what exactly is in your other working program with G54? a Z value as well or nothing? usually a G54 in the program has no other info with it. the machine reads G54 and reads the workshift number set up previously on the workshift screen
i.e.
G54
G50 S1000
G0 T0202
G96 S100 M3
G00 X10.0 Z0 M8
etc
however I worked several machines with FAPT over the last 25 years (mostly Fanuc 15/16 Mori ZL and SL models) and I've never seen FAPT output a G54. There's nothing in my docs about it either.
There are 2 possibilities and maybe both need to be set.
FAPT parameters relating to this are....
MTF parameter 1060
if bit 0 is 0 then it doesn't output a G50 X Z for each tool (this is what you want.... no G50 X Z output)
so 1060 should be xxxxxxx0 (only change bit 0... the right-most number)
or invert your bit if you have this already. i.e. if your bit 0 is 0 make it 1. if it's 1 make it 0
MTF parameter 1244
this sets the Coordinate System Setting G Code and is defaulted to '50' on my control
Possibly modify it to '54' may get you what you need. But like I said I never saw any FAPT machine output a G54 so your mileage may vary.
also note G54 in the program is usually not required on a lathe as it defaults to that on power-on. If you don't need multiple workshifts you don't need to have a G54 in the program. So stopping the G50 output with parameter 1060 is enough. if you must have it type it into the program manually.
There are many undefined or not-assigned parameters in FAPT depending on the machine tool builder they can be set to something or left at 0 or null. If your machine tool builder modified something you may need to contact them for the correct FAPT parameters.
NOTE! If most/all of your FAPT MTF params are 0 then you lost all of them and will need to set things up again.
If most of them are non-zero then you have not lost your FAPT params and your problem lies elsewhere.
To set the G54 you go to your workshift screen, move the cursor to the G54 Z value. Then touch the face of the part with your setting tool (a tool where the geometry in Z is 0) then type Z0 then press measure. If the face is +2mm (if you want to face off 2mm) then type Z2.0 and press measure
if you don't have a setting tool with 0 in Z geometry then in order to be able to set the workshift the best/correct way to must also set the tools using a similar methodology. The tool setting details are here in post#11
Need Help! Leadwell, fanuc O-T help!
once set this way to change to a new part using the same tools just bring the setting tool to touch the face and in the workshift page set G54 Z using Z0 measure as explained above.