Using spline for pipe and project it on a plane doesn't include center point

[Anonymous]

Hello, 

I've made a system of 3 pipes with a general shape of: quarter of an ellipse and quarter of a circle which illustrate half a roller-coaster loop. 

I want to intersect these 3 pipes using a set of individual planes with predefined angels relative to a reference plane and an axis as shown:

It is essential for me to project the 3 circles and their center on each plane, but I couldn't pull this throw when using the split-body or split-face tools no matter how much I tried. All of my attempts resulted with projection of only the circumference: 

You can find the source file here: 

https://a360.co/2LyVVRu

Can you assist me with this issue and provide me with some insight about what I did wrong?

Thanks in advance! 
Shay Y.  

[SaeedHamza]

Well don't even bother trying to find a center as long as you're using the Sculpt environment, Because it's never gonna give you a perfect circular shape.

To give you a general understanding of why this is happening, try creating a plane in the Sculpt environment and finish form, then try using the plane as a sketch plane, it won't work, because it'll never give you a perfect flat surface too.

In short, you'll need to create this using the solid environment

[laughingcreek]

While @SaeedHamza is right about the nature of tspline bodies, I didn't see any in your design, so I guess that's not the problem

I believe the issue is that the projected cross section isn't actually a circle.  this is because the sketch you made the circle profile on isn't normal to the path you swept it along. 

[SaeedHamza]

@laughingcreek  Yes you're right. from the images attached and the way the faces are split i thought it was a spline.

Edit : Actually I just checked the attached file and @Anonymous  isn't using any plane along path so yes, nothing normal to the path

[laughingcreek]

I'm revising my response (a bit).  the sweep planes not being normal to their respective paths is still a problem.  but I'm pretty sure even if you set it up properly the intersection projection will still be a control point spline (ie-an approximation) for this type of body.  don't think it will ever give you a true circle.  you could of coarse sketch a 3point circle over it and use that instead, and it would maintain it's link to the original that way.

[laughingcreek]

I'm further revising my statement.  It appears that that plane IS normal to the path at that point.  I didn't see how it could be.  you obviously put more thought into the geometry than I did.  the bit about the type of sketch article produced by the project command still holds true though.  3 point circle seems to be a pretty good match though.

[Anonymous]

Dear @laughingcreek  and @SaeedHamza 

First, I want to thank you both for your fast, details and fundamental replies.

It really means a lot to me 🙂 

I've red your posts and if I got you right, the final points so far are:  

1. The sweep planes aren't being normal to their respective paths. 

2. The circle isn't perfect. 

3. I can use 3 points approximation to make a close-enough circles. 

4. Planes are not perpendicular to the swiped pipe's path. 

Let me comment about these observations by adding a few more words:

Focusing on the part named "main pipe" only, you can see the the path of the swiped shape was originally created using a sketch containing an ellipse and a circle: 

Completing the sketch, I've extruded the requested profile, created an offset plane from the vertical side of the ellipse and draw a diagonal line on it (while projecting the rectangular shape along the x-axis of my extruded shape).

Finally,  I used the split body command to, obviously, split the extruded body.

This was done in order to use its edge as my path

(the mentioned bodies are "body1" and "body2" in the figure):

At last, I've created a sketch on the vertical extruded side of the ellipse, draw a circle (using parametric diameter which I've predefined) and swept it along the edge of the extruded shape "body1". In the sweep command I chose "new body" and resulted with "body3"  which was and only one I intended to make.  

(Ignore the multiple bodies seeing in the "bodies" folder as they are products of my attempts later on):

So, to treat points #1 and #2 above - the planes are normal and the circle is perfect.

About point #3 - I cannot do that since my whole design must be parametric.

Therefore I should include as must relations and constrains as possible and less "free design" objects.

About #4:

I will add that the there are two axis in my design, located at the center points of the semicircle and and ellipse and perpendicular to them. Utilizing a horizontal reference plane (shown in the following figure) I've created the inclined (angled) planes which should include the projection of the circles alone the sweep (planes 3-5, and 7-13 in the construction folder):

So by using these geometry principles, all of my angled planes are perpendicular to the swiped pipe along its path.  

So for now, my inquiry still stands. 

I hope I've cleared some of your comments and revealed more data which maybe put some light of what I did wrong or didn't take into account. 

Awaiting for your comments,

Thanks a lot! 

Shay Y. 

[TrippyLighting]

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@SaeedHamza wrote:

...a plane in the Sculpt environment and finish form ... because it'll never give you a perfect flat surface...

---

Fusion 360 only recognizes analytic geometry - solid or surface modeled BRep faces - as "flat"

Any NURBS geometry created by spline curves or T-Splines can be perfectly flat, but Fusion 360 won't recognize it as flat.

[TrippyLighting · Accepted solution]

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@Anonymous wrote:

...maybe put some light of what I did wrong or didn't take into account. 

---

You did not do anything wrong, but you did not take into account what I described in my post above.

The true surprise is that one would think that sweeping a circle along an ellipse would create analytic geometry, but that isn't the case (I have yet to check my other current CAD system how it handles that).

Sweeping a perfect sketch circle along an ellipse will not result in analytical geometry but a NURBS surface. That can be observed in the Viewport if you know what to look for:

If you sweep a circle along a circle you'll end up with a torus. That torus will not have a seam along its length becasue it's anlaytic geometry.

However, in case of sweeping a circle along an ellipse there will be a seam. the seam is the indication of a NURBS surface.

As such, even when a plane-along-path is perfectly perpendicular to an ellipse, the intersection curve between it and the swept surface will not result in another "perfect" sketch circle.

[Anonymous]

Hello dear @TrippyLighting 

Thank for you answer! 

I understand your claim and as disappointing it may sound at least it leaves me with no doubts about my way of work. Taking your answer into account, I'll try to fulfill my needs in the design without using the circles and their centers. 

Regards,

Shay Y. 

[TrippyLighting]

As I understand it, the reason you want to project circles onto those planes is to get the center point. However, that is not really needed. If you project, intersect the edge you swept along to those planes you’ll end up with just that. Center points of the swept pipe at those planes.

[Anonymous · Accepted solution]

Actually that's what I did (if I got you right).

I projected the swept path of the spline (e.g. the pipes) to each plane and resulted with their center points. 

This was good enough for me 🙂 

Thanks again for the advice!

Shay Y.