Sketch won't produce a face that can be extruded
It maybe because you're projecting from a fillet, since I found suppressing that fillet and projecting the edge worked - however un-suppressing the fillet afterwards throws a lost reference error. Or it maybe because of the amount of lost references already in your design. However deleting the projected curve and then projecting the whole body allows you to close the profile and extrude. But I recommend fixing those lost references or this sort of error could well cascade.
Also I did this with sketch 40 (I guessed since it seams sketch 43 is a copy of that). Oh and it will need constraining I didn't re-add the constraints that were deleted with the curve for this pic.
That did work!
So you have 9 yellow icons in your timeline that indicate warnings that something went wrong. Often that mens that users changed something in previous geometry that was referenced in the sketch and now he sketch cannot find that reference anymore.
Going forward, you should not work past those warnings and fix them right away.
You should also make sure that your sketches are fully dimensioned and constrained. I don't always do this for every spline I use, but "normal" geometry is fully constrain and dimensioned.
Right your first sketch already has a problem that can be seen in the resulting geometry extruded from it:
That thin "line" is a gap in your geometry:
Which initiates from your sketch:
Sketch9 where you create the hex indentation, you created on one of the origin construction planes, but then moved the sketch geometry away from the sketch pane. bad idea, unless you really want a 3D sketch. The problem is that most constraints and dimensioning do not work on 3D sketches. It is better tho create an offset construction plane, projectile center point of the hole into that sketch and create the hex profile referencing that center point.
Later on in the timeline you create a bigger hex using the proper technique. At that point in time you should hav e deleted sketch9 and the extrusion for the smaller hex.
Also, as a general rule, a lot of this is symmetric and you should only sketch half of stand then mirror and combine the solid geometry. I personally try to avoid mirroring in sketches wer ever I can or at least reduce it to a minimum whenever possible.
You also may want to make yourself familiar with Fusion 360's R.U.L.E. #1. It will help organizing sketches into those components that they belong to and a number of other goodies.
In the operation below you are moving the body away from it's origin in the component and as a consequence also away from the originating sketch, which is also fully unconstrained. Only in very rare cases may you want to do that and this isn't one of them!
I am not even a quarter through your timeline and I'll stop for now.
The problem at the end pf your timeline can be discussed when you have a stable model 😉
