[ngerard]

Trying to tap some cross holes on my okuma lathe. I have a live tool setup with a floating collet. Not sure what code to use for tapping in x.

[jrolands]

Try looking into G184. This is used to tap in the face, but I'm pretty sure u can use it for cross holes to..
If I'm not mistaken, it should look something like this:

(Drilling)
G94 X60 Z10 M242 SB=1000 T0707 M8
G183 X40 Z10 C0 I62 Q4 F120 D2
G180 (Compound fixed cycle cancel)

(Toolchange)
G00 X900 Z500 T0909 M146 M12

(Tapping)
G00 X60 Z10 M242 SB=400 
G184 X40 Z10 C0 I62 Q4 F320 
G180

G183 parameters:
C defines the starting point on the c-axis (in degrees)
I is rapid motion to, in this case X62 (use K for drilling in the face)
Q defines the number of holes in the periphery making them evenly spaced.
F is feed rate in mm/min (called by G94 in the line before). If you'r using metric of course.
D has got something to do with chip breaking, but I'm not quite sure. But I know that if u try to run without it, you will get an error.
There is also an L, but it's optional. Also having to do with chip breaking, or peck drilling or whatever.
If you want holes that are not evenly spaced you can omit the Q and list the degrees as C-words in between the G183 and G180

G184 parameters are same as G183, but the feed rate has to correspond with the tread pitch. The code above is used with an M5x0.8, where in this case u get 400*0.8=320.

Hope this helps, and please post your results.

Happy cutting