What's the secret to stop chatter on a long 1" dia HSS end mill
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default What's the secret to stop chatter on a long 1" dia HSS end mill

    Hey everyone,

    I've got a 1" dia x 6" length 4 flute HSS end mill that I am using to finish a 2" long bore that is 5" deep in an aluminum part and I cannot for the life of me get it to stop producing a rifle barrel finish from all the chatter.

    I've tried every combination from 130-315 sfm, 0.002-0.005 ipt, and 0.005-0.030 step over.

    The "best" results which are still completely unacceptable seem to be with high sfm, low chip load, and light step over which seems to go against the general consensus of wanting to load up the cutter.


    Any thoughts on other cutting conditions to try running?

  2. #2
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    8,135
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3987

    Default

    Quote Originally Posted by Mr.Chipeater View Post
    Any thoughts on other cutting conditions to try running?
    Boring head. That's what they are made for.

  3. Likes charlie gary liked this post
  4. #3
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,621
    Post Thanks / Like
    Likes (Given)
    991
    Likes (Received)
    1839

    Default

    Anything over 4xD stickout can be chattery even in carbide.

    HSS has about 1/3 the rigidity of carbide, so even worse.

    Long flute lengths further reduce rigidity, partially because you're missing material and partially because all that axial contact adds to the tool pressure. Ideally you'd have a relieved (necked) solid carbide shank with less than an inch of flute length on the tip.

    If this is a one-off job and you have no other use for that HSS cutter, I'd grind away the flutes (maybe 0.010" off the radius) so that you're only left with about 1/2" of flute on the tip. Then finish the bore by helixing down at about 0.100" per rev.

  5. Likes Bobw, Fulcircleny, mhajicek, Red James liked this post
  6. #4
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,700
    Post Thanks / Like
    Likes (Given)
    16494
    Likes (Received)
    11834

    Default

    Machine? Taper?

    And how you holding it.. The tool and the part..

    I agree with Orange Vise about grinding her back to limit your
    contact. But I'd take it a step further.

    You need to break up the harmonics. Like those fancy variable
    flute and helix endmills do. I'd start by grinding a big chamfer
    on one flute only.

    And I'll tell you a quick story of why I would do that. Years ago
    I had a series 10 Acroloc. And I was doing (trying to do) things
    with that machine it wasn't intended to do. Even with a variable
    flute/helix endmill, it would still scream at me, and then break
    off one corner.. Sometimes that one corner would break off and
    it would quiet down and cut good, other times, the broken corner
    would destroy the endmill.

    So, trying to get a leg up on the machine breaking the corners off
    my endmills, I would take the endmill out of the tube, (brand new 1/2"
    Imco, or HTC) and grind a 60 to 80 thou chamfer on one flute.. Worked
    a treat, and I've used that trick on other machines in tricky situations,
    and it works.. Not always, but its worked enough for me that I keep it
    in my bag of tricks.

    Also, if your machine isn't the most rigid thing going, ramping will add
    pressure straight upwards, through the spindle and make your machine think
    its more rigid than it is. If its going to move anyways, might as well
    control the direction of movement and use it to your advantage,
    big corner rads and chamfers can also help with that,
    sort of simulating a high feed mill.

  7. #5
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Bobw View Post
    Machine? Taper?

    And how you holding it.. The tool and the part..

    I agree with Orange Vise about grinding her back to limit your
    contact. But I'd take it a step further.

    You need to break up the harmonics. Like those fancy variable
    flute and helix endmills do. I'd start by grinding a big chamfer
    on one flute only.
    Machining it on a 40 tapper HAAS UMC750 so not the most rigid but seems to be adequate for aluminum jobs. Part is held nicely in 5th axis vise so I doubt that is contributing much.

    I'd love for a nice variable helix carbide tool but as Orange Vise pointed out, I'd still have to get such a large diameter tool it would be cost prohibitive.

    The chamfer idea is a neat trick I'll have to try sometime. The bore I'm machining is open on the other end so I'm machining as high up on the tool as I can so without the tip touching, I'm not sure chamfering the end will change anything. I suppose I could grind a spot in the middle of one flute as a way to break up some harmonics.

    A boring head would also be great.... if I had one the right size.

  8. #6
    Join Date
    Nov 2005
    Location
    Santa Barbara
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    101

    Default

    130 SFM isn't all that slow, for HSS. I'd just keep going slower. It'll eventually shut up.

    You could also try grinding down an entire flute or two. Make it a ghetto variable helix. Anything to break up the harmonics.

  9. #7
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,130
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    459

    Default

    You’re talking about the bottom surface, not the cylindrical one, are you? The question arises with me, what a mad design or function can it be that demands such. If you need a very good bottom quality and can go a little deeper, push a neat disc in there.

  10. #8
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    13,478
    Post Thanks / Like
    Likes (Given)
    2990
    Likes (Received)
    9085

    Default

    OP mentions a "rifle barrel" finish, making it pretty clear it's the bore he cares about. And I agree with those that say boring head, if he's got any BH at hand he could kludge a cutter that (flimsy as it may be) would still be superior to a HSS EM.

  11. #9
    Join Date
    Jan 2011
    Location
    Estonia
    Posts
    761
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    207

    Default

    Once again
    Long HSS-Co mills for steel finishing

    I had same problem and reducing speed and feed eliminated chatter, results were good

    But this was for outside wall. If you got 1" in 2" hole, then the engagement angle is big. And against all logic, I think smaller diameter mill may work better.

    Keep load and rpm minimal and it may work.

  12. #10
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,290
    Post Thanks / Like
    Likes (Given)
    2497
    Likes (Received)
    3109

    Default

    I (in theory) disagree about slowing it down. Normally* with chatter you either want to decrease sfm OR increase chip load.

    *4" LOC may be the problem in itself however.

  13. Likes Bobw liked this post
  14. #11
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,901
    Post Thanks / Like
    Likes (Given)
    604
    Likes (Received)
    346

    Default

    For a lark, try conventional milling instead of climbing.

  15. #12
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,339
    Post Thanks / Like
    Likes (Given)
    3864
    Likes (Received)
    2890

    Default

    Couple thoughts....obviously i dont know the part or what you have available to use. Since it is a bore....I agree with the boring head idea. Or can you grab or fixture it in a lathe? Can you ry to "helix bore " it. I have had success helix boring with an endmill to reduce chatter. It gets some of the pressure pushing axially and can help....obviously it is slower than a regular old G2 or G3

  16. #13
    Join Date
    Jan 2011
    Location
    Estonia
    Posts
    761
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    207

    Default

    Quote Originally Posted by Mr.Chipeater View Post
    Machining it on a 40 tapper HAAS UMC750 so not the most rigid but seems to be adequate for aluminum jobs. Part is held nicely in 5th axis vise so I doubt that is contributing much.

    I'd love for a nice variable helix carbide tool but as Orange Vise pointed out, I'd still have to get such a large diameter tool it would be cost prohibitive.

    The chamfer idea is a neat trick I'll have to try sometime. The bore I'm machining is open on the other end so I'm machining as high up on the tool as I can so without the tip touching, I'm not sure chamfering the end will change anything. I suppose I could grind a spot in the middle of one flute as a way to break up some harmonics.

    A boring head would also be great.... if I had one the right size.
    But you can still "bore" it with long endmill. Go to pedestal grinder and grind away about 0.2-0.5 mm of the mill edge, except the last 5mm (or even less) at the end. Now it has much smaller load and you can go helix. Almost like boring head.

  17. Likes mhajicek liked this post
  18. #14
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,272
    Post Thanks / Like
    Likes (Given)
    1320
    Likes (Received)
    816

    Default

    I'm in the relieve the flutes and helical interpolate it crowd. If you can't, I second trying conventional. You could also try running it slow. Like 50SFM and .0015IPT.

  19. #15
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    6,141
    Post Thanks / Like
    Likes (Given)
    6580
    Likes (Received)
    3475

    Default

    When I bought my first Bridgeport at 15 years old the very first tool I bought was an Enco boring head that would do your 2" bore down in the part no problem.

    You have a Haas machine that is one of their fancier turds and you don't have a boring head for a 2" bore?

    I was kinda in your shoes once with a tall outside profile that chattered. I was at Western Tool discussing my problem and they pulled out a big box of custom ground carbide tools that were wrong or returned for some reason. I found a 6" long 3/4" 2 flute carbide endmill in there that was relieved for all but the final 1/2" of flutes.

    I bought that endmill for $15 and it ran production for about 10 years in one of my VMC's. At one point, the toolchanger dropped that tool and broke one of the flutes off. It still ran forever that way with no change.

  20. Likes Bobw, DouglasJRizzo liked this post
  21. #16
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    278
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    50

    Default

    Quote Originally Posted by Mr.Chipeater View Post
    Hey everyone,

    I've got a 1" dia x 6" length 4 flute HSS end mill that I am using to finish a 2" long bore that is 5" deep in an aluminum part and I cannot for the life of me get it to stop producing a rifle barrel finish from all the chatter.

    I've tried every combination from 130-315 sfm, 0.002-0.005 ipt, and 0.005-0.030 step over.

    The "best" results which are still completely unacceptable seem to be with high sfm, low chip load, and light step over which seems to go against the general consensus of wanting to load up the cutter.


    Any thoughts on other cutting conditions to try running?
    Radial chip thinning at .005 radial and .005 feed puts your actual chip thickness at .0007. that's VERY small. Kick your feed up significantly. .015 per tooth minimum at .005-.010 stock.

  22. #17
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,130
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    459

    Default

    Quote Originally Posted by Milland View Post
    OP mentions a "rifle barrel" finish, making it pretty clear it's the bore he cares about. And I agree with those that say boring head
    Then a no-brainer, boring head, or if you can clamp work on lathe, turning. Ecocut is also nice, made by Ceratizit. Plunge and turn/bore with one tool

  23. #18
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    13,814
    Post Thanks / Like
    Likes (Given)
    4696
    Likes (Received)
    4973

    Default

    An end mill is sharp on the od so any little run out will make the hole a tiny bit oversized and leave a spiral going in. The best fix is to finish the hole with a reamer. A reamer has an OD circle-land that holds the tool center and cutting on the end only.

    Carbide end mill most likely to do the very same thing.

    Yes, to ream finish the hole the original bore would be a 1/64th or so smaller than the reamer.

    Oh, do assure that the end has an end cutting grind..that is one having a flute going to center with enough end gullet (space) so the chips can flow without bunching up. Still, the end mill likely will leave a rifle barrel finish

    and end cutting tools/cutters need more end clearance 10 to 14* is good.

  24. #19
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    975
    Post Thanks / Like
    Likes (Given)
    198
    Likes (Received)
    556

    Default

    Since you are using a haas have you tried using a G13 pocket milling cycle? In aluminum I have good luck using these pocket milling cycle.

  25. #20
    Join Date
    Nov 2012
    Location
    usa
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default

    Try doing multiple passes in 1" stepdowns or helix down in 1" increments. If your taking the 5" length in one pass your 5x diameter on depth. In my experience anything after 2x diameter deep is just asking for it to sing you a song. Use the shortest reach tool holder you have and preferably use a collet chuck and choke the end mill up as short as you can in the holder. I'm with the others on the boring head route though.

    Sent from my moto g power using Tapatalk


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
  •