Using Extrude on Circle with embeded elipses included and excludeds elipses at random

[jeffpkamp]

I have a circle 125mm across, with a second circle offset by 1.25 mm.  I put an ellipse 1.475 mm wide and 2.331 mm long with its center point on the inner circle with long axis pointing toward the center of the circle.  I use the make circular pattern tool to create 113 of these ellipses with the center of the circle as the rotation point.   

I finish my sketch and select all sketch elements and then exclude the center area of the circle (I'm making a belt with teeth).    It selects all of the ellipses and the outer ring.     However, when I extrude the selection, it randomly does not extrude ellipses

SelectionExtrusion

Selection Looks Like This

Extrusion looks like this:

[TheCADWhisperer]

Pattern features, not sketch elements. 
Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[jeffpkamp]

Here is the file.  Making the pattern with the solids did work.  It definitely still seems like a bug.  It works fine with circles, so I assume there is some sort of calculation error with the ellipses.  

[TheCADWhisperer]

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@jeffpkamp wrote:

 Making the pattern with the solids did work.   

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I don't know what this means?

You still have pattern in sketch?

Only one ellipse is needed.

It doesn't appear to have worked to me.

Also - your first sketch - the very foundation of your part is not fully defined?

Example of a fully defined sketch...

BTW - the best practices technique of Pattern Feature rather than sketch elements holds true in Autodesk Inventor Professional, SolidWorks and Creo...

[jeffpkamp]

When I said that using the solid pattern worked, I mean I made a single ellipse in the sketch, extruded it to make a body, and then used " solid>create>pattern>circular pattern " to create multiple copies of it around the center of the circle in the sketch and then joined those to the solid ring I had made.  

I tried constraining the ellipse in the sketch, but that did not seem to change anything.  I am not sure how exactly you made yours.  I made the center line of the ellipse tangent to the inner circle, the center of the ellipse was centered on a line that crossed the middle of the inner circle.  Got the same results with trying to extrude the sketch.

I now see why patterning the features is a best practice, since using sketch elements leads to double the memory (holding all the sketch objects and features made from them).    I will keep this in mind!

 

[TheCADWhisperer · Accepted solution]

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@jeffpkamp wrote:

I tried constraining the ellipse in the sketch, but that did not seem to change anything.  I am not sure how exactly you made yours. 

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Ellipse in Fusion 360 is very finicky and not well behaved.

I always create major and minor axis as construction lines first with Midpoint constraint between the two construction lines.  Even more trouble if you trim the curve...

[jeffpkamp]

I am really starting to notice just how badly they behave!  I had never used ellipses before, and I think I'll probably avoid them in the future if I can.  Thank you for your help!

[TheCADWhisperer]

What belt standard are you using?

I don't think this design matches a standard anyhow.