Need Help!- G76 Threading problem

[bmlw]

Hello all, hope someone can shed some light on this.
I am making a small flange nut that has a 32 TPI internal thread. All appears normal except that the thread seems to change pitch as it nears the bottom of the nut. I have looked at the G76 notes in the FANUC Operators manual and can find nothing wrong with my code:

N4 ( IT230400 SET POINT AT Z0)
G00T1102
G97S3500M3
G0X.45Z.2
G76X.503Z-.2K.019D100E.03125
X.503
G0Z1.0
T1100
M1

I looked at my Operators Manual (Apendixes) and found
PARAMETER 6212 Chamfering amount in thread cutting cycle Range 0 - 127, it was set at 0
PARAMETER 6213 Chamfering angle in thread cutting cycle Range 0-60, it was set at 45. I tried reseting this to 60 and then to 0 and had no luck.

Any ideas would be appreciated

BMLW

[sti2011]

Not familiar with how you use the G76 cycle in your control, but 3500rpm seems pretty damn fast for the machine to keep up with itself. It probably can't speed up or slow down the axis motion at that RPM. Try slowing down the RPM to slow your axis motion.

[bmlw]

Thanks for the input. The program was originaly set up for a Mori SL0. I am sure my DAEWOO cant hold a match to it, but it is what I have. I am cutting FC360 Brass, What would you recomend for a starting point for threading?

[dcoupar]

You're trying to go from 0 to 109 IPM and back to 0 in 0.400! The machine has to accel/decel so that is what you are seeing at the bottom of the hole.

Try it at 1000 RPM and see if the thread looks better. This may not be the ideal speed to thread brass, but you can't fight the laws of physics.

And, if 6212 is set to 0 (no chamfer), I don't believe it matters what angle you put in 6213.

[bmlw]

Thanks Dave,
I was going to try 2000rpm, but will go with 1000 tommorow and see how it goes.
I think I should also set 6012 up abit but am not sure how this works.

[dcoupar]

If you're going to part the nut off anyway, I'd leave 6212 at 0.

[sinha_nsit]

Chamfering becomes necessary when you want correct pitch up to the last thread, including partial threads. Zero chamfering means the tool is retracted exactly in axial direction, at the end of the thread. Since the spindle keeps rotating, this would spoil the last thread. If, however, the last thread is not to be used, you can go for zero chamfering.

[SanDiegoCNC]

Originally Posted by bmlw Hello all, hope someone can shed some light on this. I am making a small flange nut that has a 32 TPI internal thread. All appears normal except that the thread seems to change pitch as it nears the bottom of the nut. I have looked at the G76 notes in the FANUC Operators manual and can find nothing wrong with my code: N4 ( IT230400 SET POINT AT Z0) G00T1102 G97S3500M3 G0X.45Z.2 G76X.503Z-.2K.019D100E.03125 X.503 G0Z1.0 T1100 M1 I looked at my Operators Manual (Apendixes) and found PARAMETER 6212 Chamfering amount in thread cutting cycle Range 0 - 127, it was set at 0 PARAMETER 6213 Chamfering angle in thread cutting cycle Range 0-60, it was set at 45. I tried reseting this to 60 and then to 0 and had no luck. Any ideas would be appreciated BMLW

Here are two examples of threading cycles that should work for you...

USING G76...

M01
G28 U0. W0. M05
G00 T404 (OD THREAD TOOL)
(8-32 X 0.08 OAL)
G97 S800 M03
G00 G54 X0.17 Z0.2
G50 S800
G99 G00 X0.17 Z0.15
M08
G01 X0.17 Z0.1 F0.03
M24 (THREAD TAPER OUT OFF)
(M23 = THREAD TAPER OUT ON)
G76 X0.13 Z-0.16 K0.02 D0.0006 F0.0312
(K = MAJOR DIA MINUS MINOR DIA / 2)
(D = SUBSEQUENT DEPTHS OF CUT)
(FEEDRATE = 1 / # OF THREADS)
G00 X0.17 Z1.
M09
G28 U0. W0. M05
T400


AND G92...

M01
G28 U0. W0. M05
G00 T404 (OD THREAD TOOL)
(1/4 NPT X 0.6 OAL)
G97 S800 M03
G00 G54 X0.54 Z0.2
G50 S800
G99 G00 X0.54 Z0.15
M08
G01 X0.54 Z0.1 F0.03
G92 X0.54 Z-0.55 I0.034 F0.0555 M24
(G92 IS MODAL THREAD CYCLE)
(X0.54 IS FIRST THREAD DIAMETER)
(Z IS THE THREAD LENGTH)
(I IS THE TAPER AMOUNT OVER THE LENGTH OF THREAD)
(F IS THE FEEDRATE)
(FEEDRATE = 1 / # OF THREADS)
(EACH OF THE FOLLOWING LINES IS ANOTHER DEPTH OF CUT)
X0.525
X0.53
X0.525
X0.52
X0.515
X0.51
X0.505
X0.5
X0.495
X0.49
X0.485
X0.48
X0.475
X0.47
X0.465
X0.46
X0.455
X0.45
X0.445
X0.44
X0.435 (FINAL THREAD DEPTH)
X0.435 (SPRING PASS ON FINAL THREAD)
G00 X0.54 Z1.
M09
G28 U0. W0. M05
T400



HOPE THIS HELPS!