How do I cancel a G92 on the fly?

[Apollopeon]

Hello everyone. I just got a refurbished toshiba mill with a Fanuc 31i controller. Does anyone know how to cancel a G92 on the fly? I was using a Tosnuc 888 and it was just a matter of a G53 and recalling the fixture offset. This isn't working for me on the Fanuc.
Any help would be appreciated.
Thanks.

[HuFlungDung]

Does your mill have a G53 machine coordinate system? Does it have work offsets?

Worst case, (it has none of the above) you must return the machine to home, then re-command the G92 at that position. That is the most straightforward method of keeping track of the coordinate system shift.

[stevo1]

Applo,
Hu is correct. If you are not keeping track of what you are changing your G92 to and you want to reset it back to original state then you have to send the machine home then recall the G92.

There are a few other things that you can do to make this easier. You can create a custom G or M code that will call a macro program were you then can put the code to return it home and reset G92. It makes it easier for programming.

What exactly are you trying to do?? Why G92 instead of G54-G59?

Stevo

[Apollopeon]

I am mainly using it for running a thread milling sub in multiple locations. I also use it when I have many details that are identical in different locations. I just find it easier to program the sub programs this way. At least it is on a Tosnuc 888 control.

[dcoupar]

I might suggest you re-do your subs in incremental and simply move in absolute to the starting location of each hole and call the sub.

[ChattaMan]

Can your machine use G52?
It's similar to the workshift, but used "on the fly"

G52 X10 Y10 Z10 shifts your datum
G52 X0 Y0 Z0 Shifts your datum by zero, e.g. 'cancelling' the shift amount "on the fly"

[Arlo Tol]

Friendly advice... stay away from the G92 funktion..
It brings more trouble than comfort in my opinion and experience.

For workshifting e.d. use the G52, work incremental G91. or my personal favorite, hard-input workshift or zeropoints into your program.. using G10..