Milling 7/8-6 Double lead Acme Thread.
Close
Login to Your Account
Results 1 to 18 of 18
  1. #1
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default Milling 7/8-6 Double lead Acme Thread.

    Hello,
    I am looking for some advice on milling an internal 7/8-6 double lead Acme thread. I am working in a 5axis C42 Hermle and using CAM Software. I purchased a single point 6tpi threadmill and can not get it to create a good thread form (seems to be back cutting). The threads I am getting are washed out (coming to a point rather than a flat), though my GO Gage fits it is so washed out that my NOGO Gage fits as well. I am programming two separate 3tpi tool-paths the second's starting angle is 180 degrees from the first. I milled the minor right on the number and the major is right on as well. I suspect I need a special theadmill but not really sure.
    Any advice is appreciated.
    Attached Thumbnails Attached Thumbnails washed-out-threads-test-thread-gage.jpg   washed-out-threads-test.jpg  

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    609
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    166

    Default

    Dont you need a 3tpi threadmill? Or a single row.

  3. Likes Dwolf55793 liked this post
  4. #3
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,480
    Post Thanks / Like
    Likes (Given)
    2238
    Likes (Received)
    1018

    Default

    Your threadmill is not relieved enough on the backside to cut a 3 tpi thread.

  5. Likes Dwolf55793 liked this post
  6. #4
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    I think I need a 3Tpi threadmill but acme tip width changes when you switch your tpi. So it would have a wider tip width, and I really can not find a 3tpi Acme threadmill. Not sure about the single row though wanted some confirmation before throwing money at it.

  7. #5
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    2,059
    Post Thanks / Like
    Likes (Given)
    1302
    Likes (Received)
    2214

    Default

    You’re going to need more clearance. Just hand grind some on your tool.
    I’d say leading edge, but maybe I’m not visualizing it right.

  8. Likes Dwolf55793, doug925 liked this post
  9. #6
    Join Date
    Sep 2002
    Location
    Riddells Creek,Victoria,Australia
    Posts
    553
    Post Thanks / Like
    Likes (Given)
    143
    Likes (Received)
    100

    Default

    There are some strange answers here. The point is that you can not cut a 2 start thread with a threadmill designed for single start threads, the helix angle is only half so naturally it will not cut properly.

  10. Likes Dwolf55793 liked this post
  11. #7
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,846
    Post Thanks / Like
    Likes (Given)
    4026
    Likes (Received)
    2081

    Default

    You can't threadmill a high lead acme thread, period. The path of the tooth obliterates the flank angle. You can only threadmill when the pitch angle is less than the flank angle.

  12. Likes Dwolf55793, TeachMePlease liked this post
  13. #8
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    3,550
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3729

    Default

    Hi Dwolf55793:
    There are a couple of important things you need to be aware of:

    First; the threadmill is like a saw, and a multi tooth threadmill is like a gang saw.
    There is no helix...it is just a saw with 14 1/2 degree faces.
    Changing the relief angle does nothing...it's still just a saw.
    There is no "helix angle" on the threadmill...each tooth around the periphery of the mill spins on a common plane, unlike a tap.

    The thread form follows a helical path, so there is an angle relative to the axis of the thread at which the saw fits best.
    For external threads, if you tilt the saw into the plane of the helix, you can cut a threadform that is the same as the profile of the saw teeth unless the face angles of the teeth approach zero (square threads).
    Square threads don't work because the helix of the thread is not a plane, but the saw teeth spin in a plane, so they'll clip the corners on the entry and exit sides of the cut.

    Because the thread profile also follows a helical path (non planar) for internal threads, the saw will interfere with the threadform as one or more of three conditions appear:
    1) the saw diameter approaches the thread minor diameter.
    2) the flank angle of the thread profile is reduced.
    3) the helix angle (thread pitch) increases.

    Conventional threadmills can be made to work on 3 axis VMC's because the threadmill is substantially smaller than the minor diameter, the flank angle is 30 degrees so it clears the thread flanks more (for a 60 degree vee thread) and the pitch is reasonably shallow for single start threads.

    All of these things are working against you for your double start ACME thread.
    So you have to fake it and accept what you get:

    First, you have a 5 axis setup, so you can tilt the cutter into the helix angle and rotate the part around the tilted cutter.
    Second, you can choose a cutter that's as small a diameter as you can...this means it will clip the profile less at the entry and exit zones of the cut.

    Be aware, as soon as you tilt the cutter into the helix angle, you are restricted in how deep you can internal thread...if you go too deep, you'll bang the shank of the cutter into the opening of the hole.
    This gets worse (obviously) as the helix angle increases, so with a double start thread, you cannot thread very deep.

    That's why it's not working for you.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

    On edit: mhajicek: you beat me to it...you're exactly correct, but you can mitigate it a bit using the bodge I described above.

    MC

  14. Likes mhajicek, LexD, Dwolf55793, doug925, wheels17 liked this post
  15. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,923
    Post Thanks / Like
    Likes (Given)
    17325
    Likes (Received)
    12189

    Default

    You can't do it. It is physically impossible in a 3 axis machine.

    You could have saved yourself a whole lot of money and just bought a tiny
    little key cutter, and you would have gotten the EXACT same results.

    I looked into it years ago. I don't remember if it was a 1-4 or a 1-5. ......
    Just went and looked, 1-5..

    So I drew it up.. Using the commercially available "Thread mill" that said it could
    do it.. It CAN'T.



    Notice how the flat blows out the entire thread form.. No need for any angles
    on the tool. Its acting as basically a key cutter..

    Increase the pitch and decrease the diameter, and its just going to get WORSE, and
    you'll get a result, just like you got.

    Even on a 60 degree standard thread that is thread milled everyday, you aren't getting
    a perfect thread form.. It may fall in tolerance, but its not "perfect".. Functional,
    in tolerance, everybody is happy, but still not "perfect" on the thread form. Close,
    but not as good as turning.

    I also modeled this up doing an external thread. That may be possible with messing with
    the geometry of the cutter. Internal, impossible.



    There is a reason that mass produced acme nuts are so expensive.. Its because they are
    a huge giant F'n pain in the ass.

    Edit: I think its neat to see the actual end results.... of something that wasn't going to work anyways.

  16. #10
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,846
    Post Thanks / Like
    Likes (Given)
    4026
    Likes (Received)
    2081

    Default

    There are two ways I know of to get the proper threadform. One is with a tap, the other is single point threading on a lathe or turning center.

  17. Likes Bobw, Dwolf55793 liked this post
  18. #11
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    3,550
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3729

    Default

    Hi mhajicek:
    There is a third way, and that is to turn an undersize male electrode and burn it in with an orbital path on a sinker EDM.

    Good for when it's long and skinny or hardened or you need the threadform right to the bottom of a blind hole.

    Expensive to do, but sometimes it's the only way

    Cheers

    Marcus
    www.implant-mechanix.com
    www.vancouverwireedm.com
    Attached Thumbnails Attached Thumbnails dscn2206.jpg  

  19. Likes Dwolf55793, Bobw, mhajicek, TeachMePlease liked this post
  20. #12
    Join Date
    Jul 2004
    Location
    Houston, TX USA
    Posts
    32,832
    Post Thanks / Like

    Default

    Helix angle is 8.5 degrees at pitch dia. - tool has to clear this - even on your clunky engine lathe

  21. Likes Dwolf55793 liked this post
  22. #13
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    Quote Originally Posted by implmex View Post
    Hi Dwolf55793:
    There are a couple of important things you need to be aware of:

    First; the threadmill is like a saw, and a multi tooth threadmill is like a gang saw.
    There is no helix...it is just a saw with 14 1/2 degree faces.
    Changing the relief angle does nothing...it's still just a saw.
    There is no "helix angle" on the threadmill...each tooth around the periphery of the mill spins on a common plane, unlike a tap.

    The thread form follows a helical path, so there is an angle relative to the axis of the thread at which the saw fits best.
    For external threads, if you tilt the saw into the plane of the helix, you can cut a threadform that is the same as the profile of the saw teeth unless the face angles of the teeth approach zero (square threads).
    Square threads don't work because the helix of the thread is not a plane, but the saw teeth spin in a plane, so they'll clip the corners on the entry and exit sides of the cut.

    Because the thread profile also follows a helical path (non planar) for internal threads, the saw will interfere with the threadform as one or more of three conditions appear:
    1) the saw diameter approaches the thread minor diameter.
    2) the flank angle of the thread profile is reduced.
    3) the helix angle (thread pitch) increases.

    Conventional threadmills can be made to work on 3 axis VMC's because the threadmill is substantially smaller than the minor diameter, the flank angle is 30 degrees so it clears the thread flanks more (for a 60 degree vee thread) and the pitch is reasonably shallow for single start threads.

    All of these things are working against you for your double start ACME thread.
    So you have to fake it and accept what you get:

    First, you have a 5 axis setup, so you can tilt the cutter into the helix angle and rotate the part around the tilted cutter.
    Second, you can choose a cutter that's as small a diameter as you can...this means it will clip the profile less at the entry and exit zones of the cut.

    Be aware, as soon as you tilt the cutter into the helix angle, you are restricted in how deep you can internal thread...if you go too deep, you'll bang the shank of the cutter into the opening of the hole.
    This gets worse (obviously) as the helix angle increases, so with a double start thread, you cannot thread very deep.

    That's why it's not working for you.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

    On edit: mhajicek: you beat me to it...you're exactly correct, but you can mitigate it a bit using the bodge I described above.

    MC


    Thank you for your explanation. I kinda knew the problem but could not quite grasp what was happening. This is a one off piece, what would you say my best course of action would be? I of course could tilt (not full understanding how that helps yet though), My shop also has EDM sinker, and a cnc lathe. the part I am cutting is not round but we could probably make a fixture for the lathe.

  23. #14
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    Quote Originally Posted by Bobw View Post
    You can't do it. It is physically impossible in a 3 axis machine.

    You could have saved yourself a whole lot of money and just bought a tiny
    little key cutter, and you would have gotten the EXACT same results.

    I looked into it years ago. I don't remember if it was a 1-4 or a 1-5. ......
    Just went and looked, 1-5..

    So I drew it up.. Using the commercially available "Thread mill" that said it could
    do it.. It CAN'T.



    Notice how the flat blows out the entire thread form.. No need for any angles
    on the tool. Its acting as basically a key cutter..

    Increase the pitch and decrease the diameter, and its just going to get WORSE, and
    you'll get a result, just like you got.

    Even on a 60 degree standard thread that is thread milled everyday, you aren't getting
    a perfect thread form.. It may fall in tolerance, but its not "perfect".. Functional,
    in tolerance, everybody is happy, but still not "perfect" on the thread form. Close,
    but not as good as turning.

    I also modeled this up doing an external thread. That may be possible with messing with
    the geometry of the cutter. Internal, impossible.



    There is a reason that mass produced acme nuts are so expensive.. Its because they are
    a huge giant F'n pain in the ass.

    Edit: I think its neat to see the actual end results.... of something that wasn't going to work anyways.

    Thank you the visual is incredibly helpful. I am running a 5 axis machine does that make it possible to cut this, and if not whats my best option, I can EDM or we have a cnc lathe as well. The part is not round so I would have to figure out a fixture for the lathe though.

  24. #15
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    Quote Originally Posted by implmex View Post
    Hi mhajicek:
    There is a third way, and that is to turn an undersize male electrode and burn it in with an orbital path on a sinker EDM.

    Good for when it's long and skinny or hardened or you need the threadform right to the bottom of a blind hole.

    Expensive to do, but sometimes it's the only way

    Cheers

    Marcus
    www.implant-mechanix.com
    www.vancouverwireedm.com

    Thanks, we may do this I have to cut 2.2" deep threads so this may be my best option.

  25. #16
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,934
    Post Thanks / Like
    Likes (Given)
    1833
    Likes (Received)
    2480

    Default

    Quote Originally Posted by Dwolf55793 View Post
    Thank you the visual is incredibly helpful. I am running a 5 axis machine does that make it possible to cut this, and if not whats my best option, I can EDM or we have a cnc lathe as well. The part is not round so I would have to figure out a fixture for the lathe though.
    5 axis makes it possible, with the caveat that the length of the thread must be sufficiently short that the tool does not hit the shank when tilted to match the lead angle.

    I suspect that is not the case on your thread, and most likely the answer is no.

    Given that ACME threads are almost exclusively specified for motion transmission, the surface finish from edm might be unacceptable, which leaves two options; lathe, or U axis single pointing if your mill is capable of that.

  26. Likes yardbird, mhajicek liked this post
  27. #17
    Join Date
    Jan 2022
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    Quote Originally Posted by gregormarwick View Post
    5 axis makes it possible, with the caveat that the length of the thread must be sufficiently short that the tool does not hit the shank when tilted to match the lead angle.

    I suspect that is not the case on your thread, and most likely the answer is no.

    Given that ACME threads are almost exclusively specified for motion transmission, the surface finish from edm might be unacceptable, which leaves two options; lathe, or U axis single pointing if your mill is capable of that.

    Gotcha, that makes good since. I think we will probably end up making a fixture and turning it in there with our Okuma lathe. Seems the most straight forward and the correct way to go about it.
    Thanks again for the help!

  28. Likes mhajicek liked this post
  29. #18
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    3,550
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3729

    Default

    Hi again Dwolf 55793:
    I'm with gregormarwick on this.
    If you can single point thread it in the lathe, it will be the fastest easiest way and it will give the best outcome with the least pain.

    So I also encourage you to find a way to fixture it in the lathe and give 'er a go.
    Should work brilliantly.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining


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
  •