doubt about public elements in catia v5

[erio]

Hello everyone,
I'm new to the forum but it's been a long time since I've been following you, many answers from other posts have been very helpful and I hope to find a solution to this doubt too:wink:
I am using catia v5 to make drawings connected to each other by public elements: in practice after making a new sketch, the public issue through tools --> public elements in such a way as to be able to insert it in another design and in case of necessity, the change of the first then the same part is modified also in all other drawings in which it was inserted.
my doubt is: since the public elements are connected in the various drawings from their name (I believe), if I wanted to rename the starting sketch (what I then published, to understand), I would then lose the connection with the same sketch is all correctly renamed?
thanks in advance for the answer :finger:

 

[ARberto]

I used the public elements at first. at my expense I learned that certain automatisms not managed by a plm, create in time chain disasters. It is enough that you delete or move a file that everything becomes a torture. I allow myself to not recommend this, unless they are particular redundant. If so, I would copy the schetch of your interest in an isolated way from any element, so that on a new file you can make a paste copy without having any ties.
I hope I have explained this methodology to you.

 

[Lettore espatriato]

. .
my doubt is: since the public elements are connected in the various drawings from their name (I believe), if I wanted to rename the starting sketch (what I then published, to understand), I would then lose the connection with the same sketch is all correctly renamed?
. .

No. Don't lose the connection. At least, this happens with surfaces/solids etc., but I don't think it's different for sketches.
different is if you rename the file inside which the sketch is contained. Then you may not find the link automatically and you would be forced to re-check the correct file.

 

[Lettore espatriato]

I used the public elements at first. at my expense I learned that certain automatisms not managed by a plm, create in time chain disasters. It is enough that you delete or move a file that everything becomes a torture. I allow myself to not recommend this, unless they are particular redundant. If so, I would copy the schetch of your interest in an isolated way from any element, so that on a new file you can make a paste copy without having any ties.
I hope I have explained this methodology to you.

even the tecnigraph for some things was undoubtedly better than the cad ...
There are companies that make vehicles without plm, with publications and with a few dozen people working on it. enough to be quite sorted and the advantages become greater than (possible) disadvantages.

 

[gianni55]

Hi.

both arberto and expatriate readers are right: the first to advise caution and the second to suggest to use them consciously.

I limit myself to paste the indications of the online guide of catia:
redenomination of an element made publicthe redenomination of an element made public can affect an external catpart or a catproduct document that uses the publication by any available catia mechanism (e.g. by importing with links).
when a public item is renamed, the operation is performed in the active document. confirmed the publication, the application checks and detects the documents in the session that are affected by the new name assigned to the public item. if you need to update the related documents concerned, a window is opened for each detected impact. the application, therefore, proposes the reconnection to the links in the documents concerned in the session. you can update documents if the publication operation has been validated (click ok). you can save active and interested documents.tipsit is recommended to follow the procedure described to avoid links to damaged data in documents. if the link is not reconnected, it may not be possible to restore the documents that have links to the original publication and, subsequently, not to synchronize the data again.in general, do not rename publications when this operation produces an impact. it is recommended to rename the elements made public carefully and only if you are sure that the publication is not used elsewhere or if the whole product has been loaded (the impacts are detected only in the sessions, if the documents concerned are not loaded, the impacts are not considered).

ps for expat reader: the tecnigraph is better than the cad only because during the day you are not always sitting in the chair, but for the rest I do not regret it.

Hi.

 

[Lettore espatriato]

Hi, gianni,
Catia guide is definitely the reference.
With personal experience, with whole bodywork connected by published elements, the problems I had were related to, in frequency order:
(a) elements replaced with other similar;
b) files, with publications, renamed
c) renamed and republished elements.

the case in which, simply by renouncing the solid or the surface, I found problems with external links, it never happened to me. But I'll be lucky. (sometimes).

I do not hide that I have found myself in large Italian companies to feel "heavy and horny" of publications, and then discover that, abroad, ten times larger companies adopt publications as standard . and wonder: but how do they "those" work, having to replace every time the details within each file?

p.
Will he like to stand up, too?http://i.telegraph.co.uk/multimedia/archive/01853/adrian_newey_1853606e.jpgor maybe because with a sylouette of a motor and a little 'cheese card', you can understand in 10 minutes if the tank and the batteries below are there . or squirt the three body solutions that then your "caddisti" will put down with the due details ? bah ... I wouldn't go back , but each instrument has pro and cons. Publications, tecnigraph, cad.

 

[erio]

thank you so much to all for the interest!!
as in my case I am forced to use public elements, following the extract of the online catia guide that gianni55 published I managed to clear my ideas well.
Good Sunday to all!

 

[Lettore espatriato]

thank you so much to all for the interest!!
as in my case I am forced to use public elements, following the extract of the online catia guide that gianni55 published I managed to clear my ideas well.
Good Sunday to all!

Then, for the next time, f1.

 

[Michele_F]

Good morning to all
I am also colliding with the need to copy some reference surfaces in a part of a product to use them as a reference in the construction of a new part (the edge of a lid of a container). I tried to publish entities and make special copy/paste as suggested but the result is a copy of the complete part body... Moreover in some of the business projects I find a way to proceed differently than what you indicate: in the files there are copies of surfaces and curves indicated as surface and curve... with an icon in which in addition to the generic surface there is a red lightning... You know what that could be?

Thank you!

 

[gianni55]

1) Red lightning = fired geometry/without reference/explicit

2) publish the entities but cover the full body: I think you publish badly, if you want to publish a body surface you don't have to select the body but extract the surface and publish that
3) if business projects use different procedures, better ask the boss how he wants you to proceed

However if you want to keep the parametric references take off here my old answer:

If you want to maintain the parameter connection, you need to change the system settings:

tools/options/infrastructure/part infrastructure/general/external references
check: retains the connection with the selected object
but I also recommend you:
check: confirms the creation of a link with the selected object (in this way choose whether to use the explicit or parametric reference).

You need to know what you do well, if you change one part without thinking how it interacts with the other, you can have problems.
Moreover if you delete the product or part, you will lose the links (see the embossed post "work in context").

recommending me again to be careful that with that always active setting not handled well, you may have more trouble than benefits.

Hi.

years ago

 

[Michele_F]

Thank you. Today I am conscious of the limits of the method, using similar tools on creo and the risks were more or less the same, if the function is equal then I can manage it
Thanks again