IGES

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

John Morris> What do you mean it's not solid? When you imported did some of the surface

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

: 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