Form tapping M12 in 4140PH?
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 42
  1. #1
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    242
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    126

    Default Form tapping M12 in 4140PH?

    Before I do something super dumb: I need to tap M12x1.75 through a 40mm thick 4140PH ground plate on a 16K Speedio. Haven't worked much with 4140, and the part has a fair bit of time into it, so I'd appreciate a quick sanity check.

    My plan is to spot, drill to 11.2 mm with a carbide CTS drill, and then form tap. OSG ADO drill and XPF form tap in ER25 holders.

    Am I going to regret it? Or am I going to run out of spindle torque and just stall out? Should I just plan on thread milling this instead? Thanks in advance!

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,721
    Post Thanks / Like
    Likes (Given)
    291
    Likes (Received)
    1982

    Default

    Threadmill it for sure, IMO. Maybe your Speedio can form tap it, but why risk it?

    Regards.

    Mike

  3. Likes trochoidalpath, barbter liked this post
  4. #3
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    595
    Post Thanks / Like
    Likes (Given)
    253
    Likes (Received)
    460

    Default

    You may live to regret it, but I sure as hell want to see it happen.
    Personally, I have never form tapped anything except aluminum.

  5. Likes trochoidalpath, metalmadness liked this post
  6. #4
    Join Date
    Dec 2013
    Location
    India
    Posts
    224
    Post Thanks / Like
    Likes (Given)
    135
    Likes (Received)
    22

    Default

    Wouldn't go with it.
    Hardness will be close to 30 HRC in 4140PH, almost upper limit to what a general form tap can.

    Threadmill. Or SPPT tap.

    And you better use tap collet or synchronised tap chuck instead of plain Jane ER25...

  7. #5
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    454
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    143

    Default

    I have to agree that it could be asking for trouble. I form tap 1/2"-13 in soft 1045 on a small lathe, and it requires a lot of torque- pretty much all my machine has got.

    If you do decide to give it a go, do some tests starting with a larger pre-drill than you think you need. That will require significantly less torque than the proper drill size. Watch the tapping torque and see if you feel comfortable going with a smaller pre-drill.

  8. #6
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,811
    Post Thanks / Like
    Likes (Given)
    1785
    Likes (Received)
    2371

    Default

    I form tap harder materials all the time. 17-4 mainly, up to H900 (low 40's Rc).

    I have one part in 36CrNiMo4 QT (4340/EN24) that I form tap M8, made about a thousand of those in the last year or so, never an issue.

    Can't think of anything explicitly 4140HT that I form tap, but I can't see it being an issue from the tap's perspective.

    Whether or not your machine can manage it, I don't know. I form tap up to M16 regularly, but I have bigger machines.

  9. Likes Vishrut liked this post
  10. #7
    Join Date
    Jan 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    242
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    126

    Default

    Thanks for your feedback everyone.

    I’ll try to find a thread mill with enough reach — that might be tricky. If I can’t find a reasonable one, I’ll probably try it with a spiral point cut tap.

  11. #8
    Join Date
    Jan 2021
    Country
    FINLAND
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Why not test it on another test article first? 10K spindle will tap M16 holes to structural steel, but probably not in 4140. You might possibly have to run it at higher RPM than suggested by calculators to obtain more torque from the motor. I have slapped regular tapping paste for M16 just to make sure the lubricity is there. Maybe you could drive small start with the machine and hand tap to finish, just something my cheap ass would do before investing in new tools..

  12. #9
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    344
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    153

    Default

    Would peck tapping not be a viable option ?. I only ask because I haven't tried it yet on my 10k S500. 1/2-13 in 1018 through 1/2" plate is as much as I've needed so far.

  13. #10
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,700
    Post Thanks / Like
    Likes (Given)
    14153
    Likes (Received)
    5767

    Default

    Dunno if it helps, or if the tooling budget for this project is there.... But Carmex has this indexable that'll do what you want, for $300

    http://www.carmexusa.com/default.asp...t=28&parent=19

    Then you'd need the proper insert(s) as well...

  14. #11
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,700
    Post Thanks / Like
    Likes (Given)
    14153
    Likes (Received)
    5767

    Default

    Carmex Part Number MT 0808 C28 1.75 ISO has a usable length of 28.9mm... So if you're comfortable relieving the shank by another 11mm on your own, that'd work, and probably be cheaper. They make some thread mills with the LOC you need, but only in 1.5 or 2mm pitch, not sure how the 1.75 got skipped.

    That's the best I could find for you right now, I'll have a look at some other catalogs later.

  15. #12
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,721
    Post Thanks / Like
    Likes (Given)
    291
    Likes (Received)
    1982

    Default

    SCT PN SPTM372XLA, 1.75" thread depth: https://sct-usa.com/wp-content/uploa...sptmmetric.pdf

    Regards.

    Mike

  16. #13
    Join Date
    Mar 2007
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    554
    Post Thanks / Like
    Likes (Given)
    386
    Likes (Received)
    258

    Default

    I feel that as a general consensus we could all agree that when in doubt thread mill if your having second thoughts. These type of posts pop up quite often sometime size related or difficult material issues. Sure threadmilling takes more time but is very predictable once you’ve dialed in your settings. Look at the tourqe values it takes to drive a large tap vs the tourqe curve of your spindle, the machine may be able to do it, but do you really want to subject your precision spindle to those forces?

  17. Likes Pete Deal liked this post
  18. #14
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,309
    Post Thanks / Like
    Likes (Given)
    3189
    Likes (Received)
    1677

    Default

    Quote Originally Posted by Houndogforever View Post
    You may live to regret it, but I sure as hell want to see it happen.
    Personally, I have never form tapped anything except aluminum.
    I've done 303SS. Several hundred parts and the first tap is still good as new.

  19. #15
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    130
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    27

    Default

    What forces? Tapping has no force other than torque, surely you've experienced this by hand. Roughing or facing is much tougher on a spindle.

    Finding a decent tapping torque calculator was online was tough. Walter has what seems like a good one. Walter Machining Calculator It looked like in P8 it's 33Nm for M12 and the Speedio has 40Nm? OSG The OSG catalog estimates the same in 35HRc.

    I'm just an amateur, but when I had a tiny machine I figured out I had to calculate Tq and HP for all bigger cuts and drills, never stalled the spindle again.

  20. #16
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,905
    Post Thanks / Like
    Likes (Given)
    8219
    Likes (Received)
    9899

    Default

    Quote Originally Posted by gregormarwick View Post
    I form tap harder materials all the time. 17-4 mainly, up to H900 (low 40's Rc).

    I have one part in 36CrNiMo4 QT (4340/EN24) that I form tap M8, made about a thousand of those in the last year or so, never an issue.

    Can't think of anything explicitly 4140HT that I form tap, but I can't see it being an issue from the tap's perspective.

    Whether or not your machine can manage it, I don't know. I form tap up to M16 regularly, but I have bigger machines.

    A Brother can doo anything that your bigger machines can, and faster!
    (sounds like an Arctic Cat rider talking)


    --------------------

    Think Snow Eh!
    Ox

  21. Likes TeachMePlease liked this post
  22. #17
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,721
    Post Thanks / Like
    Likes (Given)
    291
    Likes (Received)
    1982

    Default

    Quote Originally Posted by dieselpilot View Post
    Finding a decent tapping torque calculator was online was tough. Walter has what seems like a good one. Walter Machining Calculator It looked like in P8 it's 33Nm for M12 and the Speedio has 40Nm? OSG The OSG catalog estimates the same in 35HRc.
    16,000 RPM spindle is only good for 27 Nm instantaneous (my 2016 S700X1 anyway), so maybe it makes it, maybe it doesn't.

    Regards.

    Mike

  23. #18
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,700
    Post Thanks / Like
    Likes (Given)
    14153
    Likes (Received)
    5767

    Default

    Quote Originally Posted by Finegrain View Post
    16,000 RPM spindle is only good for 27 Nm instantaneous (my 2016 S700X1 anyway), so maybe it makes it, maybe it doesn't.

    Regards.

    Mike


  24. Likes Mtndew liked this post
  25. #19
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,520
    Post Thanks / Like
    Likes (Given)
    955
    Likes (Received)
    679

    Default

    You didn't say how many holes or how many parts. I assume just one plate?

    If just one plate I would absolutely not form tap it. I had a job recently, 300 little 303 stainless bullet nose things (lathe work) with a 10-32 hole. I read a bunch of these posts and figured sure form tapping works fine on 303. Bought the tap, first part, tap broke. Switched do a spiral point tap and did the whole bunch no problems. Probably if this was a job that was worth a the process development time and money it would be worth it but for one part I would go with thread milling. Or if just a few holes I think I would just tap them with a cut tap in a little and finish them by hand. But I think a single cutter thread mill ought to work.

  26. #20
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,905
    Post Thanks / Like
    Likes (Given)
    8219
    Likes (Received)
    9899

    Default

    Pete - you did drill the hole bigger than normal eh?

    You shouldn't have had that experience under normal conditions.

    ???


    This isn't exactly the right thread to post this, but since we are kind'a there anyway....

    I had some 304 parts to tap the other day, and I have never found 304 to tap in a coolant machine with a cut tap and not break it.
    I found a used OSG form tap and went to work. (only had 18 holes)
    The tap broke straight away, and I didn't think that I had anymore taps like that in stock, but in a different app drawer I found a box of form taps this size from Jarvis.
    I used to buy many form taps from them 20 yrs ago, but I don't feel that forms are the best option most times, so I have gravitated more towards Mod Bottom SP FL taps from OSG or Morse, or similar.

    But anyway - there was a whole box of the right sized taps from Jarvis here, so I tossed one in, with hesitation....

    I got WAY better results with that (also used) TiN coated Jarvis tap than I would have gotten with a brand new TiALN (?) coated OSG!

    I had noticed on other similar jobs where I am tapping 304 (these are normally just short runs of weld-on lugs) that even a brand new (OSG) tap produces a very warm part, and even steam will come out of the spindle bore when I re-chuck parts. The Jarvis parts all came off cool.

    These results with proper hole size, not overboring like y'all like to doo.


    ------------------------

    Think Snow Eh!
    Ox


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
  •