M2 Form Tapping
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 45

Thread: M2 Form Tapping

  1. #1
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Post M2 Form Tapping

    Long time Forum reader, first time poster.

    Need help tapping M2 x .4, M2.5 x .45, and M3 x .5 holes in aluminum with 75% thread percentage. Taps snap with correct tap drill. Trying a drill the next size up drops the thread percentage causing ripped threads at assembly. Form taps and thread percentage is mandated by our customer. Torque specs for the assembly screws are mandated by our customer's customer.

    6061 T6511 aluminum
    2015 Haas VF-4SS. Tapping retract is set at 4, but we've tried both slower and faster
    Spotting with a 1/4" x 120° NC spot drill
    Using appropriate size solid carbide drills - 118° drill tip
    Formula for determining appropriate drill size for 75% metric threads: Tap O.D. - ( desired thread% x pitch ) / 147.06
    Example: (M2x.4) 2 - ( 75 x .4 ) / 147.06 = 1.796mm (.0707"), we're using a 1.8mm drill (.0709")
    Rigid tapping. We do not have any floating tap heads. We have tried multiple brands of taps. Emuge. Guhring. OSG. Union Butterfield. Balax. Probably another 5 or 6 brands that I can't remember. All coated for aluminum. TiN or similar. We have purchased new tapping collets. We have purchased an Emuge Softsynchro high performance tap holder.
    The coolant we use is a local brand I think, AFT (Advanced Fluid Technology) 619M2. The coolant concentration is nominal. I'm not a fan of the coolant, but there's no getting away from it. Coolant flow is great.
    We've tried Tap Magic for aluminum - comes in a red/white spray can and is supposed to be cinnamon scented. We've tried Moly-dee. And some other off-brand, thick as molasses, tapping compound.

    Maybe there's something simple that I just haven't thought of. Maybe there's something I just don't know about. Any help or advise would be appreciated, Thanks





    Thanks everyone! A lot of great stuff here!
    Last edited by cpreston; 10-10-2019 at 05:36 AM.

  2. #2
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    778
    Post Thanks / Like
    Likes (Given)
    59
    Likes (Received)
    294

    Default

    Are you measuring the hole your drill gives you?

    You can drill a bit under and ream to size. This also allows you to make up for tight/loose % engagement by tenths if needed.

    I would not use TiN coated taps, AFAIK TiN is kinda sticky when it comes to aluminum (not as bad as AlTiN but worse than shiny bright taps). I would think bright should be okay.

  3. Likes cpreston liked this post
  4. #3
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    177
    Likes (Received)
    1475

    Default

    Can you form tap larger, like M3 and M4, on this machine?
    Can you post a code snippet?

    Regards.

    Mike

  5. Likes cpreston liked this post
  6. #4
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,745
    Post Thanks / Like
    Likes (Given)
    1244
    Likes (Received)
    3561

    Default

    the balax chart says .072 drill size. Your a bit under that, probably why you're breaking taps. Use a .072 reamer

  7. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,583
    Post Thanks / Like
    Likes (Given)
    4191
    Likes (Received)
    2747

    Default

    Hole size is critical.
    Do you NEED 75% thread?
    As for form taps, which style are you getting? 1 vent flute? Multiple vent flutes? Myself I prefer OSG form taps, we form tap C110 copper quite often and the tap has done thousands of holes.
    Normally we buy Guhring taps, but for forming I think OSG has the upper hand.

  8. Likes SRT Mike, eaglemike, cpreston liked this post
  9. #6
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,176
    Post Thanks / Like
    Likes (Given)
    1676
    Likes (Received)
    1114

    Default

    You need bright finish uncoated roll taps.
    And 10% coolant.
    Clock drills and taps to ensure no runout.
    The threads are very fine - i would not run more than 500rpm.
    You need to do a test block with a grid of holes for test.

  10. Likes cpreston, gregormarwick liked this post
  11. #7
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    67

    Default

    Quote Originally Posted by dandrummerman21 View Post
    Are you measuring the hole your drill gives you?

    You can drill a bit under and ream to size. This also allows you to make up for tight/loose % engagement by tenths if needed.

    I would not use TiN coated taps, AFAIK TiN is kinda sticky when it comes to aluminum (not as bad as AlTiN but worse than shiny bright taps). I would think bright should be okay.
    Yes-yes... all of the above. Just 2nd-ing these suggestions. And 3rd-ing the fist suggestion that you must accurately measure hole size. Otherwise it's a crap shoot.

    Dave

  12. Likes cpreston liked this post
  13. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,429
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1621

    Default

    I like Balax for form taps, but we (fortunately!!!!) do not need to gage our holes as the work is our product. M2 = (approx) .08" so a bit larger than a 0-80 of which we do tons and tons of...

    I ran into this problem years ago, have you checked coolant for concentration, as well as fines? Fines could actually be coming thru your coolant line and adding swarf to the coolant at the tap drill (yes total PITA and hard to control)...

    As others mentioned, gage pre tap hole size as it is critical to form tapping, can also try different fits of taps, ie - H3-H2-H5.. whatever gets you to customer spec..

  14. Likes cpreston liked this post
  15. #9
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,455
    Post Thanks / Like
    Likes (Given)
    441
    Likes (Received)
    1746

    Default

    How deep?

    1.8 is the right hole size for 75% M2x.4

    I like to put my retract at .5 so the spindle isn't ramping up inside the hole...

  16. Likes barbter, eaglemike liked this post
  17. #10
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    Quote Originally Posted by Finegrain View Post
    Can you form tap larger, like M3 and M4, on this machine?
    Can you post a code snippet?

    Regards.

    Mike


    M2, M2.5, and M3 are the only 3 form taps we are struggling with for this customer. There are no other tapped hole sizes. We are new to form tapping. Mostly we cut tap or thread mill on parts for other customers. As the taps increase in size, the tap breakage is less often. So the breakage is likely related to the tap diameter.

    This is a package of parts that gets assembled by our customer. The parts come in many shapes and sizes. Some have may six M3 holes, some may have fifty eight M2 holes and eighteen M2.5 holes. These parts run in multiple locations throughout the shop. Additionally, most of the parts have M3 STI holes in them that we cut tap. We have form tap breakage throughout. So it is not just that individual mill that can't tap.

    Here is some of the code:

    T9 M06 ( M2.5 X .45 FORM TAP )
    G00 G90 G54 X-2.7523 Y1.4857 S300 M03
    G43 H09 Z0.1 M08
    G98 G84 Z-0.482 R-0.032 F5.315
    X-1.905 Y1.3999
    X-1.0373 Y1.4857
    X-0.175 Y1.3999
    X0.6902 Y1.4857
    X1.555 Y1.3999
    X2.4176 Y1.4857
    X3.124 Y1.2583
    X2.2789 Y-0.0001 Z-0.5214 R-0.0714
    X0.6902 Z-0.482 R-0.032
    X-0.175 Y0.5999 Z-0.5214 R-0.0714
    Y-0.6001
    X-1.0373 Y-0.0001 Z-0.482 R-0.032
    X-2.6289 Z-0.5214 R-0.0714
    X-2.9626 Z-0.482 R-0.032
    X0.6902 Y-1.486
    X1.555 Y-1.4001
    X2.4176 Y-1.486
    X3.124 Y-1.2586
    G80 M09

    T10 M06 ( M2 FORM TAP )
    G00 G90 G54 X2.0624 Y-1.0946 S300 M03
    G43 H10 Z0.1 M08
    G98 G84 Z-0.475 R-0.0714 F4.7244
    Y-0.1419
    Y0.1416
    Y0.1416
    Y-0.1419
    Y-1.0946
    G80 M09


    The speeds and feeds in this code are generic. The recommended RPM for a Balax M2 is S3555. We have tried anything in between S3555 and S300, thinking that might help. Not so much

  18. #11
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    .072 yields closer to 65% thread percentage. The customer demands 75% or they are tearing out threads at assembly

  19. #12
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,176
    Post Thanks / Like
    Likes (Given)
    1676
    Likes (Received)
    1114

    Default

    That's a good point about spindle ramp up - I always had an R plane of 5mm (0.2) for the mills and the lathes and then never had a problem.
    I just looked to see if I could find the make of taps we used as memory is fading, but nope.
    They were the out of round/lobe type with no oil groove though - Balax???
    Funnily enough, the ones we used to use happened to be one of the cheapest too - the taps with coatings just galled.


    Edit - I just checked an old file and for the M2, we'd drill 1.83mm dia.
    This would gauge correct (go/no-go) to British Standards, and also the core would gauge correctly too.
    BUT that was to British Standards, and you customer is asking for thread depth of 75%.
    I'm wondering if you'll be able to get this, because too small a hole leaves no-where for the material to "go".
    And on these small threads, 0.01mm increase/decrease on hole size makes a HUGE amount of difference...

  20. Likes cpreston liked this post
  21. #13
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    92
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    15

    Default

    F5.315 for a 0.45mm thread? How did you arrive at that figure? 0.45mm = .01772"

  22. Likes cpreston liked this post
  23. #14
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,745
    Post Thanks / Like
    Likes (Given)
    1244
    Likes (Received)
    3561

    Default

    just curious, why is your retract plane below the top of the part?

  24. Likes cpreston liked this post
  25. #15
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    Quote Originally Posted by Mtndew View Post
    Hole size is critical.
    Do you NEED 75% thread?
    As for form taps, which style are you getting? 1 vent flute? Multiple vent flutes? Myself I prefer OSG form taps, we form tap C110 copper quite often and the tap has done thousands of holes.
    Normally we buy Guhring taps, but for forming I think OSG has the upper hand.

    Hole size IS critical. We can manufacture these parts with a 65% thread percentage, but the torque specs on the screws will tear out threads at 65%

    Some have 1 vent flute, some have 2

  26. Likes Mtndew liked this post
  27. #16
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    I had not considered the fines! Thank you!

  28. #17
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    I actually thought that my retract HAD to be a whole number. I thought 1 was as slow as I could back out

    Most are not tapping more than .200, some are up to .350

  29. #18
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,176
    Post Thanks / Like
    Likes (Given)
    1676
    Likes (Received)
    1114

    Default

    Quote Originally Posted by cpreston View Post
    Hole size IS critical. We can manufacture these parts with a 65% thread percentage, but the torque specs on the screws will tear out threads at 65%

    Some have 1 vent flute, some have 2
    This leads to my point on post #12 then
    Are my calcs correct that a 65% thread is a 1.83mm drill size?
    Which is acceptable to British Standards (same effective tolerances as DIN too I believe) and what I used to produce quite regularly.
    So your customer maybe asking too much of a thread of that size too, by over-torqueing?

  30. #19
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    1

    Default

    Quote Originally Posted by dieselpilot View Post
    F5.315 for a 0.45mm thread? How did you arrive at that figure? 0.45mm = .01772"
    quick answer, the CAD spit it out

    Long answer, .45mm is the pitch - 1 thread. 1" divided by .01772 = 56.4446 threads per inch. S300 divided by 56.4446 = 5.31495

  31. #20
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    954
    Post Thanks / Like
    Likes (Given)
    1094
    Likes (Received)
    613

    Default

    Maybe I missed it, but when are the taps snapping? Do you have a little chamfer at the top of the hole for leadin? Have you validated the hole size after drilling?
    I agree with 1.8mm drill being correct for the M2x.4, bright taps(I like Balax), make sure it's not running out, run coolant at a minimum of 10% concentration. I keep my retracts at x4.


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
  •