Help: Creo 2.0 Save a Copy, drw has lost parameters.

[dgoodland]

I require help.

I have created a drawing template that calls parameters from Windchill 10.1 (3D Model state: &PROI_RELEASE and rev: &PTC_WM_VERSION, drawing state: &PROI_RELEASE:D, ver: &PROI_VERSION:D, and rev: : &PTC_WM_REVISION:D ...

It was pointed out to me today that when a user performs a "Save As" "Save a Copy" from Creo on the part, not all the parameters copy in the copied drawing - many turn into the text ***.

^Original

^Copy ... note: State for the 3D model, and the drawings state and version converted to ***

Why does this happen? How can I get it to save correctly?

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[TomD.inPDX]

Likely, this is because Windchill doesn't have a default value for those fields. It has to come from the new entry.

You might consider submitting a support case to learn how PTC intended this functionality to work seamlessly.

[dgoodland]

Okay... my current work around is weak - but works. I made txt files for the cells that go wrong... the user then edits the properties of the cell and "Open"s the appropriate txt file to populate with the correct text with Parameter.

Yes - this could be made into a mapkey that does it all - but it is not supposed to be a solution.

[dgoodland]

Just to clarify:

the parameters are literally lost and not just "empty" ... the values of the parameters are not ***, the parameters are replaced with the text ***. So it is not just a case of changing values for the paramerters.

[dschenken]

It fails because the result of a Save As is a new file, which has no parameters supplied by Windchill. It would be nice if PTC caused the field contents to be changed from "&parameter" to "parameter-missing" to make it easier to understand the problem. I guess the Windchill parameters and a number of other internal values are not copied to make it easier when the part is checked in; instead of having to check to see if they exist in a new file and then modifying them, they are always just added.

[dgoodland]

Better would the values be "blank" as a worst case. But it's a new part and drawing - they should exist!

Try this: Start a new part and make its drawing... the parameters work, and they have not yet been checked in either.

[magnus.salomons]

I'm on Creo 2.0 M110 and it works for me. If you want to save from Creo interface File - Save As I assume you use config option rename_drawings_with_object set to both or part.

Do you get the same error if you choose both part and drawing and File - Save As from the Creo Workspace interface?

After using Save As, from Creo interface, and opening the drawing the cell table in the format is empty but the parameters exists when checking with Repeat region - Filters

Did you check if the Parameter existed in the Creo part? This is how it looks like after Save As.

After Uploading to PDMLink the parameters get updated on both the drawing and the part.

[dgoodland · Accepted solution]

SOLVED!

Rajeev @ PTC finally found the issue... The Legacy Pro/Intralink parameters are not able to carry over. So I had to replace with the Windchill updated parameters (Which give the exact same values).

For STATE: &PTC_WM_LIFECYCLE_STATE:D WAS &PROI_RELEASE:D

For VERSION: &PTC_WM_ITERATION:D WAS &PROI_VERSION:D

For REVISION: &PTC_WM_REVISION:D WAS &PROI_REVISION:D

Note: the 😄 makes it drawing parameter specific, and without it is taken from part.

Hope this makes sense!

Daniel...