topic Re: Sweep a Solid with 2 Rails in Inventor Forum

Sweep a Solid with 2 Rails

gsuty — Fri, 19 Sep 2025 23:58:38 GMT

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.

Re: Sweep a Solid with 2 Rails

89198826955 — Sat, 20 Sep 2025 08:06:52 GMT

this is right?

(view in My Videos)

Re: Sweep a Solid with 2 Rails

SBix26 — Sat, 20 Sep 2025 14:54:38 GMT

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

Re: Sweep a Solid with 2 Rails

kacper.suchomski — Sat, 20 Sep 2025 15:00:43 GMT

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.

Re: Sweep a Solid with 2 Rails

gsuty — Mon, 22 Sep 2025 15:17:51 GMT

Thanks for the reply! This is the best solution yet, but I can't make out how yours is different than mine, other than you did it in two halves? I just don't understand why there is such an exaggerated curve in mine, but it doesn't matter, I suppose. Neither is mathmatically correct, but yours is far closer. I guess close is going to have to be good enough for horseshoes, hand grenades, and Inventor.

Maybe Autodesk will with this and put some work into the next release of Inventor....bahahahahahahaha, jk, I'm sure they'll just pour more resources into Fusion. 😐

Re: Sweep a Solid with 2 Rails

gsuty — Mon, 22 Sep 2025 15:19:18 GMT

Not quite, that creates a convex geometry that isn't what would occur if cutting with an endmill or wire EDM. Thanks for the reply though!

Re: Sweep a Solid with 2 Rails

johnsonshiue — Mon, 22 Sep 2025 22:54:26 GMT

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!

Re: Sweep a Solid with 2 Rails

SBix26 — Tue, 23 Sep 2025 00:09:49 GMT

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