O.D. milling with live tool

[jackson]

I have a Daewoo Lynx 220LM Fanuc oi-tc

i am sloting the outside od of a part, almost like cutting gears, i can cut them just fine the problem im having is that i cant find the right code (i guess) to make the tool retract at the end of the cut it just wants to rapid strait back out witch makes since because im actualy using a drilling cycle to do this so i need the right code if anyone knows what is is it make my life much easier i have not looked in the book yet just g code list
thanks

[dcoupar]

Jackson,

I'm guessing you're using a G83 to do the cutting? There is no code I know of to pull the tool up at the end of the cut before rapiding back to the start (Too bad you can't use a G92 threading cycle).

Why not use a subprogram?

Position the tool to the start of the first slot, then call the sub for the number of slots you need.

01001(MILL 10 SLOTS @ 36 DEGREES)
G28 U0 W0
T0202 (END MILL - LIVE X)
M05(STOP MAIN SPINDLE)
M35(SELECT REV. TOOL)
G97 S2000 M33
G54 X1.6 Z0.1 M08
M98 P00101002 (CALL SUB 1002 10 TIMES)
G00 M09
G28 U0 W0 M35
M30

O1002(MILLING SUB)
M89 (CLAMP C-AXIS)
G00 X1.4 (RAPID X TO CUTTING DEPTH)
G01 G98 Z-1.1 F10.0 (FEED TO BACK OF PART)
G00 X1.6 (RAPID X TO CLEAR)
M90 (UNCLAMP C-AXIS)
Z0.1 H36. (RAPID Z TO CLEAR & INCREMENT C)
M99

[Geof]

Does your controller recognise the G86 command. This is Bore and Stop; the cutter feeds to a Z depth and stops, then I think you can move the cutter away from the part before it retracts so you don't leave a mark from the retraction.

Go read the book .

[jackson]

Originally Posted by Geof Does your controller recognise the G86 command. This is Bore and Stop; the cutter feeds to a Z depth and stops, then I think you can move the cutter away from the part before it retracts so you don't leave a mark from the retraction. Go read the book .

My control recognizes G85 boring cycle witch is what im using, and it is working i was just wanting to retracted + in X. and i tool a little time and look through teh book but i have not found what it is exactly im looking for, i found cylindrical interpolation but that is not what im wanting unless i can alter it to make it work

[dcoupar]

According to my 0i-TC manual, G86 isn't supported. On a 0i-MC, G76 (Fine Boring) will stop the spindle and shift away, but not on a TC.

I don't think cylindrical interpolation will do you any good.

Didn't like the subprogram idea, eh?

[jackson]

Originally Posted by dcoupar According to my 0i-TC manual, G86 isn't supported. On a 0i-MC, G76 (Fine Boring) will stop the spindle and shift away, but not on a TC. I don't think cylindrical interpolation will do you any good. Didn't like the subprogram idea, eh?

Well i only had a couple of prototypes to make so no didnt want to mess with that much work i did save that sample that you posted thanks, if i do any more i may give it a shot, im not big on sub programing, i just dont much of it