engineering mannesmann Rexroth MTC200 / MT-CNC NC Programming Instructions 17VRS Application Manual DOK-MTC200-NC**PRO*V17-ANW1-EN-P 274929 Indramat
About this document NC Programming 17VRS Title Typ of document Doku-Type Internal filing NC Programming Instructions 17VRS Application Manual DOK-MTC200-NC**PRO*V17-ANW1-EN-P • Folder 1 / Register 2 • Drawing number: 109-0768-4194-EN/05.97 Purpose of the document This document describes the software version 005-17VRS. In earlier software versions (Docu. No. 109-0668-4183-xx), some of the functions that are described here are not contained at all, or in a restricted version only.
NC Programming 17VRS Table of Contents I Table of Contents 1 General Information .................................................................................................... 1-1 1.1 General Information ............................................................................................................................. 1-1 1.2 Program and Data Organization .......................................................................................................... 1-2 2 NC Program ...........
II Table of Contents NC Programming 17VRS Free Plane Selection 'G20'.......................................................................................................... 3-16 3.7 Diameter and Radius Programming 'G15' / 'G16' .............................................................................. 3-19 3.8 Dimensional Units .............................................................................................................................. 3-20 Inch Programming Input 'G70'..............
NC Programming 17VRS Table of Contents III 4.5 Spindle Speed.................................................................................................................................... 4-42 S-Word for the Spindle RPM Statement ..................................................................................... 4-42 Select Main Spindle for Feed Programming 'SPF' ...................................................................... 4-43 Constant Grinding Wheel Peripheral Speed (SUG) 'G66'.........
IV Table of Contents NC Programming 17VRS 5.5 Activating and Canceling Tool Path Compensation........................................................................... 5-33 Canceling Tool Path Compensation 'G40' .................................................................................. 5-33 Tool Path Compensation, Left of Workpiece Contour 'G41' ....................................................... 5-34 Tool Path Compensation, Right of Workpiece Contour 'G42'....................................
NC Programming 17VRS Table of Contents V 8.2 Tool Storage Motion Commands ......................................................................................................... 8-3 Tool Storage to Reference Position ‘MRF’.................................................................................... 8-3 Tool Storage to Home Position ‘MHP’........................................................................................... 8-3 Move Tool into Position ‘MTP’.....................................
VI Table of Contents NC Programming 17VRS 9.7 Conditional Branches Upon the Results of Arithmetic Operations..................................................... 9-16 Branch If Equal to Zero ‘BEQ’ ..................................................................................................... 9-16 Branch If Not Equal to Zero ‘BNE’............................................................................................... 9-16 Branch If Greater Than or Equal to Zero (If Minus) ‘BPL’ ...............
NC Programming 17VRS Table of Contents VII 13 NC Programming Practices.................................................................................... 13-1 13.1 Efficient NC Programming ............................................................................................................... 13-1 14 Appendix.................................................................................................................. 14-1 14.1 Table of G Code Groups............................................
VIII Table of Contents NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
General Information 1-1 NC Programming 17VRS 1 General Information 1.1 General Information A CNC (Computer Numerical Control) is a special computer used to control a machine tool, robot or transfer system. Like a personal computer, the CNC control has its own operating system, which is specifically designed for numerical applications, as well as so-called control software installed on this operating system.
1-2 General Information 1.2 NC Programming 17VRS Program and Data Organization Data structure of the CNC with user interface on an IBM-PC and an SOT (stations operator terminal). MT-CNC Data User Interface NC Program List 12 1. Parameter Set 99 1. 99 1. Tool List SOT Data Hard Disk User Interface NC List Process 1 0 NC Variable List Process 0 1 2 2 3 3 4 4 5 6 Cur.
NC Programming 17VRS General Information 1-3 Approximately 400KB available memory is present on the basic version of the CNC. As shown in Figure 1-1, the CNC-memory is divided into several areas. The individual areas are described briefly in the following sections. The CNC controller is adapted to the given machine or system by means of parameters. Up to 99 different parameter sets can be managed on the user interface.
1-4 General Information NC Programming 17VRS NC Program Package 6 5 3 4 2 1 Data for Process 0 Setup List (Optional) NC Program 1 . . NC Program 99 Fig. 1-2: NC program package Tool setup list The tool setup list contains a tool data set for each T number used in the NC-program. This tool data set defines which tool is to be used and which specifications this tool must meet.
NC Program 2-1 NC Programming 17VRS 2 NC Program 2.1 Organization of the Tool Setup Lists A tool setup list can be created for any process which uses tool. This list allows any given tool names or tool numbers to be assigned to the T numbers used in the NC-program. The Setup List also contains the tool specification data. Setup Lists can be organized to be station-specific or program-specific. up to 7 tool setup lists (1 per process) are possible.
2-2 NC Program 2.2 NC Programming 17VRS Program Organization The NC-program and its command set is based on DIN 66025 / ISO Draft 6983/2 together with specific INDRAMAT enhancements. 99 NC-program packages can be managed on the user interface. Each NC-program package can contain up to 99 NC-programs for each process. Thus, an NC-program package can consist of 693 NC-programs (7 processes * 99 NC-programs).
NC Program 2-3 NC Programming 17VRS Advance program An advance program consists of a complete sequence of NC-blocks needed to produce a workpiece. In addition to the path information needed for machining, the advance program also contains all additional auxiliary functions and branch/jump commands for subroutines and cycles. The advance program ends with the NC-block in which RET (end of program with reset) is programmed. Example T4 BSR .M6 T8 MTP G00 G90 G54 X0 Y0 Z50 S5000 M03 G01 X46 Y144 Z2 . .
2-4 NC Program 2.3 NC Programming 17VRS Process-Specific Programming The CNC is organized into a maximum of 7 processes. Each process has its own NC-block preparation which combines the data from the NC-program with data such as zero points, Setup Lists, etc. The number of processes is declared in the system parameters. Or if more than 2 processes are declared, process 0 is generally used to synchronize the other processes.
NC Program 2-5 NC Programming 17VRS 2.4 Elements of an NC Block An NC-block contains data for performing an operating step. The NCblock consists of one or more words as well as the NC control commands. The NC-block length must not exceed 240 characters, and it can be split among no more than four lines.
2-6 NC Program NC Programming 17VRS NC blocks that can be skipped In an NC-controlled machine tool, a simple way must be provided to skip NC-blocks so that certain functions such as gaging operations, part loading and unloading and the corresponding program NC-blocks can be allowed to proceed in a controlled manner or can be skipped. Blocks in a part program which are not to be processed each time the program is executed must be identified by a slash "/" at the beginning of the NC-block.
NC Program 2-7 NC Programming 17VRS Numerical value The numerical value can have signs and decimal points. The sign is located between the address letter and the numerical value. A positive sign does not need to be entered. Word Format Address Letter Value 500 X Extended Address Format Address Letter S No. Space Value 1 1000 Fig. 2-5: Word syntax Example ; Enhanced address structure for an X1 and Y1 axis G01 X1 50.45 Y1 35.
2-8 NC Program NC Programming 17VRS In terms of syntax, the label begins with a decimal point followed by at least one and no more than six legal characters. The syntax is not case sensitive. The * sign following the decimal point is reserved for INDRAMAT canned cycles. When a label is programmed in a NC-block, the label must be the first element in the NC-block after the number. A branch command using a label is considered to be a program control command, and, based on its priority, it is performed last.
NC Program 2-9 NC Programming 17VRS Comment in the Source Program Syntax ; Text Each NC-block can contain one comment in the source program which is introduced by a semicolon. All characters following the semicolon are interpreted as a comment. The term comment in the source program means that the comment is only present in the source program—that is, on the user interface—and not in the controller memory.
2-10 NC Program NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Motion Commands, Dimension Inputs 3-1 NC Programming 17VRS 3 Motion Commands, Dimension Inputs 3.1 Coordinate System The coordinate system defines the location of a point or series of points in a plane or in space relative to two or three NC axes. As a rule, the right-hand, orthogonal Cartesian coordinate system having axes X, Y and Z is used in NC technology. This system is defined relative to the main axes of the machine. Y Y B R C Z A X X Z Fig.
3-2 Motion Commands, Dimension Inputs 3.2 NC Programming 17VRS Motion Commands The motion command or traverse instruction causes an axis to move or traverse. The motion command consists of the address letter of the axis address (for example, X, Y or Z) followed by the sign (+, -) to indicate the direction of motion, and the distance to be traversed, the coordinate value. Syntax Syntax: Address Letter Coordinate Value Z 100.
Motion Commands, Dimension Inputs 3-3 NC Programming 17VRS 3.3 Dimension Input The motion commands for the axes can be entered in two different ways: • As an absolute dimension input (G90) or • as an incremental dimension input (G91). Input Data as Absolute Dimensions 'G90' With absolute dimension input all dimensions are stated relative to a fixed zero point. When the CNC-program boots, the initial setting is G90. G90 remains in effect until it is written over with G91.
3-4 Motion Commands, Dimension Inputs NC Programming 17VRS Input Data as Incremental Values 'G91' Incremental positioning defines all subsequent dimensional entries as differences relative to the NC-block starting position. G91 remains in effect until the end of the program or until it is overwritten by G90. Example Y 100 80 [P2] [P3] [P1] [P4] 60 40 20 20 40 60 80 100 120 140 X Fig. 3-3: Input data as incremental values G00 G90 G54 X0 Y0 Z3 S1000 M03 G01 G91 X50 Y50 F500 BSR .
Motion Commands, Dimension Inputs 3-5 NC Programming 17VRS 3.4 Zero Points Zero points and various reference points used to establish workpiece geometry are defined on all numerically controlled machines. Machine zero point The machine zero point is located in a fixed position at the origin of the machine coordinate system, and it cannot be moved. Icon for the machine zero point M Machine reference point The machine reference point is a defined point located within the working range of the machine.
3-6 Motion Commands, Dimension Inputs NC Programming 17VRS X R M W Z Fig. 3-5: Zero points—lathe (machining ahead of the center of rotation) 3.5 Zero Offsets The zero offsets permit the origin of a coordinate axis to be offset by a given value relative to the machine zero point. The position of the machine zero point is permanently stored in the CNC-memory and is not changed by the zero offset. Z Z' P Z Angle of Rotation 'P' for the active Plane (G18) Y P X' X 'NV' Zero Offset Y X Fig.
Motion Commands, Dimension Inputs 3-7 NC Programming 17VRS piece zero point G52. This allows an identical NC-program to be processed at various machine positions. The position of the machine zero point of each axis is declared in the drive parameters as the difference relative to the reference point. The value entered in the drive parameters corresponds to the coordinate value of the reference point in the machine coordinate system.
3-8 Motion Commands, Dimension Inputs NC Programming 17VRS The programmable zero offsets G50 and G51 become inactive when G52, G53, G54 ... G59 are programmed. CAUTION Adjustable Zero Offsets 'G54 ... G59' The adjustable zero offsets are entered in the zero offset table for those axes which are present using the user interface. The entered values function as an absolute offset relative to the machine zero point.
Motion Commands, Dimension Inputs 3-9 NC Programming 17VRS Coordinate Plane Rotation by Angle of Rotation 'P' Coordinate plane rotation is used to adapt the coordinate system of the workpiece to the coordinate system of the machine. The angle of rotation P is assigned to the individual zero offsets G54 … G59, G50, G51 and the adjustable general offset. Coordinate rotation is always active in the active plane (for example G17).
3-10 Motion Commands, Dimension Inputs NC Programming 17VRS Zero Offset Tables 'O' The CNC allows the adjustable zero offsets, G54 …G59 to be addressed up to ten times using different coordinate values. The zero offset table can be present up to ten times in the CNC. The designation for each zero offset table is zero offset table. Note: The number of zero point databases is specified by the machine builder in the process parameters. The selection criterion in the NC-program is the NC command O[0..
Motion Commands, Dimension Inputs 3-11 NC Programming 17VRS Example Y Y 100 80 60 80 Y 60 [P3] [P4] 100 40 [P2] [P5] 80 [P8] 20 60 [P7] [P1] 40 20 40 40 60 80 100 X ZO Pt. Table No. 0 20 Value G54 X17.5 Y46.5 20 [P6] Zero Pt. Table No. 1 Entry in the ZO Table with G54 : 20 40 60 80 100 X 120 X X81.0 Y29.5 20 40 60 80 100 Fig. 3-11: Calling 2 zero offset tables using G54 [Zero offset table no. 0 is active] G00 G90 G54 X0 Y0 Z10 S1000 M03 G01 X30 Y30 F1000 BSR .
3-12 Motion Commands, Dimension Inputs NC Programming 17VRS Programmed Absolute Zero Offset 'G50' Programmed incremental zero offset 'G51' The programmed zero offsets G50 and G51 move the machining zero point with • G50 absolute or • G51 incremental to the most recently selected workpiece zero point by the offset values which were declared together with the address letters.
Motion Commands, Dimension Inputs 3-13 NC Programming 17VRS Programmed Workpiece Zero Point 'G52' A workpiece zero point can be programmed as the axis position for all axes which are present using programmed workpiece zero point G52. When G52 is performed, the coordinate values to which the G52 command applies are assigned to the current position. This corresponds to the definition of the workpiece zero point relative to the current position.
3-14 Motion Commands, Dimension Inputs NC Programming 17VRS Cancel Zero Offsets 'G53' All zero offsets are canceled by programming G53. This causes the workpiece coordinate system to be switched to the machine coordinate system. • Depending on the setting in the process parameters, G53 can be the power-on default and the initial setting when the NC-program starts. • If G53 is placed in a NC-block containing G91 only the position display is switched to the machine’s actual system.
Motion Commands, Dimension Inputs 3-15 NC Programming 17VRS 3.6 Plane Selection Plane selection is an important requirement for correctly performing all motion commands in an NC-program. It informs the controller of the plane on which machining is performed in order to permit a correct calculation of the tool correction values. It also plays a role in circle programming.
3-16 Motion Commands, Dimension Inputs Note: NC Programming 17VRS The default plane is specified by the machine builder in the process parameters. A change in the selected plane overwrites the previous plane selection and remains modally active. The default plane is selected at the end of the program and upon ‘Control Reset’.
Motion Commands, Dimension Inputs 3-17 NC Programming 17VRS • The G17 ... G20 commands form a group (G code group 2). • A change in the plane selection overwrites the previous plane selection and has a modal effect. • At the end of the program (BST, RET, JMP, M02 and M30), upon a control-reset, and upon a transition to manual mode (if the process parameter „Manual axis jogging causes reset“ has been set), the NC selects the base coordinate system (Cxx.053 axis parameter, Axis defined in tight hand coord.
3-18 Motion Commands, Dimension Inputs NC Programming 17VRS Example A turning center possesses the following axes within a process (axes within the turning center (process 0)): Axis designation Axis meaning X1 X Turning slide X2 W Milling slide Y Y for milling Z Z for turning and milling C C for machining on the lateral surface B B swivel axis for the milling slide U U tailstock S1 S1 main spindle S2 S2 tool spindle for milling X1 Comment X2 B S2 Z Y U C/S1 Fig.
Motion Commands, Dimension Inputs 3-19 NC Programming 17VRS When ‘G20 Z0 C0 X2=0‘ is used for selecting the coordinate system of the subsequent lateral cylinder surface machining process, the axis meanings are allocated as follows (example): • Starting from the allocations that have been defined in the axis parameters, the axis Z obtains the axis meaning X, and the axis X1 the axis meaning Z. • In a second step, axis C obtains axis meaning Y and axis Y obtains axis meaning C.
3-20 Motion Commands, Dimension Inputs NC Programming 17VRS position. With circles the circle center points and end points are to be stated as a difference in diameter relative to the starting point. • The thread lead is interpreted as a radius dimension when machining face threads on a lathe. • Functions like constant surface speed and feed per revolution in the X direction are not affected by diameter programming.
Motion Commands, Dimension Inputs 3-21 NC Programming 17VRS Metric (mm) Programming Input 'G71' If 'inches is set in the process parameters as the basic programming unit, the subsequent values are interpreted as millimeter data and are converted to inches internally after G71 has been programmed. • Motion commands (coordinate values); for example X127mm is converted to X5 inches.
3-22 Motion Commands, Dimension Inputs 3.9 NC Programming 17VRS Mirror Imaging of Coordinate Axes 'G72' / 'G73' The programmable mirror function permits the mirror imaging of any desired coordinate axes within a machining program. When a coordinate axis is mirror imaged, the original contour is machined symmetrically opposite in the same size and at the same distance on the other side of the mirror imaging axis.
Motion Commands, Dimension Inputs 3-23 NC Programming 17VRS Example Mirror Imaging Y 70 60 50 40 4 1 30 20 10 -10 3 X 10 20 30 40 50 60 70 2 Fig. 3-19: Correlation when mirror imaging one or more coordinate axes NC program DOK-MTC200-NC**PRO*V17-ANW1-EN-P G00 G54 G90 X0 Y0 BSR .TRIA G50 X50 G73 X-1 BSR .TRIA G72 G50 X-20 Y40 G73 X-1 Y-1 BSR .TRIA G72 G50 X-50 Y20 G73 Y-1 BSR .TRIA G72 RET .
3-24 Motion Commands, Dimension Inputs NC Programming 17VRS 3.10 Scaling 'G78' / 'G79' The scaling function provides programmable scaling factors to change the scale used for the distance to be traversed on all machine axes. The activation and deactivation of the scaling preparatory G-function is programmed using the Preparatory G-functions in the part program. Scaling can be activated via G79.
Motion Commands, Dimension Inputs 3-25 NC Programming 17VRS Example Scaling Y 70 60 50 40 1 30 20 First Traverse Move 10 after Selecting Scaling -10 X 10 20 30 40 50 60 70 80 90 100 110 120 130 140 150 Y 80 70 60 50 40 30 20 10 2 X 10 20 30 40 50 100 Fig. 3-20: Example of programming using the scaling preparatory G-function NC program DOK-MTC200-NC**PRO*V17-ANW1-EN-P G00 G54 G90 X0 Y0 BSR .TRIA G50 X40 Y-70 G79 X0.5 Y0.5 BSR .TRIA G78 G00 G54 G90 X0 Y0 RET .
3-26 Motion Commands, Dimension Inputs NC Programming 17VRS 3.11 Axis Homing Cycle 'G74' The preparatory function G74 axis homing cycle allows traversing to the reference point along one or more axes in an NC-program or via MDI NCblock entry. Syntax G74 <[Axis Name][CoordinateValue=0]> Example G74 X0 Z0 F10000 G74 is non-modal. In the homing cycle, each programmed axis is moved at the homing velocity that has been entered in the axis parameters.
Motion Commands, Dimension Inputs 3-27 NC Programming 17VRS Notes on feed to positive stop • If a feed value is not programmed in the G75 NC-block, traversing is performed at the speed entered in the axis parameter ‘Max. Feed to Positive Stop’. • If the programmed final axis position value is reached, the error message: „Positive Stop not within programmed move (@-axis)” is issued.
3-28 Motion Commands, Dimension Inputs NC Programming 17VRS Cancel All Feeds to Positive Stop 'G76' The preparatory command G76 cancel all axes at positive stop causes the pre-loads on all pre-loaded axes to be canceled. The actual position value is used as the position command value so that the axis positions can be used as reference positions for further traverse moves. The distance-to-go is ignored. Syntax Notes on programming G76 G76 • G76 is active only for the NC-block in which it is located.
Motion Commands, Dimension Inputs 3-29 NC Programming 17VRS X X Start position Start position Z Z movement movement NC-block end position NC-block end position NC-block start position Target position = interrupt position Fig. 3-22: Repositioning in the program operating modes Target position = NC-block start position Interrupt position Fig.
3-30 Motion Commands, Dimension Inputs NC Programming 17VRS X Starting Position Z Max. Traverse Range for NC-block restart Max. Traverse Range for NC-block restart NC-block End Position NC-block Start Position Point of Interruption Fig.
Motion Blocks 4-1 NC Programming 17VRS 4 Motion Blocks 4.1 Axes Linear Main Axes The linear main axes span a Cartesian coordinate system. They are identified by means of axis names: • 1st linear main axis (symbol: X) • 2nd linear main axis (symbol: Y) • 3rd linear main axis (symbol: Z) The axis name (address of the axis as it is to be addressed in the NCprogram) is freely configurable; however, the meaning of the axis is defined by the position of the axis in the coordinate system (see Fig. 4-1).
4-2 Motion Blocks NC Programming 17VRS Ordinate 2nd Axis [Y] [B] G18 Plane ZX G19 Abscissa G17 Plane YZ 1st Axis [X] [A] Plane XY [C] Z Coord. 3rd Axis [Z] Fig. 4-1: Linear main axes (X, Y, Z) and rotary main axes (A, B, C) in a reference coordinate system Linear and Rotary Auxiliary Axes Linear and rotary auxiliary axes can occupy any given position in space. • 1st auxiliary axis (symbol: U) • 2nd auxiliary axis (symbol: V) • 3rd auxiliary axis (symbol: W) identify this type of axis.
Motion Blocks 4-3 NC Programming 17VRS Examples Circle Diameter 160 mm Machining Speed = F8000 Gain Factor = 7 G06, G08 Oscilloscope Function Position Values Y Axis [mm] Position Difference: Position Command Value Expansion Factor: Axis Number : 2 Axis Type: Digital Linear Axis Axis Designation: Y Process: Master Axis Number : 1 Axis Type: Digital Linear Axis Axis Designation: Z Process: Master Position Values X Axis [mm] Fig.
4-4 Motion Blocks NC Programming 17VRS Machining Speed = F8000 Gain Factor = 7 G06, G08 Oscilloscope Function Position Value Axis Y Following error: Position Command Value: Expansion Factor: 1693.7 Position Values X Axis Circle Section Evaluation in Quadrant Transition Position Deviation Fig. 4-3: Circular interpolation with Minimized Following-Error Mode, partial view The next figure shows, by way of comparison, the same circle at a path feedrate of F1000 mm/min.
Motion Blocks 4-5 NC Programming 17VRS Surface Speed = F1000 mm/min Gain Factor = 7 G06, G08 Oscilloscope Function Position Values Y Axis [mm] Position Difference: Position Command Value: Elongation Factor: 2279.2 X Axis Section of Circle Position Deviation Evaluation in Quadrant Transition Fig.
4-6 Motion Blocks NC Programming 17VRS T11 BSR .M6 G00 G90 G54 G07 G08 X199 Y136 Z5 S5000 M03 G01 Z-5 F1000 G41 X199 Y141 F8000 [or. F1000] G03 X180 Y122 I199 J122 G01 X180 Y100 G02 X180 Y100 I100 J100 G01 X180 Y77 G03 X198 Y59 I198 J77 G00 Z5 T0 BSR .
Motion Blocks 4-7 NC Programming 17VRS Circle Diameter 160 mm Feedrate =F1000 Gain Factor = 7 G07 , G08 Oscilloscope Function Position Values Y Axis [mm] Position Difference: Position Command Value: Expansion Factor: 1680.9 Axis Number: 2 Axis Type: Dig. Linear Axis Axis Name: Y Process: Master Axis Number: 1 Axis Type: Dig. Linear Axis Axis Name: X Process: Master Position Values X Axis [mm] Fig.
4-8 Motion Blocks NC Programming 17VRS • • • • ration) is activated automatically. G08 cannot be programmed again until G61 has been canceled. The G08 function is active with feedrate overrides of 1%–100%. If the feedrate override is set for more than 100%, the velocity is reduced to 100% in the NC-block transitions. The M-functions stop NC-block execution until an acknowledgment is received; thus, G08 does not work in NC-blocks in which an M-function is programmed.
Motion Blocks 4-9 NC Programming 17VRS Block Transition from F8000 to Oscilloscope Function F7000 G06 and G08 Axis Number: 1 Axis Type: Dig. Linear Axis Axis Name: X Process: Master with 4 Axes Summed Signal Generation Feedrate Change Between the 2nd Section and the Third Section from F8000 to F7000 Actual Position Position Difference Feed Fig.
4-10 Motion Blocks NC Programming 17VRS The velocity diagram (Fig. 4-12) clearly shows how the velocity of the axis is reduced to almost 0 between the workpiece areas. The remaining velocity at which the transition to the next NC-block occurs is derived from the axis parameter Cxx.017 Maximum Feedrate Change w/o Ramp. Example of a program for the velocity diagrams shown in Figs.
Motion Blocks 4-11 NC Programming 17VRS Examples Test Contour: Transition from Straight Line -> Circle Not Tangential , Circle Circle Tangential Oscilloscope Function Position Values Y Axis [mm] Position Difference: Position Command Value: Expansion Factor: 613.8 Feed: F4000 G06 , G61 Gain = 7 Position Values X Axis [mm] Position Difference Transition St. Line -> Circle Transition Circle -> Circle Not Tangential Tangential in Transition St. Line -> Circle Fig.
4-12 Motion Blocks NC Programming 17VRS Block Transition with Lag Present 'G62' With interpolation condition G62 processing switches to the next NCblock as soon as the command values for all axes programmed in the NC-block that are issued by the interpolator have reached their programmed final values. The system does not wait until the actual values have reached their final position. Any lag (following error) which may be present is not reduced as the final position is approached.
Motion Blocks 4-13 NC Programming 17VRS Diagram : Transition Straight Line -> Circle Not Tangential , Circle -> Circle Tangential Oscilloscope Function 4.0000 Axis Number: 1 Axis Name: X Axis Number: 2 Axis Name: Y Feed Summed Signal Generation Feedrate F4000 Actual Position G06 , G62 Gain = 7 Actual Position Transition St. Line -> Circle Not Tangential Transition Circle -> Circle Tangential Fig.
4-14 Motion Blocks NC-program NC Programming 17VRS G00 G54 G90 G61 G06 X200 G01 X150 F8000 ACC 40 X50 ACC 15 X-50 RET Starting point 1st straight line 2nd straight line acceleration factor 40% 3rd straight line acceleration factor 15% Return to program beginning The process parameter for maximum acceleration was set to 500 mm/sec^2 for the velocity diagram shown here.
Motion Blocks 4-15 NC Programming 17VRS Example G00 G54 G90 X40 Y40 X120 Y60 F8000 [P1] rapid traverse at maximum path velocity [P2] rapid traverse with F-word Y 60 P2 40 P1 20 20 40 60 80 100 120 X 140 Fig. 4-19: Linear interpolation, rapid traverse G00 Linear Interpolation, Feedrate 'G01' The axes programmed using the preparatory code G01 are traversed to their programmed coordinate value on a straight line relative to the current coordinate system using the current feedrate.
4-16 Motion Blocks NC Programming 17VRS G00 G90 G54 G06 G08 X0 Y0 Z10 S3000 M03 G01 X26.26 Y18 Z5 F2000 Z-5 Y80 F1200 X41 Y93.
Motion Blocks 4-17 NC Programming 17VRS Ordinate 2nd Axis[Y] ZX Plane G03 G02 G18 G02 G03 G03 G19 G17 G02 XYPlane Abscissa 1st Axis [X] YZ Plane 3rd Axis [Z] Fig. 4-22: Circular programming according to planes The radius and the starting angle of the arc is calculated from the starting point and the center point. Any radius which is determined based on the end point and the center point and is different is ignored. This means that the end point can only be used to calculate the final angle.
4-18 Motion Blocks NC Programming 17VRS Y Starting Point Center Point End Point +I (G90) -J (G91) -I (G91) +J (G90) X Fig. 4-23: Circular interpolation with interpolation parameters Example Full circle in the X-Y plane with G90 Y 100 80 I=60 60 CP 40 [P1] J=60 20 20 40 60 80 100 120 140 X Fig. 4-24: Full circle with G90 G00 G90 G54 G06 G08 X0 Y0 Z10 S3000 M03 G01 X40 Y37.24 F2000 Z-10 F500 G02 X40 Y37.
Motion Blocks 4-19 NC Programming 17VRS Example Full circle in the X-Y plane with G91 Y I=20 100 80 60 CP J=22.76 40 [P1] 20 20 40 60 80 100 120 140 X Fig. 4-25: Full circle with G91 G00 G90 G54 G06 G08 X0 Y0 Z10 S3000 M03 G91 G01 X40 Y37.24 F2000 Z-20 F500 G02 X0 Y0 I20 J22.76 Alternatively: G02 I20 J22.76 G00 G90 Z10 M05 X0 Y0 RET Example Motion commands, interpolation conditions Starting position, spindle ON Circle starting point with incr.
4-20 Motion Blocks NC Programming 17VRS Example of Programming Using Absolute Dimension Input (G90) G00 G90 G54 G06 G08 Motion commands, interpolation conditions M03 S2000 Spindle ON X34.5 Z136.5 [P1] Starting position G01 X40 Z128.
Motion Blocks 4-21 NC Programming 17VRS As can be seen from the above example, two possibilities would result for this programmed circle. Selecting the sign (R+30 or R-30) determines which circle is traversed. • The direction of motion relative to the circle end point is determined by G02 or G03. • Circle radius programming is not permissible with a traverse angle of 0° or 360°. The axes will remain at their starting points.
4-22 Motion Blocks NC Programming 17VRS Helical Interpolation Helical interpolation is a combination of circular and linear interpolation which is used to produce a spiraling tool path. The circular interpolation takes place in the selected plane (G17, G18, G19) while linear interpolation is simultaneously occurring in a third axis which is perpendicular to the plane of circular interpolation. Z -50 25 50 Y 50 X Fig.
Motion Blocks 4-23 NC Programming 17VRS Example of Programming Using Absolute Dimension Input (G90) G00 G90 G54 G06 G08 X0 Y0 Z10 S5000 M03 G01 X40 Y20 Z5 F2000 Z-2.5 X40 Y30 G02 X85 Y30 I62.
4-24 Motion Blocks NC Programming 17VRS Thread Cutting 'G33' The G33 function thread cutting can be used to cut • single or multiple point longitudinal threads, • face threads and • taper threads with a constant lead. Lead 1 Thread Longitudinal Thread Fig. 4-32: Longitudinal threads Syntax G33 The thread length is the difference between the starting point and the end point that is programmed in the G33 NC-block.
Motion Blocks 4-25 NC Programming 17VRS • If the thread is cut using positioning with minimized lag G06, the spindle speed can be changed during thread cutting by using the spindle override. The feedrate will adjust accordingly. The feedrate override will not be active. • The immediate stop (emergency off, stop in setup mode), the spindle speed and the feedrate are reduced in synch with one another and are increased in synch following a restart.
4-26 Motion Blocks NC Programming 17VRS NC-program G00 G54 G90 G06 G08 X80 Z130 S2000 M03 G01 X45.5 F1500 G33 Z30 K3 P180 G00 X80 Z130 G01 X43.5 F1500 G33 Z30 K3 P180 G00 X80 M05 RET Example [P1] Starting conditions [P2] infeed for first cut [P3] 1st thread pass [P4] Withdraw X axis [P1] Starting point [P5] Infeed for 2nd cut [P6] Second thread pass [P4] Withdraw X axis Spindle OFF Return to start of prog.
Motion Blocks 4-27 NC Programming 17VRS Calculation of the thread starting point and end point coordinates for the X axis: P5 = 47.5 - 3 = 44.5 P5 = 44.5 - 2 ∗ ( 10 ∗ TAN17 ° ) = 38.39 P6 = 38.39 + ( 105 ∗ TAN17 ° ) = 70.49 P2 = 47.5 - 1.5 = 46 P2 = 46 - 2 ∗ ( 10 ∗ TAN17 ° ) = 39.89 P3 = 39.89 + ( 105 ∗ TAN17 ° ) = 71.99 Example NC-program for face thread X 100 80 [P6] [P3] [P4] 60 40 [P1] [P5][P2] 20 20 40 60 80 100 120 140 Z Fig.
4-28 Motion Blocks NC Programming 17VRS Sequences of Thread-Cutting NC Blocks Using 'G33' The G33 function can be used to program consecutive chains of threadcutting NC-blocks containing different leads. A thread sequence can consist of • single- or multiple-thread longitudinal threads, • face threads, or • taper threads in any desired order, provided that the lead during each section of the thread remains constant. Longitudinal Lead 1 Thread 2nd Section 1st Section Fig.
Motion Blocks 4-29 NC Programming 17VRS Example NC-program for thread-cutting sequences X 100 80 [P6] 60 [P1] [P5] [P4] 40 [P9] [P10] [P3] 20 [P2] [P7] [P8] 3rd Section 20 40 1st Section 2nd Section 60 80 100 120 140 Z Fig.
4-30 Motion Blocks NC Programming 17VRS Rigid Tapping 'G63' / 'G64' Threads can be tapped without a compensating chuck using the function G63. With thread tapping without compensating chuck the spindle alignment is controlled and not, as would be the case in normal tapping, the spindle rpm. The spindle motion and the infeed motion of the axis which is programmed together with G63 are interpreted linearly. A positionable main spindle is needed for tapping without compensating chuck.
Motion Blocks 4-31 NC Programming 17VRS • The lead factor feed per spindle revolution must be programmed in a single NC-block containing G63 and G64 by using the F-word. • Depending on the parameter setting, the thread lead can be entered using 3 or 4 places to the left of the decimal point and, correspondingly 5 or 4 places to the right of the decimal point.
4-32 Motion Blocks NC Programming 17VRS Spindle already stopped at the beginning of the G63 NC-block Spindle stopped when motion is terminated G00 G54 G90 G06 G08 X0 Y0 Z10 Motion commands, interpolation conditions G01 X40 Y50 F2000 M03 S1000 [P1] 1st tapping position, spindle ON BSR .GEBO Branch to tapping subroutine Y80 M03 S1000 [P2] 2nd tapping pos., spindle ON BSR .GEBO Branch to tapping subroutine X90 M03 S1000 [P3] 3rd tapping position, spindle ON BSR .
Motion Blocks 4-33 NC Programming 17VRS NC-program using G63 and G64: Spindle stopped at the beginning of the G63 NC-block Spindle continues to turn after end of motion G00 G54 G90 G06 G08 X0 Y0 Z10 Motion commands, interpolation conditions G01 X40 Y50 F2000 [P1] 1st tapping position BSR .GEBO Branch to tapping subroutine X55 Y80 [P2] 2nd tapping position BSR .GEBO Branch to tapping subroutine X75 [P3] 3rd tapping position BSR .GEBO Branch to tapping subroutine X90 Y50 [P4] 4th tapping position BSR .
4-34 Motion Blocks NC Programming 17VRS A positionable main spindle is needed for the G65 tapping function. • The main spindle must be stopped using M05 before activating G65 tapping. • When G65 is active, it is not possible to traverse using G00; no circular and helical interpolation G02/G03 is performed, and no axis referencing G74 is performed. Feed functions relating to the NC-block transition (G08, G09, G61, G62) are suppressed. • No axis moves can be programmed in a G65 NC-block.
Motion Blocks 4-35 NC Programming 17VRS NC-program using G65: G00 G54 G90 G06 G08 X0 Y0 Z10 G01 X40 Y50 F2000 BSR .GEBO X55 Y80 BSR .GEBO X75 BSR .GEBO X90 Y50 BSR .GEBO M05 G00 X0 Y0 RET .GEBO M05 G65 F2 S500 M03 Z-7.
4-36 Motion Blocks 4.4 NC Programming 17VRS Feed F Word The feedrate in an NC-program is expressed by a feed which uses the address letters F and a feedrate which is stated directly as a constant or by means on an expression. The programmed feedrate determines the processing speed for each type of interpolation. The feedrate is restricted so that the limits entered in the parameters are not exceeded. If the F-word is programmed in conjunction with a preparatory function, the meaning can change.
Motion Blocks 4-37 NC Programming 17VRS Input Feedrate as Inverse Time Value 'G93' The machining time for a programmed workpiece can be defined by the function G93 input feedrate as inverse time value. The machining time is determined via the F-word. With the specified machining time, the controller calculates the required path velocity depending on the limit values. G93 F
4-38 Motion Blocks NC Programming 17VRS Input Feedrate in mm or inch per Minute 'G94' The programmed F-value is interpreted as the feedrate per min with the function G94 Input feedrate in mm/inch per min. G94 input feedrate in mm/min is the power-on state if set in the process parameters and G71 is active. The input feedrate is inch/min if G70 is active. The feed distance is programmed for linear axes in the active unit (mm/inch).
Motion Blocks 4-39 NC Programming 17VRS Time-Based Dwell 'G04' The G04 function can be used to program a delay time in the NC-program for functions such as relief cutting, machine control functions, etc. Syntax G04 F
4-40 Motion Blocks NC Programming 17VRS Basic Connections Between Programmed Path Velocity (F) and Axis Velocities Under interpolation conditions, the CNC computes the path velocity as follows: Path velocity equation F= ( ) + (B ∗ R ) + (C ∗ R ) X 2 + Y 2 + Z 2 + A ∗ R X Example 2 2 Y 2 Z Path velocity for thread cutting Lead P Z = V Z C = V C VB = F Fig.
Motion Blocks 4-41 NC Programming 17VRS Effect: F = VZ C = V C VB Fig. 4-43: Feed rate (F) without RZ Here, the C axis is interpolated simultaneously. With RZ The CNC interprets the F value as the resulting path velocity. NC program: G01 Z... C... RZ... F... Computation: ( F = Z 2 + C ∗ RZ mit und ) 2 Z = P∗ nW C ∗ RZ = 2π ∗ RZ ∗ nW ⇒F= P 2 + (2π ∗ RZ ) ∗ nW 2 Effect: Z = V Z C = V C F = VB Fig.
4-42 Motion Blocks 4.5 NC Programming 17VRS Spindle Speed S-Word for the Spindle RPM Statement The spindle RPM in an NC-program is expressed by a speed word which uses the address letters S and an rpm speed which is stated directly as a constant or by means on an expression. A spindle code can also be added to the speed word if a number of spindles are present. The spindle speed is restricted so that the limits entered in the parameters are not exceeded.
Motion Blocks 4-43 NC Programming 17VRS • The spindle speed values are reset after the controller has been powered on, the program loaded into the controller, and after a BST, M02, M30, RET or Control-Reset. • If the spindle extension is left out when there is more than one spindle in the process, the spindle statement will apply to the first spindle (S/S1). • The spindle direction used in the main spindle is determined by the Mfunctions: M03 spindle clockwise and M04 spindle counterclockwise.
4-44 Motion Blocks NC Programming 17VRS Example spindle NC-program—longitudinal thread machining with the 2nd X 100 80 [P4] [P1] [P3] [P6] [P2] [P5] 60 40 20 20 40 60 80 100 120 140 Z Fig. 4-45: Thread cutting—longitudinal thread with the second spindle Thread lead: Thread depth: 3mm 4mm Thread depth per cut: NC program G00 G54 G90 G06 G08 X80 Z130 SPF 2 S2 2000 M203 G01 X45.5 F1500 G33 Z30 K3 P180 G00 X80 Z130 G01 X43.
Motion Blocks 4-45 NC Programming 17VRS • When the SUG is selected with G66, the corresponding spindle must contain a valid tool data record (tool codes 1, 2 and 3 [correction type ≥ 3]). An error message will be generated if this is not the case. • When the SUG is selected with G66, the corresponding length registers for the wheel diameter must be > 0. An error message will be generated if this is not the case.
4-46 Motion Blocks NC Programming 17VRS • In the power-on state, G96 always applies to the first spindle (S/S1). If G96 is to be applied to a different spindle, the desired spindle must be selected prior to the G96 NC-block by using the SPF command. • Depending on the settings in the process parameter Bxx.041 (Spindle Speed Programming Default), G96 may be the power-on default. G96 constant surface speed (CSS) remains modally active until it is canceled by G97.
Motion Blocks 4-47 NC Programming 17VRS Upper Spindle Speed Limit 'G92' The G92 function can be used to set an upper spindle speed limit when G96 is active. When G96 is active, the surface speed is kept constant. This can lead to a spindle speed which theoretically is of infinite magnitude in the case of face turning or cutting down to the center of rotation.
4-48 Motion Blocks NC Programming 17VRS • The effective distances RX, RY and RZ give the absolute distance to the respective linear main axis. They therefore must not be programmed using a sign in the NC-program. • Effective distances having an absolute value of 0 are not programmed. • The programming of the effective distances in the NC-program is active for a single NC-block and must be programmed in the NC-block in which it is to be active.
Motion Blocks 4-49 NC Programming 17VRS NC-program Changeover Between Spindle and C Axis The changeover between C axis mode and main spindle mode is performed in terms of the NC syntax by programming the C-axis (Cxxx.xxx) or the main spindle (M03 Sxxxx). If the C-axis is programmed in the following NC-block when the main spindle mode is active, the CNC performs the changeover with the help of the SPS. NC-block preparation and NC-block processing are stopped until the changeover operation is completed.
4-50 Motion Blocks Shortest way NC Programming 17VRS In the modulo calculation „shortest distance“, G36, the command position is approached via the shortest way. G90 G36 actual position = 20° : : command position = -380° G1 C-380 F1000 : Fig. 4-48: Positioning using Modulo calculation „shortest way“(G36) • G36 is the power-on state; it may be de-selected by G37 or G38. • The power-on state G36 is restored at the end of the program (BST, RET, JMP, M02, M30).
Motion Blocks 4-51 NC Programming 17VRS 4.7 Coordinate Transformation Coordinate transformation is available for: • Face machining, and • lateral cylinder surface machining Lateral cylinder surface machining Face machining Fig. 4-51: Lateral cylinder surface and face machining The commands G30 (de-selecting coordinate transformation), G31 (face coordinate transformation), and G32 (lateral cylinder surface coordinate transformation) form the G code group „transformation functions“ (no. 17).
4-52 Motion Blocks NC Programming 17VRS • The reference spindle for feed programming with floating tapping (G63, G64, G65) must be set using the SPF command. • In the power-on state, the coordinate transformation always applies to the first spindle. If the transformation is to be applied to a different spindle, the desired spindle must be selected prior to coordinate transformation by using the SPC command.
Motion Blocks 4-53 NC Programming 17VRS Example NC program - face machining X1 [P1] 70 [P8] 60 50 40 30 [P2] [P7] 20 10 Y1 70 60 50 40 30 20 10 [P6] [P3] [P4] [P5] Fig. 4-52: Face machining with coordinate transformation NC program DOK-MTC200-NC**PRO*V17-ANW1-EN-P T12 M6 M89 S2 3500 M203 G00 G17 G54 G48 Z100 X140 C0 G31 G54 G90 G06 G08 G48 G00 G42 G94 X1 60 Y1 20 G01 Z-0.
4-54 Motion Blocks NC Programming 17VRS Selection of Lateral Cylinder Surface Machining ‘G32’ With lateral cylinder surface machining G32, the CNC produces straight lines and circles on the lateral cylinder surface according to the G00, G01, G02 und G03 blocks that are specified in the NC program. The straight lines and circles on the lateral cylinder surface can be programmeed on the plane of the developed lateral cylinder surface that is spanned by a linear axis and a rotary axis.
Motion Blocks 4-55 NC Programming 17VRS Before lateral cylinder surface machining is activated, the activated machining plane must be spanned by at least one rotary axis. This is possible using G20, free plane selection. NOTE CAUTION Detailed description When lateral cylinder surface machining is activated or de-activated, the CNC de-activates all zero offsets and sets G53.
4-56 Motion Blocks NC Programming 17VRS De-Selection of Coordinate Transformation 'G30' The CNC employs the G30 function - de-selection of coordinate transformation - to de-select an existing coordinate transformation (G31, G32). When the coordinate transformation is de-selected (G30), the zero offsets (G53) are de-selected, and tool path correction and tool length correction are de-activated (G40, G47). G30 is the power-on state; it has a modal effect. G30 is canceled by G31 or G32.
Motion Blocks 4-57 NC Programming 17VRS 4.8 Main Spindle Synchronization Use of Main Spindle Synchronization Main spindle synchronization is primarily used on lathes to transfer parts, to recess parts, to machine shafts, for polygon turning, and for non-round turning. Functionality of Main Spindle Synchronization Up to 3 spindles can be operated in sync within a process on the CNC. One spindle is used as the master spindle, while the other two spindles are operated as synchronized spindles.
4-58 Motion Blocks NC Programming 17VRS • All spindles used in a main spindle synchronization must be controlled by the same APRB card. • No more than two synchronized spindles can belong to a synchronization group aside from the master spindle. • The master spindle must have a lower drive number than the synchronized spindles within the SERCOS drive loop. • A single spindle cannot be both a master and a synchronized spindle at the same time.
Motion Blocks 4-59 NC Programming 17VRS zation speed, the NC switches to position control and rotates the synchronized spindle to the set position within one revolution using the shortest direction. If the master spindle and the synchronized spindle are stopped, the synchronized spindle simply traverses to its command position taking the existing translation ratio and the existing angular offset and position offset into account.
4-60 Motion Blocks NC Programming 17VRS Machine Data for Main Spindle Synchronization The machine data for the main spindle synchronization occupy a page 50 named main spindle synchronization. The following data structure is present in the page for each process: No. Name Value Range Description 001 Synchron. Synch. spindle 1 ok 0/1 0: synchronized operation not OK 1: Synch. operation OK 002 Synchron. Synch. spindle 2 ok 0/1 0: synchronized operation not OK 1: Synch.
Motion Blocks 4-61 NC Programming 17VRS the SPS or from the user interface, an error message will be issued. If the user attempts to do this in the NC-program using the MTD command, an error message will be issued, and the NC will stop processing. Some exceptions are the data elements 005 angular offset and 006 position offset of synchronized spindles 1 and 2. The user can modify them at any time during synchronized operation, either from the SPS via the user interface or from the NC-program. 4.
4-62 Motion Blocks NC Programming 17VRS • The master and slave axes in an active synchronized axis group must not be present as master or slave axes in a different synchronized axis group. Steps in a Follower Operation A synchronized axis group can be activated during program-controlled operation from the NC-program by means of an auxiliary function. In manual mode, the user can activate synchronized operation by means of a machine control key or some other key.
Motion Blocks 4-63 NC Programming 17VRS mode and belong to a different primary process must be transferred to the respective process before the synchronized axis group is activated, and they must not be returned to the primary process until synchronized mode is canceled. • Feed to positive stop (G75) cannot be used with synchronized mode.
4-64 Motion Blocks NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Tool Corrections 5-1 NC Programming 17VRS 5 Tool Corrections 5.1 Data Structure Used with Tool Data In order to perform the automatic tool check of which tools are installed, the tool management system needs to use the setup-list-specific tool specification data and the tool-list-specific tool actual data.
5-2 Tool Corrections NC Programming 17VRS The following comparison of the setup list and the tool list illustrates how they are used. Setup List Active Tool List Purpose Brings together the specification data of all tools required for the machining work. Prepares and stores the actual data of all tools present in the physical tool storage. Contents Basic tool data Basic tool data Edge data Edge data Identification The individual tools are identified based on the tool number and the tool ID.
Tool Corrections 5-3 NC Programming 17VRS 5.2 Setup Lists Purpose of the Setup Lists The setup list is used to define the presence of all tools required for the machining operation as well as whether and how they can be used for the machining steps which are to be performed. The setup list is also used with the automatic tool check to ensure that the tools are available and ready to use.
5-4 Tool Corrections NC Programming 17VRS NAME Base tool data Tool ID Index address ID (tool name) Storage Location Tool number Index number Correction type Number of edges Tool status Location data free half-locations old location Storage of next tool Location of next tool Storage of prev. tool Location of prev. tool Units Time unit Length unit Technology data Tool code Representation type User data User data 1 . . .
Tool Corrections 5-5 NC Programming 17VRS Tool Identification Tool name (ID) The tool name, which consists of up to 28 characters of any type, is used to uniquely identify each tool used. It is displayed within the controller system, both on the user interface as well as on the SOT (Station Operator Terminal). Any tools which are used must be uniquely named so that they can be clearly identified. Tools which can replace on another (spare tools) are listed under a single tool name.
5-6 Tool Corrections NC Programming 17VRS Fig.
Tool Corrections 5-7 NC Programming 17VRS Number of edges Up to nine edge data sets can be assigned to each tool, even though the tool may not possess this many edges. In order to not waste memory, the maximum number of edges can be reduced to one edge per tool by setting the system parameter A00.54. The number of edges specified in the setup list must be met by the given tool before it can be used for the intended machining operation.
5-8 Tool Corrections NC Programming 17VRS Fig.
Tool Corrections 5-9 NC Programming 17VRS Tool life data Maximum tool life The maximum tool life is the machining time in • minutes or • cycles which the tool can be used for to perform material-removal work from initial use until it becomes unusable under similar cutting conditions and for a given tool/material combination. • Entering a value of 0 as the maximum tool life turns off tool life monitoring for the given tool. Beginning with Version 4.
5-10 Tool Corrections Length wear factors (L1, L2 and L3) NC Programming 17VRS Length wear compensation is activated when tool length correction is activated via G48 or G49. The compensation value used to adjust for tool length wear is calculated in the tool management system by multiplying the duration of tool machining time by the length wear factor.
Tool Corrections 5-11 NC Programming 17VRS 5.3 Tool Lists Purpose of the Tool List Tool lists are used exclusively to prepare and save tool data. They can be created, modified and saved with the aid of the PC user interface while machining is taking place. This allows the user to prepare tool storage configurations for upcoming work. In this way, the time to install new tools in the tool storage system can be kept to a minimum.
5-12 Tool Corrections NC Programming 17VRS NAME Base tool data Tool ID Index address ID (tool name) Storage Location Tool number Index number Correction type Number of edges Tool status Location data free half-locations old location Storage of next tool Location of next tool Storage of prev. tool Location of prev. tool Units Time unit Length unit Technology data Tool code Representation type User data User data 1 . . .
Tool Corrections 5-13 NC Programming 17VRS Tool Identification Tool name (ID) The tool name (ID), which consists of up to 28 characters of any type, is used to uniquely identify each tool used. It is displayed within the controller system, both on the user interface as well as on the SOT (Station Operator Terminal). Any tools which are used must be uniquely named so that they can be clearly identified. Tools which can replace one another (spare tools) are listed under a single tool name (ID).
5-14 Tool Corrections NC Programming 17VRS Correction Type 1 (Drilling Tool) Correction Type 2 (Milling Tool) Correction Type 3 (Turning Tool) Correction Type 4 (Angle Attachment Tool) An Correction Type 1 tool has only 1 length correction (L3), and this correction is always perpendicular to the given machining plane.
Tool Corrections 5-15 NC Programming 17VRS Fig.
5-16 Tool Corrections NC Programming 17VRS Number of edges Up to nine edge data sets can be assigned to each tool, even though the tool may not possess this many edges. In order to not waste memory, the maximum number of edges can be reduced to one edge per tool by setting the appropriate parameter in the system parameters. The number of edges specified in the setup list must be met by the given tool in the tool storage system before it can be used for the intended machining operation.
Tool Corrections 5-17 NC Programming 17VRS Location data Free half locations Overly wide tools are identified by the datum free half locations: 0: This is a normal width tool which does not required any additional location beyond the actual location. 1: The tool overlaps an additional half location to the right and left of the actual location. 2: The tool overlaps two additional half locations to the right and left of the actual location.
5-18 Tool Corrections NC Programming 17VRS Fig.
Tool Corrections 5-19 NC Programming 17VRS Edge status The edge status bits provide information on the status of a given edge. The following table shows the edge status bits used in the tool list.
5-20 Tool Corrections Warning limit in percent NC Programming 17VRS The warning limit in percent defines the remaining tool life percent value at which the status warming „limit reached“ will be displayed. At the time of each update the tool management system checks the remaining tool life and sets the interface signal 'PxxS.MGWRN' for the SPS if the remaining tool life of a tool has reached the warning limit and if a useable spare tool is not present.
Tool Corrections 5-21 NC Programming 17VRS Length corrections (L1, L2, L3) The length corrections L1, L2, L3 of a tool edge are calculated as follows: Length corretions L1 = length L1 + wear L1 + offset L1 Length corretions L2 = length L2 + wear L2 + offset L2 Length corretions L3 = length L3 + wear L3 + offset L3 Length L3: 210.000 + Wear L3: -0.030 + Offset L3: 0.015 = Length corr.L3: 209.985 L3_min=2000mm Length correction L3=209.985mm L3_max=230mm Fig.
5-22 Tool Corrections NC Programming 17VRS Examples For tool measurement Z Determined correction values: 1) Not considering of radius Correction type 1 Edge orientation Lenth L3 0 162.13 Wear L3 Offset L3 0 0 1) Considering the radius Length L3 R Correction type 2 Edge orientation Lenth L3 Wear L3 0 162.13 0 Offset L3 Radius R 0 8 Wear R Offset R 0 0 Abb.
Tool Corrections 5-23 NC Programming 17VRS was being carried out (all moves with the exception of G00) as the machining time. However, if the tool wear factor is entered in mm/cycle or inch/cycle, the tool management system uses one cycle as the machining time. Thus, the compensation value for tool length corresponds to the tool wear factor. The tool management system automatically updates the machining time and, thus, the compensation value for length wear.
5-24 Tool Corrections 5.4 NC Programming 17VRS Tool Path Compensation Inactive Tool Path Compensation If no edge radius/cutter radius path compensation is active, the theoretical edge tip P is used as the reference point for the controller. The theoretical edge tip P will always move on the programmed contour in this case. However, this will lead to errors if the movements are not parallel to the axes.
Tool Corrections 5-25 NC Programming 17VRS Active Tool Path Compensation If edge radius / cutter radius path compensation is active (G41/G42), the CNC automatically calculates the length corrections which are active in the working plane with respect to the center point of the edge S by adding/subtracting the correct radius to/from the theoretical edge tip based on the current position of the cutting edge.
5-26 Tool Corrections NC Programming 17VRS Contour Transitions Inside corners With inside corners, the corrected NC-block transition point is based on the point at which the lines parallel to the contours intersect. R R S' S S' S R R S S' S' S R S S' theoretical edge tip edge center actual touch point Fig. 5-13: Inside corners Outside corners The tool center point must travel around outside corners so that they are not damaged. Two methods can be used to accomplish this: 1.
Tool Corrections 5-27 NC Programming 17VRS S2 ' S R S2 ' R S S1 ' S1 ' R S S2 ' R S2 ' S S1 ' S1 ' R S S1 ' S2 ' tool radius programmed NC-block transition point corrected NC-block transition point 1 corrected NC-block transition point 2 Fig.
5-28 Tool Corrections NC Programming 17VRS CAUTION With lookahead calculation of the corrected tool center point path, only the transition angle relative to the contour element of the following motion NC-block is used in the calculation and not the length of the contour element. The cases indicated in Fig. 5-16 are not recognized. S' S' S' S' S' S' S' S‘ Fig.
Tool Corrections 5-29 NC Programming 17VRS S' Fig. 5-18: Concave arc, several contour elements Since as a general rule no more than four NC-blocks can be prepared in advance, one of the next three NC-blocks must be a motion NC-block including at least a change of one axis coordinate in an axis which belongs to the selected working plane. If this is not the case, the contour move is considered to be completed, and the next contour transition will not be calculated.
5-30 Tool Corrections NC Programming 17VRS The establishment of tool path compensation requires an additional move in the working plane which is performed only in conjunction with a programmed linear movement. [Ps] Traversed Linear Movement [P1] Programmed Linear Movement R [Ps] [P0] [P1] R [P0] tool radius starting point of tool path compensation programmed starting point of the contour corrected starting point of the contour Fig.
Tool Corrections 5-31 NC Programming 17VRS [P2] [P3] Contour Violation [Ps1] R [P6] [P1], [P7] [P5] [P4] R [P0] [P1] tool radius programmed starting point of the contour corrected starting point of the contour Fig.
5-32 Tool Corrections NC Programming 17VRS Completed Linear Move [Pee] [Pe1] R [Pe0] R [Pee] [Pe0] [Pe1] Programmed Linear Move tool radius end point of tool path compensation programmed end point of the contour corrected end point of the contour Fig. 5-24: Removing tool path compensation Removing tool path compensation on an arc will not cause an error to be issued, but it will cause unpredictable contour errors.
Tool Corrections 5-33 NC Programming 17VRS Change in Direction of Compensation A change in direction of compensation functions as if it were the removal and then re-establishment of tool path compensation. [Ps0] Traversed Linear Move R [Ps1] [Pe0] Programmed Linear Move R [Pe1] R [Pe0] [Pe1] [Ps0] [Ps1] tool radius programmed end point of the first contour corrected end point of the first contour programmed starting point of the second contour corrected starting point of the second contour Fig.
5-34 Tool Corrections NC Programming 17VRS Tool Path Compensation, Left of Workpiece Contour 'G41' Tool path compensation, left of workpiece contour is activated by the G41 function command. When tool path compensation on the left of the contour is active, the tool center point moves on the left of the programmed contour when viewed in the direction of movement. It moves on a path which is parallel to the contour and which is offset from this contour by the tool radius value.
Tool Corrections 5-35 NC Programming 17VRS Example NC program - tool path compensation with G42 Y 100 80 60 40 20 20 40 60 80 100 120 140 160 180 X Fig. 5-28: Tool path compensation, right of contour (G42) NC program using G42 DOK-MTC200-NC**PRO*V17-ANW1-EN-P (TOOL CHANGE: IDENT=SF D5) T4 BSR .M6 G00 G54 G06 G08 X115 Y99.5 Z5 G01 Z2 F1000 S2000 M03 Z-10 F1200 G42 X117.5 Y99.5 F1500 G02 X98 Y80 I98 J99.
5-36 Tool Corrections NC Programming 17VRS Insert Contour Transition Arc 'G43' When tool path compensation is active (G41 or G42) G43 inserts an arc as the contour transition element for outside corners. The tool center point must travel around outside corners so that they are not damaged. An arc should always be inserted for circle ↔ straight line or circle ↔ circle contour transitions. • G43 is the power-on state. It is modally active until it is overwritten by a G44.
Tool Corrections 5-37 NC Programming 17VRS transition angle > 90° R R S R S S1 ' S2 ' S2 ' S1 ' = tool radius = programmed NC block transition point = corrected NCblock transition point 1 = corrected NC blocktransition point 2 transition angle < 90° S' S R S S' R = tool radius = programmed NC block point = corrected block transition point Fig.
5-38 Tool Corrections 5.6 NC Programming 17VRS Tool Length Compensation When movements are being performed in the direction of the tool axis and tool length compensation inactive is set, all position data relates to the position of the nose of the spindle. Z+ Programmed Z-value Fig.
Tool Corrections 5-39 NC Programming 17VRS Tool Length Correction, Cancel 'G47' The function G47 is used to cancel an already active tool length correction. When movements are being performed in the direction of the tool, all position data relates to the position of spindle nose. If an active tool length correction (G48 or G49) is canceled with G47, a programmed move in the direction of the existing main axes is expected.
5-40 Tool Corrections NC Programming 17VRS All data present in the tool list can be read. The individual data elements are addressed by means of codes. A detailed description of the TLD command is contained in Chapter 11 „NC Special Functions“. Value Range and Meaning of the Parameters Name Sym Value Range Process P 0..6 Addressing A 0 Storage S 0..2 S=0 : Magazine/turret S=1 : Spindle S=2 : Gripper Location L S=0 : 1..999 S=1 : 1..4 S=2 : 1..4 S=0 : Mag.-/turret loc.
Tool Corrections 5-41 NC Programming 17VRS How the D corrections work G18 G17 Y G19 Y Y R L2 L3 L1 R L3 L1 L2 L1 X L2 X L3 X R Z Z Z Fig. 5-33: How the D-corrections work in the process plane Geometry registers L1, L2 and L3 are not used for compensation unless tool length correction G48/G49 is active. Geometry register R is only used for compensation when tool path compensation G41/G42 is active.
5-42 Tool Corrections NC Programming 17VRS • D0 is active in the power-on state; thus, the D-corrections do not perform compensation. • A programmed D-correction is modally active. The programmed Dcorrection is canceled when D0 is programmed. D0 is automatically active after an NC-program is loaded and after a BST, RET, M02, M30, or Control-Reset.
Auxiliary Functions (S, M, Q) 6-1 NC Programming 17VRS 6 Auxiliary Functions (S, M, Q) 6.1 General Information Auxiliary functions are passed to the SPS and are then executed and acknowledged by the SPS. For this to happen, the switch functions needed in the SPS must be defined. • If an auxiliary function has been output to the SPS, block processing stops until the function is acknowledged.
6-2 Auxiliary Functions (S, M, Q) NC Programming 17VRS All M-functions with the exception of the spindle control commands Mx03, Mx04, Mx05, Mx13, Mx14, the program control commands Mx00, Mx01, Mx02, Mx30, and the block-active M-function Mx19 (x = 1...3) can be used as desired by the machine builder since they do not trigger any internal functions in the controller. • In a given NC-block, only one M-function can be programmed from each function group.
Auxiliary Functions (S, M, Q) 6-3 NC Programming 17VRS Mx14 Spindle in counterclockwise direction and coolant/lubricant ON Turn on spindle rotation in the counterclockwise direction and turn on coolant/lubricant supply if the required switching functions are defined in the SPS program. Spindle positioning The function M19 S... allows the main spindle to be stopped in a defined position.
6-4 Auxiliary Functions (S, M, Q) 6.3 NC Programming 17VRS S Word as Auxiliary Function If a process was defined without a spindle in the process parameters, the S-word has the meaning of an auxiliary function. This means that the user has an additional address letter which he can define for auxiliary functions in the SPS program. The S-function can be entered as an unsigned integer constant having up to 4 digits. The numerical range for this constant is 0 to 9999.
NC Events 7-1 NC Programming 17VRS 7 NC Events 7.1 Definition of NC Events Which can be used by the NC-program and which, like flags in the SPS program, represent any desired state defined by the programmer. NCevents can be set and reset as desired in the NC and SPS programs. Processes can be synchronized by waiting for a defined state in an NCevent. Up to 224 NC-events are available in the CNC. Thirty-two (32) local NCevents are allocated to each process.
7-2 NC Events NC Programming 17VRS Reset NC Event ‘RE’ The NC-event defined in the command parameter is reset using the command RE. If the NC-event is already reset, this command will be ignored. The NC-event continues to be reset until it is set by the SE set NCevent command, the SPS program or via the MUI/GUI/SOT interface tools. Syntax RE : RE
NC Events 7-3 NC Programming 17VRS Wait until NC Event Is Reset ‘WER’ The WER command wait until NC NC-event is reset is used in the process in which WER is programmed to stop program processing until the NC-event defined in the command parameter is reset. If the NC-event is already reset, the block continues to process without interruption. Syntax WER : WER
7-4 NC Events 7.3 NC Programming 17VRS Conditional Branches Upon NC Events Branch If NC Event Set ‘BES’ The BES command branch if NC-event set is used to continued program processing at the declared branch label if the NC-event defined in the command parameter is set. Syntax BES : BES Ö Ö BES .LABEL 1:15 BES .
NC Events 7-5 NC Programming 17VRS 7.4 Interrupting NC Events The CNC can use NC-events to influence the NC-program execution at any desired time. Since the status of NC-events can be changed by the SPS and by other processes, the NC-program can be made to branch conditional upon certain signal changes.
7-6 NC Events NC Programming 17VRS Branch on NC Event to NC Subroutine (Interrupt) ‘BEV’ The BEV command branch on NC NC-event to NC subroutine (interrupt) is used to activate monitoring of the NC-event specified in the command parameter. If the NC-event assumes the status "1", processing branches to the subroutine which is parameterized in the branch label of the BEV command. A change of the status of low-parity NC-events or of the triggering NC-event is ignored until the end of the subroutine.
NC Events 7-7 NC Programming 17VRS Cancel NC Event Supervision (Interrupt) ‘CEV’ The command CEV cancel NC-event supervision (interrupt) can be used to cancel NC-event supervision when NC-event supervision is activated by means of BEV or JEV. The NC-event supervision is canceled for the NC-event declared in the command parameter. Syntax Ö CEV
7-8 NC Events NC Programming 17VRS NC program ; normal processing CEV T1 BSR .M6 G00 G90 G54 G06 G08 X0 Y0 Z10 S3000 M03 • • • T0 BSR .M6 @50=0 O1 M52 G00 G90 G59 G06 G08 X32.5 Y65 G01 Z2 F500 M54 BEV .GEWB 6 G01 X97.5 F700 M55 M53 O0 RET .GEWB DEV M55 M53 @51=X-OTD(,,,,1) @52=Y-OTD(,,,,2) @53=Z-OTD(,,,,3) T15 BSR .M6 G90 G=54+@50 G06 G08 G01 X40 Y65 Z10 F2000 M03 S1000 G63 Z-7.5 F2 G63 Z10 F2 S1200 M04 T0 BSR .
Tool Management Commands 8-1 NC Programming 17VRS 8 Tool Management Commands 8.
8-2 Tool Management Commands NC Programming 17VRS Select Tool Spindle ‘SPT’ If several tool spindles are being used in a process, certain functions such as select edge E must be allowed to act on another tool spindle in addition to the first tool spindle. Syntax SPT The first tool spindle is always active in the power-on state. If the tool edge is to apply to a tool spindle other than the first tool spindle, the tool spindle must first be selected using SPT .
Tool Management Commands 8-3 NC Programming 17VRS 8.2 Tool Storage Motion Commands All tool storage unit motion is performed asynchronously relative to the motions on the other NC axes. The NC motion commands only initiate tool storage unit motion and do not wait until the tool storage unit has completed the motion. In the meantime, the NC-program—and thus the process—can be continued. A command can be used to scan signals to determine whether the motion which was initiated is finished.
8-4 Tool Management Commands NC Programming 17VRS Move Tool into Position ‘MTP’ The MTP command initiates a tool storage move which places the tool selected via the T-word in the NC-program in the specified position (change, installation or processing position). Syntax MTP MTP() MTP(,
Tool Management Commands 8-5 NC Programming 17VRS Move Location into Position ‘MMP’ The MMP command initiates a tool storage move which places the location selected via the T word in the specified position (change, installation or processing position). Syntax MMP MMP() MMP(,
8-6 Tool Management Commands NC Programming 17VRS Move Free Pocket into Position ‘MFP’ The MFP command initiates a tool storage motion to move the closest empty pocket to the specified position. Syntax MFP MFP() MFP(,
Tool Management Commands 8-7 NC Programming 17VRS If this command is used consistently, all tools will be returned to the pockets in which they were located before they were used in the machining process. This keeps the tool storage unit in an orderly condition. This is desirable, for example, when extra-wide tools always have to be stored in the same magazine pocket. • The CNC does not wait until the tool storage unit has completed its motion.
8-8 Tool Management Commands 8.3 NC Programming 17VRS Tool Change Commands The tool changer commands should only be used when a magazine is used as the tool storage unit and tools need to be moved between the magazine and the spindle (in some cases via grippers). Complete Tool Change ‘TCH’ The TCH command initiates a tool change between the spindle and the magazine pocket in the change position. Syntax TCH TCH() TCH(,
Tool Management Commands 8-9 NC Programming 17VRS • This command is needed for single-arm gripper systems or for gripperless tool changers if the change operation has to be divided into a pick and place sequence. Change Tool from Spindle to Magazine ‘TSM’ The TSM command initiates a tool transfer between the spindle and the magazine pocket in change position. Syntax TSM TSM() TSM(,
8-10 Tool Management Commands NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Commands for Controlling Processes and Programs 9-1 NC Programming 17VRS 9 Commands for Controlling Processes and Programs 9.1 Process Control Commands The multiple-process structure of the CNC makes it necessary to coordinate the individual processes used in the CNC. If more than two processes are present on the CNC, the process whose number is "0" is generally used for program coordination.
9-2 Commands for Controlling Processes and Programs NC Programming 17VRS A management process (process 0) must always be present. This process is responsible for synchronizing the existing processes and external mechanisms, assuming this is necessary. If the system consists of a single station, the coordination task and the axes are assigned directly to the management process.
NC Programming 17VRS Commands for Controlling Processes and Programs 9-3 Reverse Process ‘RP’ The "RP" command starts the subprogram which is addressed by the reverse vector in the declared process. Any active forward program which may be present is interrupted and the currently valid reverse vector addresses the branch-to location in the reverse program. Syntax RP Ö RP 4 RP Process[0..6] internal processes Process[7..
9-4 Commands for Controlling Processes and Programs NC Programming 17VRS Lock Process ‘LP’ The "LP" command specifies which processes must be in a defined state for the NC program to be completed. This state must remain intact until the NC program is completed. Syntax LP Ö LP 4 LP Process[0..6] internal processes Process[7..
Commands for Controlling Processes and Programs 9-5 NC Programming 17VRS Process Complete (Full Depth) ‘POK’ By programming the "POK" NC command (part O.K.), the NC programmer can determine from within the NC program when the process was completed. The "POK" command causes a signal to be sent to the SPS (process-specific).
9-6 Commands for Controlling Processes and Programs NC Programming 17VRS • The axis continues to be assigned to the primary process, even after the axis is transferred to a secondary process. Thus, axis error and their diagnostic messages are displayed in the primary process. • All axis belonging to a different primary process are freed (free) at the end of the program by "RET" or "BST" or by a control reset and by jogging axes in the setup mode; and all axes in a different process are requested (get).
Commands for Controlling Processes and Programs 9-7 NC Programming 17VRS Process 1 "B axis right" Process 2 "B axis left" .BEARB .BEARB FAX (B) WES 9 Label for the branch loop Free B axis Wait until B axis in P0 RE 9 GAX (B) Get B axis if freed in machining process BER .BEARB 10 Loop until machining is completed in P0 RE 10 RET FAX (B) WES 9 Label for the branch loop Free B axis Wait until B axis in P0 RE 9 GAX (B) Get B axis if freed in machining process BER .
9-8 Commands for Controlling Processes and Programs 9.3 NC Programming 17VRS Program Control Commands Return to NC program Begin ‘RET’ The "RET" command identifies the end of an NC program. The "RET" command acts like functions "M002"/"M030," however an auxiliary function is not passed on to the SPS. When the "RET" command is performed, processing branches to the first NC block in the active NC program, sets the preparatory functions for the power-on state, and waits for a start signal.
Commands for Controlling Processes and Programs 9-9 NC Programming 17VRS Branch Absolute ‘BRA’ The "BRA" command branches to the label set in the command parameter and continues program execution there. Syntax Ö BRA BRA .WEITER Jump to NC Program ‘JMP’ The "JMP" command jumps to the NC program number set in the command parameter and continues program execution in this new NC program in the first NC block. Syntax JMP
9-10 Commands for Controlling Processes and Programs NC Programming 17VRS Subroutine Organization A subroutine consist of the: • Beginning of the subroutine • NC blocks in the subroutine • Return from the subroutine (end) .LABEL Start of subroutine NC blocks NC blocks in subroutine RTS Return from subroutine Fig. 9-4: Subroutine structure In terms of syntax, the "jump label” begins with a decimal point followed by at least one and no more than six legal characters. The syntax is NOT case sensitive.
Commands for Controlling Processes and Programs 9-11 NC Programming 17VRS Branch to NC Subroutine ‘BSR’ The "BSR" command branches to the label set in the command parameter and continues program execution there. Syntax Ö BSR
9-12 Commands for Controlling Processes and Programs 9.5 NC Programming 17VRS Reverse Vectors The CNC permits flags to be defined for reverse programs based on various program states relating to certain machine positions. These withdrawal programs (reverse programs) are used to program how the NC axis must withdraw from the various positions and return to a defined state. The flags for the reverse programs, which are identified by labels, are referred to as "reverse vectors." The label ".
Commands for Controlling Processes and Programs 9-13 NC Programming 17VRS CAUTION All reverse vectors are cleared upon a control-reset. The branch label of the reverse program points to the basis reverse vector .HOME. The NC blocks that are defined by the reverse vectors (REV) are no longer processed. Merely the NC blocks of the base reverse vector .HOME are included. Example ; Tool changing program. N0000 .M6 ; install new tool? N0001 .M6_TOL @0:00=TLD(,0,1,1,0,5,) N0002 @0:00=@0:00-T BEQ .
9-14 Commands for Controlling Processes and Programs NC Programming 17VRS ; Reverse vectors for the tool changing program N0025 .RM6_6 Q3 Turn arm back N0026 .RM6_5 Q8 Retract gripper N0027 .RM6_4 SE 0:12 Transfer. G1 -> Mag. G0 -> Spindle N0028 TSM N0029 .RM6_3 Q6 Spindle clamp closed N0030 .RM6_2 Q5 Open gripper N0031 RTS N0032 .RM6_7 Q8 Retract gripper N0033 .RM6_8 Q6 Clamp closed N0034 .RM6_9 Q5 Open gripper N0035 .RM6_10 RE 0:12 N0036 TSM N0037 .RM6_12 BTE .
Commands for Controlling Processes and Programs 9-15 NC Programming 17VRS Branch If Tool T0 Selected ‘BTE’ The "BTE" command can be used to determine whether "T0" was last selected, in other words: whether the tool must be removed from the spindle without loading a new tool into the spindle. Syntax BTE Ö BTE .PRT0 If "T0" was programmed last, program execution continues at the branch label defined in the command parameter.
9-16 Commands for Controlling Processes and Programs 9.7 NC Programming 17VRS Conditional Branches Upon the Results of Arithmetic Operations "Branches which are conditional upon the results of arithmetic operations" relate to the results of the most recently performed arithmetic operation. Branch If Equal to Zero ‘BEQ’ The command "BEQ" is used to continue program execution at the specified label if the result of the most recent mathematical operation was equal to zero. Syntax BEQ
Commands for Controlling Processes and Programs 9-17 NC Programming 17VRS Example NC program @51=0 .NEXT @51=@51+1 @100=MTD(250,0,1,@51) @100=@100-25 BEQ .BREAK @100=@51-10 BMI .NEXT [no element of the machine data has a value of 25] M00 BRA .EXIT .BREAK [one element of the machine data has a value of 25] M00 .
9-18 Commands for Controlling Processes and Programs NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Variable Assignments and Arithmetic Functions 10-1 NC Programming 17VRS 10 Variable Assignments and Arithmetic Functions 10.1 Variables NC variables are used in an NC program to represent a numerical value. A value can be assigned to a NC variable by the NC program, PLC program or from the user interface, and the value of the NC variable can likewise be read by these programs or by the user interface.
10-2 Variable Assignments and Arithmetic Functions NC Programming 17VRS Reading/Writing NC Variable Data The values of the following addresses can be assigned to the CNC NC variables, or the following values from the CNC addresses can be written to the NC variables. Coordinate values of existing axes { XE „Variables:Variable assignments:Coordinate values of existing axes“ }The machine coordinates are read into the NC variable when the coordinate values are read.
Variable Assignments and Arithmetic Functions 10-3 NC Programming 17VRS RX=@116 DOK-MTC200-NC**PRO*V17-ANW1-EN-P Effective radius distance to the X axis via the contents of the NC variable.
10-4 Variable Assignments and Arithmetic Functions Zero offset table Auxiliary function NC Programming 17VRS Valid address: O O=@116 Select zero offset table via the contents of the NC variable. @117=O Read active zero offset table. The active auxiliary function "Q" cannot be read. Valid address: Q Q=@117 D correction Output the auxiliary Q function via the contents of the NC variable. The active D correction "D" cannot be read.
Variable Assignments and Arithmetic Functions 10-5 NC Programming 17VRS M functions The programmable M functions are subdivided into 16 M function groups. Legal address for reads: Legal address for writes: M-function M-function Group Active M(
10-6 Variable Assignments and Arithmetic Functions NC Programming 17VRS 10.2 Angle Unit for Trigonometric Functions ‘RAD’, ‘DEG’ The arguments of the trigonometric functions "SIN," "COS," "TAN" and the results of the inverse functions of the trigonometric functions "ASIN," "ACOS," "ATAN" can be stated or calculated in the unit "radians" as well as a fraction or multiple of the size of the unit circle (radius = 1) and as the unit "degrees.
Variable Assignments and Arithmetic Functions 10-7 NC Programming 17VRS Operands Operands can be: • Constants • System constants • NC variables • Address letters, and • Functions Constants Floating decimal point constants can be comprised of the following elements: • Sign of the mantissa • Up to 6 decimal places • Number of places to the left of the first through sixth decimal digit • Exponent symbol "E" • Sign of the exponent, and • Up to 2 decimal places for the exponent In order for the use of interna
10-8 Variable Assignments and Arithmetic Functions NC Programming 17VRS Operators The standard symbols for basic mathematical operations can be used as operators. + Addition − Subtraction ∗ Multiplication / Division % Remainder integer whole division (modulo) • Division by "0" will cause an error. • Higher-order operations are implemented by functions. Parentheses To nest expressions and circumvent the integrated point-before-line logic, partial expressions can be placed within parentheses.
Variable Assignments and Arithmetic Functions 10-9 NC Programming 17VRS Integer component - INT The "INT" function delivers the next smallest whole number for the operand. Example INT(1.99) INT(1.01) INT(-2.99) INT(-2.01) Square root - SQRT Ö Ö Ö Ö 1 1 -2 -2 The SQRT function produces the square root of its operand. Example Ö SQRT(2) 1.4142. The "SQRT functions" does not permit any negative operands.
10-10 Variable Assignments and Arithmetic Functions Inverse cosine - ACOS NC Programming 17VRS The operand for the ACOS function must be greater than or equal to -1 or less than or equal to +1. When the angle unit “radians” is set: Value range: -π/2 Õ ACOS(x) Õ +π/2 Example ACOS(0.5) Ö 1.047.. (π/3) When the angle unit "degrees" is set: Value range: -180 ACOS(x) +180 Õ Example ACOS(0.
Variable Assignments and Arithmetic Functions 10-11 NC Programming 17VRS Example @50=TIME • • • @60=TIME-@50 Determine active time Determine time difference The TIME function does not have an operand. Time recording starts when the controller is powered on and continues for about 50 days. Example NC program - subroutine programming Y @100=90 100 80 R=5 @102=5 60 @101=50 40 20 20 40 60 80 100 120 140 160 180 X Fig. 10-1: Rectangle as subroutine NC program T4 BSR .
Special NC Functions 11-1 NC Programming 17VRS 11 Special NC Functions 11.1 Position Values with Analog Drives The functions "PMP" and "NMP" supply the positive value of the axis which is declared to be the operand by means of the axis letters when there is a positive or negative edge at the measurement input AxxC.SRTBP.
11-2 Special NC Functions NC Programming 17VRS The meaning of the SERCOS parameters (group letter S) and their functions are described by the SERCOS committee in the publication "SERCOS Interface." The meaning of the SERCOS parameters (group letter P) and their functions are described in the documentation for the SERCOS digital drive. • The reading or writing of drive data using the "AXD command" should be programmed in a separate NC-block which does not contain any other NC-commands.
Special NC Functions 11-3 NC Programming 17VRS Oscilloscope Function Y Axis Position Values [mm] Position Deviation: Position Command Value: Expansion Factor: 1693.7 Axis Number: 2 Axis Type: Dig. Linear Axis Axis Name: Y Process: Master with Axis Number: 2 Axis Type: Dig. Linear Axis Axis Name: Y Process: Master with Circle Diameter: 160 Kreisdurchmesser 160 mm mm Position Value Axis X [mm] Fig.
11-4 Special NC Functions NC Programming 17VRS Electronic Axis Coupling and Table Interpolators Electronic axis coupling permits additional couplings to be established between axes.
Special NC Functions 11-5 NC Programming 17VRS Activating transformation in the reference program . HOME ... BRF .
11-6 Special NC Functions NC Programming 17VRS 11.3 Reading and Writing ZO Data to/from the NC Program ‘OTD’ The "OTD command" (Offset Table Data) can be used to read and write the data in the zero offset table and the zero offsets which have been activated in the NC program from the NC program. Syntax M P O V A OTD([1/2],[0..6],[0..9],[0..9],[1..
Special NC Functions 11-7 NC Programming 17VRS General requirements for the OTD command • An NC variable can be used as parameter instead of the constant. • A mathematical calculation cannot be used instead of a constant or an NC variable. • The optional parameters do not need to be set. • The commas used to separate the parameters must always be used. The zero offset values for "G50/G51," "G52" and the active zero offset value cannot be written using the OTD command.
11-8 Special NC Functions NC Programming 17VRS 11.4 Read/Write Tool Data from the NC Program ‘TLD’ The "TLD command" (tool data) can be used to read the tool data into the NC program and to write them from the NC program, however some restrictions apply to writing. Syntax P A TLD([0..6],[0], S/T [0..2] L/D E D S ,[1...999],[0..9],[1..35],[1..32]) TLD([0..6],[1],[1..9999999],[1...999],[0..9],[1..35],[1..32]) Status Data Element Edge Pocket / Index No. Storage [0..
Special NC Functions 11-9 NC Programming 17VRS Tool List Data for the TLD Command: NAME Basic tool data Tool Identification Index address Tool name (ID) Storage Location Tool number Tool index number Correction type Number of edges Tool status Location Data Unused locations Old location Stor. of next spare tool Loc. of next spare tool Stor. of prev. spare tool Loc. of prev. spare tool Units Time unit Length unit Technology data Tool code Representation type User data User data 1 . . .
11-10 Special NC Functions NC Programming 17VRS Tool Status Bits for the TLD Command: Group name Present Group information Symbol Written by Type Bit Val.
Special NC Functions 11-11 NC Programming 17VRS Edge status bits for the TLD command: Group name Group information Symbol Write access Edge orientation incorrect Edge orientation correct/incorrect o WZM EL 1 1 0 L1 incorrect L1 correct/incorrect 1 WZM EL 2 1 0 L2 incorrect L1 correct/incorrect 2 WZM EL 3 1 0 L3 incorrect L1 correct/incorrect 3 WZM EL 4 1 0 R incorrect R correct/incorrect r WZM EL 5 1 0 Type Bit Value Reserved for future enhancements (bits 6 - 8)
11-12 Special NC Functions General tests for the TLD command Tests during write operations for the TLD command NC Programming 17VRS The validity of the programmed parameter values cannot be tested until the command is executed, in other words: when the NC program is running. If one of the parameters is incorrect or illegal, the CNC performs an immediate stop and issues the following error message: Incorrect Parameter [no.
Special NC Functions 11-13 NC Programming 17VRS 11.5 Reading and Writing D Corrections from the NC Program ‘DCD’ The DCD command enables the D corrections to be read and written from the NC program. Syntax P S V DCD([0..6],[1..99],[1..4]) Value Storage Process Name Symbol Range Meaning Process P 0..6 The active process is addressed if a process number is not specified. Memory S 1..99 The active memory is addressed if the parameter is not specified Value W 1..
11-14 Special NC Functions NC Programming 17VRS 11.
Special NC Functions 11-15 NC Programming 17VRS Read and Write the Machine Data Element ‘MTD’ MTD command The MTD command (machine table data) can be used to read and write individual elements of the machine data from the NC program, provided that a write access is permitted for the given element. Syntax PG Dim1 Dim2 EL MTD([1..299],[-1000..+1000],[Element No. Dimension 2 Dimension 1 Page No. Name Symbol Range Meaning Page no. PG 1..299 001 .. 099 pages of controller machine data 100 ..
11-16 Special NC Functions NC Programming 17VRS Example @100=MTD(250,1,2,4) X=MTD(260,1,,5) @50=MTD(270,,3,6) @120=MTD(280,1,1,4)+4 MTD(250,1,2,4)=@100 MTD(260,1,,5)=X MTD(270,,3,6)=@110+@120 NOTE Read machine data element Page=250, L1=1, L2=2, EL=4 Move X axis to the position that is specified in the machine data element. L2 does not exist. L1 is of the PROCESS type. The elements of the active process are read. A specific process specification is possible. Utilization in a calculation.
Special NC Functions 11-17 NC Programming 17VRS Handling OTD Commands Possible allocations - Examples @100=OTD(,,,4,1) OTD(,,,4,1)=@110 OTD(,,,4,1)=@100+@110+@120 @100=OTD(,,,4,1)+OTD(,,,4,1) @100=OTD(,,,4,1)+OTD(,,,4,1)+OTD(,,,4,1) @100=OTD(,,,4,1) @110=OTD(,,,4,1) @120=OTD(,,,4,1) OTD(,,,4,1)=OTD(,,,5,1) OTD(,,,4,1)=OTD(,,,5,1)+OTD(,,,5,1) Illegal allocations - Examples OTD(,,,4,1)=@100 OTD(,,,5,1)=@110 OTD(,,,6,1)=@120 @100=(OTD(,,,4,1)+@110)+@120 CAUTION The OTD command can be used within an NC b
11-18 Special NC Functions NC Programming 17VRS The DCD command can be used within an NC block for reading any number of D corrections. However, only one D correction can be written to at any one time. CAUTION DCD commands in parentheses are not permitted.
NC Compiler Functions 12-1 NC Programming 17VRS 12 NC Compiler Functions 12.1 Basics NC compiler From software version 5.17 onwards, the NC compiler has been integrated into the user interface. It permits NC programs to be pre-compiled. Using these features, the following functions have been implemented: • Chamfers and roundings, • enhanced look-ahead function, • graphical NC editor (for contour and machining programming), • macro technique, and • modal function. 12.
12-2 NC Compiler Functions NC Programming 17VRS • Specifying the RD command tangentially inserts an arc of the radius RD between the preceding and the subsequent motion command. • The CF command has the following effect: Starting from the intersection point of the motion commands involved, the chamfer width CF is removed from both motion blocks; and the resulting co-ordinate values are interconnected by a linear path (G1).
NC Compiler Functions 12-3 NC Programming 17VRS Illegal commands Chamfers or roundings cannot be inserted between two motion blocks if one of the following functions is selected or de-selected: • Radius/diameter programming (G15, G16), • Changing planes (G17, G18, G19 and G20), • Transformation functions (G30, G31, G32), • Zero offsets and rotations (G50 through G59), • Dimension inch/mm (G70, G71), • Mirror function (G72, G73), • Homing axes (G74), • Travel to dead stop / canceling any axis pre-loading
12-4 NC Compiler Functions Examples NC Programming 17VRS 1. Changing tools : N0035 DEFINE M860 AS M86 M3 S10 Declutching while the spindle rotates slowly N0036 DEFINE M6 AS BSR .
NC Compiler Functions 12-5 NC Programming 17VRS Enhancing NC Functions by Macro Technique Using the macro technique enables the machine manufacturer to define customized NC functions that may be employed by the user in the NC program. Global macros can be created in the „NC programming“ („NC options“ submenu) menu item. They are valid in all NC programs and in MDI mode. Please refer to the „NC Compiler“ description for details.
12-6 NC Compiler Functions NC Programming 17VRS Intermediate position ( 80 / 50 ) X Retract position ( 80 / 75 ) Z Fig. 12-4: Retract motion with intermediate position : RETURN X80 Z50 : M30 ;Programming the intermediate position The following subroutine is entered in the cycle memory: .P_RT G0 X80 Z75 RTS ;Move to retract position cycle Note: Further DEFINE instructions and further subroutines may be defined. This enables fixed positions to be approached via an intermediate point.
NC Compiler Functions 12-7 NC Programming 17VRS Notes: • The instruction concerned is executed immediately in the NC blocks in which the user writes a modal instruction using MODF_ON. • The MODF_OFF instruction de-activates the modal instruction in the block in which it is programmed. • It must be noted that the modal function (such as MODF_ON(RD 2)) does not have an effect on blocks without axis movements (i.e. without feed axes).
12-8 NC Compiler Functions NC Programming 17VRS 2) Modal rounding and chamfering ∅X 180 RD RD 160 RD RD 140 RD RD 120 RD RD CF 100 CF 80 CF CF 60 CF CF 40 CF CF 20 CF Z 40 80 120 160 200 240 280 320 360 400 440 Fig. 12-6: Example: Modal rounding and chamfering N0000 (parts name : stairs) N0001 T3 BSR .
NC Compiler Functions 12-9 NC Programming 17VRS 12.5 Enhanced Look-Ahead Function Enhanced look-ahead function The enhanced look-ahead function optimizes the velocity curve of the programmed path movement during compilation and/or the program download. If required and without modifying the programmed contour, the look-ahead function inserts intermediate blocks in order to achieve a steadier path velocity curve.
12-10 NC Compiler Functions NC Programming 17VRS TL_RADIUS ;Specify tool radius Explanation: Using the TL_RADIUS[T no., E no.] command, the tool radii that are required for the enhanced look-ahead function may centrally be defined at the beginning of the program. The compiler employs the current T or E no. if a T no. or an E no. has not been specified. Example: : N0005 TL_RADIUS[1234567,1]=24.995 N0006 TL_RADIUS[923,3]=20.31 N0007 TL_RADIUS[9,9]=29.
NC Compiler Functions 12-11 NC Programming 17VRS Tool management Changing tools, including the related T call and the edge selection, must be performed prior to activating the enhanced look-ahead function or after it has been de-activated. Per cent acceleration correction In certain program sequences and, if applicable, depending on the tool or workpiece weight, the resulting path acceleration must be reduced.
12-12 NC Compiler Functions NC Programming 17VRS ;Grinding needles on the XY plane ;Grinding wheel radius: 2.50000 ;File name: TP1 ; N0000 (parts name: TP1) N0001 T2 BSR .M6 [SCHLEIFSCHEIBE D5] N0002 TL_RADIUS [ ] = ACD_COMP[@200] N0003 N0004 activate tool read current tool radius for compiler G0 G17 G40 G54 G71 G48 G8 G6 G98 X-0.19306 Y3.49431 S1 3000 M3 establish initial state @101=200 loop counter for number of oscillating strokes = 200 .PEN @100=@101-0 BEQ .
NC Compiler Functions 12-13 NC Programming 17VRS • WINDOW_01 (..., ..., . . .) ;Define window size for turning • WINDOW_02 (..., ..., . . .) ;Define window size for milling • CONT (..., ..., . . .) ;Definition of the initial part contour or of the final part contour : : END_CONT • FORM_20 (..., ..., . . .) ;recess - turning • FORM_50 (..., ..., . . .) ;straight elongated hole - milling • FORM_51 (..., ..., . . .) ;round elongated hole - milling • FORM_52 (..., ..., . . .
12-14 NC Compiler Functions NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
NC Programming Practices 13-1 NC Programming 17VRS 13 NC Programming Practices 13.1 Efficient NC Programming The following rules will help to ensure that the CNC operates at its maximum performance level. Note: What can be programmed in a NC block? Whatever can be programmed in a single NC block in terms of syntax should be in fact be programmed in a single NC block, provided it does not violate program flow logic. • Labels (e.g. .
13-2 NC Programming Practices NC Programming 17VRS Example NC program N0000 G00 N0001 S5000 N0002 M03 N0003 F10000 N0004 X100 Y50 Optimized for time, spindle starts after the move: N0000 G00 X100 Y50 F10000 S5000 M03 Optimized for time, spindle starts before the move: N0000 M03 S5000 N0001 G00 X100 Y50 F10000 The priority for processing an NC block in the NC memory is as follows: Block number Label N1234 .ENDE aux. fct.
NC Programming Practices 13-3 NC Programming 17VRS NC commands that stop NC block processing • Preparatory functions ∈ {G33, G50 ...
13-4 NC Programming Practices NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Appendix 14-1 NC Programming 17VRS 14 Appendix 14.
14-2 Appendix NC Programming 17VRS 14.
Appendix 14-3 NC Programming 17VRS 14.3 Table of Functions I. G00 through G20 Function G00 G01 G02 G03 G04 G06 G07 G08 G09 G15 G16 G17 G18 G19 G20 G Group 1 1 1 1 16 15 15 14 14 5 5 2 2 2 2 Meaning Description Page Lin. interpolation, rapid traverse * modal Syntax: G00 ; The programmed coordinates are traversed at maximum path velocity. 4-14 Lin. interpolation, rapid traverse * modal Syntax: G01 F value ; The programmed axes start and reach their end point together.
14-4 Appendix NC Programming 17VRS II. G30 through G49 Function G30 G31 G Group 17 17 G32 Meaning Description Page Coordinate transformation canceled * default, * modal Syntax: G30 ; G30 cancels an existing coordinate transformation. The fictive axes must not be programmed any more. 4-56 Coordinate transformation ON * modal Syntax: G31 ; The NC activates the G17 plane and the corresponding real axes become fictive axes.
Appendix 14-5 NC Programming 17VRS III. G50 through G73 Function G50 G51 G52 G53 G Group 16 16 4 4 G54 G59 4 G61 11 G62 G63 G64 G65 G66 11 16 16 7 8 Meaning Description Page Programmable absolute zero offset * block Syntax: G50 ; absolute offset of the machining zero point by the value programmed using G50 under the address letter for the axis.
14-6 Appendix NC Programming 17VRS IV. G74 through G99 Function G74 G75 G76 G77 G78 G79 G90 G91 G92 G93 G94 G95 G96 G97 G98 G99 G Group 16 16 16 16 19 19 6 6 16 16 7 7 8 8 12 12 Meaning Description Page Axis homing cycle * block Syntax: G74 ; G75 is possible with G90 or G91.
Appendix 14-7 NC Programming 17VRS V. ACC through BTE Function ACC AP AXD BEQ BER BES BEV BMI BNE BPL BRA BRF BSE BSR BST BTE G Group Meaning Description Page Programmable acceleration * modal Syntax: ACC ; The programmed constant (0 .. 100) limits the acceleration of all axes programmed in NC block ACC. 4-13 Advance program Syntax: AP ; The advance program which was selected using SP is started for the specified process.
14-8 Appendix NC Programming 17VRS VI. CEV through MOP Function CEV D DEG DEV DP E G Group Meaning Description Page Cancel NC event supervision (Interrupt) Syntax: CEV: ; CEV must be used to cancel the supervision (BEV, JEV) of a single interrupting NC event (0 .. 7). 7-7 D-correction selection * modal Syntax: D ; D1 .. D99 selects offsets defined in the D-correction table.
Appendix 14-9 NC Programming 17VRS VII. MRF through SE Function Meaning Description Page Tool storage to Reference Syntax: MRF ; Initiates the referencing sequence of the tool storage. 8-3 Tool Storage Ready ? Syntax: MRY ; Stops the NC program execution until the active tool storage movement is completed. Reading and writing the machine data elements Syntax: MTD([Page no.],[control variable 1], [control variable 2], [element no.
14-10 Appendix NC Programming 17VRS VIII. SP through WP Function SP SPC SPF SPT T TCH TLD TMS TSM WER WES WP G Group Meaning Description Page Select NC program for process Syntax: DP ; The defined NC program is selected (if no continuous selection in SPS) for the specified process. 9-2 Select main spindle for transformation * modal Syntax: SPC ; SPC selects main spindle for Transformation (G30, G31, G32).
Appendix 14-11 NC Programming 17VRS 14.4 Table of Preparatory G code Functions Legend * P S default default can be defined in process parameters NC block active I.
14-12 Appendix NC Programming 17VRS II.
Appendix 14-13 NC Programming 17VRS 14.5 File Header The editors that are available in the user interface are not the only means that may be used for creating an NC program. Any other external text editor may as well be used for that purpose. Data import The NC programs that are created with an external text editor must be provided with a file header. This enables them to be read in the corresponding file directories, using the „Data import“ function.
14-14 Appendix NC block numbers NC Programming 17VRS Several options may be selected in the main menu item 2 „Edit NC program“ of the user interface. With respect to the data import/data export function, you may define here whether or not NC block numbers will be output.
Index 15-1 NC Programming 17VRS 15 Index A ABS .................................................................................................................10-8 Absolute value function ....................................................................................10-8 ACC .................................................................................................................4-13 ACC_EFF......................................................................................................
15-2 Index NC Programming 17VRS Oblique axis ................................................................................................11-4 Virtual axis ..................................................................................................11-5 ASIN .................................................................................................................10-9 ATAN ..............................................................................................................
Index 15-3 NC Programming 17VRS BTE command..................................................................................................9-15 C Cartesian coordinate system .....................................................................3-1, 3-15 CEV ...................................................................................................................7-7 CF command ....................................................................................................12-2 Chamfers ......
15-4 Index NC Programming 17VRS DEG .................................................................................................................10-6 Delimiter character ...........................................................................................11-1 DEV ...................................................................................................................7-7 Diameter programming 'G16'............................................................................
Index 15-5 NC Programming 17VRS Input Feedrate in mm or inch per Minute 'G94'..............................................4-38 Programmed path velocity (F) .......................................................................4-40 for thread cutting.........................................................................................4-40 With RZ .................................................................................................4-41 Without RZ ............................................
15-6 Index NC Programming 17VRS G51 incremental ...............................................................................................3-12 G52 .................................................................................................................3-13 G53 .................................................................................................................3-14 G54 …G59 .........................................................................................................
Index 15-7 NC Programming 17VRS Acceleration 'ACC' .........................................................................................4-13 Block Transition with Lag Present 'G62' ........................................................4-12 Contouring Mode (Acceleration) 'G08' .............................................................4-7 Contouring Mode (Deceleration) 'G09'.............................................................
15-8 Index NC Programming 17VRS LP command ......................................................................................................9-4 M M function groups .............................................................................................14-2 M Functions ........................................................................................................6-1 M000...................................................................................................................
NC Programming 17VRS Index 15-9 Tangent - TAN ............................................................................................10-9 Time in seconds - TIME ............................................................................10-10 Operands .......................................................................................................10-7 Constants....................................................................................................10-7 Floating point constants.......
15-10 Index NC Programming 17VRS N NC block numbers .................................................... See Elements of an NC Block NC compiler......................................................................................................12-1 NC compiler functions ......................................................................................12-1 NC cycle programs .............................................................................................1-3 NC events......................
Index 15-11 NC Programming 17VRS Possible allocations between AXD, OTD, TLD, MTD, DCD............................11-16 Allocations between AXD, OTD, TLD, DCD and MTD commands ..............11-18 Illegal allocations ......................................................................................11-18 Possible allocations ..................................................................................11-18 Handling AXD commands.........................................................................
15-12 Index NC Programming 17VRS R RAD .................................................................................................................10-6 Radius programming 'G15' ...............................................................................3-19 RD command....................................................................................................12-2 RE ...................................................................................................................
Index 15-13 NC Programming 17VRS RTS command..................................................................................................9-11 RX .................................................................................................................4-47 RY .................................................................................................................4-47 RZ .................................................................................................................
15-14 Index NC Programming 17VRS Spindle speed in RPM 'G97' ...................................................... See Spindle speed Spindle stops at end of motion G63 .................................................................4-30 SPT .......................................................................................8-2 SQRT................................................................................................................
NC Programming 17VRS Index 15-15 wear registers .......................................................................................5-20 Location data ..............................................................................................5-17 Free half locations ................................................................................5-17 Old location...........................................................................................5-17 Tool identification.........................
15-16 Index NC Programming 17VRS Move location into position ‘MMP’....................................................................8-5 Move old pocket into position ‘MOP’................................................................8-6 Move tool into position ‘MTP’ ...........................................................................8-4 Tool storage enable for manual mode ‘MEN’ ..................................................8-7 Tool storage ready? ‘MRY’ ......................................
Index 15-17 NC Programming 17VRS Z Zero offsets.........................................................................................................3-6 Adjustable General Offset in the Zero Offset Table.......................................3-14 Adjustable Zero Offsets 'G54 ... G59' ..............................................................3-8 Cancel Zero Offsets 'G53'..............................................................................
15-18 Index NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
NC Programming 17VRS 16 Figures 16-1 Figures Fig. 1-1: CNC data organization .........................................................................1-2 Fig. 1-2: NC program package ...........................................................................1-4 Fig. 2-1:Setup Lists with station-specific organization........................................2-1 Fig. 2-2: Setup Lists with program-specific organization ....................................2-1 Fig. 2-3: NC program organization .................
16-2 Figures NC Programming 17VRS Fig. 4-28: Circle radius programming on lathe, behind center of rotation.........4-21 Fig. 4-29: Helical interpolation ..........................................................................4-22 Fig. 4-30: Helical interpolation with G90...........................................................4-22 Fig. 4-31: Helical interpolation with G91...........................................................4-23 Fig. 4-32: Longitudinal threads ....................................
NC Programming 17VRS Figures 16-3 Fig. 9-2: Axis transfer on a machining center having 2 machining tables ..........9-6 Fig. 9-3: Program organization in the CNC.........................................................9-9 Fig. 9-4: Subroutine structure ...........................................................................9-10 Fig. 9-5: Subroutine nesting .............................................................................9-10 Fig. 9-6: Branch to NC subroutine ................................
16-4 Figures NC Programming 17VRS DOK-MTC200-NC**PRO*V17-ANW1-EN-P
NC Programming 17VRS List of Customer Service Points List of Customer Service Points Germany Sales area Center Sales area East Sales area West Sales area North INDRAMAT GmbH D-97816 Lohr am Main Bgm.-Dr.-Nebel-Str.
List of Customer Service Points NC Programming 17VRS Outside Europe Argentina Argentina Australia Brazil Mannesmann Rexroth S.A.I.C. Division INDRAMAT Acassusso 48 41/7 1605 Munro (Buenos Aires) Argentina Nakase Asesoramiento Tecnico Diaz Velez 2929 1636 Olivos (Provincia de Buenos Aires) Argentina Argentina Australian Industrial Machenery Services Pty. Ltd. Unit 3/45 Horne ST Campbellfield VIC 2061 Australia Mannesmann Rexroth Automação Ltda.
NC Programming 17VRS Notes DOK-MTC200-NC**PRO*V17-ANW1-EN-P List of Customer Service Points
Indramat
