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Publish and Copy Geometry reference handling

Jacek_Mydlikows
6-Contributor

Publish and Copy Geometry reference handling

Does anybody know how Pro/E(Creo) handles relationship between Copy Gemetry in final part and publish geometry in original one?

There is an often issue I encounter: copy geometry misses references. I mean fileds responsible for selecting the original part and appropriate publish geom are grayed out and empty.

More, system blocks this area, making selecting new part impossible. There is no further info regarding missing references in Reference Viewer.

Retreive Ref does not work. Any attempt of selection potential parts ends with error message. It seems that system knows how the proper part is named but hide this info for user.


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8 REPLIES 8

The inability to redefin would probably happen if you are missing the Pro/ASSEMBLY license, but apart from this you should at least be able to identify the name of the missing model.

You may have to open this model into session to continue (there is a config.pro option whether to retrieve_data_sharing_ref_parts yes or no).

Jacek_Mydlikows
6-Contributor
(To:gkoch)

Thanks for help Gunter

Missing Pro/Assembly license is not a case in this situation(AAX is in place)

retrieve_data_sharing_ref_parts yes did not help either.

I noticed such problem as described in first post, happens all the time when the rename take an action, and Copy Geometry loses the reference to renamed source file.

In samples I made for investigation it occured, that not only right name of skeleton(source of publish geometry) is required, but more important is the name of top assembly where skeleton is placed. Having the skeleton and final part in session does not guarantee the success until top assembly is there too.

Nevertheless Creo should give me information what Top assembly and what Skeleton it requires to make Copy Geometry ready for changes, to find on the disc, but it fails.1.jpg

I opened final part with the notepad and search through all names of skeleton and top assembly I could remind. Might be surprised but all of them where saved there, inside in *.prt. file.

so again, it looks like the info about target model(container of publish geom) is there, but Creo claims to lose it.

Sorry for the late reply - I have been preparing and delivering a Pro/TOOLKIT training.

One of the topics in the training was the concept of "assembly path" and this applies for Creo in general.

For features created in assemblies the references are always consisting of the top object (top assembly) plus the so-called assembly path, which is an array (sequence) of feature/component IDs.

If your top assembly XYZ has a subassembly with component ID 123 and there is a part with component ID 55 containing a plane surface with ID 99, which is referenced from another model, then the references is remembered as: XYZ.asm -> ID123 -> ID55 -> ID99

For the reference the names of the subassembly or the part actually do not matter! Only the component ID must be correct and of course the surface with the ID 99 must exist in the part. The names are usually evaluated in session. Therefore you do not get the name, if the reference is missing.

Of course when opening XYZ.asm, it knows that its component ID 123 has a specific model. So if you have renamed the subassembly without the top assembly being in session (and saved afterwards), the component fails to load next time. The assembly will report the missing name.

However, if you have a version of the top assembly, where the subassembly no longer exists, then the reference will fail, knowing only the top assembly name, but not the subassembly or the actually referenced part.

That you found the names in the part, might be due to a kind of internal book keeping. However, the relevant data for the reference does not remember the names (except for top model).

In your example the sentence <Missing Ref> ID 350 in... should continue with the name of the top object of the reference - this is the context the reference has been created in. For an extern copy geom it would be the part, for a copy geometry in an assembly it would be the top assembly with a component path.

Display Full Path and Info should be helping to get more information about those references.

thank you for in-depth reply

below you can find richer information regarding references

1.jpg

I used red color to hide some details of names I do not want to share public..

Again - having such infor how would one solve such problem?.

To me Creo should allow selecting new source part and source publish geometry.

Is it possible to write a script in Pro/Toolikt to make such funcionality available?

vzak
6-Contributor
(To:Jacek_Mydlikows)

Jacek

What would you mean by "selecting new part and new PG" ? If you mean selecting new references completely then you can simply delete old Copygeom (that lost its path per Gunter explanation) and create New. All children will eventually fail, but this is unavoidable since you can select (or create) Pubgeom or completely incompatible type.

Creo will not allow to replace one Pubgeom by another (in another part) and try maintain stable IDs , such attempt may lead to serious data corruption. The only way will be with Edit References option which will narrate your selections to exact same types and number of references as in original parent.

As a side note - if you Rename models in PDM (Windchill server) then all Copygeoms (and any other assembly references) will be updated in the most clean way. You need not worry that you missed other assemblies where Renamed model is a member. I know few organizations that prohibit renaming anywhere besides PDM.

Use the link below to view an article from 2001 that explains in some detail relevant information to some of your issues. Keep in mind that is written from an earlier revision of Pro/E but the methods and concepts are still relevant and take note of the hyperlinks in the page regarding the reference viewer and it's functionality.

From your description it may be renaming of some models without the parent object(s) being in session that is causing your issue but using the steps outlined in my article you should be able to re-establish the lost references and recover your work. I had a Pro/Toolkit developer working for me at the time but did not think it worthwhile to try and automate this. We could usually resolve the lost references quickly and it does require some "thought" to get it done that may be tricky to implement in Toolkit.

http://https//web.archive.org/web/20020110010852/http://profilesmagazine.com/p16/tips_copygeom.htmlhttps://web.archive.org/web/20020110010852/http://profilesmagazine.com/p16/tips_copygeom.html#

If the link does not work let me know and I will see if I can dig up the doc.

========================================
Involute Development, LLC
Consulting Engineers
Specialists in Creo Parametric
gkoch
1-Newbie
(To:tbraxton)

Seems the link got a little screwed up, but it can be accessed when clicking the URL on the right side of the line:

https://web.archive.org/web/20020110010852/http://profilesmagazine.com/p16/tips_copygeom.html

Thank you to all

Vzak

"selecting new part and new PG" - picking up new part with new Publish Geometry

deleting the Copy Geometry was the solution I though I might be able to avoid.

I do not have any type of PDM(Intralink or PDMlink nor any extenal one). For sure this is primary cause of my problem.

Luckly enough, I stored almoast all itterations of files, so to me it would be enough to dig out from final model file, the info what was the name of top assembly before I rename it(I renamed it couple of times)

Thomas

Only second link works to me. I read the article. It is useful.

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