1. ## Single surface probing

I have a part (casting) I getting ready to machine and need to probe one surface in the y axis and translate that edge info. to the center line of the part.
Using single surface #11 in the work offset page how do you pick up one surface and move it to another location and set you work offset to that postion?

Part is 2.00 wide and need to set y0.0 at centerline. I need to translate from a Datum to centerline of the part?

Or is there another approach I need to take?

Thanks Don.

2. Is it not possible to run the y-web cycle? Then it will automatically locate to the center.

If not, you will have to insert a code like the following after it sets the single surface:

Assuming G54, the macro register for G54 y axis is #5222

#5222 = [#5222+1.0]

Use +1.0 or -1.0 depending on which direction you are shifting.

Hope this helps.

3. If you use the above example, you'll also need to move the Y zero back to where it was probed. Using his example:
%
#5222=#5222-1.
(probe)
#5222=#5222+1.

Or else it'll just keep moving 1" every time. I wouldn't do that. Depending on where you restart in a program, you could get screwed up in a hurry.

Simpler: G52 Y1.

Make sure to call G52 Y1. at each tool change. Then you can start at any tool change and have the correct location. If there's lots of tool changes:

G52 Y[#500]

Then simply changing #500 will move ALL G52 calls.

4. Originally Posted by Matt@RFR
If you use the above example, you'll also need to move the Y zero back to where it was probed. Using his example:
%
#5222=#5222-1.
(probe)
#5222=#5222+1.

Or else it'll just keep moving 1" every time. I wouldn't do that. Depending on where you restart in a program, you could get screwed up in a hurry.

Simpler: G52 Y1.

Make sure to call G52 Y1. at each tool change. Then you can start at any tool change and have the correct location. If there's lots of tool changes:

G52 Y[#500]

Then simply changing #500 will move ALL G52 calls.

Good call! Didn't really think that one all the way through for potential problems.

6. Thank you both, I will give that a try.

Thanks Don

7. So here is what I did.

G52 Y-.9842 This set me at my centerline I was looking for. I also had to add G52 Y0 before my next WPC call out. Same tool working at G54 and G55 I had no need to shift G55. It works but is this the correct way to do this? Setting #33 to fanuc

Thanks for the help.

8. Yeah, in that case I would do:

G52 X0. Y-1. Z0.
G54 M97 P100
G52 X0. Y0. Z0.
G55 M97 P150

ETC.

If you're only changing Y with G52, you don't have to type X0. or Z0., but I find that it's a nice insurance line for those times you have to start at any given tool on any given work offset. But again, not mandatory. Only M30, Reset, power off or a G92 call will reset your G52 registers.

9. Cool, Big thanks for the help.