Heidenhain iTNC 530 G200(pecking cycle)

[DULING]

Does anyone have information on how to program a pecking cycle (G200) on a tilted work plane?

I am trying to define this peck cycle on a FPT machine with a rotating head. I am trying to use G80 to set my working plane but when the drill enters and retracts out of the hole it is not makiing a linear move that follows the axis of the drill.

[cnc_ken]

Looking at your ISO program it doesn't look like your drilling on a tilted plane, but drilling in 5-axis. I believe the drill cycles only work when you define a work-plane. You'll probably have to have your post put out all drilling moves longhand. Good luck!

[hansdie]

You seem to have major problems with your posted program.

1. Don't use m128 while drilling thats for "tool center point managment".
2. use g80 to set the work plane
3. call the drill cycle after you've defined it using m99 or g79
ie
N7 G00 X+0 Y+0 A+0 C+0 G40
N8
N9 M03
N10 M08
N100 G200 Q200=+.01 Q201=-1.25 Q206=+30 Q202=+.01 Q210=+0 Q203=+0 Q204=+3 Q211=+0
N11 G00 X+0.0175 Y-3.1286 A+14.951 C-37.672
G80 A+14.951 C-37.672
M99
N14 G00 X+0.5914 Y-3.883 A+18.661 C-36.182
G80 A+18.661 C-36.182
M99
N17 G00 X+0.6207 Y-4.95 A+23.97 C-38.417
G80 A+23.97 C-38.417
M99

also check that your tool/head has enough clearence when it rotates to the new positions

[kwanthay]

Why don't you guys use Plane Spatial ? That's very smart !