need help with Canned cycles on a fanuc lathe

[firekoe]

i am trying to understand how the G90, G92, and G94 work but the book is not helping at all if some one could give me some info that would be great

[dcoupar]

In it's simplest form, use G94 to take a facing cut or two, and G90 to take a turning cut. Lets say you want to face the end of a 2.5" bar and turn it down to 2.375.

G00 X2.6 Z0.1 (POSITION TO CLEARANCE)
G94 X-0.062 Z0.005 F0.012 (ROUGH FACE - ALLOW 0.005)
Z0 F0.006 (FINISH FACE)
G90 X2.405 Z-2.04 F0.012 (ROUGH TURN - ALLOW 0.015)
X2.375 F0.006 (FINISH TURN)

G94 rapids to the Z value, feeds to X, feeds back to the initial Z, and rapids back to the initial X. This pattern is repeated for each successive block with a Z commanded. You can add an R+/- to cut a taper.

G90 works the same, except it rapids to X, feeds to Z, feeds to the initial X and rapids back to the initial Z. You can also add an R+/- to cut a taper.

G92 works the same as G90, except it uses the encoder to start the feed so you can cut a thread. You can also add an R+/- to cut a tapered thread.

The down-side to G90 and G94 is the 2nd feed move is just dragging the tool over previously cut faces... not very efficient and not usually all that good for the tool.

You can substitute U/W (incremental commands) for X/Z (absolute commands) in any of these cycles.