deep pockets 7050 aluminum thin walls pushing out with finishing
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,655
    Post Thanks / Like
    Likes (Given)
    2625
    Likes (Received)
    630

    Default deep pockets 7050 aluminum thin walls pushing out with finishing

    I am programming a aerospace part in aluminum 7050. Okuma mu6300. Part is held in dovetail and is tabbed to finish. This pocket is 2. x 6. x 2.0 deep. One wall is .06 thick and is pushing out when finishing. I cannot get it to size without going negative stock to leave. I have tried roughing and finishing in 2 steps roughing in 1 step, leaving wall at .140 and finishing in steps. Both ways wall is not flat and is over and on size in different places. I have tried a mix of 3/4 sharp 4flt and 1/2 Em .125r. Anyone have any tips for these kinds of walls. For example EM diameter, flute count, corner radius size, amount for finish pass etc.

    Thanks,

    steve austin

  2. #2
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    317
    Post Thanks / Like
    Likes (Given)
    78
    Likes (Received)
    104

    Default

    I am far from an expert but I have gotten out of similar situations by taking a very heavy finish cut and by playing around with conventional vs climb milling. Is if possible to make a "hoop" to support the outside and climb mill it (should help push the thin wall into the temporary support)?

  3. #3
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,280
    Post Thanks / Like
    Likes (Given)
    361
    Likes (Received)
    585

    Default

    Take a look at something like this: Machining Thin Walls and Floors

  4. #4
    Join Date
    Nov 2010
    Location
    Tustin, CA
    Posts
    383
    Post Thanks / Like
    Likes (Given)
    226
    Likes (Received)
    114

    Default

    Possible to machine the pocket first and then the outside? Or could make a plug to go in before you finish the outside.

  5. Likes Mtndew liked this post
  6. #5
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    595
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    199

    Default

    foam on the inside work really well, but I am guessing your running production and dont want the add'd start and spot time.
    if thats the case rough both outside an inside leaving maybe .1-.150 stock then when you do finish pass's step down about .250 alternating between inside and outside and make it so one side finishes deeper then the other side to help hold rigidity.
    I use 3 flute alumastars for deep pockets. I am assuming your tolorance is either + or - .003 or .005
    On longer lengths in either x or y you maybe have to run some taper in the program as we have had the center sucking in about .002
    also once you get deeper you will have to reduces the rpm by about 1/2 to keep the chatter away and a nice finish


    Hope that made sense.
    for example
    outside 1st fin pass at z-.125 deep
    then go to inside 1st fin pass z-.250 deep
    then go to outside 2nd finish pass z-.350
    then go to inside 2nd finish z-.500
    etc etc

    the other thing that helps with this is if you use a tool with a shorter flute length. and let the dia of the endmill above the flutes rub on the part. that actually helps stabilize the part.get a standard length 1/2" endmill and stick it out the total depth of your part. I assume your also tumbling them , if so you wont see any rub marks. if not then scotch bright is required. we tumble all out parts and never have a problem doing it this way.

  7. #6
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,029
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    945

    Default

    Quote Originally Posted by Delw View Post
    foam on the inside work really well...
    I was going to say I've filled the adjacent area with wax, if there is one ...

  8. #7
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,003
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    412

    Default

    What a stupid design of such an aluminium pocket! Certainly a wax fill is the way to go.

  9. #8
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,816
    Post Thanks / Like
    Likes (Given)
    1266
    Likes (Received)
    3651

    Default

    we used to use reverse spiral end mills for that. (ie right hand cut, left hand spiral) Without seeing the part its hard to guess, but clay or wax on the outside could help.

  10. #9
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,003
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    2070

    Default

    .06 2 inches deep, if you cannot support the outside........what tolerances are you dealing with?

    Is it the 6 inch long wall?

  11. #10
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    353
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    107

    Default

    I'd try ramping the finish passes on those walls instead of stepping it down.

  12. #11
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    I'm sort of surprised no one has said this (maybe i missed it?) but we do parts like this quite frequently.

    Get rid of those big tools. way to much tool pressure.

    I use SGS reduced neck tools but any brand should do, try a .375 or .250 cutter. The one I have in the machine right now is .250D , .250LOC 4" OAL, I think it has a .030r.

    In an SK holder or Hydro I run it balls out 15k on the genos, 45ipm .025-.1 DOC.

    YMMV

  13. Likes aarongough liked this post
  14. #12
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    213
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    34

    Default

    a huge problem I have run into in the past is 7050 moves all over the place ( reliving itself) and is very hard to get consistancy. I had 1 that was a housing 20x 30 " x 4 with .04 walls 4 inches deep ,so all the way through. I did the outside profile first. then built a 1 inch thick box that slid over the outside. then machined the inside. it had .13 radius in all corners. it had 2 chambers. I cut the small 1 out first. then made a block that slid into that. then I was able to finish the big chamber without the center wall blowing or collapsing.

  15. #13
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,379
    Post Thanks / Like
    Likes (Given)
    3167
    Likes (Received)
    2436

    Default

    Rough the part outside and inside tapered like a cone. Then finish in steps outside / in side with a 3/8 or 1/2 tool. I'd make sure I was taking a spring pass at each level as I went down. If your runnout isn't perfect and you leave some steps get a lower helix tool (35-37*) aluminum tool with 2" of flute and take a spring pass at the bottom level to clean up the wall. We do tons of parts with 1/8" thick tabs stick off the side of parts like you are talking about that are 2" from the base with this method. Have to hold +/-.002 on the tab thickness

  16. Likes CNC Hacker 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
  •