This is the second time I'm attempting to post this. The forum ate my first attempt. It showed up, then I refreshed the page and it disappeared.
So...
You might want to take an additive Sweep approach instead of a subtractive Loft approach.
You'll want to define an outside and an inside body shape first, and make the base body with the base groove by two Extrudes. Then, if you Sweep a profile around using the Path-n-Guide-Rail option, you can use those two sketched shapes. If you use the interior shape as the path, then the profile cannot "intersect itself" right? And if you use the exterior shape as the guide rail, and use the Stretch setting, then the profile must always fit the varied width of the groove all the way around.
I used a Conic Curve, but you can use a regular arc or whatever. Note that I Projected/Intersected the two faces of the groove to build my profile on, so it must always adjust to fit the groove. Notice also that I fixed one error by adding some material to the profile such that it will positively Join the main body all the way around. You'll see that it took me a few attempts to get everything worked out correctly, but the result is as desired.
Using two splines to define the exterior and interior shapes does not lend itself easily to precision. For example, it's difficult to keep one spline exactly 1/2" away from the other spline for any continuous distance. I did an Offset of the outer spline and converted that to a construction line just so I would have a reference to eyeball. If you want a more precision approach instead of an eyeball approach, you would want to build the two shapes with arcs, lines, etc. that you could precisely dimension. If you do that, take special care to make all bits tangent to each other such that the Sweep can flow smoothly around.
Fusion
