Help me cut NPT 3" 8TPI on Aluminium

[waloni]

Hi I'm trying to cut a NPT3" x 8TPI thread on a aluminium pipe but I keep getting massive buildup on the insert, which in turn destroys the thread.
I'm using the G76 canned cycle on Fanuc OT control but can someone tell me what the correct RPM of chuck and the proper P and Q values.
This is driving me nuts!! I have no trouble in cutting every other internal or external thread but this "........." doesn't want to work.

[HuFlungDung]

Hi Waloni,

I wonder what the problem is, some unusual grade of pipe? Aluminum typically threads up real nice.

Are you turning the OD taper first? I would highly recommend it.

I would try about 600 rpm.

Use coolant, even brush on a bit of thread cutting oil when it starts to get near full depth.

I'm not sure if your control uses the two line G76 format, but there is some important advantage you can gain in the first line. If the format is:
Pmra Rd
where a= tool nose angle,
you can experiment with this value, to try to force an unequal chip that will perhaps curl out of the cut a bit differently. Try a value of 20 (degrees) for a.

Here is a sample such as I would use on a Mitsubishi. It could be similar, but the syntax may be different than yours:
G0 X3.625 Z.25
G76 P022020 R.003
G76 X3.335 Z-1.75 R-.0625 P.090 Q.023 F.125

[WayneHill]

Here is 20 passes using my "Fast G-Code 4 Lathe" program. It is a program that uses constant/equal material removal on each thread pass. Thread infeed is at 29.5 degree. Neat program if I have to say so myself

http://www.cnczone.com/gallery/data/...dium/FGC4L.jpg

T01 M06
G00 Z4.0 (SAFE INDEX POINT)
X6.0
Z0.2896
X2.9339
G33 X2.9741 Z-1.0 F0.125
G00 X3.1
Z0.2853
X2.9175
G33 X2.9575 Z-1.0 F0.125
G00 X3.1
Z0.282
X2.9049
G33 X2.9448 Z-1.0 F0.125
G00 X3.1
Z0.2792
X2.8943
G33 X2.9342 Z-1.0 F0.125
G00 X3.1
Z0.2768
X2.885
G33 X2.9247 Z-1.0 F0.125
G00 X3.1
Z0.2745
X2.8765
G33 X2.9162 Z-1.0 F0.125
G00 X3.1
Z0.2725
X2.8688
G33 X2.9084 Z-1.0 F0.125
G00 X3.1
Z0.2706
X2.8615
G33 X2.9011 Z-1.0 F0.125
G00 X3.1
Z0.2688
X2.8547
G33 X2.8942 Z-1.0 F0.125
G00 X3.1
Z0.2671
X2.8483
G33 X2.8878 Z-1.0 F0.125
G00 X3.1
Z0.2655
X2.8422
G33 X2.8816 Z-1.0 F0.125
G00 X3.1
Z0.264
X2.8364
G33 X2.8757 Z-1.0 F0.125
G00 X3.1
Z0.2625
X2.8308
G33 X2.8701 Z-1.0 F0.125
G00 X3.1
Z0.2611
X2.8254
G33 X2.8646 Z-1.0 F0.125
G00 X3.1
Z0.2598
X2.8202
G33 X2.8594 Z-1.0 F0.125
G00 X3.1
Z0.2584
X2.8151
G33 X2.8543 Z-1.0 F0.125
G00 X3.1
Z0.2572
X2.8103
G33 X2.8494 Z-1.0 F0.125
G00 X3.1
Z0.2559
X2.8055
G33 X2.8446 Z-1.0 F0.125
G00 X3.1
Z0.2547
X2.8009
G33 X2.84 Z-1.0 F0.125
G00 X3.1
Z0.2535
X2.7964
G33 X2.8355 Z-1.0 F0.125
G00 X3.1
Z0.2535
X2.7964
G33 X2.8355 Z-1.0 F0.125
G00 X3.1
Z0.2535
X2.7964
G33 X2.8355 Z-1.0 F0.125
G00 X3.1
G00 Z4.0 (SAFE INDEX POINT)
X6.0
M02

[waloni]

Thanks for helping me out. The thread worked out great.
I have used parafin as lubrication and used the first gents settings for the G76 canned cycle. I have no doubt that the longer program taking equal cuts would work just as good. I unfortunatley didn't have the time to convert all the data to metric sizes for that program. But I want to try it and see how it works.
Just to tell you what the settings were.

GOX87.5 Z5.0
G76P020055Q250R0.05
G76X84.7 Z-26.0 P2230 Q600 F3.175
G0 X95. Z50.

Thanks again.