How to re-dimension sheet metal part?
You haven't shared a screencast, but I am guessing you were trying to dimension the sketch in the flat pattern. Firstly it was made by projection link on, so it's already constrained and thus cannot be dimensioned. Secondly, that sketch is a child of your sheet metal body and even if you change it it won't affect the shape. Now, the shape is pretty easy to recreate with just drawing a new sketch. But there is also a way to recreate it with help from the original body. I did this:
1. Unfold
2. Project the unfolded body, with projection link OFF. Dimension it. Include the bend line. Refold.
3. Make a new component
4. Make a Flange of the sketch made in step 2.
5. Bend, with a sheet metal rule bend radius overrode to match the original body
Now you can change dimensions of the new sketch and the new body will follow it (I have changed the appearance of original body):
File is attached.
It's hard to tell from your screencast what do you have there, but it seems you have applied 85 mm dimension on a different entity. Also lines are not coincident:
Also there is one more important point here: Generally you should not start to change dimensions of a sketch when it's still under-constrained. In the file I sent you I fully constrained the sketch as indicated by the red lock on its name in the browser and all black entities. So when I change the angle that line stays (screencast). But the one you show in your screencast is blue.
Maybe compare your sketch with mine? Long press of left mouse button close to entities brings up of list of them which might help you investigate.
you have this selected in your preferences-
when you create a sketch on a face, it projects the edges of that face into the sketch (which is why you have a shaded profile. In it's infinite wisdom, AD decided to make these projected lines nearly invisible to, and I quote, "cut down on clutter")
they also thought it was a good idea to have this selected by default on new installs, I think cause it's fun to goof up noobs with something that's impossible to find with out asking.
turn that preference off now. it's not helping you.
if you get a magnifier out, and use just the right light, you can see the project line that you put the diminsion to by accident here-
you can actually select that line and delete it if you want, to prevent accidently using it again. be aware that all the other hidden lines will still be there, lying in wait. just harder to find cus there will no longer be a shaded profile fromthem.
