How do I use a G76?

[naytep]

Trying to use a G76 with the Fanuc 0T Leadwell T6 lathe. I have had success in the past however I rarly program. Can anyone help jog my memory?
I enter it like this:

P011060
(1 spring pass, 10 chamfer amount, 60 deg infeed)

G76 X0.870 Z-1.62 R0 P0670 Q02000 F0.1111
(.87 start diam, length, R0 no taper, P depth of thread .067, Q first pass .020" deep, F= pitch)

[wms]

G76 X0.870 Z-1.62 R0 P0670 Q02000 F0.1111 (.87 start diam, length, R0 no taper, P depth of thread .067, Q first pass .020" deep, F= pitch)

X is actually the Minor (OD Thread) / Major (ID Thread) not the start diameter....

All else is correct.

G76 P011060 (Finish/Spring Passes_ Chamfer Amount_ Tip Angle) Q0010 (Minimum Cut Depth) R0010 (Finish Allowance)
G76 X (Minor/Major Diameter) Z (Cut Length) R (taper amount) P (Height Of Thread) Q (Depth Of First Pass) F (lead/pitch of thread)

[John3]

Originally Posted by naytep Trying to use a G76 ..... Can anyone help jog my memory?

Someone already has a memory jogger here...... Check out posting;

http://www.cnczone.com/forums/showthread.php?t=41192


John

[naytep]

When I run like this:
G76 P010060
G76 X0.760 Z-1.625 R0 P0.067 Q0200 F0.1111

My thread is no were near size. If I adjust the height (double it) I loose pitch. I have left the height (P) alone and adjusted with my X. But, by time my thread is of size I am no longer anywhere near the book value for the minor thread diameter (book .7408, actual .710).
This is why I have been confused.

The machine is running, but I would like to no why my numbers are so far off from actual data.

Thank You
John

[star-turn]

Whats that decimal point in the P value ????

should be P0670 not P0.067

other than checking you have set the tool correctly (geometery) and are using the correct tip all should be OK ( give/take a few thou. )

ST