[Mike Mattera]

My Fanuc 16M manual says That I can specify the number of times to repeat a sub, by using the P word.

The M98 Line below should repeat the call to sub 10, 5 times.

My question is...
Does this work on the newer controls?
Can this also be done with an "L" word (M98 P0010 L5)?

T1 M6
G0 X2. Y0. Z.1
G1 Z0. F10
M98 P50010
G0 Z.1
...
...
M30

O0010
G91 G1 Z-.2 F8.
G90
G2 X2. Y0. I-2. J0. F10.
M99


According to the manual you can have
P 0000 0000
(# of times) (Name of sub)

But the "M98 P0010 L5" is cleaner looking code.

Mike Mattera

[beege]

Not sure about the 16M, but M98P1234L5 repeats sub 1234 5 times. Pretty much the standard, I thought, but I've seen posts (forum posts) that mention M98P51234, where 5 is how many times to repeat sub 1234. I think there may be other variations. I wish it were completely standardized.

[Mike Mattera]

Thanks beege.

I figured both would work. P50010 is probably an older format. My book is from a class I took in 1996. It doesn't mention the "L" word any where. So P0010 L5 is probably the new and improved format.

Thanks again for the fast reply,

Mike Mattera

[thamain1]

But the "M98 P0010 L5" is cleaner looking code.

Mike Mattera

That is how I do it on a Fanuc and a Yasnac. In my shop we just consider "L" to be "loop". Such as in G13/G113 circular interpolation can be looped multiple times for finish etc.

[MBG]

On my haas sl-30 it is p (which is the line number) and then you have the L which is repeat..


Also, you have to put a M99 at the end of the program and then copy and paste the program to the end since that line reads PAST the M30...

[dcoupar]

On your SETTING (HANDY) page, there's a TAPE FORMAT setting.

If you set that to 1:F15, the format for calling a sub is M98 P#### L**** where L is the repeat count.

If you set it to 0:NO CNV, the format is M98 P***#### where *** is the repeat count.

I can't find what the other F15 format differences are, so changing this setting may have undesirable effects on your programs.

[g-codeguy]

Do any of you actually like running a program with this type of call? I suppose it would be okay with something like aluminum or brass. Materials we don't run a lot of. I don't like it because it treats your program as a sub. How do you re-run an operation with this type of call?

Only way I know is to call up the program, call up the line number for that operation, run that operation, and then go back the M98P******* program call again. This would run the program from the very beginning, wouldn't it?

Course I have to do the same thing anytime I need to re-run an operation that is run from within a subprogram. Maybe it is a case of being use to one way and not the other. However, I only program for lathes. In my case only the finishing operations are in a sub. If I need to re-run an operation, I will call up the sub, re-run the tool, and then finish the part while in the sub. Once the cut-off tool starts home I will hit feed hold, reset, call up the main program, & call up the block for the next subprogram operation...if necessary.

I am all ears if someone knows an easier way. Thanks.