Trouble sweeping a thread profile over a tapered spiral for BSPT thread.

chris_dalby

I am new to Onshape and having come from TurboCad, I am finding it a steep learning curve.

I have created a tapered cylinder and then a spiral in an attempt to create a BSPT thread but I am having trouble sweeping the thread profile to "cut" the thread.
I get an error, "Sweep did not regenerate properly: could not create valid swept body, check input <-Thread profile [sketch]".

I have looked at the thread profile sketch and cannot see where the problem is.

Can anyone help?

https://cad.onshape.com/documents/9238344ed16caf34f2427eca/w/1d6eeef2ef5fac13a13b4ff8/e/f30186e383d1382beb982cb4

NeilCooke

Hi @chris_dalby

Because the cone is tapered, your sketch when swept will have some edges inside the cone and some outside, so the boolean remove operation will fail. A good way to see what went wrong is to hover your mouse over the red title in the dialog to see the error message, or use New instead of Remove to see what the feature can build. What you need to fix this is a sketch like in the image below that is "overbuilt" to ensure there are no slither edges in the remove operation. Also note the "pierce" constraint circled in red between the sketch vertex and the helix. You can use construction lines to get the exact dimensions you need (as shown). The 0.1 dimension is arbitrary.

_Ðave_

The  top edge of your thread profile isn't parallel with the taper therefore half of that edge isn't protruding above the od of the taper and causing your issue. Hope that's clear, if not I'll try to explain another way.

_Ðave_

chris_dalby

Thanks to you both, Neil and Dave.

This did the trick. Can fix my other drawing now :-)

chris_dalby

I got tired of trying to sort that out so I changed the spiral and tapered cylinder to the thread minor dia and tried to add the sweep. Still no good but it would allow me to sweep a new part so thats the way I went.

Not the result I wanted but time is precious.

bradley_sauln

Have you tried the following FeatureScript? https://cad.onshape.com/documents/6b640a407d78066bd5e41c7a/w/4693805578a72f40ebfb4ea3/e/197ed76423f98702e0d8e7db

chris_dalby

I just tried it now. Great feature but it did not work. :-(  "Error regenerating". I have left the part with the TH in place if you want to take a look.
Does it not work on revolves?

chris_dalby

I found it impossible to do a tapered thread so have reluctantly gone to a parallel instead.

JAMES_SOLIDPROFESSOR

Hi Chris,

Hopefully I can help out with your thread situation! I made a quick tapered cylinder and created a thread using a Sweep. Here’s the process I used:

1. I created a conical face by drafting an Extrude feature.

2. I used the Helix command to create the sweep path on the face. Simply select the conical face, then set the number of revolutions, direction of the helix, etc.

3. In order to create the profile, I created a new reference plane that’s attached to the end point of the helix and is normal to the curve. To do this, I enabled the Reference Plane command, selected the “curve point” option, and selected the endpoint of the helix as the reference point as well as the helix itself as the reference curve.

 4. Sketch the profile on this new plane. In this case I created a triangular cutout. Just be sure that your profile won’t be self-intersecting as it’s swept around the path. This will cause an error and keep it from generating. If it does this, try adjusting the width of the profile.

  

5.      Enable the sweep command, set it to the “solid” option, and choose the sweep profile and the helix as the path. Click the green check and you should be good to go!

Hopefully that works for you! The thread could be refined a lot more than what I showed here, but it should be a good starting point for what you need.

chris_dalby

Than you for your response James, much appreciated.

Your excellent tutorial is almost identical to one I have been referring to, https://forum.onshape.com/discussion/comment/4993#Comment_4993.

Using the method you described, I have been unable to create the tapered thread on the revolve that I have in my drawing. I tried reducing the width of the thread profile to something ridiculously small just to prove it was not interfering with itself.

I have created a copy of the problematic version if you want to take a look.
https://cad.onshape.com/documents/57ffe90f67f1c910e8d195f0/w/0f0e2d1acffd62eb9eee8587/e/f5392f2548f0f974d0a7e47c

chris_dalby

Grrrrr!

What am I missing?

An example based on your very clear tutorial James.

https://cad.onshape.com/documents/56676bf63fe053b51b221225/w/8f2bd190f34d9267e8136979/e/8ebe31bd123ffc7b92b995b2

NeilCooke

Hi @chris_dalby

Because the cone is tapered, your sketch when swept will have some edges inside the cone and some outside, so the boolean remove operation will fail. A good way to see what went wrong is to hover your mouse over the red title in the dialog to see the error message, or use New instead of Remove to see what the feature can build. What you need to fix this is a sketch like in the image below that is "overbuilt" to ensure there are no slither edges in the remove operation. Also note the "pierce" constraint circled in red between the sketch vertex and the helix. You can use construction lines to get the exact dimensions you need (as shown). The 0.1 dimension is arbitrary.

_Ðave_

The  top edge of your thread profile isn't parallel with the taper therefore half of that edge isn't protruding above the od of the taper and causing your issue. Hope that's clear, if not I'll try to explain another way.

_Ðave_

chris_dalby

Thanks to you both, Neil and Dave.

This did the trick. Can fix my other drawing now :-)