LTI MOTION MotionOne CM Programming Manual

Download

Page 1

SystemOne CM – CNC

Page 2

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

MotionOne CM G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Valid for G&M Code version since: V 6.06.04.00 Doc version: V 7.00.00.01

The German version is the original of this manual.

All rights are reserved with respect to the content of this documentation and the availability to the product.

Copyright © All content of the documentation, in particular the text, photographs and graphics it contains are protected by copyright. The copyright lies, unless otherwise expressly stated, with LTI Motion GmbH.

We reserve the right to make technical changes. The content of this documentation was compiled with the greatest care and attention, and based on the latest information available to us. We should nevertheless point out that this document cannot always be updated in line with ongoing technical developments in our products. Information and specifications may be subject to change at any time. For information on the latest version please visit www.lti-motion.com.

LTI Motion GmbH LTI Motion GmbH Schlätterstraße 2 Gewerbestraße 5-9 88142 Wasserburg/Bodensee 35633 Lahnau Germany Germany Fon +49 8382 9855-0 Fon.: +49 6441 966-0 Fax +49 8382 9855-50 Fax: +49 6441 966-137 info@lti-motion.com info@lti-motion.com www.lti-motion.com www.lti-motion.com

Page 3

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Content

General information ................................................................................................................................................................ 5

Notes and symbols ....................................................................................................................................................... 5

Address letters ............................................................................................................................................................. 5

Axis numbers ............................................................................................................................................................... 5

Axis code word (AKW) .................................................................................................................................................. 6

Components of a NC program ................................................................................................................................................. 7

M Functions............................................................................................................................................................................. 8

G Functions ............................................................................................................................................................................. 9

General explanations .................................................................................................................................................... 9

G00 Positioning in rapid traverse ................................................................................................................................. 10

G01 Positioning at the feed rate .................................................................................................................................. 11

G02 Circular interpolation - Clockwise .......................................................................................................................... 12

G03 Circular interpolation - Counterclockwise............................................................................................................... 12

G04 Dwell time .......................................................................................................................................................... 13

G05 Spatial arc interpolation ....................................................................................................................................... 14

G14 Macro call ........................................................................................................................................................... 15

G17 Plane XY ............................................................................................................................................................. 16

G18 Plane ZX ............................................................................................................................................................. 16

G19 Plane YZ ............................................................................................................................................................. 16

G22 Sub program call ................................................................................................................................................. 17

G23 Text - Functions .................................................................................................................................................. 18

G25 RTCP .................................................................................................................................................................. 19

G26 Free plane .......................................................................................................................................................... 22

G27 Tool zero point .................................................................................................................................................... 24

G30 Spline interface (online spline) ............................................................................................................................. 26

G40 Deletion of the milling cutter radius correction ...................................................................................................... 27

G41 Milling cutter radius correction left ....................................................................................................................... 27

G42 Milling cutter radius correction right ..................................................................................................................... 28

G43 Milling cutter radius correction up to..................................................................................................................... 29

G44 Milling cutter radius correction via ........................................................................................................................ 30

Zero offsets and coordinate rotation ............................................................................................................................ 31

G53 Deletion of the zero offset ................................................................................................................................... 32

G70 Units of measurement inch .................................................................................................................................. 33

G71 Units of measurement mm ................................................................................................................................... 33

G72 Deletion of mirror image machining and scaling .................................................................................................... 33

G73 Mirror image machining ....................................................................................................................................... 34

G73 Scaling ............................................................................................................................................................... 35

G79 Cycle execution ................................................................................................................................................... 36

G90 Absolute measure ............................................................................................................................................... 37

G91 Relative measure ................................................................................................................................................ 38

G92 Relative zero point offset coordinate rotation ........................................................................................................ 39

G93 Absolute zero point offset coordinate rotation ....................................................................................................... 40

G94 Speed programming ............................................................................................................................................ 42

G95 Time programming .............................................................................................................................................. 43

G107 Eroding: Define the directional vector for the lift-off movement ............................................................................ 44

G181 Probe calibration ............................................................................................................................................... 45

G190 Absolute circle center ........................................................................................................................................ 46

G191 Relative circle center ......................................................................................................................................... 47

G288 Set Look Ahead parameters ............................................................................................................................... 48

G288,0 Look Ahead basic parameter ................................................................................................................... 48

G488 Simple measurement block ................................................................................................................................ 49

G488,1 Simple measurement block ............................................................................................................................. 53

G581 Continuous operation cycle rotation .................................................................................................................... 54

G781,1 Spindle offset ................................................................................................................................................. 55

G783,0 Read/Write zero points ................................................................................................................................... 56

G1000 Eroding: Velocity ............................................................................................................................................. 57

G1001 Eroding: Directions .......................................................................................................................................... 58

G1002 Eroding: Factors and modes ............................................................................................................................. 59

G1003 Eroding: Time data .......................................................................................................................................... 60

G1004 Eroding: Orbital movement in the selected plane ............................................................................................... 61

Page 4

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Parameter programming ...................................................................................................................................................... 62

Flexible G&M code Programming (FlexProg) ........................................................................................................................ 63

General ..................................................................................................................................................................... 63

Restrictions ................................................................................................................................................................ 64

General program structure .......................................................................................................................................... 64

Data types ................................................................................................................................................................. 64

Functions (general) .................................................................................................................................................... 65

Function declaration ................................................................................................................................................... 65

Macros and Q parameters .......................................................................................................................................... 65

Function definition ..................................................................................................................................................... 66

Variables ................................................................................................................................................................... 66

Communication variables ............................................................................................................................................ 67

Expressions and operators .......................................................................................................................................... 68

Mathematical functions ............................................................................................................................................... 68

Assignment of NC addresses ....................................................................................................................................... 69

Comment marks......................................................................................................................................................... 69

Point definition ........................................................................................................................................................... 69

Instructions ............................................................................................................................................................... 70

Jump marks ............................................................................................................................................................... 70

GOTO/IF ... GOTO/ IF ELSE ........................................................................................................................................ 70

FOR loops .................................................................................................................................................................. 71

WHILE loops .............................................................................................................................................................. 71

DO ... WHILE loops .................................................................................................................................................... 71

SWITCH ... CASE branching ........................................................................................................................................ 72

Sample programs ....................................................................................................................................................... 73

Index .................................................................................................................................................................................... 78

Revisions ............................................................................................................................................................................... 80

Page 5

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

General information

Notes and symbols

This description uses the following symbols:

Important notes, information or cross references to other descriptions.

This symbol indicates an example.

Address letters

Character

Function

Block number

Path condition

A, B, C

Path information A axis, B axis, C axis

Path information X axis, dwell time

Y, Z

Path information Y axis, Z axis

I, J, K

Interpolation parameters, circle center

Feed rate, time for G95 (inverse time programming)

Output address

Additional information (cutting edge correction table)

Additional information on the PLC

Spindle speed

Tool number

Machine function

Command extension

Axis numbers

Axis

Number

Axis

Number

A 0

X‘

8 X 1

Y‘

9 Z 2 P 10

Y 3 Q 11

B 4 R 12 C 5 U 13 D 6 V 14 E 7 W 15

Page 6

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Axis code word (AKW)

The cycle call-up parameters do not allow all axis letters of the andronic to be specified. This is why for some cycles the axis values other than XYZABC must be specified by means of a list containing the values for the individual axes and by means of an axis code. The axis code word describes for which axes valid values have been specified.

Note: To determine the axis code, the program WINAKW.exe in the directory C:/andron/tools or the following table in which the example is shown for the axes X, Y and Z can be used.

The program

WINAKW.exe

to determine

the axis code

The example shows how to specify values for X Y Z U V W.

FKV[1] = 45.5 FKV[3] = 15.5 FKV[2] = 43.5 FKV[13] = 45.7 FKV[14] = 5.5 FKV[15] = 4.6 Gxxx K57358

; Specify value for X ; Specify value for Y ; Specify value for Z ; Specify value for U ; Specify value for V ; Specify value for W ; Call cycle via axis code K (AKW decimal, see picture)

Page 7

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Components of a NC program

The sequence of a machining process on the machine is described by the NC program. It consists mainly of a sequence of program records. In a program record all the necessary information for a work step are included. Record numbers can be entered under the address N.

With the andronic control, the programming is also permissible without block numbers.

With program words, as a general principle, a differentiation is made between modal (latching) and non-modal words. A word is modal if its value remains effective until it is overwritten by another value, or the end of the program has been reached. In contrast, non-modal words only have an effect within the block in which they have been programmed.

The following can be programmed within a block.

Character

Function N

Block number (optional)

Path condition

Path information A axis

Path information B axis

Path information C axis

Path information X axis, dwell time

Path information Y axis

Path information Z axis

I, J, K

Interpolation parameters, circle center

Feed speed, dwell time, time display at G95 (Invers Time Programming)

Output address

Auxiliary information (correction memory)

Additional information on the PLC

Spindle speed

Tool number

Machine function

Command extension

G02 X50 Y0 I25 J0 F2000 S10000 M3 T7 M6

G02

Path condition circle in clockwise direction

X50

X coordinate

Y coordinate

I25

Auxiliary parameter circle center X coordinate

Auxiliary parameter circle center Y coordinate

F2000

Feed speed 2000 mm/min

S10000

Spindle speed 10000 1/min

M03

Machine function 'Spindle on'

M06

Machine function 'Change tool'

Special characters

The rest of the line is interpreted as a comment

;

The rest of the line is interpreted as a comment

[ ]

Jump mark, index at FlexProg

/*...*/

Encapsulated comment at FlexProg

( )

Comment, function bracket at FlexProg

Page 8

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

M Functions

Note:

The M functions initiate certain machine functions. These functions may differ depending on machine type/manufacturer.

General M functions

Function

C.*

M00

Programmed stop

M01

Optional stop

1 M02

End of program

M19

Spindle stop with defined end position

1 M30

End of program with spindle 0 Off

M functions for control type eroding "EROD"

Function

C.*

M92

Lift-off via programmed direction vector (G107 …)

2 M93

Delete last retraction point

M94

Spark erosion function AFC OFF, no forward and backward interpolation

M95

Spark erosion function AFC ON

M96

Retreat on the path ON

2 M97

Retreat via points ON

M98

Saving the actual position as a retraction point

2 M800

Switching off collision protection via NC program

M801

Switch collision protection on again

2 M802

Modulo formation off

M802

Modulo formation on

2 M900

Activate sparking out

* Comments on the M commands: 1

Function is effective at end of block

Function is effective at start of block

Page 9

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G Functions

General explanations

Property:

MODAL means that the command/function remains active until it is overwritten.

Topic:

The G functions can be divided into the following topics:

 interpolation type  special command  setup command  tool command  cycle command  eroding command

Position:

DEF = Default (active after starting the control unit)

--- = Not pre-set

Page 10

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G00 Positioning in rapid traverse

Property

modal

Topic

Axis movement

Position

---

Syntax

G00

The path information G00 programs rapid traverse movements by specifying the target point. The target point is reached by entering it either in absolute or relative dimensions. The rapid traverse speed can be defined in the MotionCenter.

G00 X50 Y50 ; The axes are moved by interpolation to point P1

Page 11

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G01 Positioning at the feed rate

Property

modal

Topic

Axis movement

Position

DEF

Syntax

G01

The path information G01 programs feed movements by specifying the target point. The target point is reached by entering it either in absolute measure or relative measure. The feed rate can be defined in the MotionCenter or programmed by means of the F parameter.

G01 X50 Y50 F2000 ; Positioning at point P1 at 2000 mm/min

Page 12

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G02 Circular interpolation - Clockwise G03 Circular interpolation - Counterclockwise

Property

modal

Topic

Axis movement

Position

---

Syntax

G02 /G03 <Parameter list>

For the circular interpolation, the axes are moved on an arc from the starting point to the end point. The movement can take place clockwise by selecting G03 and counterclockwise by selecting G03. Circular interpolation must contain the following parameters and can be applied in all 3 planes (see G17 - G18):

G02 or G03 (direction of rotation), end point of the arc, radius of the circle (R) or circle center (I, J, K) The center of the arc can be specified in absolute (G190) or relative (G191) coordinates. As an alternative to the center, the radius can be programmed directly by entering the address letter R. However, this only applies to arcs having an angle of rotation of less than 180°.

G01 X0 Y0 ; Starting point approach G02 X0 Y0 I20 J0 ; Clockwise travel to X0 Y0. Circle center at X20 Y0 (A) G03 X0 Y0 I-20 J0 ; Counterclockwise travel to X0 Y0. Circle center at X-20 Y0 (B) G02 X0 Y-40 R20 ; Clockwise travel to X0 Y-40. Radius 20 mm (C)

Page 13

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G04 Dwell time

Property

Non modal

Topic

NC command

Position

---

Syntax

G04 <Parameter list>

Unit

Seconds

Dwell time

The function G04 allows you to program a dwell time. The time is specified by the parameter X. The function is only effective blockwise. G04 must stand alone in an NC program line

For synchronization of FlexProg calculation and motion, G04 can be used, since a contour interruption takes place. This also applies to the dwell time X0.

Address

Value range

Unit

Accuracy

0 sec – 2 years Default 0

sec

Standard: 0.01 sec LPN: 10 nsec

LPN

If the control has been equipped with an LPN card and pulsing has been activated via "G1010 O1", the dwell time will be executed at higher accuracy. The time can then be programmed to the nearest 10ns, i.e., the smallest value is 0.00000001 seconds. During this time, the pulses are output to the P output of the LPN card with a predefined pulse width. For laser application, this function is called "stationary pulsing" or "piercing".

Value range: 0 – 4 500 000 sec

G04 X11.4 G04 X0 G04

; Dwell time 11.4 seconds ; Dwell time 0 seconds ; Contour interruption

Page 14

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G05 Spatial arc interpolation

Property

modal

Topic

Axis movement

Position

---

Syntax

G05 <Parameter list>

This function allows you to describe a spatial arc (spatial circle section). No information such as radius or direction of rotation exists for this function. An G&M code for spatial arc interpolation must contain the following parameters: G05, end point of the spatial arc in X, Y and Z (A), intermediate point on the spatial arc in I, J and K (B). The starting point (C) of the spatial arc is determined by the current axis position.

G01 X0 Y0 Z0 ; Starting point approach G05 X50 Y50 Z0 I20 J30 K30 ; End point at X50 Y50 Z0 ; Intermediate point at X20 Y30 Z30

Page 15

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G14 Macro call

Property

non-modal

Topic

Special command

Position

---

Syntax

G14 N = [“] Macro name [“] [Pn]

A macro is a closed program part that must be programmed only once. A macro is not executed until it is defined or called by the main program or another macro. In contrast to the genuine subprograms, macros are incorporated in the program text. A macro starts with a header in which the name of the macro is defined. No other instructions (not even block numbers) may be programmed in the header. The name of the macro must not contain more than 24 characters and stands between the character #. The end of the macro definition is marked by a block containing the instruction ##. Here, too, no other instructions may be programmed.

#Rectangle# ; Header containing the name of the macro G01 X0 Y0 F2000 ; Instructions X100 Y100 X0 Y0 ## ; End identifier

The optional inverted comma characters [“] at the beginning and end of the name only have to be entered if the name of the macro contains symbols or blanks. The optional address letter 'P', followed by a number, indicates how many times the macro is to be executed. The maximum number of repetitions is: 256

If a macro has been defined as described above, it can be called in the program as follows.

G14 N = Rectangle P3 ; Example macro called three times

Page 16

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G17 Plane XY G18 Plane ZX G19 Plane YZ

Property

modal

Topic

Setup command

Position

Preset G17

Syntax

G17 / G18 / G19

ATTENTION:

 G18 in the CNC is not according to the DIN 66025.  The use of G18 according to DIN 66025 can be activated in the XPanel user

interface – Service – F6-System programs – F4-System configuration – G&M converter – „G18 according to DIN 66025“.

NOTE:

 A change of plane via G17/G18/G19 does not cancel active zero offsets.

NOTE:

 A change of plane with G17/G18/G19 does not cancel an active rotation.

Page 17

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G22 Sub program call

Property

non-modal

Topic

Special command

Position

---

Syntax

G22 N = [“] Program name [“] [Pn] G22 N = [“] Database path: Program name [“] [Pn]

Programs that must be repeated several times can be called from a main program by entering G22. This program is available as a separate NC program in the same database as the calling main program. If the program to be called is not included in the program database of the control, the database path must also be specified. Enter the designation from "Programs / data base:" to call the database path in the XPanel. Example: G22 n="C01:ncprg_name" is loading from the user database path 1 G22 n="S05: ncprg_name" is loading from the system database path 5

The program name may contain 24 characters maximum. The optional inverted comma characters [“]

at the beginning and end of the name only have to be entered if the program name contains symbols or blanks. The optional address letter 'P', followed by a number, indicates how many times the program is to be executed. The maximum number of repetitions is: 32534

G22 N = Feed program P3 ; Feed program called three times

Page 18

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G23 Text - Functions

Property

non-modal

Topic

NC command

Position

---

Syntax

G23 N = “Text “ P<Type> I<Index>

The command G23 can be used to call up different functions with ASCII texts. The target is always to transmit a text with a length of 80 characters to the PLC, CNC or the display.

Type - P

Command

Index - I

3 Transfer text to the XPanel user interface

1-3 (Default: 1)

4 Redefines the measuring log file names of the measuring cycles "mprot.log". If no path is specified, the data are transmitted to %andronroot%\System\ (C:\Andron\System\*). Specified paths are not created by the CNC and must already exist at program start.

not necessary

Writes the values of the communication variables into a log file. The name for the log file is specified according to the same rules as for P=4, whereby the database path of the current G&M code program is used as standard.

IKV index 0 – 999 Default: 0

G23 P3 N=“Finishing part1“

Text is displayed in the prompt of the XPanel position menue in line 1.

G23 P3 N =“ Finishing part1“ I1

Text is displayed in the prompt of the XPanel position menue in line 1.

G23 P3 N =“ Finishing outside“ I2

Text is displayed in the prompt of the XPanel position menue in line 2.

G23 P4 N =“C:\Messung_123.log“

Beginning with this program line, the measuring cycles of the log file will be named with the specified designation C01: and the path specification and no longer with "C:\andron\ SystemData\Repository\Local Control\Measuring Protocol\mprot.log"

IKV[100] = 156 G23 P5 N =“C:\Daten_123.log“ I100

The value of IKV[100] is written into the log file "C:\andron\SystemData\Repository\Cycles\Measuring Protocol\Daten_123.log".

Page 19

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G25 RTCP

Property

modal

Topic

Transformation command

Position

---

Syntax

G25 <Parameter list>

RTCP describes the functionality of keeping a (TCP - Tool Center Point) constant during the movement of rotatory axes. Despite the use of rotatory axes, the position of the TCP relative to the workpiece does not change. RTCP normally effects a compensation movement of the corresponding axes if one of the rotary axes is moved. RTCP can be switched on/off with the H parameter to G25. The storing and restoring of RTCP states is administered specifically to the program, i.e. if RTCP is deactivated in the sub-program but the state RTCP active was stored in the main program, the state RTCP is actively restored after returning from the sub-program and the RTCP command.

G-Befehl

Bezeichnung

Bedeutung

G25 H0

Switch off RTCP

RTCP is deactivated

G25 H1

Switch on RTCP

RTCP is activated according to the kinematics of the machine defined in the machine parameters.

G25 H2

Save RTCP state

The state of RTCP (ON/OFF) is stored in the buffer, e.g. to be used with tool change NC sets

G25 H3

Restore RTCP state

The state of RTCP (ON/OFF) stored in the buffer is restored, e.g. with a temporary deactivation in the tool change NC sets

Page 20

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Functional description

Axis traverse movement in milling lengthwise axis direction

The use of axis traverse movement in milling lengthwise axis direction is possible by defining the cinematic models regardless of an activated transformation.

Activation/deactivation must be realised by adaptations in the PLC software:

1. On/Off button

2. LED ON for active / LED OFF for inactive

3. Flashing LED for invalid selection or selection not acknowledged by the CNC

Selection of traverse movement in milling lengthwise axis direction via this key on the machine operating panel in manual mode (not MDI, not AUTOMATIC interruption!).

The traverse movement is carried out by pressing the traverse movement keys in positive or negative direction (+/- and selection of the corresponding fixed path 1mm, 0.1mm, 0.01mm, 0.001mm or free movement via the +/- keys or the hand wheel). A negative traverse path is preset by a movement to the tool tip and a positive traverse path is preset by a movement to the tool shank.

Moving in the milling lengthwise axis direction is not possible in the automatic mode.

Activation and deactivation of 5-axis transformation

The status of the transformation is displayed in the status area in the top right corner on the XPanel with the text "G25 RTCP” on an icon.

Activation in the manual mode is possible by pressing the corresponding key. Activation in the MDI and automatic mode is also possible by entering G25 H1.

In the position display, the position in the programming coordinate system (PROG system) is always shown on the display of the control positions. Upon activation or deactivation, the coordinates move depending on the position of the rotatory axes.

G25 H1 G25 H0

RTCP can be activated and deactivated as often as required within an G&M code program.

Behaviour upon NC RESET

If RTCP is active, it also remains active after an NC RESET.

Page 21

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

EMERGENCY STOP by operator, PLC, control programs

RTCP is not reset automatically.

EMERGENCY STOP due to drive error

RTCP is not reset automatically.

Referencing all axes or one axis

RTCP is not reset automatically.

Tool change with RTCP active

G25 H2: RTCP must be deactivated in the tool change program. The status of the function (on or off) is saved at the same time.

G25 H3: After tool change, the previous status of the RTCP function in the tool change program is restored.

Changing axis settings in RTCP

The axis setting can be changed manually in the automatic interruption mode and the program can be continued. The speed control is, however, optimised with regard to the previous axis setting and is maintained. The changed setting is retained until the next rotary axis positioning takes place.

Moving axes in MDI with RTCP active

All axes may be moved in MDI. There is no restriction as a function of the RTCP function.

G72/G73 Mirroring and RTCP

The G73 command makes it possible to activate the mirroring around the X or Y axis or also both axes (prior to the activation of RTCP).

Programmed feed F

The programmed feed with active RTCP always refers to the resulting path of all programmed axes.

The tool is set down in a configurable order. For large angular positions, we therefore

recommend positioning the rotatory axes in the manual mode.

Page 22

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G26 Free plane

Property

modal

Topic

Setup command

Position

---

Syntax

G26 <Parameter list>

Syntax

G26 without parameters deactivates the plane function

The command is used for defining the rotation of the programming coordinate system. It effects a rotation around the specified angles in the given order, the center of rotation is the current zero point. The aim is the definition of a new machining plane which must not obligatorily be parallel to one of the main planes. No movement takes place after specification of G26. But the display of the current control position changes to the position with reference to the new system. After the command was entered the changed coordinate system immediately becomes effective.

Parameters

Description

Switch H is used to define the application of rotation WX, WY and WZ. If H is not specified, H0 is applied.

The rotations are defined by means of Euler angle resp. solid angle. The angles are defined as follows:

 WX - Rotation around the current Z axis  WY - Turning around the new Y axis  WX - Rotation around the new Z axis

The rotations are always executed in this order, I, J and K must not necessarily be specified. The specification of WX and WY is normally sufficient.

The angular positions are to be applied in a given order, which is specified with I, J, and K. As a default the following order applies: I1 J2 K3. Independent from the programmed order, the angles are specified as follows with reference to the machine coordinate system:

 WX - Rotation around the X axis  WY - Rotation around the Y axis  WZ - Rotation around the Z axis

The defined angles define rotations in the stationary machine coordinate system. The order is therefore not to be specified. An angle defined with WX rotates the coordinate system around the not-turned X axis of the machine system, no matter if other rotations already apply.

 WX - Rotation around the existing X axis  WY - Rotation around the existing Y axis  WZ - Rotation around the existing Z axis

The parameter R can be used to control whether the defined rotation shall take place with reference to the stationary machine axes or shall be rotated relative to the current, already turned system. If R is not specified, R0 is applied. R can be used with all angle variants of H.

new rotation is relative to the current coordinate system

new rotation applies in reference to the machine coordinate system

WX, WY, WZ

These parameters contain the angles to be set. Parameter H controls how to determine these angles to reach the new position.

I, J, K

Order of the rotations with H1 where the following applies:

 I is the position of the rotation WX around the X axis  J is the position of the rotation WY around the Y axis  K is the position of the rotation WZ around the Z axis

If no order is specified, the following applies: I1 J2 K3. If an order is specified for the rotation, all the defined angles must be programmed with an information regarding the order. For H0 and H2 it is not necessary to specify an order.

Page 23

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G26 not belongs to the group of commands for change of plane.

It can be combined with G17, G18 and G19.

Pocket milling on non-parallel planes, kinematics swivel head/rotary table

 cuboid workpiece with pocket geometry on inclined plane  point X70 Y30 Z50 is the marginal point of the new machining plane  the pocket has the sizes 35x20x25 [mm]  blue coordinate system is created by movement with G92  G26 rotates and swivels the system into the new position, the yellow coordinate system and the

searched machining plane (dark-gray) is created

... ; Tool selection, technological data G53 ; delete all zero offsets G56 ; Workpiece zero with coordinate system parallel to ; the machine coordinates system (light-green) G92 X70 Y30 Z50 ; Zero offset to the workpiece (blue) G26 H1 WZ=-45 WY=30 K1 J2 ; rotation of the system first around the Z axis ; (WZ=-45 K1), then swiveling of the system ; around the new Y axis (WY=30 J2) - the new ; programming coordinate system (yellow) ; is created ;G26 WZ=-45 WY=30 ; same command by using Euler resp. solid angles, ; easy application, here as a comment G25 H1 ; activate RTCP G0 C45 B30 ; swivel G87,1 B2 Z25 K5 X35 Y20 R4 J1 I40 D0 E250 ; Cycle definition in standard coordinates G79 X15 Y0 Z0 ; Executive instruction G26 ; Cancelation of the plane definition, G56 and G92 ; is active again G53 ; Cancelation of the absolute and relative ; zero offset G56 ; Activation of the workpiece zero ... ;

Example of order G26 H1 WZ=-45 WY=30 K1 J2 Example of Euler G26 WX=-45 WY=30 Example of cancelation G26

Page 24

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G27 Tool zero point

Property

modal

Topic

Transformation command

Position

---

Syntax

G27 <Parameter list>

The command is used to define a movement and rotation of the tool system. It causes a movement of the leading point of the control to the specified point. G27 does not cause any movement, but it causes a jump in the display of the control position when activated. After the specification, the changed tool system becomes active immediately.

Parameter

Description

X, Y, Z, C

These parameters contain the movements to be defined.

G27 is usually programmed after a tool or spindle change if this change have an effect on the leading position of the control. The new programming of G27 cancels all previously valid values, i.e.:

 all previously valid parameters are deleted, set to 0.0,  the axes that have actually been programmed are transferred to the new offset/rotation,  cascaded information on the offsets are not possible.

All movements of the rotary axes are compensated by the control when G27 is active, as if the rotation is executed in the tool zero point. This ensures that all relevant compensation movements are calculated and moved in the interpolation cycle from the changed positions of the C axis. Therefore, the RTCP function is automatically activated at the same time as the tool zero point. The deactivation of RTCP also occurs automatically with the cancellation of G27. Therefore it is not necessary to program G25 within G27.

G27 is activated/deactivated either in the NC program or in MDI.

Movement

The offset to be specified consists of components X, Y and Z and is specified from the new tool zero point. The reference system is the tool coordinate system parallel to the machine coordinate system with the origin around the center of the tool holder.

Rotation

In addition to moving the tool zero point, the parameter C can also be used to specify a rotated clamping of the tool. The angle also refers here to the position of the tool clamping system in relation to the new system. The tool in Fig. 2 is rotated by 30° in the clamping. The angle is specified in cycle G27 as parameter C.

G27 X-25 Y-10 Z50 C-30

Page 25

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Status

The status of the tool zero compensation is displayed in the panel. If cycle G27 has been activated in MDI or AUTOMATIC, the corresponding symbol is displayed.

G27 was activated for an electrode offset, at the same time RTCP was switched on.

Kinematics

Activation of the dynamic TCP routing requires the correct specification of the machine kinematics in the MotionCenter. Using the example of an eroding system with C-axis in the tool holder, the following entry would be necessary:

Parameter

Description

Wert

E-0-0700

Kinematics model of the machine

Illustr.: Machine configuration in the MotionCenter, setting Kinematics model of the machine

Page 26

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G30 Spline interface (online spline)

Property

modal

Topic

Traverse command

Position

---

Syntax

G30 <Axis information> or <Spline head data>

{ pos, pos, [pos, ...,] ric, ric, [ric,...,] weg [,Fwert] pos, pos, [pos, ...,] ric, ric, [ric,...,] weg [,Fwert] ... pos, pos, [pos, ...,] ric, ric, [ric,...,] weg [,Fwert] }

To make the analysis of the created NC set with spline efficient and fast, the spline data are reduced to an introductory path condition G30 with spline head data and a block matrix. The converter recognizes from this the start situation (cf. path starting point up to now) and treats this accordingly. First spline arch point is implicitly the position which has been reached until then. Start direction in the first spline arch point is the direction vector arising due to the Euclid distance calculation. I.e. the direction vector between the current position and the first entry of the spline arch points. This needs to be taken into account in the calculation of the first arch length (resulting path) in the start interval within the program to be created (e.g. Mastercam). Within the spline head data it is possible to also optionally declare the direction of start at the starting point of the spline.

The following parameters are used for definition:

Axis information

Possible axis information: A B C X Y Z The axis information defines the axis allocations and the order of the subsequently expected positions and directions. At least two must be and a maximum of 6 axis indications can be available.

Spline head data

Axis identifiers of the axes involved (A, X, Z, Y, B, C, U, V) in control sequence with optional start direction [ric]. Between the axis information and/or the start direction components there is no delimiter (space or comma) necessary. If start direction components are used, the NC converter expects a directional component for every axis identifier. The directional components are not necessarily standardized.

pos

Position of an axis

ric

Direction part (directional component) of an axis, not necessarily standardized

path

Approximated curve length in mm (convention: In the calculation of the curve or arch length, mm is set to be the same as degrees and either all axes should/have to be involved or a 'fictive path' that contains the speed profile should/have to be indicated.)

Fvalue

Optional indication of speed in mm/min related to the resulting path in the interval.

A X Z Y ; axis identifier without direction of start component (axis information) A0.7 X1.0 Z0.33 Y0.1 C0.0 ; axis identifier with direction of start component (spline head data)

Page 27

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G40 Deletion of the milling cutter radius correction

Property

modal

Topic

Tool command

Position

DEF

Syntax

G40

Entering G40 will switch of all active milling cutter radius corrections (G41 - G44).

G41 Milling cutter radius correction left

Property

modal

Topic

Tool command

Position

--- Syntax

G41

The contour of a workpiece can only be machined if the radius of the tool used is taken into account. Only the coordinates of the workpiece contour are programmed. The control will calculate the tool path on the basis of the saved tool parameters. With G41, the milling cutter radius correction takes place on the left from the workpiece. The viewing direction is the direction of travel of the tool.

 After selecting the milling cutter correction (G41/G42), a G00 or G01 must be programmed in

the same or in the following block.

 A change in the direction of compensation is only possible via G40.  It is not allowed the change the current plane of compensation (G17-G19). Before selecting a

different plane, you have to deselect the milling cutter radius correction.

 During compensation, no zero offset (G54-G59) may be programmed. The active zero offset may

not be changed when the milling cutter radius correction has been selected.

Page 28

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G42 Milling cutter radius correction right

Property

modal

Topic

Tool command

Position

---

Syntax

G42

The milling cutter radius correction takes place on the right from the workpiece. The viewing direction is the direction of travel of the tool.

 After selecting the milling cutter correction (G41/G42), a G00 or G01 must be programmed in

the same or in the following block.

 A change in the direction of compensation is only possible via G40.  It is not allowed the change the current plane of compensation (G17-G19). Before selecting a

different plane, you have to deselect the milling cutter radius correction.

 During compensation, no zero offset (G54-G59) may be programmed. The active zero offset may

not be changed when the milling cutter radius correction has been selected.

Page 29

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G43 Milling cutter radius correction up to

Property

modal

Topic

Tool command

Position

---

Syntax

G43

With G43 active, the tool path is corrected up to the contour. When an interpolation movement is carried out within the current plane, at the end of movement, the tool center in each axis is offset by the radius before the programmed end point. The function G43 is mainly used for "approaching" the contour to be compensated.

With G43 active, only blocks containing linear movements (G00/G01) may be programmed. Circles or circle arcs (G02/G03) are not allowed.

G0X-10Y10 ;Approach pre-position Z0 ;Approach pre-position G1F2000 G43 ;Enable G43 G42 ;Enable milling cutter radius correction G01 Y20 ;Contour X50 ;Contour Y-10 ;Contour G40 ;Disable milling cutter radius correction

Page 30

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G44 Milling cutter radius correction via

Property

modal

Topic

Tool command

Position

---

Syntax

G44

With G44 active, the tool path is corrected via the contour. When an interpolation movement is carried out within the current plane, at the end of movement, the tool center in each axis is offset by the radius behind the programmed end point. The function G44 is mainly used for "approaching" the contour to be compensated. The path condition can be canceled by the functions G40, G41 and G42.

With G44 active, only blocks containing linear movements (G00/G01) may be programmed. Circles or circle arcs (G02/G03) are not allowed.

G0X-10Y30 ;Approach pre-position Z0 ;Approach pre-position G1F2000 G44 ;Enable G44 G42 ;Enable milling cutter radius correction G01 Y20 ;Contour X50 ;Contour Y-10 ;Contour G40 ;Disable milling cutter radius correction

Page 31

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Zero offsets and coordinate rotation

The zero offset makes it possible to move the program or workpiece zero to any desired position within the control range. After a zero point offset, all programmed positions are referred to this new point. The following zero offsets are available:

 SETPOS function in the user interface  RCS1 clamping position correction based on PRESET  Preset function G50 - G52  Programmable absolute zero offset G93  Saved zero point offset G54-G59  RCS2 clamping position correction based on zero offsets  Programmable relative zero offset G92  Programmed rotation with G92 W or G26

Illustration: Zero offset and coordinate rotation

Page 32

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G53 Deletion of the zero offset

Property

modal

Topic

Setup command

Position

DEF

Syntax

G53

G53 will switch off all zero offsets (G54 – G59 P0-P99, G92, G93).

Page 33

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G70 Units of measurement inch

Property

modal

Topic

Setup command

Position

---

Syntax

G70

The measures given are in inch. At the end of the program, the home position is always restored. In the home position, the default is always G71 (mm).

G71 Units of measurement mm

Property

modal

Topic

Setup command

Position

DEF

Syntax

G71

The measures given are in mm.

G72 Deletion of mirror image machining and scaling

Property

modal

Topic

Setup command

Position

DEF

Syntax

G72

A mirror image machining and / or a scaling of the coordinates system is canceled.

Page 34

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G73 Mirror image machining

Property

modal

Topic

Setup command

Position

---

Syntax

G73 Axis designator [-1][+1]

The sign of the programmed dimensional value of an axis can be inverted by mirror image machining. For example, a sign inversion of the X axis is a mirror imaging on the Y axis, if machining takes place in the XY plane. Mirror image machining does not involve a reflection of zero point offsets. During mirror imaging on one axis only, the control will interchange:

 the sign of the coordinates of the mirror imaged axis,  the direction of rotation during circular interpolation (G02/G03),  the machining direction during the milling cutter radius correction (G41/G42).

Mirror imaging is cancelled:

 by the path condition G72, which will cancel the inversion of all axes (reflection is deleted).  by a G73 block, the address of the axis and the value +1. In this case, only the mirror imaging

of the programmed axis is cancelled.

G73 X-1 Y-1 ; The coordinate system is mirror imaged on the X and Y axes

Page 35

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G73 Scaling

Property

modal

Topic

Setup command

Position

---

Syntax

G73 <Parameter list>

The coordinate values of the linear axes of the control can be increased or decreased by a scaling factor. The reference point is the origin of the coordinate system, which will affect in general not only the shape of the workpiece but also its position on the clamping table. The programmed zero offset values will also experience a change in scale. Scaling only refers to the axes of the active plane. The value programmed under "W" is a scaling factor. This means that values greater than 1 will result in an increase in scale and values smaller than 1 in a decrease in scale.

A scaling will be cancelled by:  a block containing G72. In this case, any mirror image machining that may be active will be

cancelled.

 a block containing G73 and W1.0.

G73 W1.5 ; The current plane (XY) is scaled by 50% (increased)

Page 36

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G79 Cycle execution

Property

non-modal

Topic

Cycle command

Position

---

Syntax

G79 <Axis positions>

The function G79 executes a previously defined cycle. When the function is called without any additional parameters, the cycle will start at the position at which the individual axes are positioned. In addition, execution parameters can be specified.

Page 37

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G90 Absolute measure

Property

modal

Topic

Setup command

Position

DEF

Syntax

G90

When an absolute measure is entered, all measures given refer to a fixed zero point. This zero point is always the zero point of the control. The associated numeric value of the path information describes the target position in the coordinate system. The function is effective modally. The traverse distance is calculated from the target coordinates and the current position.

G00 X0 Y0 ; Approach pre-position G41 ; Enable milling cutter radius correction G90 ; Absolute measure programming is switched on G00 X60 Y80 ; The tool is positioned at the starting point A (X60, Y80) in rapid traverse G01 X140 F2000 ; Line interpolation to point B (X140, Y80) Y20 ; Travel to point C (X140, Y20) X60 ; Travel to point D (X60, Y20) Y80 ; Travel to point A (X60, Y80) Y100 ; Moving free G40 ; Disable milling cutter radius correction

Page 38

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G91 Relative measure

Property

modal

Topic

Setup command

Position

---

Syntax

G91 <Parameter list>

When entering a relative measure (incremental measure), the numeric value of the path information corresponds to the traverse distance. The programmed sign determines the direction of travel. It is possible to switch between absolute measure input and relative measure input in the program any number of times.

G00 X0 Y0 ; Approach pre-position G41 ; Enable milling cutter radius correction G91 ; Relative measure programming is switched on G00 X60 Y80 ; ;The tool is positioned at the starting point A (X60, Y80) in rapid traverse G01 X80 F2000 ; X axis by 80 mm in positive direction to point B (140, Y80) Y-60 ; Y axis by 60 mm in negative direction to point C (X140, Y20) X-80 ; X axis by 80 mm in negative direction to point D (X60, Y20) Y60 ; Y axis by 60 mm in positive direction to point A (X60, Y80) Y20 ; Moving free G40 ; Disable milling cutter radius correction

Page 39

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G92 Relative zero point offset coordinate rotation

Property

modal

Topic

Setup command

Position

---

Syntax

G92 <Axis positions> <Rotation>

G92 moves the position of the zero point by the values specified in the current coordinate system. If the path condition G92 is called several times in a parts program, the offset vectors add up. Translatory and rotatory offsets and data on the rotation in the main plane can be programmed.

Parameters

Description

X, Y, Z, …

(all existing axes) new zero point in the machine coordinates

Rotation of the coordinate system on the current plane

The angular position of the programming coordinate system can be changed using G92.

The programmed movements therefore are not carried out in the actually existing axes

but are composed of the movements of several axes where directional changes are

possible as well.

This may also apply to manual mode and MDI depending on the configuration of the

control.

The rotation defined with W is not deactivated when the plane is changed.

Zero offset

G92 X11.3 Y30 ; Coordinate system offset by 11.3 mm (relative)

Coordinate rotation

G92 W-10.5 ; Rotation of the coordinate system by -10.5 degrees (relative)

Description

No movement takes place after specification of G92. But the display of the current control position changes to the position with reference to the new system. The changed coordinate system becomes immediately effective after the specification; the same applies to the possibly specified angle. The programmable rotation is handled like a command for the definition of a free plane (G26). All previous rotations are kept if G92 W.. is specified, thus the current plane is turned further. Relative rotations which are programmed with "G26 .. R1", are also additive, that means the already turned system is turned further. The G26 command offers many more ways to specify rotations and therefore is to be preferred over the specification of G92. G92 is activated in the G-Code program or in MDI. G92 is cancelled by the specification of another absolute zero point offset with G54-G59 and with G93 with another parameter list, by deletion of all offsets with G53, and by programming of a free plane or cancelation of all rotations by G26.

Zero offset

The command is used for programing of an absolute zero offset for all translatory and rotatory axes. The workpiece zero is moved to a certain absolute position in the working area.

Coordinate rotation

Besides the specification of offsets for all axes, also rotations in the active plane can be defined by using parameter W. The center of rotation is the specified or already active zero point. Positive angles of rotations will rotate the programmed path counterclockwise, negative ones clockwise.

Cancelation of the zero offset and rotation

G53, G54-59, G93

Cancelation of the rotation

G26

Page 40

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G93 Absolute zero point offset coordinate rotation

Property

modal

Topic

Setup command

Position

---

Syntax

G93 <Parameter list>

G93 defines the absolute position of the workpiece in the machine system. Translatory and rotatory offsets and data on the clamping position can be programmed. G93 with parameters cancels the programmable zero point offset G54-G59 and any previous G93 offsets. G93 without parameters is ineffective. To delete the programmed offsets and rotations, G53 can be used.

Parameters

Description

X, Y, Z, …

(all existing axes) new zero point in the machine coordinates

Rotation of the coordinate system on the current plane

WX, WY, WZ

These parameters contain the angles to be set. Parameter H controls how to determine these angles to reach the new position.

The rotations are defined by Euler angle or solid angle. The angles are defined as follows:

 WX - Rotation around the current Z axis  WY - turning around the new Y axis  WX - Rotation around the new Z axis

The rotations are always executed in this order, I, J and K must not necessarily be specified. The specification of WX and WY is normally sufficient.

I, J, K

 WX - Rotation around the X axis  WY - Rotation around the Y axis  WZ - Rotation around the Z axis

Order of the rotations with H1 where the following applies:

 I is the position of the rotation WX around the X axis,  J is the position of the rotation WY around the Y axis,  K is the position of the rotation WZ around the Z axis

 WX - Rotation around the existing X axis  WY - Rotation around the existing Y axis  WZ - Rotation around the existing Z axis

The angular position of the programming coordinate system can be changed using G93.

The programmed movements therefore are not carried out in the actually existing axes

but are composed of the movements of several axes where directional changes are

possible as well. This applies also to the manual mode and MDI.

Page 41

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

None of the programmed rotations is deactivated when the plane is changed.

Example of Euler: G93 (X200 Y150 Z50 C30 H0 WY=1.2 WX=3.4) Example of order: G93 (X200 Y150 Z50 C30 H1 WY=1.2 WX=3.4 J2 K1) Example of cancelation: G53 G54-59 again G93

Description

No movement takes place after specification of G93. But the display of the current control position changes to the position with reference to the new system. The changed coordinate system becomes immediately effective after the specification; the same applies to the possibly specified angle.

G93 is activated in the G-Code program or in MDI. G93 is cancelled by specification of another absolute zero point offset with G54-G54, the re-programming of G93 with another parameter list or by deletion of all offsets with G53. The angle programming by WX, WY and WZ is to be preferred over the plane-dependent rotation with parameter W. The rotation of program parts, however, should be realized with G26 or G92.

Zero offset

The command is used for programing of an absolute zero offset for all translatory and rotatory axes. The workpiece zero is moved to a certain absolute position in the working area.

Coordinate rotation

Besides the specification of offsets for all axes, also rotations in the active plane can be defined by using parameter W. The center of rotation is the specified or already active zero point. Following changes of the zero point effect a cancelation of the rotation.

RCS (Rotated Coordinate System) As an alternative to W there is the possibility to compensate the clamping position by specification of the angular deviation which was measured during the setup. It is also called the RCS function. These specifications refer to the clamping position and therefore do not depend on the plane definition or can be changed by them. Switch H is used to define the application of rotation WX, WY and WZ. The order of the individual parameters in the NC record has no effect on the order of the rotations.

Rotations in the system of the zero offsets G93 are called RCS2 (RCS – Rotated Coordinate System).

Page 42

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G94 Speed programming

Property

modal

Topic

Setup command

Position

---

Syntax

G94 <Parameter list>

Depending on whether the dimensions are set by the path conditions G70 or G71, the feed speed is programmed in mm/min (degrees/min) or inch/min (degree/min). The function is automatically switched on when a G-Code program is loaded and is effective modally. G94 can be cancelled by the path condition G95.

Page 43

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G95 Time programming

Property

modal

Topic

Setup command

Position

---

Syntax

G95 <Parameter list>

With the function G95 time programming, the machining time can be determined for a programmed path route. This is worthwhile when axes with different speed behaviors (e.g. linear axis and rotational axis) are involved in a movement. The feed speed using F-word is then no longer programmed (G94) in mm/min (inch/min) as is usual but a code word calculated by the specified time (inverse time programming) needs to be programmed in which this movement is to be processed. From the resulting machining time, the control calculates the required path speed for this, taking into account threshold values path velocity. If no new F-word is programmed in a block with a traverse movement, the F-word of the preceding block is used. The function is modally effective and can be deleted by the path condition G94. With G95 active, only blocks with G01 may be programmed. G00 commands are programmed as with G94 with the 'rapid movement automatic speed'.

Two different INVERSE TIME programming times can be used:

Normal Invers Time

Normal Inverse time programming

Extended Invers Time

Extended inverse time programming. EIT must allow be used when during the calculation of the code word via NIT a value less than '1' results (see example). All handovers from the G&M code can be handed over in float format. Normally, however, the integer format is used.

Procedure with EIT programming:

If the ratio feed/path is smaller than 1, calculate the E-value (Increase multiplication factor in 10 increments until the ratio is greater 1. The E-value is set to 10000 as a standard feature). Then determine the relevant F-value with the E-value determined in this way. EIT is always programmed with a negative preceding sign (*-1024).

The following address letters are used for definition:

N The N-value is optional and denotes the multiplication factor for NT. If the N-value is not programmed, the multiplication factor is set to 1.0.

E The E-value is optional and denotes the multiplication factor for EIT. If the E-value is not programmed, the multiplication factor is set to 10000.0.

T1 M6 S2000 M3 G00 Z10 G95 E1 ; Switch on EIT (multiplication factor = 1) G01 Z-11.999 A19 C0 F-204800 X70.003 Y-3.547 A19 C0 F-2165142 X69.85 Y-2.689 A19 C0 F-2186417 X69.551 Y-1.871 A19 C0 F-2186756 X69.114 Y-1.117 A19 C0 F-2185486 X68.553 Y-0.45 A19 C0 F-2185632

Page 44

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G107 Eroding: Define the directional vector for the lift-off movement

Property

modal

Topic

Eroding command

Position

---

Syntax

G107 < Parameter list >

The command G107 can be used to define a direction vector for the lift-off movement during eroding.

NOTE: Please note that any defined transformations (e.g. G26) must be taken into consideration.

Definition for the call in the G&M code:

Axis

Description

X, Y, Z, … U, W, V; A0=, A1=, … A15=

Standardized parts of the CNC axes for the lift-off movement with a vector. The lift-off path is defined with G1001 Bxx..

G107 X0 Y0 Z1

Page 45

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G181 Probe calibration

Property

non-modal

Topic

Cycle command

Position

---

Syntax

G181 < Parameter list >

Emptying of the content of log files:

Emptying of the file 'andronin.log'. The content of the specified log file, but not the file itself, is deleted. Other meanings of the address D.

Emptying of the mprot.log (ASCII)

Page 46

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G190 Absolute circle center

Property

modal

Topic

Setup command

Position

DEF

Syntax

G190 <Parameter list>

The dimensions for the circle center can be given either in absolute or incremental coordinates. One of the two functions is set automatically via the system configuration. G190 and G191 are active only when G90 is also active. If G91 is active, the circle center is relative anyway, and the status of G190/G191 becomes meaningless. If G190 is active, the circle center will be entered in absolute coordinates. This means that programming is done analogously to straight line interpolation from the zero point of the control.

G90 G00 X-15 Y60 Z10 G41 G01 X0 Y50 G01 X50 G190 G02 X80 Y20 I50 J20 G01 Y-10 G40

Page 47

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G191 Relative circle center

Property

modal

Topic

Setup command

Position

---

Syntax

G191 <Parameter list>

If G191 is active, the circle center can be programmed as the distance from the starting point of the circle.

G90 G00 X-15 Y60 Z10 G41 G01 X0 Y50 G01 X50 G191 G02 X80 Y20 I0 J-30 G01 y-20 G40

Page 48

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G288 Set Look Ahead parameters

When programming "G70 - Dimensions in inch", all lengths given in µm

are evaluated in 1/10000 inch.

G288,0 Look Ahead basic parameter

Property

modal

Topic

Setup command

Position

--- Syntax

G288 <Parameter list> or G288,0 <Parameter list

This command allows the Look Ahead parameters to be changed from the G&M code. However, the Look Ahead parameter cannot exceed the limit values in the in the MotionCenter. In the “General cycle presetings G288“, 6 Look Ahead types can be determined which can then be called up using G288 Lx. In addition, it is possible to change individual parameters. A parameter that has the value -1 resets it to EEPROM values. A detailed description you can find in the Look Ahead documentation.

The following address letters are used for definition:

R Feed rate [mm/min]

D Rapid traverse speed [mm/min]

E Quality of input data [μm]

H Contour precision [μm]

K Smoothing of contour [ms]

N Max. acceleration [m/s2]

O Jerk limit acceleration [m/s3]

X Jerk limit X-axis [m/s3]

Y Jerk limit Y-axis [m/s3]

Z Jerk limit Z-axis [m/s3]

A Jerk limit A-axis [m/s3]

B Jerk limit B-axis [m/s3]

C Jerk limit C-axis [m/s3]

Page 49

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G488 Simple measurement block

Property

non-modal

Topic

Cycle command

Position

---

Syntax

G488 <Parameter list>

The cycle G488 Simple measurement block is used for determining the switching point of a selected control axis (axis numbers 0 to 15) in a selected plane (G17/G18/G19) or the axis combination X Y Z. The NC cycle is not executed until a "touch probe" tool type (tool management) that has been clamped in the spindle is detected as active tool.

The following address letters are used for definition:

Axis number used for carrying out the measurement. Single-axis 0-15, two-axis 17-19, multi-axis 900+Axis code. (Example Z axis - A2, XY plane - A17, X-Y and Z axis - A914 only)

X Search path. Specifies the relative axis movements of the axis or axes selected by means of the address [A] If an axis is to carry out no movement at all, a relative path of 0 must be entered.

Y see X

Z see X

B Positioning feed

E Measuring feed

I Repeat measurements. Specifies the repeat measurements. Each measurement is carried out again from the start position.

K Shaft probing method. Calculation method for determining the measurement result.

C Activate Point log C0 - Protocol output disabled (Default) C1 - Protocol version 1 C2 - Protocol version 2

R Starting position. After completion or interruption of the measurement, a retraction to the starting position will take place. R1 - moved back to starting position R2 - moved back to measuring position

Page 50

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G488 A1 X30 Y0 Z-30 B1000 E300 I5 K0 C0 R1 G79

To determine the axis code word, the program WINAKW.exe in the directory 'C:/andron/Tools' can be used or the following table in which the example is shown for the axes X, Y and Z.

Axis

DEZ

HEX Axis

DEZ

HEX A 1 1 X´

256

100

X 2 2 Y´

512

200 Z 4 4 P

1024

400

Y 8 8 Q

2048

800 B

10 R

4096

1000

20 U

8192

2000 D

40 V

16384

4000

128

80 W

32768

8000

The binary value produces 14 decimally (axis code word of the axes X, Y and Z)

Page 51

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Procedure

Movement

Feed

1. Probe 1st corner 

Measuring feed

2. Move free 1st corner 

50 mm/min

3. Probe 1st corner  (measurement result)

10 mm/min

4. Move free 1st corner 

50 mm/min

5. If desired: Positioning to the start position / position measurement result

Positioning feed

Measurement log 1

Axis number with which the measurement was carried out, result of the measurement depending on the input surface or ball center (for the axis with the axis number or depending on the level of the Xaxis), result of the measurement depending on the input surface or ball center (for the Y-axis), result of the measurement depending on input surface or ball center (for the Z-axis), starting position (for the axis with the axis number of depending on the level of the X-axis), starting position (for the Yaxis), starting position (for the Z-axis). Maximum measurement value (for the axis with the axis number or depending on the level of the Xaxis), maximum measurement value (for the Y-axis), maximum measurement (for the Z-axis), minimal measurement value (for the axis with the axis number or depending on the level of the Xaxis), minimum measurement value (for the Y-axis), minimal measurement value (for the Z-axis), minimal measurement value leap (for the axis with the axis number or depending on the level of the X-axis), maximum measurement value leap (for the Y-axis), maximum measurement value leap (for the Z-axis), number of repetitions, measurement number, notification method, tool diameter from the tool administration. Tool length from the tool administration, tool number, calculate radius, point protocol activated, calculate probe transformations from G181, move back to start position / measurement position

Measurement log 2

X probe position depending on input surface or ball center, Y probe position depending on input surface or ball center, Z probe position depending on input surface or ball center, tool diameter from the tool management, tool length from the tool management, tool number, calculate radius? 1 = YES, calculate measuring probe transformations from G181? 1=YES, move back to start position? 1=YES

Saving the measuring log

The measurement log is saved as standard under: %andronroot%\SystemData\Repository\Local Control\Measuring Protocol

The storage location or storage path can be changed via G23.

Page 52

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Communication variables for FlexProg

Cycle

Description

Variable

Meaning

G488

Simple measurement block

IKV [2000]

Cycle number

IKV [2001]

Extended cycle number

IKV [2002]

Tool number

IKV [2003]

Axis number used for carrying out the measurement

IKV [2004]

Number of repeats

IKV [2005]

Averaging method

IKV [2006]

Radius calculation

IKV [2007]

Point log activated

IKV [2008]

Calculate touch probe transformations from G181

IKV [2009]

Retract to the start position / measuring position

FKV [2000]

Measurement result depending on the input for surface or sphere center (for the axis carrying the axis number or depending on the plane of the X-axis)

FKV [2001]

Measurement result depending on the input for surface or sphere center (for the Y-axis)

FKV [2002]

Measurement result depending on the input for surface or sphere center (for the Z-axis)

FKV [2003]

Start position( for the axis carrying the axis number or depending on the plane of the X-axis)

FKV [2004]

Start position (for the Y-axis)

FKV [2005]

Start position (for the Z-axis)

FKV [2006]

Maximum measured value (for the axis carrying the axis number or depending on the plane of the X-axis)

FKV [2007]

Maximum measured value(for the Y-axis)

FKV [2008]

Maximum measured value(for the Z-axis)

FKV [2009]

Minimum measured value (for the axis carrying the axis number or depending on the plane of the X-axis)

FKV [2010]

Minimum measured value (for the Y-axis)

FKV [2011]

Minimum measured value (for the Z-axis)

FKV [2012]

Maximum measured value jump (for the axis carrying the axis number or depending on the plane of the Xaxis)

FKV [2013]

Maximum measured value jump (for the Y-axis)

FKV [2014]

Maximum measured value jump (for the Z-axis)

FKV [2015]

Tool diameter from the TM

FKV [2016]

Tool length from the TM

Page 53

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G488,1 Simple measurement block

Property

non-modal

Topic

Cycle command

Position

---

Syntax

G488,1 <Parameter list>

The measuring cycle G488.1 is a reduction of cycle G488. That means, this cycle does not check whether an erosion control has been selected or a probe has been replaced. In addition, the cycle will stop at the current position after the first measurement, so that the measurement signal is still present. This means, for example, that movement to starting position (R2) is not possible. Also several measurements simultaneously (e.g. I2) are not possible. The program is closed with a corresponding error message. Apart from these restrictions, the meaning of the parameters remains identical to cycle G488.

In addition, there is the parameter J.

J Level of the measuring signal J0 – The measuring signal is „low-active“, that means with a falling edge of the signal is being measured. J1 – The measuring signal is „high-active“, that means with a rising edge of the signal is being measured.

Page 54

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G581 Continuous operation cycle rotation

Property

non-modal

Topic

Cycle command

Position

---

Syntax

G581 <Parameter list>

Cycle G581 is used for the continuous rotation of the rotary axes at a defined speed. Other axis travels (e.g. in the X, Y and Z axis directions) can be programmed independently of this rotary motion. The continuous operation is stopped automatically at the end of the program. The command will not be executed during block search. A continuous operation axis started by the command G581 may not participate in any other motion for the duration of the continuous operation. The rotary speed cannot be affected by the feed potentiometer.

The following address letters are used for definition:

A Axis selection. This input selects (1) or deselects (0) the corresponding axis.

B see A

C see A

N Speed of the selected axis in revolutions/minute. The sign determines the direction of rotation of the axis.

G581 A1 B0 C1 N30

Page 55

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G781,1 Spindle offset

Property

modal

Topic

NC command

Position

---

Syntax:

G781,1 N<Spindle number> X<Offset in X> Y<Offset in Y> Z<Offset in Z>

Syntax:

G781,1 N<Offset number> X<Offset in X> Y<Offset in Y> Z<Offset in Z> A<Offset in A> B<Offset in B> C<Offset in C> G781,1 N<Offset number> K<Axis code> G781,1 I<IKV index>

The spindle offset is used for offset definition of the tool system. It offsets the guiding point of the control system by the vector specified. G781,1 causes no movement, but results in case of activation in a jump in the position indication of the control system. After specifying, the new guiding point is immediately active.

G781,1 is usually programmed after replacement of a spindle when this replacement has to influence the guiding position of the control system. The offsets remain effective after switching off. During switch on, spindle offset is activated with referencing. Cascaded specifications for the offsets are not possible. The offset is always specified absolutely. To check the active spindle offsets, the number can be read out and verified in FlexProg.

Address

Command

Applicabl e range

Offset number: The parameter N is used to establish the offset number. N is an obligatory parameter. N-1 deletes the offset that was valid before. N0 to N254 are valid offset numbers.

-1 to 254

X, Y, Z A, B, C

Offset: XYZABC are used to specify the offset of the guiding point. The vector applies from the guiding point of the main spindle without offset to the guiding point of the loaded spindle. Each offset, including that of individual axes, will NOT delete an offset that has been valid up to now. Individual offsets can be deleted by specifying offset ZERO. All offsets will be deleted by entering N-1.

K Alternatively to entering the axis addresses XYZABC directly, the offset can also be entered via a list of FKV and a decimal axis code. First, all required values must be assigned FKV[axis number] = offset for axis and then G781,1 N<offset number> K<axis code> must be called up. (For determining the axis code, see: General information - axis code)

0 - 65535

I IKV index in NC program for returning the active spindle offset number. The parameter I can be used individually or together with N, X, Y or Z. (Example: 21 for IKV[21])

0 - 1000

Activation:

G781,1 is activated/deactivated in the NC program or in MDI.

The offset applies then in all operating modes and is maintained after switch off.

Display:

The current status of the spindle offset in displayed in the status area of the

position menu.

G781,1 N0 X10

G781,1 N0 X10 Y20 Z20

G781,1 I25

;Offset tool system for offset number 0 in X by 10mm, previously

applicable offsets in Y und Z will be deleted.

;Offset tool system for spindle 0 in X, Y and Z

;Write number of active spindle offset to IKV[25]

Page 56

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G783,0 Read/Write zero points

Property

modal

Topic

Special command

Position

---

Syntax

Write to the zero offset table:

G783,0 <Parameter list>

G783,0 can be used for:

 activating zero points

 reading data from the currently active zero offset table and using them in the NC program or

 writing NC program data in the zero offset table.

The following address letters are used for definition:

O Number of the desired zero point.

N Page of the zero offset table. If N is not used, the first page applies.

D Action:

0 - activate zero point

5 - write

9 - read

X, Y, Z,

A, B, C

Write action:

The transmitted value is entered to the zero point of the relevant axis.

Read action:

Enter value "zero"! (The value is not evaluated, only the address is used.)

Axis number: To read and write further axes, as an alternative to the direct axis address

(X,Y,Z,A,B,C), the andronic axis number can be used.

Address of the parameter:

To be able to write the value to the zero offset table, the value for further axis or

parameters must have been transmitted to a separate parameter “L<Value of the

axis/parameter>”.

L Transmitting the zero point to the zero offset table.

This parameter is only used when writing to the zero offset table and using the parameter

“K<axis number of the universal axis>”

R Specification of the index of the target variable to which the zero point is to be written.

Allowed range FKV[2000] - FKV[2199] This parameter is only used when reading from the

zero offset table!!

When programming “G70 – Dimensions in inch” all linear mm dimensions are

evaluated as inch values.

Axis

K Axis K

Axis

A 0

X´ 8

ANG

16 X 1

Y´ 9

RCS

Z 2 P 10 WX

18 Y 3 Q 11 WY

B 4 R 12 WZ

20 C 5 U 13 H

D 6 V 14

E 7 W 15

G783 D0 O55 N2

G783 D5 O54 N2 X3.55

G783 D5 O54 N2 K1 L3.55

G783 D9 O54 N2 X0 R2009

G783 D9 O54 N2 K1 R2009

;corresponds to G55 P2, but may be used variable in FlexProg

;Zero offset table write G54 P2 X-axis = 3.55

;like example 1 only programmed as universal axis

;read G54 P2 zero offset table X-value and write in FKV [2009]

;like example 3 only programmed as universal axis

Page 57

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G1000 Eroding: Velocity

Property

modal

Topic

Eroding command

Position

---

Syntax

G1000 <Parameter list>

The command G1000 can be used to define different eroding velocities.

The following address letters are used for definition:

Word

Description

Unit

A Approach velocity

mm/min

B Lift-off velocity

mm/min

E Eroding velocity

mm/min

G1000 E60 B18000 A18000

Page 58

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G1001 Eroding: Directions

Property

modal

Topic

Eroding command

Position

---

Syntax

G1001 <Parameter list>

The command G1001 can be used to define different eroding directions.

The following address letters are used for definition:

Word

Description

Unit

A Start up path Path at the start of the interval which is driven with reduced acceleration

B Interval path: Maximal path for returning during an interval – otherwise first returning point

C Short interval path: Path for returning during short interval path

I Approach path: Path of approaching erosion contour after an interval or interruption which isn’t moved with feed or rapid motion but eroding Length of the 3rd step during an interval needed for stop of feed rate.

J Path for returning within contour: During moving backwards according to erosion generator the erosion contour is left in the direction to the last returning point when the length of the path for returning within contour is made within the erosion contour (measured according to the already achieved erosion progress). If this path is equal to zero, than a movement to the last returning point is

made immediately. Is this parameter very large a whole returning within the erosion contour is possibly done.

Eroding Flushing Eroding

G1001 A0.000 B10.000 C1.000 I0.000 J0.000

Page 59

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G1002 Eroding: Factors and modes

Property

modal

Topic

Eroding command

Position

---

Syntax

G1002 <Parameter list>

The command G1002 can be used to define different eroding factors and modes.

The following address letters are used for definition:

Word

Description

A Factor start-up acceleration

E Factor speed eroding forward

H Factor speed eroding backward

K Factor speed of the radius change orbital movement forward, direction erosion front

L Factor speed of the radius change orbital movement backwards, direction circle center

I Factor (returning point) RZP eroding forward (move to erosion contour)

J Factor RZP eroding backward (leave path)

B Mode of interval

0: no interval

1: Time controlled („cyclic“)

2: Generator controlled („adaptive“)

3: Generator and time controlled (both)

C Command:

0: Switch of High-Speed-Jump

1: Switch on High-Speed-Jump, mode 1

D Additional factor for erosion velocity

>= 1.0

Application: If only forward signals are present during erosion for a given wait time (see

G1003), than the velocity for moving is increased by this factor until forward signals are

constantly present.

N Additional factor for for the speed of an orbital movement (see also G1004 Exxx).

∆f =

∙

min

∆b =

∙

min

Factor speed eroding forward

resp. factor RZP eroding forward

Factor speed eroding forward

resp. factor RZP eroding backward

Eroding reference speed

min:

Cycle time

G1002 A1.000 B3 C1 E0.350 H0.650 K0.700 L1.300 I0.350 J0.650 D5.000 N1.200

Page 60

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G1003 Eroding: Time data

Property

modal

Topic

Eroding command

Position

---

Syntax

G1003 <Parameter list>

The command G1003 can be used to define different eroding time datas.

The following address letters are used for definition:

Word

Description

Unit

A Number of reverse signals for a short lift-off Usage: If the controller detects this number of reverse signals in sequence during eroding, a short lift-off is started.

B Cycle of interval Time between two intervals

sec

D Wait time, until the additional factor for the erosion velocity is applied Application: If only forward signals are present during erosion for a given wait time (see G1003), than the velocity for moving is increased by this factor until forward signals are constantly present.

sec

E Delay, until the use of the additional factor for the speed of orbital movement. Usage: If there is only one forward signal during an orbital movement during this delay, the orbital movement is then accelerated by the additional factor as long as the forward signal remains constant.

G1003 A50 B0.400 D1.500 E0.500

Page 61

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

G1004 Eroding: Orbital movement in the selected plane

Property

modal

Topic

Eroding command

Position

---

Syntax

G1004 <Parameter list>

The G1004 command can be used to start or stop an orbital movement in the selected plane. The

parameters listed below are used to define orbital movement.

The following address letters are used for definition:

Word

Description

Unit

K Command: Orbital movement

0: Switch off the orbital movement

1: Switch on the circular orbital movement

2: Switch on the circular orbital movement with a controlled radius

3: Switch on the conical orbital movement

R Radius (required if K word ≠ 0)

E Velocity (required if K word ≠ 0)

ms/rotation

H Height of the cone (required if K word = 3)

G1004 K1 R0.005 E1000

Page 62

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Parameter programming

These parameters allow the calculation with variables within the G-Code program, the formulation of

the conditions for executing program parts and the use of program branches and loops. G-Code

program s containing parameter instructions must contain the code "#Para" at the beginning of the

file.

Syntax

Qn = [-]Expression1

Qn = [-]Expression1 Operator Expression2

n = Index of the Q parameter [0 ..... 255]

Operators = +, -, *, /

Q1 = [-]Numeric value

Q1 = [-]Q2

Q1 = Q2 + Q3

Q1 = 10 * Q3

The Q parameters can be used in combination with all valid NC addresses. Valid addresses are the

axis designators, feed and spindle addresses. (G01 X=Q22 F=Q3 S=Q1 M3).

In order to be able to branch/jump in different places, jump marks can be introduced. Jump marks

(max. 256) are in square brackets.

[Mark1]

[Feed]

The jumps to these marks can be realized via GOTO or IF ... GOTO. GOTO jumps directly to the

specified jump mark. With IF ... GOTO is only branched to the jump mark if the condition behind IF

applies. (Comparison operator)

GOTO feed

IF Q1 > Q2 GOTO feed

Six comparison operators are offered:

Page 63

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Flexible G&M code Programming (FlexProg)

General

A key enhancement of the functionality of the NC language and the parameter programming is the

flexible programming (FlexProg). The use of global and local variables, the free definition of functions

with call-up parameters and return value as well as the use of control structures for the conditional or

repeated execute facilitate the programming of complicated procedures and calculations substantially.

This is supplemented by the option of the formulation of complex mathematical expressions with

several bracket levels and the well-known simple use of the results in the G-Code program. All these

elements are also part of higher programming languages, for instance 'C/ C++“, a programming

language often used in technical and mathematical applications. In addition, the available data types

and parameter records offer the option of using G-Code program s with analog-C programs

cooperatively.

Primarily the rules of parameter programming apply. In contrast to pure parameter programming,

substantially more functionality is available to the user of FlexProg with less effort for ancillary times,

such as e.g. the necessary implementation time. With the options of programming, the responsibility

of the programmers also increases. The effectiveness of a program thus depends substantially on the

selected program structure. As a basic principle, more comprehensive calculations should not be used

in traverse commands so as to avoid loss of speed in contours.

All calculations are implemented during the duration of the program and of course require computing

time. FlexProg is particularly well suited for workpieces that only differ from one another slightly or

with which the processing steps result during the duration. FlexProg thus offers the option of

parameterizing and implementing the processing similar to cycles. To be able to use a G-Code

program with FlexProg functionality, the activation of the calculation modules of the control is

necessary. This is done by the code '#PARA_EXPR' at the beginning of the program.

Page 64

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Restrictions

 Despite great similarity of the language with the programming language 'C', it applies that the

instructions are processed line by line.

 If more than one calculation expressions are used in one line, at least one space must be after

each expression, otherwise a correct assessment of the individual expressions is not possible.

 In expressions, round brackets '(...)' can be used for structuring. These can also be used in

nested form.

 With FlexProg programs, macros are treated as functions without return value. The initialization

run during implementation, as still necessary with '#PARA', is therefore no longer necessary.

 There are differences in the use of point definitions (G78). These are also parametrizable in

FlexProg programs with calculation specifications and thus can be use considerably more flexible.

 The Time programming with G95 is not available.

 Spline contours with G30 are not permissible within FlexProg programs. Splines with G31 to G35

are permitted.

 Pure calculation instructions may not stand in one line with instructions to NC addresses. Care

should be taken to ensure a clear division per block of calculations and NC instructions. Only with the allocation of values or calculation specifications to NC addresses, are deviations from this rule permissible.

 The control of syntax and semantics of the programs is greatly restricted through the options of

conditional and unconditional jumps. Some errors are only recognizable during the runtime.

 For FlexProg programs, particular comment rules apply.

 The automatic supplementing of missing parameters in the circular programming with G02/G03

is not possible within FlexProg programs. The circular parameters are to be indicated in their entirety, i.e. end point and center point or end point and circle radius.

 Bracketing

{ may stand at the beginning of the first line of an instruction block. } must stand in a separate line.

General program

structure

A FlexProg program consists of a program core and a number of functions and/or macros that are all

in one file. The program core does not require any explicit marking and also does not have any call-

up parameters. If variables are agreed in the program core, these are valid in the entire program, i.e.

also in macros and functions, and of course can also be changed.

- #Para_Expr -> Program code

- Declaration of the functions

- Definition of the global variables

- Definition of macros

- Program core

- Definition of the functions

Data types

The data types used in FlexProg are void, Int, Float and Double. They are used both as Handover

values as well as with the return values. The data type void serves as a placeholder (engl. empty,

vacancy, hollow space…).

Type

Byte

Bit

Post comma

Area

Void - - - - Int 4 32

none

4.29 10-8 – 4.29 108

Float 4 32

7 significant

1.18 10

-39

– 3.4 1038

Double

15-16 significant

2.23 10

-308

– 1.79 10

308

Page 65

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Functions (general)

Functions consist of a declaration part and a definition part. Functions always have a type, a

name and a list of call-up parameters that can also be empty. All instructions belonging to a function

must stand in the relevant curly brackets (instruction block).

Function

declaration

So that the Compiler can check the functions used and their call-up, all functions used must be

declared before the definition. It must be announced which result type has the function, which name

it gets and which data types in which order may appear as a parameter list. The declaration of the

functions used must be done at the beginning of the program, i.e. directly behind the code

'PARA_EXPR'. Each function is declared in one line.

Syntax

DECLARE <Data type> <Function name> (<Parameter list>)

The Function name may consist of the reserved words of the language. Letters, numbers and the

underscore '_' can be used in the function name.

The parameter list is the listing of the values to be handed over when the function is called up. The

types Int, Float and Double can be used. If the parameter list is empty, the type VOID can be

entered. Each parameter in the list is to be preceded by the data type.

DECLARE

void

Deliver () ; Function without return, without handover value

DECLARE

void

Rectangle (float Xvalue) ; Function without return, with handover value

DECLARE

float

Calculate X (void) ; Function with return, without handover value

DECLARE

float

Jump (int number) ; Function with return, with handover value

Macros and

Q parameters

Macros are programmed as in the standard G&M code. They act like functions without argument and

without return value. They need to be defined before use.

#MacroName#

G01 X20

G...

Q parameters are always of double data type and have an index of 0....255

Q234 = 123.4567

Page 66

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Function definition

The function definition consists of the function head with the information on the function call and the

instruction block that contains the variable agreements and instructions. Function definitions may not

be nested. In contrast to the declaration, the Key word 'DECLARE' is missing and the parameter list

must contain names for the individual parameters. The first instructions of the instruction block

normally contain the local variables. If a return value is agreed, this must be transferred with the

RETURN command to the calling function.

Syntax

<Data type> <Function name> (<Parameter list>) ->function head

{

..... -> instruction block

}

void rectangle (float Xvalue, float Yvalue) ; function head

{ ; Beginning of instruction block

G91 ; Relative measure

G01 Y=Yvalue ; Move Y to Yvalue

X=Xvalue ; Move X to Xvalue

Y=-Yvalue ; Move Y to negative Yvalue

X=-Xvalue ; Move X to negative Xvalue

G90 ; Absolute dimension

} ; End of instruction block

Variables

Variables are a key extension of the NC syntax. For the named data types, variables and one-

dimensional fields can be defined and used. This is done by indicating the data type and Variable

name. With the exception of a few restrictions that result from the linguistic scope of the G&M code

and the extensions (e.g. while, if, goto, float), this name can be freely selected.

Designators for symbolic variables consist of at least 2 letters at the beginning of the name to

preclude any confusion with NC addresses. The underscore is also permissible there. Numbers and

also be used in the name. It is recommended that the variable type is indicated in the name, for

example 'f_depth' for a FLOAT variable. Variables are not automatically initialized during the

definition, use of capital and lower case is possible, but no differentiation is made. The agreement of

the global variants is always done at the beginning of the G-Code program. Local variables can be

used in functions. The definition is done according to the parameter list in the function definition.

Global variables are available to all program parts for reading and writing access within a G-Code

program. They can therefore also be used in functions, procedures and macros. They need to be

defined at the beginning of the program.

Local variables can only be defined and used in functions. After the function is no access is possible

any more. With the repeated call-up of functions too, the values of the local variables cannot be

restored again.

The variables are declared in the program head as follows:

Syntax

DECLARE <Data type> <Variable name>

If several variables of the same time are used, the declaration is as follows:

Syntax

The Data type can be Int, Float or Double. Variables can also be indexed one-dimensionally.

float Xdelivery

int number

int flag[10]

double X_Pos, Y_Pos, Z_Pos

Page 67

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Communication

variables

These variables permit an exchange of data between G-Code program s and various control

parameters and vice versa. These can be measurement values of the cycles or parameters from the

tool management. The communication variables can be used for all permissible computing operations

and instructions to NC addresses (axes). Calculations are carried out during the runtime of the G-

Code program. Calculations are not permitted in the index, int variables, however, can be used.

IKV [Index]  Integer communication variable

FKV [Index]  Float communication variable

The index must be in [...] and has a range of value from [0...32768] (stands in the EEPROM). The

user should use the index 0....1999 as indices from 2000 among others are used by the measuring

cycles and may overwrite user data.

IKV [10]

FKV [1004]

int Hallo

Hallo = 5

FKV [Hallo]  Int variables can also be used as an index

If the control is converted to globally valid variables (the DWORD 'bGlobalQ' is inserted in

the registration {HKLM\SOFTWARE\andron\NCConverter} and the value >0 is assigned

to it) IKV and FKV variables no longer exist. QI and Q are used in an analogous manner to

them. (QI = IKV and Q = FKV)

Page 68

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Expressions and

operators

Expressions consist of operands and operators. The operands are variables, constants, parameters

or expressions. The assessment of an expression supplies a value that is dependent on the type of

the operators used. The value assignment is an expression. It is the most used form of assignment of

values to variables and parameters. The expression to the right of the assignment operator is

calculated and the value assigned to the variable on the left. A variable is an expression that refers to

an already defined, modifiable memory area, i.e. variables and parameters. The bit operators can only

be applied to integer variables.

(IKV or INT).

Syntax

Variable = Expression

Q125 = 100.876

FKV [2001] = Q100 * sin (Q23)

Residual path = Calculate residual path (value 1, value 2)

The following operators can be used in FlexProg:

Arithmetical operators

Assignment of values

+ Addition

- Subtraction, negative preceding sign

* Multiplication

/ Division

Comparison operators

smaller than

> greater than

equal

smaller than/equal to

greater than/equal to

not equal

Logical operators

Logic OR operation

Logic AND operation

! Logic reversal (NOT)

Bit operators

OR operation of bits

& AND operation of bits

~ Complement (unary)

^ Exclusive OR operation of bits

Bit shift to the right

Bit shift to the left

Mathematical

functions

Function

Description

Function

Description

Function

Description

SIN (X)

Sine angle

ASIN (X)

Sine reversal

SINH (X)

Sine base E

COS (X)

Cosine angle

ACOS (X)

Cosine reversal

COSH (X)

Cosine base E

TAN (X)

Tangent angle

ATAN (X)

Tangent reversal

TANH (X)

Tangent base E

CEIL (X)

Round up

FLOOR (X)

Round down

LOG (X)

Log base E

EXP (X)

Exponent base E

SQRT (X)

Root formation

ATAN2 (X, Y)

Partial arcustan.

LOG10 (X)

Log base 10

POW (X, Y)

X to the power of Y

FABS (X)

Absolute value

Page 69

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Assignment of NC

addresses

Constants, variables, parameters and also expressions can be assigned to the following addresses:

- X, Y, Z, A, B, C, U, V

- I, J, K, R

- F, S, D, E

- W, O, N, H, L

Syntax

NC address = [-] Constant

NC address = [-] Qn

NC address = [-] IKV[n]

NC address = [-] FKV[n]

NC address = expression

G1 X=Center*cos(Q4) Y=Q10*sin(Q4) Z=delivery + IKV [1300]

G1 X=-Q5 Y=FKV [1555] F=Feed1

Comment marks

Comments in round brackets '(...)' are not permitted. These brackets are reserved for the formulation

of expressions. Program comments can be done using the following signs:

; The rest of the line is comment, any place in the block

// The rest of the line is comment, any place in the block

% The rest of the line is comment, only possible at the beginning of the block

/* ... */ Comment marks for beginning and end, comments over more than one lines are

also possible

Point definition

As per G78, points (maximum of 63) can be defined parametrized. The values for the individual axes

can be parametrized and can also be done as a calculation specification. These are calculated anew to

the runtime of the program each time they are called up. If, for instance Q4, as shown below, is

changed after the G78 block, the value determining Y is also changed.

G78 P1 X=IKV[2] Y=Q4+Q3 Z10 ; for P1, calculations are indicated

G0 P1 C90 ; and now the first call-up; in place of P1, the

; calculation specifications are used, internally, the following:

; G0 X=IKV[2] Y=q4+q3 Z10 C90

Q4 = Q4 + Q10 ; Q4 is changed

G0 P1 C90 ; second call-up; P1 is replaced again, the calculations

; executed, the new Q4 is used as a target position

; another value is traversed for Y than with the first call-up

Page 70

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Instructions

Simple instruction

A simple instruction consists of a completed expression. An expression is deemed to be completed

when all round brackets are closed again and behind the last valid part expression there is no

operation sign but rather an empty space, tabulator or the end of the line. An explicit sign for the end

of the expression is thus not necessary.

X_New = X_Old +100

Instruction block

With the help of curly brackets, instructions are grouped together. This means that all definitions and

instructions belonging to a function are noted in curly brackets, this is then called the functional

block. At each point where an expression can stand, an instruction block can also stand. These can

also be nested as required.

void deliver ( )

{

int variable1, variable2

Variable1 = IKV [2010] + 1 ; Count up

...

}

Jump marks

Jump marks must be in [.....] brackets, may only be a maximum of 32 characters long, must stand

alone in a line and a maximum of 256 jumps marks must be available in the G-Code program .

[Start]

GOTO/IF ... GOTO/

IF ELSE

Jump commands are defined with GOTO instructions. GOTO instructions are either alone in the block

or together with IF instructions. Behind the GOTO command there is the jump mark to which it is to

be branched. With IF, conditions for jumps, the conditional execution of instructions or instruction

sequences, can be formulated. With ELSE; an expression_2 which is to be alternatively processed can

be initiated. This branch is only reached in the case expression wrong.

 With example 1, the branching is to the jump mark

 With example 2, branching is only done to the jump mark if the <expression> is true

 With example 3, instructions1 are only executed if the <expression> is true Otherwise,

the instructions2 are processed.

GOTO [jump mark]

IF <Expression> GOTO [jump mark]

IF <Expression>

{

Instructions1

.....

}

Else

{

Instructions2

.....

}

Page 71

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

FOR loops

With FOR, the conditional and repeated execution of program parts can be formulated. For the case

<Expression2> is true, the following program part, including <Expression3> is processed. In the case

<Expression2> is not true, the system jumps to the next instruction after the loop. If an

<Expression> is not used, the comma needs to be set nevertheless. (, <Expression2>,

<Expression3). In the expressions 1-3, no traverse commands or NC addresses may be used.

Instead, only calculation expressions and comparisons may be used. With the key word BREAK, the

loop can be terminated early. With the key word CONTINUE, the next loop run can be initiated before

the loop end has been reached. As many FOR loops can be used in the program as required and

these can be nested in one another.

FOR ( <Expression1>, <Expression2>, <Expression3> )

{

Instructions

.....

}

- <Expression1>is processed once at the start of the loop

- <Expression2>= true -> execute loop

- <Expression3>is processed during every loop run. A counter is often counted up/down here.

WHILE loops

With WHILE, the conditional and repeated execution of program parts can be formulated. For the

case <Expression> is true, the following program part is processed. In the case <Expression> is not

true, the system jumps to the next instruction after the loop. In the expression, no traverse command

and no NC addresses may be used. Instead only calculation expressions and comparisons may be

used. The loop can be terminated early with the key word BREAK. With the key word CONTINUE, the

next loop run can be initiated before the loop end has been reached. As many FOR loops can be used

in the program as required and these can be nested in one another.

WHILE (<Expression>) ->

is checked here

{

Instructions

.....

}

If <expression> is true, the instructions are processed. Otherwise, they are skipped. The loop query

is done at the beginning of the loop.

DO ... WHILE loops

With DO ..... WHILE, the conditional and repeated execution of program parts can be formulated. For

the case <Expression> is true, the following program part is processed. In the case <Expression> is

not true, the system jumps to the next instruction after the loop. In the expression, no traverse

command and no NC addresses may be used. Instead only calculation expressions and comparisons

may be used. The loop can be terminated early with the key word BREAK. With the key word

CONTINUE, the next loop run can be initiated before the loop end has been reached. As many

DO...WHILE loops can be used in the program as required and also nested in one another.

{

Instructions

.....

}

WHILE (<Expression>) ->

is checked here

This loop is run through once in any case. If <expression> is true, the loop is run through again. (as

long as the <expression> is wrong). The loop query is done at the end of the loop.

Page 72

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

SWITCH ... CASE

branching

With the SWITCH instruction, a multiple branching can be programmed very easily. The individual

CASE branches can be terminated with BREAK and the system jumps to the end of the instruction. If

the BREAK is not at the end of a branch, the following branch is also processed. If none of the

options applies, the DEFAULT branch is processed, if available. In the <expression>, no traverse

command and no NC addresses may be used. Instead only calculation expressions and comparisons

may be used. As many SWITCH instructions can be used in the program as required and these can be

nested in one another.

SWITCH (<Expression>)

{

CASE X:

{

Instructions

.....

}

CASE X:

{

Instructions

.....

BREAK

}

CASE X:

{

Instructions

.....

}

DEFAULT:

{

Instructions

.....

}

The SWITCH... CASE instruction determines at the beginning the value of (<Expression>) this value

is then compared in the CASE branches with X. If it matches, the instructions in this branch are

processed. If no value matches, the instructions in the DEFAULT branch are processed. If no BREAK

is at the end of a branch, the next branch is also processed (even if the value of X does not match

(<Expression>).

Page 73

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Sample programs

#Para_Expr ;Functional example

DECLARE

void

MoveCorner ()

DECLARE

void

MoveCircle (

int

number)

DECLARE

float

StartPos ()

DECLARE

double

EndPos (

float

value)

float

GlobalVar

G00 X0 Y0 Z0

GlobVar = -2

MoveCorner ()

MoveCircle (3)

G01 X=StartPos() Y=Startpos()

G01 X=EndPos(GlobalVar) Y=EndPos(GlobalVar*2)

M30

void

MoveCorner () ; Function, without argument, without return value

{

G01 Y10

X10

}

void

MoveCircle (

int

number) ; Function, with argument, without return value

{

FOR (, Number >0, Number=Number-1)

{

G02 X0 Y0 I10 J0

}

float

StartPos () ; Function, without argument, without return value

{

RETURN (3.141)

}

double

EndPos (

float

value) ; Function, with argument, with return value

{

RETURN value=value*3.7

}

Page 74

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

#Para_Expr ;Rectangle example

DECLARE

void

rectangle (

float

Xvalue,

float

Yvalue)

F1000

G01 X0 Y0 Z0 ; Move to zero

Rectangle (10,10) ; Move rectangle 10x10

G01 X25 Y25 Z0 ; 2. position

Rectangle (7.453,13.443) ; 2. move rectangle

G93 W60 ; Turn coordinates system by 60 degrees

G01 X-14 Y-25 ; 3. position

Rectangle (7.453,13.443) ; 3. move rectangle

M30

void

rectangle (

float

Xvalue,

float

Yvalue) ; Definition of the function 'Rectangle' { G91 G01 Y=Yvalue X=Xvalue Y=-Yvalue X=-Xvalue G90 }

Page 75

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

#Para_Expr ; Loops example

Q1=0 Q2=30 ; X and Y width Q4=6 ; miller diameter Q5=Q2/2 Q6=50 Q7=1 Q10=3 Q11=3 Q99=1

F4000 G72 ; scaling off G90 ; Rel. G00 X0 Y0 Z0 G91 G01

[Main] SWITCH (Q7) { CASE 1: Q7=Q7+1 GOTO Loop normo BREAK

CASE 2: Q7=Q7+1 GOTO Loop inverse BREAK

CASE 3: Q7=Q7+1 GOTO Move eight BREAK

DEFAULT: GOTO end ; ! Do not forget colon BREAK }

[Loop normo]

WHILE (Q6<100) ;WHILE loop ( 45 runs ) { X10 Y-3 FOR (,Q5>10,Q5=Q5 -1) ;FOR loop ( 4 runs) { Y10 DO ;DO ... WHILE loop ( 5 runs) { X-3 Y-5 Y+7 X+5 Q4=Q4 - 0.7 } WHILE (Q4>2) Y-10 X5 } Q6=Q6 +1.1 GOTO Main } . . .

further see next page

Page 76

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Continuation

[loop inverse]

G73 X-1 Y-1 Q6=50 Q5=15 Q4=6 Q99=1

WHILE (Q6<100) ;WHILE loop ( 45 runs ) { X10 Y-3 FOR (,Q5>10,Q5=Q5-1) ;FOR loop ( 4 runs) { Y10 DO ;DO .. WHILE loop ( 5 runs) { X-3 Y-5 Y+7 X+5 Q4=Q4 -0.7 } WHILE (Q4>2) Y-10 X5 } Q6=Q6+1.1 GOTO Main }

[MoveEight] G01 X0 Y0 Z0 G02 X=Q1 Y=Q1 I=Q2 J=Q1 WHILE Q7>1 { G73 X= (-Q7 * 0.25) Y= (-Q7 * 0.25) G02 X0 Y0 I25 J0 G01 X0 Y0 Z0 G72 Q7=Q7-1 } G01 X0 Y0 Z0 M30 [End]

Page 77

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Page 78

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Index

Absolute circle center 46 absolute measure 37 Address letters 5 AKW 6 arc 12 Axis code word 6 Axis numbers 5

block numbers 7

change of plane 16, 23 circular interpolation 12 continuous operation cycle rotation 54 coordinate rotation 31 cycle execution 36

data types 64 DEF 9 direction of rotation 12 direction vector 26 Dwell time 13

eroding factors and modes 59 eroding time data 60 Eroding velocity 57

F parameter 11 feed movements 11 feed rate 11 FlexProg 63 free plane 22

H parameter 19

inch 33 incremental measure 38 inverse time programming 43

Machine functions 8 Macro 15 Macro call 15 Macro name 15 macros 65 Mathematical functions 68 measures 33 milling cutter radius correction 27

milling cutter radius correction left 27 milling cutter radius correction right 28 milling cutter radius correction up to 29 milling cutter radius correction via 30 milling lengthwise axis direction 19 mirror image machining 33, 34 mm 33 modal 7, 9

non-modal 7

Offset number 55 online spline 26 Orbital movement 61

Parameter programming 62 path information 10 plane 16 position transformation 19 Positioning 10, 11 program structure 64

Q parameter 62 Q-Parameter 65

rapid traverse movement 10 rapid traverse speed 10 Relative circle center 47 relative measure 38 Revisions 80 rotation 22 RTCP 19

scaling 33, 35 Simple measurement block 49 spatial arc 14 spatial arc interpolation 14 spatial circle section 14 speed programming 42 Spindle offset 55 spline 26 spline arc point 26 spline interface 26 Sub program call 17 Subroutine call 18

target point 10 TCP 19 Text functions 18 time programming 43 Tool Center Point 19 Tool zero point 24

Page 79

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

zero offset 31, 32, 56

zero offset table 56

Page 80

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

Revisions

Id.-Nr.

Version

Stand

Additions and changes

1400.010B.0-00

V7.00.00.00

11/2016

First Version (only field test release)

1400.010B.0-01

V7.00.00.01

04/2018

New G code functions:

 G23 Text - Functions  G181 Probe calibration  G781,1 Spindle offset  G783,0 Read / write zero offset  G488,1 Simple measurement block

Additions:  G1001 … G1004 Eroding

FM/AP

Page 81

MotionOne CM

G&M Code Programming Manual

Id.-Nr.: 1400.210B.0-01 ▪ Stand: 04/2018

LTI MOTION MotionOne CM Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual