Not able to copy a part body & paste special "as a result with link" within the same c

[hims1980]

Hello everyone,

i am not able copy a part body & paste special "as a result with link" within the same catpart, when I do this catia shows a error message that "copy paste operation is impossible due to selection problems in master part or in master feature. The feature naming is incomplete.Recreate the master feature". Can anyone help regarding this?

Thanks, Himanshu

 

[TibiX]

Hello hims1980,

Just to be sure, you copy the body and then paste it on the top-most (the father), right? If not, that's probably the source of your problem.

If that's not it, you can try using CATDUAV5 (File -> Desk... -> right-click the CATPart -> select CATDUAV5... from the list -> select the Clean radio button whilst making sure you have checked tests 1, 2 and 3 to be run and click Run); some errors that might cause your copy-paste issues would probably be corrected.

More information about CATDUA can be found here and here.

Hope this helps,
Best of luck!

CATIA V5 R21 – mold tool design engineer
plastics industry

 

[hims1980]

Hello Tibix,

Thanks for your reply. I tried the CAT DUA V5 Utility & cleaned the file, I found one error which was fixed by CAT DUA V5, But still I am receiving the same error message.

I am sending you the jpg image attached below, in which I want to copy the "Matrice sup" part body & paste special below that, hope this will give some idea to you.

Thanks,

Himanshu

 

[TibiX]

Is Matrice Sup a body created with copy-paste operation or have you created it features like pad and fillet and so on?


CATIA V5 R21 – mold tool design engineer
plastics industry

 

[hims1980]

Matrice Sup consists of features like pad,pocket,fillet etc...

Himanshu

 

[TibiX]

You said that you tried using CATDUA, but did you try copying the body and then pasting it on the top-most (the father)?

CATIA V5 R21 – mold tool design engineer
plastics industry

 

[hims1980]

Hello Tibix,

I just noticed that, basically this is a forging die component & there is a logo embossed on the forging part, subtraction of which from the die component results in a logo engraved in the die component. There is one another cat part without this logo , I just tried the copy paste special with link operation in that file & it is working fine.
I think there is some problem while creating the logo (may be using pad command) on the forging part. Any way, I have to ask the designer of this forging part to modify the cat part. Many thanks for your precious time & help.

Thanks

Himanshu

 

[TibiX]

You're welcome!

CATIA V5 R21 – mold tool design engineer
plastics industry

 

[jackk]

Himanshu,

I'm not sure what that message means, but running CATDUA is a good idea as Tibix suggested. Please let us know if the designer is able to fix the problem.

One thing I noticed right away when looking at the tree is you have non-hybrid geometry, but you are running CATIA in Hybrid Design mode. I'm not sure if this is causing the problem, but I would suggest you use Tools+Options to turn-off (disable) Hybrid Design mode. (Part Bodies should always have green gear icons - you have gray icons in the image you attached)

 

[itsmyjob]

Looking at your picture I see the body (and Partbody) is (are) with a grey icone. If I am correct it means this is an non-hybrid design solid (file) but you work within an hybrid design enable environment. That be be a problem.

Eric N.
indocti discant et ament meminisse periti ​