I am having trouble shelling a part I have designed. Every time I try, with no matter what thickness, I get the following message:
"The attempted shell operation had non-manifold inputs. Try with manifold inputs."
I have no idea what this means, can anybody help?
I've attached a copy of the file
Solved! Go to Solution.
There are multiple issues with the model.
The serious issues are shown in red in attached image.
1. Extrusion 6 is sick and does not do anything - delete it.
2. Sliver face - Manage>Rebuild All gets rid of this (but never should have had it in the first place - dimension sketches and use symmetry).
3. Zoom way in on the smaller red circle - did you really intend for this triangular hole to go all the way through the part?
4. Shelling the entire part does not make logical sense. Shell is global - I suspect your true design intent is to shell only part of the features.
5. sketches aren't dimensioned - yet when I dimension Sketch1 it is perfect. Why did you delete dimensions?
6. You don't indicate what thickness you really really want.
7. You don't indcate what (or none) faces you want to remove with the shell.
BTW - you didn't need to create any workplanes - all of your sketches could have been created on Origin workplanes. (a more robust technique of modeling)
Your sketches are a little rough.
Missing obvious tangencies.
I would use as few points in a spline as possible.
I often start with only two points and adjust Handles and Curvature to get my curve.
If I then need to add more nodes for more control - I add as needed.
Maintain tangency with other geometry.
Tip: When shelling an entire part do Shell feature after first feature.
Then drag the Shell Feature below EOP and create next feature.
Drag EOP below shell to test.
Repeat for each feature.
This way you know when a problem is going to occure earliest in the design process.
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