always has
the coordinates X0, Y0, and Z0.
Position specifications in the form of Cartesian coordinates
To simplify things, we will only consider one plane of the coordinate system in the following
example, the X/Y plane:
Points P1 to P4 have the following coordinates:
Position Coordinates
P1 X100 Y50
P2 X-50 Y100
P3 X-105 Y-115
P4 X70 Y-75
;
;
<
<




3
3
3
3





Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 15
Example: Workpiece positions for turning
With lathes, one plane is sufficient to describe the contour:
Points P1 to P4 have the following coordinates:
Position Coordinates
P1 X25 Z-7.5
P2 X40 Z-15
P3 X40 Z-25
P4 X60 Z-35
=
;




3
3 3
3




Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
16 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Example: Workpiece positions for milling
For milling, the feed depth must also be described, i.e. the third coordinate (in this case Z)
must also be assigned a numerical value.
Points P1 to P3 have the following coordinates:
Position Coordinates
P1 X10 Y45 Z-5
P2 X30 Y60 Z-20
P3 X45 Y20 Z-15



3
3
3
3
 



3
3

<
=
<
;

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 17
1.1.3 Polar coordinates
Polar coordinates can be used instead of Cartesian coordinates to describe workpiece
positions. This is useful when a workpiece or part of a workpiece has been dimensioned with
radius and angle. The point from which the dimensioning starts is called the "pole".
Position specifications in the form of polar coordinates
Polar coordinates are made up of the polar radius and the polar angle.
The polar radius is the distance between the pole and the position.
The polar angle is the angle between the polar radius and the horizontal axis of the working
plane. Negative polar angles are in the clockwise direction, positive polar angles in the
counterclockwise direction.
Example
Points P1 and P2 can then be described – with reference to the pole – as follows:
Position Polar coordinates
P1 RP=100 AP=30
P2 RP=60 AP=75
RP: Polar radius
AP: Polar angle
3ROH
;
<
3
3
r
r





Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
18 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
1.1.4 Absolute dimensions
Position specifications in absolute dimensions
With absolute dimensions, all the position specifications refer to the currently valid zero point.
Applied to tool movement this means:
the position, to which the tool is to travel.
Example: Turning
In absolute dimensions, the following position specifications result for points P1 to P4:
Position Position specification in absolute dimensions
P1 X25 Z-7.5
P2 X40 Z-15
P3 X40 Z-25
P4 X60 Z-35
=
;




3
3 3
3




Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0 19
Example: Milling
In absolute dimensions, the following position specifications result for points P1 to P3:
Position Position specification in absolute dimensions
P1 X20 Y35
P2 X50 Y60
P3 X70 Y20
;
<



3
3
3




Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
20 Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
1.1.5 Incremental dimension
Position specifications in incremental dimensions
In production drawings, the dimensions often do not refer to a zero point, but to another
workpiece point. So that these dimensions do not have to be converted, they can be specified
in incremental dimensions. In this method of dimensional notation, a position specification
refers to the previous point.
Applied to tool movement this means:
The incremental dimensions describe the distance the tool is to travel.
Example: Turning
In incremental dimensions, the following position specifications result for points P2 to P4:
Position Position specification in incremental dimensions The specification refers to:
P2 X15 Z-7.5 P1
P3 Z-10 P2
P4 X20 Z-10 P3
=
;


3
3 3
3





Note
With DIAMOF or DIAM90 active, the set distance in incremental dimensions (G91) is
programmed as a radius dimension.