Datum Feature Symbol "Duplicate Label" of Deleted Symbol 2D DRW mode

[BG_9869104]

Think it is the same as old thread https://community.ptc.com/t5/3D-Part-Assembly-Design/Find-set-datum-tag-creo-4/td-p/657064
bug ? https://www.ptc.com/en/support/article/CS304721

I'm in CREO 7.0.3.0
Also Windchill 11.1 m020

Get Duplicate Label warning about datum symbols that have been deleted.

Can DRW file be cleansed of all deleted datum symbols to not get duplicate label warning?

How it happens: I save a copy of a model I want to make a similar part of/different version. The model and drw are saved to the new file. As is there are 2 datum feature symbols(A and B) made in the 2D drawing attached to dimension leaders. I edit the geometry of the model and that ends up deleting the dimension the datum feature symbols were attached to so the symbol is as deleted and not longer in the DRW tree when returning to the DRW. Now when I try to place the datum feature symbols A and B are still consumed somehow and I get "duplicate label". I can find no way to clean the old datum feature symbols from the file.

Tool I used to make the Datum symbols:

Original drawing 

Save copy as + deleted dimension with datum A tag + try to add tag to new displayed dimension

The suggested solution in CS304721 is new DRW file.... Which is a pain in Windchill right? Have to go offline create new with same name and import as modified to replace the Windchill file of the same name?

No way to clean the DRW file of deleted datum tags?

 

[StephenW]

That is a very good question! I am still asked about this here in the office on occasion. Sometimes its a simple drawing that can easily be re-created. Usually it is something that we will not re-create.

The good thing about the "duplicate underline" is that it doesn't print. So ignoring is actually an option. Of course ignoring will mean that the next user has to ignore it also and the next and the next...how many times will I be asked about it...well...FOREVER!  I do sometimes have fun with it and tell the next user that it must have been something they did since it didn't show up on my PDF!!!  I let them stew on that for a little while and then go back and tell them....sometimes.

[BG_9869104]

So far I have been forced to ignore and then manually check for REAL duplicate datums. Maybe I will find time to test if placing the tag on the model in model annotation mode has the same issue or not. That is more complicated to teach users and then I have to force people toward MBD faster than I want (have to define the company standard from a wild west do whatever past and do all the creo config). 

[BG_9869104]

Found several articles that report this has been fixed.
https://www.ptc.com/en/support/article/CS326152?source=support_assistant

https://www.ptc.com/en/support/article/CS325473?source=support_assistant

This one gives workaround which I hope was not the implemented FIX in later CREO releases. I have not tested yet. Plus I do not want the GTOLS owned by the DRW. 

Workaround:
For newly created in the future, set the Destination of geometric tolerance is drawing instead of model by default via config.pro default_gtol_owned_by_model no

https://www.ptc.com/en/support/article/CS348077?source=support_assistant

[StephenW]

That's good hopefully. I do not currently have Creo 4 M150. I may asked our PTC admin to make it available for testing

[BG_9869104 · Accepted solution]

I was given a workaround fix by PTC support. I have successfully cleared the duplicate label from multiple drawings.

https://www.ptc.com/en/support/article/CS324109

There is a magic DRW DTL option that does the trick 
update_drawing 10097712
This gets applied and then disappears from the DRW DTL option list after closing detail options once. Have to get the symbols to refresh. Then Review tab > Update Sheets. At this point the duplicate label warning is gone but there is still a red line under datums. Regen. Still?. Click on symbol to highlight then click in open space. Still? change datum letter to something else them back again. It better have gotten rid of the red line by now. just attack it with every update and refresh you know. 

[JonasC]

Appeared in Creo 10.0.0.0 and could be solved with your given solution.

[dhebel]

I also have a work around for this.  You don't have to go offline or have a specific version of Creo...

The drawing in question has one or more Duplicate Label errors for newly created datum feature symbol(s).

Start a new drawing, Import > Drawing/Data, select the drawing in question.

Save the New Drawing; close and erase the drawing in question.  Save A Copy of the New Drawing; Select the drawing in question to overwrite, confirm that an object with the same name already exists in workspace.  Close/Erase all,  Open the drawing, delete unnecessary sheets, et cetera.

[JB_9909913]

"Accepted Solution" is not working for me, but I found one that is - so I was trying to respond to post but cannot. Simple as looking in the Drawing Tree - see CS285444

[BG_9869104]

If the datum tag is still in the tree that is a different form of the issue. I see in CS285444 the datums tags are under the gtol still there to be deleted/fixed. My original issue was there was nothing in the tree left to edit/fix. Similar issues divided by nuisance.