User's Guide. Servo CNC System. for Windows Programming and Operation. SW Version 5.0 Manual Version 1.1b. Form

Transcription

1 User's Guide Servo CNC System for Windows Programming and Operation SW Version 5.0 Manual Version 1.1b Form

2 Copyright 2006 ServoSource. All rights reserved The software contains proprietary information of ServoSource; it is provided under a license agreement containing restrictions on use and disclosure and is also protected by copyright law. Reverse engineering of the software is prohibited. Due to continued product development, this information may change without notice. The information and intellectual property contained herein is confidential between ServoSource and the customer and remains the exclusive property of ServoSource. If you find any problems in the documentation, please report them to us in writing. ServoSource does not warrant that this document is error-free. No part of this publication may be reproduced, stored in a retrieval system, or transmitted in any form or by any means, electronic, mechanical, photocopying, recording or otherwise without the prior written permission of ServoSource. Servo II is a registered trademark of ServoSource. Microsoft, Windows and Windows NT are registered trademarks of Microsoft Corporation. VenturCom's Real-time Extension (RTX) for Windows NT and for Windows XP Professional are distributed under a licensing agreement with VenturCom Inc, now Ardence, a Citrix Company. RTX is a registered trademark of VenturCom, Inc. Adobe and Acrobat Reader are either registered trademarks or trademarks of Adobe Systems Incorporated. Gibbs SFP, Virtual Gibbs, and GibbsCAM are registered trademarks of Gibbs and Associates. All other companies and product names may be trademarks or registered trademarks of their respective holders. This document was created using AuthorIT, Total Document Creation (See ServoSource 1224 Main Street Stockton, Kansas USA Document Assembly SW Phone: +1 (785) Fax: +1 (785) techsupport@servosource.com Web:

3 1 Introduction Typographical Conventions Before you start using this guide, it is important to understand the terms and typographical conventions used in the documentation. For more information on specialized terms used in the documentation, see the Glossary at the end of this document. The following kinds of formatting in the text identify special information. Formatting convention Triangular Bullet( ) Special Bold Emphasis CAPITALS KEY+KEY KEY KEY MENU OPTIONS Type of Information Step-by-step procedures. You can follow these instructions to complete a specific task. Items you must select, such as command buttons or items in a list. Also used for variables. Used to emphasize the importance of a point and for field names in status displays. Names of keys on the keyboard and pendant, for example, CTRL, ALT, F11, or MANUAL. Key combinations for which the user must press and hold down one key, then press another, and then release both, for example, ALT+F4, or MANUAL+SET. Key combinations on the pendant for which the user must press and release the first key and then press and release the second key, for example, RAPID SET. Menu choices required to initiate an action or procedure. WARNING A warning alerts you to a situation or action that could result in personal injury. CAUTION A caution provides information about a situation or action that could damage the Servo System or result in lost work or time.

4 2 Servo CNC System User's Guide NOTE A note presents information that is important enough to require emphasis. TIP A tip provides suggestions and pointers on techniques, usage, and "good practices" based on the experiences of CNC and manufacturing experts. Contacting Servo Products Company We hope the answers to all your questions are in the Servo CNC System for Windows NT User's Guide and Help System or the Servo CNC System: Installation, Operation and Maintenance manual for your machine. If your problem is not listed or the suggested solutions do not clear the problem, contact your dealer or Servo Products Technical Support. Servo Products Company Technical Support 433 North Fair Oaks Avenue Pasadena CA USA Phone: or Fax: info@servoproductsco.com Web: NOTE If you are having a programming problem, be prepared to , mail or fax the cnc file, a sketch of the geometry you are trying to program, the servont.ini file and tool.ini file tool table listing. NOTE DO NOT return any item to Servo Products Company without first receiving a Return Authorization (RA) number from Servo Products Company. Include the RA#, company name, address, telephone number, name of contact, and reason for return. Package the item properly to avoid ADDITIONAL damage. See the appendix "Axis Motor Removal and Installation" in the machine manual for how to package a Servo II motor.

5 87 C HAPTER 6 Programming Manual part programming requires the programmer to describe the detailed operations that the machine is to perform using codes and numeric values that the machine control can understand. The part program directs the motion of the cutting tool around the workpiece to generate the desired geometric shape. The part programmer uses the part dimensions, cutting tool geometry, feed and speed calculations, and fixture design to create the instructions to cut the workpiece. Writing a CNC Program (page 71) lists steps to follow. In This Chapter File & Code Formats...87 Sequence Number (N word)...88 Axis Commands (XYZC IJK words)...89 Feed Rate Commands (DEF words)...95 Preparatory Functions (G Codes)...96 Canned Cycles Machine Functions (M Codes) Subroutines (P Cycle) Spindle Speed Commands (S word) Tool Select Commands (T word) Program Comments ( and! Block Delete Code / File & Code Formats Files must use ASCII character coding, which is automatic if you are using the Servo editor to create your programs. If you are using a different editor, word processor, or a CAD/CAM or other programming system, check the output for compatibility. Numerical Values Numerical values are read as integers, unless they contain a decimal point. For example, in G70 Inch mode, X2 is read as 2 inches. In G71 Metric mode, X2 is read as 2 millimeters. A word address without a value has an assumed value of zero, for example, Y is read as Y zero. Leading zeros are not required, except for P cycle labels. For example, G02 and M00 are the same as G2 and M0, but P02 defines subroutine 2; P2 causes an error.

6 88 Servo CNC System User's Guide Block Format - CNC Mode The program codes are in word address format, meaning that the letter in front of a number indicates how the control interprets the data. The letter may be upper or lower case (capital or small). Letters used to identify variables in canned cycles are described in the section on the canned cycle. The basic data format for CNC is as follows N5 G3 XYZCIJK-4.8 DEF4.2 T2 M3 P7 S4 Block Format - Pendant Mode The program codes are in word address format, meaning that the letter in front of a number indicates how the control interprets the data. The letter may be upper or lower case (capital or small). Pendant mode programs created on the PC/SOC have the following basic data format: N5 G2 XYZC-4.8 DF4.2 M3 P7 NOTE N words and comments are stripped out when the program is transferred to the pendant. See Codes valid for Pendant transfer (page 69). Sequence Number (N word) The N word is used as a sequence number for a block (line, command). The letter N is followed by one to five digits ( ). It is used to identify blocks of information. Sequence numbers are not required. They are useful when searching for information in a program or to keep track of what portion of a program is currently being run. In CNC Run and Verify, the most recent N word is displayed as Sequence # on the first line of the CNC Status tab. In Teach or Pendant modes, programs transferred from the pendant to the PC contain sequence numbers added by the system. In programs transferred to the pendant from the PC, any sequence numbers are stripped out.

7 Chapter 6 Programming 89 Axis Commands (XYZC IJK words) Cutter motion can be made along any of three axes, all of which are mutually perpendicular; that is, they are at exact right angles to each other. These axes of motion are identified by the letters X, Y, and Z. This is known as the Cartesian coordinate system. By common practice, the X, Y, Z and C words identify the following slide movements. Axis X Y Z C Slide Movement Table left and right Saddle forward and back Quill, knee, or column slide (head) up and down Rotary table clockwise and counterclockwise rotation The I, J and K words are used in circular interpolation to define the signed distance from the arc start point to the arc center along the X, Y and Z axes respectively. NOTE If you have a unique Servo II CNC System installation, you may be using these codes in a non-standard manner. For example, if you have both knee and quill, the quill should be C and the knee Z. Figure 4: Twodimensional Cartesian coordinate system. The Coordinate System Let's start with the two-dimensional Cartesian coordinate system. If you define the intersection of the two base lines as the origin (that is, zero for each value), the X values to the right of the origin are positive (indicated by a plus + sign), and X values to the left of the origin are negative (indicated by a minus - sign). Similarly, Y values above the origin are plus, and Y values below the origin are minus. All values falling in the upper right-hand quadrant are positive. In the lower right-hand quadrant, values of X are positive, whereas values of Y are negative, and so-on around the graph.

8 90 Servo CNC System User's Guide 3-D Coordinate System Figure 5: Threedimensional coordinate system. Now add the third, or Z, axis. The Z axis represents vertical tool motion. With a negative Z axis value, the quill moves down and/or the knee moves up (decrease the distance between the head and the table). With a positive Z axis value, the quill moves up and/or the knee moves down (increase the distance between the head and the table). The relationship of the three axes is shown in the figure. If you define the nearest lower left-hand corner of the solid as the origin, then all values of X, Y, and Z lying within the solid are positive. If you project each axis outside the solid as shown in the figure, you include negative values of X, Y, and Z. This follows the same concept as datum line dimensioning. This also allows you to establish an absolute zero reference or datum at any convenient place and then represent the dimensions with positive and negative numbers. On the milling machine, there are three degrees of the motion: table leftright, saddle in-out, and quill, knee or head up-down. These axes are respectively labeled X, Y, and Z. Although the tool remains stationary and the part moves, programs are written as though the tool itself had three degrees of freedom. For example, a move of the table to the right is labeled a negative (-) move, since the result is as though the tool were moving to the left. This may seem confusing at first, but writing the program as though the tool were moving simplifies matters, since the signs come out to be consistent with the part drawings. Positive and Negative Motion Defined On the milling machine, there are three degrees of the motion: table left-right, saddle in-out, and quill, knee or head up-down. Although the tool remains stationary and the part moves, programs are written as though the tool itself had three degrees of freedom. For example, a move of the table to the right is labeled a negative (-) move, since the result is as though the tool were moving to the left. This may seem confusing at first, but writing the program as though the tool were moving simplifies matters, since the signs come out to be consistent with the part drawings.

9 Chapter 6 Programming 91 Absolute & Incremental Each axis position is defined as either absolute G90 or incremental G91. The absolute position is based on the "datum" or zero origin of the program. The incremental position is based on the current position of the tool. An example of an absolute system would be mail delivery from the Post Office. Streets all have a "0" starting number that are east and west or north and south, the positive and negative of our system. Then each house has its own number. So each location has its own address. Incremental systems are prone to error. If one increment is missing or incorrect, all the others that follow are in the wrong location. Figure 6: Absolute and incremental coordinate positions. Example: Absolute & Incremental coordinate positions Absolute and incremental positions for Point 1 through Point 4 are listed below. Absolute All coordinate positions are written with respect to the datum. Pt1 X.5 Y.55 Pt 2 X1.5 Y.55 Pt 3 X2.5 Y.55 Pt 4 X3.5 Y.55

10 92 Servo CNC System User's Guide Incremental All coordinate positions are written with respect to the position at the start of the move - also called the current position. from Datum To Pt 1 X.5 Y.55 Pt 2 Pt 3 Pt 4 X1 X1 X1 to Datum X-3.5 Y-.55 Angles Angles in canned cycles and the G22 rotation command are measured in absolute decimal degrees. The absolute zero for an angle is at 3 o'clock. A negative value is clockwise from the 3 o'clock position. Figure 7: Angle conventions. Example: Converting to decimal degrees To convert from degrees/minutes/seconds to decimal degrees: Remember : 1 degree = 60' minutes = 3600" seconds So: 45 30' = 45.5 Problem: Convert to decimal degrees 62 45' 30" Solution: = 62 + (45/60) + (30/3600) = =

11 Chapter 6 Programming 93 Programming the Rotary Table Figure 8: Rotary table directions for positive pitch. In Pendant and CNC modes, the rotary table is programmed with a C code followed by the angular value in decimal degrees (page 92). The feed rate (page 95) uses a D code for degrees per minute. The rotary axis can be programmed in absolute or incremental modes. NOTE The examples given here are based on a Servo II with the rotary table mounted horizontally on the left end of the table. The C axis pitch in the machine configuration table is.25". Clockwise and counterclockwise are defined looking at the face of the turntable, with the Servo II motor to the left. NOTE You can change the direction of rotation of the rotary table. On the Configure menu, select Machine, and enter a negative pitch value for the C axis, for example, NOTE On the pendant, the left DIRECTION< key rotates the turntable CCW. The right DIRECTION> key rotates the turntable CW. NOTE The Run and Verify graphics do not support the C axis. All views reflect the XYZ axes only. TIP When you create a program using the rotary C axis, "dry run" the program on the machine to check that the positive and negative angular coordinates are indeed going in the expected direction. See the NOTES above. In absolute mode beginning at zero degrees, the command G90 C350 rotates the turntable 350 degrees clockwise. Again beginning at zero, the command G90 C-10

12 94 Servo CNC System User's Guide rotates the turntable 10 degrees counterclockwise to the absolute 350 degree position. In incremental mode, a negative value rotates the turntable counterclockwise and a positive value rotates the turntable clockwise. In incremental mode, the command G91 C40 rotates the turntable 40 degrees clockwise beginning from the current position. Commands of greater than 360 degrees are allowed. If you "wind-up" the rotary axis, that is, use values of greater than 360 degrees, the Position Register shows the number of turns. In a rapid move, the turntable goes directly to the commanded position without "unwinding". For example, if the table is at 380 degrees (Position shows 1T ), and you enter, G90 G00 C0 the turntable will rotate 20 degrees to zero at the rapid feed rate. Example: Converting linear feed to rotary feed The formula for converting a linear feed rate to a rotary feed rate is: D = 360 ( F / π d ) where: D = rotary feed rate (dpm) F = linear feed rate d = diameter of workpiece π = pi = D = 360 ( 10 / π 4 ) D = dpm when: F = 10 ipm d = 4" Example: Rotary index for drilling holes This program drills three holes, 120 degrees apart. G0 G90 X0 Y9 Z1 C0 (Start-up F5 (Set Z feedrate G81 C.05 T0 D-.3 (Set drill variables Y0 C0 (Drill at 0 degrees C120 (Drill at 120 deg C240 (Drill at 240 deg G0 G90 Z1 (Move Z up X0 Y9 C0 (Go to start M30

13 Chapter 6 Programming 95 Example: Rotary table cutting All four axes can move and cut simultaneously using G01 linear interpolation. These programs, for parts such as turbines, are frequently long and complex, requiring CAD/CAM for proper position calculations. A simple spiral "thread" with a lead of.25" by 1" long, cut at a linear feed rate of 2 ipm, is shown in this example. (4 x 360 = 1440) G1 X-1 C1440 D230 F2 Feed Rate Commands (DEF words) The XYZ feed rate is programmed in inches per minute (ipm) in G70, or millimeters per minute (mmpm) in G71. XY feed rates are programmed using an F code. For Pendant or Teach mode, Z feed rates are also programmed using an F word. In CNC mode, the Z feed rate is programmed using an E word. The C axis rotary table is programmed in degrees per minute (dpm) using a D word. The default feed rate value is the power on state for the control. In the event that several feed rates apply to a command, the slowest one is used. For example, if F = 32 and E = 10, an XZ cut will be at 10 ipm. Feed rate values in the table are given for a Servo SAM mill or Servo II retrofit control each with the standard 5 pitch lead screw and Impact Mini- Mills. For a 10 pitch lead screw, such as is typical for a standard Bridgeport knee, divide by 2. Axis Code Feed Rate Range Configuration ipm XY F Z E C D dpm dpm mmpm SAM mill or Servo II with 5 pitch lead screw Impact acme screw Impact ball screw Servo II 10 pitch lead screw Impact acme screw Impact ball screw Servo II (.25 pitch) Impact (.1 pitch) The default E and F feed rate is 5 ipm or 127 mmpm. The default D feed rate is 100 dpm. (Note: The maximum feed rate that can be taught on the pendant is 50 ipm for a 5 pitch lead screw.)

14 96 Servo CNC System User's Guide Preparatory Functions (G Codes) G00 Rapid Positioning Moves A preparatory function, known as a G code, is required to change the programmed mode of operation of the control. The preparatory function consists of the letter G followed by one, two or three digits. The leading zero is not required. More than one G code can be programmed in one block of information as long as the codes do not cancel each other, such as G90 and G91 programmed in the same block. G code commands are either modal or non-modal. Modal commands stay in effect until changed or cancelled. Non-modal commands are valid only in the block in which they appear. The Reference section has a comprehensive list of G codes in the G Code Table (page 202). The G00 (G zero) function causes the machine to operate in rapid positioning mode with absolute or incremental data input. The starting point of the path is defined by the XYZC coordinate position at the end of the previous block or command. The end point is the programmed coordinates contained in the block of data. All programmed axes will move simultaneously, but not in a straight line. G00 cancels G01, G02, and G03. The previously programmed feed rates (DEF values) are not cancelled. Axis Rapid Configuration XY Z C 190 ipm 400 ipm 100 ipm 200 ipm 95 ipm 100 ipm 200 ipm 3800 dpm 9000 dpm SAM mill or Servo II with 5 pitch lead screw Impact acme screw Impact ball screw Servo II 10 pitch lead screw Impact acme screw Impact ball screw Servo II (.25 pitch) Impact (.1 pitch) CAUTION When programming a rapid move, it is important to be sure that the path of the tool will clear the work and any fixtures or holddowns. The speed cannot be overridden by the feed rate override control, except for the zero position, which stops all motion. All axes move simultaneously, but not in an interpolated path.

15 Chapter 6 Programming 97 Figure 9: Path of a rapid move. Example: G00 Rapid moves Using the figure above, you are at A and wish to move at rapid to B. The command is: G90 G00 X19 Y10 To move in incremental mode from A to B, the command is: G91 G00 X16.5 Y5.5 To stop at B to change a tool or manually drill a hole using the quill, the command is: G90 G00 X19 Y10 M00 G01 Linear Interpolation at Feed Rate The G01 function causes the machine to operate at the programmed feed rate as the axes travel along a straight line with absolute or incremental data input. The starting point of the path is defined by the XYZC coordinates of the previous block. The end point is the programmed coordinates contained in the block of data. All programmed axes will move simultaneously (using linear interpolation). G01 cancels G00, G02, and G03. Figure 10: G01 single axis move. Example: G01 one axis cut

16 98 Servo CNC System User's Guide Using the figure above, suppose you are positioned at A and wish to make a cut to B at a feed rate of six inches per minute. In absolute mode, the command is: G90 G01 X30 F6 To return to A in absolute mode, the command is: X8.5 From A to B in incremental mode, the command is: G91 G01 X21.5 F6 To return to A in incremental mode, the command is: X-21.5 Note that in the absolute example, the X value is written with respect to the zero datum. In the incremental example, the X value is the distance between A and B. Also note that there is no Y dimension in the block, since you are not changing the Y value. Figure 11: G01 in the XY plane. Example: G01 two axis cut Using the figure above, make a diagonal cut in the XY plane. Assume that the tool is positioned at A and you want to cut from A to C at a feed rate of fifteen inches per minute. In absolute mode, the command is: G90 G01 X30 Y12.5 F15 In incremental mode, the command is: G91 G01 X21.5 Y7.5 F15

17 Chapter 6 Programming 99 Since the destination C represents a change in both axes, the block must contain both X and Y coordinates. Now make a cut back along the same line from C to A. In absolute mode, the command is: X8.5 Y5 In incremental mode, the command is: X-21.5 Y-7.5 In incremental, the coordinates are written with respect to the tool location at the start point of the cut. Since the tool is moving in a negative direction in both axes to arrive at A, both coordinates (X and Y) are negative. Figure 12: G01 in three axes XYZ. Example: G01 three axis cut Using the rectangular solid in the figure above, suppose you need to make a ramp cut from A to B. The data block written in the absolute mode with a ten inch per minute feed rate is: G90 G01 X3.25 Y0 Z-1.62 F10 E10 In the incremental mode, the command is: G91 G01 X3.25 Y-2.75 Z-1.62 F10 E10 You can also make moves in selected planes. For example, returning from B to datum in absolute: G90 G01 X0 Z0 or incrementally: G91 G01 X-3.25 Z1.62

18 100 Servo CNC System User's Guide A single Z axis move is a plunge cut, for example, from C to B: G90 G01 Z-1.62 or incrementally: G91 G01 Z-1.62 G02, G03 Circular Interpolation Figure 13: G02 reference in XY, XZ and YZ planes. The G02 function indicates that the axes motions will generate a full arc or a segment of an arc in the clockwise direction. The plane in which the arc is generated is defined by the G17/18/19 code. The arc radius is defined by the end point and the incremental coordinates from the start point to the center of the arc (I,J,K). G02 cancels G00, G01, and G03. (See examples.) The G03 function is the same as G02 except in the counterclockwise direction. G03 cancels G00, G01, and G02. Notice that the circle on the XZ plane appears to be going counterclockwise in response to the G02 code. This is because the view is shown as though we were standing in front of the mill, and in order to view the XZ plane correctly, we would have to stand behind the mill. The rotations are valid for a view of the plane from the positive end of the axis perpendicular to the plane (in this case, the positive end of the Y axis). The problem doesn't appear in our illustration of the YZ plane since we are viewing it from the positive end of the X axis. NOTE G17. If your entire program is in the XY plane, you do not have to specify

19 Chapter 6 Programming 101 Figure 14: Full circle or begin and end on an axis. Example: Arcs begin and end on an axis The simplest case is a full 360 degree circle in the XY plane starting on an axis. Using the figure above, suppose you wish to make a full circle clockwise (G02) from point A on the circumference of the intended circle and lying on the X axis of the part. The command is: G02 I1.25 Since you are making a full circle, the end point is the same as the start point. J is 0 because you are starting on the X axis of the circle. No J value is required since J is 0. Note that the sign of I is plus (+). I and J define the center of the arc with respect to start point. Since the center of the arc is positive (to the right) with respect to the start point, I is positive. If you start at B, A clockwise full circle is: G02 I-1.25 Starting at C (on the Y axis), the incremental coordinate of the radius is - J, so the command is: G02 J-1.25 starting at D, the command is: G02 J1.25 In all cases above, you could have made the circle in the CCW rotation by replacing G02 with G03. To make a 90 or 270 degree arc from A to C, since the illustration does not indicate the absolute coordinates of the circle, you have to define the end point C, using incremental X and Y coordinates (G91): G91 G02 I1.25 X1.25 Y1.25

20 102 Servo CNC System User's Guide Now, return along the same arc path from C to A, still without knowing the absolute coordinates of the circle: G91 G03 J-1.25 X-1.25 Y-1.25 If the center of the circle is the (0,0) datum, the 90 degree arc from A to C is: G90 G02 I1.25 X0 Y1.25 and the 90 degree arc from C to A is: G90 G03 J-1.25 X-1.25 Y0 Figure 15: Arcs begin and end at any angle. Example: Arcs begin or end at an angle You can begin at any angle on a circle and end at any angle. Using the figure above, make a full circle CW, beginning at D, a point on a 1.25 radius which lies at a 45 degree angle from the X axis of the circle. Since you are not beginning on an axis, you have to define both the I and J components of the radius. Since the angle is 45 degrees, I and J have the same size as found by: 1.25 cos 45 degrees =.8839 To get the signs of I and J right, remember that they define the center of the arc with respect to the start point D. The command is: G02 I.8839 J No end points (X and Y) are required, since you are making a full circle and no G91 is required, since the control interprets all I and J dimensions as incremental. If you want to make an arc clockwise, beginning at D and ending at E. You have to put in coordinates of E. In incremental mode, the command becomes: G91 G02 I.8839 J X Y

21 Chapter 6 Programming 103 Suppose the center of the circle is the (0,0) datum. The same move written in absolute is: G90 G02 I.8839 J X.8839 Y From D and ending at F: G90 G02 I.8839 J X0 Y-1.25 Figure 16: G18 and G19 programming examples. Example: Arcs in the XZ or YZ plane (G18/G19) Using the figure above, make a clockwise arc from A to B. Since we don't know the absolute location, the block would read: G91 G19 G02 J1.5 starting at B and returning to A. G91 G19 G03 Y-1.5 Z-1.5 K-1.5 Now program the circle on the XZ plane starting at C and going clockwise (as viewed) to D. Remember there is an apparent reversal of rotation when in the XZ plane is viewed from the front of the mill! The block would be: G91 G18 G03 X1.067 Z I K Starting at D and returning to C: G91 G18 G02 X Z K1.5

22 104 Servo CNC System User's Guide If we know the coordinate system datum point, we could write any of the above examples in absolute notation. For example, if the coordinates of position D are X3 and Z.5, the data block in absolute for an arc from D to C would be: G90 G18 G02 X Z K1.5 In a practical case, D would also have a Y coordinate, but it wouldn't show up in the data block because it wouldn't change for a contour in the XZ plane. Example: Helical interpolation In the XY plane, this cut creates a spiral ramp or, with appropriate tooling, can be used to cut threads. A Z axis value is added to a G02 or G03 data block. The Z axis value is distributed evenly as the arc is cut. For example, using a circle with a 1.25 radius and adding.25 lead for a full circle, the command is: G91 G02 I1.25 Z-.25 This will machine a spiral ramp down.25 in 360 degrees of arc. To do a thread with, for example four turns, use the command above in a subroutine and call it four times. NOTE Cutter diameter compensation cannot be used with helical interpolation. G04 Dwell The G04 function sets a dwell time from.05 seconds to 999 seconds. The format is G04 Fn where n is the number of seconds. NOTE The maximum dwell time for programs run on the pendant is approximately 65 seconds. Example: G04 Dwell per revolution dwell in seconds = desired # of revolutions / [spindle RPM / 60] If the desired dwell time is 3 revolutions and If the spindle speed is 1500 revolutions per minute # of seconds = 3 revs / [ (1500 rev/min) / (60 sec/min) ] = 3 / 25 =.12 seconds = G04 F.12

23 Chapter 6 Programming 105 G17, G18, G19 Modal Plane Select These functions select the plane for circular interpolation (G02 and G03). The G17/18/19 code can be in the same block with a G02 or G03 code but must be before the G2 or G3 code, for example G19 G2 X.3 Z.4 I.6 Clockwise and counterclockwise direction is determined by looking toward the selected plane from the positive axis normal to the plane. Figure 17: G02 and G03 directions for G17, G18, and G19. G17 selects the XY plane and is the power on default. G17 is modal and cancels G18 and G19. G18 selects the ZX plane. G18 is modal and cancels G17 and G19. G19 selects the YZ plane. G19 is modal and cancels G17 and G18. NOTE Cutter compensation (G41/42) is valid in G17 only. A G40 is required before programming a G18 or G19. NOTE The C axis used as Z is not supported. Figure 18: G18 cylinder using ball nose endmill. Example: Arcs using a ball nose endmill A ball nose endmill is best to use when cutting an arc in the XZ or YZ plane. Program to the center of the ball as shown in the figure below. The tool maintains a tangent relationship with the arc.

24 106 Servo CNC System User's Guide The program below cuts a 2" long cylinder in the XZ plane using a.250" diameter ball nose endmill. N010 G90 X3 Y2.5 Z1.2 N015 E6 F6 N020 G0 X2.2 Y0 N025 Z.4 N030 G1 X1.8 N035 P0110 (LENGTH 2" N040 G90 G1 X2.2 N045 Z1.2 N050 M25 N055 G0 X3 Y2.5 M30 ( P01 (SR CYLINDER + ADVANCE N100 G90 G18 G2 X.3 Z.4 I-.75 N105 G91 G1 Y.1 N110 G90 G3 X1.8 Z.4 I.75 N115 G91 G1 Y.1 M12 Figure 19: G18 cylinder using flat bottom endmill. Example: Arc using a flat endmill When a flat bottom endmill is used, program a clockwise and counterclockwise cut to the "edge" of the tool. The program below cuts a 2" long cylinder in the XZ plane using a.250" flat bottom endmill. N010 G90 X3 Y2.5 Z2 N015 E6 F6 T0 N020 G0 X2.15 Y0 N025 Z.4 N035 P0120 (LENGTH 2" N040 G90 G1 X2.15 N045 Z2 N050 M25 N055 G0 X3 Y2.5 M30

25 Chapter 6 Programming 107 G21 Scaling and Mirror Image ( P01 (SR N095 G1 X2.025 (CUT TO CYL START N100 G18 G2 X1.4 Z1.025 I-.625 N105 G1 X1.3 (CUT.1 ACROSS TOP N110 G0 X.65 (MOVE TO SAFE PLACE N115 Z.4 (Z START LEVEL N120 G1 X.775 (CUT TO CYL START N125 G3 X1.4 Z1.025 I.625 N130 G1 X1.5 (CUT.1 ACROSS TOP N135 G0 X2.15 (MOVE TO SAFE PLACE N115 G91 Y.1 (MOVE TO NEXT CUT N140 G90 Z.4 (Z START LEVEL M12 G21 is used for both scaling and mirroring. The G21 code allows the program, or section of the program to be mirrored on each axis, or scaled. The format is G21 Xn Yn Zn where n is +1 or -1 to mirror or some other value if the part is also scaled, for example.5 for 1/2 scale. To return to normal polarity and 1:1 scale program G21 X1 Y1 Z1 When G21 is active, the "Scaling" values are displayed on the G-Code status tab (page 24). CAUTION For safety, it is good practice to cancel the G21 code in the first block of any program using G21. Guidelines for G21 1 For safety, it is good practice to cancel the G21 code in the first block of any program using G21. This is done by programming: G21 X1 Y1 Z1. 2 The mirror centerline, also known as the mirror or reflection plane, is most easily programmed using a G94, which is an absolute X, Y, or Z offset from the program datum point (absolute zero). The program example (page 110) shows two methods for defining the mirror centerline. 3 If the part is programmed in absolute mode, the scale origin is absolute zero, unless moved by a G94 code. If the part is programmed in incremental mode, the scale origin is the tool position when the G21 is commanded. See the example (page 112).

26 108 Servo CNC System User's Guide 4 Scaling can cause some cuts to equal zero. This can affect cutter compensation and generate various error messages. If cut comp is a problem, try using a smaller diameter tool, change the lead-in cut to increase the distance, or put the lead-in before you set the scale. 5 Unequal scale values can be used, for example G21 X.8 Y.9, however, circular interpolation will not work properly. The X and Y values must be the same to make a circle, however, not necessarily the same sign. 6 When the mirror image of an axis is set, the control simply changes the sign of every coordinate read for that axis. Also, if only one of the axes for an arc or circle is reversed, the direction of the arc (clockwise or counterclockwise) is reversed. If only one axis is reversed, the direction of motion around the part is also reversed. That is, climb cuts become conventional cuts and vice versa. 7 The Z axis can also be mirrored, however care should be taken when approaching and retracting from the workpiece. A Z axis mirror image turns the concave (female) half of a mold into the convex (male) half of a mold. Make sure the tool approach and retract are not mirrored or the tool will collide with the part! Figure 20: Mirroring about the Y axis. Example: G21 right- and left-hand parts To machine these parts, the program is written for the right-hand part. Then, the mirror of the Y axis is the left-hand part. Typically, a subroutine is used for the basic program. A program to machine a right-hand and then a lefthand part can be done as follows: G21 X1 Y1 (Cancel mirror imaging P0101 (Machine the right-hand part G21 X-1 (Mirror image the X axis P0101 (Machine the left-hand part M30 ( P01 (The program for the : (right-hand part M12 (goes here

27 Chapter 6 Programming 109 Figure 21: Mirroring about the X and Y axis. Example: G21 symmetrical about 0,0 Parts that are symmetrical about 0,0 include both wheel-like parts and parts with right-left symmetry. Suppose a part is symmetrical top-to-bottom and side-to-side. Rather than programming each of the four quadrants separately, the program might be written as shown below the figure. G21 X1 Y1 (Cancel mirror image P0101 (Machine the upper rgt-hand quad G21 X-1 (Mirror X P0101 (Machine the upper lft-hand quad G21 Y-1 (Mirror X and Y P0101 (Machine the lower lft-hand quad G21 X1 Y1 (Cancel mirror X and Y P0101 (Machine the lower rgt-hand quad M30 ( P01 (The program for the upper : (right-hand quadrant goes here M12

28 110 Servo CNC System User's Guide Figure 22: Using G21 on a multiple part fixture. Example: G21 multiple part fixture When machining several identical parts on one fixture, you can sometimes machine more parts per machining cycle if some are turned 180 degrees, as shown in the figure below. A convenient way to do this is to first write a subroutine for one part. Then, define another subroutine that reverses both the X and Y axes and then calls the first subroutine. This example shows two programs, one in incremental mode and one in absolute more that also uses G94. This program uses incremental mode for the subroutines and programs an absolute move to each start point to position properly for the incremental move. G21 X1 Y1 Z1 (Cancel mirror image G0 G90 X0 Y1 Z1 (Go to start part 1 Z.05 (Z to clear plane P0101 (Machine part 1 G0 G90 X1.7 Y-.2 (Move to part 2 P0201 (Machine reverse part G21 X1 Y1 (Set normal symmetry G0 G90 X1.9 Y1 (Move to part 3 P0101 (Machine part 3 G0 G90 X3.6 Y-.2 (Move to part 4 P0201 (Machine part 4 G21 X1 Y1 (Set normal symmetry G0 G90 X0 Y1 Z1 (Go to start pt M30 (End of main program ( P01 (SR to mach normal part G91 G1 Z-.2 E2 (Incremental mode Y-1 F10 X1 Y.3 X-.5 Y.4 X-.5 G0 Z.2 Y.3 M12 (End SR for normal part (

29 Chapter 6 Programming 111 P02 G21 X-1 Y-1 P0101 M12 (SR to machine reverse part (Mirror part (Machine part (End SR for reverse part This program uses absolute mode for the subroutines and a G94 code to temporarily move the datum for each part. The subroutine has an absolute move to the start point. G21 X1 Y1 Z1 (Cancel mirror image G0 G90 X0 Y1 Z1 (Go to start part 1 Z.05 (Z to clear plane P0101 (Machine part 1 G94 X1.7 Y.8 (Set origin for part 2 P0201 (Machine reverse part G21 X1 Y1 (Set normal symmetry G94 X1.9 Y0 (Set origin for part 3 P0101 (Machine part 3 G94 X3.6 Y.8 (Set origin for part 4 P0201 (Machine part 4 G21 X1 Y1 (Set normal symmetry G94 X0 Y0 (Set origin to datum G0 G90 X0 Y1 Z1 (Go to start pt M30 (End of main program ( P01 (SR to mach. normal part G90 G0 X0 Y1 (Absolute mode start pt G1 Z-.15 E2 Y0 F10 X1 Y.3 X.5 Y.7 X0 G0 Z.05 Y1 M12 (End SR for normal part ( P02 (SR to mach. reverse part G21 X-1 Y-1 (Mirror part P0101 (Machine part M12 (End SR for reverse part

30 112 Servo CNC System User's Guide Figure 23: Scaling and scale origin. Example: G21 scaling The scaling feature allows the position of each axis to be proportionally increased or reduced under program control. This can be used to adjust for shrink factors in molds. It can also be used to run a scaled prototype of a larger part that would otherwise be cut on a larger machine. When G21 is active, the "Scaling" values are displayed on the G-Code status tab (page 24). The figure shows the scale origin. If the part is programmed in absolute mode (G90), the scale origin is absolute zero, unless moved by a G94 code. If the part is programmed in incremental mode (G91), the scale origin is the tool position when the G21 is commanded. N010 F10 E2 T0 G40 (Start-up N020 G90 G0 Z1 N030 X0 Y0 N040 T13 (.187 dia endmill N050 G94 X2.1 Y.5(Set scale origin N060 G21 X.5 Y.5 (Set scale N070 P0101 (Cut Part N080 G21 X1 Y1 (Cancel scale N090 G94 X0 Y0 (Set origin to datum N100 G90 G0 Z1 N110 X0 Y0 T0 M30 ( P01 (Basic part at datum N301 G90 G0 X-.2 Y-.2 N302 Z.1 N303 G41 (CutComp ON left N304 G1 X-.2 Y-.2 Z-.05 N305 X0 N306 Y.8028 N307 G2 I.25 J0 X.4415 Y.9635 N308 G1 X1.25 Y0 N309 X-.2 N310 G40 (CutComp OFF N311 Z.1 M12

31 Chapter 6 Programming 113 A program that allows for a 3% shrink factor in a mold might be done as follows: G90 G0 X Y Z (Program start-up G21 X1.03 Y1.03 (Set scale P0101 (Machine mold G21 X1 Y1 Z1 (Cancel scale G90 G0 X Y Z (Return to start-up M30 ( P01 (The basic program for the G90... (mold goes here : M12 G22 Rotate The G22 code allows the program, or section of the program to be rotated around the datum point or around an offset datum defined using G94. The format is G22 Xn where n is an absolute angle (page 92) of rotation in decimal degrees (page 92). At the end of the program, reset the angle to zero by programming G22 X0 NOTE The G94 point is not identical to the center of rotation for a rotated pattern. Figure 24: Rotate toolpath example. Example: G22 toolpath rotation

32 114 Servo CNC System User's Guide The tool path is defined in its "original" location in subroutine P01. The subroutine is in absolute. G94 and G22 are used to reposition and rotate the path. For example, to find the G94 coordinates of Part 2, side = 1.5 x sin 45 = 1.5 x = X = = Y = = Notice that the T code for cutter compensation is defined before any G94. This is because the XYZ offset values associated with a T command supersede the offset values of the G94 command. The cutter compensation is defined within the subroutine. It is turned off before positioning to a new location, otherwise that move will also be a compensated move. N1 F10 E2 T0 G40 (Program start-up G90 G0 Z1 X-0.5 Y2 T4 (T4=.250 dia endmill G94 X-1.5 Y-2 (Position to Part 1 G22 X0 (Set rotation P0101 (Cut Part 1 N2 G94 X Y (Position to Part 2 G22 X45 (Set rotation P0101 (Cut Part 2 N3 G94 X-3 Y-.5 (Position to Part 3 G22 X90 (Set rotation P0101 (Cut Part 3 N4 G94 X Y (Position to Part 4 G22 X135 (Set rotation P0101 (Cut Part 4 N5 G94 X-4.5 Y-2 (Position to Part 5 G22 X180 (Set rotation P0101 (Cut Part 5 N6 G94 X0 Y0 (Return to original 0 G22 X0 (Set rotation to 0 G90 G0 Z1 (Return to Z home X-.5 Y2 (Return to XY start pt M30 (End main program P01 (Basic part at datum N301 G90 G0 X-.2 Y-.2 (Move to start cut N302 Z.1 N303 G41 (Cut comp Left T4 N304 G1 X-.2 Y-.2 Z-.05 N305 X0 Y-.2 N306 X0 Y.8028 N307 G2 I.25 X.4415 Y.9635 N308 G1 X1.25 Y0 N309 X-.02 Y0 N310 G40 N311 Z.1 M12

33 Chapter 6 Programming 115 G40, G41, G42 Cutter Diameter Compensation The G40 code cancels cutter diameter compensation left or right. Figure 25: G41 and G42 cutter diameter compensation. The G41 and G42 codes allow you to program the edge of the part without being concerned about the actual diameter of the tool. The tool diameter is then supplied from the Tool Table. Left or right are defined as follows: when looking in the direction of the cut, for G41 the tool is on the left hand side of the material, for G42 the tool is on the right hand side of the material. G40 or G42 cancel G41. G40 or G41 cancel G42. TIP Pretend the tool is a car and you are sitting in the car driving along in the direction you want the tool to cut. Where is the tool in relation to the material to be cut? Choose LEFT if the tool is to the left of the material, choose RIGHT if the tool is to the right of the material. Cutter Comp Rules & Guidelines 1 The G41 or G42 codes must be followed by a linear move that begins without compensation and ends with compensation as shown in example "Lead in (page 117)". The G40 code must be followed by a linear move that begins with compensation and ends without compensation as shown in example "Lead out (page 118)".

34 116 Servo CNC System User's Guide Figure 26: Tight spots for cutter compensation. 2 If you need to change to the opposite cutter compensation direction, that is from left G41 to Right G42 or vice versa, use the G40 command to cancel first. Then start the opposite direction. You may want to make the startup or ending moves "in air." 3 The compensated tool "rolls around" sharp corners with a zero radius to keep the tool in contact with the workpiece. 4 New T codes are not allowed inside a compensated path. 5 G21 used for mirror image causes cutter comp to cut the "wrong" side. G21 used as a scale factor can be used with cutter comp. 6 Canned cycle G codes automatically turn cutter compensation off (G40). If you had cutter comp on (G41 or G42) before you programmed a pocket, frame, face, or drill pattern canned cycle, it will be OFF when you exit the canned cycle. 7 When used with subroutine calls (P codes) and returns (M12), program the G41/G42 and cancel G40 entirely within the subroutine as shown in the G22 example or entirely outside. Do not turn it on outside the subroutine and off inside the subroutine; the results can be bizarre. 8 In cutter compensation, the system "looks ahead" to see where the tool is going in order to plan the appropriate end point for each cut. Because of this, cutter comp does not allow a 180 change in direction. For example, if you try to move from X1 to X0 and back to X1, the system displays ERROR: Tool is too large. When cutting a slot that is the width of the tool, follow the example (page 120). 9 Cutter compensation can not be used with circular interpolation in the XZ and YZ planes (G18 and G19). 10 Cutter compensation does not support different lead screw pitches for the X and Y axes. 11 The cutter compensation look-ahead can not prevent gouging when a tool enters or exits a confined space as shown below. It is up to the programmer to verify that the tool can fit through the required openings.

35 Chapter 6 Programming 117 Cutter Comp Tips TIP One T code can be used for a roughing tool and another for a finishing tool. Or, you may program for the nominal tool diameter and use the compensation function to adjust for the difference between the programmed tool and the actual tool. For example, if you write the program for a.156 diameter endmill, and the tool is actually.154 diameter, enter for the diameter in the Tool Table. TIP In some cases, it may be necessary to "fool" the system in order for the beginning and ending of cuts to work exactly as the machinist would like. For example, you may have to program two XY approach moves to get the tool to the desired position. One of these moves can be "in the air" followed by a Z move to the cut plane, before the second XY move. The best approach is perpendicular to the line to be cut. TIP Make sure cutter compensation is OFF before positioning for drilling or going to the Start Point or tool change position. Otherwise the tool will move to the compensated position. TIP Program your tool path without cutter compensation first, but allow for "starts'n'ends" as stated in the rules. Then turn cutter compensation on (Left or Right) to see and debug the compensated path. Sometimes errors occur with cutter compensation on that don't happen when it is off. Figure 27: Starting cutter compensation. Example: Starting cutter comp The G41 or G42 code must be followed by a linear move that begins without compensation and ends with compensation.

36 118 Servo CNC System User's Guide Figure 28: Ending cutter compensation. Example: Ending cutter comp When cutter comp is turned off, the G40 code must be followed by a linear move that begins with compensation and ends without compensation.

37 Chapter 6 Programming 119 Figure 29: G41 Example Part with cutter comp off and cutter comp left. Example: G41 Toolpath The first figure shows the toolpath for no cutter comp. The second figure shows the toolpath for G41. The tool (T4) is a.250 diameter endmill. The program is shown below the figures. N10 E2 F10 T0 N15 G90 G0 X-.5 Y1 Z1 (Start up N20 X.2 Y-.75 (Position XY N25 Z.05 T4 (Call T4 N30 G1 Z-0.1 (Plunge Z N35 G41 (Comp on left N40 Y-.5 N45 X0 N50 G2 J.5 X0 Y0.5 N55 G1 X0.634 N60 X1.5 Y0 N65 Y-0.3 N70 G2 I-0.2 X1.3 Y-0.5 N75 G1 X-.1 N80 Y-0.75 N85 Z.05 N90 G40 (Turn Comp off N95 G0 X-.5 Y1 Z1 M30

38 120 Servo CNC System User's Guide NOTE The "Engineering Drawing" for dimensions and a manual program can be found here (page 210). Figure 30: G42 the "slot" solution. Example: G42 "The slot solution" In this example, the tool is.250 diameter and the slot is.25 wide. The normal solution is to program the tool to cut up the center of the slot. When using cutter diameter compensation, you program the edge of the part. However, to prevent cutter compensation from choking on the 180 turn at the end of the slot, program the slot width.0001" wider than the tool as shown in program below. N10 G90 G0 X0 Y0 T4 N20 G1 X-.15 Y-.15 N30 G42 N40 X0 Y0 N50 X.5 N60 Y.625 N70 G91 X.2501 N80 G90 Y0 N90 X1 : : G70, G71 Inch, Metric Programming The G70 code is the default or power on state for the control. All data are interpreted as being in the inch dimension system with X1 read as 1 inch. G70 cancels G71. After a G71 code, all data are interpreted as being in the metric dimension system with X1 read as 1 millimeter. G71 cancels G70. G90, G91 Absolute, Incremental Programming The G90 code causes the control to read all XYZC values as absolute coordinates, that is, all coordinates are written with respect to the zero datum. G90 is the default power on state for the control. G90 cancels G91.

39 Chapter 6 Programming 121 G92 Position Preset The G91 code causes the control to read all XYZC values as incremental distance commands, that is, all coordinates are written with respect to the position at the start of the move. If the direction of motion is minus, the incremental distance value must be preceded by a minus sign. If the direction of motion is plus, no sign need be entered; absence of a sign is interpreted to be a plus by the control. G91 cancels G90. Go here to see an example (page 91). TIP The choice of programming in absolute or incremental is usually dictated by the drawing you are using to write the program. Sometimes a shop drawing has all the dimensions referenced to a single datum so that G90 absolute is the appropriate choice. At other times, the program requires a number of repetitive moves, in which case G91 incremental is the better choice. The G92 code provides the ability to preset XYZC absolute position registers to any desired dimension. The machine slides will not move in response to this block. The G92 command allows the translation of an original coordinate system to a new part coordinate system. This is convenient if multiple parts on a fixture are made. However, since the G92 preset command replaces the previous contents of the absolute registers, a new G92 preset command and a positioning move will be necessary to return to the original coordinate system. When setting up a new part, G92 can be used in MDI mode to set the part datum as shown in the example (page 54). CAUTION G92 destroys the previous contents of the absolute registers. This means that if you interrupt the run with a STOP that resets the program or Emergency Stop, the program does not know where the original datum (X0 Y0 Z0 C0) is.