Creo Parametric - "Selected part is not active. Select again" error when placing datum "In Dim"

[mvicenzi]

I am using Creo Parametric Release 3.0 and DatecodeM190

Creo Prametric - Drawing
I have created a part and a set datum tag annotation with "On Geometry" option.
I have created a new drawing of the part.
When I try to link the datum tag to a dimension in drawing ("In Dim" option), it's reported error "Selected part is not active. Select again" in prompt.

I found the article 'CS118991 "Selected part is not active. Select again" error reported when attempting to place datum "In Dim" in Pro/ENGINEER, Creo Elements/Pro, and Creo Parametric' in Knowledge Base, but when I try to open it I get the message "Sorry. Article 118991 was not found".

Could you help me to solve the problem and be able to link the datum tag to the dimension?

Regards

Here are the errors that I faced
"Selected part is not active. Select again" error reported when attempting to place datum "In Dim" in Creo Parametric

[sacquarone]

Hello @mvicenzi 

I faced same issur first when trying to access article https://www.ptc.com/en/support/article/CS17031 We aplogy for this icnonvenience. However, when trying to access it again (a second time), the URL worked as expected. Maybe would you like to try accessing it again?

Anyway, this issue is due to the fact that:

1. DFS (Datum Feature Symbol, previously called  Set Datum Tag annotation) is owned by 3D Model
2. The dimension is crearted and completely owned ONLY by Drawing object

Root cause of point 2 is probably due to the fact that dimension in drawing was created while option create_drawing_dims_only was set to yes in config.pro (default value being no). My suggestion to resolve this:

1. Delete the Drawing dimension
2. Set create_drawing_dims_only to yes in config.pro and Apply it (at least in session)
3. Recreate the Drawing Dimension

=> After having followed above steps, I expect you to be able to attached the DFS to the Drawing Dimension.

Refer then to article 17143 for a better understanding (pros versus cons) of what values yes and no drives in the system for this create_drawing_dims_only option

Regards,

Serge

[mvicenzi]

Hello @sacquarone,

Thank you for your answer.

I have just tried to do what you suggested but I keep having the same problem.

I closed Creo, set create_drawing_dims_only to yes, reopened Creo and recreated the drawing dimension, but I see the same error reported.

I attached some files to show you what I have done and the error shown (the picture shows the result of setting the file config.pro).

Regards 

[sacquarone · Accepted solution]

Hello @mvicenzi 

We may discuss in italian (I'm Italian/French guy), but let('s stay in English for others. Thanks for your movie. Related to this:

• Please consider it's not reproducible with a default session of Creo Parametric 3.0 M170 (no access to a M190 for a quick test in this version, but probably not related to version used) => See movie at the end of this post
• I did a mistake in my previous post (sorry for that ...). You need to create the diameter dimension (in drawing environment) while create_drawing_dims_only set to  the default value no (and not yes, otherwise, it's expected that issue occurs) ... Sorry for this confusion

Hope this will clarify and help a bit as next step.

Regards,

Serge

[mvicenzi]

Thank you very much @sacquarone, the problem is fixed! 🙂

Regards