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Relating drawing parameters... Is it possible?

pacesetter1
1-Newbie

Relating drawing parameters... Is it possible?

Hello,

My Assemblies and parts have a parameter called "description" which is designated for PDM. I would like my drawing files to have the same parameter so it can be searchable in Intralink.

Is there a way to relate the parameter "description" in the drawing, to be equal to the parameter "description" in the model of the drawing?

Thank you,

Jeff

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3 REPLIES 3

If you are creating from part and drawing from scratch.

Rename - Rename in Session- Common Name (if you fill the common name as description, it can be searchable in Intralink).

Also, in config.

LET_PROE_RENAME_ILINK_OBJECTS (hidden) - yes

LET_PROE_RENAME_PDM_OBJECTS  - yes

If already uploaded drawing and parts to Intralink and need to rename. You may need to check the Rights to rename.

I'm not using Intralink so I don't know if it will help.

In the drawing you can create a drawing program with the following line:

DESCRIPTION:D=DESCRIPTION:0

This will set the drawing parameter DESCRIPTION equal to the model parameter DESCRIPTION if that is what you are trying to do.

mender
6-Contributor
(To:WayneN)

A side note to the drawing program method:  ':0' will work only if the drawing is of a part and it is the first part in session.  Because there are useful use cases this doesn't cover well, we recently introduced a :MDL syntax, which means 'the current drawing model at the time this was entered', and is translated to :# in the database (so it does not change when/if you change the current drawing model afterwards).  As of Creo 2 M160 and Creo 3 M040, you can put a drawing program "DESCRIPTION:D=DESCRIPTION:MDL" in your drawing template, and it'll have the desired result.

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