Variable Section Body FS, no edges on faces

samuel_l

Hello everyone,

I am using the variable section body FS to do a sweep on a 3D curve and keep my section normal to a plane, because the normal sweep feature keeps twisting the face just a little bit (about 1 degree).

The problem I am having is that there are no edges on the part faces, so it's hard to work on the part because I can't use faces as planes for sketches or other operations.


With the custom feature


Normal sweep


Is there a way to create edges so that the flat faces are useable as planes?

Is there an other tool to make sweeps with a reference direction that could do the trick?

Thank you,

S1mon

Can you share a pubic model? It looks like you're sweeping a rectangular section. It might be more simple to just extrude the path and do some offset surfaces. If this is bending around in 3D, there might be a way to create some strategic cross sections and do a loft, or more of a piece-wise sweep. Sweep is often one of the least accurate features when the inputs have any complexity.

samuel_l

Thanks for your fast answer! Here is a simplified part studio with the targeted operations at the end

https://cad.onshape.com/documents/c1316b12bb5e2357e6c48c1c/w/5e851077bed385739460a54d/e/70eda57b096005e2bab71d96

S1mon

You really only need a 3D sweep for one of the transitions. I've made a copy with two simple sweeps and then a loft to handle the tricky bit. This keeps the parts you want as flat surfaces flat, and only curves the areas that need it. I'm sure this could be simplified a bit more, but this should get the idea across...

samuel_l

Thank you for the tip, it works great.

@S1mon

I was just wondering, would a sweep with the section normal to the right plane be simpler if the option existed?

Thanks again it works great,

S1mon

@samuel_l

I'm not exactly sure what you mean by "simpler", but in general, Sweep behaves best with the Section normal to the Path. In other CAD systems, having a point on the section which pierces the path is usually a good idea (or even required). I'm not sure if it makes much difference in Onshape, but I usually do it out of habit. You can break both of these rules, but it may make things more complex.
 
In Onshape, the sweep section doesn't have to be at one end or the other of the path. I sketched my "Sketch 1" on the Front plane for "Sweep 1".

glen_dewsbury

another option. I swept a surface along your curve then thickened. Leaves flat faces that you can use for sketch planes along most.
https://cad.onshape.com/documents/1d4e9076b16f1ac59d74d99a/w/9296fcba859140baec43f7b4/e/fe64119313073f5c2714ae60

steve_shubin

@samuel_l

https://cad.onshape.com/documents/eb9428b5809b060a0a454f36/w/99a7824647c8ddf8a0f56be0/e/5f2f2a15ec1369adb4c5c002

So there’s four methods ——

1. That used to make TEST
2. SWEEP
3. SWEEP FACES then THICKEN
4. EXTRUDE then THICKEN

Because TEST only has one face at top and bottom also, it will take more time to get an understanding of what’s going on with it

The other three —  I started by looking for parallel faces

Of those three, none of them were completely parallel from end to end

But one was more parallel than the others

And that’s the last one — EXTRUDE then THICKEN (herein ET)

On a cursory visual inspection, comparing TEST against ET, it seems that TEST is pretty close to ET. Now being as ET has faces on the left and right that are parallel, well this shows that there is no twist in ET. So if TEST is fairly close to ET, then it makes me wonder where that one degree twist is in TEST

steve_shubin

@samuel_l said:

Is there a way to create edges so that the flat faces are useable as planes?

There is a way to have faces for planes that you can sketch on

https://cad.onshape.com/documents/eb9428b5809b060a0a454f36/w/99a7824647c8ddf8a0f56be0/e/5f2f2a15ec1369adb4c5c002

I took a little closer look at things

TEST is not going to hack it. Because upon splitting the face (see GIF below this paragraph) I ended up with non-planar faces. Deduced from the fact that I was not able to use those faces created by the splits for sketches

As for the other two parts, the one made with SWEEP and the one made with SWEEP then THICKEN, they both have faces that are not parallel as demonstrated in a GIF in the above message.

For best results, use the EXTRUDE then THICKEN method. 

1. This method has more parallel faces
2. There is no twist
3. You’ll be able to use the faces to sketch on. See GIF directly below