High Feed Milling in Aluminum?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,470
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    925

    Default High Feed Milling in Aluminum?

    Here's an oddball. I've got some parts I did because a local business needed a few prototypes fast. Well, they want me to make more but my pricing was too high. I had them redesign the part to get a certain feature (heat sink) so I could attack it normal to the surface instead of using a slitting saw at 90deg. There are cross slots (basically a bunch of rectangles sticking up from the surface) that have 0.125" between then and they are 0.5" tall.

    Am I crazy to think I can try a small solid carbide high feed to quickly zig-zag down between these features? Side wall finish isn't important. I was going to use a Niagara N13996 since I've used those before in steel and have some idea for starting parameters.

    Otherwise, ball end mill? Stub flute reduced shank?

    If I can do this I can likely get the price in line with what they want. Otherwise, I'm not dropping my price and not making my hourly rate, I'll just pass.

  2. #2
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    367
    Likes (Received)
    28

    Default

    When you CAMed it, did the time get down to what you needed? I'll often try it in CAM before committing to a process. Sometimes Volumill is not the best solution to roughing.

  3. #3
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    53

    Default

    If the geometry works with a ballnose you should be able to go pretty fast with a .125" ball, .5" reach isn't too bad. You will probably be limited by spindle speed more than anything.

    We run a lot of rib cutters on mold parts, usually milling steel in our case but it looks like we would run a tool like this (in steel) at 20,000rpm .002"/tooth and .006" downsteps just as a point of reference. Should be able to go a bit harder in aluminum, although it would be easier with more rpms

  4. #4
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    2187
    Likes (Received)
    769

    Default

    Quote Originally Posted by Chris59 View Post
    When you CAMed it, did the time get down to what you needed? I'll often try it in CAM before committing to a process. Sometimes Volumill is not the best solution to roughing.
    beware blindly following the estimated machining times as they will vary WILDLY depending on the type of toolpath, machine kinematics and capability etc.
    for example, if you program a small part (lets say 2" square pocket) at 500 IPM, it'll tell you a ridiculously small #, but in reality no machine would achieve real life 500 IPM inside a 2" pocket, especially corners etc.

  5. Likes mhajicek liked this post
  6. #5
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    2187
    Likes (Received)
    769

    Default

    Quote Originally Posted by 007Rob View Post
    If the geometry works with a ballnose you should be able to go pretty fast with a .125" ball, .5" reach isn't too bad. You will probably be limited by spindle speed more than anything.

    We run a lot of rib cutters on mold parts, usually milling steel in our case but it looks like we would run a tool like this (in steel) at 20,000rpm .002"/tooth and .006" downsteps just as a point of reference. Should be able to go a bit harder in aluminum, although it would be easier with more rpms
    why ball? wouldnt that be a lot of tool pressure.

  7. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,145
    Post Thanks / Like
    Likes (Given)
    5754
    Likes (Received)
    3928

    Default

    You could zig zag down, but I doubt that would be faster than a slitter in aluminum.
    I wouldn't bother buying a high-feed style end mill, just use a bullnose if you go that route.

    Or depending on your setup and holding, you could make a special slitter arbor that has spacing for multiple slitter cutters and do it all in one shot.

  8. Likes BT Fabrication liked this post
  9. #7
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,498
    Post Thanks / Like
    Likes (Given)
    1427
    Likes (Received)
    1556

    Default

    I would try a stub reduced shank from Harvey. Get 3 so you can break one finding out how fast you can go. At 15k and .125 deep slotting I bet you could feed 150 to 225 ipm"?, at least on the first pass. Chip evacuation may be the limiting factor.

    If you can use a .1575" diameter cutter then the Garr roughers are the way to go. They are available in 8,10, 12, and 15mm loc. An 8mm reduced shank with Tib2 could feed .25" deep and 225 ipm with clearing the chips being the limiting factor. I ran a 3/16" stub .24" deep 120 ipm at 6k for a few years slotting 6061 plate so I am familiar with these tools. If I had more coolant pressure to clear the chips I could have fed much faster. I only have a 1/4hp pump which works fine for everything else but sucked for this operation.

  10. Likes barbter liked this post
  11. #8
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,071
    Post Thanks / Like
    Likes (Given)
    240
    Likes (Received)
    611

    Default

    Depends on how many parts you are making but I would try an endmill and zig zag it back N forth. Another option is plunging it out and then do a finish pass to clean it up.

  12. #9
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    53

    Default

    Quote Originally Posted by empwoer View Post
    why ball? wouldnt that be a lot of tool pressure.
    I guess you have a point, I was just thinking the bigger radius on a ball would have a greater chip-thinning effect in a full slot. A high feed tool making a slot the same size as the tool will have similar issues as it gets deeper and starts engaging on the corners.

  13. #10
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,778
    Post Thanks / Like
    Likes (Given)
    810
    Likes (Received)
    836

    Default

    Quote Originally Posted by 007Rob View Post
    I guess you have a point, I was just thinking the bigger radius on a ball would have a greater chip-thinning effect in a full slot. A high feed tool making a slot the same size as the tool will have similar issues as it gets deeper and starts engaging on the corners.
    Off topic, but oddly enough I often rough ribs in hard mold steel with a ball endmill. A ball after all is the strongest cutting shape. I have done crazy deep ribs that way. 10:1 cutting dia ratio is a piece of cake, 15:1 is still doable in hard S-7, but with caution.

  14. Likes 007Rob liked this post
  15. #11
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,360
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    657

    Default

    Quote Originally Posted by DavidScott View Post
    I would try a stub reduced shank from Harvey. Get 3 so you can break one finding out how fast you can go. At 15k and .125 deep slotting I bet you could feed 150 to 225 ipm"?, at least on the first pass. Chip evacuation may be the limiting factor.

    If you can use a .1575" diameter cutter then the Garr roughers are the way to go. They are available in 8,10, 12, and 15mm loc. An 8mm reduced shank with Tib2 could feed .25" deep and 225 ipm with clearing the chips being the limiting factor. I ran a 3/16" stub .24" deep 120 ipm at 6k for a few years slotting 6061 plate so I am familiar with these tools. If I had more coolant pressure to clear the chips I could have fed much faster. I only have a 1/4hp pump which works fine for everything else but sucked for this operation.
    You talking the knuckle form fine pitch ripper?

  16. #12
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,498
    Post Thanks / Like
    Likes (Given)
    1427
    Likes (Received)
    1556

    Default

    Quote Originally Posted by barbter View Post
    You talking the knuckle form fine pitch ripper?
    Yes.

    And I need more characters...

  17. Likes barbter liked this post
  18. #13
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,366
    Post Thanks / Like
    Likes (Given)
    9914
    Likes (Received)
    9418

    Default

    Rick, are you wanting to attack it this way because the slitting is slow? Or do you want to eliminate the 3rd operation?
    I ask because: no way you are going to get anywhere near the speed of an optimized saw, with an end-mill!
    If the volume is there to afford an application specific saw? Call AB Tools and get a good saw.
    How fast were you feeding the saw you originally tried it with?

    I saw your pic of those on IG. I would slit that all day every day.
    I can't remember, do you have a 4th in your mill? Could help to keep the shank short. But, AB will make whatever you need.

    If you end up not wanting the job, send them my way! LOL

  19. Likes Matt_Maguire liked this post
  20. #14
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,470
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    925

    Default

    Thanks for the replies! I have a few of the Harvey reduced shank in the tool box already, and could give those a try. As wheelie guessed, this is more about multiple operations than it is the absolute speed. My biggest issue is being chief cook and bottle washer, and I just can't spend the time to tend a machine for a few days while my product line parts are sitting on the material rack waiting to be cut, and the phone is ringing, and the emails are coming in, and the checks need to be signed, and... I also already have some of the small high feeds I could try. No really small ball mills, though. I have a nice HSS slitting saw that I could do these with (my first run I was limited because McMaster only has jeweler's saws in 0.045" which was the original slot width and I needed something next day - I had a lot of issues with chip packing due to the fine tooth count). It has dished top and bottom for clearance and low tooth count, but it does not have staggered teeth. I don't have a 4th axis.

    No matter what, the quantity here is only 40-50 EAU, with releases of 4-8 parts a month. Wheelie if you saw it, the whole assembly I had quoted at $49.XX plus $4.XX for the little angle bracket that was added later. Customer is targeting $30 per complete assembly. I don't think the Okuma will do it. I could do it with a Speedio, I bet. But I'd still be machine tending.

    On a side note, I don't buy from AB anymore after some IG posts last year. That's all I'll say as I don't want to shit up a thread with it. I have Sharon Cutwell here locally as well as Integrity Saw and Tool, and both are fast and make very good tools at competitive prices. Harvey is usually very expensive, but I can get it next day.

  21. #15
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,470
    Post Thanks / Like
    Likes (Given)
    387
    Likes (Received)
    925

    Default

    How about this - is it realistic to run a 1/8" thick, 2" slitting saw, 34-38T, 0.500" deep at 0.0008" per tooth and 970rpm? Or am I still going to see chip packing?

  22. #16
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    14,118
    Post Thanks / Like
    Likes (Given)
    3083
    Likes (Received)
    9358

    Default

    Quote Originally Posted by Rick Finsta View Post
    How about this - is it realistic to run a 1/8" thick, 2" slitting saw, 34-38T, 0.500" deep at 0.0008" per tooth and 970rpm? Or am I still going to see chip packing?
    If I had my choice, I'd be looking for a coarser tooth saw, perhaps 15-18T @ 2". Higher RPM, work feed up to what you're comfortable with. Shouldn't pack unless it's poor geometry or coolant flush.

    I would want it keyed, with a short, stout arbor, and the work securely held to make sure I couldn't rip it from the vise. .002"-.003" per tooth, maybe more if everything feels good.

  23. Likes Delw, wheelieking71, jaguar36 liked this post
  24. #17
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    1,292
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    522

    Default

    Rick
    we used to use a ton of these when heat sinks were popular back in the 90's. if you dont have a indexer make a fixture and lock in vise.

    we used them in full rad and sharp corner. got them in carbide tips and highspeed steel I honestly cant remember where I got them I think thrustan? or something like that. keyways are a must if feeding fast. finish is awsum as well one or 2 passes,

    pic is of the style
    McMaster-Carr

  25. #18
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,366
    Post Thanks / Like
    Likes (Given)
    9914
    Likes (Received)
    9418

    Default

    Quote Originally Posted by Rick Finsta View Post
    How about this - is it realistic to run a 1/8" thick, 2" slitting saw, 34-38T, 0.500" deep at 0.0008" per tooth and 970rpm? Or am I still going to see chip packing?
    This is exactly what I was talking about!
    How about a 3" x .125" saw, 9 teeth, 4,000rpm, .0004~5"/tooth. I have a spare you can try!

    Quote Originally Posted by Rick Finsta View Post
    On a side note, I don't buy from AB anymore after some IG posts last year. That's all I'll say as I don't want to shit up a thread with it.
    Message sent on IG........

  26. #19
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,366
    Post Thanks / Like
    Likes (Given)
    9914
    Likes (Received)
    9418

    Default

    Quote Originally Posted by Milland View Post
    If I had my choice, I'd be looking for a coarser tooth saw, perhaps 15-18T @ 2". Higher RPM, work feed up to what you're comfortable with. Shouldn't pack unless it's poor geometry or coolant flush.

    I would want it keyed, with a short, stout arbor, and the work securely held to make sure I couldn't rip it from the vise. .002"-.003" per tooth, maybe more if everything feels good.
    Yes Sir! A lot of my machinist buddies hate saws. Not me! Let 'er rip! But yea, need to get the tooth count in ALU way down.

  27. #20
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    6,416
    Post Thanks / Like
    Likes (Given)
    6862
    Likes (Received)
    3723

    Default

    I cut a lot of 1/8" deep .062" grooves in 6061 with a 3" HSS saw. I think I've ten folded the recommended feedrate and the original saw is going strong years later.


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
  •