I tested the Edit Attachment method in Creo 3.0 M130 and if works fine.
But guess what, the "bug" was fixed in Creo 4.0 M020, so it doesn`t work anymore.
Well done PTC, fixing bugs that shouldn`t be fixed.
I don't have M020 so I can't confirm, but I would be surprised if they fixed it. Are you sure you tried a case in which the same entity (line, surface, etc) is in the other view?
OK. FYI I tested in Creo F000 and it still works there. It does appear to have been changed from your video. If that is the case then it was changed in M010 or M020.
I got an answer from PTC:
"This was an intentional bug fix in Creo 3 M140 and Creo 4 M020. We do not allow the user to show the balloons on a view of a different simp rep."
I will try to convince them, that it was a very useful bug and they should return it.
The only method for repeat regions I have found that is reliable is to create assembly-level component parameters. These are associated with the component, not the part or sub-assembly. As a result they are stable.
The down side is that at first it seems like some work, but the upsides include: there is never a 'fix region' problem; items that should not appear in the BOM can be easily filtered out by assigning a particular flag value or by not assigning the cparam at all.
An additional upside is that item numbers can be assigned before the drawing is made so there is no need to hold up an external ERP system for drawing release. If parts are replaced the cparam sticks with the component so the balloons stay the same, unless the user wants to assign a new item number to them.
Overall, my experience was that the upfront effort to establish the cparams more than made up for chasing seemingly random changes due to the way Repeat Regions automatically evaluate and they take less time to update than fix/unfix.
Since the cparams are fixed to the model, they are identical across simplified reps and will automatically reflect the correct callouts for the related rep. If one is clever an additional cparam for the assembly step can prevent the same component from being called out twice on a drawing. You need to create a repeat region for each simplified rep/assembly step. This can be more convenient on multi-sheet drawings as the region can be on the same sheet as the related views.
Final answer from PTC:
It is not planned for Creo 5.0, but given the high number of votes, PM expects this to be implemented in future releases.
So I guess we will have to fina another workaround. Which probably does not exist.
Or use a method described in previous post, by dschenken.
It may not work for you, but we have changed our work intructions to allow not using Find Balloons all together. Instead we have balloons that just simply have the part numbers were the default find balloons are.