Feed/Speed ADjusting for Endmill
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Jul 2020
    Country
    CANADA
    State/Province
    Manitoba
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    4

    Default Feed/Speed ADjusting for Endmill

    Hello everyone.
    I have some issues with getting the feeds and speeds dialed in with end mills. I am running a 1/2 TiALN Coated Endmill in 1018 steel. Our machine is a NL3000y mill/turn center.
    I was running the end mill at 220 SFM, 0.0035 feed/tooth, recommended by local supplier. Full length of cut (1") and a .06 step over. After the first part, roughly 40 minutes of work I was seeing a dull edge and tiny, tiny chips on the flutes already, coating also seemed to be showing signs of wear. What are the first adjustments I need to make to prolong tool life?

    Also - if I make the switch to 1045 material, how much do my variables need to change?
    Thanks everyone for your help.

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    419
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    104

    Default

    I run almost twice that SFM in 316SS.

  3. #3
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,987
    Post Thanks / Like
    Likes (Given)
    5642
    Likes (Received)
    3813

    Default

    Quote Originally Posted by jephw View Post
    Hello everyone.
    I have some issues with getting the feeds and speeds dialed in with end mills. I am running a 1/2 TiALN Coated Endmill in 1018 steel. Our machine is a NL3000y mill/turn center.
    I was running the end mill at 220 SFM, 0.0035 feed/tooth, recommended by local supplier. Full length of cut (1") and a .06 step over. After the first part, roughly 40 minutes of work I was seeing a dull edge and tiny, tiny chips on the flutes already, coating also seemed to be showing signs of wear. What are the first adjustments I need to make to prolong tool life?

    Also - if I make the switch to 1045 material, how much do my variables need to change?
    Thanks everyone for your help.
    220 sfpm in 1018? With carbide?? 1" depth of cut and a .06 stepover is gravy.
    Find a new end mill supplier because that person is a moron.
    If this were in my VMC, I'd run it 3x faster (if not more) with that depth of cut and stepover.
    And that's with just a generic variable helix end mill from our resharp guys.

  4. Likes 5 axis Fidia guy liked this post
  5. #4
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,893
    Post Thanks / Like
    Likes (Given)
    2536
    Likes (Received)
    1292

    Default

    Good quality endmills pay for themselves pretty quickly. I like Helical for steels and Ti. Also, as has been discussed recently in another thread, use a corner radius whenever possible to maximize cutter life.

  6. #5
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    496
    Post Thanks / Like
    Likes (Given)
    239
    Likes (Received)
    417

    Default

    If this is a mill turn center, perhaps the live tooling that holds said endmill is being over taxed.

    We all know that the further stick out, and large parts sometimes need to be backed off due to resonance.

    How do the cuts sound? Is it squealing or crunchy sounding during the cut?

    I will say, most of my 1/2" endmills are running in the 350-550SFM range depending on setup in 1018.

  7. Likes mhajicek liked this post
  8. #6
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,271
    Post Thanks / Like
    Likes (Given)
    915
    Likes (Received)
    512

    Default

    Quote Originally Posted by Houndogforever View Post
    If this is a mill turn center, perhaps the live tooling that holds said endmill is being over taxed.

    We all know that the further stick out, and large parts sometimes need to be backed off due to resonance.

    How do the cuts sound? Is it squealing or crunchy sounding during the cut?

    I will say, most of my 1/2" endmills are running in the 350-550SFM range depending on setup in 1018.
    I agree...how does it sound? I believe those machines are supposed to have nice live tooling ability but that sounds a bit heavy for my lathes.

  9. #7
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,400
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2715

    Default

    Quote Originally Posted by jephw View Post
    Hello everyone.
    I have some issues with getting the feeds and speeds dialed in with end mills. I am running a 1/2 TiALN Coated Endmill in 1018 steel. Our machine is a NL3000y mill/turn center.
    I was running the end mill at 220 SFM, 0.0035 feed/tooth, recommended by local supplier. Full length of cut (1") and a .06 step over. After the first part, roughly 40 minutes of work I was seeing a dull edge and tiny, tiny chips on the flutes already, coating also seemed to be showing signs of wear. What are the first adjustments I need to make to prolong tool life?

    Also - if I make the switch to 1045 material, how much do my variables need to change?
    Thanks everyone for your help.
    .
    obviously things are effected by
    .
    tool length stickout amount
    tool holder length
    rigidity of machine
    rigidity of part has a effect
    hp of machine available (some rpm hp available can be much less than motor hp)
    part material and size of hard spots (some lots of metal might be 10x worst to machine)
    ability to hold part and distortion amounts by overtight work holding
    total tooling cost
    total scrap part costs
    .
    it wouldnt be the first time a part in a mill turn setup moved during machining.
    obviously using higher hp and tons of cutting forces can cause problems.
    .
    also some tooling might cost 2x more or 1/2 tool life but able to put a mirror finish
    on a part. just saying there are often tradeoffs for more important things wanted.

  10. #8
    Join Date
    Dec 2017
    Country
    CANADA
    State/Province
    Alberta
    Posts
    70
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    15

    Default

    Quote Originally Posted by jephw View Post
    Hello everyone.
    I have some issues with getting the feeds and speeds dialed in with end mills. I am running a 1/2 TiALN Coated Endmill in 1018 steel. Our machine is a NL3000y mill/turn center.
    I was running the end mill at 220 SFM, 0.0035 feed/tooth, recommended by local supplier. Full length of cut (1") and a .06 step over. After the first part, roughly 40 minutes of work I was seeing a dull edge and tiny, tiny chips on the flutes already, coating also seemed to be showing signs of wear. What are the first adjustments I need to make to prolong tool life?

    Also - if I make the switch to 1045 material, how much do my variables need to change?
    Thanks everyone for your help.
    What endmill is it? This sounds like a general purpose cheap endmill.
    If I were using a high performance variable flute end mill I would be starting in the 700 SFM, .0045 IPT range at that depth of cut and stepover.

  11. #9
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,580
    Post Thanks / Like
    Likes (Given)
    619
    Likes (Received)
    8548

    Default

    A true TiALN coating will do nothing at 220 SFM in 1018.
    In fact it will hurt performance of the tool against uncoated.
    Some of the better (read higher priced) TiALN coats have TiCN mixed in which does like low surface footage,
    This done for two reasons, one to increase the bond to the substrate and two to help with many customers not making enough heat to convert the TiAln to Al2O3.
    If coated at this low speed I'd be in TiCN. Some would say TiN but TiCN likes the lower speeds better.

    Unsure how much of the 40 minutes is actual tool in the cut time.
    Some would consider this not that bad but I'd think you might be giving up a lot of part cycle time with SFM this low.
    Is the 220 a machine limitation?
    Bob

  12. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,987
    Post Thanks / Like
    Likes (Given)
    5642
    Likes (Received)
    3813

    Default

    Oh god....he's back.


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
  •