How do you create parametric parts from IGES.asm file?

[wookie]

Hi,

Does anyone know how to create normal parmaetric part files from an IGES assembly file.
I am currently using ProE 2000i2 and have just recieved this IGES file which contains a full assembly for me to work on.
However, although the assembly is made up of different parts, the features on each part are not accessible. This creates a problem because i cannot redefine the part features or even view the dimensions.

Please, if anyone knows how to get around this, it would be much appreciated.

Cheers

 

[looslib]

Remodel the parts from the existing design.

There is no translator that maintains parametrics, unless you have a custom translator that reads one format and recreates the parametric part in the new format.




Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[wookie]

The assembly is quite complicated and has a number of parts with lots of features.
Without defned dimensions, is it best just to use Anlysis-Measure-tools to gain the required dimensions??

Surely there must be a better way to do this?

Does this mean that IGES files are for 'read/view-only'??

Can you suggest another format for file transfer that will not lose information?

Cheers for your help.

 

[Hora]

No, they are not read-only. You can add features after importing. But you cannot have access to their historical data.

-Hora

 

[wookie]

Sorry guys, but what is the point of IGES files then!!??

I can't believe i'm gonna have to remodel the whole assmebly from scratch.

Having the ability to add features and redesign the existing assembly is good, but if days have to be spent on remodelling original data, then that just seems like timewasting!

Sorry for blowing off steam, but i'm not looking forward to this!!

 

[im4cad]

If you have an IGES for the whole assembly and you want to create parts from it, you can do it, and you'll be able to use the existing geometry as it is, without having the possibility to redefine the shape of the existing surfaces, but you have to have the "Import Data Doctor" module.

Try this for creating one of your part:

Feature --> Redefine --> Select the IGES file -->Heal Geometry --> Delete --> Uncheck everything except "Surface" (if you want to keep surfaces)--> Select item --> Select all the surfaces you want to delete --> Done Sel --> Done --> Done/Return

Now you have just the surfaces that you need for one of your parts, and can do it again, and again for all of them, but you have to create copies of your initial IGES file for any of the parts you need.
This way you can create your parts with minimum work by using the existing geometry instead of starting from scratch.
I hope this is useful for you. Now relax and enjoy your creation

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[wookie]

Thanks mate, i'll give that a go!

Cheers

 

[im4cad]

Ooooops, I figured out too late that you're using 2000i2, and I gave you directions for 2001. I hope there's no problem for you.

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[peglor]

One handy method of getting a lot of dimensions out of an imported IGES file is to open the file into a drawing and start adding dimensions there instead of using the measure function. It also gives a handy printable version of the drawing to work from if you have to draw the model as a native ProE file.

The handiest method I've used for this is to have two people working on the drawing, one using the measure and drawing mode to get dimensions from the IGES file for each feature and the other to create the features. Works well if you've got the facilities.

The main reason for exporting files is so that data can be sent from ProE to FEA/CFD/Manufacturing packages for further processing. Preserving the parametric behavior between packages usually isn't possible because different packages use different methods to create their features.