[shaikaa1]

How i cancel G92 command?

haas mill c.n.c

[dcoupar]

One way is to G28 the machine and G92 X0 Y0 Z0. Why are you using G92? You should be using G54-G59, etc.

[shaikaa1]

G92 I used to move a subroutine several times a constant distance

and how i wright what u said?

mdi

g28;
g92 xo yo zo;

??

[Geof]

Get your Haas manual and read about G10 and G52.

With G10 you can enter G54 (and all the others) work coordinates froma program. For instance G10 L2 G90 P1 X Y Z enters whatever values you put with the X, Y, and Z into the G54 offsets. This means you can move your work zero around to use a subroutine at different locations.

G52 X Y Z creates a secondary work zero with reference to you main work zero and you can use a different G52 location for each subroutine.

These can be better than G92 because with G10 your work zero is at the location you defined and with G52 you can cancel it by using G52 X0. Y0. Z0.

[SeymourDumore]

First, you do as Dcoupar says. Use G28 or G00 G53 X0 Y0 Z0 to move absolute home, then type G92 X0 Y0 Z0.

Second, you cancel it in your head by NEVER EVER using it again!!!:stickpoke

Geof's post explains all the other, insourmountably superior alternatives to G92.

[charger19690]

I completely agree with the previous posts...

Do Not Use G92

I get into this argument alot at work with my boss and management and if you are not familiar with the way each machine uses this code and how to re-designate it to machine Zero there can be numerous issues with this code. I have seen many crashes from this code because people cannot get it back to Machine Home.

And, each time I would have to get that machine book out to find out how to re-designate the machine home.

G10's are the way to go.

Mike in MN
http://www.cncbasics.com
http://www.cncbasicsforum.com

[HuFlungDung]

It is a good thing to thoroughly understand G92, even if you don't use it (much). It can be very very handy with 4th axis work.

I think in the Haas control, you can always go into the work offset register and see what residual value has accumulated in the G92 offset (down at the bottom). It might be worth a shot to command G92 X0Y0Z0 and see if it zeroes the register values. Then return to machine home and check the register again. If it shows a value, then command G92 X0Y0Z0 again.