Maintaining Location Reference during Copy and Paste. 1

[spartan2674]

Hello,

I have a engine part in CATIA which is located at some distance from the origin. I make a surface extract of the part (using the create datum element option). I then copy this surface extract and paste it in another CATPart file. It automatically locates itself at the origin in the destination file. I even tried Paste Special with as Result and as Result with Link and also as as Specified in Part Document but in vain. How can I paste it in such a way that it maintains its original position as in the engine ?

 

[weavedreamer]

Is the part inside of a product? If so, the copy/paste is picking up the surface relationship to the part origin from which it is copied. You could generate a catpart from product to do your copy/paste from, if this is the case.

 

[spartan2674]

Hello weavedreamer, thanks for your reply. The engine part is a CATPart file which lies in a huge product file. Each part in there has its own coordinate system. I hope this is what you asked in your post.

Could you elaborate on the generating a catpart from product ?

 

[weavedreamer]

Use the 'Generate CatPart from Product . . .' from the 'Tools' pulldown. Select the part containing the reference origin you desire along with your engine part. You should then be able to do extract the desired geometry from the volumated solid and execute your Copy/Paste from within the newly generated CatPart.

 

[solid7]

If I understand correctly, you want to be able to extract something from the rest of the model, and have it placed relative to the detail part, as it is located in the assembly, correct?

If so, you can just double click on the part you want to make the reference in. (make it your in-work part) Then, from the assembly, choose the feature that you want to duplicate, and extract, dissasemble, etc. If it's a solid, a dumb representation will be created, along with any specific features that you asked for.

Now, I'm not testing this at the moment, so I'm wandering off into speculation here - but in order for what I've described to work, and if I remember correctly - I believe that you have to set up the following option:

Tools -> Options -> Infrastructure -> Part Infrastructure -> External References -> Use Root Context In Assembly (should be checked, I believe)

Again, not sure of that, but please let me know how it works. On a daily basis, I duplicate parts and features from assembly locations into part workspaces, and this works for me.

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[spartan2674]

Thank you weavedreamer and solid7 for your tips. The generation of CATPart from Product seems to work for now. But there is another problem. When I use this option for some parts, I get the following message....

Incident Report:

The Part xxxxx is not updated. The result is not safe : Features in xxxxx may be not present or wrong, some
attributes may be lost or wrong. Update xxxxx.


What does this mean ? Is a local update the solution ?

 

[solid7]

Update the product before you generate the CATPart, and you will not see that message.


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