[Hiredgun]

im making 2 parts that are the same. lets say they are 5 inches on apart on x axis how do you program for that. tormach with mach3. you use G54 i think but can someone give me an example.

[Geof]

The simple way is to use G54 for the work zero on one part and G55 for the work zero on the other, then just duplicate your program and run through the first section using G54 and the second section using G55.

This is simple but inefficient because you complete one part with all its tool changes before going on to the second part.

A more efficient approach is to put each tool in its own subprogram and then have a master program select the work zero and then call the subprogram.

The sequence is:

G54 (Select first work Zero)
M98 P(or O)1nnnn (Where 1nnnn is the program number for the tool 1 subprogram)
G55 (Select second work zero)
M98 P(or O)1nnnn
G54
M98 P(O)2nnnn (2nnnn is tool 2 subprogram)
G55
M98 P(O)2nnnn
etc
etc
for all the tools

[BobWarfield]

It's pretty straightforward. G54 through G59 give you 6 work offsets, in this case, you want to use 2 since you are making 2 parts.

So, let's say you use G54 and G55. G54 is at x=0, y=0 and G55 is at say x=5, y=0 if you want to offset it 5" in X. You set up the x and y offsets in Mach3.

Now, write a program as though there is one part. Stick G54 in front of it. Copy the code, and put G55 in front of the second part. Same code works for each one because the work offset handles the coordinate shift.

There are other ways to use work offsets, but that was the simplest explanation I could give.

Cheers,

BW

[mactec54]

Hi Hiredgun

If you don't want to do the sub program thing, there are other ways that are quite simple, but you need to write a little more code, or just cut & copy/paste the program, you only need one work offset for simple stuff

Just use your G54 X0Y0 this is your first work offset/part start point & the only one you need.

Don't forget A ( Z ) move up to clear your work before the( GOX0Y0 ) move if you tool is down you will crash into your work

G54
G90G0X0Y0
Part program
No end of program needed just the Z move

G0Z1.0 at end of program
G54
G90G0X5.0Y0 Next Part/second part position
Next Part Program or the same program as the first just cut & copy/paste


Program end
G0Z1.
M9
M5
G0X----Y----- were ever you want the machine to go
M30

[Hiredgun]

thanks for all the help guys that solved my problem quickly, thank you.