does publish effect representation?

[jackk]

In another post, someone wrote:

" 3) if you are not using publications you must be working in design mode and not visual. Difference being cache turned on in options."

I didn't know there is a relationship between publishing and design/visual mode.

Am I just mis-interpreting the quote, or does publishing have some effect on representation?

Obviously, you must be in Design mode to publish elements.

 

[DBezaire]

Jack - I just made the assumption that if he (the user) knew nothing of publications, that he would not be using design/visual mode. There are no relationships between publishing and design/visual.
Sorry for the confusion

Derek

 

[solid7]

Actually, I know nothing of publications, as I don't work in a tailored business stream. It was only recently that someone even suggested the idea of publications to me, as part of their normal processes. I still have not figured out (in layman's terms) what publications are supposed to be for.

Please keep in mind - I do offsite design, and very seldom does my finished product become (immediately and untouched) part of an actual engineering process. When it does, I still have not been asked to do anything with them.

I'm speaking to your assumptions about someone not knowing about publications because of their working mode...

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[DBezaire]

Publications are basically a time/date stamped pointer to items you want to link. It adds enormous stability to a linked assembly. Helps organize shared items.

In respect to his methodology/terminology I assumed a lack of knowledge for publications. I thought I might point him in a direction that has saved me countless hours with stabilizing some assemblies.

 

[solid7]

So a publication is nothing more than a non-updateable entity - so what distinguishes it from paste "as result"? (why use one over another)

I know that you've used the "time stamp" reference. Where is the advantage/visibility over using dumb solids?

Thanks for your input.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[DBezaire]

A publication will update if the keep link with selected object is on in the options page. The icon for the entity will display different if it is published. The path in the assembly will appear in the name. If you maintain the links in the assembly, a publicated entity is easier to reconnect.
If I publicate a lofted surface to be used to split a solid in a different part then I change the split surface to an extrusion. I would open up the publication menu - select the share entity - select the new entity to share - assembly updates.
I will send you an example. R14 or R16?

Regards,
Derek

 

[solid7]

Version is not important. I'd be happy to learn more about this. Please send whatever you have.

Thank you.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[catiajim]

One of the biggest advantages is when the element being linked is replace. If the Publication Name of the replacing element is the same as that of the original element, all of the downstream linked parts will automatically pick up the new element.

Example: I have an aircraft loft. In it I have published the surface as UPPER_WING_LOFT. I now design my ribs and spars in context (i.e. in the assembly) with my "Keep Link with Selected Object" turned ON.

Now I want to create a new airplane. This airplane uses a different airfoil. To get the new wing design, I simply swap out the old loft with the new loft. As long as the surfaces contain identical Publication Names, all of the ribs and spars will update.

This is a greatly simplified example, but you get the point.

 

[catiajim]

PS If I didn't use PUBLISH, I would need to go into each part and manually REPLACE each linked surface with the new one.