Sweep Advice

Is there anyway to transform a circle (start) into an ellipse (end) along a sweep path?
Think of an exhaust shape.
Do I use the sweep command or another?

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You will want to use the loft command. One end the ellipse, with two of the ellipse points constrained coincident to the plane on which the centerline lies. On the other end, create your circle and use the split entities command to break the circle into 4 cordial arcs. Constrain two of those points to your centerline plane and the other two at 90 degree intervals to the centerpoint of the arc ( several ways to do this ).
It is not 100% necessary to break the circle into segments, but SW may decide to connect your ellipse to the circle in an inappropriate fashion, giving it an hourglass shape. SW also does this if lofting between two circles along a centerline. The only way to be sure is to provide points which sw will align to. It usually is easiest to pre-select the two points of the sketches that you wish aligned ( although inexplicably, sometimes sw won't allow it for some sketches, but does for others ) before clicking the loft command.
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Brian Hokanson
Starting Line Products
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That 70's tick has good advice - if you can do it, a sweep with guides gives great results (a sweep-with-guides is a macro for creating a loft) The only trouble is that you may have to be extra careful creating the guides. Remember, you need only two - one for the major axis width and one for the minor assuming that the path isthrough the centerpoints. Lots of folks run into problems over-constraining the sections - only use as many guides as required to fully define the section.
If the loft is the only way to go, Brian is correct that it can be dodgy with the points to connect closed contours like circles and ellipses. Even if you think you are very precise when you make your selection it can still be a little off which might mess up some designs. Splitting curves is a solid way to help control but can mess things up in some situations. You can add a guide curve to control that connection point precisely without having to split the curves. Then you can actually delete the guide from the loft defnition (after the loft built once) and the loft will still use that connection vector! This is a tricky way to get the pick points precise without having the guide actually influence the shape (again, depends on your design goals, but my guess from the info in your post is that you don't want the guide to mess with the geoemtry)
One last thought - you can also choose to do a 'centerline' loft if you need the transition to follow a 'path'.
Whih of the three routes you take depends on the geometry and whatever future editing you expect to do. Hard to pick one without seeing the application, but it would probably be a good educational experience to do it all three ways (when time permits) to see the differences in setup and results.
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If you need to ensure that you are closely following your centerline and connecting points properly, construct an additional loft with a straight, perpindicular ( to the cross section shapes ) centerline of the same length as your curved one. Compare volume of the two solids. If the solid using the curved centerline is smaller, its a good indication that its loft points have not been connected properly.
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Brian Hokanson
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Use "Loft" instead of "Sweep"
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Easy. Done it plenty. Sweep works perfectly for this.
Start with this: --Use a straight line for a path. --Make two guide curves that define ellipse major and minor axes along the entire length of the sweep path. --Make section with a single full ellipse, center of ellipse constrained with pierce to the straight line path, axis nodes constrained with pierce to the other two guide curves. --Make your sweep with ellipse sketch section, straight line sketch for main path, and two guide curves
Once you are familiar with doing this from a straight path, transforming the technique to curved paths is logical.
Remember a circle is an ellipse with equal major/minor axis lengths.
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