Publication

Hi,
Im new catia user,tell me use of PUBLICATION and then how to use?

[MrCATIA]

Hi Sara,

In CATIA V5, Publication is a method that will save you alot of time if you do "Relational Design" and "morphing" of parts that contain External References to other parts.

By Publishing parent geometry, you are telling other users which geometry they should use to drive their designs. If the options are set correctly, users can be forced to only use published geometry for External References.

Published geometry can also be used for Assembly Constraints, to make sure parts are assembled per the design intent.

The big benefit is when you change the the parent geometry. If published, the changes will pass down to the children parts when they are updated. If not published, the child parts will have update errors requiring users to manually replace all the broken links (external references and constraints) with the new parent geometry.

This is a methodology that your company should set as a standard procedure that all users follow.

THANKS Mr Catia.

[marcofa]

About publication philosophy.
Will be better tu publish ALL Catpart always? In this case How to publish automatically?
OR
ONLY Catpart involved on relationship with others Catpart? But in Assembly all Catpart are in relation, so ALL Catpart will be better to be published.

Without publishing I found that when I modify sketch of Catparts, when I go back to Assemly they lost constraints ( ! and disconnected); I need to delete !constraint and retype a new one. Will be this problem solved with publishing?
Marco

[MrCATIA]

Good questions, Marco!

As you suggested, only Publish elements that will be used as linked geometry in other parts and products.

This includes:

Geometric features (points, centerlines, planes, surfaces,etc) that will drive other features in other parts (External References with links).

Geometric features (axis, centerlines, faces, planes) that will be used in assembly constraints.

(I can't think of an example of publishing the entire CATPart (can you do that?), but I often publish a PartBody that I will copy&paste with link)

It is a good practice to name all publications, instead of using the default CATIA names (ie: "pivot axis" instead of "line.3")

In most cases; changes to sketches shouldn't make constaints go bad as long as you just modify existing geometry. But if you add new geometry, make sure you update the publication as well!

[marcofa]

Thank you for the answer.
A simple example:
I built an assembly i.e. gearbox: primary shaft, small gear, big gear and secondary shaft. I have to build 4 Catpart, that I will assemble in a Catproduct with constraints (axis coincidence, shaft offset, gear offset, gear surface contact etc).
In this case I suppose it's necessary to publish all 4 Catpart to not loose constraints in case of geometry modification, i.e. gear diam or gear Z etc.
Many features of Catparts are involved in constraint. I need to select any line or palne or axis and publish separately or I can publish simply all 4 catparts? How publish the entire catpart?
Thanks
Marco

[MrCATIA]

CATParts cannot be published.

Within each CATPart, you should publish the geometric features that will be used to establish assembly constraints.

[marcofa]

Catia v5 r 12
Sorry but there is a toolbar button "publish element", when clicked open window "publics elements" with option publish surface edge axis etc, where I can select Part body that is named Part body and I can change the name.
What is this ? Is not Catpart publishing?
Marco

[marcofa]

I send exemple as before.
What I have published with my publishing? All surfaces, edges, axis etc. , or nothing?
Marco

[MrCATIA]

In the example you attached, only the Partbody is published.

To use published geometry for assembly constraints, you have to publish the features (axis coincidence, shaft offset, gear offset, gear surface contact etc) that will be used from this part.