Bounding Box on Drawing Views: any way to change?

[maxh3]

I'm doing a print for a multibody part that has an exploded view, and every drawing view has a huge bounding box (the dotted line thing you grab to move the views around.) In order to get all of the views on the print, the boxes are overlapping, and it's really difficult to select and move a view on the inside; I have to move the other views away, then move that view, then move the other views back.

Is there any way to shrink these boxes down so they only contain the visible part of the veiw?

 

[weevoe]

I have used the crop view to eliminate this problem.

 

[CorBlimeyLimey]

Have you checked there is no stray sketch element, hidden part or reference geometry (non-auto-sized plane, point, axis) in the model?

 

[rbpmc]

Loose notes get attached to drawing views as well - then you move them somewhere and the drawing view gets enlarged.

 

[ctopher]

Per weevoe's comment, I also sometimes crop the view.
A few versions ago we could manually resize the drawing view bounding box. I don't know why the option was removed.
More info: Link

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[maxh3]

Thanks for the crop view recommendation, but it won't work on detail views, or views that have detail views on them, which consist the majority of my views.

I don't have any notes attached that then enlarged the boxes. I also don't have any stray sketch elements, hidden parts, or reference geometry that I know of. My initial top, front, and right planes are blown up large, apparently causing the bounding box issue, and I've figured out which feature is causing it, but not why. I have a split. I inserted a reference plane .02" into the part (using the bottom of the part for the definition of the reference plane) then used that to split the part into 2 bodies. For some reason, this feature makes the initial planes all blow up large. I can drag the bar at the bottom of the feature tree up, and as soon as that feature is suppressed, the planes go back to just larger than the part. Any idea why?

My exploded view only separates the parts an inch or so; much less than the growth of the plans and corresponding view boundaries.

 

[CorBlimeyLimey]

Other people have reported the same problem but, unlike you, they had not been able to find a reproduce-able cause.
I suggest you submit that to your VAR as a bug.

If you do a search in the KB for large view boundary, quite a few SPRs will be listed, and you will be able to vote for some of them to escalate their priority.

 

[DiegoLGraves]

Max, set the sheet scale smaller so the view size is smaller, then drag the views approx where you want them, and then reset the sheet scale back. You might find it helpful to turn on the grid as a reference. You can also lock the view focus from the feature tree to help in selecting the view you want to move.

regards, Diego

 

[mjcole]

How about just making a 3d PDF?

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
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[maxh3]

BTW, I did contact our VAR and he had me use the SolidWorks Rx tool to capture a video of me suppressing and unsuppressing the Split feature that was causing the planes (and bounding boxes) to blow up. Upon running this tool, the problem immediately went away, and I was no longer able to replicate the issue! The issue survived multiple re-boots of SolidWorks and the computer, but somehow running the Rx tool magically fixed it.