This project shows and example of creating a boat hull using Fusion 360.

I've included some details (description below and design files) as to how I create the "rails" for the lofts. I used the Loft to under Surface Modelling tools and Thicken to create the solid model.

You might say, "why not use Solid modelling to create the loft then shell to hollow it out?" Try it and see. That tight corner at the bow will probably limit how thick it can be and often leads to cryptic errors. Also, this will make all the surfaces the same thickness which you might not want.

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The idea is to draw two orthogonal sketches, then create a third sketch and use the "Intersection Curve" tool under "Create -> Project / Include". This creates curves in 3 dimensions based on the first two sketches. I like to rename those first two sketches Side and Top respectively. The other thing this project shows is using the Loft tool from the Surface Modelling (rather than Solid Modelling), then using Create Thicken" to the surface.

Another part of this approach is to work with "Half Hulls" (just like the shipwrights of old) as long as possible and then mirror it. Boats are almost always symmetric and that keeps you from having to duplicate operations on the left and right sides.

So here's how I did it. I've included the .f3d file so you can follow along if you like.

I first created a side view sketch, drew the "lines" right side or YZ plane. Then I created another sketch for the top view and drew lines for the projection onto Top (XZ plane). Next I created a third sketch and use the Intersection Curve tool to include these curves in 3-space. These 3 dimensional curves will be used for rails when creating the loft. It actually doesn't matter which plane you attach this third sketch to, but I like to use the side view. Hide those first two sketches. I like to rename this third sketch "Lines" and at this point have only it showing.

The next step is to create some cross sections. In my case I created some construction planes using "Plane at Angle" of 90 deg from the "Stem" and "Stern" reference lines in my side view sketch and created two more sketches. Next edit sketch #4, and use "Project / Include -> Intersect", hovering over the curves from the Lines sketch should put a red dot where the curve intersects the sketch plane. selecting that turns the red dot into a little purple circle. Once you have the intersection between the sketch plane and all the curves you can connect the dots with line segments. Repeat this process for sketch #5.

Now the magic happen! Switch to Surface modelling and show the lines and the two cross section sketches (#4 and #5) and the "Lines" sketch. Using the loft tool, Select the profiles lines at the back (sketch #4) and then the front (sketch #5) now go to the "rails" and select each one that connects your two profiles. If all goes well a preview of your hull should be created. At this point I use the Surface Patch tool to create surfaces for the transom and bow.

Once you have the surfaces defined, you can thicken them and mirror the other side. Depending how thick you made it and the angles involved, the thickening process may have added some material on the opposite side of the mirror plane, In that case you might have to use "Split Body" and remove the extra material from the opposite side.

Now you can switch back to Solid Modelling and add any nautical things you can think of (a rudder, outboard motor, sails, anchor, etc).

Please let me know in the comments if you think I should make a video of this process.

Regards,
-Bob M