Need to trim chuck jaws on Older Cadet with OSP5020L. On Haas machines I use G72 canned cycle. Anyone know the equivelant on this Okuma? Thanks.
Need to trim chuck jaws on Older Cadet with OSP5020L. On Haas machines I use G72 canned cycle. Anyone know the equivelant on this Okuma? Thanks.
Okuma has a bunch of LAP cycles. Do you not have a book?
I do have a programming manual but the canned cycles are for threading cycles and drilling cycles. Not one of these seems to match to a simple OD turn or facing can cycle. I am sure this older controller to do the face and turn cycles especially since it can perform threading cycles, but I must just simply be overlooking them. A sample program line for facing would be most helpful. This is a Haas facing cycle I use alot and wish to repeat on the Okuma; G72P1Q2D.035F.004
Thanks again,
Wow. You are lost. Doesn't your machine have IGF programming? Part of what you were looking for is on the web page I referenced for you: "G85 Call of Rough Bar Turning Cycle (LAP)" and "G81 Start of Longitudinal Shape Designation (LAP)" and "G87 Call Finish Turning Cycle (LAP)". I bet if you searched deeper on the web you could come up with the syntax and parameters for these operations.
It's LAP (Lathe Auto Programming) for Okuma, not a "canned cycle"
Take an sample from manual and it will work.
and now for a useful answer
G85 is equivalent to Fanuc G71
G87 is equivalent to Fanuc G70
G81 marks the start of a longitudinal cutting contour
G80 marks the end of the contour
The contour is named N500
here's a simple boring program for Okuma ......
G00 X2.0 Z.1
G85 N500 D0.100 F0.010 U0.010 W0.005
N500 G81
G00 X2.5
G01 Z-2.0 F0.005
X2.0
G80
G87 N500
and for facing.....
G82 marks the start of a transverse cutting contour
G80 marks the end of the contour
The contour is named N600
here's a simple facing program for Okuma ......
G00 X8.0 Z1.0
G85 N500 D0.100 F0.010 U0.010 W0.005
N600 G82
G00 Z0
G01 X0 F0.010
Z1.0
G80
G87 N600
Do you have the manuals for what he's trying to figure out? I'm up against the same problem and have the manuals too. They aren't very clear on what's going on, and when you're coming from Fanuc on 5 different cnc lathes, and have that system engraved in your noggin on how to do things, it's as clear as mud.
- - - Updated - - -
...for anyone reading this thread without a manual..... here is list of G Codes for Okuma Lathe.
https://www.helmancnc.com/okuma-lathe-g-and-m-codes/
DJ