[GITRDUN]

Working on a Fanuc OM control, probably early 90s model. I am trying to use G10 as a work shift but having some trouble. I like to setup my work coordinate to be centered over the top left corner of a vice and then use work shifts in the program to reposition the 0 coordinates so all programs will be set by setting one work coordinate and i can use mulitple vices useing a different work coordinate for each if needed. I am familiar with using working coordinates and then useing the G52 work shift on Haas machines setup as Fanuc. Works great. But on the Fanuc OM when it reads the G10 line it replaces the specified work coordinate parameters with the specified parameters on the G10 line. And if you reset or end the program the work coordinate parameters do not reset to the origional numbers. Only way around that i can see is to give another G10 line at the end of the program to reset the G54 etc etc to its origional numbers, but thats a little over complicated and a bad way to do things. So whats the simple or proper solution to use G10 for a work shift and not a programmed working coordinate? Or am i trying to use it for something it wasnt intended for?
My work around so far is to program as follows.

G54 G00
G90 X0 Y0
G92 X Y Z
XO Y0
G43 H1 Z-.25
-
-
-
G91 G28 G00 Z0
G28 X0 Y0
M30

I havent tried this but i see no reason this wouldnt work. However i would like to use a simple work shift if possible to simplify things a bit.

[stevo1]

The quickest and easiest way if using the G10 would be to set variables equal to G54 before you start machining and then program them back at the end.
Ex. #2501 is X for G54, #2502 is Y for G54 and #2503 is Z for G54.

…start or program
#100=#2501
#101=#2502
#102=#2503
…
G10L2P1X()Y()Z()
…
...
G10L2P1X#100Y#101Z#102
M30

I would recommend that you keep your G54 as is (top left of vise) and never change it. This way you never have to worry about changing it back. You could then use G55-G59 and shift them all you want but you just have to have at the start of your program setting G55-G59 set to the value of G54. Say you want to use G55. These variables for G55 are #2521=X, #2522=Y, #2523=Z

…start of program
G10L2P2X#2501Y#2502Z#2503
G55
…
G10L2P2X()Y()Z()
…
M30

Also remember that you do not have to put the specific number in the G10 line. If you want to incrementally shift put a G91 in the G10 line. So if you program G91G10L2P1X2.Y2.Z2. it will add 2. to each existing value in the G54.

Stevo

[sinha_nsit]

This is fine (the variables are 2501, 2601 and 2701 for X, Y and Z of G54, in 0i series).
But if we are using system variables, what is the need for using G10?
A serious limitation of G10 is that it cannot determine the existing values; it can only overwrite or increment/decrement the current values.

Edit:
A power cycle clears the shift caused by G92 which remain valid only in the current machining session (a solution to your problem).

[Andre' B]

I do or have done all of the above and more.

In the end if you need to save a work offset location for long term nothing is better then a notebook and a pen.

[dcoupar]

We're assuming he has the User Macro option?

[GITRDUN]

So far i think the G10 is useless for what i am wanting to do with it. As Sinha stated the G10 can only over write the existing values which isnt what i need. I need to be able to call up a work coord, and then offset that coord by the amount specified in the program. So my work around was this.

G59
G54
G00 X0 Y0
G92 X Y Z
N1 M00
MACHINEING LINES -
-
-
-
G00 G91 G28 Z0
G28 X0 Y0 M09
G90 M05
M99 P1 (send program to line N1)
M30

This works great. I leave the last work coord blank (G59), and set my work coord in G54 coord. If i dont call up the G59 blank coord before the G54 the machine will not overwrite the coordinates set by the G92 line if it has allready been ran through one cycle and restared at the start by accident. The G59 blanks out any previous coord set by G54 etc etc or G92, the G54 then sets the work coord and the G92 specifies the offset amount from the corner of the vise to the desired 0 locations.

A simple work shift could make this so much less complex.