Threading question.

[chrisryn]

I have a problem with some pipe threads I am cutting. I have 5 machines deticated to cutting these threads. I can't work the chatter out on my black steel tubing. I have increased rpm decreased rpm. Increase and decreased cutting depth. I recently change style of insert. Took my thread passes from 14 to 7 perfect threads. Now all of the sudden with no change I get chatter. Not on all machines at once just random ones. Everything is identical machine,insert, program. One will chatter one won't, the next day the other will chatter and the other won't. I am using a G76 cycle and it on a fanuc Oi control. I can post code if it is needed.

[Geof]

Is it maybe differences in the material? I have not worked with black pipe but with different batches of round bar I have found the conditions to prevent chatter on one lot where different to another lot. When they had all been cut to length and mixed up it was a real pain.

Do your pipes have distinct markings so you can possibly sort them and try to find out if it is material differences.

[chrisryn]

No no markings thats a good idea but would be classified as a non value added waste(gotta remeber were lean). I agree that it could be material. Our material venders never get anything right anyways. I am going to rebore my softjaws and see if that was a possible cause. I am trying to solve this quickly and quietly. Managment love root cause analysis meetings that take several months to get to the actual root cause

[Geof]

How are you threading, just plunging straight in?

Maybe try the alternate flank in feed (if that is the correct name) in G76, this is where the tool takes a smaller cut alternately on each side of the thread. If your machine does not have this ability you can simulate it by using G92 in subroutines, go to half depth with one G96 using a Z starting position moved forward half a pitch, then half depth with the z moved back half a pitch and finish with one on center. This way you can avoid taking any cuts using the full flank of the insert.

EDIT changed G96 to G92 (Too darn many G codes to remember )

[chrisryn]

I have done some research on the different type of infeeds. What I can't figure out is were in the G76 is the infeed located. Here is an example of the G76 lines.

G76 P020160 Q70 R000
G76 X1.705 Z-1.37 P560 Q250 F.0869

What controls the type of infeed.

[Geof]

On Haas machines it is the P but Haas use the single line format for G76 so I don't know if yours will be the same.

Actually on reading it I may be interpreting it wrong because it only seems to allow single edge cutting; this would be P1 with A30.

[chrisryn]

In the first line the last two numbers of the P****** is tool angle. Accoriding to my insert rep if change the 60 to 00 it will use both sides of the insert. If I leave it at 60 it chases. I still don't know if it will do the flank style infeed. I have never used g92 before I was going to try it when I run those parts again. I was going to use g76 to get to .01 of my final depth then use the g92 to make a clean up pass.

I have never used G92 before.

[extanker59]

A rep told me a few years ago to use modified flank. That would be P****58
He said to set the angle a couple of degrees less than the actual. It works for me but I rarely cut large threads.
Good luck
Chris

[extanker59]

I hesitate to bring this up but I've had threading problems before and they got fewer and farther between when I switched to lay down threading. The ability (and need) to change the anvil for different diameter threads solved many problems. If you're using lay down, double check the anvil (some manufacturers call it the shim). Sorry if this is old hat to you.

[chrisryn]

Thanks for the advice. Thats not an issue here we cut two types of threads and the laydown insert has specific holders for each insert so thats not an issue.

[extanker59]

Last time, I promise, then I'll stop. Depending on the diameter (some pipe threads being large) it's likely the laydown holders were shipped with a standard shim that doesn't apply for your diameters. For example, the Carbaloy standard shim for our holder is GX 16-1. With 14 TPI that's good for 1" to 2.5" diameters. Otherwise you need a different shim. I'll shut up now. Good luck.
Chris

[chrisryn]

Don't worry about it I need all the ideas I can get. Right now I have the operator boring out the softjaws we use. If that doesn't fix it I am gonna try and put a G92 after the G76 for a finish pass. If that doesn't work then I'll write a macro that will use all G92 commands and then assign it a G code.