Hi @android111 ,
the answer is both yes and no for the many reasons stated above. Fusion is primarily a parametric CAD modeler that produces more rigid analytical solid and surface bodies.
That said, you can do this in Solid, Surface or the Form workspaces (as @davebYYPCU stated)
I'll attach my example. But it's important to note that you have to understand the limitations of a parametric modeler, the overhead it imposes on modeling, and how to negotiate "around" it to get the result that you are aiming for.
For this example, I created two sketches to represent the boundary of the box ("cube"), note that I removed all the constraints from the curves except for the coincident constraints at each adjacent line endpoint. I know this will give me the freedom to move those pairs of points in coordinate space as I wish.

Then create two lofted faces (using the corresponding opposite curves for the inputs) for the inputs of the main lofted body of the box. Note that Fusions modeling kernel will accept sketch profiles or surfaces/faces as inputs for lofts. However, if you pull a sketch out of plane (i.e. one point of a rectangle is not on the sketch plane) the profile will fail and so will any subsequent features.
So I used the two surface bodies (Body1 and Body2) as input for the solid loft.
Hint: turn off the sketch visibility, when building the loft to make selecting the surface bodies easier)

Now turn on the visibility of the sketches and Move vertices to change the shape of the box

You now have a parametric box that modifies as you expect. it is important to note that while it is parametric, it is nowhere close to being fully defined, this makes some designers and engineers uncomfortable proposing this workflow, but I've seen it used quite successfully for conceptual work.
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hope this helps,
Jamie Gilchrist
Senior Principal Experience Designer