5X drill output on mill-turn

[jcrook]

Hi,
I am drilling the OD of a cylinder. I have a Daewoo Puma Mill-Turn, Fanuc 16T. It is an X,Z,C type setup. My workcell in Pro-E is setup as 5-axis. The tool axis for these holes is PARLEL X. We are currently using G-post utilizing merged posts, PARLEL X(UNCX01.F02), PARLEL Z(UNCLX01.F12), and a regular turning post(UNCL01.F02). My question:
Pro-e is outputting a RAPID, GOTO/, a CYCLE/DRILL, GOTO/ again and then a CYCLE/OFF for the 1st hole in the CL file. The subsequent holes are output as RAPID, GOTO/, RAPID/, GOTO/, CYCLE/DRILL, GOTO/, CYCLE/OFF. Seems to be an extra RAPID/ and GOTO/ for holes 2-8. I currently have 8 holes programmed. The extra RAPID/ and GOTO/ is caused by the Retract Cylinder dimensions being re-output. This may be causing my issue.
I've been in the OFG, can't find any settings to change this output. I tried changing the setting on the "Identical Points Handling" page under "Motion" -> "General". This did not change output. I've been to the parameters page of the machining sequence. The only setting I find is CYCLE_OUTPUT that might influence the output. The 2 options are BY_HOLE or BY_HOLESET. I've tried both, no difference. I even changed the SCAN_TYPE to different setting, no difference either.
I don't know if there's an additional setting in the Plabel file under "Advanced" in the OFG that I don't know about. It's manageable, I just edit the NC code, but I don't want to do this. Any ideas?
Do I need to handle all this in the FIL file, search ahead in the CL file for each additional CYCLE/DRILL and get the endpts and output them? Seems extremely unnecessary.

Thanks in advance for any help,
Jay Crook.
<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />

 

[chf65]

jay,

None of these parameters affect this GOTO. This is due to the retract surface because Pro/NC is making the extra moves to take you to the retract cylinder between holes (basically, doing what you asked it to do).

Just remove the retract cylinder, and make sure though that your CLEAR_DIST, PULLOUT_DIST and RAPTO_DIST are set correctly to clear your moves.

 

[jcrook]

Thanks Charles,


I adjusted the CLEAR_DIST to match the cylindrical retract plane and this eliminated the extra X and Z move between holes. I need a retract because the alternative is selecting the part OD. I still have the G80 M90 drill cycle cancel and spindle un-clamp between holes, but this will work.


M1
(NO.4 CDRILL, RADIAL ROTARY)
G0 G20 G40 G97 G98
M35
G28 H0.0
G50 C0.0
T0404
M33 S1200
/G1 X10. Z-.313 F350.
G0 X10. Z-.313 C135.
X2.2 Q1000 M8
G87 X1.37 Z-.313 R0. C135. Q1000 F3.5
G80 M90
G87 X1.37 R0. C180. Q1000 F3.5
G80 M90
G87 X1.37 R0. C225. Q1000 F3.5
G80 M90
G87 X1.37 R0. C270. Q1000 F3.5
G80 M90
G87 X1.37 R0. C315. Q1000 F3.5
G80 M90
G87 X1.37 R0. C0. Q1000 F3.5
G80 M90
G87 X1.37 R0. C45. Q1000 F3.5
G80 M90
G87 X1.37 R0. C90. Q1000 F3.5
G80 M90
M9
G0 G80 G18 X10.0 Z8.0
/G28 U0 W0 M9



The Fanuc control is set to look for an incremental R distance from retract plane to a clearance point to start drilling from not an absolute diameter. I still haven't figured out why it outputs a CYCLE/OFF after every CYCLE/DRILL. This only appears in 5X mode and using a CSYS with Z pointing up through what would normally be X axis. I've tried selecting 3X but you have to create a CSYS thru the center of each hole. Maybe this "IS WHAT IT IS" and I'm going to have manipulate the output in the FIL file.


CYCLE / DEEP, DEPTH, 0.315000, STEP, 0.100000, IPM, 3.500000, CLEAR,$
0.100000
GOTO / 0.0000000000, 1.0000000000, -0.3130000000, $
-0.0000000000, 1.0000000000, 0.0000000000
CYCLE / OFF
CYCLE / DEEP, DEPTH, 0.315000, STEP, 0.100000, IPM, 3.500000, CLEAR,$
0.100000
GOTO / -0.7071067812, 0.7071067812, -0.3130000000, $
-0.7071067812, 0.7071067812, -0.0000000000
CYCLE / OFF
CYCLE / DEEP, DEPTH, 0.315000, STEP, 0.100000, IPM, 3.500000, CLEAR,$
0.100000
GOTO / -1.0000000000, 0.0000000000, -0.3130000000, $
-1.0000000000, 0.0000000000, -0.0000000000
CYCLE / OFF



Thanks, Jay.