Healing an import from IGES

[robtheg]

I have an IGES file consisting of surfaces. After import, I sew those surfaces into a solid. Since the surfaces don't quite match up, problems develop later on. I want to manually/automatically edit those surfaces after import and before the sew but I can't find any way to do it.

The surfaces come in as Sheet Bodies and the sub-type on the Part Navigator classifies them as UNPARAMETERIZED_FEATUREs.

I've tried everything I know and couldn't find anything in the help files either. Increasing the modeling tolerance doesn't help. My natural inclination is to try to edit these as NURBS surfaces, but perhaps they aren't NURBS at all?

 

[uwam2ie]

New in UG?
Data translation is a complex subject. Is the geometrie in the source system a solid then move to step.-> Better results. What is the source cad system then I can give some how to's. Very complex faces? Analyse the geometrie after sew with analyse geometrie.
uw

 

[Xwheelguy]

uwam2ie,

Sounds more like new to modeling, not just UG

robtheg,

I believe you need to give a detailed description to the problems you're having 'later on' for anyone to accurately diagnose what the real problem might be. Are you having problems sewing? Are there large gaps between the surfaces? Have you tried untrimming and re-trimming the surfaces to the proper boundaries? Are you having continuity issues? Basically, your question is a bit vague & is kinda like going to the doctor and just saying "I don't feel good".

UNPARAMETERIZED FEATURE means there is NO HISTORY that you can use to modify it, like curves or sketches. For example, if you create a Through Curve Mesh feature, then copy it to another layer, the copy is unparameterized or dumb. However, if you have the correct licensing, you can use UG's wonderful editing tools to manipulate the surface in many different ways, or, with the correct licensing, you can utilize Shape Studio to manipulate the surfaces with X-Form, Deform, Translate, Refit, Rebuild & Match Edge.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[HellBent]

rob...there are some commands built into the standard surfacing package that can help you with those surfaces. The "Enlarge" command will allow you to increase the size of surfaces and then you could trim them together. Also, I do tons of 3d molds with imported IGES data. That means I need good sews in order to do all the trims involved in a mold (slides, lifters, pins, inserts, etc.) I've found that increasing the sew tolerance (not the modelling tolerance...but the tolerance right in the "Sew" command dialog) can eliminate most problems. Most times, if you do your sew and it passes the geometry checker (Analysis->Examine Geometry), you should be okay for future modelling operations. Play with that sew tolerance once and then check out how much of a difference that makes in the amount of errors you get with "Examine Geometry"...you'll be surprised. But like Tim said...if you work with a lot of imported data investing in the advanced surfacing licenses would be a wise choice, there are a lot of additional commands that will speed up your editing considerably.

Take care....

 

[robtheg]

Sorry for the delay in responding. Here's a more specific description of the problem.

The surfaces from the IGES file sew into a solid nicely, so I haven't needed to play with the tolerances yet.

I'm trying to make a simple fixture for the part. So I'm creating a block that encloses the part, then I subtract the part from the block. That all works fine.

Now, to create a proper fixture I then try to extrude the lower sufaces of the part upward through the material in a subtraction operation. This is where things start going wrong. I get an error when I select a certain face saying "Selected objects will result in a self intersection section". Playing with the tolerances in "modeling preferences" did not help.

The surfaces coming from the IGES import have gaps between them. I think this is the reason for the problem. NURBS modeling is not a problem for me but if I need the shape studio lisence then I'm hosed since my company doesn't have that at this time.

 

[cowski]

Rather than creating an extrude from sewn faces, try using offset face on your fixture part. Depending on how you were trying to extrude faces from the sewn solid this may give you the same results.

 

[HellBent]

I see what you're trying to do now rob. You just want a nest of "half" of the part...basically. Extruding faces can be hit or miss. Your end result is very similar to actually creating a mold. There are functions such as "offset face" or "thicken sheet" that can help if it's a simple shape. But if it's got any ribbing, bosses, fillets, or funky corners that create any tiny surfaces you probably won't have much luck with those commands. In such cases you'll almost always end up doing some surfacing to get it to work.

Assuming that your "nest" block is bigger than the part, I would recommend doing it like this...take that IGES data, seperate it into the upper and lower halves, and then create runout surfaces around it. Then sew the half together that you need along with the runout surfaces you just created and use that sewn surface as a trim sheet for the top of your block.

There are actually dozens of different ways to do this but without seeing the part this is all I can recommend. Depending on how big of an area of the part you're nesting there are other ways like just sewing the one side of the part together and then appying thickness to that surface followed by trims to define the sides of the block. But again..without seeing exactly what you've got to work with it's hard to say what way to go.

Take care...