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How to sweep over a cylindrical face along a projected curve instead of a helix
maarten_sesink
Member Posts: 6 ✭
I am new to Onshape and to CAD design in general. I am trying to design a gear with its teeth swept along a curve I have projected on a cylindrical surface. This works fine when I use a helix, but it won't generate properly, or at al similarly, when I select a projected curve on the same surface in place of the helix. Is it at all possible what I am trying to achieve? If so what am I doing wrong? Thanks!
Best Answers
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MDesign
Member Posts: 282 ✭✭✭
just need to extend the profiles into the hub to eliminated the non manifold error. in this example I did one tooth and patterned it. I applied the fillet after the loft was well. then second example I just lofted the whole sketch as you had via the path then subtracted out the hole.
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GregBrown
Member, Onshape Employees, csevp Posts: 219 
Your sketch is not the most optimal for this tooth profile (it is made of a large number of obviously non-tangent line segments, the root fillet is not tangent to the tooth, etc)
If you want to try to make a "wavy" tooth gear you could piggyback on top of the excellent Spur gear custom feature… https://cad.onshape.com/documents/5742c8cde4b06c68b362d748/v/1db29081376c095cf10e2a3d/e/c72760543a0d4412e72f6d38
Make a dummy gear the appropriate size - I think yours is 23 teeth, module=1mm, (i.e. PCD=23mm) Give it some arbitrary depth like 5mm. Make another Spur gear offset from this: you could transform copy, make it from scratch, or a 1000 other ways it is not so important… Now Loft between two faces of these dummy parts with Normal to profile as the boundary conditions for both profiles. Use Connections and pick two appropriate vertices on the teeth you want connected. You only have to do this for a single pair, the loft will take care of itself.
Check it out here: https://cad.onshape.com/documents/40a250b23fd3c4edabf65acf/w/dc15b086669c71b347a59ee4/e/b07d08c99dfa0e176d7ccdce
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glen_dewsbury
Member Posts: 835 ✭✭✭✭
Ah. Posted this without a browser refresh . Then saw your post Greg.
You may want to check off reapply features in the circular pattern.
I also eliminated the sketch circular array. Better as a feature pattern of the sweep. More efficient.
Used an actual curve instead of a bunch of lines, much more effective and smoother curve with less control points to form tooth.
1
Answers
The error message is doing its job - it's telling you that with the current selections you are trying to create non-manifold geometry (which is not valid for our geometric modeler.) In other words the Sweep path is such that at some point(s) along the path there is a zero thickness intersection between Part 1 and the teeth you are creating. You might want to try some of the Profile control options in the Sweep feature, or change the path, or the section… If you share a link to your doc we could see more and try to help.
Thanks for responding! I didn't doubt the error message was right, I just had no idea how to resolve it, even after researching, as I am completely new to cad design. I did mess around with those options but couldn't fix it. Thanks for wanting to take a look.
Here's the link: https://cad.onshape.com/documents/9d957defda8d469e5d434fbf/w/3a5262695619b16c3426a1ea/e/a6248b03b31df5d5510bd977
You might have to use a loft with a path instead of sweep.
The learning center is also a good place to start
https://learn.onshape.com/
Thanks. I already tried that but it gave the same error message. Possibly because I do not know how to precisly offset the two faces along the top and bottom diameters by the same amount as the curve travels down the cylinder sideways. Although the value I have must be an extremely close aproximation. Still I sustpect there is something other/more fundamental I don't understand underlying the failures with both methods.
Thanks, I'll take a look, I would like to get more familiar with the software.
Still, if someone has another idea that could help me resolve this specific issue that would be very welcome.
just need to extend the profiles into the hub to eliminated the non manifold error. in this example I did one tooth and patterned it. I applied the fillet after the loft was well. then second example I just lofted the whole sketch as you had via the path then subtracted out the hole.
Your sketch is not the most optimal for this tooth profile (it is made of a large number of obviously non-tangent line segments, the root fillet is not tangent to the tooth, etc)
If you want to try to make a "wavy" tooth gear you could piggyback on top of the excellent Spur gear custom feature… https://cad.onshape.com/documents/5742c8cde4b06c68b362d748/v/1db29081376c095cf10e2a3d/e/c72760543a0d4412e72f6d38
Make a dummy gear the appropriate size - I think yours is 23 teeth, module=1mm, (i.e. PCD=23mm) Give it some arbitrary depth like 5mm. Make another Spur gear offset from this: you could transform copy, make it from scratch, or a 1000 other ways it is not so important… Now Loft between two faces of these dummy parts with Normal to profile as the boundary conditions for both profiles. Use Connections and pick two appropriate vertices on the teeth you want connected. You only have to do this for a single pair, the loft will take care of itself.
Check it out here: https://cad.onshape.com/documents/40a250b23fd3c4edabf65acf/w/dc15b086669c71b347a59ee4/e/b07d08c99dfa0e176d7ccdce
Ah. Posted this without a browser refresh . Then saw your post Greg.
You may want to check off reapply features in the circular pattern.
I also eliminated the sketch circular array. Better as a feature pattern of the sweep. More efficient.
Used an actual curve instead of a bunch of lines, much more effective and smoother curve with less control points to form tooth.
https://cad.onshape.com/documents/2aa4d8be793100e5fa95fbf3/w/3a7c3fa108289bbe811a4c08/e/b8cdfef91bbca1c38a6c0c07
Thanks so much for taking the trouble to figure it out! Very grateful for all the detailed feedback. I'm learning a lot and my issue is solved 👍️