Long Tool Holder Chatter
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Long Tool Holder Chatter

    Hello,

    I am programming our new 500mm Horizontal. I need to access the side of the part when the pallet is indexed at 90 degrees and therefore need an 8" long ER16 collet holder. I have a 2 flute 1/4" carbide drill/endmill that I am using to put a chamfer on the hole. I am getting some terrible chatter on the hole and can not seem to get rid of it.

    The material is 6061 Aluminum. I drill the hole first so that the drill/endmill has less material to remove. I also tried spotting the hole first. I slowed the RPM down to 4k and up to 6k. I also tried feedrate. I can't seem to find something that works. It doesn't have any side load cause I'll I'm doing is a G81 cycle.

    I see these Die/Mold shops with super long holders and great finishes. I'm amazed at what they can achieve when I'm having problems with this little issue.

  2. #2
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Montana
    Posts
    30
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    18

    Default

    Ditch the drill/mill. Absolutely the worst choice in pretty much all applications. Then go back to manual techniques... 500 to 1000 RPM, feed in inches per hour, and a little dwell should get you there. Check runout as well.

    ETA if this is a production deal, consider taking the largest holder that will not quite fit (ER20?), then turn it down to where it JUST clears. You are looking for every advantage you can get when you've got this much gauge length.

  3. #3
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,510
    Post Thanks / Like
    Likes (Given)
    10048
    Likes (Received)
    2947

    Default

    So... Is the 1/4" for clearance? Because if this is literally just a chamfer, rather than interpolate, just take a 2FL 1/2" spot drill and plunge to depth, dwell if necessary, and retract? All the force will be axial rather than radial, which should decrease your chatter.

    At least, that's how I'd try to do it, though I don't do big parts, so that's just my best guess.

  4. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    Quote Originally Posted by wishin4snow View Post
    Hello,

    I am programming our new 500mm Horizontal. I need to access the side of the part when the pallet is indexed at 90 degrees and therefore need an 8" long ER16 collet holder. I have a 2 flute 1/4" carbide drill/endmill that I am using to put a chamfer on the hole. I am getting some terrible chatter on the hole and can not seem to get rid of it.

    The material is 6061 Aluminum. I drill the hole first so that the drill/endmill has less material to remove. I also tried spotting the hole first. I slowed the RPM down to 4k and up to 6k. I also tried feedrate. I can't seem to find something that works. It doesn't have any side load cause I'll I'm doing is a G81 cycle.

    I see these Die/Mold shops with super long holders and great finishes. I'm amazed at what they can achieve when I'm having problems with this little issue.
    .
    longer tool holders require much slower rpm. usually you do a series of tests with each standardized tool setup and create a chart or database that shows feeds and speeds tried and what works ok and not ok.
    .
    longer tool holders where you have 20" gage length you rarely get a very good finish. best you get is a ok finish. and feeds in the 1 or 2 ipm are not unusual.

  5. #5
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,769
    Post Thanks / Like
    Likes (Given)
    1608
    Likes (Received)
    4726

    Default

    If this is production, use a larger countersink that can fit and plunge the chamfer.

    For the chatter, since this is a new machine have you checked spindle deflection and drawbar force? While it's unlikely, you could have a form error on the spindle taper (CAT or HSK?), or low drawbar force. You can also check the actual holder in that spindle, see if it deflects easily. If it's worn it may not be mating with the taper correctly.

  6. #6
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    obviously you aint done much with really long tools and tool holders like 20" long
    .
    you should try 20" long drill bits only .250" dia or even .5" dia
    .
    feeds and speeds got nothing to do with tool tip over heating. more to do with vibration resonance. you get the right frequency and a drill can easily break even when feeds and speeds are in the ok range for a short tool.

  7. #7
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,769
    Post Thanks / Like
    Likes (Given)
    1608
    Likes (Received)
    4726

    Default

    Quote Originally Posted by DMF_TomB View Post
    obviously you aint done much with really long tools and tool holders like 20" long
    .
    you should try 20" long drill bits only .250" dia or even .5" dia
    .
    feeds and speeds got nothing to do with tool tip over heating. more to do with vibration resonance. you get the right frequency and a drill can easily break even when feeds and speeds are in the ok range for a short tool.
    If that's aimed at me, you're wrong. I've had to make my own extended tooling for boring, insert milling, and drilling that's easily more difficult than your 20" - 1/4" example. And made it work, though tuning and other optimizations. On C-frame machines, so more difficult than a horizontal.

    For gosh sake, Tom - don't you have a spreadsheet to work on or something? Take your assumptions with you...

  8. Likes Mike1974, 360427, lumley32 liked this post
  9. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,184
    Post Thanks / Like
    Likes (Given)
    1425
    Likes (Received)
    1501

    Default

    I don't think I would like trying an 8" er16. Can you get a slim-fit collet in there? They seem to be more rigid (relatively speaking). Or maybe a couple shrink fits for these applications... I suspect you are going to run into this more and more.

  10. Likes dstryr liked this post
  11. #9
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    i am not talking about anybody.
    .
    i am saying long tools require a learning curve especially on vibration resonance. got nothing to do with tool tip overheating limits. usually you create a database or chart so for a standardized tool setup you got a record of what works better and what doesnt work ok. that way you are not relearning to use a specific tool setup every few months or years. you got a record and go right to using optimal settings and save a lot of wasted time reinventing the wheel so to speak.

  12. #10
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,309
    Post Thanks / Like
    Likes (Given)
    861
    Likes (Received)
    1398

    Default

    Quote Originally Posted by wishin4snow View Post
    The material is 6061 Aluminum. I drill the hole first so that the drill/endmill has less material to remove. I also tried spotting the hole first. I slowed the RPM down to 4k and up to 6k. I also tried feedrate. I can't seem to find something that works. It doesn't have any side load cause I'll I'm doing is a G81 cycle.
    Keep slowing it down.

    Rigidity decreases exponentially with length (to the 3rd power). So an 8" toolholder deflects roughly 8X as much as a 4" holder.

    In the future, try to find tapered toolholders, or make your own by clamping a straight shank chuck in a larger chuck to get the length you need. Also, when you're out that far, every little bit helps. If you can get away with a 7" toolholder, it's going to run a lot faster than an 8".

  13. #11
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    actually anti vibration tool holders which can be extremely expensive some over $10,000. each and cheaper ones easily over $1000. actually do help reduce vibration
    .
    literally you can have 2 boring bars and the anti vibration one can run 2x faster and hold tighter tolerance.

  14. #12
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,769
    Post Thanks / Like
    Likes (Given)
    1608
    Likes (Received)
    4726

    Default

    Quote Originally Posted by Orange Vise View Post

    In the future, try to find tapered toolholders, or make your own by clamping a straight shank chuck in a larger chuck to get the length you need. Also, when you're out that far, every little bit helps. If you can get away with a 7" toolholder, it's going to run a lot faster than an 8".
    Sometimes you can get a faux anti-vibration effect from setting up holders this way, just make sure you don't lose your TIR and balance control.

    I guess at the low speeds balance isn't too much of an issue.

  15. #13
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    anti vibration tool holders are made of special metals and internal parts designed to internally dampen vibration. if you ever pick one up you can tell they are much heavier than normal.
    .
    same as a big carbide end mill feels heavier than same size HSS end mill

  16. #14
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    6,769
    Post Thanks / Like
    Likes (Given)
    1608
    Likes (Received)
    4726

    Default

    Tom, there's more than one way to try to dampen vibration. Nested tooling is one way, albeit not typically as effective as a proper anti-vibe bar. And the plus for nested tools is most people already have the elements at hand, and no tuning is needed (although it can be done though adjusting stickout, etc.).

  17. #15
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,995
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    in general where length to dia ratio is over 5x you get vibration problems with steel tool holders. if 10" long tool holder is less than 2" dia and many are smaller dia, then they tend to vibrate easy
    .
    many a job i had to side mill and had to have tool holder dia small enough, tool holder would not rub on part or fixture

  18. #16
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    780
    Post Thanks / Like
    Likes (Given)
    765
    Likes (Received)
    440

    Default

    Another approach would be to do it with a ball endmill at 45°; that should give you a much shorter reach.

  19. #17
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,465
    Post Thanks / Like
    Likes (Given)
    4058
    Likes (Received)
    2646

    Default

    Quote Originally Posted by wishin4snow View Post
    Hello,

    I am programming our new 500mm Horizontal. I need to access the side of the part when the pallet is indexed at 90 degrees and therefore need an 8" long ER16 collet holder. I have a 2 flute 1/4" carbide drill/endmill that I am using to put a chamfer on the hole. I am getting some terrible chatter on the hole and can not seem to get rid of it.

    The material is 6061 Aluminum. I drill the hole first so that the drill/endmill has less material to remove. I also tried spotting the hole first. I slowed the RPM down to 4k and up to 6k. I also tried feedrate. I can't seem to find something that works. It doesn't have any side load cause I'll I'm doing is a G81 cycle.

    I see these Die/Mold shops with super long holders and great finishes. I'm amazed at what they can achieve when I'm having problems with this little issue.
    Is the chamfer critical? Or is it just for deburring reasons?
    If it's not critical, You could use a larger drill and go to the chamfer size, THEN drill the hole.
    If it IS critical, then I would try a smaller pilot hole, then chamfer it, then drill the hole. And which "drill mill" are you using?
    For chamfering I really like the spiral flute chamfer mills from Lakeshore Carbide:
    Chamfer Mills | Carbide End Mills, Thread Mills | Lakeshore

  20. Likes Bob E liked this post
  21. #18
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,245
    Post Thanks / Like
    Likes (Given)
    406
    Likes (Received)
    1630

    Default

    Quote Originally Posted by wishin4snow View Post
    ...I slowed the RPM down to 4k and up to 6k. I also tried feedrate. I can't seem to find something that works. It doesn't have any side load cause I'll I'm doing is a G81 cycle.
    Just a simple chamfer?

    Stick a single flute chamfer tool in there and slow your RPM waaaay down. 700-800 range. Jeez, the tool change takes longer than the cut, no reason to run 4K+, it doesn't gain you anything...

  22. Likes TeachMePlease, Matt_Maguire liked this post
  23. #19
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,184
    Post Thanks / Like
    Likes (Given)
    1425
    Likes (Received)
    1501

    Default

    Quote Originally Posted by jancollc View Post
    Just a simple chamfer?

    Stick a single flute chamfer tool in there and slow your RPM waaaay down. 700-800 range. Jeez, the tool change takes longer than the cut, no reason to run 4K+, it doesn't gain you anything...
    True enough, but when you spend your days cutting aluminum you kind of get used to having the spindle live at or near the max rpm...


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
  •