URGENT.

[alncolo]

Hi all

Am very new to CNC

Programming a Supermax with Fanuc OT Control

Trying to thread a Nut INTERNALLY

tried using G76 but the Graphics Display shows it still cutting EXTERNAL thread
WHY?????????????????????????/
x91.6
z1.0 M08
G76 P011060 Q030
G76 X91.6 Z-11.0 P4580 Q030 F1.5875 (16 TPI )

WHY is this not working

[Karl_T]

On my machine, ID vs. OD is determined by the X position being smaller than the G76 X. And this X position also determines the pullout position at the end of each cutting pass so you have to choose this value carefully. In short, try changing your X91.6 to something smaller.

Karl

[dcoupar]

tried using G76 but the Graphics Display shows it still cutting EXTERNAL thread
WHY?????????????????????????/
x91.6 <--- must be less than major diameter - 2* height of thread
z1.0 M08
G76 P011060 Q030
G76 X91.6 (major) Z-11.0 P4580 (height) Q030 F1.5875 (16 TPI )

Also, your P value seems to be incorrect. Are you specifying 4.58mm (0.180) or 0.458mm (0.018)? Neither sounds right for 16 TPI)

[g-codeguy]

What is the thread size call out on the drawing?

[maz43]

Your P value for a 16 tpi ID thread should be P3380.
Your X start point should be smaller than your X value in the G76 line for an ID thread.
Good luck.

[dcoupar]

maz43: It appears as if he's programming in millimeters. I believe your P3380 is 0.0338 inches, correct?

[g-codeguy]

Appears it isn't too "URGENT" after all.

Mr. Coupar, my Hardinge manual says the format for P and Q is Q4 P4 for inch and Q3 P3 for metric. We know this means P3380 is .3380 for inches. What I don't know is how the control handles an extra digit. Does in simply ignore the left most digit in P3380 making it .380 for metric? The machine manual doesn't say. The Fanuc operator's manual I looked at doesn't even mention the number of digits allowed in the address.

What I can tell the original poster is that the machine appears to be threading an OD thread because his P-value is too large. Plus his start position accentuates the problem. We use to have a Hardinge Super Precision (now at a sister company). P3500 is .03500 with it, but when the program runs on a standard Hardinge it becomes .3500 and it acts like the OP is describing.

[dcoupar]

g-codeguy: I believe P can have 8 digits. So P12345678 would be 1234.5678 inches, or 12345.678 millimeters. And I don't think it ignores any digits. The way I read it, P3380 is .3380 inches or 3.380 millimeters. But you're right that it doesn't appear to be URGENT anymore.

[g-codeguy]

Originally Posted by dcoupar g-codeguy: I believe P can have 8 digits. So P12345678 would be 1234.5678 inches, or 12345.678 millimeters. And I don't think it ignores any digits. The way I read it, P3380 is .3380 inches or 3.380 millimeters. But you're right that it doesn't appear to be URGENT anymore.

You are most likely correct. That is why his ID thread appears to be an OD thread. .1803 inch is a bit much for thread height on a 16 pitch thread. The tool is going to drop down a fair amount to start its threading cycle. Especially since his approach and ending thread dimensions are the same. Wouldn't be quite so bad if the approach was where it should be.