Need Help!- 2" 4.5 thead! Chhhaaattteeerr!!

[CoolhandLuke]

I am running some nuts on a CNC lathe and I can't get the chatter out. No matter what I do, the speeds and feeds. No way no how. I have spent nearly 8 hours and I am nearly at my wits end. I tried taking .015 per pass with 10 spring cuts to .002 per pass with 10 spring cuts. Chatter. Tried running 100 rpms to 500 rpms. Nothing is working. My threading tool is 1.250 od and it is in as far as I can get it and still have clearance. Thead is 1.375 deep. Any suggestions? It seems to me like the whole carrage is vibrating. As far as this job goes, I think that I might be in over my head.

[RICHARD ZASTROW]

Where is your tool tip positioned relative to centerline? If it's low it might be digging in and rebounding, causing chatter. If it's high, the tool can be forced back and rebound back in to the cut. I,m ASSuming this is an ID thread????

You can always cheat by making the threads undersize and finish with a tap. LOL

Dick Z

[cam1]

Hi:
Are you feeding in at 90 degrees or 29? What material are you threading?
If you can feed in on the leading edge of the tool, then you will have alot less chatter (front edge does all the cutting).

regards

[CoolhandLuke]

Tool is on center, and this is an ID thread. I believe that it's feeding in at 90. I used the canned cycles on the conversational software that comes with the controller. Controller is a Centroid on a Venture lathe. Seems as if the entire carage is vibrating. I tightened all the gibbs and made sure that everything was as secure and rugged as I could get. Hope this helps you guys figure out what is going on.

[HuFlungDung]

What style of tooling are you using: Laydown threading or top-notch, or other type? Carbide, I presume?

Chatter can be tough to dampen, do you have any trouble with chatter when boring holes on this machine?

Can you write out a longhand version threading routine if you must? It may just not be feasible to use a canned threading cycle if it does not cut one side of the thread at a time, because that is a lot of surface for the tool to scrape against.

I am not a believer in a lot of spring passes, maybe 2 at most, because taking more can encourage chatter to develop. Once the surface gets roughened with a chatter pattern, then the chatter is self perpetuating.

I also believe in a manly first cut, then back off the depth on each succeeding cut. 4.5 pitch...I dunno, my first pass might be .04 deep (X0.08 ) if the tool will stand it. Then .03 then .02 and so on. Minimum depth for roughing might get down to .005, but the trick is to get there with as few passes as possible, keep the tool loaded and prevent chatter from beginning.

Higher spindle speeds will create more chatter, but they also can create much smoother threads. I'd try to keep the SFM up around 300 fpm or 600 rpm in this case.

[juergenwt]

Feed in at 29 1/2 deg. That is 29 1/2 from the 90 deg pos. Reduce your feed- in rate as you go deeper.

[shay z]

you can also try to shorten the tool.

check the tool's insert pocket. maybe the insert moves.