[motter71]

I need to turn some threads on a cnc lathe and need some feed and rpm help. I am turning 1.25" -7 UNC threads on CR material. Also, any help on depth of cut would be helpful. Thanks.

[Lyfordln1]

What lathe, what control?

[motter71]

IkegaiAX20Z. Fanuc 6T control.

[fizzissist]

My 6TB manual shows the code for threading as G76, where:
X Minor Dia for OD thread (Major dia for ID)
Z Distance in Z
K Height of thread (the radius value, including the tool radius)
D Depth of 1st cut (no decimal...ie: D100 )
E Feedrate (Pitch, to 6 places)
A Angle of thread (60deg standard, so A60 is your word)

Manual says not to use G96, constant surface speed, while threading.

You should be able to easily and comfortably start at 1500rpm, first cut of .02", about 10 passes


If anyone has any better info, please update me so I know too.

[Dwane]

From past experience on old Fanuc controls, I remember the thread lead not turned accurately at that high an RPM. 7 TPI = .1428 FPR. 500 RPM might be my starting point.
I could be wrong, just my 2 cents.
Dwane

[Lyfordln1]

Note that "D" is 4 places. ie. D0100 is .0100

[fizzissist]

Note that "D" is 4 places. ie. D0100 is .0100

My control was set to 'leading zero suppression', so it wasn't needed.
Good point to take note of though.

[motter71]

Thanks to all for the help. We turned the threads at 565 rpm's with a feed rate of .1428. Great advice and it made my life easier. Especially since I only pretend to be a machinist. Thanks again.