Making a stp file into a solid

[boydt]

A customer of ours has sent a stp file of a gearbox housing, (pretty complex). I can open it but it gives the error of overlapping geometry. Then I cannot solidify it so I can modify it. Any ideas?

 

[AHA-D]

Open it as an assembly so that the individual parts are kept and created as PRT separately. STEP "knows" about solids, parts and assemblies.


Alex

 

[design-engine]

I first make a copy of the file into a separate folder and read it into Microsoft word. There is a header file... I like to see what software it is written from. Often times that file was exported from Pro/ENGINEER and if you have customer contact you can often as for the native geometry.

Design engine has often received complex geometry like a gear box. First the customer wants to create a solid then create an STL file. In WF 3.0 users have quite a bit of flexibility for riping apart that iges or step data and rebuilding it. although this method often requires surfacing expertise the method is strait forward no matter what the complexity is of the part. Simple steps to delete ... rebuild either inside import functions or outside using Pro/SURFACE

First determine the problem. Attack the problem by either delieting and rebuilding the surface or by zipping gaps

If you continue having problems consider hiering someone or empower yourself by taking this class I designed. [url]http://www.proetools.com/courses/pro_surface/advanced_import .htm[/url]

 

[boydt]

I would love to attend one of your surface classes. But I doubt I could ever get my boss to let me go

Just getting back to this again. I was on the phone with our customer just now. They are using UG. What is the best format to output from UG to put into PRO? I have tried a step and igs but neither work well. The most recent I tried was a step and it looks really good but I cannot use it, I cannot solidy it. I am trying to use there part and casting models to build a process model from. Any ideas????

 

[jimshaw]

step and iges are standardized languages, so for translation it's not going to get much better. The problem, I believe,is the source geometry. Make sure they highlight all solids prior to export, to ensure you get as much data as possible. As far as poor modeling practice in the source data, welcome to the world of CAD, where "nobody is as good as you are"


Not being able to solidify surfaces in ProE means that you do not have a perfectly enclosed volume bound by surfaces. This could be due to either gaps or overlaps, and it just takes time and patience to investigate and heal... Could you provide a screenshot?

 

[design-engine]

Those big aluminum housings are the hardest.

I should say before I start a big iges repair job I always make a backup of the original file to see where the file came from.

1. backup
2. read into Microsoft word (to see the header) to determine where the file originated from. The darn thing was probably exported from Pro/E (that happened to me 50 percent of the time)
3. then I try IGES first (because it is usually not the perfect) then try STEP (better usually) just to look at how the geometry comes in.

Then there is a whole process for systematically squashing each bug (as I typically say)


I just read my other post of almost the same thing. And I can't delete this post. Any admins on here? Fix that hu?


Edited by: design-engine

 

[boydt]

My customer spent a lot of time trying things on his end and still the result is the same. I finally went to PTC for help on this one. They told me the same thing you guys are saying about voids in the surfaces. This is one of them things where in the back of my head I knew this was more than likely the problem but I just didn't want to deal with it

PTCsent me a suggested technique to help me fix this. I looked the model over for a few minutes yesterday and could not see any obvious voids. When I get back to it I guess I will have to turn out the lights and put on my 100X magnifying glasses and examine every square millimeter of it. Re-modeling is starting to sound better.


Thanks guys

 

[magneplanar]

it is possible to tune the step file for export and there are different levels like ap214, ap203

"AP203 applies to representations of mechanical parts and assemblies.
AP214 applies to representations of data relating to automotive design.
Present day AP203 files typically contains the boundary representation
model, assembly data, and a limited amount of other product information.
AP214 files typically contain colors, layers, and generic resources."

 

[magneplanar]

here is a useful link for setting up the export/import between softwares:

this link leads to recommendations for IDEAS to pro-e

[url]http://www.prostep.org/en/services/bp/cadkombi/ideasproengin eer.htm[/url]

cheers,

M

 

[foolmankh]

I used to re-model from stp, it's hard word but it's worth. It helped me to increaseskill and work effectively.


Good Luck with it bro

 

[tommypurple2]

Step model is the best format to get a UG file into Pro E.....


I use pre WF colors (fix all the yellow geometry by edit definition the imported feature. Heal all the problems using edit boundry and zipping gaps.


If you can not find any issues on your model and it says it is not closed try to copy all surfaces and then paste them. it should crash out saying that there is a problem with the geometry. If you then investigate your model it will highlight the problem for you.

 

[JustinHager]

Exporting STEP files from SolidWorks 2010 for Use in Pro-Engineer program.

Problem:

I am a SolidWorks User and I found that when I export large files to FTP to customers, some of them with ProE are not able to use the cut tool to modify our container.
I found that, with the help of you nice people, my model was comeing in with ALL surfaces.

Proposed Solution/Somthing to try:

I had a check box in the properties menue that says "Split Periodic Faces" usually this is checked. Usually I get a broken body of just surfaces. When Un-Checked, I get bodies that don't need to be knitted together or anything.

Hope this helps