What's new
What's new

Locating a thread start

TRC

Aluminum
Joined
Jun 22, 2022
Greetings,

A part I made need to have a thread start at a certain location and I'm not sure how to put it on a blueprint. I haven’t found anything in my handbook and it does not appear to be standard.

There are three parts: one externally threaded, one internally threaded (the nut) and one to be squeezed between the two previous one (referred as part 3).

The goal is that when the special nut is going to rotate by 90 deg, it's going to translate by a certain amount and lock with a part between those threaded part and the nut.
  1. Align the externally threaded and the nut to allow part 3 to pass
  2. Push part 3 against the externally threaded part
  3. Rotate the nut to lock the assembly together
Here are a few pictures (you can switch between them using the arrows onto the pictures):

Is there is any standard way to transmit to a machinist this information without ending with an expensive pile of scrap?
 
How are you going to inspect the individual part? All the jobs I’ve ever done where a thread required clocking the customer provided a gauge to inspect the part against.

You could add a section view and tolerance the distance to the first full thread.

But clocking threads is a pain. It would be much better to decide what tolerance you need on clocking and engineer that requirement out. You could potentially add whatever features you need to be able to adjust it to be in-tolerance at assembly. You have c-sunk holes on the flange, it would be better (cheaper) to add as many patterns as will fit than clock the thread.
 
How are you going to inspect the individual part? All the jobs I’ve ever done where a thread required clocking the customer provided a gauge to inspect the part against.
The precision is not that important. What matter is that the part is locked and that there is enough material to prevent plastic deformation while tightening the bolt.

I guess I could make a gauge, but I would still need to draw since there is no way I'm convincing my client to lend his medical equipment to allow them to test them onto the original parts.

You could add a section view and tolerance the distance to the first full thread.
Like that?
But clocking threads is a pain. It would be much better to decide what tolerance you need on clocking and engineer that requirement out.
As an engineer and an hobby machinist, may I ask why?
You could potentially add whatever features you need to be able to adjust it to be in-tolerance at assembly. You have c-sunk holes on the flange, it would be better (cheaper) to add as many patterns as will fit than clock the thread.
I tried to avoid this solution, but since I have to fit this onto an already existing machine, I do not know the exact fit and the said machine is hard to access, since it's always being used. Plus this need to be properly aligned with the dowel pin and everything.

Would it not have been a retro-engineered part, I would agree with you and do a simpler coupling mechanism, but the original machine seem to be using this as well. Worst case I will change il later before that hit production if this is too expensive.
 
As an engineer and an hobby machinist, may I ask why?
Everything in the chain effects the starting position of the thread. If it is a turned part you have the spindle resolver, spindle speed, the ramp rate of the servo, how was the insert touched off, insert-insert variations, phase of the moon etc. Thread milling is easier, at least you have a more consistent start for where the cutter enters the work.

Say you want to clock it with in 5°, that is 5°/360°*1mm pitch, or a total of .0139mm (.0005in). That's a pretty small number to chase around. If you call out the depth to the thread on a section line, how to you measure the location of that feature accurately? Section it and use an optical comparator? Fart around with a CMM? To check it in the machine you'd need some sort of gauge, maybe a finger or ball on some indicator. Well how do you make that and to what tolerance and how do you and calibrate it? It snow balls. If you can engineer that requirement out you're better off.

Some times it's required like a locking bayonet like you have, or what's on a Kwik Switch or Erickson spindle nose. And those just suck. You end up needing a gauge that you can install and check the thread position, then tweak an offset and throw that part away and try again. The functional gauge can be arbitrary at first but if you want to make a second gauge, then it gets complicated again.
 
Last edited:
It sounds like a proprietary fitting that was designed to be difficult to reproduce.
Greetings,

A part I made need to have a thread start at a certain location and I'm not sure how to put it on a blueprint. I haven’t found anything in my handbook and it does not appear to be standard.

There are three parts: one externally threaded, one internally threaded (the nut) and one to be squeezed between the two previous one (referred as part 3).

The goal is that when the special nut is going to rotate by 90 deg, it's going to translate by a certain amount and lock with a part between those threaded part and the nut.
  1. Align the externally threaded and the nut to allow part 3 to pass
  2. Push part 3 against the externally threaded part
  3. Rotate the nut to lock the assembly together
Here are a few pictures (you can switch between them using the arrows onto the pictures):

Is there is any standard way to transmit to a machinist this information without ending with an expensive pile of scrap?
a note: a note on the print can clarify expectations.
 
  • Like
Reactions: TRC
Say you want to clock it with in 5°, that is 5°/360°/1mm pitch, or a total of .0139mm (.0005in). That's a pretty small number to chase around. If you call out the depth to the thread on a section line, how to you measure the location of that feature accurately? Section it and use an optical comparator? Fart around with a CMM? To check it in the machine you'd need some sort of gauge, maybe a finger or ball on some indicator. Well how do you make that and to what tolerance and how do you and calibrate it? It snow balls. If you can engineer that requirement out you're better off.
Ok, if I get it straight, any vertical offset would make this part completely inaccurate if it's thread milled for a small pitch? I agree with you that .014mm is small to run after, but that also mean that 20° is .002' for a thread this small, and also leave me with 70° of supporting materials. Worst case, both the nut and the externally threaded part would be at the worst possible configuration and still allow me 50° of supporting material, which should be enough since the force applied onto this assembly is pretty small.

However, wouldn't it be easier to make an internally threaded jig that allow any already threaded cylinder to have it's upward face to be just at the right spot to allow this to be located easily?

I'm not very knowledgeable in the abyss that is the CNC's world, but wouldn't making a one off jig easier of an high production run? Or would the idea of making a jig be frowned upon nowadays?

It sounds like a proprietary fitting that was designed to be difficult to reproduce.
I swear I saw this kind of mechanism in another industry, so I guess it's not a proprietary design, but the original machine is swiss made, which explain a lot...
 
Last edited:
Thread the part first then thread it into a fixture and stop against the face then do the other features. This is the only way to make them consistent.
 








 
Back
Top