Problem with ellipsoidal section ducts - screenshot provided

3D Design
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ellipse_pipe_help.png
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Hello 

try to do it via a smoothing

Departure sketch / arrival sketch

and to help a little more 

 Guide curves

it should do it

@+

3

Rather than doing a sweep 

Straightening

A starting sketch

A sketch of arrival 

with guide curves

it should do it

@+

1 Like
4

rather than doing a sweep 

passes via a smoothing

Starting Profile

Arrival Profile

and some guide curves if needed

@+

1 Like
5

Hello

Which version are you on and can you share your file?

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Choose a smoothing over a sweep

it should do it

@+ ;-)

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Hello thank you for looking into my problem,

Here is the file https://gofile.io/d/vLmGSN

I use solidworks 2018

Sweep doesn't work either and complains about my guide-curve/3d-sketch that doesn't touch the 2 sides if I remember correctly, while I put the endpoints on the planes :(


tronxy-xy2pro_nozzle-fan_without-plate.sldprt
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Smoothing

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Hello @ 30187066b5

Your guide curve should connect to the end sketches and not (like INventor) to the face.

I understand that your way of doing things is in the logic of the neutral fiber but it is enough from your existing curve to make another parallel plane and tangent with the vertex of the ellipse. In this sketch you project your neutral fiber guide curve because it will serve as a guide line and wow that's it.

A small image that I hope is explicit.

Kind regards


elipsoide_courbe_-_curved_pipe_-_2020-08-02_14_28_01-window.jpg
3 Likes
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Hi @ Zozo

if I understood the problem correctly

it's not  on the same vertical plane

so you have to go through a smoothing

or twist the balayage a bit

@+

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Good evening @gt22

Indeed it is not on the same level and it is also sloping.

In addition, its guide curve is not in one piece, there is a curve plus a small straight line, but above all there is no adjustment of the spline.

I remain convinced that you need at least two guide curves, one at the top of the ovoid and the other on the side.

But if @ 30187066b5  want to have a perfect profile, you will need at least three guide curves or even 4 to master the profile.

Indeed, if I understood correctly, it is a pipe and in order for the fluids not to be disturbed, the section must be constant to avoid throttling and potentially cavitation if the flow of the fluid is important. Given the thickness of the tube, there must be pressure.

I'm going to try to make the model with four guide curves to show what I'm explaining. I hope I don't have to make intermediate profiles to keep the inside section intact.

Kind regards
To pluche

PS: I'll do a little explanation to @ 30187066b5  unless you have a better idea in the meantime to achieve the desired result


v3_elipsoide_courbe_-_curved_pipe_-_2020-08-02_14_28_01-window.jpg
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Good evening @ 30187066b5 

Here is a small intermediate explanation.

Kind regards

PS: tell me if we continue the explanation or if you have solved your PB

 


elipsoide_courbe_et_raccord_sur_pente.pdf
1 Like
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Hello

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.

This is my little drop in the mill

Good night


tuyau_elliptique.sldprt
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Good evening Pierre

Have you been able to look at the plaintiff's piece which is a little more complicated than that.

Kind regards

1 Like
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If you want a clean room

I repeat, there's no choice

you have to go through a smoothing 

@+;-)

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Good evening

To answer Zozo, let's say that the image sent by 30187066b5 (??) is not very explicit. I can just guess an elliptical cross-section pipe that follows a 3D trajectory. If this path does not involve twisting, a sweep could work. The advantage of a scan is that the section is kept at all points of the trajectory.

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):

  1. Define the trajectory to the neutral fiber
  2. 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.
  3. connect each dial equivalent to the ellipses (the three sections) by splines 
  4. 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
  5. 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 ....


lissage.pdf
2 Likes
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Hello @Pierre Mihailovic

We agree on the method. ;-)

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.

Kind regards

1 Like
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Hello @ all

to complete the previous post ;-)

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.


2020-08-04_11_21_59-solidworks_premium_2019_sp5.0_-_tronxy-xy2pro_nozzle-fan_without-plate.sldprt.jpg
3 Likes
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Good evening @tous

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 .

Kind regards


courbes_guides_mises_en_forme_-_2020-08-04_22_10_25-.jpg
1 Like
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@ Zozo well seen the artsite ;-)

I enter see the beginning of the good walkthrough 

at least that is the way I would go

If I had the ins and outs in an operational file that I could convert to SW 2017 (preferably to parasolid)

I will try to form this said piece 

but for me you're on the highway  to success 

@+ ;-)

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