G76 THREADING

Hi everyone.

OK, I have been programming fanuc lathes since 1988. Using the 2 line G76 for threads. I have just started with a new company and the control I'm using is a 30i on a CMZ 2 axis lathe .

I tried programming a 16mm x 2 ext thread. But no matter what I did the first pass was at 13.7 mm. Very deep and not good. I tried starting at 24mm, 30mm etc. Still drops straight to 13.7 mm for the first cut. How does the system decide where the 1st cut begins?

G0X20.0 Z5.0
G76 P020060 Q010 R0.05
G76 X13.400 Z-50.0 P1228 Q307 F2.0

I have used the manual guide and that's OK, but why??

Cheers all

Pete

Sorry it is a 32i

and I just noticed it goes below the x value straight away

Hi,

Probably your first G76 line isn't okay, try;

G76 P020060 Q100 R0.05 or G76 P020060 Q100 R50
G76 X13.454 Z-50. P1227 Q300 F2.

I've used a fanuc control that uses thread angle from the perpendicular of the thread axis
(ie. choice of 0, 15, 25, 27.5, 29, & 30)
Also try P020029 .... 29° to allow clean up on flank of thread

Quote:

---

Originally Posted by singist48

Hi everyone.

OK, I have been programming fanuc lathes since 1988. Using the 2 line G76 for threads. I have just started with a new company and the control I'm using is a 30i on a CMZ 2 axis lathe .

I tried programming a 16mm x 2 ext thread. But no matter what I did the first pass was at 13.7 mm. Very deep and not good. I tried starting at 24mm, 30mm etc. Still drops straight to 13.7 mm for the first cut. How does the system decide where the 1st cut begins?

G0X20.0 Z5.0
G76 P020060 Q010 R0.05
G76 X13.400 Z-50.0 P1228 Q307 F2.0

I have used the manual guide and that's OK, but why??

Cheers all

Pete

---

Rough calculations:
Core dia = 13.4
Thread height = 1.2
OD = 13.4 + 2x1.2 = 15.8
First DOC = 0.3
First roughing X = 15.8 - 2x0.3 = 15.2
You are saying that it is 13.7
Please check if the program is typed correctly on the machine.

Initial X does not matter, as you have seen.