Small taps in aluminum?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    698

    Default Small taps in aluminum?

    I need to tap a bunch of blind holes in 6061, 2 mm x 0.4 x about 10 deep. I've not done small stuff like this before. Should I use a floating holder or rigid tap? What speed would be a conservative starting point? Hoping not to break too many of these dinky taps. I usually tap very slowly (usually in SS), but there are about 800 holes to do here.

  2. #2
    Join Date
    Jun 2006
    Location
    Melbourne Australia
    Posts
    544
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    30

    Default

    I'd be inclined to form the threads on a machine with rigid tapping.
    I've had success forming M4 x 0.7 20mm deep in 304 stainless with these:
    https://www.walter-tools.com/SiteCol...ng-2009-en.pdf

    Good luck.

  3. #3
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,326
    Post Thanks / Like
    Likes (Given)
    973
    Likes (Received)
    4076

    Default

    Whatever you do a good quality aluminum will save a lot of nightmares, say no to Chinese crap.

  4. Likes Larry Dickman, Bobw, swarf_rat, DanASM liked this post
  5. #4
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,419
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    1009

    Default

    Done alot of M2x.4mm in 6061 Kaiser select precision rod. Form tap, held rigid in collet chuck. Push my old Haas to 2500 rpm tap speed and go. If it would handle rigid faster I would but I think its only rated for 2k. One tap is on aprox hole #9k

  6. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,204
    Post Thanks / Like
    Likes (Given)
    4783
    Likes (Received)
    3150

    Default

    Quote Originally Posted by swarf_rat View Post
    I need to tap a bunch of blind holes in 6061, 2 mm x 0.4 x about 10 deep. I've not done small stuff like this before. Should I use a floating holder or rigid tap? What speed would be a conservative starting point? Hoping not to break too many of these dinky taps. I usually tap very slowly (usually in SS), but there are about 800 holes to do here.
    What machine?
    I would tap as fast as your machine can tap accurately. Rigid tap.
    Of course on our Brother I would go 6k rpm, but on our Hyundai-Kia Fanuc 0 mill, I wouldn't even try it because the spindle can't stop and reverse fast enough, so about 300rpm max.
    Our Okuma mills I would go about 3k rpm or so.

  7. #6
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    698

    Default

    I am unfortunately familiar with foreign aluminum and always buy US sourced product. The machine is a DMC63V, not sure what speed it might be rated for. The positioning is accurate (glass scales) but how quickly it can start or stop I don't know.

  8. #7
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    172
    Likes (Received)
    881

    Default

    I don't get to carried away with tap RPM... 500 for prototype and 1000 for production. Prevents math errors and I think it is easier on the machine. On 800 holes I wouldn't get to excited about the potential improvement in cycle time to go up into the multiple of thousands.

    I have had difficulty with small threaded holes in aluminum. The threads looked fine and I didn't break many taps, but I have had issues getting them to pass QC. Whenever I get much below 2-56, I have a tendency to ream the holes after drilling. I consider the error in hole diameter and the subsequent impact to the other thread dimensions to be a percentage, rather than a straight numerical error. In other words, a couple thou error in diameter on a 1/4-20 is much less significant that the same diametrical (big word bonus points) error in a 0-80... unfortunately, my potential error in drill diameter seems to be about the same regardless of drill size.

    I think that some of the modern stub length carbide "engineered" drills can hold drastically better tolerance than the old HSS jobber drills, but it seems to take more fiddle fucking with drill sizes and cutting conditions than ordering reamers in a couple tenth increments and picking the one that gages out correctly. Especially considering the relatively low volume of holes you need to tap.

  9. Likes Chris59, hanermo liked this post
  10. #8
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,130
    Post Thanks / Like
    Likes (Given)
    662
    Likes (Received)
    484

    Default

    I never have done M2 but lots of M3 holes. I will second what G00 Proto said- start by making sure your hole diameters are what you think they should be before you start tapping. I gone wrong here before.

  11. #9
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    698

    Default

    I think I'll try a rigid holder and start at 500 rpm to see how it goes. The hole diameter thing is why I'm reluctant to use form taps for this or other short runs. There are numerous studies indicating that formed thread are great - provided you have exactly the right pilot hole diameter. Otherwise, they can be crap and still pass QC because of the formed shape. In long runs you can spend the time to get them just right. Cut threads on the other hand can have fairly large variations on pilot hole without big changes in strength.

  12. #10
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    982
    Post Thanks / Like
    Likes (Given)
    228
    Likes (Received)
    628

    Default

    On a Speedio I would run that rigid with a form tap at 6k RPM.

  13. #11
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    698

    Default

    Wonder if it actually gets to 6K? 10mm at 0.4 is only 25 revolutions. 1/4 of a second at 6K. It can come up to speed out of the hole, but must stop and reverse in the hole. What is the acceleration rate of that Speedio spindle?

  14. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,429
    Post Thanks / Like
    Likes (Given)
    225
    Likes (Received)
    1699

    Default

    Oh geez, don’t get us Speedio guys going, we’ll never shut up

    The spindle accel/ decel is PDQ. I would not be surprised if my S700 could hit 6,000 in this scenario, but I don’t really know.

    Regards.

    Mike

  15. Likes Mtndew, Pete Deal liked this post
  16. #13
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    848
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    495

    Default

    Quote Originally Posted by swarf_rat View Post
    Wonder if it actually gets to 6K? 10mm at 0.4 is only 25 revolutions. 1/4 of a second at 6K. It can come up to speed out of the hole, but must stop and reverse in the hole. What is the acceleration rate of that Speedio spindle?
    Speedio spindle takes less than .1 seconds to get to 6k. At 6k it's almost like a light switch. You can go from M3 to M4 at 6k and you might not see it reverse. Here is a video of Synchronized tapping on Brother:

    YouTube
    Last edited by BROTHERFRANK; 03-03-2020 at 03:15 PM.

  17. #14
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,031
    Post Thanks / Like
    Likes (Given)
    730
    Likes (Received)
    402

    Default

    I am curious - is there some accuracy “standard” a tapping process must conform to in order for it to be considered “rigid tapping”? I am knee-deep in a rigid vs non-rigid tapping situation at work so it’s on my mind. I am thinking something like, “spindle rotation must be within “x” degrees of theoretical position for a given linear position as a function of thread pitch.” or something. On that note, how “off” is a machine without rigid tapping? Like - what’s the difference in terms of real numbers?

  18. #15
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    4,457
    Post Thanks / Like
    Likes (Given)
    433
    Likes (Received)
    2709

    Default

    Form tap!

    the difference in speed on that machine between 1k and 2k rpm is small. 500 is just silly slow

    drill with a standard hole drill, measure actual hole size, tap, check with gauge and also check minor diameter

    thread can pass the gage but fail the minor. Even if you have get an odd size drill, it is worth it. The smaller and finer the fussier they are going to get.

    you should break zero taps and have that tap for years

    I think we get over 20k holes out of #6, maybe 50k I dunno

  19. #16
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,938
    Post Thanks / Like
    Likes (Given)
    2296
    Likes (Received)
    1550

    Default

    It depends how big/good your machine is. Robodrills will acc/dec faster than #40 taper machines.
    I would rolltap with bright finish tap (no coating) at S1500 and 10% concentration coolant

  20. #17
    Join Date
    Sep 2009
    Location
    barcelona, spain
    Posts
    2,458
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    1462

    Default

    I am very interested in the final result.
    Please post.

    Have no doubt the brother spindle, as a servo motor, can get to 6000 rpm in 0.1 secs, as posted previously.

    At 6000 rpm, 0.4 mm / rev, or 100 revs/sec, it would be ..
    .. 25 revs (10 mm deep) in 0.25 secs.

    If the brother spindle can reverse in 0.1 secs, this would be 10 revs or 4 mm in depth at 0.4 mm/rev from 6000 rpm.
    Very curious to know actual specs and actual results.

  21. #18
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    34
    Likes (Received)
    11

    Default

    Tapmatic, no spindle reversing.

  22. #19
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,632
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    698

    Default

    Quote Originally Posted by WRL View Post
    Tapmatic, no spindle reversing.
    But, a host of other problems.

  23. #20
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    34
    Likes (Received)
    11

    Default

    Quote Originally Posted by swarf_rat View Post
    But, a host of other problems.
    I’ve had good luck with them.


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
  •