How to get best "mirror" machined flat finish on 6061 aluminum
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 67
  1. #1
    Join Date
    Mar 2002
    Location
    Brisbane, CA, USA
    Posts
    1,671
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    191

    Default How to get best "mirror" machined flat finish on 6061 aluminum

    We're working on a new product that starts as a long block of 6" x 1" 6061 aluminum.

    The top of this block needs to be highly polished, after some pockets have been machined in it.

    On the prototype, with the tooling we currently have we're using a 3" diameter APKT insert based face mill to make a 0.012" skim cut on the block, but with about 70% overlap it takes 3 passes and we're seeing some transition lines on the part, along with some fine machining lines.

    We then go through a power sanding and then buffer wheel polishing procedure to get a pretty nice close to mirror finish, and this has been fine for the prototypes.

    But I need to speed the process up for the real products. To reduce the amount of sanding and polishing required, I need to improve the finish quality of the facing skim cut we're taking.

    Starting from scratch, what would be the best facing mill design and insert type to get the best possible finish on the facing cut we're taking?

    Its ok if its a very slow pass, it will still pay off in reducing the sanding/polishing step.

    Looking around a little it appears that a one or two insert based "fly cutting" type tool might be the best approach, is that true? (and if its that simple, I might just fabricate the tool)

    I've never used and don't know anything about "wiper" inserts, would a wiper insert help?

    Thanks,

    Paul T.

  2. #2
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,695
    Post Thanks / Like
    Likes (Given)
    453
    Likes (Received)
    261

    Default

    I've read that diamond inserts make a lovely finish on aluminum and other soft metals.

    There's never been enough money here for me to try it though.

  3. #3
    Join Date
    Jun 2006
    Location
    Huntsville Alabama
    Posts
    1,767
    Post Thanks / Like
    Likes (Given)
    1014
    Likes (Received)
    669

    Default

    Try the 3" Shear Hog facemill by A B Tools inc. I've been using them for about 2 years and they are The Ticket on AL.

  4. #4
    Join Date
    Dec 2007
    Location
    Southeastern US
    Posts
    6,080
    Post Thanks / Like
    Likes (Given)
    652
    Likes (Received)
    2404

    Default

    Get a PCD insert, the bigger the radius the better.

  5. #5
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    12,356
    Post Thanks / Like
    Likes (Given)
    1463
    Likes (Received)
    2556

    Default

    Make sure your inserts have an 'up sharp' edge, meaning no edge prep to get the best finish. One insert in the cutter is the cleanest but will slow down the feed possible. A wiper will allow a faster feed but won't help the ultimate finish. A cutter wider than the material like a flycutter will eliminate the marks left by multiple passes.

    We cut with Iscar E90AL face mills where possible with the APCR inserts for aluminum, they work about the same as Shearhogs. We feed fairly slow but not excessively so. Then we sand it with a DA orbital sander with 320 paper and buff.

    You need some serious power to buff it economically, that might be what is missing. If you have a 3/4 or 1 hp buffer you'll die of old age getting it polished. Pick up a 5 hp min. buffing machine, get some big wheels and the right compounds and it will only take minutes.

  6. #6
    Join Date
    Mar 2009
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8,398
    Post Thanks / Like
    Likes (Given)
    5772
    Likes (Received)
    10122

    Default

    You'll need a cutter the width of the part to get rid of overlap marks. Might be cheaper to make your own.

    I might do my finish pass on the block before cutting the pockets. The cutter may be happier with a less interrupted cut. Might not matter though, just something to consider.

  7. #7
    Join Date
    Jun 2001
    Location
    downhill from Twain\'s study outside Elmira, NY
    Posts
    10,745
    Post Thanks / Like
    Likes (Given)
    3883
    Likes (Received)
    3624

    Default

    What you really need is a good tight shaper. M42HSS bit with 5% cobalt. Sharpen like for finish cut on steel, or (alternately) with some side sheer and a largish nose radius. Stone the edge to a good polish. Any DOC you want. Fine step over. Use ATF for cutting fluid, run shaper as fast as it will go without rocking. You'll get an irridescent polished finish looking better than ground. Nice thing is shaper will run unattended except to load & unload parts.

    BTW, I've never tried it, but in a production environment it might be worth making a heavy stick holder to take APKT or similar high shear carbide insert, and experiment to take the "vagaries" out of who sharpens the bit.

    smt

  8. #8
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    16,370
    Post Thanks / Like
    Likes (Given)
    11943
    Likes (Received)
    11315

    Default

    ''The top of this block needs to be highly polished, after some pockets have been machined in it.''

    If it's got to be an optically good polished finish, polish it first then cover with masking tape and m/c,- thro' tape and all,..... IME mechanical polishing can/will round over thin sections, edges etc,....... which mightn't be what's wanted.

  9. #9
    Join Date
    Feb 2008
    Location
    Brisbane Australia
    Posts
    1,048
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    88

    Default

    Make yourself a single point flycutter with a PCD tip that spans the whole surface ( it will need to be well balanced). Spin it up real fast, and do 1 finish pass. You will be able to shave in the reflection.

  10. #10
    Join Date
    Mar 2002
    Location
    Brisbane, CA, USA
    Posts
    1,671
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    191

    Default

    Fellas, thanks a lot for all the responses.

    Based on your suggestions, here's what I'm thinking.

    Make an 8" diameter single point "fly cutter" style cutting tool out of a balanced length of 2" square 1018 steel (Stephen, this setup is the closest I'll be able to get to a shaper).

    Use a CCMT insert lathe tool on the end of the fabricated cutter. I chose CCMT because you can get PCD tipped CCMT inserts from these guys:

    http://amtektool.thomasnet.com/viewi...176?&forward=1

    If for some reason the PCD insert doesn't work out, I can use the extra sharp and polished CCMT inserts from Curtis at:

    http://www.latheinserts.com/category.sc?categoryId=46

    I'll use the largest radius I can get in that insert size, which is .031"

    I know the single point method will be slow, but that's ok, while we're facing one my shop guy can be sanding/polishing on another one.

    Does anybody see any flaws in this scheme or a better way to go?

    Mud, thanks for the comments on the buffer, what we've found so far is that once we sand it to the point where the machining lines are no longer visible it buffs up surprisingly fast, even on our (ok, you nailed it) 3/4HP buffer. If we try to start buffing while the machining lines are still visible, you either can still see them or if you buff hard enough to get rid the lines, you get some waviness from the buffing.

    So its the sanding operation that's taking most of the time right now, so I think if we can get the surface to a much smoother machined state, the sanding will go much faster.

    I'm surprised with how nice a polished surface we're getting now though even with the prototypes, 6061 really polishes up nice.

    Paul T.

  11. #11
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    5,105
    Post Thanks / Like
    Likes (Given)
    642
    Likes (Received)
    1013

    Default

    If you had enough work like that to amortize the cost of the tool, there is one new cutter out on the market that I've tried that is simply amazing for really fine finishes in aluminum.

    It's a Valenite V650 "V-Flash" cutter. The only inserts available for them are PCD and CBN, and they are intended to be a "finish" face mill. With the full-edge PCD inserts you could do some serious roughing too. Be prepared for high speeds and high feeds. The 3" six-insert cutter a friend of mine recently bought is the "coarse pitch" version and he's running full out at 10,000rpm and 300 ipm feed and getting a consistent 6 microinch finish. He's now wondering what kind of finish he'd get by adding a wiper insert (or two, for balance).

    If he had a 25,000 rpm spindle and the fine-pitch (9 insert) version, the cutter is rated for 28,000 rpm, but he'd have to feed it in rapid.

    .005" fpt x 9 x 28,000 rpm = 1260 ipm. That's the 32m/m rapid rate of his machine! He got a little discount from his distributor that he bought it from, but the list price was $968 for the cutter and $108 each for the inserts (.13 max d.o.c.) He said he made his money back for the cutter in less than 6 weeks over the 45 ipm he was running before to get a coarser finish. No more polishing required. Machines the parts and ships 'em.

    http://valenite.com/internet/4558/In.../vflashcat.pdf
    Last edited by PixMan; 09-08-2009 at 07:46 PM. Reason: link wasn't working

  12. #12
    Join Date
    Feb 2009
    Location
    Vancouver, B.C. Canada
    Posts
    1,816
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    94

    Default

    If you are doing a lot of these parts it may be worthwhile investigating a vibratory lap. Essentially a flate plate that oscillates in a random pattern, you place your part on it with some appropriate grinding/polishing media and it polishes it flat and shiny.

  13. #13
    Join Date
    Aug 2007
    Location
    Snowy Arizona
    Posts
    1,235
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    170

    Default

    Paul, I was recently informed about APKT inserts and their tolerance...or not so tight tolerances. Anyway, was using an in-the-machine (with polished APKT inserts) stock one for facing and had a pretty poor finish. I had Curtis Payne send me a 3" Ripper, same feed/speed and the finish probably improved from a 125 to a 32, although I didn't check it. HUGE improvement.

    I needed the 3" for another job so I call to get the big radius inserts that are cataloged at 0.355"R - well that's a misprint. The largest radius is 0.125"R, which was also fine for this job, but Curtis had told me of quite a few guys that needed the 1/8"R and he couldn't help them with the Ripper, now he can. There were actually quite a few catalog misprints on the insert radi - like 3 of 5 are wrong, give Curtis a call to strighten it out.

    Back to the facing, I think the finish cut was at 0.050" doc and 0.002"/tooth on the last job, I would guess the finish is in the 16 range with no mismatch between passes, only a better finish on the overlap area. The Ripper is a fine product, but it is not for those who want to spend 2X on the body and 50% more for inserts. Down side, no PCD inserts.

    Give Curtis a call.


    Steve

  14. #14
    Join Date
    Sep 2002
    Location
    Lawrenceville GA USA
    Posts
    5,978
    Post Thanks / Like
    Likes (Given)
    471
    Likes (Received)
    1133

    Default

    I have found that I get the best finishes when I have all my cuts go the same direction. That is I climb mill rather than go back and forth like most face milling routines. This may just be on my machine, I dont know if anyone else has the same experiance or not.

    Charles

  15. #15
    Join Date
    Mar 2009
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    8,398
    Post Thanks / Like
    Likes (Given)
    5772
    Likes (Received)
    10122

    Default

    Quote Originally Posted by CBlair View Post
    I have found that I get the best finishes when I have all my cuts go the same direction. That is I climb mill rather than go back and forth like most face milling routines. This may just be on my machine, I dont know if anyone else has the same experiance or not.

    Charles
    Yes, I always do that if I need multiple passes and a fine finish.

  16. #16
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,685
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    799

    Default

    Nachi brand works amazing. They are DLC coated and they actually recommend using it dry on Aluminum. APET160508PDFRSN-DLC100. I made the mistake by using it to rough and take deep depths of cut, nut the best and it wore out quickly. I dont think it has the edge strength. But for fine finishing it is amazing. High rpms and fine feed the chips are like Aluminum dust. Hard to take a good picture from the reflection, inserts are blue in color.



  17. #17
    Join Date
    Aug 2009
    Country
    UNITED STATES
    State/Province
    Nevada
    Posts
    1,699
    Post Thanks / Like
    Likes (Given)
    187
    Likes (Received)
    460

    Default

    Polished from milling I dont think this is possible. You can get a very nice finish from several cutters with high speed low feed. I havent ever heard of the above insert so maybe something has changed over the years. Polished means micron level ridges which you are not going to get milling.

  18. #18
    Join Date
    Mar 2002
    Location
    Brisbane, CA, USA
    Posts
    1,671
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    191

    Default

    Thanks again for all the helpful tips fellas.

    Frank, will those APET inserts you mentioned fit in an APKT face mill?

    Thanks,

    Paul T.

  19. #19
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,685
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    799

    Default

    Paul,
    As long as the other digits line up it should fit. 3rd digit is only a tolerance spec.

  20. #20
    Join Date
    Mar 2002
    Location
    Brisbane, CA, USA
    Posts
    1,671
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    191

    Default Tool tip radius limits?

    It looks to me that it would be best in this cut to use the largest tool tip radius possible, and the CCMT inserts I'm looking at now to use have a max radius of only .031"

    But looking around I ran across some round RCGT-AK inserts that are also highly sharp and polished for aluminum.

    They are available in diameters starting at .236" and going up from there.

    I've never used a round insert before, will they work ok for this light (0.010") kind of finish cut in 6061, or is this too big a radius to get a good cutting operation and finish?

    Thanks

    Paul T.


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
  •