How to identify constaint that prevents sketch item movement
The solution has already has been pointed out to you but I will put it into a video.
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John Hackney, Retired
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I found this almost by accident (I was looking for overlapping geometry). I found that there are 3 points in your circle centers, and that if I choose the "last" one (that doesn't map to a circle), and delete it, the sketch is freed up. So, my guess is that there is a fixed, or projected point sitting there that is freezing the movement of that geometry. I don't know how it came into existence, though.
I do think that the handling of these "point stacks" is one of Fusion's weak points in sketch. I wish there were a better way to visualize these points, manage coincident constraints, etc. It is very confusing.
Jeff Strater
Engineering Director
That WAS how I identified the problem, by finding that point stack. There is no systematic way to do this, no tool you can use that will identify the ONE constraint that is the problem. Often there are 3 or 4 constraints that conflict and removing ANY of them will fix the problem. In this case, the geometry looked very underconstrained to me - few dimensions. So, likely there had to be a fixed or projected geometry somewhere in that sketch. It was not visible, so therefore, I went looking for duplicate (stacked) geometry, which is often the culprit (because new users sometimes don't realize that you should not sketch over top of existing geometry, creating those duplicates). I use Select Other (long left mouse press) to find duplicates. I found one at the center point. There were 3 points there. When you move the mouse over one of the points, if it is a center point, the circle highlights. The first two highlighted the two circles, so they likely were not the culprit (not guaranteed, just not likely), so I guessed at the third. I selected it, and deleted it, and the sketch went blue (underconstrained) again. Often, this will take a few iterations. You delete the wrong thing, so you undo, and try a different one.
It doesn't matter to me whether you accept that as a solution or not.
Jeff Strater
Engineering Director
I agree that the best practices workflows are neither well documented, nor does the software itself guide you to them (or away from the bad workflows).
"How does one sketch on a face without doing this?"
By default, when you sketch on a face, that face's edges are all projected into the sketch, controlled by this setting:
However, (and this is admittedly confusing), a UX decision was made to not show that geometry as sketch geometry (because otherwise the sketch would be too "cluttered"), so you just have to "know" that that geometry is there. You can kind of infer its existence, because there is a profile defined. For instance, I sketched on the top of this cube, and drew a circle:
and, if I make the body invisible, you can see the rectangular profile:
and if you are editing that sketch, you can see the coincident and perpendicular constraint preview:
and, you can define a rectangle by drawing only 3 lines:
I am not defending this (I actually argued against this "invisible projected geometry" change), just trying to explain how it works.
Jeff Strater
Engineering Director
