multiple vise's

[smitty]

Got another one for you pro's,
I have 2 vise's set up, and will be machining the same part on both vise's. Questions is, how do I program the second vise, without having to program the entire lengh from vise #1?
I think this is a sub-routine, but not sure how to do it.
Any advice you can offer would be great,
Smitty

[NeoMoses]

The first idea that comes to mind is to accurately measure the distance between vises, then model it that way in your CAD package, and generate the G-Code for the 2 vises at the same time, in the same file. This requires that the parts be set up exactly the same way in each vise each time, though.

My second idea would be to move the tool to the zero point on the second vise, re-sett the zero point while running the program, then re-run the existing code. Although I've never done this before, I believe a G92 is what you're looking for. Here's what is stated in the TurboCNC.txt file:

************ G92 Preload of registers/Set machine coordinates ************ This code sets the position of any or all axes to a specific value. Use this to reset the position inside a program. No motion will occur. Usage: G92 X0 ;Zeroes X axis G92 X0 Y0 Z0 ;Zeroes all principle axes on a mill G92 Z1.234 ;Z is now set to 1.234 You must be in the master coordinate system to use this code. All of the other offsets (1-20_ follow the master. Ergo, if the origin in offset 1 is set to be exactly 3" away from the master origin (in G53 mode), then that relationship is maintained as the master origin moves. Use jog mode to setup the coordinate offsets (tool offsets) and save them through the file menu. This command is not modal in versions 3.1 and up.

I'm not sure if there's a better way to do this, but those were the first 2 ideas to come to mind. Hopefully someone more experienced than myself will give you a better solution.

[DavidB]

Set vice one as G54,Set vice two as G55 to G59(GOG90G54XOY0 example).
Now with your program have a G54 at the start.
Copy and paste the whole nc file to the end of itself and change the G54 in the pasted program to G55.Check tool retracts to miss anything that might be in the way from when the tool finishes on vice #1 and to get to the start of program on vice #2.Hope this helped.
If your using a hedeinhan control this is no good,if so let me no and i'll tell you how

[DavidB]

Another way is a Datum shift and call program again. Good luck

[smitty]

Thanks for the help,
I will give these a try later today and post my results.
Smitty

[smitty]

Thanks for all the advice, lots of great info here!
I ended up using the G92 code, and then cut and pasted the needed info and let her run. Had to close my eyes at first, ok quick hand on the PANIC button, and all has worked out very well. Just need to make some minor adjustments and it is a done deal.
Now I know why programmers get paid so much, the de-bugging of the program can be nuts!!!
Smitty