Call local sub and G52 shift while in a canned cycle

[JWK42]

Here is something I didn't know could be done. I call the drill cycle then call the hole location sub N1610, then G52 program zero shift, then call hole location sub ect. all while still in the canned cycle. G80 turns it off after drilling 6 different parts 5" wide in 'X' and 3" wide in 'Y' . The L0 in the canned cycle inhibits the cycle until the next set of 'X' -'Y' values are found in the sub. I have only tested this on our Haas simulator.



%
O5555 (TEST G52 ZERO SHIFT)
N10 (WRITTEN 10-22-2008 09:26:05)
N20 (MODIFIED 10-23-2008 09:37:19)
N30 ( TOOL #1 IS A NO. 7 DRILL )
N40 G53 G00 Z0. ( RESTART TOOL #1 HERE )
N50 G53 G00 X-20. Y0.
N60 T1 M06
N70 S1234 M03
N80 G54 G00 G90 X1. Y1.
N90 G43 Z0.25 H1 D1 M08
N100 G81 G98 R0.1 Z-0.25 F6. L0 (Call Drill Cycle)
N110 M97 P1610
N120 G52 X5.
N130 M97 P1610
N140 G52 X10.
N150 M97 P1610
N160 G52 Y3.
N170 M97 P1610
N180 G52 X5.
N190 M97 P1610
N200 G52 X0.
N210 M97 P1610
N220 G80 (Exit Drill Cycle)
N230 G52 X0. Y0.
N240 G53 G00 Z0. M09
N250 G53 G00 X-20. Y0.
N260 M01 ( OP STOP )
N270 ( TOOL #2 IS A .25-20 TAP )
N280 G53 G00 Z0. ( RESTART TOOL #2 HERE )
N290 G53 G00 X-20. Y0.
N300 T2 M06
N310 S1234 M03
N320 G54 G00 G90 X1. Y1.
N330 G43 Z0.25 H2 D2 M08
N340 G84 G98 R0.1 Z-0.25 F50. S1000 L0 (Call Tap Cycle)
N350 M97 P1610
N360 G52 X5.
N370 M97 P1610
N380 G52 X10.
N390 M97 P1610
N400 G52 Y3.
N410 M97 P1610
N420 G52 X5.
N430 M97 P1610
N440 G52 X0.
N450 M97 P1610
N460 G80 (Exit Tap Cycle)
N470 G52 X0. Y0.
N480 G53 G00 Z0. M09
N490 G53 G00 X-20. Y0.
N500 M30 ( END OF MAIN PROGRAM )
N1610 (NO. 7 DRILL / .25-20 TAP)
N1620 X1. Y1.
N1630 X2. Y1.
N1640 X3. Y1.
N1650 X4. Y1.
N1660 X4. Y2.
N1670 X3. Y2.
N1680 X2. Y2.
N1690 X1. Y2.
N1700 M99
%

[Geof]

Yes Haas lets you do all kind of interesting things. I have done hole patterns where each hole has its own work zero with the hole placed at X0. Y0. and instead of editing in the program you just put the hole locations in the work zero table.