Need Help!- Old, tired and confused...

[Buzzwerk]

I got back into the prototype business after a looooong hiatus and I'm trying to get caught up on all this new fangled CNC stuff. I'm bleary eyed as I write this question hoping someone on this board could/would help me out.

We usually do "one off" projects, but sometimes we will do multiples. At times, the parts can be somewhat complex and therefore programming intensive. I'm using ProManufacture (ugh) to program/generate tool paths and it does not allow me to duplicate "operations" An "operation" is ProManufacturese for a program. I am wanting to have the machine complete a program and than step over and repeat the program. (because I'm old and tired and I don't want to have to completely re-create a program so I can run more than one part)

There has to be a way to edit the post and to step over in "X" and or "Y" and repeat a whole program.

As I said, I'm old and confused and I'm getting cranky trying over and over to edit the post so the program will run until it's finished and then step over in "X and/or "Y" and start again. The owner is getting pissed off with me using machine time to try and figure out.

It's probably just a matter of just adding a few lines of code into the post but I can't for the life of me figure it out. Please and thank you.

BTW: We running HAAS machining centers.

[KenFoulks]

Check out Haas' forum, there is a similar question:

http://atyourservice.haascnc.com/faa...-machine-tool/

[plastibob]

If your talking pro/e mfg you can accomplish this a number of ways.

1) you can handle at the controller & Gcode level.
2) you can pattern toolpaths or operation in Pro/e
3) you can translate toolpaths in Pro/e

[Buzzwerk]

Originally Posted by plastibob If your talking pro/e mfg you can accomplish this a number of ways. 1) you can handle at the controller & Gcode level. 2) you can pattern toolpaths or operation in Pro/e 3) you can translate toolpaths in Pro/e

I'm aware you can pattern individual "sequences" in ProMan and I do when it's efficient, but it is my understanding that one can not pattern "operations" (which is a drag because it would make things much easier and I wouldn't be asking the question I did). If you know how to pattern "operations" please share how it's done and I will be in your debt.

Anyhoo...a kind gentleman on a different thread suggested that since we drip feed our CNC's. I can easily edit the post, by copying and pasting of the original program and changing the g54 offset to g55, etc.

That's about the time I said DUH?!? and decided that I should cut down on my coffee consumption.

Thanks all!

[MrWild]

There is a way. You make an incrimental move to the new position and call it your new 0,0

[Geof]

You are using a Haas which can use local subroutines. Make your Promanufacture operation into a subroutine by numbering the first line N1000 and making the last line M99 instead of M30.

Now write a bit of code like this:

O00000 (Multi operation program)
G54 (set first work zero)
M97 P1000 (go to subroutine)
G55 (second work zero)
M97 P1000 (go to subroutine)
etc
etc
M30 (end program)
N1000 (first line of your subroutine, i.e the Promanufacture program)
etc
etc
etc
M99 (end of your subroutine)

There are other ways to do it but I think this is the easiest way.

[traceflair]

I like to fixture my parts a set length apart so instead of finding G55, G56, G57, etc. I simply find G54, have the subroutine change that G54 to the location of the next part, and then loop. Four parts would look something like this:

O001 (Main Program)
G10 L2 P1 G90 X__ Y__ (Setting G54 within the program)
G54;
M97 P1 L4;
M30;

N1 (Subroutine)
______; (Operations of the subroutine)
______;
______;
G10 L2 P1 G91 X3.; (Shifting G54 3" in the positive direction)
M99;

This saves time and reduces the margin for human error by only using one fixture offset instead of four.