MotionOne CM G&M Code Programming Manual

Transcription

1 SystemOne CM CNC

2 2 MotionOne CM MotionOne CM Valid for G&M Code version since: V Doc version: V 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 LTI Motion GmbH LTI Motion GmbH Schlätterstraße 2 Gewerbestraße Wasserburg/Bodensee Lahnau Germany Germany Fon Fon.: Fax Fax: info@lti-motion.com info@lti-motion.com

3 MotionOne CM 3 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 G01 Positioning at the feed rate G02 Circular interpolation - Clockwise G03 Circular interpolation - Counterclockwise G04 Dwell time G05 Spatial arc interpolation G14 Macro call G17 Plane XY G18 Plane ZX G19 Plane YZ G22 Sub program call G23 Text - Functions G25 RTCP G26 Free plane G27 Tool zero point G30 Spline interface (online spline) G40 Deletion of the milling cutter radius correction G41 Milling cutter radius correction left G42 Milling cutter radius correction right G43 Milling cutter radius correction up to G44 Milling cutter radius correction via Zero offsets and coordinate rotation G53 Deletion of the zero offset G70 Units of measurement inch G71 Units of measurement mm G72 Deletion of mirror image machining and scaling G73 Mirror image machining G73 Scaling G79 Cycle execution G90 Absolute measure G91 Relative measure G92 Relative zero point offset coordinate rotation G93 Absolute zero point offset coordinate rotation G94 Speed programming G95 Time programming G107 Eroding: Define the directional vector for the lift-off movement G181 Probe calibration G190 Absolute circle center G191 Relative circle center G288 Set Look Ahead parameters G288,0 Look Ahead basic parameter G488 Simple measurement block G488,1 Simple measurement block G581 Continuous operation cycle rotation G781,1 Spindle offset G783,0 Read/Write zero points G1000 Eroding: Velocity G1001 Eroding: Directions G1002 Eroding: Factors and modes G1003 Eroding: Time data G1004 Eroding: Orbital movement in the selected plane... 61

4 4 MotionOne CM Parameter programming Flexible G&M code Programming (FlexProg) General Restrictions General program structure Data types Functions (general) Function declaration Macros and Q parameters Function definition Variables Communication variables Expressions and operators Mathematical functions Assignment of NC addresses Comment marks Point definition Instructions Jump marks GOTO/IF... GOTO/ IF ELSE FOR loops WHILE loops DO... WHILE loops SWITCH... CASE branching Sample programs Index Revisions... 80

5 MotionOne CM 5 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 N Block number G Path condition A, B, C Path information A axis, B axis, C axis X Path information X axis, dwell time Y, Z Path information Y axis, Z axis I, J, K Interpolation parameters, circle center F Feed rate, time for G95 (inverse time programming) O Output address D Additional information (cutting edge correction table) E Additional information on the PLC S Spindle speed T Tool number M Machine function W 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

6 6 MotionOne CM Axis code word (AKW) The program WINAKW.exe to determine the axis code 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 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)

7 MotionOne CM 7 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) G Path condition A Path information A axis B Path information B axis C Path information C axis X Path information X axis, dwell time Y Path information Y axis Z Path information Z axis I, J, K Interpolation parameters, circle center F Feed speed, dwell time, time display at G95 (Invers Time Programming) O Output address D Auxiliary information (correction memory) E Additional information on the PLC S Spindle speed T Tool number M Machine function W Command extension G02 X50 Y0 I25 J0 F2000 S10000 M3 T7 M6 G02 X50 Y0 I25 J0 F2000 S10000 M03 M06 Path condition circle in clockwise direction X coordinate Y coordinate Auxiliary parameter circle center X coordinate Auxiliary parameter circle center Y coordinate Feed speed 2000 mm/min Spindle speed /min Machine function 'Spindle on' 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

8 8 MotionOne CM M Functions Note: The M functions initiate certain machine functions. These functions may differ depending on machine type/manufacturer. General M functions M Function C.* M00 Programmed stop 1 M01 Optional stop 1 M02 End of program 1 M19 Spindle stop with defined end position 1 M30 End of program with spindle 0 Off 1 M functions for control type eroding "EROD" M Function C.* M92 Lift-off via programmed direction vector (G107 ) 2 M93 Delete last retraction point 2 M94 Spark erosion function AFC OFF, no forward and backward interpolation 2 M95 Spark erosion function AFC ON 2 M96 Retreat on the path ON 2 M97 Retreat via points ON 2 M98 Saving the actual position as a retraction point 2 M800 Switching off collision protection via NC program 2 M801 Switch collision protection on again 2 M802 Modulo formation off 2 M802 Modulo formation on 2 M900 Activate sparking out 2 * Comments on the M commands: 1 Function is effective at end of block 2 Function is effective at start of block

9 MotionOne CM 9 G Functions General explanations : : Position: MODAL means that the command/function remains active until it is overwritten. The G functions can be divided into the following topics: interpolation type special command setup command tool command cycle command eroding command DEF = Default (active after starting the control unit) --- = Not pre-set

10 10 MotionOne CM G00 Positioning in rapid traverse Position --- modal Axis movement 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

11 MotionOne CM 11 G01 Positioning at the feed rate Position modal Axis movement DEF 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

12 12 MotionOne CM G02 Circular interpolation - Clockwise G03 Circular interpolation - Counterclockwise Position --- modal Axis movement 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)

13 MotionOne CM 13 G04 Dwell time Non modal NC command Position --- 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 X 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 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: sec G04 X11.4 G04 X0 G04 ; Dwell time 11.4 seconds ; Dwell time 0 seconds ; Contour interruption

14 14 MotionOne CM G05 Spatial arc interpolation Position --- modal Axis movement 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

15 MotionOne CM 15 G14 Macro call Position --- non-modal Special command 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

16 16 MotionOne CM G17 Plane XY G18 Plane ZX G19 Plane YZ Position modal Setup command Preset G17 G17 / G18 / G19 ATTENTION: G18 in the CNC is not according to the DIN The use of G18 according to DIN can be activated in the XPanel user interface Service F6-System programs F4-System configuration G&M converter G18 according to DIN 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.

17 MotionOne CM 17 G22 Sub program call Position --- non-modal Special command 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: G22 N = Feed program P3 ; Feed program called three times

18 18 MotionOne CM G23 Text - Functions Position --- non-modal NC command 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 not necessary 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. 5 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 Default: 0 G23 P3 N= Finishing part1 G23 P3 N = Finishing part1 I1 G23 P3 N = Finishing outside I2 G23 P4 N = C:\Messung_123.log IKV[100] = 156 G23 P5 N = C:\Daten_123.log I100 Text is displayed in the prompt of the XPanel position menue in line 1. Text is displayed in the prompt of the XPanel position menue in line 1. Text is displayed in the prompt of the XPanel position menue in line 2. 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" The value of IKV[100] is written into the log file "C:\andron\SystemData\Repository\Cycles\Measuring Protocol\Daten_123.log".

19 MotionOne CM 19 G25 RTCP Position --- modal Transformation command 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 G25 H2 G25 H3 Switch on RTCP Save RTCP state Restore RTCP state RTCP is activated according to the kinematics of the machine defined in the machine parameters. The state of RTCP (ON/OFF) is stored in the buffer, e.g. to be used with tool change NC sets The state of RTCP (ON/OFF) stored in the buffer is restored, e.g. with a temporary deactivation in the tool change NC sets

20 20 MotionOne CM 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.

21 MotionOne CM 21 EMERGENCY STOP by operator, PLC, control programs EMERGENCY STOP due to drive error Referencing all axes or one axis RTCP is not reset automatically. RTCP is not reset automatically. 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 Moving axes in MDI with RTCP active G72/G73 Mirroring and RTCP Programmed feed F 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. All axes may be moved in MDI. There is no restriction as a function of the RTCP function. 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). 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.

22 22 MotionOne CM G26 Free plane modal Setup command Position --- G26 <Parameter list> 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 H H0 H1 H2 R R1 R0 WX, WY, WZ I, J, K 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 These parameters contain the angles to be set. Parameter H controls how to determine these angles to reach the new position. 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.

23 MotionOne CM 23 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 Example of Euler Example of cancelation G26 H1 WZ=-45 WY=30 K1 J2 G26 WX=-45 WY=30 G26

24 24 MotionOne CM G27 Tool zero point Position --- modal Transformation command 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 Rotation 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. 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

25 MotionOne CM 25 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 Kinematics model of the machine 30 Illustr.: Machine configuration in the MotionCenter, setting Kinematics model of the machine

26 26 MotionOne CM G30 Spline interface (online spline) Position --- modal Traverse command 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 ric path Fvalue Position of an axis Direction part (directional component) of an axis, not necessarily standardized 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.) 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)

27 MotionOne CM 27 G40 Deletion of the milling cutter radius correction Position modal Tool command DEF G40 Entering G40 will switch of all active milling cutter radius corrections (G41 - G44). G41 Milling cutter radius correction left Position --- modal Tool command 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.

28 28 MotionOne CM G42 Milling cutter radius correction right Position --- modal Tool command 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.

29 MotionOne CM 29 G43 Milling cutter radius correction up to Position --- modal Tool command 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

30 30 MotionOne CM G44 Milling cutter radius correction via Position --- modal Tool command 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

31 MotionOne CM 31 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

32 32 MotionOne CM G53 Deletion of the zero offset Position modal Setup command DEF G53 G53 will switch off all zero offsets (G54 G59 P0-P99, G92, G93).

33 MotionOne CM 33 G70 Units of measurement inch Position --- modal Setup command 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 Position modal Setup command DEF G71 The measures given are in mm. G72 Deletion of mirror image machining and scaling Position modal Setup command DEF G72 A mirror image machining and / or a scaling of the coordinates system is canceled.

34 34 MotionOne CM G73 Mirror image machining Position --- modal Setup command 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

35 MotionOne CM 35 G73 Scaling Position --- modal Setup command 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)

36 36 MotionOne CM G79 Cycle execution Position --- non-modal Cycle command 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.

37 MotionOne CM 37 G90 Absolute measure Position modal Setup command DEF 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

38 38 MotionOne CM G91 Relative measure Position --- modal Setup command 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

39 MotionOne CM 39 G92 Relative zero point offset coordinate rotation Position --- modal Setup command 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 W 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 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

40 40 MotionOne CM G93 Absolute zero point offset coordinate rotation modal Position --- Setup command 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 W WX, WY, WZ H0 H1 I, J, K H2 Rotation of the coordinate system on the current plane 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. 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 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. 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 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.

41 MotionOne CM 41 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).

42 42 MotionOne CM G94 Speed programming Position --- modal Setup command 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.

43 MotionOne CM 43 G95 Time programming Position --- modal Setup command 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 Extended Invers Time Normal Inverse time programming 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 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 E 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. 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 T1 M6 S2000 M3 G00 Z10 G95 E1 ; Switch on EIT (multiplication factor = 1) G01 Z A19 C0 F X Y A19 C0 F X69.85 Y A19 C0 F X Y A19 C0 F X Y A19 C0 F X Y-0.45 A19 C0 F

44 44 MotionOne CM G107 Eroding: Define the directional vector for the lift-off movement modal Eroding command Position --- 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 X, Y, Z, U, W, V; A0=, A1=, A15= Description 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

45 MotionOne CM 45 G181 Probe calibration non-modal Cycle command Position --- 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. D1 Emptying of the mprot.log (ASCII)

46 46 MotionOne CM G190 Absolute circle center Position modal Setup command DEF 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

47 MotionOne CM 47 G191 Relative circle center Position --- modal Setup command 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

48 48 MotionOne CM 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 Position --- modal Setup command 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 D E H K Feed rate [mm/min] Rapid traverse speed [mm/min] Quality of input data [μm] Contour precision [μm] Smoothing of contour [ms] N Max. acceleration [m/s 2 ] O Jerk limit acceleration [m/s 3 ] X Jerk limit X-axis [m/s 3 ] Y Jerk limit Y-axis [m/s 3 ] Z Jerk limit Z-axis [m/s 3 ] A Jerk limit A-axis [m/s 3 ] B Jerk limit B-axis [m/s 3 ] C Jerk limit C-axis [m/s 3 ]

49 MotionOne CM 49 G488 Simple measurement block Position --- non-modal Cycle command 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: A 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 Y Z B E I K C R 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. see X see X Positioning feed Measuring feed Repeat measurements. Specifies the repeat measurements. Each measurement is carried out again from the start position. Shaft probing method. Calculation method for determining the measurement result. Activate Point log C0 - Protocol output disabled (Default) C1 - Protocol version 1 C2 - Protocol version 2 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

50 50 MotionOne CM 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 X 2 2 Y Z 4 4 P Y 8 8 Q B R C U D V E W The binary value produces 14 decimally (axis code word of the axes X, Y and Z)

51 MotionOne CM 51 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 X- axis), 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 Y- axis), starting position (for the Z-axis). Maximum measurement value (for the axis with the axis number or depending on the level of the X- axis), 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 X- axis), 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.

52 52 MotionOne CM Communication variables for FlexProg Cycle Description Variable Meaning G488 Simple measurement block IKV [2000] IKV [2001] IKV [2002] IKV [2003] IKV [2004] IKV [2005] IKV [2006] IKV [2007] IKV [2008] IKV [2009] Cycle number Extended cycle number Tool number Axis number used for carrying out the measurement Number of repeats Averaging method Radius calculation Point log activated Calculate touch probe transformations from G181 Retract to the start position / measuring position FKV [2000] FKV [2001] FKV [2002] FKV [2003] FKV [2004] FKV [2005] FKV [2006] FKV [2007] FKV [2008] FKV [2009] FKV [2010] FKV [2011] FKV [2012] FKV [2013] FKV [2014] FKV [2015] FKV [2016] 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) Measurement result depending on the input for surface or sphere center (for the Y-axis) Measurement result depending on the input for surface or sphere center (for the Z-axis) Start position( for the axis carrying the axis number or depending on the plane of the X-axis) Start position (for the Y-axis) Start position (for the Z-axis) Maximum measured value (for the axis carrying the axis number or depending on the plane of the X-axis) Maximum measured value(for the Y-axis) Maximum measured value(for the Z-axis) Minimum measured value (for the axis carrying the axis number or depending on the plane of the X-axis) Minimum measured value (for the Y-axis) Minimum measured value (for the Z-axis) Maximum measured value jump (for the axis carrying the axis number or depending on the plane of the X- axis) Maximum measured value jump (for the Y-axis) Maximum measured value jump (for the Z-axis) Tool diameter from the TM Tool length from the TM

53 MotionOne CM 53 G488,1 Simple measurement block Position --- non-modal Cycle command 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.

54 54 MotionOne CM G581 Continuous operation cycle rotation Position --- non-modal Cycle command 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 B C N Axis selection. This input selects (1) or deselects (0) the corresponding axis. see A see A Speed of the selected axis in revolutions/minute. The sign determines the direction of rotation of the axis. G581 A1 B0 C1 N30

55 MotionOne CM 55 G781,1 Spindle offset Position --- modal NC command : G781,1 N<Spindle number> X<Offset in X> Y<Offset in Y> Z<Offset in Z> : 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 N X, Y, Z A, B, C K I 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. 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. 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) 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]) Applicabl e range -1 to 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]

56 56 MotionOne CM G783,0 Read/Write zero points Position --- modal Special command 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 N D X, Y, Z, A, B, C K L R Number of the desired zero point. Page of the zero offset table. If N is not used, the first page applies. Action: 0 - activate zero point 5 - write 9 - read 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. or 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>. 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> 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 K A 0 X 8 ANG 16 X 1 Y 9 RCS 17 Z 2 P 10 WX 18 Y 3 Q 11 WY 19 B 4 R 12 WZ 20 C 5 U 13 H 21 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

57 MotionOne CM 57 G1000 Eroding: Velocity Position --- modal Eroding command 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

58 58 MotionOne CM G1001 Eroding: Directions Position --- modal Eroding command 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 mm B Interval path: Maximal path for returning during an interval otherwise first returning point mm C Short interval path: Path for returning during short interval path mm I Approach path: Path of approaching erosion contour after an interval or interruption which isn t moved with feed or rapid motion but eroding mm Length of the 3 rd 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). mm 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 B C1.000 I0.000 J0.000

59 MotionOne CM 59 G1002 Eroding: Factors and modes modal Eroding command Position --- 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 A E H K L I J B C D N Description Factor start-up acceleration Factor speed eroding forward Factor speed eroding backward Factor speed of the radius change orbital movement forward, direction erosion front Factor speed of the radius change orbital movement backwards, direction circle center Factor (returning point) RZP eroding forward (move to erosion contour) Factor RZP eroding backward (leave path) Mode of interval 0: no interval 1: Time controlled ( cyclic ) 2: Generator controlled ( adaptive ) 3: Generator and time controlled (both) Command: 0: Switch of High-Speed-Jump 1: Switch on High-Speed-Jump, mode 1 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. Additional factor for for the speed of an orbital movement (see also G1004 Exxx). f = e min b = e min Factor speed eroding forward resp. factor RZP eroding forward Factor speed eroding forward resp. factor RZP eroding backward e: 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

60 60 MotionOne CM G1003 Eroding: Time data Position --- modal Eroding command 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 sec forward signals are constantly present. 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

61 MotionOne CM 61 G1004 Eroding: Orbital movement in the selected plane Position --- modal Eroding command 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) mm E Velocity (required if K word 0) ms/rotation H Height of the cone (required if K word = 3) mm G1004 K1 R0.005 E1000

62 62 MotionOne CM 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. Qn = [-]Expression1 Qn = [-]Expression1 Operator Expression2 n = Index of the Q parameter [ ] 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: < > = <= >=!= < > = <= >=!=

63 MotionOne CM 63 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.

64 64 MotionOne CM 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 callup 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 Float significant Double significant

65 MotionOne CM 65 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. 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 Q234 =

66 66 MotionOne CM 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. <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 onedimensional 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: DECLARE <Data type> <Variable name> If several variables of the same time are used, the declaration is as follows: <Data type> <Variable name1>, <Variable name2>, <Variable name3> 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

67 MotionOne CM 67 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 [ ] (stands in the EEPROM). The user should use the index 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)

68 68 MotionOne CM 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). Variable = Expression Q125 = 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 >0 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

69 MotionOne CM 69 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 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 G0 P1 C90 Q4 = Q4 + Q10 G0 P1 C90 ; for P1, calculations are indicated ; 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 is changed ; 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

70 70 MotionOne CM 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] } ; 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] 1 IF <Expression> GOTO [jump mark] 2 3 IF <Expression> { Instructions1... } Else { Instructions2... }

71 MotionOne CM 71 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>) { Instructions } -> is checked here 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. DO { 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.

72 72 MotionOne CM 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>).

73 MotionOne CM 73 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 () { G01 Y10 X10 Y0 X0 } ; Function, without argument, without return value void MoveCircle (int number) ; Function, with argument, without return value { FOR (, Number >0, Number=Number-1) { G02 X0 Y0 I10 J0 } } float StartPos () { RETURN (3.141) } ; Function, without argument, without return value double EndPos (float value) { RETURN value=value*3.7 } ; Function, with argument, with return value

74 74 MotionOne CM #Para_Expr ;Rectangle example DECLARE void rectangle (float Xvalue, float Yvalue) F1000 G01 X0 Y0 Z0 Rectangle (10,10) G01 X25 Y25 Z0 Rectangle (7.453,13.443) G93 W60 G01 X-14 Y-25 Rectangle (7.453,13.443) M30 void rectangle (float Xvalue, float Yvalue) { G91 G01 G90 } Y=Yvalue X=Xvalue Y=-Yvalue X=-Xvalue ; Move to zero ; Move rectangle 10x10 ; 2. position ; 2. move rectangle ; Turn coordinates system by 60 degrees ; 3. position ; 3. move rectangle ; Definition of the function 'Rectangle'

75 MotionOne CM 75 #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 G90 G00 X0 Y0 Z0 G91 G01 ; scaling off ; Rel. [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 BREAK } ;! Do not forget colon [Loop normo] WHILE (Q6<100) ;WHILE loop ( 45 runs ) { X10 Y-3 FOR (,Q5>10,Q5=Q5-1) ;FOR loop ( 4 runs) { Y10 Y-10 X5 } Q6=Q GOTO Main }... further see next page DO { X-3 Y-5 Y+7 X+5 Q4=Q4-0.7 } WHILE (Q4>2) ;DO... WHILE loop ( 5 runs)

76 76 MotionOne CM 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 Y-10 X5 } Q6=Q6+1.1 GOTO Main } DO { X-3 Y-5 Y+7 X+5 Q4=Q4-0.7 } WHILE (Q4>2) ;DO.. WHILE loop ( 5 runs) [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]