I'm always wary of smoothing which requires a lot of guide curves. In this case, I would prefer a scan, taking care to define the profile in a plane perpendicular to the trajectory. This plane is of course defined as passing through one end of the trajectory. Moreover, I will only worry about the outside of the pipe, it is only once the pipe is obtained satisfactorily that I will hollow it out by a shell function that will guarantee me a constant thickness. Integrating the inside of the pipe from the beginning may be problematic because a concentric ellipse is a spline and smoothing, or sweeping, with a spline is necessarily more delicate than with an ellipse. In the attached example (SW 2019) I finished the trajectory (3D sketch) with a 3D spline that I scanned in a second step because I still haven't found a way to drive the twist of a 3D spline (if anyone knows, I'm interested). That way I treat it separately.
To meet GT22, of course a smoothing theoretically gives a great deal of creative freedom and therefore should allow you to obtain the desired volume. But the delicate point is there. There is a great deal of freedom and therefore it is possible to define any curve as a guide curve as long as it starts from the start section and ends on the finish section. However, the pipe will physically follow a single curve that will depend on its material and its implementation and not on the virtual route on SW. It is therefore necessary to think carefully and define guide curves that reflect reality. If it's a smoothing that we want to use I think we should (see pdf attached):
Define the trajectory to the neutral fiber
draw at least three sections in planes perpendicular to the trajectory (beginning, middle and end), to make life easier, use derived sketches or a block to do so.
connect each dial equivalent to the ellipses (the three sections) by splines
impose for each spline at their intersections with the sections a tangent and a curvature identical to those of the trajectory at its point of intersection with the plane of the sections
Select these splines as guide curves
After indeed the image provided may not have allowed me to understand the problem and I answer a little off ....
I think we have to wait for the applicant to come forward again: because if we look at his sketches, there are two options that need to be specified.
The start of the outer section is a square or rectangle and the end is an ellipsoid. This means that making coherent guide curves is not so easy. The inside of the tube has an ellipsoid start. However, in his attempt he used an ellipsöid for both sketches.
So surely the easiest way is to make a full tube with a sweep and then a removal of material by sweeping. That way, with a single guide curve instead of the existing neutral fiber spline, it should allow you to achieve the result as you suggest.
Second hypothesis, the exterior and interior sketch are both an ellipsoid, it is much less complicated without being trivial for all that.
I don't know if you were able to use the file but the tube section is 4.5 x 3 for the outside and 3 mm x 1 mm so the slightest defect will have big consequences on the flow of the fluid. It will probably be a part made in Print-3D so additional imprecision to be avoided because the precision is rather around 0.2 mm with HP's multijet powder technology and rather 0.5 with the fusing wire technique and provided that the machine is not a 3D RepPap with minimalist precision.
If you do the same section as the rest of the part with the sweep and the guide curve, it just works. Theonly precaution to take is to have the guide curve in one piece (with a spline adjustment - see one of my previous posts on the adjustment of the spline)
Kind regards
Note: In the example below made with the applicant's part, the inner section is homogeneous without deformation.
I come back to the subject one last time because as pointed out @Pierre the whole thing is twisted by 20° while going down.
So I rectified to have the curvature and twist as desired @ 30187066b5
@GT22 or another eminent gifted person, will find a more elegant solution maybe but here is my tip in the meantime ;-)
1°) the author has only given a curve at the level of the neutral fiber 2°) To have two parallel guide lines correctly oriented with respect to the neutral fiber, in a sketch I drew a horizontal line in the small radius of the ellipse and then I made a scan surface indicating the 20° twist at the end. Then I made two constrained 3D curves on both edges of the surface, which gave me the two parallel twisted and descending guide curves. 3°) In fact I was forced to make a smoothing with two rectangular sketches (start and finish) then a smoothing with the two guide curves to obtain the twist and the desired descent. 4°) To obtain the ovoid hole I did the same manip as the 2° but with a smaller dimension and above all by doing a smoothing material removal.
Note : I have recovered all the possible sketches of the original model, so this is not an example strictly speaking.
In the photo above you have the result with the obviously and in the attachment the way to have two parallel and twisted guide curves .
I note your enthusiasm developed around this problem not very well posed by an author who seems to have disappeared from the radar... It must be the butterfly effect.
As for me, I'm still looking for the CAD file that seems to exist.
To return to the 20° twist, I would lean towards a sudden value, perhaps even without the knowledge of the author who would misunderstand the twisting of a 3D curve, rather than a stated desire to twist the geometry. So before putting these 20° in the specifications, we should make sure of their legitimacy.
I will finish by side with GT22 who is quite right, Zozo_mp is very close to winning the cup.
As an attachment you have the file in Parasolid format. If anyone wants the SW 2019 version, just ask.
I think that the form is easily explained and understood if you look at all the sketches. In fact, if you look at the attached image and look at all the sketches for future volumes, you can see that the part we made is extended by a straight part that connects to a hollow (like a large countersunk head) see attached image. The same goes for another part.
Note that once you know how to twist and change the slope, it is possible to make the two main hollow channels in a single extrusion with the Smoothing and Material Removal function instead of making end-to-end extrusions. But hey! It's not what we're asked ;-) (hihhihihihi!!!!! )
Your interpretation of the rest is in my opinion wrong.
Look at the attachment with the explanation. The previous one was not very clear when it is not attached
For the file I have been working since the beginning on the @ 30187066b5 I file without changing anything. The one I sent you just contains my proposal. But the sketches are not transmitted to the Parasolid file.
I have As explained draw a 3 d curve on the ins and outs
on which I created a surface smoothing
for explicit that it can work even if it's not on the same level
That's all
and it allows you to always have exactly the same profile all along the guide curve
What from the view of your part does not seem quite the case on the geometry of the profile in theory we should have the same profile for each perpendicular plane along the guide curve
On the other hand, you know that I'm a marble in surface, so could you tell me how you fill the space between Surface-Smoothing 1 and Surface-Smoothing 2.
In other words, I only work in volume while you go through the Surface phase which is simple. But what about the empty space to be filled (what function allows this.)
By the way, I don't understand why I was forced to go through two guide curves when you didn't need to. I did a little surface still ;-) ;-) to make my guide curves.
To try to understand I made an angular offset like the model and then your surface-smoothing to a funny head. (see Attachment) Just like mine before I did two guide curves.
It is the angular offset that would ultimately force us to make two guide curves.
What do you think? We don't get paid a lot but we have a lot of fun;-)
it's not going to do it ................ ;-( ...........; -( (dispute mode with ear pulling and period blowing on the fingers)
I don't know what you did
but my internal part is like that
so well as it should be and in line with the initial profile and arrives ;-(
you had to move the internal curve line to the smoothing with the 2 green dots which must absolutely be on the right fiber from end to end
then to make a full body you just have to create the surfaces that are missing, sew them and say I want a volume (check the cell)
In addition, you'll see that I deliberately left a space between the exit of your elbow and my sketch resketch via a sketch offset and create a surface that doesn't touch your elbow
but quickly adjustable
but I repeat it was only for the example (but it also works in volume) although sometimes he doesn't like splines
simply out of habit and as I know that we go a hair + far in surface area than in volume (deformation of the material) in the handlebars and we can have smaller radii
I often do this ;-)
if you need + explanation tell me
To confirm my words, reopen the file I'm posting and hide the smoothing surface 2
What I did on 1° screen
on the 2° a transparency
and in theory and practice if you create a perpendicular plane(s) via a constrained point on the construction line (spline in 3D sketch) in yellow
Yes! but my fingers hurt a lot after your period ;-)
Not easy to use the mouse now ;-)
We could almost set a ruler if I take your last image with the pink extrusion, it works because the sides of the squares of the sketches are parallel to each other, but if you tilt one of the two squares then you need guide lines. This is even more visible with the ellipse.
Indeed for the ellipse if the angle of arrival is slightly twisted there too you need guide curves that cannot be done freehand, hence my tip to have an ellipse keeping the 2.5 x 1 all along the curvature. This is so that there is no brake or turbulence for the fuide.
Here is an example to conclude the topic (pouf, pouf, pouf)
