I assume your G300 line looks similar to mine from my BS19: (if not, it should)
G300 X-.05 Z3.05 T0505 (your Z may be up to 8" depending on your z1 stroke)
Just to get the simple stuff out of the way, what exactly is the Z value in your G300 line? do you have the decimal in the right spot?
Is your program in metric and machine in inches? then you could have a value like Z100.(mm) in your G300 line. If your program was in MM and machine was in Inches you would have a huge over travel like you're describing. Just something to check. I only have a parameter manual for a 16/18i series and In/MM is parameter 1001 bit 0 (INM).
0 is Metric
1 is Standard
If its not that you have some other problem.
What happens if you MDI in G28W0 on Z1? If it goes home just fine with G28W0, the problem is in your code. If it over travels with a G28, then your machine coordinates are messed up and you have bigger problems to solve.
Also, Do you have a G150 (or G50) Z-.005 (right hand cutoff)
or G150 (or G50) Z.440 (left hand cutoff) to establish your new part zero?
here is the opening block for every program I write. Yours should be similar (but probably not the same)
#105=.072(CUTOFF SHIFT)
G65P9002T505D.250S4000M3X-.05F.0008 (auto cutoff/barload macro call)
M9#### (SUB PROG)
G0G18G20G40G97G99T0M8 (safety line)
M11 (main collet open)
G4U.4
G300X-.05Z3.05T0505 (machining origin)
G150Z-.005 (new part zero)
M10 (main collet close)
G4U.4
G0Z-.05 (clear)
G0X1.496 (x home)
CNC Product Manager / Training Consultant