Newbie- Okuma cadet 4020 mill m&g codes

[Al53154]

I cannot get this machine to run a M98Pxxxx sub program in EIA.
Machine skips right over the M98 Pxxx command and goes to the next position.
It also does not recognize the G98 command when drilling tapping. I need to jump over clamps ect.
It alarms out with alarm# 425 Alarm B unusable g code 62.

Does anyone have a list of M&G codes for this machine?

Thanks, Al

[BlueChip]

You are programming with Fanuc format ... the OSP is different :

M98 P1234 would be CALL O1234

No G98 ... you need :

G71 Z ( this is your initial plane ... this block is prior to your canned cycle call )
M53 is G98
M54 is G99

Hope this helps ...

Real World machine Shop Software at ... Kentech Inc. - Real World Machine Shop Software

Want to convert your Fanc programs to OSP ... or OSP ones to Fanuc ??
Check out CNC XChange from Kentech Inc.

[Al53154]

Thank you very much BlueChip. All is good now

[Al53154]

What is the OSP command that would work the same as the Fanuc M99?
I want the program to keep running untill I stop it.
This is a new (old) machine and I would like to keep it cycling the program it's going to be running for a day or two to see if there are any problems with it.

Thanks, Al

[BlueChip]

The command RTS is used at the end of a subprogram ... like M99 on the Fanuc.

Real World Machine Shop Software at ... Kentech Inc. - Real World Machine Shop Software

[Perfect Circle]

Try this link out

Okuma Lathe G M codes G-codes M-codes

Hope this helps you, though its for a lathe =/
Good Luck~!

[Al53154]

RTS works fine for the sub prg. I want to keep running the main program, without having to press cycle start each time. RTS in place of M30 in the main alarms out.
Thanks again, Al

[littlerob]

right before the end of the program. Enter this exactly;

GOTO N100

on the second line, at the top of the program enter this;

N100.

This will loop the main.

Robert