Cut Threads

Hello to all,

When I model threads in a shaft without a thread relief at the end
using the Helical Sweep>Cut command I don't want the last thread to
end abruptly but gradually. Like when you're single pointing the
thread and pulling the cutting tool slowly.

Is there a way to do a gradual ending to the thread?

Thank you for your expertise.

 

I was a little disappointed, initially, at seeing the abrupt end to a blind cut thread. And experimented with different ways to 'simulate' a more realistic blind thread end. But even that depends on the method of production. So, when I've done single pointing on a Hardinge that has travel stops and a lever for backing out the cross slide, I got a somewhat tapered lead out which could be approximated by using the flat face of the thread end as a sketching plane and simply extruding straight through. When milled or rolled thread, the result was a rounded lead out that could be approximated with a revolved cut using revolved cut and the thread end as the sketched profile. The hard part is figuring out to get the normal planes and an axis on a plane with that thread profile. But, when you look at it, you'd be surprised at how little difference in geometry exists between a straight extruded cut and this kind of revolve. The threads I've cut on a screw machine with a spring loaded threading attachment. Four threading inserts sprang open at the proper depth. The end of the thread was not totally abrupt but more that the straight extruded cut through. Bolts are cut this way if they are not hot headed (rolled in while the metal is still yellow-red) and some threads are forged which means the form is in the die. Maybe you could make a cut following a curve-through-points trajectory that started at the root and went half a turn around, winding up at the surface, about half a pitch advanced. Might work if the trajectory were tangent at both ends. Another suggestion: don't make the threads subtractive, make them additive: thread base at root diameter, thread as solid extrusion instead of cut and run this into the shoulder. Not realistic but not as abrupt as the square end of the cut thread.

However, all these bright ideas aside, I (and I suspect most other Pro/e users) gave up on helical swept threads a long time ago because
a.. cosmetic threads accomplish the same thing and capture more parametric information, same as the Hole tool does
b.. helical sweeps are computationally intensive, require a lot to accomplish little beyond the decorative or the 'ooh/ahh' factor: adding extra work the the irrelevant, prettifying the ridiculous, is super-irrelevant
c.. just try regening an assembly filled with bolts with helical sweep cuts; or change a thread pitch in a family table of bolts with helical cut threads and be prepared to wait.
Something neat to learn as a student, something people have tried to put to good use but that is not in everyday use in the modelling world. Don't waste your time prettifying or perfecting the irrelevant.

David Janes

 

After I have successfully cut my helical sweep, I go back in & add a little
"tail" to the end of my sweep profile sketch. For external I go away from
the center, for internal I go towards the center. I just make them on the
fly, quickly, nothing fancy.

This can sometimes fail if you reference a centerline when creating the
thread form sketch. What I do is position my threads using a temporary
centerline on the P.D. Then I delete the centerline & dimension the form
to the sweep profile. Truncating at the Major or minor (internal or
external) threads & wham! its pretty damn close to a "real" thread. I make
them slightly looser when getting rapid prototypes made & they work well.

We use the cut threads rather than cosmetic for 3 reasons. One is weight
(volume) which must be very accurate on small parts that are high volume.
Second reason is we make working prototypes from the models. Third is that
they look cool as hell in drawings & jpegs from the models. The marketing
pukes LOVE the pics. Tapered pipe threads look very cool.

 

It's hard (at least for me) to describe so I went ahead & posted some jpegs
of what the sweep profile, thead form, & a cut away view of the threads with
the run-out.

http://home.comcast.net/~imageguy/sweep.jpg

http://home.comcast.net/~imageguy/thread_form.jpg

http://home.comcast.net/~imageguy/pipe_thread.jpg

 

Another cute violation of OCCAM´s razor.

Things made much more complicated than necessary.
For marketing purposes and the joy of playing with 3DCAD.

But that´s the way it goes once computers are powerful enough
(an engineer´s manpower and -time seems not to count any more).

Before standardization of threads was invented and nuts´n´bolts
became most common some hundred years ago physical threads were cut
*manually*, one by one, in a process as difficult as forging a sword.

It seems at least engineering is heading back there.

 

Amen to that!

I'm the poor bastard who has to grind the thread profile in the mould cores.
Often, all you get to take the measurements from is a poorly translated solid.
Then, when you ask for a simple cut-view of the thread, preferably as a DXF file
(all you really need is basically the pitch, the pitch diameter and the bottom
diameter) you get a cut view consisting of thousands lines and splines and
whatnot, all in the wrong scale, and all in a multitude of hideous colors.

Sometimes I want to cry...

 

Don't cry for me Jan Nielson...

 

Seems that the SLA machine can't seem to make a thread without them being in
the STL.
At least the one we use.

 

Waaaahhh...