Best method for slotting aluminium?
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Oct 2013
    Location
    United Kingdom
    Posts
    144
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    24

    Default Best method for slotting aluminium?

    I have a job coming up that involves producing an enclosed 10mm wide slot through 20mm thick aluminum plate, the slots are approx 400mm long and there's about 300off to machine. Machine is a Mori Seiki MV-Junior and I'd like to keep the rpm to below 5000, any suggestions on tooling and method would be appreciated, I don't machine much aluminum.

  2. #2
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,458
    Post Thanks / Like
    Likes (Given)
    4049
    Likes (Received)
    2636

    Default

    Quote Originally Posted by gmc1724 View Post
    I have a job coming up that involves producing an enclosed 10mm wide slot through 20mm thick aluminum plate, the slots are approx 400mm long and there's about 300off to machine. Machine is a Mori Seiki MV-Junior and I'd like to keep the rpm to below 5000, any suggestions on tooling and method would be appreciated, I don't machine much aluminum.
    Well, with an MV-Junior you're belt driven, correct?
    If tolerance isn't really an issue I'd use a 10mm 2 flute UNcoated carbide end mill, and ramp down the center. You won't be able to go full depth and slot that with that machine.
    HSS could even be an option given your RPM limitations.
    Typically you'd go as fast as your spindle will allow when cutting aluminum.

  3. #3
    Join Date
    Oct 2013
    Location
    United Kingdom
    Posts
    144
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    24

    Default

    I should just clarify one point, I'm not looking to break any records, I'm just looking for a stable process that can be left to nibble away on it's own.

  4. Likes Cycle1000 liked this post
  5. #4
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,687
    Post Thanks / Like
    Likes (Given)
    7042
    Likes (Received)
    7152

    Default

    Why the 5000rpm cap?

  6. #5
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    187
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    96

    Default

    10mm = 0.3937"

    I would use a 3/8 endmill on the center line of the slot, then finish the walls with it if you need close dimensions and good finishes. You may be able to do the roughing in one pass with a 1" long endmill, your ratio is only 2:1.

  7. Likes exkenna, Cycle1000 liked this post
  8. #6
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,241
    Post Thanks / Like
    Likes (Given)
    1790
    Likes (Received)
    797

    Default

    Call ExKenna and order a 5/16x .88 LOC "streaker" (or comparable) brand endmill.
    Run a high speed path at full depth, and a 5-10% radial stepover. Keep your (radial chip thinned) IPT around .001-.002 and you should blaze through the slots.

  9. Likes exkenna liked this post
  10. #7
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    755
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    286

    Default

    Quote Originally Posted by gmc1724 View Post
    I should just clarify one point, I'm not looking to break any records, I'm just looking for a stable process that can be left to nibble away on it's own.
    What fun is that?

    While I'd be tempted in our machines to go full depth with a 3/8" tool, I know what kind of coolant flow I have with the flood coolant; I don't know how your coolant flow is.

    And since you sound like you're okay with it nibbling away and taking a couple minutes longer than technically possible, I'd use a 3/8 tool down the middle in 2, maybe 3 passes just to be "safe". You want to avoid chips getting packed in the flutes. They can, and will, weld into the flutes if you don't have enough coolant to flush them out.

    with a 3/8" tool going 5000rpm, lets say a 3 fluter (2 would be good, 4 is too many but you can use it) you could go about 30" inches per minute (about 800mm/min, 550mm/min for a 2 fluter) for the full slot down the middle (taking 2 or 3 passes of course) and that would be conservative

    after going full slot down the middle, step out to finish the walls the last little bit at a bit faster feeds.

    Some would say that's too slow, and they might be right, but it will work, and you probably won't break any provided your workholding is good and you have good coolant.


    Just thought as I walked away, if you do want to go *a bit faster*, 1 minute saved on a 300pc job is 5 hours of cutting time. You could save a day of work just pushing this one tool a bit faster. Up to you.

    And if Tom chimes in about how trying to save one minute of cycle time can cause 10 hours of fixing the machine, and how he has spent hours removing broken drills 10" deep into his 10000$ parts...
    Last edited by dandrummerman21; 11-14-2018 at 09:41 PM. Reason: 800mm not 80 lol

  11. Likes DethloffMfg liked this post
  12. #8
    Join Date
    Oct 2013
    Location
    United Kingdom
    Posts
    144
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    24

    Default

    Quote Originally Posted by dandrummerman21 View Post
    What fun is that?

    While I'd be tempted in our machines to go full depth with a 3/8" tool, I know what kind of coolant flow I have with the flood coolant; I don't know how your coolant flow is.

    And since you sound like you're okay with it nibbling away and taking a couple minutes longer than technically possible, I'd use a 3/8 tool down the middle in 2, maybe 3 passes just to be "safe". You want to avoid chips getting packed in the flutes. They can, and will, weld into the flutes if you don't have enough coolant to flush them out.

    with a 3/8" tool going 5000rpm, lets say a 3 fluter (2 would be good, 4 is too many but you can use it) you could go about 30" inches per minute (about 80mm/min, 55mm/min for a 2 fluter) for the full slot down the middle (taking 2 or 3 passes of course) and that would be conservative

    after going full slot down the middle, step out to finish the walls the last little bit at a bit faster feeds.

    Some would say that's too slow, and they might be right, but it will work, and you probably won't break any provided your workholding is good and you have good coolant.


    Just thought as I walked away, if you do want to go *a bit faster*, 1 minute saved on a 300pc job is 5 hours of cutting time. You could save a day of work just pushing this one tool a bit faster. Up to you.

    And if Tom chimes in about how trying to save one minute of cycle time can cause 10 hours of fixing the machine, and how he has spent hours removing broken drills 10" deep into his 10000$ parts...
    So I have a budget of 18mins per slot on these, I know that's a lifetime but if I can get it down to half that without standing over the e-stop I'd be happy. Is the general consensus to use 2 flute or 3 flute? High helix? Carbide or HSS? The flood coolant supply is quite good and the machine is old but decently rigid.

  13. #9
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,091
    Post Thanks / Like
    Likes (Given)
    171
    Likes (Received)
    1438

    Default

    Quote Originally Posted by gmc1724 View Post
    So I have a budget of 18mins per slot on these, I know that's a lifetime but if I can get it down to half that without standing over the e-stop I'd be happy. Is the general consensus to use 2 flute or 3 flute? High helix? Carbide or HSS? The flood coolant supply is quite good and the machine is old but decently rigid.
    Well that's a really lot of time for that operation . I get 1/3 in^3/min. We can do better .

    I'd consider a carbide corncob style of rougher in 3/8" size. At your 6,000 RPM and .002" chipload x 3 flutes, that's 36 IPM so a 2 depth cut toolpath would take 1 minute. Same speed and feed for the finish down each side and you are at 2 minutes.

    Regards.

    Mike

  14. Likes wheelieking71, Rstewart liked this post
  15. #10
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,687
    Post Thanks / Like
    Likes (Given)
    7042
    Likes (Received)
    7152

    Default

    Its a 3/8" end-mill, in shiny plastic. Why the low RPM? Is that all you have available?

  16. #11
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    900
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    570

    Default

    Jwshultz alumigator 3/8 with the roughing cuts up the side they haul ass.


    Sent from my iPhone using Tapatalk Pro

  17. #12
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,175
    Post Thanks / Like
    Likes (Given)
    777
    Likes (Received)
    2235

    Default

    Quote Originally Posted by wheelieking71 View Post
    ....Why the low RPM? Is that all you have available?
    6K was standard on the MVJR. I'm guessing he wants to stay under max RPM due to spindle concerns. The MVJR was a table guard type machine too so chips and coolant flying might be a consideration too.

  18. #13
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    755
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    286

    Default

    Quote Originally Posted by gmc1724 View Post
    So I have a budget of 18mins per slot on these, I know that's a lifetime but if I can get it down to half that without standing over the e-stop I'd be happy. Is the general consensus to use 2 flute or 3 flute? High helix? Carbide or HSS? The flood coolant supply is quite good and the machine is old but decently rigid.
    I just wanted to mention that if you take the speeds/feeds I mentioned above, I didn't convert my inches per minute to mm per minute right. should be around 800mm per minute when I said 80.

    As someone else mentioned, you'd get that slot done in just a few minutes even if you take 3 passes and a finish pass.

  19. #14
    Join Date
    Nov 2007
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,492
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    263

    Default

    Since you are RPM limited I would look for a tool that thrives off of feed.

    I highly recommend the 3 flute Destiny DiamondBack 3/8" carbide rougher.
    Then, as others have mentioned a fast finish pass on the sidewalls with a Destiny 3/8" 3 flute Viper.
    With the Stealth Moly-S coating these are very hard to beat. Exceptional tool life and MRR.

    Diamond Back S&F - Destiny Tool

    X

  20. Likes wheelieking71, Philabuster liked this post
  21. #15
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,992
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2593

    Default

    Quote Originally Posted by gmc1724 View Post
    I have a job coming up that involves producing an enclosed 10mm wide slot through 20mm thick aluminum plate, the slots are approx 400mm long and there's about 300off to machine. Machine is a Mori Seiki MV-Junior and I'd like to keep the rpm to below 5000, any suggestions on tooling and method would be appreciated, I don't machine much aluminum.
    .
    depends on part shape. if part vibrates badly you might need to use more than one pass roughing. usually better to use end mills made for aluminum on aluminum. coolant helps gets chips out of the way and helps prevent chips sticking to cutter
    .
    obviously cost of part is a factor. if part moves in vise and is scrapped that can be expensive. many parts you use too much vise pressure it leaves vise marks which are unacceptable on part. also parts tend to bend or distort when vise extra tight. thats why often vise is often rechucked at lower torque before finish cuts
    .
    most take a later finishing cut for precision and sharper corners as rougher often has bigger radius on corners


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
  •