Remove Body from CATPart in a drawing view? 1

[Runz]

I have a CATPart with 2 bodies. I want to create a drawing view with only one of the bodies active (Shown). How is this done.

Thanks,

 

[Albigger]

when first placing your view, instead of just clicking on the projection plane, first highlight the body you want shown in the drawing in the tree, then select the view projection plane.


If you already have a view, while in drafting select the view and go to edit modify links and switch to the 3d part, then select the body you want, then switch back to drafting and choose "add all." then update.

 

[jimicatia]

just deactivate the body to not to show on the drawing.

 

[Albigger]

If you're going to do that you could just hide the body (put it in no-show space) and it won't show up on the drawings. That's how I drafted for a while, but I find the way in my previous post to be much easier when having to update drawings.

 

[solid7]

just deactivate the body to not to show on the drawing.

That's a very poor way to work. It's unacceptable in most any respectable design department. Aside from that, it's not practical, as deactivating a part simply for a drawing, means that you also don't get to use it anywhere else. Unless, of course, you choose not to update your drawing, which is an equally poor solution.

The best way to overcome this problem, appears to be to use assembly structure, instead of multi-body parts, so that you have the Overload Properties available. I do realize that this is not an option for everyone, but it solves the problem instantly. Even if you choose to use fixed constraints on all your parts, (while positioning in assembly coordinates) it would be better than this multi-part body mess...

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[snowfire]

You are right. But, many times I do need a multi-body part. Something like a wire, it deformed in the assembly, but in drawing it is flat. And one part can't have two part No. If CATIA has the overload founction for bodies, it will be great. Many problem from flexible parts will be solved.

Forever Young

 

[solid7]

I haven't used layering in V5. Is this an option (with filters) for Multi-PartBodies? Anyone?

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Catia Design|Catia Design News|Catia V5 blog

 

[itsmyjob]

I cannot apply a filter to a view like in V4. So the best solution is the link modification.

I would like to use filters/layers in V5 but you really have to define the methodology first. And we have some many files without layers now...

Eric N.
indocti discant et ament meminisse periti ​

 

[catiajim]

We use two parts for deformable parts. The detail, which is the Master, carries the actual part number. The other part is a Bogus Part Number, and it is related to the assembly part number, shows the deformed shape. This way, we can account for parts with multiple next assemblies (multiple bogus part numbers) and multiple deformed shapes.

 

[itsmyjob]

like Jim, we use VPM.

And multi-use partnumber is our solution.

Eric N.
indocti discant et ament meminisse periti ​

 

[snowfire]

It may be a solution. But, when I assemble a spring into an assembly, there are 5 instances, and each instances has different deformation. when the assembly changed ,the spring should change accordingly. The spring is one part, just too hard to do such things in CATIA.

Forever Young

 

[catiajim]

That's where we use the bogus part number at the assembly level - we put each of the 5 deformed shapes into that CATPart (yes, we use a multi-body part here - it's the only time we allow it).

 

[jackk]

Every company has their own methodologies.

For springs and other flexible parts, we make different CATParts, but store them in PM with different suffix (PN1234-3D1, PN1234-3D2, PN1234-3D3, etc)

We try to avoid multi-body parts, but one of our exceptions is molded parts with inserts. I just designed a plastic fan that has a metal hub. Another exception is over-overmolded plastic/rubber housings.