Problem using shrinkwrap 1

[davidinindy]

Is it possible to shrinkwrap non-native assemblies? I have an engine assembly I put together from imported CATIA files. It's going into one of our designs, which is already a pretty large file.
Considering all we're interested in is the overall look and the mounting holes, etc. We could get rid of all of the internals.
I've tried numerous times to shrinkwrap this assembly, and it either freezes my computer, or just boots me out alltogether. My computer surpasses Pro/E's minimum requirements.
Any tips?

David

 

[jeff4136]

How are you trying to create it and what type? I don't know but suspect it might be more or less normal (suspect the process can be / is a resource guzzler).

 

[Hora]

I give you 2 hints:

1. (CATIA 5) If you are familliar with CATIA, then save your assembly as a part. (look under Tools menu. Then save your CATIA part as STEP. Import your STEP file in ProE as PART.

2. If you received the STEP file from outside, then delete or suppres all unwanted parts and save your assembly as IGES Solid file with FLTAT STATE option. This method works for me all the time and is more accurate than shrinkwrap. Then import back your IGES file as PART.

Good luck,

-Hora

 

[mloew]

Dave,

While this suggestion does not solve your exact problem, I would like to suggest that you use this opportunity to create what I call an "Interface Model". Create a single part that contains just the datum geometry for the interfaces. There are several advantages to doing this:

Light-weight representation of your system
Uses native Pro/E geoemtry (useful for making a print; uses all shown dimensions)
Good reference control (you can substitute the translated model without messing up dependant components)

Let me know if there is more interest, I can make a FAQ posting on this.


Best regards,

Matthew Ian Loew


Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[davidinindy]

I forgot to mention I'd searched thru the "knowledge base" and foud this to be a common problem, but they had no solutions or work-around listed.
The supplier exported these files from Catia. I got them as Pro/E files, so have no idea of what settings he used.
I'll definately try the 2nd suggestions of Hora's. A star for you in advance for such an in depth soggestion.

David

 

[Hora]

Thanks David. Do not forget to suppress al unwanted parts from the assembly file. It will help a lot!

Keep us informed how it worked.

-Hora

 

[davidinindy]

I gave up on shrinkwrapping it. It wants to remove surfaces from the outside of the parts, and is ust generally junk.
Hora, Where do you set that FLTAT STATE option? I click on options in the iges export, and it gives me a line to load a config file.
I have tried so many things to get this engine model manageable, but have succeeded only in setting a record for number of crashes in one day. LOL
I thought it was my system spec's, but another engineer here hasa system that is far superior to mine, an his crashes trying to do some of the same things.

David

 

[Hora]

David,

When you export to IGES you have several options.

The IGES export window has a group of check boxes called EXPORT (where you can choose Wireframe, Surfaces, Solids etc etc), a button called CUSTOMIZE LAYERS, and a combo box for Quilts, then a group for the COORDINATE SYSTEM a small button with an arrow and the combo box and at least the last group called FILE STRUCTURE with a combo box from where you can choose: FLAT, ONE LEVEl, ALL LEVELS, ALL PARTS.

This is what I have in ProE 2001 for assembly export. This method allways worked for me. As I told you, create a simplified representation and remove all unwanted components. If not, the export file will be huge. Then export this simplified rep to IGS (solid or surfaces) as FLAT.

Let me know if it works foe you.

-Hora

 

[davidinindy]

OK... We've struggled with this model and got a working machine that we're selling... now i'm trying to take my model and make a parts manual.
I've got a chassis group, engine group, etc...
I'm trying to create an exploded view of the engine and it's parts. Every time I move a part, I have to wait 5 minutes for it to regenerate. This is getting old. I've tried Geometry reps, and messed with trying to shrinkwrap the engine block and parts that are not necessary for the exploded view.
At this point if I export the engine as IGS, and reimport, I'll have to redo all my constraints... Very tedious...
If I set the shrinkwrap setting to 1, my geometry just dissappears. If I set it to 2, I get a waterpump that looks like a pyramid...
I've got a new computer that has much more memory and a better graphics card, and meets all of PTC's supported spec's.
Any other ideas?

David

 

[Hora]

David,
Keep the assembly in shade mode if you want to regen faster.Forget the wireframes when you have imported components.

The explode states I think only ProE can interpret them. Export option will fix the component to their original constraints. A better way is to move he components in assembly mode. See the following: thread554-155134.

-Hora

 

[davidinindy]

I figured out today that it's better to create your exploded state in the model mode, versus drawing mode... Works much better, and drawing regens faster.
Thanks

David