IGES

I read the IGES postings in here ( so you know)

I made a model of my SAE formula car in Solid Works and I want to test in
FEA in mechanica because thats the only student pakage I got. So the only
way to import is by saving as Pro/e part or IGES in solidworks and then
importing IGES or opening part in Pro/e. But when I run MEchanica and I put
my loads and constraints, the test says that the load and constraints are
not part of the model. Then I check and only a few of the tubes that compose
the frame are actually solid. the rest of the model import looks solid but
its not. has anyone found a solution to this? Is there a free translator
I can download?

fonss

 

What do you mean it's not solid? When you imported did some of the surface
boundaries get messed up and you got surfaces rather that a solid?

If this is the case you just need to redefine the import and clean up the
boundaries. Then change the attributes in the redefine to make is solid.

Or try saving it as a step file.

 

What release of Pro/E? In Wildfire I've found that you click on the
Imported feature in the tree, click Redefine, a Geometry menu shows up.
Click on Heal geometry, all surfaces, Compute, Accept (Ignore the next
totally misleading message) and go to Feature Attributes and click Make
Solid on the window that pops up. How'd I do? All from memory might be
slightly off.I think this functionality is something called import data
doctor?

I assume you don't have standalone Mechanica do you? There you could
fiddle with the Import Settings. I've never got STEP to work directly
into Independent Mechanica. has anyone else? Into Pro works very well...
but I still think I've had to do the above.

Oh, if it's not obvious if something is solid you can Do Model Analysis
and try to get a volume. Oh sorry, that might have been obvious.

-Dan

 

yeah you are right, its similar in 2001 and it also works in student
edition. John Morrison helped me with the problem by email, here is the
solution:

I think I have the fix for you.

Here it is step by step:

1. Feature redefine and select the import feature out of the model tree
2. The hit Heal Geometry and select manual
3. Next select Zip Gaps
4. Then select Auto Select
5. Last hit Zip Gaps and done.

This should give you a good solid to work with. I did it and it gave me
one. Just a hint: If you unshade your model and the edges are purple then
it's not solid. The yellow edges are the ones that have the problems. I
will attach my Pro E file and hopefully it will work for you, but go ahead
and try to fix your model first.

I also found that in solid works you don't always have just one solid.
sometimes making extrusions if you don't select "merge" it will create
another solid. A simple solid will translate to Pro/e with no need to fix
it but a complicated geometry with rounds etc will need some fixing. I don't
have the stand alone mechanica. A simple ofject created in solidworks and
translated into pro/e will be able to be analysed by FEA in mechanica.
Complicated geometry will require fixing no matter where it came from. In
the standalone mechanica one can fix the mesh but in this one if the autogem
doesn't like the geometry, you need to redifine it or use idealizetions to
simplify so it doesn't need a mesh where the problem is. I hate mechanica
student edit but its the only thing I have...



fonss

 

: I read the IGES postings in here ( so you know)
:
<snip>
: Then I check and only a few of the tubes that compose
: the frame are actually solid. the rest of the model import looks solid but
: its not.

As a general rule, for export to iges or step, you need to make sure part accuracy
is set high enough. Your thin walled tubing (small wall thickness, long tubes), is
precisely the kind of circumstance where accuracy values come into play,
particularly when exporting or doing merge intersects to create mold cavities or
in making manufacturing models. The accuracy bug may also bite you for parts that
are thin shells with large, overall dimension or in sheetmetal where the large
size of the part contrasts with the thinness of the sheet thickness or in
composite laminations.

BTW, accuracy is probably set at a default value of .0012 in your start part. You
can modify this value for each part with 'Edit>Setup>Accuracy'. If you haved
Absolute accuracy enabled, you will see both Relative and Absolute accuracy in
this menu. If you select Relative accuracy, the message line will tell you what it
is currently set at. But, for export/import functions, set the absolute accuracy
value to at least .002. The smallest setting will allow calculating decimal values
to their true precision.

Regarding 'Heal geometry', I have run into circumstances, like yours ~ exported
solid, turned out as a mixture of surface and solid, even features missing ~ tried
to zip gaps, but it told me there was nothing wrong. When I reset part accuracy,
zip gaps was then able to find the problems and it automatically regenerated to
solid. In another recent case, I exported to iges surface quilt, imported it as a
feature and tried to create a solid from it. It wouldn't even recognize the quilt
for 'Edit>Solidify' until I changed part accuracy. Then, no problem, the
'Solidify' menu is available and creates the solid, as you'd expect, flawlessly.

A lot is riding on that part accuracy setting, especially for exports. Changing it
will often fix problems before they appear in the iges. If you'd like to prevent
accuracy problems from cropping up in this manner, change the start part so
accuracy has a smaller decimal value.

David Janes