atc not in tool change position oitd fanuc

Just got a brandy new 244" lathe with a fanuc oitd control with manual i.
I use gibbscam for programming and I am working with my rep to create a post for this lathe, which I have done about 4 times in the past 15 years.

The machine is a poreba north america lathe with a china tag Microcut challenger.
Everything works great but this lathe has to be home in X with the light lit for it to index or I get ATC "X" NOT IN TOOL CHANGE POSITION alarm 1103.
Now a little on how it is setup.
"X" true zero is the center of the machine.
The home position in +X is 36.001 the grid shift was factory set to 35.000057
the machine rounds it to 36.001
If I use a GOG53XOZ-145.2345 it goes home ok but will not perform a tool change.( no ref light)
If I in MDI use a G28 X36.001 it will go home and light the home light and perform a tool change
If I write a G28 X36.001 and run the program it does a soft over travel in X.
Does anyone have a clue to what Im doing wrong, Ive been at this for about two weeks which included installing the machine on its foundation setting up everything else that goes with it and this is my last hurdle to running the machine full auto.
I have lots of experience over 35 years but this is one I hope someone can help me through.....Im sure its something real stupid on my part so go easy on me while you tell me how much of a bonehead I am.
Regards
:drowning:

Why aren't you using G0 G91 G28 U0. for X axis and G0 G91 G28 W0. for Z axis?

The reason is because the Fanuc sets a bit in the ladder logic that will turn on the ref light when you G28 the axis to it's home position. When you move the axis to it's home position without using the G28 it doesn't set the ZP1 to ZP4 bits (machine referenced bits)which turn on the ref light. So if you need the ref lights on you have to reference the axis. To bypass the soft over-travel check use G91 G28 X0 You may want to cancel all active offsets before doing the move as well.

Don't need the g91 if using u and w. just g28u0.

Thank you for the information.
I was using a G91 and I kept getting improper G-Code.
The G28 U0 works perfectly.
Time to make the Donuts.
I knew it was something dumb on my part.
I owe you one!
Mark