Is it possible to sweep a solid along two rails? I can loft a line along those rails and sculpt the part, but the geometry is pretty far from the result if you were to actually program and cut a part as I intend to do. I can create 'close' geometry, and sketch lines all down the path and loft it nearly correctly, but is there a way to do this simply and correctly? A sweep along two rails would do it, but I can't figure out how. Part is attached.
The difficulty with lofts is that they can create curvatures that you don't want. If this piece (or something similar) is to be machined with a straight cutter, then the solid sweep with two guide paths is really the only exact method.
But it appears that Inventor doesn't have this capability (yet). The attached file (Inventor 2026) uses Loft surface and Split, and looks really good, but I make no claims that it is mathematically exact.
Since it is symmetric, I modeled half and then mirrored.
Sam B
Inventor Pro 2026.1.1 | Windows 11 Home 24H2
A secondary advantage is that when creating the toolpath in the CAM program, you will be able to select these edges instead of faces anyway, so the geometry of the solid will not determine the geometry of the physical part.
Kacper Suchomski
Hi! Inventor Solid Sweep does not support Guide Rail option. As a result, the "Guide Rail" is subject to anybody's interpretation. I use the guide rail as the twist axis. The result definitely has a lot of room for improvement. Please take a look at the attached part.
Many thanks!
I created my loft surface the opposite direction to yours-- the sections are the top (curvy) sketch and the bottom edge; the rails are the two angled lines. Note, however, that since I modeled only half of the part, the two rails are not parallel.
So I wondered if adding a middle section line to your model might produce a better-looking model for you, and it does. I can't see any difference between yours and mine after adding that additional line to yours.
There are still some key differences, though-- your model produces one continuous face, but the only straight edge on that face is the bottom edge. On mine, it produces six faces, apparently tangent continuous, but still separate faces. But: all of the edges except the arcs are truly straight lines, even the edges between curved faces, so I'd say mine is closer to the ideal. (Note: I tested the edges for straightness by starting the Work Axis tool-- it highlights only linear edges as you move around the model, so it's a pretty quick and reliable test).
Sam B
Inventor Pro 2026.1.1 | Windows 11 Home 24H2
