I'm trying to create a sweep along the surface of an outer cylinder on a curved object.

koki_okoshi · January 2024

I'm trying to create a swept object along the helix of an outer cylinder on a curved object to create a ditch.

However. it doesn't generate one properly for unknown reasons, and I've been stuck for more than 2 hours.

I've already tested out several ways to adjust the position of a graphed triangle but to no avail.

I would be very appreciative if anyone could help me solve this problem as this is pretty urgent.

The error code says "Swept 1 did not generate properly; Could not create a valid swept body, check input."

Here's the link to my Part Studio:
https://cad.onshape.com/documents/1014749151f35a39edc72c66/w/48176e670c5dcde4ea151154/e/378014e07afff1127e6a025f?renderMode=0&uiState=65b244c0cac8940ccef52701

Thanks,
Koki

Image: https://us.v-cdn.net/5022071/uploads/editor/n1/c20uehjewxsm.png

bje

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Image: https://us.v-cdn.net/5022071/uploads/editor/2q/isy1ovwgbwi1.png

S1mon · January 2024

If you want to add modeled threads to a hole, there are custom features which will do this for you.

https://forum.onshape.com/discussion/19009/threadlab-internal-external-modeled-cosmetic-threads-with-external-thread-callouts/p1

In this case, your sweep is self intersecting, or at the very least, if the geometry is perfect, the swept shape shares a helical edge. This results in a non-manifold shape that the Parasolid kernel cannot handle. If you change the width just slightly (e.g. from 2.0 to 1.95), the sweep works fine:

Image: https://us.v-cdn.net/5022071/uploads/editor/nj/m28vk6800t5o.png

Real threads have flats or radii at the tips or roots depending on if they are internal or external.

https://en.wikipedia.org/wiki/ISO_metric_screw_thread

koki_okoshi · January 2024

Yes, this worked!
However, I'd like to make the ending more natural as if the helix continues outside on the cylinder-shaped space.
How can I achieve this?

Image: https://us.v-cdn.net/5022071/uploads/editor/oy/q5ar0tai1t2j.png

robert_scott_jr_ · January 2024

You could create a cylinder with your first extrude by using New instead of Remove and put the helix on the cylinder, continuing on with the sweep. This creates the threaded body to subtract from part 1. - Scotty

https://cad.onshape.com/documents/b533c40445a1bec85ddfe846/w/e099702c4b6b16024f60d9d0/e/0493dd49b412463d37e3e92e

koki_okoshi · January 2024

Yes, this worked!
However, I'd like to make the ending more natural as if the helix continues outside on the cylinder-shaped space.
How can I achieve this?

robert_scott_jr_ · January 2024

Note that the cylinder with the external threads extends beyond the curved face of Part 1 thus avoiding the abrupt thread end in the boolean operation. - Scotty

rick_randall · January 2024

robert_scott_jr_ said:

You could create a cylinder with your first extrude by using New instead of Remove and put the helix on the cylinder, continuing on with the sweep. This creates the threaded body to subtract from part 1. - Scotty

https://cad.onshape.com/documents/b533c40445a1bec85ddfe846/w/e099702c4b6b16024f60d9d0/e/0493dd49b412463d37e3e92e

This approach is spot on - but you still need to create a chamfer on the edges of the hole(s). I would recommend you chamfer before creating threads then follow Scotty's procedure. Try using the thread pitch as the chamfer width ( this usually yields good results).

rick_randall · January 2024

I have copied and edited your model - See if these changes are what you were looking for.

https://cad.onshape.com/documents/6077fd54eef61c8c70e46848/w/52387a220c4a6d1b3a075a2e/e/409470315c41b3bb93bf6af1

I'm trying to create a sweep along the surface of an outer cylinder on a curved object.

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