"Heal" surface to make a part solid geometry

Lucas_Kuhns

I imported a STEP file from a potential customer and one "part" showed up as a surface in the part studio. Upon further inspection, I realized that it is missing a face. This may be the incorrect term but how would I "heal" that surface and convert this part to solid geometry?

S1mon

If it's just a rectangular face that's missing, probably the fastest is either:

1. Loft a surface from one edge to the opposite edge, using add / merge with all
2. Right click - Select / Select loop/chain connected edges, then select the Fill tool, add / merge with all

You could also set up a sketch plane (or use an implicit mate connector) and sketch the outline of the missing face (using "use edge"). Then create an offset surface selecting the sketch face with and offset of zero. Then you'll need to boolean the two surface bodies together which should create a solid.

Lucas_Kuhns

Thank you for your help. I was able to use the Fill tool to get the missing face. However, the boolean tool isn't doing anything for me to make it a solid part. Using Fill with new surface plus the boolean joint yields the same result as just using Fill with add / merge.

The screenshot below is with a section view applied. It's still just a hollow shell. The Enclose tool wasn't working either for some reason. The error message was "Enclose 1 did not regenerate properly: Selections do not enclose a region." I have all surfaces selected though and pretty sure there are no gaps.


Now I just realized I can get it to work by using Thicken on the inside surfaces or the outside surfaces. This is a lucky break that the part is sheet metal design so that "works" but I still feel like I'm just missing something super obvious and simple. I'm clearly not a surfacing modeler!

Lucas_Kuhns

Nevermind! There was one more missing face. So two Fill (add / merge with all) was all that was needed.

MichaelPascoe

There is a view option for "Highlight boundary edges", this will help you identify those open edges.

Lucas_Kuhns

Wow, thank you! I never saw that there. I've been doing CAD for 10 years but when it comes to this surfacing, I feel like it's my first week.

EvanReese

Also relevant is my Cap Surface feature. All it does is pick any open edges of a surface body, and try to use Fill on them. You can only choose one continuity type per feature, so it can be limited, but for many things like this it's a nice quick way without having to find and pick edges manually.

S1mon

One warning. Sometimes when things fail to import correctly, not only are they missing a face or two, but the open edges may not be coplanar as far as Onshape is concerned. Loft, Fill or Cap surface may be happy to create something which closes the hole up, but it can be possible for it to be distorted. Depending on what you need to do with your model this can be a big pain. There are ways of cleaning up these problems, but just be careful. 

EvanReese

Sounds like you've earned some wisdom the hard way here. I hadn't thought of that. I could probably make the feature show planar faces as green and non-planar as some other color without too much trouble.