Suggested Practice For Tight Tolerance Slot
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default Suggested Practice For Tight Tolerance Slot

    I have to machine a 5mm slot in aluminum with a tight tolerance. Position is critical, as is the width of the slot. I'm using a Bridgeport CNC knee mill. My procedure so far has been:
    • Center Drill two holes
    • Drill 11/64 two holes
    • Pocket Mill with3/16" carbide end mill, stepping down .05" on Z 2500 RPM and 3" min feed and do a finish pass.(Machine tops out at 3000RPM )


    I'm close, but not close enough. I'm getting enough cutter deflection that I'm having a tough time staying within the .0004" high tolerance limit. I'm using a solid collet and only have as much cutter sticking out as needed and have barely enough flute length to break through (15mm deep).

    Any suggestions as to procedure, speeds & feeds, number of cutting flutes, finish allowance and/or Z steps?



    Oh and did I mention I'm very limited for tool holders, I have 80 of them to do, they're all different and they're in a hurry?

    tolerance.jpg

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,665
    Post Thanks / Like
    Likes (Given)
    275
    Likes (Received)
    1887

    Default

    Use a smaller endmill. 3/16" is only .009" smaller than the slot size so it's going to "mash" into each end of the slot and make a mess. I'd use a stubby 1/8" instead, so the cutter has some room to work.

    Regards.

    Mike

  3. Likes mneuro liked this post
  4. #3
    Guest Guest

    Default

    I am assuming your CNC mill is the open loop stepper motor type, that will make it impossible to hold .0004 if that is what you mean. You will have to run them and sort, no way around that if I understand correctly. If this job is for an employer it should be outsourced if that CNC mill is all you have. If you are self employed and took that job I am afraid you made a big mistake.

  5. #4
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    986
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    411

    Default

    I would neck the endmill so there's only maybe .100" of flute. The rest behind it can just be a few thou smaller.

    The 2 reasons:

    1: the endmill might have a tenth or 2 of taper along the length of flute. it could even run out a tenth or 2 from the shank, and even your spindle.

    2: your endmill will flex less when you're at the top, because it doesn't have the flutes higher up rubbing on the wall. The deeper you go, the more that is rubbing the wall, the more deflection you go. Necking it down will reduce it

    Oh and yes, a smaller endmill might be better for you. Seems counterintuitive, but the smaller endmill will behave around the slot end radii better. Try 5/32.

  6. Likes AARONT liked this post
  7. #5
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,649
    Post Thanks / Like
    Likes (Given)
    16321
    Likes (Received)
    11742

    Default

    Take a spring pass, and if it doesn't true up, I'd swap out the endmill.

    Or, try taking a finish pass at each cut depth, and if its still tapered,
    change the endmill out.

    It doesn't take much to wear a small taper in an aluminum specific
    endmill. Did you happen to cut some steel with it recently? I bit
    myself in the ass last week because of that with a 3/16" endmill and
    a tight slot. I had used that endmill to take a little corner off
    a piece of 4140 a while back (I ran out of 4 fluters that were short).

    On the end of the slots, If it will land in tolerance, I wouldn't swing
    the radius. Square it up. Swinging that tiny radius, unless you've got
    a really smart control on that bridgeport, your feed rate around there is
    going to be huge. The cutter is swinging a .006 or so radius, with a .094
    cutter radius, so you're feed is actually about 47ipm around that radius.

    Make sure your ways are lubed up real good, a little bit of stick slip can
    completely screw you up. Make sure your backlash settings are dialed in.

  8. Likes 706jim liked this post
  9. #6
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    986
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    411

    Default

    Quote Originally Posted by Bobw View Post
    On the end of the slots, If it will land in tolerance, I wouldn't swing
    the radius. Square it up. Swinging that tiny radius, unless you've got
    a really smart control on that bridgeport, your feed rate around there is
    going to be huge. The cutter is swinging a .006 or so radius, with a .094
    cutter radius, so you're feed is actually about 47ipm around that radius.
    Do you have that formula for figuring that handy? I know I had it printed out, but can't find it now, and for some reason google isn't cooperating with the terms I'm using lol.

  10. #7
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    103

    Default

    Max out the rpm. 500 is way too slow. 500 is 25sfpm.

  11. #8
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    Quote Originally Posted by Finegrain View Post
    Use a smaller endmill. 3/16" is only .009" smaller than the slot size so it's going to "mash" into each end of the slot and make a mess.
    I thought about that, but it seemed like a long way to reach with an 1/8" end mill, plus I don't have a solid collet for an 1/8". I did just find a carbide 5/32 with a 3/16" shank that might work.

  12. #9
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    Quote Originally Posted by dandrummerman21 View Post
    I would neck the endmill so there's only maybe .100" of flute. The rest behind it can just be a few thou smaller.
    DOH! I forgot about trying relieving the cutter.

  13. #10
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    1286
    Likes (Received)
    804

    Default

    Quote Originally Posted by dandrummerman21 View Post
    I would neck the endmill so there's only maybe .100" of flute. The rest behind it can just be a few thou smaller.

    The 2 reasons:

    1: the endmill might have a tenth or 2 of taper along the length of flute. it could even run out a tenth or 2 from the shank, and even your spindle.

    2: your endmill will flex less when you're at the top, because it doesn't have the flutes higher up rubbing on the wall. The deeper you go, the more that is rubbing the wall, the more deflection you go. Necking it down will reduce it

    Oh and yes, a smaller endmill might be better for you. Seems counterintuitive, but the smaller endmill will behave around the slot end radii better. Try 5/32.
    This. Neck that endmill and go with a smaller cutter. All of that engagement is going to kill you.

  14. #11
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    Quote Originally Posted by Dualkit View Post
    If this job is for an employer it should be outsourced if that CNC mill is all you have.
    I told them that, but the decision was made by people who don't even know what the green button looks like. This is to fix something someone further up the food chain f'ed up

  15. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,665
    Post Thanks / Like
    Likes (Given)
    275
    Likes (Received)
    1887

    Default

    Quote Originally Posted by TwoWheeler View Post
    I thought about that, but it seemed like a long way to reach with an 1/8" end mill, plus I don't have a solid collet for an 1/8". I did just find a carbide 5/32 with a 3/16" shank that might work.
    Not meaning to be a PI, but are you sure you have the shoes for this job?

    Anyhoo, use a "Long Reach Stub Flute" endmill, 1/8" or 5/32".

    Regards.

    Mike

  16. #13
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    Quote Originally Posted by AARONT View Post
    This. Neck that endmill and go with a smaller cutter. All of that engagement is going to kill you.
    Yeah, I just found a 5/32 with a 3/16 shank that might work. Forgot about relieving the cutter. I was kind of mentally locked in to the 3/16" because I'm using it to plunge the round 5mm hole to get location (and then reaming to size).

    Part of the problem is that I only have about 5 tool holders (and *I* am the tool changer), so I need to work around that obstacle, too.

  17. #14
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    I brought more tools with me, when I came here than what they have. I just told them to order a few. My box is the tool crib.

    All I can do is do do the best I can with it and tell them take it or leave it. Silly academics just don't take "no" for an answer until you prove it.

  18. #15
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,499
    Post Thanks / Like
    Likes (Given)
    1857
    Likes (Received)
    1557

    Default

    I would be using a 3/16 endmill, edit the program to get a slower feedrate around the radiuses and coolant nozzle directed down into slot to clear out chips. Seeing as you have a BP likely your coolant isn't sufficient to blow the chips out of the slot, so maybe clear out the chips with an air gun for the final passes.

    I'd start programming it slightly undersize measure and then cutter comp or rewrite the program to bring it to finish size.

    And then I'd scratch my head as to how I'm going to measure the slot. That would probably require a walk down the street to borrow some Deltronic pins from a friend. I assume your measuring on the machine as you go.

  19. #16
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,649
    Post Thanks / Like
    Likes (Given)
    16321
    Likes (Received)
    11742

    Default

    Quote Originally Posted by dandrummerman21 View Post
    Do you have that formula for figuring that handy? I know I had it printed out, but can't find it now, and for some reason google isn't cooperating with the terms I'm using lol.
    Its just a ratio. .006R to .094R.. 15.6 ish to one.. 3ipm X 15.6 ish equals 47ish.

  20. Likes dandrummerman21 liked this post
  21. #17
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,776
    Post Thanks / Like
    Likes (Given)
    2318
    Likes (Received)
    1181

    Default

    Super sharp undersized cutter, lots of coolant, keep skimming until you get it.

  22. #18
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,209
    Post Thanks / Like
    Likes (Given)
    2463
    Likes (Received)
    3085

    Default

    I didn't see total thru cut? (total depth). We run 1/8em up to .625 and .75 deep (not in one cut, and not to .0004"), but an 1/8 is pretty stout if you can keep the flutes to bare minimum for the depth, alum material right?

    Also, go with uncoated, 3 flute. Uncoated because on a microscopic level a coating will 'round' off the sharp edges. And even though you are the tool changer, it might be worth it to set up 2 tools to rough and finish instead of beating your head against the wall for "one and done" approach...

  23. Likes Bobw liked this post
  24. #19
    Join Date
    Jan 2021
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    78
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    27

    Default

    Quote Originally Posted by Mike1974 View Post
    I didn't see total thru cut? (total depth). We run 1/8em up to .625 and .75 deep (not in one cut, and not to .0004"), but an 1/8 is pretty stout if you can keep the flutes to bare minimum for the depth, alum material right?
    I'm not concerned so much about breakage as I am flex, so the bigger, the better. I can go 5/32 or 11/64, too. Depth is .6, in aluminum.

    Quote Originally Posted by Mike1974 View Post
    Also, go with uncoated, 3 flute. Uncoated because on a microscopic level a coating will 'round' off the sharp edges. And even though you are the tool changer, it might be worth it to set up 2 tools to rough and finish instead of beating your head against the wall for "one and done" approach...
    I'm going to try relieving the shank, stepping down, maybe .05 steps and then doing a couple of free passes at full depth - this should allow the part of the cutter where the flutes are, to cut only the bottom...or that's my theory. If I use a flex collet, instead of a solid collet, the runout might work in my favor...if the runout is more pronounced at the tip than close to the shank. I have a piece of scrap I'm going to do a bunch of experiments on, we'll see.

    The problem with doing tool changes - besides it cutting into my web surfing - is that I have a whole -eight- tool holders to work with and about seven or eight operations on the same part. I have to balance needing holders for one thing, with needing them elsewhere.

  25. #20
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    986
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    411

    Default

    Quote Originally Posted by TwoWheeler View Post
    The problem with doing tool changes - besides it cutting into my web surfing - is that I have a whole -eight- tool holders to work with and about seven or eight operations on the same part. I have to balance needing holders for one thing, with needing them elsewhere.
    Buy some holders? Holders are cheap. What is it, R8?

    How much of a hurry can they be in, if it has been over a day and you haven't tried relieving the tool yet?


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
  •