High speed machining aluminum... An open discussion.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 40
  1. #1
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default High speed machining aluminum... An open discussion.

    My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

    1/2 3 flute end mill

    2020 sfpm ( 15,432 rpm)
    .008 chip load (feed 370)
    20% step over (.100)
    200% axial depth (1.000) max

    I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

    I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.


    So, what is everyone else's go to high speed parameters? Discuss!

  2. Likes frank Texas liked this post
  3. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,057
    Post Thanks / Like
    Likes (Given)
    160
    Likes (Received)
    1417

    Default

    BT30 spindle (not dual-contact)
    3/8" or 1/2" 3-flute
    16,000 RPM
    288 IPM (.006" chipload)
    35% stepover
    Up to 1" axial for 3/8", 1-1/4" for 1/2"

    I'm very happy with these parameters. Roughing is usually only like 10% of my cycle times so I spend a lot more time optimizing and tuning elsewhere.

    Regards.

    Mike

  4. Likes BRIAN.T, barbter, frank Texas liked this post
  5. #3
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by Finegrain View Post
    BT30 spindle (not dual-contact)
    3/8" or 1/2" 3-flute
    16,000 RPM
    288 IPM (.006" chipload)
    35% stepover
    Up to 1" axial for 3/8", 1-1/4" for 1/2"

    I'm very happy with these parameters. Roughing is usually only like 10% of my cycle times so I spend a lot more time optimizing and tuning elsewhere.

    Regards.

    Mike
    That's great, and those are wildly different numbers then mine. I knew this would be interesting. Thanks

  6. #4
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,442
    Post Thanks / Like
    Likes (Given)
    952
    Likes (Received)
    992

    Default

    Depends on what you are roughing with. Corncob mills will put you in a different state as far as chip loads go. 3/8" mills are .01"- .035" per tooth, and those are just for starters. Almost always I can't hold onto my parts well enough to even start to push the endmill, bummer.

  7. Likes BRIAN.T, StirlingMachine liked this post
  8. #5
    Join Date
    May 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,493
    Post Thanks / Like
    Likes (Given)
    885
    Likes (Received)
    1611

    Default

    One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.

  9. Likes Larry Dickman, dstryr, AARONT liked this post
  10. #6
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,207
    Post Thanks / Like
    Likes (Given)
    347
    Likes (Received)
    563

    Default

    Quote Originally Posted by [email protected] View Post
    One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.
    They sure do if the guy runs it in dry run. I’ve solved that problem for my guys more than once

  11. Likes Mtndew liked this post
  12. #7
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,630
    Post Thanks / Like
    Likes (Given)
    686
    Likes (Received)
    1856

    Default


  13. #8
    Join Date
    Nov 2007
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,488
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    261

    Default

    Quote Originally Posted by BRIAN.T View Post
    My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

    1/2 3 flute end mill

    2020 sfpm ( 15,432 rpm)
    .008 chip load (feed 370)
    20% step over (.100)
    200% axial depth (1.000) max

    I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

    I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.


    So, what is everyone else's go to high speed parameters? Discuss!
    So many variables.. tool, spindle, fixturing, etc. I think your numbers are just fine.
    If your spindle is happy and the part stays in the vise all is good.
    The real question: Are you making good money at these parameters? If so, you're golden.

  14. Likes frank Texas liked this post
  15. #9
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by Hazzert View Post
    They sure do if the guy runs it in dry run. I’ve solved that problem for my guys more than once
    I'm sure he is referring to the machines ability to accelerate.

    Quote Originally Posted by [email protected] View Post
    One can program 370 or 800 inches per minute, but does one actually receive what one asked for? One thinks likely not.
    As for acc/Dec my 3 axis mills (which are all the same) have a Max feed rate of 370, which I have no problem achieving with the correct Gcode. Without the high speed codes in place the mills only get up to about 200ipm. My 5 axis tops out at about 1200ipm. I've never tried anything above about 500ipm. But ide be inclined to agree that people who program at outrageous feeds rarely see those numbers in practice.

  16. Likes frank Texas liked this post
  17. #10
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by exkenna View Post
    So many variables.. tool, spindle, fixturing, etc. I think your numbers are just fine.
    If your spindle is happy and the part stays in the vise all is good.
    The real question: Are you making good money at these parameters? If so, you're golden.
    Yeah you are absolutely right. My cat40 (single contact...? Is that the opposite of dual contact) don't always love those numbers. My HSK spindle, sounds like I'm cutting air. Hsk is a beautiful thing.

  18. #11
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by gkoenig View Post
    Ahhhhhb so good! Thanks man! Shit made my day.

  19. #12
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,313
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    357

    Default

    20 percent is aggressive but that chipload is light. .010 to .015 with a 15 to 18 percent stepover. If the material is held rigidly I dont think your numbers are too far off. If you have the drawbar force and taper for it double that chip load. Most aluminums are just butter needing to be peeled off

  20. Likes BRIAN.T liked this post
  21. #13
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    2,606
    Post Thanks / Like
    Likes (Given)
    1267
    Likes (Received)
    1262

    Default

    Quote Originally Posted by DavidScott View Post
    Depends on what you are roughing with. Corncob mills will put you in a different state as far as chip loads go. 3/8" mills are .01"- .035" per tooth, and those are just for starters. Almost always I can't hold onto my parts well enough to even start to push the endmill, bummer.

    That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.

  22. Likes frank Texas liked this post
  23. #14
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    714
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    259

    Default

    Quote Originally Posted by Mike1974 View Post
    That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.
    I often have the same problem. And for most jobs, that is enough, don't try to hog it out super fast, and that is enough.


    For slightly better protection, when running steel only holding onto that much, I go with the talon grip jaws that bite in a bit. It is an obvious improvement, but also obviously only works if you are milling all around the part and can flip it.

    But lately, I am beginning to consider making my own dovetail soft jaws for those really pesky jobs that i only have a bit to hold onto and need a lot sticking out of the vise. I have a dovetail cutter and some dovetail jaws for the 5th axis vise, and because I see how securely those dovetails hold onto the part, I have a 3axis job on my desk here that I'm gonna dovetail first, because we had pullout issues on it before.

    As for speeds and feeds in aluminum, I only have 6000rpm on most machines, so for roughing applications, 6000rpm/150ipm/.25"stepover/1" deep.. I drop to 5000rpm/60ipm/.5" deep for full slotting applications, 1/2" endmill in 7075

    I am not breaking any records by any means, but gets the job done quick.
    Last edited by dandrummerman21; 04-16-2019 at 03:14 PM. Reason: wrote wrong feedrate duh.

  24. #15
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by Speedie View Post
    20 percent is aggressive but that chipload is light. .010 to .015 with a 15 to 18 percent stepover. If the material is held rigidly I dont think your numbers are too far off. If you have the drawbar force and taper for it double that chip load. Most aluminums are just butter needing to be peeled off
    That is fascinating, you're approach is backwards from mine, though I definitely love the idea of less stepover with a larger chip, but again on my 3 axis I'm limited with my feeds. Im going to see what kind of chip.i can make on my 5 axis soon. Thanks.

  25. #16
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by dandrummerman21 View Post
    6000rpm/300ipm/.25"stepover/1" deep..

    I am not breaking any records by any means, but gets the job done quick.
    Don't sell yourself short, that's a hell of a chip you're making. Is this cat40?

  26. Likes J Gilles liked this post
  27. #17
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    95
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    19

    Default

    Quote Originally Posted by Mike1974 View Post
    That is my problem. We do sooo much variety, but most of it ends up being held onto .05" in standard vise jaws. Yes, I know there are better ways to hold onto minimal stock, but we don't have it. Also, as someone else said, roughing is normally (for us anyways) about 5-10% of the time so I don;t see the point in pushing the rough balls out... I know there are other factors, but a big run for us would be 50 pieces too.
    It took me about 2 years to convince the owner that more stock was well worth the extra money. Faster roughing, faster setups, far less error. When I started here we (they) would saw cut most parts to size then try to machine precision parts. It was embarrassing.

  28. #18
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,354
    Post Thanks / Like
    Likes (Given)
    3144
    Likes (Received)
    2400

    Default

    Quote Originally Posted by BRIAN.T View Post
    My go to feeds and speeds for roughing aluminum are... Sometimes I push, sometimes not, but this is my starting point.

    1/2 3 flute end mill

    2020 sfpm ( 15,432 rpm)
    .008 chip load (feed 370)
    20% step over (.100)
    200% axial depth (1.000) max

    I was talking to a pretty experienced guy a while back who told me he was regularly at 800 inches per minute. Which got me wondering "what does he know that I don't?"

    I've concluded that either he was trying to impress me with some Titan type numbers or his stepover is 10% or less, in which case what's the point? 800 ipm at 10% or 400 @ 20.


    So, what is everyone else's go to high speed parameters? Discuss!
    I'd say your biggest improvements will be from increasing stepover by 5% increments until you find the limit. I have machines with 50hp but roughing tends to be such a small percentage of the overall cycle time for us most of the time. I usually find way more cycle time improvement by running multiple parts a cycle, reducing air cutting, moving to 4/5 flute aluminum finishing cutters. Only takes one chucked part or one broken tool to wipe out the savings of pushing away from process reliability and then it was all for nothing unless you are like Tony or Greg trying to run 10k parts a week and pushing for seconds in saving

  29. Likes DethloffMfg, exkenna liked this post
  30. #19
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    2,606
    Post Thanks / Like
    Likes (Given)
    1267
    Likes (Received)
    1262

    Default

    Quote Originally Posted by BRIAN.T View Post
    It took me about 2 years to convince the owner that more stock was well worth the extra money. Faster roughing, faster setups, far less error. When I started here we (they) would saw cut most parts to size then try to machine precision parts. It was embarrassing.
    I tried to 'sell' talon grips here... Oh well, it appears the agreement is 'fast enough' for roughing when it is such a small part of the machining process. With the odd standouts making a bazillion parts a year.

  31. #20
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,442
    Post Thanks / Like
    Likes (Given)
    952
    Likes (Received)
    992

    Default

    I am doing more and more aluminum plates that have to be machined on all surfaces but I get to put a radius on the top, my design. This allows me to reduce the wasted material to a bare minimum but I only get to hold onto .03" to .05" of the part. I despise any waste and the quantities are in the thousands a year so any savings will add up, my designs so as long as they sell I will be making them. It's been a long time coming but I just made a small batch of steel wedge clamps and stops with teeth .015" apart to use in my fixtures. I have found that I only need to bite into the aluminum about .001"-.002" for it to hold. The difference between a smooth clamping surface and one with teeth is AMAZING!!!! So nice to go from babying the thing for fear the parts will pull out of the fixture to not giving it a thought cause they are not going to move, period!


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
  •