chatter issues milling a pocket
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    Feb 2014
    Location
    Ohio
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    35

    Default chatter issues milling a pocket

    I'm milling these pockets in annealed 8620 with an Iscar Heli2000 with APKT inserts. 500SFM, .005IPT, ramping down at 2° to .150" deep per pass. I get a loud screech as it goes around and it's leaving chatter marks. Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue. I tried adjusting speed and feed with no effect. Any suggestions?

    Also, what's a good way to deburr the corners of this on both ends? Hand held flap wheel? Wire wheel? Thanks for any tips.
    2015-05-23-11.29.59.jpg

  2. #2
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I think the cutting parameters are o.k.
    Due to the geometry of the finished part, when the cutter is in the corners there is no rigid lateral support to absorb the pressure of the cutting action. I'm guessing the part is chattering, or the part and tool are resonating together. Would a round pocket cut in a set of soft jaws would give more contact and support? Can you flip the part over and use a larger diameter tool and/or a shorter extension?

  3. #3
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,234
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2656

    Default chatter

    Quote Originally Posted by Ukraine Train View Post
    I'm milling these pockets in annealed 8620 with an Iscar Heli2000 with APKT inserts. 500SFM, .005IPT, ramping down at 2° to .150" deep per pass. I get a loud screech as it goes around and it's leaving chatter marks. Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue. I tried adjusting speed and feed with no effect. Any suggestions?

    Also, what's a good way to deburr the corners of this on both ends? Hand held flap wheel? Wire wheel? Thanks for any tips.
    2015-05-23-11.29.59.jpg
    .
    part vibration usually means lowering depth and or width of cut, lowering sfpm, lowering feed. sometimes a smaller diameter cutter is used.
    .
    leaving .010 to .020 for a finish cut usually reduces any burr left. often the chatter marks from a roughing cutters are removed by the finish cut so minor chatter marks does not matter much

  4. Likes shamanj liked this post
  5. #4
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    8,090
    Post Thanks / Like
    Likes (Given)
    414
    Likes (Received)
    6677

    Default

    Quote Originally Posted by Ukraine Train View Post
    .....Interestingly, I started this job with worn inserts and it went ok, but when I flipped to the fresh side I started having the issue.
    Maybe a hint here?
    Bob

  6. #5
    Join Date
    Sep 2011
    Location
    NJ, USA, Lebanon
    Posts
    344
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    105

    Default

    I would use a smaller diameter solid carbide endmill. Less cutting forces and such.

  7. Likes Milland, jrmach, shamanj, jdj liked this post
  8. #6
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,824
    Post Thanks / Like
    Likes (Given)
    573
    Likes (Received)
    308

    Default

    Quote Originally Posted by CarbideBob View Post
    Maybe a hint here?
    Bob
    I had a chatter problem milling an aluminum wheel some years back. Long extension on a brand new 1/2" HSS 2 flute.
    After the cutter was "broken in" which took about 15 minutes, the chatter disappeared. Maybe something similar is happening here with the fresh inserts.

  9. Likes jdj liked this post
  10. #7
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    8,090
    Post Thanks / Like
    Likes (Given)
    414
    Likes (Received)
    6677

    Default

    Yup,
    and what is weird is that every carbide company in the world used to give out "hone stones" with their name on it for free like candy.
    Every machinist had a Kennametal, Carboloy, Valenite, or Newcomer stone. We bought them by the thousands. Much better than ink pens or hats.
    The purpose, get rid of chatter by intentionally dulling the edge and actually increasing the cutting load....... Strange, eh. more load, less chatter, and longer tool life.
    You would just hit the edge of each tool with the stone and life would be so much better for you.
    Now coatings mean you need the right edge prep before it is coated and these stones are hard to come by.
    At one time you could order any carbide up-sharp, A,B or C honed. Today a very different world of catalog/internet standards and no longer true.
    Sadly only the volume users get their choice of edge prep now inside a grade so most just have to live with dropping off feeds and speeds.
    The price for progress and lower cost inserts.
    Bob

  11. Likes lowCountryCamo liked this post
  12. #8
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,829
    Post Thanks / Like
    Likes (Given)
    1827
    Likes (Received)
    5505

    Default

    Quote Originally Posted by CarbideBob View Post
    Yup,
    and what is weird is that every carbide company in the world used to give out "hone stones" with their name on it for free like candy.
    We bought them by the thousands.
    The purpose, get rid of chatter by intentionally dulling the edge and actually increasing the cutting load....... Weird, eh. More load, less chatter.
    Now coatings mean you need the right edge prep before it is coated.
    Bob
    Hi Bob,
    Is it fair to say those were also the days of much larger carbide grains, and the reason to "dull" the edges was to reduce the risk of larger grains digging in to the workpiece and being pulled out? The traverse rupture strengths would have been lower too, so lowering the chance of sharp edges grabbing the work and overloading the tool could be a factor.

    What do you think?

  13. #9
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,657
    Post Thanks / Like
    Likes (Given)
    2625
    Likes (Received)
    632

    Default

    I always thought to reduce chatter you wanted a sharper cutter to reduce cutting force. Although after reading what CarbideBob wrote that does make sense to me.

  14. Likes jdj liked this post
  15. #10
    Join Date
    Mar 2012
    Location
    Quebec, Canada
    Posts
    628
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    201

    Default

    Grab a good carbide endmill and youll get rid of the chatter. The apkt facemill just bang around on every insert biting the stock a endmill is sharp will reduce the cutting force and cut instead of banging. Im pretty sure its going to fix your problem and might be even faster.

  16. Likes jdj liked this post
  17. #11
    Join Date
    Feb 2014
    Location
    Ohio
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    35

    Default

    Thanks guys. Maybe I'll try a 1/2" endmill. Should I just follow the pocket contour or would it be better to sort of work my way from the inside-out to reduce the step over? I wanted to use the inserted-endmill because I have 300 of these to do and figured it would be cheaper to replace a few inserts rather than a few $60 endmills.

    I'll also do a finish pass to try to knock the burrs down.

  18. #12
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,829
    Post Thanks / Like
    Likes (Given)
    1827
    Likes (Received)
    5505

    Default

    If your fixturing is stable enough, I'd run as large a drill as you can fit into the slot (either middle, one end, or both ends), then set up a narrow stepover, full depth high speed/feed path for a 1/2" or so vari-flute style four flute endmill. Rough to .020, change to a dedicated finish mill for a final pass. This could be a five or six flute finisher, let it wail...

  19. #13
    Join Date
    Mar 2012
    Location
    Quebec, Canada
    Posts
    628
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    201

    Default

    Drop a 1/2 inch drill in the middle of the pocket and hsm the pocket with a 1/2 endmill and you should use around 3 endmill should be faster and time is money so worth the extra bit of $ in tools. Tools are consumable time should always be priority on a 300 pcs run. If the job take 3 hours less your endmill are going to be paid for.

  20. #14
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,497
    Post Thanks / Like
    Likes (Given)
    3467
    Likes (Received)
    2057

    Default

    Drop the biggest drill you can in then rest machine with an HSM path. No point starting with a small drill and a larger one will give the chips somewhere to go. Get an air blast in there too.

  21. Likes shamanj, jdj liked this post
  22. #15
    Join Date
    Apr 2013
    Location
    Australia
    Posts
    658
    Post Thanks / Like
    Likes (Given)
    217
    Likes (Received)
    266

    Default

    Deburr: just use a chamfer tool or a spot drill and just kiss the edges with a .2mm DOC on all edges so you don't slice yourself open on it. Being a handwheel sharp edges may bite.

  23. #16
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,962
    Post Thanks / Like
    Likes (Given)
    1312
    Likes (Received)
    3816

    Default

    You don't say what cam system you're using, but switch to an HSM like Optirough or Volumill. Use an 1/2" 5fl em, as a starting point, 5k rpm, 120 ipm, 12% stepover and .75 doc. No coolant. (air blast if possible) Your burr problem will go away as well.

  24. #17
    Join Date
    Oct 2007
    Location
    detroit,mich.
    Posts
    4,704
    Post Thanks / Like
    Likes (Given)
    4710
    Likes (Received)
    418

    Default

    YES! a drill is a "primative" tool, but still very efficient in the right area. After that, a variable helix type solid carbide end mill is very hard to beat!

  25. #18
    Join Date
    Feb 2014
    Location
    Ohio
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    35

    Default

    Thanks for the suggestions. I use NX for CAM software, but still learning. I'll play around with it to get a HSM path. Where do you like to get your variable helix end mills? I think I've checked with my local shop supply place before and they didn't have these.

  26. #19
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,884
    Post Thanks / Like
    Likes (Given)
    1092
    Likes (Received)
    739

  27. #20
    Join Date
    Nov 2011
    Location
    Enid, Oklahoma
    Posts
    260
    Post Thanks / Like
    Likes (Given)
    1354
    Likes (Received)
    120

    Default

    I think you'll be fine with what you're using as far as tooling, I'll bet the problem lies in the workholding.Your pockets are right on top of where the parts are unsupported.

    I used to run parts like this all the time, and like you i started with a 3 jaw chuck on its back and had loads of chatter.

    If your parts are consistent O.D., then interpolate a circle into some thick softjaws in a vise like I did, and the problem should go away.

    If you're careful, while its running, put your hand on the part and you can verify to a certain degree that it is the parts that's vibrating.

    I do have to agree with everyone else though a salid carb em with a hsm toolpath would be superb, but i'm always used to making do with what i have.



    my .02


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
  •