need to send a customer a dumb model

[daiosama]

the company wants me to send our customer a model with no model/history tree.

They just want the model sent out.

Here is the problem.. I would send it as an iges, stp, neu, etc. but when I export the model and reimport, the models are not coming in solid.

These parts are extremely complex parts.

Any idea how to save these parts as Pro/E parts but without any editable model tree?

I am using wildfire 5.0

 

[design-engine]

Just send the model as a step and let them deal with it. If you think the customer will require a solid model then try it yourself first.

Export the STEP.
Create a new file using your standard start part.
import the step file into that new file.
See if it is solid or not.

If the file you export does not come in Solid then adjust your accuracy so the import part has the same accuracy that your part that your exporting has.
works every time!

Im going to southern GA and to Jennings FL (tracktime) and to Daytona FL for the Daytona 200 if anyone wants to meet up for beers? the fist two weeks of March.
Edited by: design-engine

 

[daiosama]

I tried doing the step thing numerous times trying different settings and still the re-importing is not working well. It would take me nearly a day to fix the model with the number of errors.


This model has nearly 1000 surfaces to it. and many are styled.

 

[tobbo]

i assume you are exporting is as a solid. (and not as a surface model)


do you have the possibility to import it in another cadsystem to see if you get the same result?


(or rather more, import it in a older version of pro/E)


Can IDD take care of the problems for you? One day of fixing doesn

 

[dgs]

Have you tried Shrinkwrap? If it's going to be re-imported into Pro/E, I'd use that or a neutral file.

 

[hauskey]

Another possibility is to create a 3D PDF.

 

[daiosama]

shrinkwrap - failed to generate the part
nuetral - same amount of errors as reimporting from stp, but different areas.

I have an old computer with wildfire 3.0 on it and it didn't do any better job reimporting.

and yes, it is being saved as a solid.

The problem is that the original "A Surface" data came from the studio of one of the automotive OEMs. And style data is typically garbage to begin with. So you clean the style data up the best you can to begin with, but it always seems to end in data translation errors.

 

[tomhartman]

what about an E-drawing?

 

[garymig]

try using .sat format?

 

[agarfiel]

I use this process whenever I need to create a dumb database:

1) Create a new part, this will be the database you send to the client.
2) Create an external copy geom of all solid surfaces from the old part. Make sure you un-check the "dependent" box under options.
3) Solidify the external copy geom.

This creates a dumb database that references all the geometry the original part, but doesn't fail if the original part is not included.

 

[michaelpaul]

save the parts as Edrawings and send them the edrawings files and a link to the edrawings viewer. they can see/spin/cross section all the parts. even assemblies.

there's a free edrawings publisher and a paid one. the free one will work if all you both want to do is view the files. it's much easier than trying to convert to a neutral format type. i've yet to have a problem with any edrawings data I've saved from right within pro-e

Edited by: michaelpaul

 

[kenppy]

I'll second the edrawing solution which I often use but if you have the professional version make sure to turn OFF the measure and stl creation if you don't want the data to be used without permission.

 

[proehelp.com]

Are you familiar with the import data doctor?

That problem occurs because your geometry is so complex. Then failures in the geometry occur when exporting it in a neutral format.
You can fix this problem with the import data doctor and "solidify" the surface again.
It's a very powerful tool. You will need very good surface handling skills.

 

[Indusign]

try saving a copy as PDFU3D, generates a 3D PDF file that can be opened with the PDF viewer, you can spin, zoom, isolate parts/sub-assemblies.

 

[miguelVR]

Maybe you can post one file here,


and we can try some things.

 

[krow72]

This will do what you want. Open the part file and go to file>mirror part. Choose mirror geometry only. This will save a mirror with no data. then file>mirror part of the mirrored part. This is the file that you will send to your customer. It is a workaround but works if you need to send a pro-e file without features.