link a parameter between parts

[CAD_user]

I hava a parameter in one part, that defines it's height. I would like to link this parameter to other parts, for when i change the parameter in the first part, every part updates with the new height.

How can i make this?

[dschenken]

The best controlled method uses a feature that used to be called a 'layout' that has been re-branded as 'notebook' The file format is identified with a .lay suffix.

A Notebook can contain simple sketch elements as well as parameters that can be 'declared' in any number of models.

See http://support.ptc.com/help/creo/creo_pma/usascii/#page/assembly%2Fasm%2Fasm_three_sub%2FAbout_Declaring_Notebooks.html%23 for hints about using them for your requirement.

An alternative would be to create relations that use the session ID of the component to flag the correct model to retrieve a value from. However, if some change is made as to which model should drive other models then all other models would need to be altered. Also, this requires the source model to be in session to correctly update the referencing models. A Notebook has a much smaller memory footprint.

[CAD_user]

Hello, thanks by your reply. Definitely with notbook it's possible.

Can you show me an example of  create relations that use the session ID of the component to flag the correct model to retrieve a value from? Sometimes I don't have a notebook, and I need to share a parameter between parts, and I still  didn' found of how to do it.

Thanks

[BHOoi · Accepted solution]

In case you have not got the answer. Here are the steps to extract a parameter value from a reference part:

I also attached the PPT and example files here for your reference. Hope it helps.

[CAD_user]

Many thanks 🙂

That's really what i was looking for. That really solves my problem.

By the way, You did an awesome presentation to show how to do it. Really nice job.

[KenFarley]

Don't you have to have both parts in session for the relation to work? If you only open up part 2 but not part 1, doesn't a warning about a missing external reference happen? I use an assembly as a "skeleton" to create parts that become a weldment and I get those warnings if I don't load up the assembly before opening any of the parts that depend on it.

[BHOoi]

yes, whenever you retrieve the part, its referenced part(s) will be brought in to the session as well to ensure everything is up to date. This is the beauty of associativity, isn't it?

There are some settings in config that control the retrieval of the references but personally I still prefer to bring in all related parts into the session. I only turn on the settings(not to retrieve the referenced parts/skeletons/master parts) when I open up other people's files for viewing purpose to speed up retrieval.

[pausob]

Nice! I never knew you could link information from parts together like what you've shown - that is, without first

putting them both into an assembly.

In the assembly context, it is relatively easy to find the ID (go to the "show" menu in the the relations dialog box).

So with your method, how does one determine the session ID ?

[BHOoi]

By the same way, via assembly. A temporary assembly can be created solely for checking the session ID of the part being referenced. The assembly can then be ignored, or quit without saving.

Note the same method can be used to retrieve parameters from data sharing part such as merge or inheritance. In this case, the feature ID is used instead of session ID.