Roughing end mill help
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 56
  1. #1
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default Roughing end mill help

    I haven't had much experience using a roughing end mill in a cnc machine previous to this part so I am a bit in the dark on how to run it. We have a lot of material to remove so it's important I get it right so we don't burn through tools! The material is 4140A, the set-up is not an issue, plenty to grab by in the vice. I am using a HSS 3/4 diameter x 1-5/8 length roughing endmill, machine has 20HP. I am side milling, the required depth is 1.5 inches. My initial numbers are 1.5 axial depth of cut, .116 radial depth of cut, speed 500 RPM and feed of 6.6 ipm. After the first piece the endmill seems to be cutting fine but already looks a bit worn, should I not be taking the full 1.5 inch depth at once?

    Thanks for your help!

  2. #2
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    138
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    82

    Default

    I would guess that you could bump up your feed considerably with that little radial engagement. Have you looked at the manufacture recommended speeds and feeds?

  3. #3
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Manitoba
    Posts
    260
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    106

    Default

    Are you cutting through mill scale? Your numbers aren't that far off maybe a bit more feed. Coolant?

  4. #4
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    930
    Post Thanks / Like
    Likes (Given)
    86
    Likes (Received)
    457

    Default

    Any reason (other than cost) you aren't using carbide? How much total do you need to remove?

  5. Likes Bobw, mhajicek, PegroProX440 liked this post
  6. #5
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    43

    Default

    I think you might be running a little too fast. Does your em have a coating? Sounds slow but I think 350 rpm and 5.0 in/min would be where I would start. That's .0039"/tooth and 64f/min.

  7. #6
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,742
    Post Thanks / Like
    Likes (Given)
    491
    Likes (Received)
    273

    Default

    One problem with not taking the full 1.5 depth is that you wear out the end of the flutes before the rest of the cutter is done. I'd go full depth.
    Years ago, I had to use long 1.5" diameter roughing HSS mills on a weldment. I think the cut length was 6". Anything carbide we had was too short or ran too rough.
    Just keep a good flood of coolant on your mill or it "could" weld to the part.
    (Ask me how I know.....)

  8. #7
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Wow guys thank you for all the quick responses!
    We are using plenty of coolant. I think we could use a larger radial engagement but I am forced to feed into a corner so I was afraid it would be too much engagement in the corner. Not using carbide because I don't have much experience with this type of cutter and didn't wanna blow up an expensive tool! The chips look good (at least from what I can tell), small and silver, no crazy colors. The endmill does not have any coating on it, we just ordered something fairly cheap from MSC...so our cutter could be the problem.

    We aren't cutting through any scale, it is a nice squared block. We have a lot of material to remove: 1.5 x 4 x 3.5 twice on 22 pieces (approximately, from memory)

  9. #8
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    930
    Post Thanks / Like
    Likes (Given)
    86
    Likes (Received)
    457

    Default

    Quality doesn't cost, it pays.

    Are you leaving an island or facing? I'd almost say you should just plunge mill with the proper size cutter.

    Let's be real with ourselves for a minute, a cheap uncoated hss endmill is not going to last long in 4140...let alone 22 pieces worth.

  10. Likes HuFlungDung, Bobw, DavidScott liked this post
  11. #9
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,629
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    3301

    Default

    That is probably a max depth condition for a tool that diameter. I'd go for a 1" solid carbide rougher from Maritool. That is such a sweet cutting tool I wish I could use it more. Plus, it's carbide: you can get something done in an hour!!

    I had a bunch of 3/4" HSS roughers given to me, so I used them up on a job. Surprisingly, those would keep cutting when they looked like they were getting pretty dull. But with HSS, you are wasting time running too slow, that's got to add up to cost savings using carbide when the metal removal is serious.

  12. #10
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Part starts as a rectangle and when its done it is an L with the large leg of the L against the back jaw. So it is sounding like our issue is the tool mostly. Would I run similar numbers with a carbide rougher or coated hss?

  13. #11
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,629
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    3301

    Default

    Quote Originally Posted by SamS View Post
    Part starts as a rectangle and when its done it is an L with the large leg of the L against the back jaw. So it is sounding like our issue is the tool mostly. Would I run similar numbers with a carbide rougher or coated hss?
    If you go for the beefier carbide tool, you can increase the feed rate. This more than makes up for having to run the rpm lower than for a 3/4" endmill.

    For me, a lot of what guides my choice of feed rate is how the machine setup reacts to the cut, If it is purring along, you feel comfortable increasing the feed. So don't limit yourself with a tool too small when the situation allows for the sturdier tool.

  14. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,612
    Post Thanks / Like
    Likes (Given)
    93
    Likes (Received)
    1132

    Default

    Looks like you are only removing 1.2 in^3 per minute. I should think you could do 10x that with your 20 HP, using carbide tools and HSM toolpaths. I would suggest commodity 1/2" 4- or 5-flute straight endmills instead of much more expensive 3/4" endmills. HSM parameters are readily found in this forum for the asking.

    Regards.

    Mike

  15. Likes Bobw liked this post
  16. #13
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Manitoba
    Posts
    260
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    106

    Default

    Quote Originally Posted by HuFlungDung View Post
    If you go for the beefier carbide tool, you can increase the feed rate. This more than makes up for having to run the rpm lower than for a 3/4" endmill.

    For me, a lot of what guides my choice of feed rate is how the machine setup reacts to the cut, If it is purring along, you feel comfortable increasing the feed. So don't limit yourself with a tool too small when the situation allows for the sturdier tool.


    I agree. If you were using 3/4" carbide endmill, your feed could easily increase 2 to 3 times. Most machines will run out of HP before maxing out a 1" carbide so you're still limited. But for tool longevity and rigidity in cutting steel, you can't beat it. For 22 parts it's worth spending the $100 up front. 1" carbide? I can't imagine my 15 HP spindle being able to make full use of it.

  17. #14
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,546
    Post Thanks / Like
    Likes (Given)
    12078
    Likes (Received)
    9687

    Default

    I'm going to be a dick..

    That's 1.15 cubic inches a minute.. About a 1hp cut.. On a 20hp machine.

    You might as well sell the damn machine and buy a hammer and chisel.

    A half inch varifult, Maritool, Titan, Imco etc... Will cost under $50 each,
    and tear up a shit load of material. Even trying to baby it, you should be
    able to pull 4 cubic inches a minute.. Letting it rip, 10+ easily.. Turn that
    whole block to chips in 2 minutes..

    This is 4340 annealed, essentially the same as your 4140.. One single
    sub $50 endmill created 3 of those piles (I know, it was the last pile,
    and all the barrels in the shop were full, and the cleaning guy was
    coming in the morning.) Pulling somewhere around 12 cubic inches a minute..

    And it wasn't even on a real machine, it was a Fricken Fadal for cripes sake.




    I think its already been said, but you are playing the false economy game,
    save a few dollars on a single endmill, and lose $100's to $1000's because
    you didn't want to buy a quality tool for $5 more, that would last longer
    and move material a hell of a lot quicker..

    And did you buy just one?? You NEVER buy ONE.. If you buy one, it gets
    lonely and commits suicide.. If you buy 3, the first one wants to go
    party with the other 2 in the box, so it lasts forever.

  18. Likes HuFlungDung, mjk, mountie, gkoenig, SamS and 13 others liked this post
  19. #15
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,629
    Post Thanks / Like
    Likes (Given)
    1189
    Likes (Received)
    3301

    Default

    Quote Originally Posted by Rigor View Post
    I agree. If you were using 3/4" carbide endmill, your feed could easily increase 2 to 3 times. Most machines will run out of HP before maxing out a 1" carbide so you're still limited. But for tool longevity and rigidity in cutting steel, you can't beat it. For 22 parts it's worth spending the $100 up front. 1" carbide? I can't imagine my 15 HP spindle being able to make full use of it.
    With a 1.5" depth of cut, you can always make use of the rigidity of the 1" diameter tool. The machine in use may dictate what is best: if your machine has no gearbox for low range, then perhaps you're better off running a smaller diameter tool at higher rpm to get the spindle into it's better part of the torque curve.

    PS: and your feed rate (in IPM) should definitely increase 4 times or more, for the carbide tool over the HSS.

  20. #16
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    We bought 4, we learned that lesson before! You're helping me out a ton so I don't care if you're a little bit of dick. I should have mentioned we are using conversational programming for this part so HSM toolpaths are out of the equation. I totally see your point and I'll learn from this! My only worry with getting a 1/2 endmill is the rigidity to cut 1.5 inch depth.

  21. Likes Bobw, ManualEd liked this post
  22. #17
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,612
    Post Thanks / Like
    Likes (Given)
    93
    Likes (Received)
    1132

    Default

    Quote Originally Posted by SamS View Post
    My only worry with getting a 1/2 endmill is the rigidity to cut 1.5 inch depth.
    Not a big deal with HSM toolpaths where deflection is pretty low, and is mostly inline with the cutting direction as opposed to traditional toolpaths where the deflection is more perpendicular to the cutting direction such that you start seeing the tool banging against the wall of the part.

    Regards.

  23. #18
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    So I was able to run the program once I decreased by axial depth of cut. So it's cutting (albeit slowly) until the carbide cutter comes in from Maritool. We went with the 3/4 coated carbide from them. If you don't mind helping me again what would be some safe numbers to start off with side milling with carbide cutter? We are climb milling, still force to go into a .7 radius corner. Material is 4140A. Thanks again guys!

  24. #19
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,546
    Post Thanks / Like
    Likes (Given)
    12078
    Likes (Received)
    9687

    Default

    Quote Originally Posted by SamS View Post
    So I was able to run the program once I decreased by axial depth of cut. So it's cutting (albeit slowly) until the carbide cutter comes in from Maritool. We went with the 3/4 coated carbide from them. If you don't mind helping me again what would be some safe numbers to start off with side milling with carbide cutter? We are climb milling, still force to go into a .7 radius corner. Material is 4140A. Thanks again guys!
    Which ONE did you get???

  25. #20
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    5

    Default

    Part #: 1010-.750-1.5
    4 Flute Carbide TIALN Coated Roughing End Mill 3/4 x 1.5 flute length

  26. Likes Bobw liked this post

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
  •