Struggling with chatter on semi-tall profile finish pass, help!
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 53
  1. #1
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default Struggling with chatter on semi-tall profile finish pass, help!

    First off, this is my nemesis, finishing tall profiles in one pass with no chatter. I can never seem to find the magic recipe.

    Material = 6061. Profile is 1.112" x .312" x 1.410" tall. Two of the outside corners have a .120" rad. The other two a .010" rad.
    Can't finish with Z steps. Has to be one pass. I am using a dead-sharp 1/2" M.A.Ford X-AL 3fl in a Schunk hydro.

    I have been all over the map with all parameters. I've tried leaving anywhere from .050" to .010" for finish.
    SFM everywhere from about 300 up to about 1800. Chip load from .0015" up to .006". I can't find the sweet spot.
    Also increasing the feed around outside corners anywhere from 110% to 175%.

    So far the best I can do is .015" leave, 524sfm, .002"ipt, and 120% feed around corners.
    But the finish still isn't great. And its still chattering, especially around the outside corners. Even with a brand new tool.

    I am sure it is the super narrow width of the material. But, can't figure out how to overcome it.
    I'm giving up for tonight. Tomorrow I'm going to try like ZERO RPM (not really zero, but super slow). I don't know what else to do.
    Also, I'm kind of stuck with this tool. I'm limited to what I have on hand with a 1.5" flute and square corner.

    I'm real close to running out of extra stock. And, I have to be running tomorrow. I'm stumped. Where would you go from here?

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    170
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    55

    Default

    Id try 200-250 sfm .01 doc .002-3ipt

    Sent from my SM-A115AP using Tapatalk

  3. Likes wheelieking71 liked this post
  4. #3
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,613
    Post Thanks / Like
    Likes (Given)
    1008
    Likes (Received)
    3159

    Default

    Why the one pass requirement rather than a Z stepdown?

  5. #4
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default

    Quote Originally Posted by Vancbiker View Post
    Why the one pass requirement rather than a Z stepdown?
    Picky customer (getting pickier). I deliver in the white. He doesn't want to see any visible evidence of steps.

  6. #5
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    13,017
    Post Thanks / Like
    Likes (Given)
    2946
    Likes (Received)
    8953

    Default

    If all else fails, grind a small flat on the shank and try a sidelock.

    The small inherent eccentricity in a sidelock, not to mention the variable stiffness due to how a sidelock works, may break up harmonics that cause chatter.

    Use some of the existing test pieces to work out final parameters, don't keep cutting fresh metal until you're close.

    And order some more endmills, of a few different flavors. Sometimes brand S will work better than H, or G, or...

    Oh, yeah - when was the last time you checked drawbar force on that spindle?

  7. #6
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default

    Quote Originally Posted by Milland View Post
    If all else fails, grind a small flat on the shank and try a sidelock.

    The small inherent eccentricity in a sidelock, not to mention the variable stiffness due to how a sidelock works, may break up harmonics that cause chatter.

    Use some of the existing test pieces to work out final parameters, don't keep cutting fresh metal until you're close.

    And order some more endmills, of a few different flavors. Sometimes brand S will work better than H, or G, or...

    Oh, yeah - when was the last time you checked drawbar force on that spindle?
    I wouldn't even bother with a flat for this cut. Just crank the screw down. Do it all the time. I get your thinking on breaking up the harmonic though!
    Don't have time to order end-mills. This job is HOT. It is one I subbed out when I simply did not have time to do it.
    And it got rejected! (did you see where I mentioned customer is getting pickier?) Regardless, customer needs parts NOW.
    This machine just got a new spindle motor. Drawbar is A-Okay.

  8. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,254
    Post Thanks / Like
    Likes (Given)
    2486
    Likes (Received)
    3099

    Default

    Might seem anti-intuitive, but could be chatter from brand new sharp edges. We see that alot with 2" loc endmills. After they run for a while the chatter seems to go away. I think we run about 300sfm and .004ipt. Can you polish/work by hand, or is it going to be a high volume run?

  9. Likes wheelieking71, Shawnrs, MoriMillMan, Ox liked this post
  10. #8
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,563
    Post Thanks / Like
    Likes (Given)
    1662
    Likes (Received)
    2133

    Default

    Quote Originally Posted by Mike1974 View Post
    Might seem anti-intuitive, but could be chatter from brand new sharp edges. We see that alot with 2" loc endmills. After they run for a while the chatter seems to go away. I think we run about 300sfm and .004ipt. Can you polish/work by hand, or is it going to be a high volume run?
    Agree with this. I have had the same experience with 12mm x 50mm 3fl in 6061T6. Brand new endmill squeals, and absolutely nothing will stop it, fades when they have dulled a bit, but flip side is deflection increases and a little bit of wall taper rears it's head. Nothing to do with the thin wall either, parts I was doing were solid.

    Squeal can be mitigated by really pushing the chipload, but by the time you have actually quieted it down the vertical scallops are pretty big. 12mm x 50mm 3fl is just a nasty size to get to work.

    If you get a bit of advance warning next time, a bigger tool is the easiest solution. I have a couple of 20mm x 55mm 4fl polished endmills that I use for external profiling on aluminium, and ofc internal if the rads allow for it, mirror finish every time with those.

  11. Likes wheelieking71 liked this post
  12. #9
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default

    Couldn't sleep, came back out here.
    I got acceptable results taking a .015 cut @ 1600rpm and 19ipm. I did try a larger tool like you suggested gregor. No dice, way worse.
    I don't think it is the tool that is singing at me. I think it is the material.
    It is still squealing a little bit. But there is zero chatter in the finish. So, I'm gonna run with it.

    Not really high volume Mike, 100pcs. But, I don't hand finish anything. These parts don't pay that much!

  13. Likes Mike1974, gregormarwick, Shawnrs, Ox liked this post
  14. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,910
    Post Thanks / Like
    Likes (Given)
    5577
    Likes (Received)
    3767

    Default

    There's no way to lay the part down and cut it? it might involve an extra operation but it just might be the answer.

  15. #11
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    13,017
    Post Thanks / Like
    Likes (Given)
    2946
    Likes (Received)
    8953

    Default

    Quote Originally Posted by Mtndew View Post
    There's no way to lay the part down and cut it? it might involve an extra operation but it just might be the answer.
    He's got outside corner radii, not ideal to try them laid down. And, if they're a feature on a larger part it's even more annoying.

  16. #12
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    531

    Default

    Have you tried finishing with a conventional cut? We have a couple of jobs that require long endmills that have to finish the ends of extruded material. The part that sucks the most on these jobs is the part sticking out 3-4 inches outside the vise and when we make a climb cut it squeals real bad but using a conventional cut on the finish pass seemed to give us the best finish.

    I also agreed to what Mike said about new endmills, we have similar issues with chatter on new endmills but over a time as the endmills wears a bit the chatter seems to go away.

  17. #13
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,317
    Post Thanks / Like
    Likes (Given)
    13571
    Likes (Received)
    5143

    Default

    I get that Z steps might not be acceptable.... But what about a constant finish from spiraling down around the boss at a 2° or 3° ramp?

  18. Likes mhajicek liked this post
  19. #14
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    343
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    98

    Default

    Quote Originally Posted by TeachMePlease View Post
    I get that Z steps might not be acceptable.... But what about a constant finish from spiraling down around the boss at a 2° or 3° ramp?
    This is a good idea as it should provide a uniform appearance. It also puts a portion of the cutting load in the stiffer Z direction. Not ideal for tool wear, but should be good for 100pcs.

  20. #15
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,677
    Post Thanks / Like
    Likes (Given)
    280
    Likes (Received)
    1895

    Default

    Quote Originally Posted by Mike1974 View Post
    Might seem anti-intuitive, but could be chatter from brand new sharp edges. We see that alot with 2" loc endmills. After they run for a while the chatter seems to go away. I think we run about 300sfm and .004ipt. Can you polish/work by hand, or is it going to be a high volume run?
    Eh, I've not seen that, at least with YG-1 Alu Power. I can tell a marked difference between an unused 1/2" x 2" and a used one. The new one always outperforms the used.

    Speaking of YG-1, I would try an Alu Power 3-flute. They have, IME, done better than anything else.

    Regards.

    Mike

  21. #16
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default

    Quote Originally Posted by Mtndew View Post
    There's no way to lay the part down and cut it? it might involve an extra operation but it just might be the answer.
    No, the whole feature sits on a floor, and all the walls and rads have to be square corner at the bottom.

  22. #17
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,268
    Post Thanks / Like
    Likes (Given)
    913
    Likes (Received)
    512

    Default

    Quote Originally Posted by wheelieking71 View Post
    Couldn't sleep, came back out here.
    I got acceptable results taking a .015 cut @ 1600rpm and 19ipm. I did try a larger tool like you suggested gregor. No dice, way worse.
    I don't think it is the tool that is singing at me. I think it is the material.
    It is still squealing a little bit. But there is zero chatter in the finish. So, I'm gonna run with it.

    Not really high volume Mike, 100pcs. But, I don't hand finish anything. These parts don't pay that much!
    So that’s about 200 SFM....slowing down the speed has become my go-to trick for chatter in both turning and milling. I’m turning 4340 right now at 125SFM to keep the chatter monster away. Also, like others have said, we stone a 3/8” em for a squeaky job and it works. Happy you’re making chips!

  23. Likes MoriMillMan, wheelieking71 liked this post
  24. #18
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,910
    Post Thanks / Like
    Likes (Given)
    5577
    Likes (Received)
    3767

    Default

    I wonder if conventional cutting would do the trick?

  25. #19
    Join Date
    Nov 2005
    Location
    Santa Barbara
    Posts
    313
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    101

    Default

    When I get much below 300SFM or so in aluminum, I usually have better luck with HSS tools, ground for cutting steel instead of aluminum. Carbide doesn't like going that slow, and high positive angles tend to pull the part into the tool. Put it in a sidelock holder, and dull it on purpose. Take a brand new 4 flute HSS tool, and run a penny down the length of each flute, pushing straight into the edge. It's probably more removing the microscopic grind burrs than dulling, but it seems to help. (doesn't do a damned thing on carbide) And it doesn't leave any nicks, like a used tool would have. Spin that as slow as you have to. At some point, you'll definitely get rid of the chatter.

  26. #20
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,199
    Post Thanks / Like
    Likes (Given)
    9553
    Likes (Received)
    9263

    Default

    Great tips guys. I hadn't thought to try a conventional cut. Should have!
    Its running now though, and I'm gonna let it run as is. The parts look good.

  27. Likes Mtndew liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •