Shell Artifacts

[SEC_CAD]

Hi I am trying to shell my model to have a wall thickness of 2.6mm. The Shell operation is creating features that are less than 0.5mm in size. How do I command the Shell operation to not create these features?

[johnsonshiue · Accepted solution]

Hi! I think this is a bug indeed. The weird faces came from the fact that some vertical faces are gone due to large offset distance. The artifact faces help keep the model water tight. Inventor Shell works well when the offset does not lead to topological change. When there is topological change (change in number of faces or edges on offset), failures or weird behaviors can happen. If I understood how it worked correctly, the fix might not be available soon. In the meantime, you can use Delete Face -> Heal to remove the artifact faces.

Many thanks!

[SEC_CAD]

Thanks @johnsonshiue but Delete Face deleted half of my model or refused to do anything regardless of which face of each artifact I selected.

I ended up creating extra sketches and extruding them to mask the faulty areas.

[SBix26 · Accepted solution]

Here's the Delete Face fix (Inventor 2021 file).  You just missed picking all the faces that needed to be deleted, eight of them altogether.

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Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
LinkedIn

[SEC_CAD]

Thanks @SBix26 I knew it had to be my fault.

BTW - I changed one of my dimensions by 0.5mm and the whole model fell apart.

I am now making a different approach and running into more Shell bugs. I have deleted the 'waist' and am now just trying to do a shell of a simpler shape. Inventor refuses for Wall=2.6 but is happy with Wall=2.0. I can't see the problem.

[ChrisDShaw · Accepted solution]

@SEC_CAD 

I can't say I have a solution to your specific issue but I know on the project I worked on last year I had issues with shell either failing to resolve or returning errors and artifacts. What I found is that the errors were cause where multiple (greater than 3) internal faces being created by the shell command intersected.

Looking at the model images you provided you may want to try creating you block with the side cuts. Shell that to your desired thickness then extrude your channel shape though the part. It's not an ideal solution but it should give you a clean part.

[johnsonshiue · Accepted solution]

Hi! Here is the solution with Delete Face. The artifact faces need to be deleted all together. Selecting those faces is indeed tricky. You can delete the face on the top first and then look inside the model. After that, delete the "Delete Face" feature.

Sorry! I did not notice Sam alread posted the Delete Face solution! Sorry for the duplication!

Many thanks!

[johnsonshiue]

Hi! I took a look at the second case. I think I know where the problem is. Like I mentioned, Shell and Offset are not good at handling topological change. For this case, the offset cylindrical face is going to touch the top planar face causing the edges to break into pieces. This is a condition that the Shell and Offset cannot handle at the moment.

Many thanks!

[SEC_CAD]

Thank you all for looking at this issue and for your feedback.

Thanks @SBix26 for the fixed model. I love @johnsonshiue trick of deleting the obscured face first to get access to the artifact faces, then deleting the delete.

This is such a simple part but I have been pulling it apart and rebuilding it for a couple of days! My final solution was to avoid the complex shell altogether and build it as two separate solids which get combined together, along the line of what @ChrisDShaw suggested.

I appreciate the community help 🙂

Cheers!