Trying to loop incremental code

[jaco...@gmail.com]

I've got a project that has repetitive features (blades) about the b table axis. The gcode for a single feature is about 5mb, so having all 6 features is too big. I changed the code to incremental and ran a few minutes of it on the PNC to verify the code generated correctly. My thought was that I could make the code a sub program and run a macro loop to call the code 6 times. When I made a sample macro the PCN gave the warning that M97 and M98 were not recognized codes.

Are there any other suggestions on how to loop a code multiple times and rotate the B table an additional angle between code repetitions?

[Manohj Kumaar]

Hi Jacob,

If all of your blade profiles are same you can use circular pattern to do 3+1 axis machining. Hope this will help out

[jaco...@gmail.com]

Manohj,

I don't know what you mean by circular pattern. I know how to make the full 360 pattern in cam. The challenge is that I can't have them all in one .nc file and I don't want to have to baby sit my PNC and load 6 different files throughout the day.

[Tokyo Pav]

I’m not sure if pocketnc has it implemented but you could use this kind of technique to overcome the issue.
http://wiki.linuxcnc.org/cgi-bin/wiki.pl?SubProgramFiles
Regards
TP

[jaco...@gmail.com]

Tokyo,

Thanks, that link set me to a path were I figured it out.

Subroutines were what worked, thought it seems the PNC doesn't support logical loops (IF, WHILE, etc). http://wiki.linuxcnc.org/cgi-bin/wiki.pl?SubroutineSample

So here is a sample code to explain for others how to repeat incremental or absolute code.

(Start of file)

#500=0 (#500 is an example variable with a starting value of 0, will be used for B angle)

o1000 sub (start of subroutine code to be repeated)
G0 B#500 (rapid movement to B angle stored in #500 value)
(Your g-code here)
o1000 endsub

o1000 call (first call of the subroutine with B = 0 deg)
#500 = [#500+90] (increases stored value of #500 by 90)
o1000 call (2nd call of subroutine, now with B = 90 deg)
#500 = [#500+90] (increases stored value of #500 by 90)
o1000 call (3rd and final call of subroutine, now with B = 180 deg)

M30 (end of file)

Depending on if you have incremental or absolute will change how you do things, but this is an example of what I'll use.

[Tokyo Pav]

Excellent work. Thanks for posting how you implemented the solotion. This will help others for sure.
Regards
TP

[joum...@gmail.com]

This work will definetly help me later on.
Thank you so much!

[joum...@yahoo.com]

It seems I am struggling with the call function...
I did include sub and endsub before the call in the same program, but I get an error: cannot find O100 file.
I manage with a while endwhile loop without the call function.
But I am curious about the exact way of calling subroutines...
If someone can help.

[Ross D]

Hi, Thank-You, I used your example, worked GREAT !!   In the past I've only ever used the old Fanuc method with M97, M98, M99  Thank-You again