Post By Bobw
Post By oldbikerdude37
Acme Threading ID
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.
Not so quick a Q Prop you can have a lotta problems thread milling acme......... external or internal?........... diameter? ..... pitch?...# of starts?
I don't know about single point, but Advent Tool in Illinois pretty much specializes in acme thread mills.
I've used lathe threading bars for this application. No biggy.
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.
I see its not an easy question after a couple calls. Seems nobody makes a 3/8-8 Acme tap.
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.
Originally Posted by behindpropellers
ACME Right Hand Taps
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.
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.
Throwing out 5 axis trickery, or 4th....
Originally Posted by T. Jost
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.
Originally Posted by Bobw
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.
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.
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.
Originally Posted by T. Jost
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:
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.
Some of you guys would crap when you seen my ghetto fixtures,
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.
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
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.
Originally Posted by Bobw
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.
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"