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I've been trying to get this sweep to work for a while now. It works with a solid circle. It doesn't work with an annulus. I can provide more info if necessary. I made sure the order of the features matched what I've seen in other threads about this issue but that doesn't seem to help. Every time I try to build it, I get the error "The intermediate profile # 2 could not be solved." enter image description here

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You are missing a huge number of guide curves in this scenario. I've taken a screenshot showing what happens when you have an internal and external diameter guide curve for just one 'tooth' on your profile - the other vertices aren't guided, attempt to go in a straight line, and produce self-intersecting geometry that can be previewed, but not built.

Two of 8 guide curves

I am, therefore, going to suggest another way to model your part, since adding all of those curves would be exceptionally time consuming...

Given that your "Flow Axis" is a straight line, this would make much more sense if it were built using a revolve, rather than a sweep. This gives you full control over the cross section.

I have modelled your part using the following procedure:

  1. Create a 'master sketch', showing the internal profile, external profile, and the root of the grooves. I've assumed that the wall thickness should scale down as the diameter reduces (what would happen if the sweep/guide curve procedure you were trying had 'worked'), but if you wanted constant wall thickness, then simply edit the 'master sketch' to use 'offset' curves from the outer diameter, rather than the curves shown.
  2. Revolve the inner area, the solid segment of the body through 360 degrees
  3. Revolve the outer area, the 'ribs', through 8 degrees (my geometry is an arbitrary guess, of course)
  4. Circular Pattern the rib revolve into 24 instances

Demo Gif

Finished Item

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