Modeling a Scalene Ellipsoid Mold

[justinm715]

Hey everyone,

I'm trying to create a SW mold of a scalene ellipsoid (for example, something like: en.wikipedia.org/wiki/File:Ellipsoid_321.png - think of it like a smoother slightly squashed rugby ball). I am using SW 2009, and the ellipse button looks like this: dl.getdropbox.com/u/102450/SWellipse.png . As you can see the Radius 1 and Radius 2 features are angled. This is VERY inconvenient to work with. How can I get it to be 'normal' - that is, along the X and Y axes instead of these rotated axes?

Furthermore, when I do get an ellipse profile finally set up, how can I "squash it" after revolving it to make it scalene?

Also, I don't know why, but when I want to modify a sketch feature I can't get the Property Manager to show up. For example, I sketch a Circle then leave sketch mode. I would like to modify the radius of this circle, but I cannot get to the side pane where I can set that. How can I get the circle property manager to show up?

[shift1313]

well i couldnt get your pictures to work but i know what shape you are trying to draw. I would start with two sketchs and a loft operation. 1st sketch on the front plane. Draw a vertical reference line at the origin. Draw an ellipse of your dimensions and trim it at that vertical reference so you have a section. In your second sketch on the Right plane you will draw the other ellipse using that same center line reference. I took that line from the first sketch and Converted Entities. Then Loft between these two making sure to set your start and end constraints to "normal to profile". then you will have a 1/4 of the figure and can mirror it to produce the rest.



Also when you are creatings things in sketch mode using the properties panel this does not fully define them. you need to add dimensions and constraints to your sketches to fully define them. Skipping basic sketch constraints and dimensions is a bad idea when working in CAD

[justinm715]

Thank you for the quick response, shift! Very helpful. Simpler than I thought. Does your SW ellipse sketch tool also have "angled" radii? I've attached a screenshot of my window and the ellipse the tool produces on the front plane. I just want a regular, non-angled ellipse.

[shift1313]

the problem is your sketches arent fully constrained. If you look in the bottom right of your screen it will either say Fully Defined or Under Defined. When the sketch lines are blue, they arent defined. When they turn black they are. What you can do is go to Add Relation and add a horizontal relation between one of the control points and the xy origin point. This will snap it in line, then you need to add two dimensions for height and width. before you do this i suggest drawing your vertical reference line and then trim the ellipse. I dont have solidworks at home but i can show you this tomorrow if you have a hard time with it.

Like i said you need to understand and be able to apply sketch dimensions and constraints(relations). This is not a step that you can skip. It needs to be understood long before you create models and assemblies or else you will be in for big headaches later, trust me

[justinm715]

I think I've done what you said: I have two fully defined parts of ellipses. I created them by drawing two construction line segments (driven by smart dimensions) to represent the radii for one part of the ellipse on the front plane - this was followed by trimming. I repeated this process for the right plane. I'm trying to loft them together but I keep getting a "Cannot knit sheets together" error. I've attached my part file if it helps.

[shift1313]

I was able to loft and knit the surfaces with your sketch, but i would do this as a solid. First i mirrord what you have there about a single plane and make sure to check the knit surfaces box. then just repeat until you have the top half, then mirror that over the top plane and voila. Here are some screen shots for you of how i modeled it. The first time i modeled it i only drew 1/4 of it but more could be done with a single loft and a single mirror. After the first two curves are created(they are closed profiles so they can be used as a loft for a solid), i start a 3rd sketch on the same plane as the 1st sketch and draw the compliment to the 1st sketch. Then mirror the 1/2 about its flat face and merge solids.

First step is the vertical reference line(dashed) and my elipse fully defined, notice the lines are all black. Second image is after the trim operation and converting the small section of the vertical reference line back to a non reference line(note. you dont have to make it a reference line to start, its just a habit for me.). 3rd image is my 2nd sketch on the Right plane which is the smaller elipse. 4th image is after the trim operation. 5th image(missing the 3rd sketch) is the loft, 6th is the mirror.

[justinm715]

It seems you have a circular (not an elliptical) profile on ellipse4.jpg - not quite a scalene ellipsoid. I've done it with 3 different radii but the resulting shape looks a little weird. There's this little sharpness you see in the iso view (see below). Is that how it's supposed to be rendered?

[shift1313]

mine isnt circular. the center is 4" tall, 8" wide in one direction and 5" wide in the other. regardless the procedure would still be the same. Here is one with a little more exaggerated geometry. If you view it shaded without edges those lines will dissapear. Basically because it was mirrored about that plane(line) it will be visible. If you actually render it those lines should not be there, UNLESS your original sketches were not setup properly and your loft settings for start/end were not done correctly. It will however keep these lines as not visible parting or split lines. Meaning when you apply a material you can do it to just a segment. Ive never tried to remove split lines, only add them so im not sure if you can remove them or not.

[justinm715]

Hmm isn't it suppose to look like an ellipse and not a diamond-shape on the lower left? I've attached my fitting of an ellipse: