Rigid Tapping - Breaking Taps on Tormach
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default Rigid Tapping - Breaking Taps on Tormach

    Hi Guys,

    New machine owner, need some help. I keep breaking taps on my Tormach. It has rigid tapping and i'm using an ER20 tap collet, standard ER collet.

    M2.5 X 0.45 Tap size.
    6061 Aluminum
    Fusion 360
    Tormach

    Do I need a dedicated tool? I thought I could just use a standard ER Collet holder if I had rigid tapping.
    Last edited by nyjiki; 01-20-2020 at 03:44 PM. Reason: Typo

  2. #2
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    150
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    31

    Default

    Post your code and maybe someone can help you. What taps are you using? What size is your hole before tapping? Bottom hole or thru hole. We need more details.

  3. #3
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks VTM,

    Through hole tap, my drill size is a #45 drill / 0.820" / using a YMW spiral bottoming tap. I can't even hit bottom of the part before the tap breaks. I'm using a ER tap collet with just an ER holder. My machine has rigid tapping.

    Here's my code:

    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
    G20 (Inch)
    G30

    N10(M2.5x.45 tap)
    T25 G43 H25 M6
    S250 M3 M8
    G54
    G0 X1.8 Y0.6705
    G0 Z0.38
    G0 Z0.28
    S250
    G98 G84 X1.8 Y0.6705 Z-0.65 R0.28 F4.4
    X1.998 Y0.4295
    X2.802
    X3. Y0.6705
    X3.198 Y0.4295
    X4.002
    X4.2 Y0.6705
    X4.398 Y0.4295
    X5.202
    X5.4 Y0.6705
    X5.598 Y0.4295
    G80
    G0 Z0.38
    M5 M9

  4. #4
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,062
    Post Thanks / Like
    Likes (Given)
    573
    Likes (Received)
    565

    Default

    Quote Originally Posted by nyjiki View Post
    Thanks VTM,

    Through hole tap, my drill size is a #45 drill / 0.820" / using a YMW spiral bottoming tap. I can't even hit bottom of the part before the tap breaks. I'm using a ER tap collet with just an ER holder. My machine has rigid tapping.

    Here's my code:

    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
    G20 (Inch)
    G30

    N10(M2.5x.45 tap)
    T25 G43 H25 M6
    S250 M3 M8
    G54
    G0 X1.8 Y0.6705
    G0 Z0.38
    G0 Z0.28
    S250
    G98 G84 X1.8 Y0.6705 Z-0.65 R0.28 F4.4
    X1.998 Y0.4295
    X2.802
    X3. Y0.6705
    X3.198 Y0.4295
    X4.002
    X4.2 Y0.6705
    X4.398 Y0.4295
    X5.202
    X5.4 Y0.6705
    X5.598 Y0.4295
    G80
    G0 Z0.38
    M5 M9

    Your original post said 4-40 tap but your program says 2.5 X .45, which is it? But, to your point, if it is 4-40, you are using a way undersize drill if you are using a .082" drill. My tap chart calls for .089 (#43) drill. 4-40's are hard enough, don't make it any harder.

  5. #5
    Join Date
    Mar 2013
    Location
    NW Pa
    Posts
    437
    Post Thanks / Like
    Likes (Given)
    62
    Likes (Received)
    191

    Default

    I didnt do the math but it looks like you programmed the wrong tap
    N10(M2.5x.45 tap)

  6. #6
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,334
    Post Thanks / Like
    Likes (Given)
    891
    Likes (Received)
    1333

    Default

    That’s awful deep for that size tap. I’d switch to a roll tap

  7. Likes TDegenhart liked this post
  8. #7
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,062
    Post Thanks / Like
    Likes (Given)
    573
    Likes (Received)
    565

    Default

    In addition to using the wrong drill, your feed is wrong. If you are going to use 250RPM, then your feed should be F6.25. 250RPM X .025 pitch=6.25 feedrate.

    Is the program you posted the actual program you are using? Because it is programmed for a 2.5MM X .45.

    Paul

  9. #8
    Join Date
    Jul 2010
    Location
    corvallis,or
    Posts
    878
    Post Thanks / Like
    Likes (Given)
    90
    Likes (Received)
    370

    Default

    Haven't looked at your code but why are you using a bottoming tap on a through hole? Spiral point gun tap will reduce cutting forces. Also might want to consider form tapping it.

    Teryk

    Sent from my XT1710-02 using Tapatalk

  10. Likes TDegenhart liked this post
  11. #9
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Sorry meant M2.5X0.45 tap

  12. #10
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    I was thinking roll forming it as well. The bottoming tap was what we had, didn't think about the cutting forces. Thanks for the input

  13. #11
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Yes, I wrote the wrong Tap, thanks for the input.

  14. #12
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks for the input, how fast would you go?

  15. #13
    Join Date
    Jul 2002
    Location
    Phoenix, AZ USA
    Posts
    1,742
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    217

    Default

    I don't know on your Tormach, but most of the time when you are rigid tapping your federate is the pitch, not the pitch times rpm.

  16. #14
    Join Date
    Sep 2006
    Location
    SW Wisconsin
    Posts
    587
    Post Thanks / Like
    Likes (Given)
    59
    Likes (Received)
    161

    Default

    Are you using Path Pilot? If you are and it still follows Linuxcnc then G33.1 is for rigid tapping.

    G33.1K(pitch)Z(depth)

    Ed.

  17. #15
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    3,784
    Post Thanks / Like
    Likes (Given)
    825
    Likes (Received)
    2613

    Default

    On my VMC's I always use IPM. On the lathe, it's IPR.

    Either one is fine, you just better know which one you are using...

    @OP- get your speeds and feeds better- for 250rpm you should feed at 4.43 rather than 4.4. You can round away the third decimal place, but not the second. 250 is way too slow anyway,

    I'd run that tap no less than 1500 rpm, which would work out to 26.574 IPM feed.

    It's a small tap, and spiral flute taps are more fragile than SP/Plugs. If you machine has peck tapping, take it in 2 or 3 pecks.

  18. Likes Booze Daily, nyjiki liked this post
  19. #16
    Join Date
    Feb 2005
    Location
    Akron, OH
    Posts
    1,913
    Post Thanks / Like
    Likes (Given)
    305
    Likes (Received)
    1447

    Default

    I'd be shocked if your tap even had .65" of flutes. The deepest M2.5 tap on McMaster only goes 1/2" and Balax doesn't have anything deeper in that size either. If you run out of flute, you snap immediately, even if everything else is perfect.

  20. #17
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Used a reduced neck tap, I can clear the depth but I think I took too much depth for an ER Collet holder. Thanks

  21. #18
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    I can't peck, i've been looking for someone using a "Q" value in their G84 for their path pilot and I can't find it.

  22. #19
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Yes! Only issue is that I can't find a "Q" value for a standard G84 code that would help me take this depth. I think i'm breaking taps because i'm taking a single pass the tap

  23. #20
    Join Date
    Feb 2005
    Location
    Akron, OH
    Posts
    1,913
    Post Thanks / Like
    Likes (Given)
    305
    Likes (Received)
    1447

    Default

    Quote Originally Posted by nyjiki View Post
    Used a reduced neck tap, I can clear the depth but I think I took too much depth for an ER Collet holder. Thanks

    Which is great, but a spiral flute tap pulls the chips up behind the cut, so once you run out of flutes, they pack up and snap.

    Or keep faffing about looking at your collets. Your choice.


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
  •