Best type milling cutter for maximum metal removal
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Aug 2010
    Location
    GA
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default Best type milling cutter for maximum metal removal

    By that I mean we have a huge chunk of bronze(3,500lbs.) and our customer wants us to make chips out of it; that's it. Our customer melts the bronze down and their furnace lost power the other day. They were left with this big blob of bronze and they need it machined into shavings so they can start back melting it. Anyway, we're currently using a 6" face mill with positive geometry, .100" depth of cut at 48" IPM. We're just running a simple loop program that spirals in and then down again; rinse and repeat. The piece is in a Mori Seiki MV65 with 25hp at the spindle and a maximum spindle speed of 6,000. Any suggestions with another type cutter? I was thinking maybe something like a 2" milling cutter with radius inserts? Or maybe a 10" face mill? Though I'm not sure about the spindle load with that size cutter.

  2. Likes memphisjed liked this post
  3. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    seeing how it might have slag or hard spots mixed in I would watch for sudden insert failures.
    .
    many facemills with bigger inserts can take 0.2"DOC and ipt feeds of .010 to .020" ipt, if loadmeter near 100% than thats your machines limit obviously

  4. #3
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,629
    Post Thanks / Like
    Likes (Given)
    731
    Likes (Received)
    714

    Default

    I would get a plunge cutter and use that toolpath strategy, probably the fastest way to remove material if your cam can program it decent.

  5. #4
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,085
    Post Thanks / Like
    Likes (Given)
    1338
    Likes (Received)
    725

    Default

    Got a 3" indexable endmill? I'd spiral in with one of those, LOC maybe 1.5x to 2x D, using HEM/HSM/HFM cutting parameters. Maybe take all the cutters you're considering, plug them into HSMAdvisor, and see which gives you the highest MRR.

  6. #5
    Join Date
    Aug 2010
    Location
    GA
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Thanks all for the suggestions. Appreciate it.

  7. #6
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    137
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    23

    Default

    Ide just like to say that sounds like a hell of a fun time. Also it seems like you're in a better position then any of us to figure out which cutter works the best. I have zero actual input for you, other then have fun.

  8. #7
    Join Date
    May 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,507
    Post Thanks / Like
    Likes (Given)
    886
    Likes (Received)
    1637

    Default

    Quote Originally Posted by cranny View Post
    By that I mean we have a huge chunk of bronze(3,500lbs.) and our customer wants us to make chips out of it; that's it. [snip] The piece is in a Mori Seiki MV65 with 25hp at the spindle and a maximum spindle speed of 6,000.
    How the hell are you holding this thing? Any chance we can get a picture or two?

  9. Likes specgrade, Screwmachine liked this post
  10. #8
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    15

    Default

    I think 5axis has the right idea. Since Z is likely to be your stiffest axis. Plunge cut adjusting DOC and feed rate to max mrr.
    As a aside someplace on the web is a video of a vmc plunge cutting Ti using thru the tool LN2 as coolant. Rather impressive.

  11. #9
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,941
    Post Thanks / Like
    Likes (Given)
    399
    Likes (Received)
    6577

    Default

    A second vote for 5axis.
    It's hard to beat plunge roughing for MRR rates.
    Bob

  12. #10
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    689
    Post Thanks / Like
    Likes (Given)
    141
    Likes (Received)
    740

    Default

    I'll be the whipping boy with an alternate theory. Years ago I had a similar job... turning perfectly good metal into chips for the sake of the chips. Long story that involved a guy that checked himself out of a mental institution to pursue his dream of altering weather patterns with magnetics

    I finally decided that the best tool was the biggest corn cob rougher we could chuck up, buried as deep as the flutes would allow. We ran it days and days on end, just chugging along. We tried the inserted method, but sooner or later, an insert went hen shit and wiped out a bunch of stuff. The corn cob cutter would get dull and give a bunch of warning. It seems like we had someone that would sharpen the cutters, so we kept a couple in rotation.

  13. #11
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,638
    Post Thanks / Like
    Likes (Given)
    1222
    Likes (Received)
    2601

    Default

    Quote Originally Posted by 5 axis Fidia guy View Post
    I would get a plunge cutter and use that toolpath strategy, probably the fastest way to remove material if your cam can program it decent.
    Basically the dumbest CAM package on Earth will do it. Using basic point selection and a Drilling Toolpath, the user defines the cut parameters.

    But I agree it's pretty quick. Drilling big ass holes is king, but you need the HP to push giant Drills.

    R

  14. #12
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,941
    Post Thanks / Like
    Likes (Given)
    399
    Likes (Received)
    6577

    Default

    Quote Originally Posted by litlerob1 View Post
    Basically the dumbest CAM package on Earth will do it. Using basic point selection and a Drilling Toolpath, the user defines the cut parameters.

    But I agree it's pretty quick. Drilling big ass holes is king, but you need the HP to push giant Drills.

    R
    Yes basically drilling holes but with not full engagement and the step matters a lot.
    Once upon a time there were manual mills.
    This step and plunge was how you made lots of stock go away fast and every machinist knew how to do it along with the step that worked for any given cutter.
    Bob

  15. Likes Limy Sami liked this post
  16. #13
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    the basics
    1) you are limited by your machines hp. some cutters are more energy efficient that is remove more cubic inches per minute per hp but some cutters if you hit slag and destroy $1000 cutter within 10 seconds somebody saying they saved 1 hour but it cost a extra $1000. not sure how much they saved
    .
    2) cutting forces. when you put tons of force on a part you better make sure it wont move on you. sometimes small movement and there goes a $1000. cutter broken in pieces going flying
    .
    3) tooling cost if you end up using a extra $500. in tooling to make chips sometimes spending only $100. on tooling but taking a couple hours longer is worth it.

  17. Likes Cycle1000 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
  •