I'm trying to create the roughly sketched shape in the attached image.
The starting profile is 2 concentric circles with an outer diameter of 80 mm and the arrival profile is also made up of 2 concentric circles of 40 mm.
I used the "swept" function here but on the one hand it doesn't allow me to select the arrival profile, so I have a tube of constant thickness so I would like the final diameter to be smaller and on the other hand, I would like to be able to make the profile according to the guide line in gray which is supposed to increase the diameter at the beginning of the curve before refining it towards the end.
I hope that is more or less clear.
But hey, I tried the "swept" or "loft" function but impossible to get what I want.
The problem is that you are using Bossage: Swept Base instead of using Bossage/Smoothed Base. A second sketch must be made with the diameter 40mm. For the guide curve, because you have a bit of a tight turn, it is not excluded that you have defects in this part. If this were the case, the two existing guidelines would have to be used instead of one.
Be aware that when you make various section reductions or turns, there is no other choice most of the time than to put intermediate sketches or even additional guide lines otherwise the part is deformed. The first image is made with two parallel guide curves, the second is made with four guide curves placed 90° from each other. The colors of both solutions show that the same result is obtained.
Well, I worked a little on my form and I went through surfaces because I think I wasn't going to get out of it.
I have pretty much what I want but I can't manage to do something very elegant.
In particular, the top of my piece is quite angular and it is perhaps because of this that I cannot give thickness, in this case on the inside, to my envelope.
I tried to use the tangency vectors, I pretty much succeeded for the bottom but not for the top
The shape is very different from what you told us at the beginning: I understand why the surface is necessary ;-)
In any case, very nice work and especially with the method you used (curve to curve). We have our colleague @gt22 who is well versed in the surface he should give you solutions.
Given the complexity of the piece, I think that we should work as long as possible in the surface which offers more possibilities than the volume (restricting and sewing in particular), and only thicken the surfaces at the end of the process. A possible result (c. 2018) starting from your model is in the attached file, but with one weakness: the thickening from the inside of the surface is stubbornly refused by SolidWorks, probably because of the small radius of curvature of the ellipses at the end of the feet. On the other hand, it is accepted from the outside. If the external dimensions must be respected, it may be necessary to resume the modeling of the basic surfaces by defining the interior of the part.
Kind regards M.Blt
PS: I can see the shape of the base, what will the seat look like?
In fact, the symmetry function must use the "body symmetry" option to act on the entire right part of the part. The body is to be selected in the "Solid body" branch of the construction shaft. What fooled you is that during its creation, the body takes the name of the last function of its construction tree (in your case, it will be the Cut-Extrude5). The attached image will be more explicit than my gibberish.
