Hi @GRSnyder, I understand that my first post didn't address your question directly and since my model was somehow simpler than the actual lid, you've dismissed concerns which I've raised, without investigating them.
This time I've toked time to go through it step by step.
First, what are the reasons for Shell failure?
To know what might have happened, we must know how Shell works.
Very briefly, Shell is actually offsetting each face of a model, then extends them until they intersect with neighboring, then it trims them at the intersection and stitch them.
Failure can occur on each of these steps.
A single face can be built in a way that an offset of a specific value would self-intersect, therefore couldn't be created.
An offset face may not be extendable for the required value and failed for same reasons as above.
Set of offset faces may not have an intersection where necessary and Fusion doesn't have a clue how to fill the gap.
The way to investigate the failure is to offset your model manually and look for individual failures or gaps.
The way you've defined a draft angle for the recessed wall is the reason for Shell failure. Corner in a picture below will have a gape when offset.
I've recorded a screencast where I show you that gap.
I also show how you can repair it, but you must know that my method while work, is not suitable for manufacturing. In general making, this Shell is questionable, since it's a part that will be made in vacuum forming technology, which requires only one mold (I will elaborate on this later).
Before watching screencast I must add one more thing about how Shell works.
Above I've mentioned that Shell is offsetting each face individually, which is not quite like that (just on a general level). When we have a set of tangent faces (or with a higher grade of continuity) Shell is offsetting them together. The reason for that is that when offset individually they would not intersect at all, they would pass each other (this is a well-known problem in CAD, known as near-coincident and near tangent, caused by inaccuracies in geometry representation, caused by the use of floating numbers in computer graphics).
I'm telling you this because when you making this manual offsets for whatever reasons you must offset tangent faces together as I do in the screencast.
Now few notes:
The gap I'm talking about is shown at 3:00-3:05.
At the very beginning, I'm showing that Shell works when made outside the part and you can see how specific new intersection looks like. This way Shell is possible because surfaces overlap each other without gaps.
At 0:40-0:45 I'm showing that geometry of a shown face is falling in a wrong direction for inside Shell to succeed.
This moment is the most significant information about geometry you've created.
First, it's telling me that you want an inside shell, where it has no purpose in further manufacturing. And if any purpose (like visualization) it should mimic an actual technology and should be an outside Shell (maybe rescaled for visualization). The reason for that is simple, any CAM programming must be done on the best available geometry.
Geometry from Shell is always an inferior quality to the original one. In a case of vacuum forming, we design surfaces of a mold first and any other are derived from those.
Secondly, this geometry is telling me that you had no specific idea about that recessed pocket, and its shape is accidental.
How do I know that?
That "drafted" wall of recessed pocket is twisting and don't keep the constant angle to any of planar faces. In result in the very middle, this wall is more vertical that drafted wall above, but at the shown place (mentioned 0:40-0:45) is less vertical and intersects face above on the wrong side for inside Shell to work.
Further investigation only reassured me in my suspicions.
You've created pockets bottom by moving constant offset of a sketch (with use of a planar face). There is no way you could have guessed what angle you would get for "draft" on that pocket (not mentioning that this move was non-parametric).
You've made it this way because you couldn't think of any other way, and it looked fine so you had no problem with it.
Until Shell at least.
In my original post, I've skipped that long investigation and shown what conclusion led me to, which is for a successful design you must articulate your intent with a meaningful geometry.
Since you didn't like my simplified lid. I've created another screencast with a new lid and a new design intent.
I don't think that you have a problem with Fusion, but rather with your design articulation. I would like to speak briefly about that specifically, the design articulation.
To properly articulate you design intent you must define the intent, and name the properties of geometry that will fulfill that intent.
In case of your lid, you must know why recessed pocket is at an angle, and why at that specific angle. Why the walls of that pocket are drafted if they are drafted. Same applies to sketches, why arcs. Why that, not another shape.
Your answers might be as vague as you like. You can say that the reasons for having angled pocket are purely aesthetic. But then how less aesthetic is not angled pocket? If you don't have an answer to that then any additional factor (like the angle on pocket) is useless and its existence is not justified.
To be less abstract, you don't know why you've used an offset on a sketch for the bottom of the pocket. Same for the exact position of it. It's because you don't know the design intent, but even if faked you must make one.
CAD programs serve the single purpose, manufacturing of an artifact.
Whatever purpose this pocket serves, it's geometry must meet manufacturing requirements.
In my example, I've assumed that draft on the pocket is done with a simple tapered drill and is machined at a specific angle that will make this pocket tapered also to the main surface at minimum 3deg (required for unmolding the part). These assumptions defined the geometry (like the outline of pockets bottom, which is not an outline of a sketch), and used tools (sweep with path and guide surface, to get a constant draft against the bottom).
Knowing the purpose of the geometry I can also find solutions for problems that will occur further in the design.
This way parametric tool like Fusion is used to embed design intent. In my sketch, I've added dimensions for a minimum angle for unmolding and dimensions for drills which I plan to use.
I wish you will take the time to read this and that will be helpful eventually.
