Help with tapping a 0-80 UNF in 6061-t6 Aluminum on a Haas VF2
Close
Login to Your Account
Results 1 to 5 of 5
  1. #1
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Help with tapping a 0-80 UNF in 6061-t6 Aluminum on a Haas VF2

    So I have roughly 5000 holes to tap on small parts made out of 6061-T6. My callout is a 0-80 UNF tap .224 down in a blind hole thats .287 deep. What I have gathered so far is the following:

    -Use a # 54 Carbide Circuit Board drill (not sure why) @ 6000 RMM & 10 IPM
    -Use a roll form tap @ 1200 RPM with normal coolant

    Is this info good? also, can I expect 1 tap to get thru all 5000 pcs? Thanks for the help guys!

  2. #2
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    826
    Post Thanks / Like
    Likes (Given)
    1048
    Likes (Received)
    548

    Default

    I'd suggest the 229 series drills from MA Ford. They are made for performance in aluminum. What ever the maximum rpm of your machine, and use the feed per rev they suggest. The are carbide, 3 flute, and work very very well.
    Agree for the form tap. I don't know which VF-2 you have. It might make a difference, as in how much distance to allow for accel/decel/reverse. If you machine can hold tolerance, I'd suggest 1500 rpm. That's what I was using without issue on an older VF-2, as well as some newer machines (through 2012). Your speed will be limited by the machines' ability. If the machine is capable, you could run 6K - but I'm pretty sure the VF-2 can't do that. If you have spare taps and material, try tapping at 2K, 2.5K, etc. Use a bright finish tap, or check with a tap mfr and make sure you are using the correct coating for aluminum. The wrong coating will ruin your day.
    Might need to have your R plane higher above the part than the drill cycle, again depending on machine performance.
    Suggest rigid tapping if you machine is in good shape, don't use a spring loaded tool.
    Double check to be sure feed per revolution is correct, DAMHIK.
    Good luck!

  3. #3
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,969
    Post Thanks / Like
    Likes (Given)
    4526
    Likes (Received)
    2994

    Default

    That tap should last a lot longer than 5k holes. But we all now how things work in this line of work lol.
    If you're not familiar with form taps, the drilled hole size is crucial.

  4. Likes Larry Dickman liked this post
  5. #4
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,314
    Post Thanks / Like
    Likes (Given)
    209
    Likes (Received)
    1629

    Default

    0-80 form tap gets a .055" hole, so I would be drilling a lot faster than 6,000 RPM. Yes, I would use a carbide drill. I like MA Ford "Twister Drill". This is currently what I get when I order "Quick-Change Carbide Drill Bits" from McMaster-Carr, and they have worked a treat for me.

    Make sure you get and use a teeny tiny spotting drill -- normal-sized spotting drills have a web that is likely wider than .055", so you wont get a localizing cone.

    Make sure your drilled hole stays very close to .055". Just a little bit over that and your minor diameter will be too big. Hole size too small, minor diameter will be too small, and you're much more likely to break the tap.

    For the tapping, I would again go a lot faster -- 80 TPI takes quite a while at only 1,200 RPM.

    Regards.

    Mike

  6. #5
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    808
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    281

    Default

    Keo center drills work better than spot drills and last a 100 times longer. I run them in #0 and #1 size for small holes. both 45 and 30 degree.


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
  •