Results 1 to 17 of 17
Like Tree3Likes
  • 1 Post By Bobw
  • 2 Post By oldbikerdude37

Thread: Acme Threading ID

  1. #1
    behindpropellers is online now Stainless
    Join Date
    Dec 2008
    Location
    NE OHIO
    Posts
    1,284

    Default Acme Threading ID

    Quick question:

    Can I buy a single point acme thread thread mill? Need it for a proto and would be nice if I can use it for other stuff.

  2. #2
    Limy Sami is online now Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,384

    Default

    Not so quick a Q Prop you can have a lotta problems thread milling acme......... external or internal?........... diameter? ..... pitch?...# of starts?

  3. #3
    T. Jost is online now Cast Iron
    Join Date
    Jan 2007
    Location
    Hillsboro, Kansas USA
    Posts
    372

    Default

    I don't know about single point, but Advent Tool in Illinois pretty much specializes in acme thread mills.

  4. #4
    i_r_machinist is offline Titanium
    Join Date
    Apr 2007
    Location
    Dublin Texas
    Posts
    2,233

    Default

    I've used lathe threading bars for this application. No biggy.
    i_r_

  5. #5
    Heavey Metal is online now Titanium
    Join Date
    May 2011
    Location
    Texas
    Posts
    2,950

    Default

    It is geometricly impossible to threadmill an internal acme

    You can get close

    You can do it with some tricky 5 axis stuff but not very deep.

    Singlepoint it.

  6. #6
    behindpropellers is online now Stainless
    Join Date
    Dec 2008
    Location
    NE OHIO
    Posts
    1,284

    Default

    Alright...

    I see its not an easy question after a couple calls. Seems nobody makes a 3/8-8 Acme tap.

  7. #7
    Bobw's Avatar
    Bobw is online now Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    5,377

    Default

    In a lot of situations, I don't see how you can do it. Its much like trying to threadmill a square thread.

    I drew these up a while ago, and I've posted them before. its a 1-5. Internal and external, using a threadmill
    with the actual threadform.





    I can see how you can fudge an external thread by modifying the flank, I can see how you could fudge an
    ID thread to "work", but its not going to be right. If it was a large ID thread with a fairly shallow helix, I could
    see fudging it so it was actually in tolerance, sort of.

    Kind of like trying to threadmill a square thread with a key cutter.

    I can see getting it close and then chasing it with a tap.

  8. #8
    Limy Sami is online now Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,384

    Default

    Quote Originally Posted by behindpropellers View Post
    Alright...

    I see its not an easy question after a couple calls. Seems nobody makes a 3/8-8 Acme tap.
    Any help?

    ACME Right Hand Taps

  9. #9
    oldbikerdude37's Avatar
    oldbikerdude37 is offline Stainless
    Join Date
    Jun 2010
    Location
    milton freewater oregon
    Posts
    1,744

    Default

    small acme is a pain to single point. a 5/8" 10tpi is a problem as you have to use a bar thats 3/8" and take many passes.

    I could see thread milling could be dead simple.

  10. #10
    T. Jost is online now Cast Iron
    Join Date
    Jan 2007
    Location
    Hillsboro, Kansas USA
    Posts
    372

    Default

    Bobw;
    You've got a lot more machining experience than I do, but I believe that your logic on the impossibility of acme thread milling is flawed. If you apply the same visual experiment to any thread you will find that the theoretical disk breaks through the perfect thread form. It would be true if you were trying to grind a thread form without canting the work-piece or doing something else to get things lined up with the helix angle.

    Thread mills have very steeply relieved flanks so they don't screw up the thread form. They are also shaped so that they produce the right form. They are not a proper acme form but they make one, if that makes any sense. They are discrete teeth that are rising (or descending) while they are cutting. Thread milling any thread form is theoretically possible but you can't do it with something that will gauge as an acme thread.

    I don't have the proper technical jargon for this so I'll stop trying to sound like I do. IT IS POSSIBLE to thread mill acme threads.

    Todd

  11. #11
    Bobw's Avatar
    Bobw is online now Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    5,377

    Default

    Quote Originally Posted by T. Jost View Post
    Bobw;
    You've got a lot more machining experience than I do, but I believe that your logic on the impossibility of acme thread milling is flawed.
    Throwing out 5 axis trickery, or 4th....

    I understand how you can fudge the thread form on a threadmill to get a correct threadform in the part. It becomes easier and easier as several things
    happen, included angle becomes bigger, diameter becomes bigger, helix angle decreases. They can also become impossible as diameter decreases, included angle
    shrinks(square thread) and helix angle increases (multi start threads).

    2 things going against you right there on an ACME. 29 degree included angle, and they are usually really steep compared to a standard 60 degree thread.

    I wish on those drawings that I had also done a model of a sharp 29 degree included thread. Anyways... You have that flat crest on the OD, you can't fudge that.
    No amount of trickery or fancy grinding can fudge that. On that thread that I modeled(its what I needed to make), the flat crest blows out the entire threadform, all of it, gone. You could threadmill that same thread with an acme shaped tool or a simple keycutter (relieved properly so it will cut, same thickness as the crest of the thread) and come up with the exact same result.

    Tool diameter(spinning disc) plays a part too... Still can't fudge that flat crest.

    An acme threaded rod will thread into it, but it won't be an acme thread. And sometimes that's good enough.
    gregormarwick likes this.

  12. #12
    oldbikerdude37's Avatar
    oldbikerdude37 is offline Stainless
    Join Date
    Jun 2010
    Location
    milton freewater oregon
    Posts
    1,744

    Default

    Quote Originally Posted by Bobw View Post
    Throwing out 5 axis trickery, or 4th....

    I understand how you can fudge the thread form on a threadmill to get a correct threadform in the part. It becomes easier and easier as several things
    happen, included angle becomes bigger, diameter becomes bigger, helix angle decreases. They can also become impossible as diameter decreases, included angle
    shrinks(square thread) and helix angle increases (multi start threads).

    2 things going against you right there on an ACME. 29 degree included angle, and they are usually really steep compared to a standard 60 degree thread.

    I wish on those drawings that I had also done a model of a sharp 29 degree included thread. Anyways... You have that flat crest on the OD, you can't fudge that.
    No amount of trickery or fancy grinding can fudge that. On that thread that I modeled(its what I needed to make), the flat crest blows out the entire threadform, all of it, gone. You could threadmill that same thread with an acme shaped tool or a simple keycutter (relieved properly so it will cut, same thickness as the crest of the thread) and come up with the exact same result.

    Tool diameter(spinning disc) plays a part too... Still can't fudge that flat crest.

    An acme threaded rod will thread into it, but it won't be an acme thread. And sometimes that's good enough.
    You may know way more than me but I never did care about a root diameter of the max crest diameter, thats not where the work gets done at all. that stuff means almost nothing.

    Again lot of guys over complicate things and need a $20,000 butt hair gauge to get it done. those boys better learn a few tricks or I will be at thier shop buying stuff for .05 cents on the dollar.

    Some of you guys would crap when you seen my ghetto fixtures, others would make money and keep the magic tricks under their hat.

    My point it the fact its not hard to do. get the job done and don't chaise your tail all day, kids in china do it every day, maybe 15 hours a day.
    flatbelt and najnielkp like this.

  13. #13
    T. Jost is online now Cast Iron
    Join Date
    Jan 2007
    Location
    Hillsboro, Kansas USA
    Posts
    372

    Default

    I will concede that the anti-acme-thread-milling may have a point. It may not be possible to thread-mill "PERFECT" acme threads. In fact it is not possible to thread mill any kind of perfect threads. Microscopically there are a series of flats left by any interpolation of an arc or helix. Even with a chord error of 1 ten millionth of an inch there is still error.

    The acme threads I had to mill (internal and external by the way) did not have to gauge or match any standard. They just had to work and play well with each other. Perhaps I wasn't making acme threads. But my customer found them to be superior to the previous shop's efforts that were made from comercially purchased acme nuts welded into a boss to create the internal threads and lathe turned acme threads. I guess it all comes down to what works in a given situation.

    Maybe it's all voodoo and smoke. But the thread-mills I used worked out alright for me. Perhaps the people who market Acme-Thread-Mills should be prosecuted for fraud but I won't be joining the class action suit.

  14. #14
    Bobw's Avatar
    Bobw is online now Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    5,377

    Default

    Quote Originally Posted by T. Jost View Post
    But the thread-mills I used worked out alright for me. Perhaps the people who market Acme-Thread-Mills should be prosecuted for fraud but I won't be joining the class action suit.
    If you actually have one, measure it or something. I'd love to be proved wrong. I'd like to swing it and see. If its possible, I'd be happier than a pig in..... mud. At this point, I don't think it is.

    I do appreciate the "it has to work". I'm a huge fan of that, and practice it when possible, unfortunately... sometimes.... to pay the bills.... you have to take jobs and sell them to people that actually care if its right. Doesn't have to work, just has to be to print. If I had a dollar for everytime it was to print and didn't work, I'd be rich.

    Old biker dude:
    Some of you guys would crap when you seen my ghetto fixtures,
    I've had them, I still have them, I'll keep making them. I made a nylon surface plate for a job. I actually bolted a 20X40, 2 inch thick nylon surface plate to my machine.
    Wood is fine, especially when it comes from a dry rotted busted pallet, those stupid door/window shims are fantastic for taking up a little play here and there, honestly far better
    than a jack screw, and I love my jack screws, they can bend a casting or weldment back into shape real quick.

    Here is a crappy one I built 8 years ago. The base plate is a scrap part and all the uprights are undersize material bought by a customer.



    The guy who was running the shop at the time told me it looked like shit, and it does. Oddly I don't work there anymore and the customer actually bought that giant
    mass of crap from my previous employer, along with the 2nd 3rd and 4th op fixtures, used them at least a dozen times in the past few years.



    If you can threadmill an internal Acme, show me. I've showed you why I don't think it will work, at least correctly.

  15. #15
    Heavey Metal is online now Titanium
    Join Date
    May 2011
    Location
    Texas
    Posts
    2,950

    Default

    When you thread mill a part so that it is right with wires it will not gague (because of the concave flank)If you thread it to gague the pd is off.

    If your makeing both parts and all that it needs to do is screw together you can make that happen

    But I am not bitching I make my liveing fixing others f***ups thanks

  16. #16
    gregormarwick is online now Stainless
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    1,520

    Default

    Quote Originally Posted by Bobw View Post
    Throwing out 5 axis trickery, or 4th....

    I understand how you can fudge the thread form on a threadmill to get a correct threadform in the part. It becomes easier and easier as several things
    happen, included angle becomes bigger, diameter becomes bigger, helix angle decreases. They can also become impossible as diameter decreases, included angle
    shrinks(square thread) and helix angle increases (multi start threads).

    2 things going against you right there on an ACME. 29 degree included angle, and they are usually really steep compared to a standard 60 degree thread.

    I wish on those drawings that I had also done a model of a sharp 29 degree included thread. Anyways... You have that flat crest on the OD, you can't fudge that.
    No amount of trickery or fancy grinding can fudge that. On that thread that I modeled(its what I needed to make), the flat crest blows out the entire threadform, all of it, gone. You could threadmill that same thread with an acme shaped tool or a simple keycutter (relieved properly so it will cut, same thickness as the crest of the thread) and come up with the exact same result.

    Tool diameter(spinning disc) plays a part too... Still can't fudge that flat crest.

    An acme threaded rod will thread into it, but it won't be an acme thread. And sometimes that's good enough.
    I've been through this before, drawn up the same models, done the same head scratching, and come to the same conclusion. Correct thread form ACME threadmilling is not possible with three axis', unless the pitch/diameter happens to be such that the helix angle will allow the flank angle to swing without gouging. On all the acme threads I've looked to do this way, the helix angle is always too much.

    Cutter relief is irrelevant in this case as it's the thread form itself that will gouge. I cannot conceive any means of compensating the cutting edge to generate the correct threadform without gouging.

  17. #17
    4GSR's Avatar
    4GSR is offline Titanium
    Join Date
    Jan 2005
    Location
    Victoria, Texas, USA
    Posts
    2,769

    Default

    A place I worked at several years ago, near Houston, we thread milled 8-pitch stub acme threads day in- day out. Of course the smallest was around 1.500"

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
  •