Copying Part Bodies to Another Part

[flangewiper]

Is there a way of copying a Part Body from one Part to another and taking all the associated geometry with it? I don't want to paste it with a link back to the old part and I dont want a dumb solid.

 

[solid7]

No, but here's a workaround...

File -> New From (select file you want to copy from)

1) Delete all unwanted solid bodies
2) Tools -> Delete useless elements
3) Everything that remains gets selected, copied and pasted


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[flangewiper]

That works OK if I want to copy the geometry into a new part but what about if I have a piece of solid geometry in one part (say a B surface rib or boss) that I want to put into another part that already contains a load of geometry. A power copy might work but I want to keep all of the geometry in exactly the same form as in the original part so it is fully parametric and can be modified if necessary.

I think I know what the answer is - use Hybrid Design. In this instance the solid and all the geometry associated to it are created in the same Part Body and can be copied and pasted into another Hybrid Part. But if you don't use Hybrid modelling and the solid's parent geometry is contained in a Geometric Set it doesn't work. CATIA doesn't seem able to gather all geometry together to enable a copy / paste operation unless thay are all in the same part body.

 

[solid7]

I laid the example out, as if you were going to put the geometry into a part already full of other geometry. The geometry being imported would still retain its geometrical set and part body info, so it's an ideal choice for a workaround, without having to do hybrid design.

If deleting all solid bodies, (except the one that you want to use) and running "delete useles elements" is too difficult, then I'm not sure that I understand what you're after.

It would be ideal if you could copy, with the same sort of logic that goes into moving elements between geometrical sets - i.e., the "move unshared parents" - but I don't think that's feasible for a non-hybrid design, as you've mentioned.

Good luck.


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Professional and reliable CAD design engineering services - Specializing in Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[flangewiper]

Sorry, I still don't get it. All File > New from seems to do is create a new part. If I have two parts, Part A contains the geometry I want to copy and part B is the part I want to copy to, what is the procedure? Maybe I'm just being thick but I can't seem to get it to work.

Thanks

 

[solid7]

Yes, it creates a new part. One that you can tear apart, risk-free. You keep only the info that you want before copying and pasting it where you want it.

Again - with the new part, delete ONLY the solids that you don't want, and then run the "delete useless elements" command. Whatever is left, move into one geometrical set, if necessary.

Finally, copy and paste whatever is left. It will be logically organized, and you don't have to lose it in the mess of the rest of the tree.


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Professional and reliable CAD design engineering services - Specializing in Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[catiajim]

If you know what the wireframe parents are of your Body, simply place that Geometric Set into the Part Body itself (right click on the Geometric Set, Geoemtric Set.Object, Change Geometric Set). Now you can copy/paste your Body into the other CATPart.

 

[flangewiper]

Works now - thanks folks.