Trying to get rid of tool chatter

[TMashino]

Hi all,

I'm looking for some quick help here. I am machining 6061 Alum. I have holes that are about 7/16 in diameter and go just over 2" deep. The bottom of the wholes have a full radius to them. I have drilled out to 3/8 drill bit to remove stock. Now I am trying to finish up the holes using a 3/8 diameter ball nose endmill. My first program ran about 5000 RPM with 15 ipm with depth of cut of .03" deep with about a 1/16 step over. CHATTER!! I have tried it again slowing my speed down (to about 5%) and feed down (to about 2500 RPM) with chatter still. I next tried 1/4 depth of cut with .01" step over and still get chatter. Any suggestions from the group? I don't know if I still need to slow the speed and feed down further than I already have or if I need to try something different. Any body have an suggestions?

Thank you

[howecnc]

Finish as much as you can with a regular endmill. Then leave .001 to finish the full radius.

[howecnc]

also plunge on center with a 3/8 ball prior to milling maybe.

[keen]

Hi - 2" deep X 3/8" is too much to nc mill to form without melt down chatter. I would use a finish plunge cut on centre with a 7/16 ball nose or grind a 7/16drill ball nose - and even then watch the S and F. suggest S500 -800 and around F 100 - 200 trial it in scrap to get the workable parameters - think of it as a reaming cut.

[keen]

(The Z F is metric)

[flick]

Is the chatter all the way down, or just at the bottom radius? If the latter, try using a smaller radius than a full ballnose on your 3/8 em (if you have the capacity to program the contour with a smaller radius).

Either way I would go with a light stepover (.005" to .01") and a fast feed (about .005" CLPT). Should be able to ramp down about .05" to .1" DOC with those parameters.

What you're doing is tricky. It's mostly about finding the frequency at which that particular tool/holder/spindle combo is most stable. The Tormach spindle may not have the speed to do it. I've got a Haas office mill at work with 30000 RPM spindle right now, and I expect I could find the sweet spot with that machine just by playing with the overrides until it shuts up.

[TMashino]

Thanks for all of your input. After thinking about it all last night, I came into work extra early to work on it again. After taking a closer look, the diameter of the finished is .492". With the tolerances I was given, (+-.020") I decided to clear it out with a 31/64 drill bit, then "ream" it with a 1/2" ball. I don't know why this didn't come to me sooner. I guess that my perfectionist mentality made me overlook the obvious!