Different configuration in one file?

[loki3000]

Is it possible to make a part - a gear for example - that has two different configurations in one file:
-a simplified one with only the kinematic diameter (basically a simple cylinder) for the assembly and asm drawings (where full geometry is not needed)
-a fully featured model of the gear for the detailed drawing of the gear and perhaps assembly for rendering purposes

i would like to have both cfgs in one file, like the solidworks configurations option.
but ideally i would like to specify somehow which cfg to use in the drawing (can be done in swx)

 

[jagandeep]

Catia has design table functionality just like Solidworks configurations but with very limited functionality. If you use more than one instance of same part in assembly, you can't have different configuration for all of them i.e. they all will have same configuration. You need to save as part to get different config.
Google can help you

 

[KevinDeSmet]

Maybe this can help you out, you use this in the context of the Product in which you want to have your gear part be simplified in. It's definitely a bit of a hurdle and I'm not even sure if it'll work for your needs or not.

http://catiadoc.free.fr/online/pstug_C2/pstugbt0310.htm

As Jagan said, Design tables for this purpose are pa-the-tic as multiple instances with different configurations in a Product are not supported, like seriously!

 

[jagandeep]

Design Table Tutorial

http://catiacentral.com/catiav5tutorial/how-create-simple-design-table-catia

How to add part with design table to catalog

http://catiacentral.com/catiav5tutorial/how-catalogue-design-table-catia

 

[GELFS]

Hello Loki3000,

Each Instance of a Part or Product in an Assemply can have many Associated Representations.
The Default Representation is the representation as defined in the relevant CATPart.
All other representations shall be CATShapes.

I hope it helps.

-GEL

 

[loki3000]

yes, catshapes might be the answer.
is it possible to invoke a custom catshape in a drawing for example?

 

[GELFS]

Hi Loki3000,

I'm not sure what you mean by "invoke a custom catshape in a drawing".

If the question is,

"Which representation(s) will be used by the auto-created drawing of the assembly?"

then the answer is as follows:
1.The instance representation which will be used for the auto-creation of the drawing of an assembly is the active representation of the instance at the time of the creation.
2.This means that in the drawing file are stored reference(s) to the instance's active representation.
3.If you go back to the assembly and change active representation(s) the drawing will remain intact.

-GEL

 

[GELFS]

Some corrections/additions to my previous posts
Post of 10 Jun 13 17:03 Each Instance of a Part or Product in an Assemply can have many Associated Representations.
The Default Representation is the representation as defined in the relevant CATPart.
All other representations shall be CATShapes, Model, ... .
Post of 10 Jun 13 21:15

1.The instance representation which will be used for the auto-creation of the drawing of an assembly is the active representation of the instance at the time of the creation.
2.This means that in the drawing file are stored reference(s) to the instance's active representation file.
3.If you go back to the assembly and change active representation(s) the drawing will remain intact.



-GEL

Imposible is nothing