Did you figure this out? Instead of G54, G55 like you would use on a Fanuc based machine, you use G15H1, G15H2, G15H3, etc...
For tool height offset, instead of G43 H1, H2, H3 like Fanuc, you use G56H1, G56H2
The way you put your program name in the file is $programname.MIN So the "$" at the beginning is important and the ".MIN" is important(.MIN is OKUMA's nc code extension)
You must have a % at beginning and end of program. Below is a quick example of a program that really does nothing but touch the top of a part where the Z work offset is off the top of the part. Items in parentheses are just comments and aren't read by the machine. Those are just there for your clarification. Hope this helps!
$PROGRAMNAME.MIN%
G30 P1 (SEND SPINDLE UP)
M6 T2 (CHANGE TO TOOL 2)
G0 G90 G15H1 X0 Y0 (RAPID TO THE ABSOLUTE POSITION OF X0 Y0 IN WORK OFFSET 1)
G0 G56H2 Z3. (RAPID TO 3 INCHES ABOVE THE PART, CALLS FOR TOOL OFFSET 2 TO BE USED WITH TOOL 2 CURRENTLY IN SPINDLE)
M8 (COOLANT ON)
G1 Z0. F10. (FEED TO THE TOP OF THE PART AT 10 INCHES PER MINUTE FEED RATE)
G00 Z3. (RAPID TO 3 INCHES ABOVE THE PART)
M9 (COOLANT OFF)
M5 (SPINDLE OFF)
G30P1 (SEND SPINDLE UP)
G0 G91 Y50. (SEND TABLE FORWARD)
M02 (END OF PROGRAM)
%
okuma cadet mate osp700m
Reply with Quote
