How can I create and ellipsoid?

luis_suarez

Hi, can someone please teach me how to create an ellipsoid in onshape?
a=25mm b=50mm and c=12.5mm
Thanks in advance, Ive been trying for hours 

leon_poot

How about transforming (scaling) a sphere non-uniformly? As far as I can see non-uniform scaling isn't possible in Part Studio, but I gave it a try in FeatureScript, and it looks quite alright to me.


Have a look, let me know if it's any useful or if I have completely missed what an ellipsoid should look like.
https://cad.onshape.com/documents/e5ce6148b9fd30e37eb1f69f/v/291b6cee261376d404f7a701/e/a6629890f4aec0014627bd56

Jake_Rosenfeld

Hi Luis!

I did this for you but it was definitely a little complicated:

https://cad.onshape.com/documents/532b38f642224df15d401cfa/w/941a58bc127033d70d4b7727/e/144129212c83fa16f0095271

To accomplish it I sketched the cross section of the ellipsoid on all three default planes.  On two of the ellipses I bisected the sketch faces with matching lines down the center (this is so I could select half of the ellipse instead of the whole thing).  On the third ellipse I "split" the ellipse at the four points that intersect the major and minor axes.

https://cad.onshape.com/help/Content/sketch-tools-split.htm

I then lofted the first ellipse into the second ellipse using the split third ellipse as a guide curve.

Written down in text, this is probably confusing.  Feel free to copy the document and edit the features to see how I did it.

john_mcclary

https://cad.onshape.com/documents/c79dd64af6d9e510c22beb9f/w/cd3ff3163e4881619d96b993/e/9cfdc6ae30d7675951f88868

@Jake_Rosenfeld  you beat me to it by 1 minute , but I don't think this is good enough yet...
the lofts are comming to edges.. I see you have the same thing happening

Jake_Rosenfeld

Hmmmmmm

Yeah it appears this approach doesn't yield tangency over the 4 lofts:



(If anyone is confused, this visualization is the 'Curvature visualization' option in the cube menu under the view cube)

I'll chat with some people about making ellipsoids tomorrow.

As a side note, it should be pretty easy to make a mathematically correct ellipsoid if any two of its axes are equal (should be just one simple rotation).

john_mcclary

https://cad.onshape.com/documents/c79dd64af6d9e510c22beb9f/w/cd3ff3163e4881619d96b993/e/9cfdc6ae30d7675951f88868

Best I could get was 3 overlapping parts, one from each axis, but they don't bool union because the intersecting surfaces are reaching infinity.
and each part's poor approximation You would have to do this an infinite amount of times Defiantly no workaround I can muster up @luis_suarez.. sorry

leon_poot

How about transforming (scaling) a sphere non-uniformly? As far as I can see non-uniform scaling isn't possible in Part Studio, but I gave it a try in FeatureScript, and it looks quite alright to me.


Have a look, let me know if it's any useful or if I have completely missed what an ellipsoid should look like.
https://cad.onshape.com/documents/e5ce6148b9fd30e37eb1f69f/v/291b6cee261376d404f7a701/e/a6629890f4aec0014627bd56

john_mcclary

nicely done @leon_poot

leon_poot

Cheers @john_mcclary.
Apparently there is already a FeatureScript out there for non-uniform scaling (I completely missed that), but funnily enough it looks very much the same

ilya_baran

Leon's scaled sphere solution is correct -- I don't actually currently know of another way of constructing an ellipsoid (for three arbitrary radii) in Onshape.
This is my nonuniform scale feature: https://cad.onshape.com/documents/ccbbbcd87f9c80f9650af745/v/d3f3849203d96becc718a958

Jake_Rosenfeld

@leon_poot or @john_mcclary it seems like it would be pretty easy to make an 'Ellipsoid' custom feature that takes in center, x, y, and z lengths if either of you want to try your hand at it.

If not I can try it out this weekend.

john_mcclary

@Jake_Rosenfeld
Yea, one of these days I'll sit down and learn FS

but it looks like @leon_poot nailed it already

Jake_Rosenfeld

Oops! I thought leon made a sphere and just wrote a non-uniform scale.  Turns out he wrote thing as one feature! Nice job @leon_poot !!

leon_poot

Thanks @Jake_Rosenfeld, glad you like it.

luis_suarez

Thanks guys this was a headache!

andrew_roley

@leon_poot There appears to be a bug with the transform: when I choose a location other than the origin, it is not actually centered about it. E.g. a point 25mm from origin in Y direction. If Length X and Y are 25mm, it will be centered about 0,50,0. If Length X and Y are [50,25] mm, it will be centered about 0,37.5,0.

In other words, it is being moved by an extra Length.X^2/Length.Y in the Y direction, up to a max of Length.Y

S1mon

This is a pretty old thread. The built-in transform tool has a non-uniform option now. Unless I'm missing something, it works as it should.

EvanReese

I also made a Sphere primitive custom feature which has non-uniform options. Handy for slappin' some geometry out there quickly.

S1mon

@Evan_Reese

Thanks for reminding me of that set of tools.

BTW there's an issue with the Lattice example:

EvanReese

Ooh, thanks! fixed it.

nicholas_radzykewycz

Okay, pardon if I have missed something obvious, but why would you not make an ellipse sketch and then just use the revolve command for this? That's what I would have done.

eric_pesty

nicholas_radzykewycz said:

Okay, pardon if I have missed something obvious, but why would you not make an ellipse sketch and then just use the revolve command for this? That's what I would have done.

You would still have one axis that would be circular if you did it this way.