I have a Fanuc 18T control on a Nakamura-Tome TMC 2011 lathe. Does anyone know the code to activate the G54 program? Ours is missing and we need to run a multiple program.

Usual format for a mill with similar controller;
G0 G90 G54 X pos. Y(Z) pos.

G54 is not a program. It is a Work Offset. We run a lot of end washers. Usually 5 per barfeed. Barfeed with the G54 somewhere in the operation before (or on) the first block calling for turret movement. Run all the operations that are done to all the parts such as Driil, Rough Face, Rough Turn, & Rough Bore, etc.

Call up the subprogram that finishes each individual part like so:

N1G54M98P1001 (RUN 1ST PART)
M1

N2G55M98P1001 (RUN 2ND PART)
M1

....

....

N5G58M98P1001 (RUN 5TH PART)
/M99
M30
%

I will assume that you know how to set the work shift and work offsets.

Now if you can't find a G54 on the offset screen somewhere, that is a different story. Machine builder decides whether to use G54-G59 or G10P0 to set the work shift. We have a Nakamura-Tome TW20, but for the life of me I can't remember if it uses G54-G59 or G10P0. I can check Monday morning. Haven't had to program it lately as it has been running the same job for about 4 years now.

If it doesn't use G54-G59 to set the Work Offsets, then the program would look a little different. On most of our barfeed machines I set the work shift. On a few I use a variable as I don't know if they will be setting up with an extended nose collet or a standard collet.

Program would look like this:

N100G10P0Z-1.74 (BARFEED)
or
N100G10P0Z-#530 (BARFEED) (I always include the minus sign so that the operator/setup person doesn't have to remember it.)

Run operations to all parts as before.

N1M98P1001 (RUN 1ST PART)
G10P0W.197 (W.197 is width of part plus width of cut-off tool plus .005 for finish facing on the next part)
M1

N2M98P1001 (RUN 2ND PART)
G10P0W.197
M1

....

....

N5M98P1001 (RUN 5TH PART)
/M99
M30
%

Hope this has been enough information for you to figure out how to run multiple parts on your machine. Ask if you have any more questions. Plenty of people on here willing to help.

I have a Fanuc 18T control on a Nakamura-Tome TMC 2011 lathe. Does anyone know the code to activate the G54 ?.

Send me an email address by via PM.
Al.

Your 18t may be like my 21t on an SC-300L. There are no work coordinate offsets 'cause it has a fixed local coordinate system. Running multiple sub-programs with changing machining conditions requires a G10 for the Z offset along with an M98 and the 'P' subprogram call. As g-codeguy talks about.