Using up 3/4 inch carbide endmills too quick
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    South Dakota
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    4

    Default Using up 3/4 inch carbide endmills too quick

    Hey guys, I'm having a little trouble getting more life out my 3/4 inch carbide endmills. I only get to use them about twice before they need to be resharpened. Granted each time is on a 6 to 8 foot brake that I mill. I only have it running at .1 Z depth and it only fully engaged on each part for 200 to 300 inches at about .050 depth. The rest of it is side milling maybe .05. I'm cutting 1145 steel and my endmills are solid carbide. I'm using flood coolant, spinning the endmills at 1790 RPM, and feeding at 30 IPM. This next time I'll try it at 20 IPM. What am I doing wrong? Thanks!

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,257
    Post Thanks / Like
    Likes (Given)
    200
    Likes (Received)
    1590

    Default

    Sounds like you are using your endmill like a facemill, if it's only .05" deep and 100% engagement. I would try an inserted facemill instead. You can tune the inserts for the material and conditions, and inserts are cheap compared to 3/4" carbide.

    If not that, how about stubby 1/2" endmills? You need more passes, but cutters are much cheaper.

    Regards.

    Mike

  3. Likes Bobw liked this post
  4. #3
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,050
    Post Thanks / Like
    Likes (Given)
    13928
    Likes (Received)
    10722

    Default

    What am I doing wrong?
    350sfm, is the steel hardened or no???

    I'm going to say that your problem is that you are running coolant.
    That thermal shock thing..

    From too much experimenting, I've found that (at least for me), the break point
    from wet to dry is about 300sfm in mild steel.. Lower for harder materials.

    Are you coated???

    That dark purple stuff gets slicker than snot and hard as hell when it gets HOT!!!
    If you are running coolant, you may not be generating a high enough temp to let the
    coating work its magic.

  5. Likes Mtndew liked this post
  6. #4
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,750
    Post Thanks / Like
    Likes (Given)
    4355
    Likes (Received)
    2884

    Default

    Quote Originally Posted by Bobw View Post
    350sfm, is the steel hardened or no???

    I'm going to say that your problem is that you are running coolant.
    That thermal shock thing..

    From too much experimenting, I've found that (at least for me), the break point
    from wet to dry is about 300sfm in mild steel.. Lower for harder materials.

    Are you coated???

    That dark purple stuff gets slicker than snot and hard as hell when it gets HOT!!!
    If you are running coolant, you may not be generating a high enough temp to let the
    coating work its magic.
    This would be my suggestion as well.
    Cut it dry.
    And maybe use an indexable shoulder mill for the .100" depth cut.
    OR
    Or get an endmill with a larger corner radius.

  7. #5
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,503
    Post Thanks / Like
    Likes (Given)
    303
    Likes (Received)
    673

    Default

    that's a chip load of .004 on a 4 flute tool and about 350FPM. You don't mention the failure mode of the end mill- wear or chipping or? Is this a coated tool or?? My guess is its thermal shock from your coolant but that's only 1 possibility. I have had good luck with coated tools and an air blast in steel. Blue chips are a good indicator of getting the heat out in the chip and that's a combo of RPM and chip load. Have you consulted the tool manufacturer?

  8. #6
    Join Date
    Oct 2009
    Location
    near Seattle, Washington, USA
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    477
    Likes (Received)
    797

    Default

    How is your part fixtured? If it's allowed to bounce around it's going to beat the crap out of your cutter.

  9. Likes bryan_machine liked this post
  10. #7
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    South Dakota
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    4

    Default

    The endmills are not coated. The Steel is not hardened. I'm running 350 SFM. The endmills are wearing down on the corner and then starting to chip. I'm roughing out the pocket with a 1.5 inch carbide inserted cutter and going back in and finishing with the 3/4 inch. I'm using endmills with a sharp corner to get the 90 degree edge in the pocket. I don't have air blast capabilities at the moment. The chips are coming off with no color change. I'm running a vertical mill so if I run without coolant the chips should fall away. I'll probably try cutting it without coolant this next time. The part weighs about 800 pounds and is fixtured vertically. I've got it hanging pretty solid. I'll probably try it without coolant next. Thanks for the tips!

  11. #8
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,126
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    433

    Default

    Like others have said.

    1) It is not aluminum, so even carbide will wear. If you don't want to wear off the tip, use indexed endmill for facing operations. ALso ditch coolant.

    --OR--

    1) Use coated carbide.
    2) Ditch Coolant

  12. #9
    Join Date
    Oct 2009
    Location
    near Seattle, Washington, USA
    Posts
    1,453
    Post Thanks / Like
    Likes (Given)
    477
    Likes (Received)
    797

    Default

    Quote Originally Posted by RustyRedneck View Post
    The endmills are not coated. The Steel is not hardened. I'm running 350 SFM. The endmills are wearing down on the corner and then starting to chip. I'm roughing out the pocket with a 1.5 inch carbide inserted cutter and going back in and finishing with the 3/4 inch. I'm using endmills with a sharp corner to get the 90 degree edge in the pocket. I don't have air blast capabilities at the moment. The chips are coming off with no color change. I'm running a vertical mill so if I run without coolant the chips should fall away. I'll probably try cutting it without coolant this next time. The part weighs about 800 pounds and is fixtured vertically. I've got it hanging pretty solid. I'll probably try it without coolant next. Thanks for the tips!
    In that case it might be more economical to rough with a 3/4" cutter with either radiused or chamfered corners and then come back in with a smaller sharp corner cutter.

  13. Likes Bobw, kevin66, doug925 liked this post
  14. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,220
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2654

    Default

    Quote Originally Posted by RustyRedneck View Post
    Hey guys, I'm having a little trouble getting more life out my 3/4 inch carbide endmills. I only get to use them about twice before they need to be resharpened. Granted each time is on a 6 to 8 foot brake that I mill. I only have it running at .1 Z depth and it only fully engaged on each part for 200 to 300 inches at about .050 depth. The rest of it is side milling maybe .05. I'm cutting 1145 steel and my endmills are solid carbide. I'm using flood coolant, spinning the endmills at 1790 RPM, and feeding at 30 IPM. This next time I'll try it at 20 IPM. What am I doing wrong? Thanks!
    .
    usually measure tool life in minutes with 60 minutes often considered normal tool life.
    .
    tool length and tool holder length can effect cutting parameters easily 100 to 1000% . normally its best to try different cutting parameters and record data. tool life, amount milled, surface finish, any sudden tool failures, normal wear or failure mode.
    .
    like any scientist you try experiments and record data. then decide on whats better to do.

  15. #11
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    South Dakota
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    4

    Default

    While I was gone the boss ordered a 3/4 inch inserted endmill and it showed up other day. Programmed for it and away we go. Seems to be working well so far. may have eliminated the carbide endmill from this process.

  16. Likes SND liked this post
  17. #12
    Join Date
    Aug 2016
    Country
    ALAND ISLANDS
    Posts
    1,393
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    96

    Default

    hy / a bit late, but :

    ... try not changing directions inside the material; improve the toolpath if possible
    ... check the dwells ?
    ... plunge @ corners
    ... what holder is it ?

    check for variants for the tool corner : radius, chamfer, sharp

    check if the new tool has bigger corner radius ?

    Quote Originally Posted by RustyRedneck View Post
    I'm using endmills with a sharp corner to get the 90 degree edge in the pocket
    here you are ... finishing tools are better to be carbide integral than with inserts / if you will have problems with the new tool with inserts, consider a smaller integral one

    be sure that, when cutting the walls, tool is not cutting @ bottom


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
  •