Lathe Code. Lathe Specific Additions. 1 de 15 27/01/ :20. Contents. 1. Introduction DesktopCNC?

Transcription

1 1 de 15 27/01/ :20 Lathe Code EmcKnowledgeBase RecentChanges PageIndex Preferences LinuxCNC.org Search: Lathe Specific Additions Contents 1. Introduction 2. Lathe G codes 2.1. DesktopCNC 2.2. Haas Lathe Codes 2.3. OKUMA OSP 2200 ('80 vintage) 3. Threading 3.1. Mitsubishi G SIEMENS 840D, EMCO Variant 3.3. OKUMA OSP 2200 ('80 vintage) 3.4. Add other versions of G33 4. Multi pass Thread Cutting Canned Cycle 4.1. This is fanuc style canned cycle 4.2. Macro Canned Cycle 5. Constant Surface Speed 6. Sample Threading Programs 6.1. Synergy 1/4 20 thread program 6.2. Roltek Sample Threading Program 7. Mastercam Threading Parameters Pages 1. Introduction CNC lathe operation has been a topic of discussion as long as rayh and probably mshaver have been hanging around this software. This page is designed to provide a comprehensive set of specifications for this essential ability. 2. Lathe G codes There are a number of different sets of codes used by cnc makers to handle lathe specific operations. Included are those from a couple of sources. These are not meant to be overwhelming. They are intended to show the range of operations possible on common commercial lathes. As we begin to build in lathe functionality, we need to do it in a way that permits the expansion of functionality without the need to rewrite earlier abilities DesktopCNC?

2 2 de 15 27/01/ :20 This is from a list at G32 is used for Plain Threading Cycle G33 Threadcutting, constant lead G34 Threadcutting, increasing lead G35 Threadcutting, decreasing lead G46 is used for Turning Canned Cycle G47 is used for Facing Canned Cycle G66 is used for Stock Removal Roughing G67 is used for Stock Removal Finishing G76 is used for Canned Cycle, Thread Cutting Cycle G70 is used for Canned Cycle, Finishing Cycle G71 is used for Canned Cycle, OD Roughing Cycle G72 is used for Canned Cycle, Face Roughing Cycle G73 is used for Canned Cycle, Profiling Cycle G74 is used for Canned Cycle, Face Grooving Cycle G75 is used for Canned Cycle, OD Grooving Cycle G90 is used for Cutting Cycle A G92 is used for Thread Cutting Cycle G94 is used for Cutting Cycle B M10 Clamp M11 Unclamp M12 Synchronization Code M19 Oriented Spindle Stop 2.2. Haas Lathe Codes G00* RAPID POSITIONING MOTION (X,Z,U,W,B) (SETTING 10, 101) G01 LINEAR INTERPOLATION MOTION (X,Z,U,W,B,F) G01 CHAMFERING AND CORNER ROUNDING (X,Z,U,W,B,I,K,R,A,F) G02 CW CIRCULAR INTERPOLATION MOTION (X,Z,U,W,I,K,R,F) G03 CCW CIRCULAR INTERPOLATION MOTION (X,Z,U,W,I,K,R,F) G04 DWELL (P) (P=seconds. milliseconds) G05** FINE SPINDLE CONTROL MOTION (X,Z,U,W,R,F) (LIVE TOOLING) G09 EXACT STOP, NON MODAL G10 PROGRAMMABLE OFFSET SETTING (X,Z,U,W,L,P,Q,R) G14** MAIN SPINDLE SHIFT TO SUB SPINDLE G15** MAIN SPINDLE SHIFT TO SUB SPINDLE CANCEL G17** CIRCULAR MOTION XY PLANE SELECTION (G02,G03) (LIVE TOOLING) G18* CIRCULAR MOTION ZX PLANE SELECTION (G02,G03) (SETTING 56) G19** CIRCULAR MOTION YZ PLANE SELECTION (G02,G03) (LIVE TOOLING) G20* VERIFY INCH COORDINATE POSITIONING (SETTING 9 needs to be INCH) G21 VERIFY METRIC COORDINATE POSITIONING (SETTING 9 needs to be METRIC) G28 MACHINE ZERO RETURN THRU REF. POINT (X,Z,U,W,B) (Fanuc) G29 MOVE TO LOCATION THROUGH G29 REF. POINT (X,Z) (Fanuc) G31** FEED UNTIL SKIP FUNCTION (X,Z,U,W,F) G32 THREAD CUTTING PATH, MODAL (X,Z,U,W,F) G40* TOOL NOSE COMPENSATION CANCEL G41/G42 (X,Z,U,W,I,K) (SETTING 56) G41 TOOL NOSE COMPENSATION, LEFT (X,Z,U,W) (SETTING 43, 44, 58) G42 TOOL NOSE COMPENSATION, RIGHT (X,Z,U,W) (SETTING 43, 44, 58)

3 3 de 15 27/01/ :20 G50 SPINDLE SPEED MAXIMUM RPM LIMIT (S) G51 RETURN TO MACHINE ZERO, CANCEL OFFSET (Yasnac) G52 WORK OFFSET COORDINATE POSITIONING (Yasnac) G52 GLOBAL WORK COORDINATE SYSTEM SHIFT (Fanuc) G53 MACHINE COORDINATE POSITIONING, NON MODAL (X,Z,B) G54* WORK OFFSET COORDINATE POSITIONING #1 (SETTING 56) G55 WORK OFFSET COORDINATE POSITIONING #2 G56 WORK OFFSET COORDINATE POSITIONING #3 G57 WORK OFFSET COORDINATE POSITIONING #4 G58 WORK OFFSET COORDINATE POSITIONING #5 G59 WORK OFFSET COORDINATE POSITIONING #6 G61 EXACT STOP, MODAL (X,Z) G64* EXACT STOP G61 CANCEL (SETTING 56) G65** MACRO SUB ROUTINE CALL G70 FINISHING CYCLE (P,Q) G71 O.D. / I.D. STOCK REMOVAL CYCLE (P,Q,U,W,I,K,D,S,T,R1,F) (SETTING 72, 73) G72 END FACE STOCK REMOVAL CYCLE (P,Q,U,W,I,K,D,S,T,R1,F) (SETTING 72, 73) G73 IRREGULAR PATH STOCK REMOVAL CYCLE (P,Q,U,W,I,K,D,S,T,F) G74 FACE GROOVING, or HIGH SPEED PECK DRILL CYCLE (X,Z,U,W,I,K,D,F) (SETTING 22) G75 O.D. / I.D. PECK GROOVING CYCLE, (X,Z,U,W,I,K,D,F) (SETTING 22) G76 THREAD CUTTING CYCLE, MULTIPLE PASS (X,Z,U,W,I,K,A,D,F) (SETTING 86, 95, 96, 99) G77** FLATTING CYCLE (I,J,L,R,S,K) (LIVE TOOLING) G80* CANCEL CANNED CYCLE (SETTING 56) G81 DRILL CANNED CYCLE (X,Z,W,R,F) G82 SPOT DRILL / COUNTERBORE CANNED CYCLE (X,Z,W,P,R,F) G83 PECK DRILLING CANNED CYCLE (X,Z,W,I,J,K,Q,P,R,F) (SETTING 22, 52) G84 TAPPING CANNED CYCLE (X,Z,W,R,F) G85 BORE IN, BORE OUT CANNED CYCLE (X,Z,U,W,R,L,F) G86 BORE IN, STOP, RAPID OUT CANNED CYCLE (X,Z,U,W,R,L,F) G87 BORE IN, STOP, MANUAL RETRACT CANNED CYCLE (X,Z,U,W,R,L,F) G88 BORE IN, DWELL, MANUAL RETRACT CANNED CYCLE (X,Z,U,W,P,R,L,F) G89 BORE IN, DWELL, BORE OUT CANNED CYCLE (X,Z,U,W,P,R,L,F) G90 O.D. / I.D. TURNING CYCLE, MODAL (X,Z,U,W,I,F) G92 THREADING CYCLE, MODAL (X,Z,U,W,I,F) (SETTING 95, 96) G94 END FACING CYCLE, MODAL (X,Z,U,W,K,F) G95** END FACE LIVE TOOLING RIGID TAP (X,Z,W,R,F) G96 CONSTANT SURFACE SPEED, CSS ON (S) G97* CONSTANT NON VARYING SPINDLE SPEED, CSS OFF (S) (SETTING 56) G98 FEED PER MINUTE (F) G99* FEED PER REVOLUTION (F) (SETTING 56) G100 MIRROR IMAGE CANCEL G101 G101 MIRROR IMAGE (X,Z) (SETTING 45, 47) G102 PROGRAMMABLE OUTPUT TO RS 232 (X,Z) G103 LIMIT BLOCK LOOKAHEAD (P0 P15 max. for number control looks ahead) G105 SERVO BAR COMMAND G110 G111 WORK OFFSET COORDINATE POSITIONING #7 #8 G112** CARTESIAN TO POLAR TRANSFORMATION G113** CARTESIAN TO POLAR TRANSFORMATION CANCEL G114 G129 WORK OFFSET COORDINATE POSITIONING #9 #24 G159** BACKGROUND PICKUP / PART RETURN

4 4 de 15 27/01/ :20 G160** APL AXIS COMMAND MODE ON G161** APL AXIS COMMAND MODE OFF G184 REVERSE TAPPING CANNED CYCLE (X,Z,W,R,F) (SETTING 130) G187 ACCURACY CONTROL FOR HIGH SPEED MACHINING (E) (SETTING 85) G194 SUB SPINDLE / TAPPING CANNED CYCLE G195 LIVE TOOLING VECTOR TAPPING (X,F) G196 LIVE TOOLING VECTOR TAPPING REVERSE (X,F) G200 INDEX ON THE FLY (X,Z,U,W,T) M00 PROGRAM STOP (SETTING 42, 101) M01 OPTIONAL PROGRAM STOP (SETTING 17) M02 PROGRAM END M03 SPINDLE ON FORWARD (S) (SETTING 144) M04 SPINDLE ON REVERSE (S) (SETTING 144) M05 SPINDLE STOP M08 COOLANT ON (SETTING 32) M09 COOLANT OFF M10 CHUCK CLAMP (SETTING 92) M11 CHUCK UNCLAMP (SETTING 92) M12** AUTO AIR JET ON (P) M13** AUTO AIR JET OFF M14** MAIN SPINDLE CLAMP M15** MAIN SPINDLE UNCLAMP M17 ROTATE TURRET FORWARD (T) (SETTING 97) M18 ROTATE TURRET REVERSE (T) (SETTING 97) M19** ORIENT SPINDLE (P,R) M21** TAILSTOCK ADVANCE (SETTING 93, 94, 106, 107, 121, 145) M22** TAILSTOCK RETRACT (SETTING 105) M23 ANGLE OUT OF THREAD ON (SETTING 95, 96) M24 ANGLE OUT OF THREAD OFF M30 PROGRAM END AND RESET (SETTING 2, 39, 56, 83) M31 CHIP AUGER FORWARD (SETTING 114, 115) M32 CHIP AUGER REVERSE (SETTING 114, 115) M33 CHIP AUGER STOP M36** PARTS CATCHER ON M37** PARTS CATCHER OFF M41 SPINDLE LOW GEAR OVERRIDE M42 SPINDLE HIGH GEAR OVERRIDE M43 TURRET UNLOCK (FOR SERVICE USE ONLY) M44 TURRET LOCK (FOR SERVICE USE ONLY) M51 M58 OPTIONAL USER M CODE SET M59 OUTPUT RELAY SET (N) M61 M68 OPTIONAL USER M CODE CLEAR M69 OUTPUT RELAY CLEAR (N) M76 PROGRAM DISPLAYS INACTIVE M77 PROGRAM DISPLAYS ACTIVE M78 ALARM IF SKIP SIGNAL FOUND M79 ALARM IF SKIP SIGNAL NOT FOUND M85** AUTOMATIC DOOR OPEN (SETTING 51, 131) M86** AUTOMATIC DOOR CLOSE (SETTING 51, 131) M88** HIGH PRESSURE COOLANT ON (SETTING 32) M89** HIGH PRESSURE COOLANT OFF M93** AXIS POSITION CAPTURE START (P,Q) M94** AXIS POSITION CAPTURE STOP M95 SLEEP MODE (hh:mm)

5 5 de 15 27/01/ :20 M96 JUMP IF NO SIGNAL (P,Q) M97 LOCAL SUB ROUTINE CALL (P,L) M98 SUB PROGRAM CALL (P,L) M99 SUB PROGRAM/ROUTINE RETURN OR LOOP (P) (SETTING 118) M109** INTERACTIVE USER INPUT (P) M110** TAILSTOCK CHUCK CLAMP (SETTING 122) M111** TAILSTOCK CHUCK UNCLAMP (SETTING 122) M119** SUB SPINDLE ORIENT (P,R) M121 M128 OPTIONAL USER M CODE INTERFACE WITH M FIN SIGNAL M133** LIVE TOOL DRIVE FORWARD (P) M134** LIVE TOOL DRIVE REVERSE (P) M135** LIVE TOOL DRIVE STOP M143** SUB SPINDLE FORWARD (P) M144** SUB SPINDLE REVERSE (P) M145** SUB SPINDLE STOP M154** C AXIS ENGAGE (SETTING 102) M155** C AXIS DISENGAGE M164** ROTATE APL GRIPPERS TO "n" POSITION (Pn) M165** OPEN APL GRIPPER 1 (RAW MATERIAL) M166** CLOSE APL GRIPPER 1 (RAW MATERIAL) M167** OPEN APL GRIPPER 2 (FINISHED MATERIAL) M168** CLOSE APL GRIPPER 2 (FINISHED MATERIAL) 2.3. OKUMA OSP 2200 ('80 vintage) G0 rapid G1 feed G2 clockwise circle G3 anticlockwise circle G4 dwell f1000 is 10 seconds G13 front tool turret mirror image ( changes count direction of X axis and changed offsets ans compensation direction) G14 back turret mirror image (same as above) G25 28 chuck barrier definitions G33 35 Threading G40 cancel compensation G41 compensation left G42 compensaion right G50 origion shift and max rpm G80 cancel auto program mode and used for line jumping G81 ap mode longitudal cutting G82 ap mode face cutting G83 ap mode grooving G85 ap mode bar turning G86 ap mode copy turning G87 ap mode finishing cycle G90 absolute position mode G91 incremental mode (X and Z) G92 incremental mode X G93 incremental mode Z G94 feet per minute mode G95 inches per revolution mode G96 constant cutting speed mode G97 contant rpm mode

6 6 de 15 27/01/ :20 M22/23 thread chamfer on/off M24/25 chuck barrier on/off T =tool position number 02=tool offset number later systems used a third number to designate compensation number 3. Threading 3.1. Mitsubishi G33 Mitsubishi lists G33 for both thread cutting and tapping G33 Z# Q# E#(F#) Z is thread length Q is the shaft angle for the start E is the thread lead They select either tpi or lead using a parameter elsewhere SIEMENS 840D, EMCO Variant EMCO lists G33 for both thread cutting and tapping G33 X# Z# I/K# X is end position in X for thread Z is end position in Z for thread I/K is thread pitch 3.3. OKUMA OSP 2200 ('80 vintage) G33 X# Z# I# K# F# X is start position of thread (depth) Z is end position of thread I is amount of taper in radius K is change in lead per revolution (varible pitch thread) F is lead G22/23 turns chamfering on and off you would set a starting point with a G0 away from thread then G33 would rapid in X to start point, feed to programmed Z point, feed out in X then rapid back to the G0 programmed point 3.4. Add other versions of G33 please 4. Multi pass Thread Cutting Canned Cycle Single pass lathe threading is limited in cutting ability and requires a rather large diameter bar in order to cut without serious deflection. Most machine tool makers use canned cycles or macros in order to implement threading that cuts many times across the thread in order to produce the final threads. Below are several examples of ways to achieve multi pass threading

7 7 de 15 27/01/ : This is fanuc style canned cycle G76P(m)(r)(a) Q(d min) R(d); G76X_ Z_ R(i) P(k) Q(dd) F(l); m = Number of finishing cuts r = Chamfering amount a = Angle of tool tip d min = Minimum cutting depth (specified in radius value) d = Finishing allowance (in radius value) X = X axis destination Z = Z axis destination i = Taper value (in radius value) k = Height of thread (in radius value) dd= Depth of first cut (in radius value) l = Lead of thread Example: G76 P Q100 R200; G76 X60.64 Z 25. P3680 Q1800 F6.; Cuts a thread with one finishing cut, no chamfer on the exit of the tool, with a tool tip angle of 60deg. It will have a minimim depth of cut of.1mm and will have a finishing allowance of.2mm. The minor diameter of the thread is 60.64mm and it will cut a thread 25mm long in the Z minus direction. The height of the thread is 3.68mm and the depth of the first cut is 1.8mm and the thread has a lead of 6mm. This thread is a straight thread with no taper. (q and a borrowed from cad_cam_edm_dro group about 2002) Are Q, R, I, and the second P always in the implied decimal format? Since Z, X, and F are decimalized, it seems kind of strange to mix the two in the same code doubly so since retrofits have all kinds of different resolutions. Yes for some reason Q,R,I and the 2nd P are as I put in the example, I don't know why but as I said all three Fanuc machines that I have use the same format. Possibly this could be changes in the parameters of the machine. I'm a bit unclear the effect of the chamfering amount in the second two chars of the P word. Is the thread chamfered with the threading tool explicitly by the G76 cycle? Seems like one would want to to this with another tool, but I guess it could be pretty convenient though as part of the threading action. Or is this just "stay out" information so the cycle can be optimized? The chamfering amount is on the retraction of the tool at the end of the thread. If you leave this amount at 00 the thread will end in a groove (no chamfer) but if you use 05 this will chamfer the thread out to the major diameter of the thread for a distance of 5mm Macro Canned Cycle The following specification is from a company that wishes to remain nameless here. I'm told that this is the Swiss Army Knife of thread cutting systems. It used a common g33 call but repeated for the number of passes needed to cut and spring the threads to near perfect. Gxxx LATHE THREAD CYCLE <OD/ID/TAPER/MULTIPLE START/VARIABLE LEAD> Inch/Metric? Absolute G90 Mode Only With The Exception of M3/M4 No Other M or G Codes Allowed

8 8 de 15 27/01/ :20 NOTE: CYCLE IS DEVELOPED FOR DIAMETER COMPENSATION, G41/G42 AN ENDS IN G40 MODE. CYCLE WILL POSITION Z AXIS (1) PITCH +.11 INCH, 2.76 MM BEFORE G33 IS ACTIVATED. Gxxx FORMAT: REQUIRED: Gxxx B..E..J..O..R..U..V..W..Z.. OPTIONAL: N..Gxxx A..B..C..D..E..F..H..I..J..K..M..O..Q..R..S.. W..X..Z.. NOTE: Because of 80 character line limitation, it may be nec pass in letter address values, in Two or More Lines. S FORMAT: N10 Gxxx A..B..C..D..E..F..H..I..J..K.. First line up to 80 N20 M..O..Q..R..S..U..V..W..X..Z.. Second line up to 80 cha NOTE: CYCLE WILL NOT EXECUTE AXIS MOTION UNTIL Z VALUE IS PA ALWAYS PASS IN Z VALUE IN LAST LINE. LETTER ADDRESS ASSIGNMENTS: A = Infeed Angle. <10 Deg. Default> B = Number Of Rough Passes. C = Number Of Spring Passes. <0 Default> D = Variable Lead, Final Lead Value At End Of Thread. <Default E = Initial Lead Value At Beginning Of Thread. <Pitch> F = Positioning Feedrate. <Default Modal Rate> H = Number Of Thread Starts (1 Start Default) I = First Pass Incremental Depth. <Default Cycle Calculated Dep NOTE:IF "I" IS PASSED IN, THEN ALL SUCCESSIVE ROUGH CUT DEPTHS <TOTAL DEPTH 1ST DEPTH/NUMBER OF RGH. CUTS 1.=SUCCESSIVE D E.G. ( /10. 2.)=.0047 FOR EACH SUCCESSIVE PASSES. IF "I" IS NOT PASSED IN, THEN ALL ROUGH CUT DEPTHS WILL B BY CYCLE. <TOTAL DEPTH/SQUARE ROOT OF NUMBER OF CUTS=1S <SQUARE ROOT OF LAST CUT+1. * 1ST DEPTH=SUCCESSIVE DEPT E.G. (.0625/SQRT(10.)=.0198) 1ST DEPTH SQRT(2)*.0198= = ND DEPTH SQRT(3)*.0198= = RD DEPTH, ETC. J = Finish Pass Incremental Depth. K = Plus Or Minus Taper Per Inch/Millimeter?. Plus Taper = +Z D Example of Plus Taper.75/ft = K,.75/12. or K.0625 Example of Minus Taper.75/ft = K,.75/12. or K.0625 <0 Taper Default> NOTE: CYCLE WILL CONVERT DIAMETER TAPER INTO RADIUS TAPER, M = Spindle On, M3 CW/M4 CCW. O = Tool Orientation. 1, 1, 2, or 2. O = 1. OD Thread Tool Tip +X Direction O = 1. ID Thread Tool Tip +X Direction O = 2. OD Thread Tool Tip X Direction O = 2. ID Thread Tool Tip X Direction Q = Pull Out At End of Thread. <Default X Retract And One Rev. Q = 1. X Z Retract At 45 Degrees And Thread Lead Feedrate. NOTE: 45 DEGREE RETRACT, WILL POSITION Z AXIS PAST THE Z FI EQUAL TO THE DEPTH OF THREAD, PLUS L842 VALUE.

9 9 de 15 27/01/ :20 R = X axis Incremental Start/Retract? Clearance Distance From S S = Spindle Speed. U = Minor Diameter. <Smallest Starting Dia.> V = Major Diameter. <Largest Starting Dia.> W = Z axis Absolute Start Thread Position. <Thread Face> X = X axis Absolute Center Position of Thread. <X0 Default> Z = Z axis Final Absolute Thread Position. EXAMPLES OF CALL TO FOLLOW: #1) Turn a straight, single lead outside diameter thread, which dia. of 5.0" and minor dia. of 4.5". Threads per inch equal clearance equals.1". A 45 deg. X Z retract is required rough passes, and 3 spring passes. First pass depth equal Finish pass depth equals.01. The tool tip points in a plus The absolute position of thread depth is Z 1.5. The absolut thread start is Z0. CALL LINE: Gxxx B8. C3. E,1./10., I.05 J.01 O1. Q1. R.1 U4.5 V5. W0 Z 1 NOTE: "I" first pass depth was passed in equal to.05, there successive passes will be of equal depth. #2) Same example as #1, but make this thread a minus.75 taper Create a (2) line call. CALL LINE: Gxxx B8. C3. E,1./10., I.05 J.01 K,.75/12., O1. Q1. R.1 U4. W0 Z 1.5 #3) Same example as #1, but add 100 RPM spindle speed, CW direc make multiple start threads equal to 4 starts. Create a (2) CALL LINE: Gxxx B8. C3. E,1./10., I.05 J.01 O1. H4. Q1. R.1 S100 M3 U4.5 V5. W0 Z 1.5 PARAMETER ASSIGNMENTS: Lx27 = Rough Pass Counter Lx28 = Spring Pass Counter Lx29 = Incremetal Clearance Z Ramp on <Init L inch> Lx30 = Z Axis Start G41/G42 Ramp on Lx31 = Incremental Clearance Final Z Ramp on Position <Init 1 P Lx32 = Z Axis Start After Ramp on Lx33 = Average Depth Of Successive Rough Passes Lx34 = Start/End? Taper Radius Factor Lx35 = G00/G01 Mode When Cycle Is Called Lx36 = X Axis Clearance Position At Start Lx37 = X Axis Cut Position At Start Lx38 = X Axis Cut Position At End Lx39 = X Axis Position At End Of 45 deg Out feed Lx40 = Z Axis Position At End Of 45 deg Out feed Lx41 = X Retract Position At End Point Lx42 = Incremental Clearance X Axis At End Of 45 deg Out feed Lx43 = X Axis Position At Ramp on Lx44 = Z Axis Position Of End Point Relative To Infeed Angle Lx45 = Incremental Multiple Start Spindle Angle

10 10 de 15 27/01/ :20 Lx46 = Multiple Thread Start Counter Lx47 = Spindle Angle Synchronization Lx48 = Tangent Function Of Infeed Angle Lx49 = X Directional Sign Lx50 = Z Directional Sign Lx51 = Cutter Left/Right? G41/G42 <While Cutting> Lx52 = Cutter Left/Right? G41/G42 <Retracting Cut> Lx53 = E Word Value For 1 Spindle Rev., On Retract From Thread Lx54 = E Word Value At Start Of G33 L854=SQRT(SQ(initial lead) 2.*L831*L855) Lx55 = D Word Value At Start Of G33 L855=(SQ(final lead) SQ(initial lead))/(2.*thread length Lx56 = Calculated Depth Counter Lx57 = Accumulated Total Calculated Incremental Depth 5. Constant Surface Speed Constant surface speed is an essential tool for the lathe programmer. It is used to improve surface finish when facing or when turning. There is a very quick but comprehensive pdf that introduces the use of it here. [CSS] G50 Maximum Spindle RPM G96 Constant Surface Speed G97 Constant Surface Speed Cancel 6. Sam ple Threading Program s 6.1. Synergy 1/4 20 thread program Parameters Class name: American Standard Thread Class 2 External Class id number: Name: _AS Type: External Tpi: 20 Major diameter: 0.25 Pitch diameter: Minor diameter: Angle of thread: 60 Initial depth: 0.02 cleanup passes: 2 Synergy How to To actually create the thread do these 4 steps after starting Synergy: 1) Hit the Turn tab 2) Tools >Read: Read in an odthreading tool Tools >Read Tool ( 3) Macros >Threading: pick the tool, the thread type and the 0. Specify the start position in Z (.1? ), End pos Z ( 1? ), it but the answers are ignored ( I know, why ask, but it uses the 4) Execute >Default Lathe: Give it prog. name ( prog ) and ID #

11 11 de 15 27/01/ :20 Edit >CNC Output: Gives you.. G code Program %1234 ( ****PROGRAM **** ) (*** T0101 *** odthd.60deg_q1 ***) N1G50X5.Z5.S1500 N2G00T0101M38 N3G96S410M08 N4M03 N5G0X.35Z N6X.21 N7G33Z F.05 N8G0X.35 N9Z N10X.1984 N11G33Z 1.F.05 N12G0X.35 N13Z N14X.196 N15G33Z 1.F.05 N16G0X.35 N17Z N18X.196 N19G33Z 1.F.05 N20G0X.35 N21Z5. N22X20. N23G00T0100 N24M09 N25M30 Credit Bob Schuppel * bobs@webersys.com * (262) * Weber Systems * W134 N5514 Campbell Dr.* Menomonee Falls, WI Roltek Sample Threading Program This program shows some modification of a 1/4 20 thread. Fanuc post G code program ( ****PROGRAM **** ) (*** T0101 *** odthd.60deg_q1 ***) % (1/4 20 THREAD) N0010 T0100(INDEXING TURRET TO TOOL) G50 S2000 G96 S410 M3 M8 G0 X.35 Z.1 T0101(CALLING TOOL OFFSET ON 1ST RAPID MOVE) X.2231 G32 Z 1. F.05

12 12 de 15 27/01/ :20 G0 X.35 Z.1 X.2079 G32 Z 1.F.05 G0 X.35 Z.1 X.1959 G32 Z 1.F.05 G0 X.35 Z.1 (2 SPRING PASSES AFTER FINAL DEPTH) X.1959 G32 Z 1.F.05 G0 X.35 Z.1 X.1959 G32 Z 1.F.05 G0 X.35 G0 X5.0 Z.1 M30 % Credit Roltek 7. Mastercam Threading Param eters Pages

13 13 de 15 27/01/ :20

14 14 de 15 27/01/ :20

15 15 de 15 27/01/ :20 EmcKnowledgeBase RecentChanges PageIndex Preferences LinuxCNC.org This page is read only. Follow the BasicSteps to edit pages. View other revisions Last edited August 25, :46 pm by Chris Morley (diff)published under a Creative Commons License