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

 

The problem is that when I do a cross section view (it's an airplane

Please submit an enhancement request. It counts sort of like a vote for
this enhancement.

 

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?

 

Thanks, but I tried this and it won't work. For whatever reason, it

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.

 

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.

 

So, basically, I'm going to have to find a way to solve all of these

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.

 

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.

TOP

 

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?

 

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.

 

I left Heal All on overnight and it fixed a few gaps, leaving 213

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.

 

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"

 

I was about to suggest that. It is also frequently the fastest way to deal
with imported autocad files.

 

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.