Surface to Solid? + Section View

Hello,
After importing my model (with help from you guys) from 3D Studio Max to SolidWorks, SolidWorks has imported 109 Solid Features and 49
Surfaces. Everything looks great.
The problem is that when I do a cross section view (it's an airplane and I need to see the interior), while it's letting me set up the cross section, I can see through everything. However, when I click the green checkmark, only the solids get cut in half and the surfaces are no cut, so I can't see the interior of the airplane through the fuselage surface. Is there any way to change the section view settings so that section view cuts through everything like it does in the preview?
Barring that, is there an easy way to convert surfaces to very thin solids? I can do an offset surface which makes another surface very close to the other, so it seems like it shouldn't be a big deal to fill in this gap between them. I have tried a few things, anybody know if this is possible?
Thanks again for all the help,
Kevin
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Look in the help files for `thicken'. You should be able to thicken surfaces that are causing you problems. Sounds like you will need to uncheck the box that says: merge result.
Good Luck, jk
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On Jun 18, 11:21 am, "John Kreutzberger"

Thanks, but I tried this and it won't work. For whatever reason, it just says "unable to thicken surface". I've tried unchecking the merge box, checking the merge box, thickening very large or very small amounts, changing thicken direction, and tried this on multiple of the Imported Surfaces, and I get just this same error message every time.
Also, how do I submit an enhancement request? On SolidWorks.com forums?
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This usually means that your surface has a curvature somewhere less than the thickness offset value. This would create a self intersection of the surface on thickening. This is usually caused by a surfacing problem in creation or translation that is giving you a kink in the surface.
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Since this is imported geometry, there may be some faulty bodies. Have you used tools/check or import diagnosis?
Enhancement requests are submitted via a form on the subscription services web site. Go to solidworks.com and start looking under technical support. You'll have to get logged into the "customer portal", but there are also a lot of other useful things in there.
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I just ran this and have 192 faulty faces and 42 gaps. Am running the heal all feature.
So, basically, I'm going to have to find a way to solve all of these problems before being able to convert to solids? I am really fairly new to solidworks and CAD in general, so I'm not looking forward to having to delete faces, insert new ones, knit, and so forth. I am an intern and have to turn a 3D Studio Max model of a whole airplane into a usable solidworks model. I was hoping that everything would just kind of work, but I guess this won't be the case.
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Unfortunately, you may indeed have a grim job ahead of you. If I remember correctly, Max uses faceted models, and SW uses BREP models. This is a much bigger difference than just different file formats.
If you have alternate paths to importing the model (different formats, etc.) you might try those to see if you get fewer errors. The guys who actually use Max (not me) might be able to chime in with more advice.
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I left Heal All on overnight and it fixed a few gaps, leaving 213 faulty faces and 19 gaps. I know what I'll be doing for the next week! Quick question though: I am dealing with an imported STL. As soon as I do anything to repair the faulty faces, like delete one and make a new face that doesn't intersect my solid, the option to go back to Import Diagonostic is grayed out. This is stupid since there is no way I can remember where all 213 faulty faces are. Please tell me there is a way around this?
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just a comment from the peanut gallery ...
one option, import to 2 different files. one part for reference, one part for repairing. create an assembly with both parts, let the fun begin.
what'd you expect, a miracle "fix it" button. ;)
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Import diagnostics is only available if an imported body is the only thing in the feature manager tree. I've had some trouble besides that, even. I don't like it either.
We have to get by using tools, check after we start making features. It's not the same tool, but it can serve some of the same purposes.
You might try exporting and re-importing a Parasolid file to strip your new features out of the tree and get back to import diagnostics. Sometimes I've had better results saving in other formats as well. The different formats sort of filter the geometry. You might even experiment with saving out individual bodies to work on, then bring them all back into one file. I've never explored that myself, but it's an idea that may save some processing time.
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I think the best you can do with an imported STL file is to use it as a scaffold to build your own part around. STL files are all triangular faces. Even if you manage to get it nicely healed up into a solid or clean surfaces, it will still just be a collection of triangles.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
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I was about to suggest that. It is also frequently the fastest way to deal with imported autocad files.
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On Tue, 19 Jun 2007 08:56:18 -0700, snipped-for-privacy@saic.com wrote:

You're going to want a product like Geomagic Studio that is specifically for reverse engineering. Max uses polygonal models for the most part. (Yes they do NURBS too but we'll be nice and not talk about it).
http://www.geomagic.com/en/products/studio /
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Thanks for this...
What ended up happening was I fixed the model manually over about 5 full days of work. In the 3D studio max model, a lot of the features were overlapping (ie someone took a cylinder and just shoved it into a wall and didn't delete the part of the cylinder inside the wall), so solidworks had a really hard time making coherent surfaces out of everything. To solve this problem (SW recognized 100 solids and 40 busted surfaces), I would take the cylinder, drag it out of the wall by exactly 1000 inches, fix it up using tools->check and figuring out what was wrong, and then moving it back to exactly where it was after I fixed the problems, knitted it, and thickened into a solid.
Then, my supervisor decided that he didn't like all the triangles, so I basically ended up remodeling the whole thing with surfaces using the triangles as a skeleton, as suggested above.
I've learned a ton about solidworks and thank you very much for all your help.
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On 19-Jun-2007, snipped-for-privacy@saic.com wrote:

I had a similar problem with IGES imports of some complex vehicle body panels. I needed to use them in an assembly, but not being able to thicken made it tricky. Like you I had faulty faces and gaps and could not heal the problems.
Further to another thread on this newsgroup, I downloaded the evaluation of Rhino 3D, imported the IGES into Rhino, saved it as Rhino format, then imported that into SW.
I was then immediately able to knit all edges, and thicken the model, something I could not do in SW. Absolute accuracy was not required, so I can't say if this looses some model info.
YMMV
--
Greyhound

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Please submit an enhancement request. It counts sort of like a vote for this enhancement.
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The section tool does not recognize surface bodies. You have two options. One is to leave the surfaces surfaces and trim them back using a planar surface coplanar with your section plane. The other alternative is to knit them into solids.
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