Your model is out of date. The grey corners signify that something is wrong.
There are 3 things that can show up: a thin grey box around the drawing, thick grey corners, or both.
The thin grey box means that the part file is newer than the view in the drawing. This typically happens when you open the part, change it, save it, and then open the drawing. SE is telling you that the view may not be representative of the part. If you right-click on the view and select 'Update View', the view will update and the box should disappear. Clicking the 'Update Views' icon will update all views at the same time.
The thick grey corners show up in the following example: Part A has an 'Include Part' feature linked to part B. You make a drawing with views of part A. Then you modify part B. If you don't update part A before you reopen the drawing, the corners will show up. SE is telling you to open part A and update the link to part B. No amount of 'Update Views' will solve the problem.
When both show up, you have a combination of the two conditions, so update accordingly.
Don't go updating blindly, though. Sometimes the outlines are useful. Perhaps you only work with one part, never creating new parts for revision steps, but you do create new drawings for each revision (this is bad drafting practice...). So, when you look at an old revision, chances are the views will have outlines. If you update to remove the outline, the old data will be lost.
Hope this helps,
Chris Kirchen
