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Fill a hollow object
andrea_6
Member Posts: 7 ✭✭
Hello. I have an object with a hole inside. I want to make it solid, how can I fill hidden holes?
0
Best Answer
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NeilCooke
Moderator, Onshape Employees Posts: 5,875 
Trust you @philip_thomas to think of that!
Wouldn't it be quicker to make a big cube, subtract the part from the cube (keep tools), delete the cube, then union the original part with the leftovers?
Senior Director, Technical Services, EMEA7
Answers
I recommend trying our Delete Face tool. More info here: https://cad.onshape.com/help/Content/deleteface.htm
Depending on the complexity of your model, you should be able to use that tool, select all the internal faces, and the model will fill.
If you make your document public and include a link to it here, we may be able to help more.
-Noa
Lets say your part is called Part1
1) Generate a cube around your part (Part2)
2) Use Transform/copy to make an identical cube (Part3)
3) Boolean subtract Part1 from Part2 (keeping tools)
4) Hide Part1 Part2 Part3
5) Delete all other bodies (these are the voids)
6) Show Part1 Part2 Part3
7) Boolean subtract Part2 from Part3 (you now have an exact copy of the original part (minus the voids)
8) Optional - this step preserves the original body ID - use this step if Part1 has been derived somewhere else or used in an assembly. Boolean union Part1 and Part2 (make sure you select Part1 first).
This process is very repeatable and works for any number of voids. Because the steps are always the same, it would lend itself very well to a custom feature (FeatureScript).
I hope this helps
Wouldn't it be quicker to make a big cube, subtract the part from the cube (keep tools), delete the cube, then union the original part with the leftovers?
I also had issues with voids.
I slowly realized this after my 3D printer slicer (Cura) was simulating some very strange wall geometry that I could not resolve in the slicer settings.
I was about to finish with Neil & philip_thomas' solutions using the Boolean feature. That's when I noticed the negative space wasn't producing additional parts to union with.
I thought the boolean operation must have filtered out this small void because of a small feature limit or something, or because it treated it as a gap rather than OP's voids. This would have been easy to just re-create the part with a final boolean operation.
Then I realized my mistake.
The voids originally came from a sketch profile for a revolve feature closing itself at 0mm from the curved sidewall. For whatever reason, this wasn't perfect (the plane might not have been orthogonal to the wall) and was the source of my issue. I resolved this by offsetting the closed surface into the wall of the part with an offset from an internal wall. This completely solved my issue, and I no longer needed a workaround.
In other words, good design practices help avoid issues.