Find set datum tag - creo 4

[StephenW]

I copied an existing drawing that already had an A and B datum that was defined in the drawing as "set datum tags". During the modeling, the attachment points (both shown dimensions in the drawing) were removed.

I go back to the drawing, I tried creating datums A and B as "set datum tags" and it tells me they already exist.

In the past, i have been successful finding stuff like this with the find tool. Not this time. I tried find in the drawing, every find option I could use. I tried in the model. No luck there.

Just to be clear, these are drawing created set datum tags using the "datum feature symbol" from within the drawing. Little red underline on the B datum means it's a duplicate name.

The question is, how do I find a missing "set datum tag" within the drawing. I use the term "set datum tag" specifically because that is what it is called and what the find tool found when I created another that it did find in the drawing.

[StephenW]

I ran in to this problem again. I'm perplexed. 

[StephenW]

I decided that this problem is drawing specific. If I make a new drawing with the same model, the problem doesn't exist. I also found that this drawing was copied but with a new and different model and the drawing had the same problem.

[jbush]

Same problem here in Creo 4.

Looks like it's a bug: https://www.ptc.com/en/support/article/CS304721

[StephenW · Accepted solution]

https://community.ptc.com/t5/3D-Part-Assembly-Design/Datum-Feature-Symbol-quot-Duplicate-Label-quot-of-Deleted-Symbol/td-p/758134?source=ArticleViewerRelated

The answer was in this post

https://www.ptc.com/en/support/article/CS324109?_gl=1*3mjv2y*_ga*MTYyNzY4Mjk4LjE2ODQ5MjM3MDI.*_ga_1QBT6P6HR1*MTY4NDkzMTQxMy4zLjEuMTY4NDkzMjI0NS4wLjAuMA..&source=copyurl

• Users can repair the data in Creo Parametric 4.0 M150, 6.0.5.0, 7.0.2.0 and 8.0.0.0 by setting the dtl option update_drawing to 10097712:

1. File > Prepare > Drawing Properties > click Change next to Detail Options
2. Set Option to: update_drawing
   • Both the Option and Value must be entered manually (because this is a hidden option) for Add / Change to become available
3. Set Value to: 10097712
4. Click Add / Change > OK
5. Then Review tab > Update Sheets

• How to set detail options: CS137953
• About hidden detail options: CS31562

• Fix for earlier datecodes and releases (including Creo 5.0):

1. Create a new drawing
2. Import the affected drawing into the new drawing with Layout tab > Import Drawing/Data
3. Save a copy of the drawing detail options from the old drawing and import them to the new drawing
4. Recreate missing annotations and compare drawings for any changes that might have occurred in the copying process, like bug fixes or missing entities