Creating solid from surfaces

chris_campbell957

I imported an airplane model (.stp file) from OpenVSP which resulted in a huge bunch of surfaces and no solids. I found that in many cases I could boolean union the surfaces together and they became solid parts. Some of the airfoil parts needed to have a face added to close them off, which I was able to do by lofting one side of the airfoil to the other.

Unfortunately the main wing stubbornly refuses to be boolean unioned into a single part like the others. The outboard sections do actually union ok, but I have now spent many hours trying to do the same for the central sections, and am starting to lose my sanity. They are nothing more than two surfaces, and I want to close the ends off and make a solid - seems like it ought to be no more than a few seconds work...


Here's what I have tried, this turned out to be more like an exercise in discovering every possible error message:

1. Loft between end of top surface and bottom surface -> boolean operation failed to return a valid part

2. Fill between end of top surface and bottom surface -> cannot add surface to existing geometry

3. Enclose between top and bottom surfaces -> selections do not enclose a region

4. Boolean union of top and bottom surface -> ok

5. Loft between top and bottom of 4. -> could not create loft with given information. Check profile order, intersections or end conditions

6. Fill between top and bottom of 4. -> boolean resulted in no geometry change. The parts do not intersect or are totally contained.

7. Boolean union with outboard wing section -> cannot use a mix of solids and surfaces

For the 1. case, I get this confusing display with some other surface showing up that I didn't select:

Lofting between the surfaces at the outer end (furthest from where the planes are showing) does actually work, but that's not enough to complete a part and the exact same procedure fails to create a face on the other end. In case it wasn't obvious I'm new to Onshape so I must be missing something simple. At this point I've still spent more time watching tutorials than actually using the program myself, and about 80% of my time so far has been bashing my head on this one problem. Any tips would be helpful.

https://cad.onshape.com/documents/615e16a00e387f4b68c0c40b/w/84d00c341c6bf2883c775f69/e/e75aec7956928c98de4cc84b

mahir

I'm not sure what you're doing wrong, but I had no problem adding two Fills and an Enclose.

https://cad.onshape.com/documents/12e1ababe3f08f11d7dee4e8/w/ff93dc72c736a43e6f7fc05b/e/fcc75bd6eedc8e6c4bb23808

chris_campbell957

Thanks for taking a look mahir. I can fill one end but not the other.

I made a video just in case there's something about my procedure that I'm doing wrong:
https://youtu.be/lnWiFjFnc6Y

fwiw I'm using Chrome on Linux (version 96.0.4664.110)

mahir

That's weird. I don't have any issues with the second Fill and am doing it the same exact way. The only difference is I'm using Chrome on Win10 vs Linux. Might be time to submit a bug or support request. 

The only other thing I can think of is to uncheck "Merge with all", and then only select the visible surfaces to merge with. Again, I didn't have to do this, but it's worth a try.

billy2

You need to keep track of solid vs. surface. Watch the folders parts & surfaces and look for parts vs. surfaces. There's not a good indicator saying your manifold is surfaces or solids. Enclose is the operation that takes surfaces and evaluates them to solids. All other operations to solids is automatic making things confusing. The last fill surface operation will result in a solid automatically. I've already put in a IR to stop automatic conversion to solids.

Us guys that are surfacers want to stay surfacing.

For now, watch the folders to see what state your geometry is in. Remember that in OS you can add fillets to laminated (knitted) (whatever we call them now) surfaces. It's really hard to know if your geometry is a solid manifold or a surface manifold. 

chris_campbell957

I tried this again yesterday and I was able to fill the face on both ends, as long as I selected 'New' instead of 'Add'. Coulda sworn I already tried that many times in my first session, but I suppose it's possible that I didn't. Having the default 'add' option work on one end but not the other is kinda confusing and I'm still not sure why that should be the case, or why that extra un-selected surface showed up in red.

billy2

@chris_campbell957 I've opened your document and danced through your tree.


Please organize your work into folders. It's nicer for the next guy to enter into something organized versus stepping through a model one feature at a time.


This was the 1st thing that caught my attention feeling this should be a fill verses a loft:



I think this is a problem and I wouldn't do this in my design:


Loft 7 has 2 edges with 3rd & 4th being 0 length. It's amazing they (OS or parasolids) got this to work, it didn't use to be acceptable. Even though they have if working, I'd stay away from this type of stuff.

This imported geometry is fairly simple but it could have errors. Solids are evaluations and have tolerances. I think this model is dancing in/out of acceptable tolerances. If OS allowed an adjustment on tolerance you could dial things down and get this model working better. I find that boolean union is more forgiving than the add when creating multiple surfaces but it's dangerous to union when add didn't work.

When I'm modeling, I'm insuring that everything is clean and stable because when I ask OS to solidify, I don't want it think about it. I think you have a lot things that barely work in this model and at the end, it's a house of cards.

Loft 1 looks flat but you can't create a sketch on it. It's non-planer but it looks like it might be. It did solidify in boolean 7, but that scares me.

If this was a production part, I'd investigate everything.

Where'd your import geometry come from?