Issues with Showing Item Balloons by View - Creo 4.0

[dbower-3]

Have an assembly drawing created in Creo 2.0.

Working on the drawing now in Creo 4.0 M020.  Having an ssue showing item bubbles on an assembly view, showing bubble by view... nothing shows up.  But if I select 'by component and view', and pick each part... they show up. 

Anyone having similar issues??

[Mahesh_Sharma]

Try clearing the region (Table > balloons > Clear region) and recreate balloons by view.

[dbower-3]

Thanks for the suggestion.  Tried that, did not work.

[Mahesh_Sharma]

Just to check, assembly view and repeat region table are of same representations (if not there might be a warning in message area). Try adding drawing option update_drawing as all (File > prepare > Drawing options) and after that update the sheets. Prior adding this option make sure you saved your work as it something goes wrong, drawing can revert back to original state. 

[dschenken]

I have always seen issues with balloons not showing up when they are expected to. There must be some convoluted path that is taken that favors not showing balloons. I don't know if it is intentional or just careless.

Sometimes I've had to create new views, show all the balloons there, and then switch the balloons to the desired views.

[dbower-3 · Accepted solution]

The below is the solution the worked in my situation.  The next question.... What changed?  Havent  ever had this issue before, now all of a sudden I have to do this in every drawing to get balloons to show up?  My drawing setup file hasnt changed in the past few years.

Thanks for the responses and suggestions.

Please do the following:

1. Retrieve the drawing
2. File > Prepare > Drawing Properties
3. Detail Options > change
4. Set Option: to update_drawing
5. Set Value: to 2200736
6. Add/Change > OK > Close
7. Review > Update Sheets and Update Tables

Table > Create Balloons > By View > pick view

[cgorni]

The behavior observed here matches a Software defect impacting drawings created before Creo 2.0 M100.

Code fix for drawings are usually protected to preserve their existing display at retrieval, as they may have gone through an approval process.

This fix can be enabled by the update_drawing detail option (hidden), as highlighted in the above reply, more information on this option can be found in article CS31562

If using drawing templates you may want to apply all available fixes when upgrading to a new Creo release: setting the detail option update_drawing to all, updating the sheets and saving back the templates.