In Sketch4 if I click on the face and select Convert Entities I get an error. So I selected the edges individually to see which one was causing the error. Even if I just sketch a line across the endpoints I don't get a closed loop?

Not sure what is happening. If you go to your Guide Curve Sketch and mirror the line that will not convert edges, then change it to a construction line you can then go into Sketch 4 and do a convert edge on the construction line from your Guide Curve Sketch.

The mirror is doing some weird thing to the data would be my guess.

I do not create many shapes like this so I do not have enough experience to draw from.

It will be interesting to hear what Jason thinks.

Regards,

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Anna Wood
SW2008 SP3.0, Windows Vista SP1
IBM ThinkPad T61p, T7800, FX570M, 4 gigs of RAM
http://designsmarter.typepad.com/solidmuse
http://www.phxswug.com

I ended up doing a work-around the problem by creating Sketch 4 before the fillets were added. I was then able to select the bottom face and Project Entities and add sketch fillets.

Always do fillets as the last step. Unless other feature depends on them or it can't be the last for any reason. SW have problem projecting curves even when they're perfectly round. Sometime you can project them, sometime you can't.

The problem lies in the sweep......extrudes are better if possible..as the math is easier. The sweep guides are trying to hold some of the faces flat, but I think there is something going awry tolerancewise in the software and thus the convert entities is choking on some small math error. Suppressing the fillets help but you could have problems later still.

I've attached a model done with two extrudes....the underlying geometry will be cleaner. I only use sweeps and lofts when absolutely necessary. Often I use extrudes...then cut the solid with a sweep or lofted surface.

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Jason
-I don't know if I'm alive and dreaming, or dead and remembering.

"Chuck Norris can speak braille."