Siemens SINUMERIK 840DE, SINUMERIK 840D, SINUMERIK 840Di, SINUMERIK 840DiE, SINUMERIK 810D Programming Manual

...

Download

Page 1

Programming Manual 10/2004 Edition

SINUMERIK 840D/840Di/810D Fundamentals

Page 2

Page 3

SINUMERIK 840D/840Di/810D

Fundamentals

Programming Manual

Preface

Fundamental Geometrical Principles

Fundamental Principles of NC Programming

Positional Data

Programming Motion Commands

Path Action

Frames

pplicable to the following controls: SINUMERIK 840D powerline SINUMERIK 840DE powerline (export version) SINUMERIK 840Di SINUMERIK 840DiE (export version) SINUMERIK 810D powerline SINUMERIK 810DE powerline (export version) software version NC 7

Feedrate Control and Spindle Motion

Tool offsets

Special functions

Arithmetic Parameters and Program Jumps

Subprograms and Repetition of Program Sections

Tables

List of abbreviations

10.2004 Edition

6FC5 298-7AB00-0BP1

Page 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 to property damage only 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.

Copyright Siemens AG . All rights reserved. The distribution and duplication of this document or the utilization and transmission of its contents are not permitted without express written permission. Offenders will be liable for damages. All rights, including rights created by patent grant or registration of a utility model or design, are reserved.

Siemens AG Automation and Drives Postfach 4848, 90327 Nuremberg, Germany

Siemens Aktiengesellschaft 6FC5 298-7AB00-0BP1

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 2005 Technical data subject to change

Page 5

Preface

Structure of the documentation

The SINUMERIK documentation is organized in 3 parts:

• General documentation

• User documentation

• Manufacturer/service documentation

Audience

This document is designed for machine tool users. The document describes in detail all the technical facts an operator needs to understand how to program the SINUMERIK 840D/810D control systems.

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.

Please contact your local Siemens office for more detailed information about other SINUMERIK 840D/810D publications and publications that apply to all SINUMERIK controls (e.g., universal interface, measuring cycles, etc.).

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.

Validity

This Programming Guide applies to the following controls:

SINUMERIK 840D powerline 7

SINUMERIK 840DE powerline (export version) 7

SINUMERIK 840Di 3

SINUMERIK 840DiE (export version) 3

SINUMERIK 810D powerline 7

SINUMERIK 810DE powerline (export version) with operator panels OP 010, OP 010C, OP 010S, OP 12,

or OP 15 (PCU 20 or PCU 50)

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

iii

Page 6

Preface

Export version

The following functions are not available in the export version:

Function 810DE 840DE

Five axis machining package − −

Handling transformation package (five axes) − −

Multi-axis interpolation (> four axes) − −

Helical interpolation 2D+6 − −

Synchronized actions, stage 2 − O1)

Measurements, stage 2 − O1)

Adaptive control − O1)

Continuous dressing − O1)

Utilization of compile cycles (OEM) − −

Sag compensation, multi-dimensional − O1)

− function not available

1) limited functionality

Hotline and Internet address

If you have any questions, please get in touch with our hotline:

Description

A&D Technical Support Phone: +49 (0)180 50 50 222

Fax: +49 (0)180 50 50 223

Please send any queries about the documentation (suggestions or corrections) to the following fax number or email address:

Fax: +49 (0)9131 98 21 76

E-mail: [email protected]

Fax form: See the reply form at the end of the document.

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 "Advanced" is intended for use by technicians with in-depth, comprehensive programming knowledge. By virtue of a special programming language, the SINUMERIK 840D/810D control enables the user to program complex workpiece programs (e.g., for sculptured surfaces, channel coordination, etc.) and greatly facilitates the programming of complicated operations.

Fundamentals

iv Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 7

Preface

The commands and statements described in this Guide are not specific to one particular technology.

They could be used, for example, for the following:

• Grinding

• Cyclical machines (packaging, woodworking)

• Laser power controls

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 8

Page 9

Preface ......................................................................................................................................................iii

1 Fundamental Geometrical Principles ......................................................................................................1-1

1.1 Description of workpiece points ................................................................................................. 1-1

1.1.1 Workpiece coordinate systems.................................................................................................. 1-1

1.1.2 Definition of workpiece positions................................................................................................ 1-2

1.1.3 Polar coordinates ....................................................................................................................... 1-5

1.1.4 Absolute dimensions.................................................................................................................. 1-5

1.1.5 Incremental dimension............................................................................................................... 1-7

1.1.6 Plane designations..................................................................................................................... 1-8

1.2 Position of zero points.............................................................................................................. 1-10

1.3 Position of coordinate systems ................................................................................................ 1-11

1.3.1 Overview of various coordinate systems ................................................................................. 1-11

1.3.2 Machine coordinate system ..................................................................................................... 1-12

1.3.3 Basic coordinate system .......................................................................................................... 1-15

1.3.4 Workpiece coordinate system.................................................................................................. 1-17

1.3.5 Frame system .......................................................................................................................... 1-18

1.3.6 Assignment of workpiece coordinate system to machine axes ............................................... 1-20

1.3.7 Current workpiece coordinate system ..................................................................................... 1-21

1.4 Axes ......................................................................................................................................... 1-22

1.4.1 Main axes/Geometry axes ....................................................................................................... 1-23

1.4.2 Special axes............................................................................................................................. 1-24

1.4.3 Main spindle, master spindle ................................................................................................... 1-24

1.4.4 Machine axes ........................................................................................................................... 1-24

1.4.5 Channel axes ........................................................................................................................... 1-25

1.4.6 Path axes ................................................................................................................................. 1-25

1.4.7 Positioning axes....................................................................................................................... 1-25

1.4.8 Synchronized axes................................................................................................................... 1-26

1.4.9 Command axes........................................................................................................................ 1-27

1.4.10 PLC axes...............................................................................................................

1.4.11 Link axes .................................................................................................................................. 1-27

1.4.12 Lead link axes .......................................................................................................................... 1-28

1.5 Coordinate systems and workpiece machining ....................................................................... 1-30

2 Fundamental Principles of NC Programming.......................................................................................... 2-1

2.1 Structure and contents of an NC program ................................................................................. 2-1

2.2 Language elements of the programming language ................................................................... 2-2

2.3 Programming a sample workpiece........................................................................................... 2-21

2.4 First programming example for milling application .................................................................. 2-22

2.5 Second programming example for milling application ............................................................. 2-23

2.6 Programming example for turning application ......................................................................... 2-26

................... 1-27

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

vii

Page 10

Table of contents

3 Positional Data........................................................................................................................................ 3-1

3.1 General notes............................................................................................................................. 3-1

3.1.1 Program dimensions .................................................................................................................. 3-1

3.2 Absolute/relative dimensions ..................................................................................................... 3-2

3.2.1 Absolute dimension (G90, X=AC) .............................................................................................. 3-2

3.2.2 Incremental dimensions (G91, X=IC)......................................................................................... 3-6

3.3 Absolute dimension for rotary axes (DC, ACP, ACN) .............................................................. 3-10

3.4 Dimensions inch/metric, (G70/G700, G71/G710) .................................................................... 3-12

3.5 Special turning functions .......................................................................................................... 3-15

3.5.1 Dimensions for radius, diameter, (DIAMON, DIAMOF, DIAM90) ............................................ 3-15

3.5.2 Position of workpiece ............................................................................................................... 3-17

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA ....................................... 3-19

3.7 Selection of working plane (G17 to G19) ................................................................................. 3-25

3.8 Working area limitation (G25/G26, WALIMON, WALIMOF) .................................................... 3-28

3.9 Reference point approach (G74) ............................................................................................. 3-32

4 Programming Motion Commands ........................................................................................................... 4-1

4.1 General notes............................................................................................................................. 4-1

4.2 Travel commands with polar coordinates, polar angle, polar radius ......................................... 4-4

4.2.1 Defining the pole (G110, G111, G112) ...................................................................................... 4-4

4.2.2 Traversing commands with polar coordinates, (G0, G1, G2, G3 AP=..., RP=...) ...................... 4-5

4.3 Rapid traverse movement (G0, RTLION, RTLIOF) ................................................................... 4-9

4.4 Linear interpolation (G1) .......................................................................................................... 4-14

4.5 Circular interpolation types, (G2/G3, CIP, CT)......................................................................... 4-16

4.6 Circular interpolation with center point and end point (G2/G3, I=, J=, K=AC...) ...................... 4-20

4.7 Circular interpolation with radius and end point (G2/G3, CR).................................................. 4-24

4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)....................................... 4-26

4.9 Circular interpolation with polar coordinates (G2/G3, AP=, RP=)............................................ 4-28

4.10 Circular interpolation with intermediate and end points (CIP).................................................. 4-30

4.11 Circular interpolation with tangential transition (CT) ................................................................ 4-3

4.12 Helical interpolation (G2/G3, TURN=)...................................................................................... 4-36

4.13 Involute interpolation (INVCW, INVCCW)................................................................................ 4-38

4.14 Contour definitions ................................................................................................................... 4-43

4.14.1 Straight line with angle (X2... ANG...) ...................................................................................... 4-43

4.14.2 Two straight lines (ANG1, X3... Z3... ANG2) ........................................................................... 4-44

4.14.3 Three straight lines (ANG1, X3... Z3... ANG2, X4... Z4...) ....................................................... 4-45

4.14.4 End point programming with angle .......................................................................................... 4-47

4.15 Thread cutting with constant lead (G33) .................................................................................. 4-47

4.15.1 Programmable run-in and run-out paths (DITS, DITE) ............................................................ 4-54

4.16 Linear progressive/degressive thread pitch change (G34, G35) ............................................. 4-56

4.17 Tapping without compensating chuck (G331, G332)............................................................... 4-57

4.18 Tapping with compensating chuck (G63)................................................................................. 4-59

4.19 Stop with thread cutting(LFOF, LFON, LFTXT, LFWP, LFPOS) ............................................. 4-61

Fundamentals

viii Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 11

Table of contents

4.19.1 Retraction for thread cutting (LFOF, LFON, LIFTFAST, DILF, ALF) ....................................... 4-61

4.19.2 Lifting on retraction (LFTXT, LFWP, LFPOS, POLF, POLFMASK; POLFMLIN)..................... 4-63

4.20 Approaching a fixed point (G75) .............................................................................................. 4-66

4.21 Travel to fixed stop (FXS, FXST, FXSW) ................................................................................ 4-67

4.22 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM) .................................................. 4-71

5 Path Action ............................................................................................................................................. 5-1

5.1 General notes............................................................................................................................. 5-1

5.1.1 Programming path travel behavior............................................................................................. 5-1

5.2 Exact stop (G60, G9, G601, G602, G603)................................................................................. 5-4

5.3 Continuous-path mode (G64, G641, G642, G643, G644) ......................................................... 5-7

5.4 Acceleration behavior .............................................................................................................. 5-15

5.4.1 Acceleration response, BRISK, SOFT, DRIVE........................................................................ 5-15

5.4.2 Influence of acceleration on following axes (VELOLIMA, ACCLIMA, JERKLIMA).................. 5-17

5.4.3 Technology G groups (DYNNORM, DYNPOS, DYNROUGH, DYNSEMIFIN, DYNFISH)...... 5-19

5.5 Smoothing the path velocity..................................................................................................... 5-20

5.6 Traversing with feedforward control, FFWON, FFWOF........................................................... 5-21

5.7 Contour accuracy, CPRECON, CPRECOF ............................................................................. 5-22

5.8 Dwell time, G4.......................................................................................................................... 5-24

5.9 Internal preprocessor stop ....................................................................................................... 5-25

6 Frames .................................................................................................................................................. 6-1

6.1 General ...................................................................................................................................... 6-1

6.2 Frame instructions ..................................................................................................................... 6-4

6.3 Programmable zero offset.......................................................................................................... 6-6

6.3.1 Zero offset (TRANS, ATRANS).................................................................................................. 6-6

6.3.2 Axial zero offset (G58, G59) .................................................................................................... 6-11

6.4 Programmable rotation (ROT, AROT, RPL) ............................................................................ 6-13

6.5 Programmable frame rotations with solid angles (ROTS, AROTS, CROTS) .......................... 6-24

6.6 Programmable scale factor (SCALE, ASCALE) ...................................................................... 6-25

6.7 Programmable mirroring (MIRROR, AMIRROR) ..................................................................... 6-29

6.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT)..................... 6-34

6.9 Deselect frame (G53, G153, SUPA, G500) .....................

........................................................ 6-38

6.10 Deselect DRF (handwheel) offsets, overlaid motions and transformation (DRFOF, CORROF,

TRAFOOF)............................................................................................................................... 6-39

7 Feedrate Control and Spindle Motion ..................................................................................................... 7-1

7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)............................................................... 7-1

7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC) ............................... 7-9

7.3 Position-controlled spindle operation (SPCON, SPCOF) ........................................................ 7-11

7.4 Positioning spindles (position-controlled axis operation) (SPOS, M19 and SPOSA).............. 7-12

7.5 Milling on turned parts (TRANSMIT)........................................................................................ 7-19

7.6 Cylinder surface transformation (TRACYL) ............................................................................. 7-21

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 12

Table of contents

7.7 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF) ................................. 7-23

7.8 Percentage feedrate override (OVR, OVRA) ........................................................................... 7-25

7.9 Feedrate with handwheel override (FD, FDA) ......................................................................... 7-26

7.10 Percentage acceleration override (ACC option) ...................................................................... 7-30

7.11 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN).................................... 7-32

7.12 Spindle speed (S), direction of spindle rotation (M3, M4, M5)................................................. 7-34

7.13 Constant cutting rate (G96, G961, G97, G971, LIMS)............................................................. 7-37

7.14 Constant grinding wheel peripheral speed (GWPSON, GWPSOF)......................................... 7-41

7.15 Programmable spindle speed limitation (G25, G26) ................................................................ 7-42

7.16 Multiple feedrate values in one block (F.., ST=.., SR=.., FMA.., STA=.., SRA=..)................... 7-43

7.17 Blockwise feed (FB...) .............................................................................................................. 7-45

8 Tool offsets............................................................................................................................................. 8-1

8.1 General notes............................................................................................................................. 8-1

8.1.1 Tool offsets................................................................................................................................. 8-1

8.1.2 Tool offsets in the control's offset memory ................................................................................ 8-2

8.2 List of tool types ......................................................................................................................... 8-5

8.3 Tool selection/tool call T........................................................................................................... 8-12

8.3.1 Tool change with T commands (turning).................................................................................. 8-12

8.3.2 Tool change with M06 (mill) ..................................................................................................... 8-12

8.4 Tool offset D ............................................................................................................................. 8-15

8.5 Tool selection T with tool management ................................................................................... 8-17

8.5.1 Turning machine with circular magazine (T selection)............................................................. 8-18

8.5.2 Milling machine with chain magazine (T selection).................................................................. 8-19

8.6 Tool offset call D with tool management .................................................................................. 8-20

8.6.1 Turning machine with circular magazine (D call) ..................................................................... 8-20

8.6.2 Milling machine with chain magazine (D call) .......................................................................... 8-21

8.7 Activating the active tool offset immediately ............................................................................ 8-22

8.8 Tool radius compensation (G40, G41, G42) ............................................................................ 8-23

8.9 Contour approach and retraction (NORM, KONT, KONTC, KONTT)...................................... 8-32

8.10 Compensation at the outside corners (G450, G451) ............................................................... 8-38

8.11 Smooth approach and retraction.............................................................................................. 8-42

8.11.1 Approach and retraction (G140 to G143, G147, G148, G247, G248, G347, G348, G340, G341)

................................................................................................................................................. 8-42

8.11.2 Approach and retraction with enhanced retraction strategies (G460, G461, G462)................ 8-54

8.12 Collision monitoring (CDON, CDOF, CDOF2) ......................................................................... 8-58

8.13 2 ½ D tool offset (CUT2D, CUT2DF) ....................................................................................... 8-61

8.14 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR)................ 8-63

8.15 Grinding-specific tool monitoring in parts programs (TMON, TMOF) ...................................... 8-66

8.16 Additive offsets ......................................................................................................................... 8-68

8.16.1 Select offsets (via DL numbers)............................................................................................... 8-68

8.16.2 Specify wear and setup values ($TC_SCPxy[t,d], $TC_ECPxy[t,d]) ....................................... 8-69

8.16.3 Delete additive offsets (DELDL)............................................................................................... 8-70

8.17 Special handling of tool offsets ................................................................................................ 8-71

Fundamentals

x Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 13

Table of contents

8.17.1 Mirroring of tool lengths ........................................................................................................... 8-73

8.17.2 Wear sign evaluation ............................................................................................................... 8-74

8.17.3 Coordinate system of the active machining operation

(TOWSTD/TOWMCS/TOWWCS/TOWBCS/TOWTCS/TOWKCS) ......................................... 8-75

8.17.4 Tool length and plane change.................................................................................................. 8-78

8.18 Tools with a relevant cutting edge length ................................................................................ 8-79

9 Special functions..................................................................................................................................... 9-1

9.1 Auxiliary function outputs ........................................................................................................... 9-1

9.1.1 M functions................................................................................................................................. 9-5

9.1.2 H functions ................................................................................................................................. 9-7

10 Arithmetic Parameters and Program Jumps ......................................................................................... 10-1

10.1 Arithmetic parameter (R).......................................................................................................... 10-1

10.2 Unconditional program jumps .................................................................................................. 10-3

10.3 Conditional program jumps (IF, GOTOB, GOTOF, GOTO, GOTOC) ..................................... 10-5

11 Subprograms and Repetition of Program Sections............................................................................... 11-1

11.1 Use of subprograms................................................................................................................. 11-1

11.2 Subprogram call ....................................................................................................................... 11-4

11.3 Subprogram with program repetition ....................................................................................... 11-6

11.4 Program section repetition ....................................................................................................... 11-7

12 Tables................................................................................................................................................... 12-1

12.1 List of statements ..................................................................................................................... 12-1

12.2 List of addresses .................................................................................................................... 12-22

12.3 List of G functions/preparatory functions ............................................................................... 12-30

12.4 List of predefined subprograms ............................................................................................. 12-44

12.4.1 Predefined subprogram calls ................................................................................................. 12-44

12.4.2 Predefined subprogram calls in motion-synchronous actions ............................................... 12-57

12.4.3 Predefined functions .............................................................................................................. 12-58

12.4.4 Data types ..............................................

................................................................................ 12-63

A List of abbreviations................................................................................................................................A-1

A.1 Abbreviations ............................................................................................................................. A-1

Glossary ..................................................................................................................................... Glossary-1

Index

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 14

Page 15

Fundamental Geometrical Principles

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

<

<

=

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

;

1-1

Page 16

Fundamental Geometrical Principles

1.1 Description of workpiece points

Turning:

<

=

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:

Fundamentals

1-2 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 17

Fundamental Geometrical Principles

1.1 Description of workpiece points

<



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



;



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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-3

Page 18

Fundamental Geometrical Principles

1.1 Description of workpiece points

Example of turning positions

Points P1 and P2 are defined by the following coordinates:

;

<

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

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

Fundamentals

1-4 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 19

Fundamental Geometrical Principles

1.1 Description of workpiece points

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:

;

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-5

Page 20

Fundamental Geometrical Principles

1.1 Description of workpiece points

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:

P1 corresponds to X25 Z-7.5

P2 corresponds to X40 Z-15

P3 corresponds to X40 Z-25

3

3 3







3



;







P4 corresponds to X60 Z-35

Fundamentals

1-6 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 21

Fundamental Geometrical Principles

1.1 Description of workpiece points

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

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)

Example of turning

The positions for points P1 to P4 in incremental dimensions are as follows:







3

;



Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-7

Page 22

Fundamental Geometrical Principles

1.1 Description of workpiece points

;

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.

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.

Fundamentals

1-8 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 23

Fundamental Geometrical Principles

1.1 Description of workpiece points

Milling:

*

*

*

;

Turning:

Working planes

;

*

*

*

The third coordinate axis is perpendicular to this plane and determines the infeed direction of the tool (e.g., for 2½ D machining).

The working planes are specified as follows in the NC program with G17, G18 and G19:

Plane

X/Y G17 Z

Z/X G18 Y

Y/Z G19 X

Designation

Infeed direction

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-9

Page 24

Fundamental Geometrical Principles

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:

Reference points

::

;

Turning:



;



%



0

$

:



They are:

M Machine zero A Blocking point. Can coincide with the workpiece zero point (only turning

machines).

W Workpiece zero = Program zero

Fundamentals

1-10 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 25

Fundamental Geometrical Principles

1.3 Position of coordinate systems

R Reference point. Position determined by cams and measuring system.

Start point. Can be defined for each program. Start point of the first tool for machining.

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

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 subsection headed "Axis types".

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-11

Page 26

Fundamental Geometrical Principles

1.3 Position of coordinate systems

Milling coordinate system:

;

Turning coordinate system:

<

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.

;

=

Fundamentals

1-12 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 27

Fundamental Geometrical Principles

1.3 Position of coordinate systems

Right-hand rule

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.

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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-13

Page 28

Fundamental Geometrical Principles

1.3 Position of coordinate systems

=

<

;

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.

Fundamentals

1-14 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 29

Fundamental Geometrical Principles

1.3 Position of coordinate systems

=

%

<

&

<

&

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-15

Page 30

Fundamental Geometrical Principles

1.3 Position of coordinate systems

%DVLFFRRUGLQDWHV\VWHP IRUIURQWIDFH

;

%DVLF FRRUGLQDWHV\VWHP IRUSHULSKHUDOVXUIDFH

:RUNSLHFH FRRUGLQDWHV\VWHP IRUSODQHRIURWDWLRQ

;

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.

Fundamentals

1-16 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 31

Fundamental Geometrical Principles

1.3 Position of coordinate systems

Further determinations



<0&6

<%&6



<%=6

<6=6



<:&6

:&6



;:&6



%=6

%DVLFIUDPHEDVLFRIIVHW

'5)RIIVHW]HURRIIVHWH[WHUQDO

%&6

.LQHPDWLFWUDQVIRUPDWLRQ

0&6

0&6 0DFKLQH&RRUGLQDWH6\VWHP%&6 %DVLF&RRUGLQDWH6\VWHP

%=6 %DVLF=HUR6\VWHP 6=6 6HWWDEOH=HUR6\VWHP

:&6 :RUNSLHFH&RRUGLQDWH6\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.

1.3.4 Workpiece coordinate system

3URJUDPPDEOH)5$0(

6=6

**VHWWDEOH)5$0(6



;%&6



;0&6



;%=6



;6=6



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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-17

Page 32

Fundamental Geometrical Principles

1.3 Position of coordinate systems

The workpiece coordinate system is always a Cartesian coordinate system and assigned to a specific workpiece.

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 DURXQGWKH=D[LV

=

<

=HURRIIVHW

;

;

<

<

;

It is a spatial description of the workpiece coordinate system

The following components are available within a frame:

• Zero offset

• Rotate

• Mirroring

• Scaling

Fundamentals

1-18 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 33

Fundamental Geometrical Principles

1.3 Position of coordinate systems

These components can be used individually or in any combination.

Mirroring of the Z axis

;

=HURRIIVHW

:

=HURRIIVHW

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.

;

0

;

... 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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

;

1-19

Page 34

Fundamental Geometrical Principles

1.3 Position of coordinate systems

• 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.

• 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.

Fundamentals

1-20 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 35

Fundamental Geometrical Principles

1.3 Position of coordinate systems

<0 =

;0 ;

;

=0 =

*

The settable frames are activated in the NC program by means of commands such as G54.

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.

<

&XUUHQWZRUNSLHFH FRRUGLQDWHV\VWHP

=

<

)UDPH

=

)UDPHVHWWDEOHRIIVHWDQGURWDWLRQ )UDPHSURJUDPPDEOHRIIVHWDQGURWDWLRQ

Several zero offsets are possible in the same program.

)UDPH

; :RUNSLHFH FRRUGLQDWHV\VWHP

;

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-21

Page 36

Fundamental Geometrical Principles

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

*HRPHWU\D[HV

0DFKLQHD[HV

*HRPHWU\D[HV

3DWKD[HV

6\QFKU D[HV

3RVLWLRQLQJ D[HV

.LQHPDWLFWUDQVIRUPDWLRQ

3RVLWLRQLQJD[HV

&KDQQHOD[HV

&RPPDQG D[HV

0DFKLQHD[HV

6SHFLDOD[HV

3/&D[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.

Fundamentals

1-22 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 37

Fundamental Geometrical Principles

1.4 Axes

• 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.

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.

5HYROYHUVZLYHO D[LV

7RROV

;

0DLQVSLQGOH PDVWHUVSLQGOH &D[LV

*HRPHWU\ D[HV

6SHFLDOVSLQGOH

6SHFLDOD[LV

7DLO VWRFN

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).

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-23

Page 38

Fundamental Geometrical Principles

1.4 Axes

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.

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.

Fundamentals

1-24 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 39

Fundamental Geometrical Principles

1.4 Axes

The machine axis names are programmed only in special cases, such as reference point or fixed point approaching.

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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-25

Page 40

Fundamental Geometrical Principles

1.4 Axes

• Loaders for moving workpieces away from machine

• Tool magazine/turret

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.

Fundamentals

1-26 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 41

Fundamental Geometrical Principles

1.4 Axes

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.

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.

1&8

&KDQQHO

&KDQQHO

/LQNPRGXOH+:

'

$

$

$

/LQNFRPPXQLFDWLRQ

1&8

&KDQQHO

/LQNPRGXOH+:

'

%

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-27

Page 42

Fundamental Geometrical Principles

1.4 Axes

Precondition

The participating NCUs, NCU1 and NCU2, must be connected by means of high-speed communication via the link module. References: /PHD/, Configuring Manual 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: Function description /FB/ B3, Multiple Operator Panels and NCUs

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: Function description /FB/ B3, Multiple Operator Panels and NCUs

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.

Fundamentals

1-28 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 43

Fundamental Geometrical Principles

1.4 Axes

'

%

1&8

,QWHUSRODWRU

6HUYR

%

1&8Q



1&8

,QWHUSRODWRU

6HUYR

'

$

6HWSRLQWVIURP$

&KDQQHOFRQWURO E\IROORZLQJ D[LVD[HV

$FWXDOYDOXHV IURP$

1&8OLQNPRGXOH

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

Programming

Prerequisites

• Tangential correction

• Electronic gear (ELG)

• Synchronous spindle

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.

• 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 571-573.2, Link Module

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-29

Page 44

Fundamental Geometrical Principles

1.5 Coordinate systems and workpiece machining

• 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: /FB/ Function description B3, Multiple Operator Panels and NCUs

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

Fundamentals

1-30 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 45

Fundamental Geometrical Principles

1.5 Coordinate systems and workpiece machining

$[LVPRYHPHQWSURJUDPPHGLQWKHZRUNSLHFHFRRUGLQDWHV\VWHP

'HVFULSWLRQRIWKH ZRUNSLHFHJHRPHWU\YLDJHRPHWU\ D[HVHJ;<=

)UDPHFDOFXODWLRQ 2IIVHW75$16 5RWDWLRQ527 6FDOLQJ6&$/(

&RQWRXULQ&DUWHVLDQ FRRUGLQDWHV\VWHP RIWKHFKDQQHO%&6

7RROUDGLXVFRPSHQVDWLRQ

0RYHPHQWRI WRRO]HUR LQ%&6

7RROOHQJWKFRPSHQVDWLRQ .LQHPDWLFWUDQVIRUPDWLRQLIDFWLYH

'HVFULSWLRQRIWRRO RULHQWDWLRQE\PHDQVRI RULHQWDWLRQYHFWRU(XOHUDQJOH

5RWDU\D[HVIRU D[LVWUDQVIRUPDWLRQ

5HPDLQLQJWUDYHUVLQJ LQVWUXFWLRQV YLDVRFDOOHGVSHFLDOD[HV HJ&89

)UDPHFDOFXODWLRQ 2IIVHW 6FDOLQJ

Path calculation

0RYHPHQWRIPDFKLQHD[HVRIFKDQQHODEF

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)

;

SRLQW

9DOXH

$EVROXWH

$EVROXWHSRVLWLRQ

6HW SRLQW YDOXH

6HW

SRVLWLRQ

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).

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

1-31

Page 46

Fundamental Geometrical Principles

1.5 Coordinate systems and workpiece machining

193

193

$EVROXWHGLPHQVLRQVVHWSRLQWIRU3

$EVROXWH GLPHQVLRQV VHWSRLQW IRU3

$FWXDOYDOXH

:.3

$FWXDOYDOXH

3

0RWLRQ

:.3

'LVWDQFH

3

Fundamentals

1-32 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 47

Fundamental Principles of NC Programming

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 ... ;1st Set

Set N20 G2 Z37 ... ;2nd 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.

Punch tape format

File names:

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-1

Page 48

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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

%flange3_MPF = part program flange3

For further information on downloading, creating, and storing parts programs, please refer to:

/BAD/, /BEM/ Operating Instructions HMI Advanced, HMI Embedded section "Program operating area" / "Services operating area"

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 extension 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

Fundamentals

2-2 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 49

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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.

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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-3

Page 50

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

LF End of block

Tab character Separator

space character Separator (blank)

Words

Note

Non-printable special characters are treated like blanks.

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.

:RUG

$GGUHVV

*

:RUG

$GGUHVV

1XPEHUVWULQJ

:RUG

$GGUHVV

; 6

1XPEHUVWULQJ

6HW

The address character of the word is usually a letter. The sequence of digits can contain a leading sign and decimal point. The leading sign always appears between the address letter and the sequence of digits. The positive leading 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 "L

Fundamentals

2-4 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

" (LINE FEED = new line).

Page 51

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

Note

The "L

" 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 "L

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.

Word sequence in blocks

In order to keep the block structure 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…)

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-5

Page 52

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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.

Block number

Note

Main blocks can be contained in both main programs and subprograms. The control does not check whether a main block contains all the necessary information.

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.

Fundamentals

2-6 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 53

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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(...)

ADIS Rounding clearance for path functions fixed

B=DC(...) B=ACP(...) B=ACN(...)

C=DC(...) C=ACP(...) C=ACN(...)

CHR=... Chamfer the contour corner fixed

D... Cutting edge number fixed

F... Feed fixed

FA[axis]=... or FA[spindle]=... or [SPI(spindle)]=...

G... Preparatory function fixed

H... H=QU(...)

I... Interpolation parameters variable

J... Interpolation parameters variable

K... Interpolation parameters variable

L... Subprogram call fixed

M... M=QU(...)

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]=...

SPOSA=... SPOSA[n]=...

Q... Axis variable

R0=... to Rn=... R...

Rotary axis variable

Axial feed (only if spindle no. defined by variable)

Auxiliary function Auxiliary function without read stop

Miscellaneous (i.e., special) function Miscellaneous fct. w/o read stop

Spindle position fixed

Spindle position across block boundary fixed

Arithmetic parameter, n can be set via MD (default 0-99)

- Axis

fixed

variable

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-7

Page 54

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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(...)

Y... Y=AC(...) Y=IC(...)

Z... Z=AC(...) Z=IC(...)

AR+=... Aperture angle variable

AP=... Polar angle variable

CR=... Circle radius variable

RP=... Main block fixed

:... variable

Axis " absolute " incremental

Axis variable

variable

"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.

Fundamentals

2-8 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 55

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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.

Example:

X7 ;No "=" required, 7 is a value, but the "=" character can 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:

;also be used here

Address Meaning

X, Y, Z Axis addresses

I, J, K Interpolation parameters

S Spindle speed

SPOS, SPOSA

M Special functions

H Auxiliary functions

T Tool number

F Feed

Spindle position

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 M[SPINU]=3 ;Clockwise rotation for the spindle, whose number is stored in

T[SPINU]=7 ;Selection of the tool for the spindle, whose number is stored

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

;SPINU variables. the

;SPINU variables. in the

;SPINU variables.

2-9

Page 56

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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 Subprogram call

M Miscellaneous (i.e., special) function

N Subblock

P Number of program passes

R Arithmetic variables

S Spindle speed

T Tool number

: Main block

Example for programming:

N10 G54 T9 D2

Fixed addresses with axis extension

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 extension, the axis to be traversed is enclosed in square brackets.

You will find a complete list of all fixed addresses in the Appendix.

Fundamentals

2-10 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 57

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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

• Approximate positioning 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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-11

Page 58

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

Operators/mathematical functions

Operators and mathematical functions

+ Addition

- Subtraction

* Multiplication

/ Division

DIV Division, for variable types INT and REAL

MOD Modulo division (INT type only) produces the remainder of INT division, e.g.,

: Chain operator (for FRAME variables)

Sin() Sine

COS() Cosine

TAN() Tangent

ASIN() Arcsine

ACOS() Arccosine

ATAN2() Arctangent2

SQRT() Square root

ABS() Absolute number

POT() 2nd power (square)

TRUNC() Truncate to integer

ROUND() Round to integer

LN() Natural logarithm

EXP() Exponential function

Meaning

Notice!: (type INT)/(type INT)=(type REAL); e.g., 3/4 = 0.75

Notice!: (type INT)DIV(type INT)=(type INT); e.g., 3 DIV 4 = 0

3 MOD 4=3

Comparison and logic operators

== 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

Fundamentals

2-12 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Meaning

Page 59

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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. Leading 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

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

;numeric extension (1), "=" required

;"=" required

Names

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.

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

• Subprograms

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-13

Page 60

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

• Vocabulary words

• 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 vocabulary words must not be used as identifiers. Separators are not permitted between the individual characters.

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.

Fundamentals

2-14 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 61

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

• All identifiers beginning with "E_ " are reserved for EASYSTEP 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.

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 leading sign ±(231 - 1)

REAL Real numbers (fractions with decimal

point, LONG REAL to IEEE)

BOOL Boolean values: TRUE (1) and

FALSE (0)

CHAR ASCII character specified by the

code

STRING Character string, number of

characters in [...], maximum of 200 characters

AXIS Axis names (axis addresses) only Any axis identifiers in the channel

FRAME Geometrical parameters for

translation, rotation, scaling, and mirroring

±(10-300 … 10+300)

1, 0

0 … 255

Sequence of values with 0 ... 255

Identical elementary types can be combined in arrays. Up to two-dimensional arrays are possible.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-15

Page 62

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

Constants

Integer constants

Integer with or without leading 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!

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 "Programming Guide Advanced"):

$MC_TOOL_MANAGEMENT_MASK='H3C7F' ;Assignment of hexadecimal values to

The maximum number of characters is limited by the value range of the integer data type.

Binary constants

;machine data

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.

Fundamentals

2-16 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 63

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

Example for machine data (see also "Programming Guide Advanced"):

$MN_AUXFU_GROUP_SPEC='B10000001' ;Assignment of binary constants to

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

;machine data bit 0 and 7 are set

Skipping blocks

Blocks, which are not to be executed in every program pass (e.g., execute a trial program run), can be skipped.

1

1

1

1

1

1

1

1

1

1

1

1

3URJUDPH[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 instructions in the skipped blocks are not executed; the program continues with the next block, which is not skipped.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-17

Page 64

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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.

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 (":").

For further information refer to

References: /PGA/, Programming Guide Advanced.

Fundamentals

2-18 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 65

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

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

N50 ;Section no. 12, housing for submersible pump type

;on November 21, 1994 TP23A

Note

Comments are stored and appear in the current block display when the program is running.

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 vocabulary word "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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-19

Page 66

Fundamental Principles of NC Programming

2.2 Language elements of the programming language

Setting alarms

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]<<)

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 vocabulary word "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 MMC.

Programmable cycle alarms

A character string containing up to 4 parameters can be specified in addition to the alarm number for the predefined subprogram SETAL.

Fundamentals

2-20 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 67

Fundamental Principles of NC Programming

2.3 Programming a sample workpiece

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

2.3 Programming a sample workpiece

Programming

Procedures

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.

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.

• 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?

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-21

Page 68

Fundamental Principles of NC Programming

2.4 First programming example for milling application

– 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)?

• 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

• Start the parts program

References: See Operator's Guide

Note

Alarms can occur during program verification. These alarms have to be reset first.

Fundamentals

2-22 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 69

Fundamental Principles of NC Programming

2.5 Second programming example for milling application

Machine manufacturer

The machine data settings must be defined correctly before the program can run on the machine.

References: /FB1/ Functional description, K2, "Axes, Coordinate Systems,.."

Programming 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,

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

;tool offset, spindle clockwise

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/Functional description, K2, "Axes, Coordinate Systems,.."

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********************

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-23

Page 70

Fundamental Principles of NC Programming

2.5 Second programming example for milling application

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 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

Fundamentals

2-24 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 71

Fundamental Principles of NC Programming

2.5 Second programming example for milling application





N215 X4.25 ;Drill third hole N220 MCALL N221 SUPA Z0 D0 M5 M9 ;Delete modal call. Z axis traverses to ;machine

N225 SUPA X0 Y0 MSG () N230 M30 ;End of program



5



;Drill second hole

zero











;'3



 







'LPHQVLRQVDUHLQLQFKHV

6LGHYLHZ 'LPHQVLRQVLQLQFKHV



5

5

Dimension drawing of workpiece "The Raised Boss" (not to scale).



Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-25

Page 72

Fundamental Principles of NC Programming

2.6 Programming example for turning application

Radius programming and tool radius compensation

The sample program contains radius programming and tool radius compensation.

Programming 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

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

N130 G0 G53 X280 Z380 D0 M5 ;Move to tool change location N135 M30 ;Program end

tool change location

compensation

Fundamentals

2-26 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 73

Fundamental Principles of NC Programming

2.6 Programming example for turning application

5

r

5















5







;

5











Machine manufacturer

The MD settings must be defined correctly before the program can run on the machine.

References: /FB/ Functional description, K2, "Axes, Coordinate Systems,.."

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

2-27

Page 74

Page 75

Positional Data

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°.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-1

Page 76

Positional Data

3.2 Absolute/relative dimensions

• 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.

• Diametral programming, DIAMON on

• Diametral programming, DIAMOF off

Diametral 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(...)

Fundamentals

3-2 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 77

Positional Data

3.2 Absolute/relative dimensions

Parameters

G90 Absolute reference dimension X Y Z Axis identifiers of the axes to be

AC Absolute dimensions non-modally effective

traversed

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

N20 G1 Z-5 F500 ;Tool infeed at feedrate N30 G2 X20 Y35 I=AC(45) J=AC(35) ;Circle center point in absolute

N40 G0 Z2 ;Retracting N50 M30 ;End of block

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

;

;XYZ, tool, spindle on ;clockwise

dimensions

3-3

Page 78

Positional Data

3.2 Absolute/relative dimensions

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

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

N40 G1 Z-40 ;Retracting

Description

Absolute dimensions, G90

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.













;to position XYZ

dimensions

Non-modal absolute dimensioning AC

When G91 is active, AC can be used to allow entry of incremental dimensions for individual axes in a specific block.

Fundamentals

3-4 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 79

Positional Data

3.2 Absolute/relative dimensions

Milling:



*



*

 

 



*

*

;

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 G90 is performed using the commands DIAMON, DIAMOF or DIAM90.

For dimensioning for diameter or radius see

Circular interpolation, G2/G3

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-5

Page 80

Positional Data

3.2 Absolute/relative dimensions

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.





 

;

Fundamentals

3-6 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 81

Positional Data

3.2 Absolute/relative dimensions

N10 G90 G0 X45 Y60 Z2 T1 S2000 M3 ;Absolute dimensioning, rapid traverse to N20 G1 Z-5 F500 ;Tool infeed at feedrate

N30 G2 X20 Y35 I0 J-25) ;Circle center point in incremental 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.

;

;XYZ, tool, spindle on clockwise

dimensions













N5 T1 D1 S2000 M3 ;Tool, spindle on clockwise N10 G0 G90 X11 Z1 ;Absolute dimensioning, rapid traverse to

N20 G1 Z-15 F0.2 ;Tool infeed at feedrate N30 G3 X11 Z-27 I-8 K-6 ;Circle center point in incremental

N40 G1 Z-40 ;Retracting N50 M30 ;End of block

;position XYZ

dimensions

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-7

Page 82

Positional Data

3.2 Absolute/relative dimensions

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

N30 G90 X50 ;Traverse to position X75, the offset

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:

;not traversed ;is traversed



*



*

 

 



*

;

*

Fundamentals

3-8 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 83

Positional Data

3.2 Absolute/relative dimensions

Turning:

;

*

*



*

*



G91 extension

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.

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

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-9

Page 84

Positional Data

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(…)

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

ACN Absolute dimensions, approach position in negative

direction 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

;

Fundamentals

3-10 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 85

Positional Data

3.3 Absolute dimension for rotary axes (DC, ACP, ACN)

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

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 positions 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).

;clockwise direction (positive), the tool ;mills a circular groove

$&3 $&1

0D[LPXP 7UDYHUVLQJUDQJH

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-11

Page 86

Positional Data

3.4 Dimensions inch/metric, (G70/G700, G71/G710)

All of the commands are non-modal.

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

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 system of units set in G700/G710.

The controller interprets all feedrates used with G700/G710 in the programmed system of units, unlike G70/G71.

The programmed feedrate value is modal and thus does not change automatically on subsequent G70/G71/G700/G710 selections.

Example of milling

Change between metric and imperial input with basic setting metric (G70/G71).

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])

Fundamentals

3-12 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 87

Positional Data

3.4 Dimensions inch/metric, (G70/G700, G71/G710)

*

* *





Description





*

;

G70 ;is active until deselected by G71 or ;end of program

program







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,

N50 X1.18 Y3.54 N60 G71 X 20 Y30 ;Enter positions in mm N70 G0 Z2 M30 ;Retract in rapid traverse, end of

G70 or G71

You can instruct the control to convert the following geometrical dimensions (with necessary deviations) into the system of units not set and enter them directly:

Examples

• Positional data X, Y, Z, ...

• Intermediate point coordinates I1, J1, K1

Interpolation parameters I, J, K and circle radius CR in circle programming

• Thread lead (G34, G35)

• Programmable zero offset (TRANS)

• Polar radius RP

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-13

Page 88

Positional Data

3.4 Dimensions inch/metric, (G70/G700, G71/G710)

Further information

All other parameters such as feedrates, tool offsets or settable zero offsets are interpreted (when using G70/G71) in the default system of units (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/, Description of Functions, Basic Machine, G2 section "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 system of units is used.

References:/PGA/ Programming Guide, Advanced, Section "Movement Synchronized Actions".

/FBSY/ , Description of Functions, Synchronized Actions

Fundamentals

3-14 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 89

Positional Data

3.5 Special turning functions

3.5.1 Dimensions for radius, diameter, (DIAMON, DIAMOF, DIAM90)

Function

The free choice of diameter or radius dimensions allows you to program the dimensions straight from the engineering drawing without conversion.

Programming

',$021

'

;

'

',$02)

5

;

5

After power up of

• DIAMON/DIAM90, diameter dimensions are defined for the specified transverse axis. as diameter.

• DIAM90 is displayed as a diameter, irrespective of the traversing method (G90/G91) the actual value of the transverse axis. This also applies to reading of actual values in the workpiece coordinate system with MEAS, MEAW, $P_EP[x] and $AA_IW[x].

DIAMON

DIAMOF

DIAM90

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-15

Page 90

Positional Data

3.5 Special turning functions

Parameters

Absolute dimensioning (G90) Incremental dimensioning DIAMON Diameter Diameter

DIAMOF Radius (for default, see DIAM90 Diameter Radius

The diameter programming is set with DIAM90 for G90 and

machine manufacturer)

the radius programming for G91.

Further information

The commands for diameter and radius data are modal.

By programming DIAMOF you can switch at any time to radius as dimension.

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, independent of G90/G91 interpolation parameters inG2/G3, if these are programmed with AC absolutely

(G91)

Radius

Example

• Actual values read in the workpiece coordinate system in MEAS, MEAW, $P_EP[X], $AA_IW[X] (see PGA, Programming Guide "Advanced")

N10 G0 X0 Z0 Approach starting point N20 DIAMOF Diameter input off N30 G1 X30 S2000 M03 F0.7 X axis = transverse axis; radius

N40 DIAMON Diameter dimensions active N50 G1 X70 Z-20 Traverse to diameter position X70 and

N60 Z-30 N70 DIAM90 Diameter programming for absolute

N80 G91 X10 Z-20 Incremental dimension N90 G90 X10 Absolute dimensions N100 M30 ; End of program

dimensions active Traverse to radius position X30

Z–20

dimensions and radius programming for incremental dimensions

Fundamentals

3-16 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 91

Positional Data

3.5 Special turning functions

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.

:RUNSLHFH ]HUR IURQW

:RUNSLHFH ]HUR UHDU

;

0DFKLQH

**RU75$16

;

0DFKLQH

** RU75$16

;

:RUNSLHFH

; :RUNSLHFH

= :RUNSLHFH

:RUNSLHFH

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-17

Page 92

Positional Data

3.5 Special turning functions

;

7UDQVYHUVHD[LV

Parameters

/RQJLWXGLQDOD[LV

'

'

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)

Fundamentals

3-18 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 93

Positional Data

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-19

Page 94

Positional Data

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA

Turning:

;

Programming

Call-up G54

Or G55

Or G56

Or G57

Or G505 … G599

Switching off G53

Or G500

Or SUPA

Or G153

*

Fundamentals

3-20 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 95

Positional Data

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA

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

G500 G500=zero frame, default setting,

SUPA Non-modal deactivation, including programmed offsets,

G153 Non-modal suppression of settable, programmable and total

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 zero offset (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. handwheel offsets (DRF), external zero offset and PRESET

offset. basic frame

Example

• Programmable scalings, e.g., SCALE, ASCALE

• Programmable mirrorings, e.g., MIRROR, AMIRROR

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-21

Page 96

Positional Data

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA

;

Description

*

*

*

75$16;0

;

N10 G0 G90 X10 Y10 F500 T1 ;Approach N20 G54 S1000 M3 ;Call the first zero offset,

N30 L47 ;Run program, in this case as a N40 G55 G0 Z200 ;Call the second zero offset 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

;spindle clockwise subprogram ;Z via obstacle

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

Fundamentals

3-22 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 97

Positional Data

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA

6FDOLQJ

;

5RWDWH

2II FVHW

;

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.

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

3-23

Page 98

Positional Data

3.6 Zero offset (frame), G54 to G57, G505 to G599, G53, G500/SUPA

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".

Fundamentals

3-24 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Page 99

Positional Data

3.7 Selection of working plane (G17 to G19)

Function

By specification of working plane, in which the 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

Programming

;

,QIHHG

Call-up

G17

G18

G19

*

*

*

,QIHHG

Parameters

G17 Working plane X/Y G18 Working plane Z/X G19 Working plane Y/Z

Fundamentals Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1

Infeed direction Z Plane selection 1st - 2nd geometry axis Infeed direction Y Plane selection 3rd - 1st geometry axis Infeed direction X Plane selection 2nd - 3rd geometry axis

3-25

Page 100

Positional Data

3.7 Selection of working plane (G17 to G19)

Important

In the basic setting, preset for millingG17 (X/Y plane) and G18 (Z/X plane) for turning.

With selection of the tool path compensationG41/G42 (see section "Tool offsets") the working plane must be specified so that the control can correct the tool length and radius.

Example for milling

The "conventional" approach with milling tool:

• define working plane (G17 basic setting for milling),

• select tool type (T) and tool offset values (D),

• switch on path compensation (G41),

• program traversing movements.

N10 G17 T5 D8 ;G17 selection of the working plane, here

N20 G1 G41 X10 Y30 Z-5 F500 The radius compensation is performed in N30 G2 X22.5 Y40 I50 J40 Circular interpolation / tool radius

X/Y T, ;D tool selection. The length compensation is performed in the Z direction

the X/Y plane. compensation in the X/Y plane.

Description

It is advisable to define the working plane G17 to G19 at the beginning of the program. In the basic setting the Z/X plane is preset for turning G18

Fundamentals

3-26 Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1