Annotation balloons do not attach to exploded drawing view

When creating a drawing file from an assembly that has an exploded view there are times where the annotation balloon may not attach as intended while in the exploded state.




A common cause of this problem is creating the exploded view while in a perspective view mode in the assembly file. This view mode distorts the display of SOLIDWORKS and subsequent views created while enabled. If an exploded view is created while perspective view is enabled the SOLIDWORKS drawing view will have difficulties attaching annotations to parts because of this distortion (even if the model appears correct in the view).


Unfortunately simply disabling perspective mode will not correct the problem since the exploded view was already created with perspective mode enabled. The first step is to disable the Perspective view mode found in Views -> Display.




Once disabled, delete the exploded view from the configuration tab. This is to make sure the old view isn't accidentally used within the drawing file and the problem returns.




After creating a new exploded view, go back into your drawing and refresh the view pallet so it is updated with the assembly. Click on the drawing view you wanted to be in the exploded state and reference the newly created view.




Balloons should now attach as intended to the model in spots that previously failed to attach.




If balloons still fail to attach as intended, or no numbers appear and a ? or * show inside the circle, please contact Hawk Ridge Systems at 877.266.4469 for the U.S or 866.587.6803 for Canada for further troubleshooting and help.

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  • I had this issue (on SW2021, SP4.1 (which is fixed in SP5.1)), but the problem was not due to perspective mode. I was unable to select entire subassemblies in the drawing view that displayed the exploded view. The problem only seemed to affect some of the subassemblies. From what I have observed, my issue had to do with the exploded view itself and, I am guessing, its reference to the parts within the problematic assembly file.

    I had originally selected each part of the problematic subassembly individually when creating the exploded view step. Instead of selecting subassembly1, I selected part1 and part 2 of subassembly1.

    I was able to correct the problem by editing the exploded view feature, opening each step that contained the problem parts/assemblies, and then selected only the subassembly part as the reference (subassembly1, instead of part1 and part2). I had to do this for all steps that manipulated the problem assembly.

    I then went back to the drawing view and, for some reason, sometimes it fixed the problem right away, and other times, rebuilding, force rebuilding, or saving did not make it work. The solution that I found for that was to select the drawing view that contained the exploded view, and change the "Reference Configuration" and then switch back to the desired exploded view.

    This is what worked for me. Hopefully, this information can help someone else. 


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