First you will have to redefine your 3 planes. Have 1 plane bisect the part down the middle, and the other 2 perpendicular to it.
Create a copy of the solid body in the same position and then hide it.
Then, I would suggest creating several equally spaced surfaces offset from either side of the center plane, at each inflection point. closer if necessary. Then, split the part into segments using the surfaces you created. Create sketchs on each surface following the ouline of each cross-section, but creating crisp corners and maintaining uniform wall-thickness.
Hide the sectioned bodies, and show the copied body from above.
Repeat the process in the direction perpendicular to the center plane. sectioning the part in increments at each inflection point. At each section, create a spline that pierces each of the section sketches above to create your guide curves.
After all that is done, loft all of the section sketches together using the guide curves.
We create solid models off of scanned data (mesh surfaces) all the time, and we use a program called RapidWorks that simplifies this process greatly.
how big is this part? it measures 299 inches in on direction!
- ctrl-drag Front plane and tell the dialog to make maybe 6 at a spacing of 40 inches.
- open a 3d sketch and make intersection curves between each plane and all the faces each plane touches
- use a fit spline to make all of the little splines for each curve into one continuous spline.
- you will need to make additional planes outside of the bounds of the part.
- on the end close to the Front plane, draw an arc that kind of matches the part (this part is guessing)
- on the end far from the Front plane, draw a straight line...
- make a loft using all of the splines using the SelectionManager
- tweak the two guessed sketches until it gets as close as you need it.
- trim the surface to the shape you want and thicken it