I have do idea what is actually happening, but it looks like your preview has the ends both with tangencies perpendicular to the sketches and that your actual loft either lost those tangencies or they went to very small values. You could check those conditions and modify them to get something closer to what you wanted.
Save a copy before you try fixing it and send it in to your VAR. If you are accurately describing what happened, it looks like a bug.
If you can post your file - we perhaps could give you some more discerning feedback.
It appears to me that you have your loft split down the middle, because of your main connector (the green dots) when I do this I get the same results, right-click while inside of the feature and show all connectors and eyeball them to line up. You'll get the shape you want. Sort of ..
I think what is happening here is that Solidworks has a difficult time determining where the different segments need to join up to form the loft. This is an annoying shape to model, you'll want to ensure the fillets are clean and consistant throughout the shape as they morph into the circular base.
I uploaded a sample how I might have made this, nevermind the mess as it's just an example, but I first made a theoretical model by lofting just the circle and unfilleted rectangle, this is the Loft1 feature, and spent some time tweaking the connectors as this shape is critical for the next step.
Now the edges produced are still a little wobbly so you'll have to decide if this is sufficient for your purposes, it better because otherwise you should make a manual spline for each corner edge.. tons of fun doin' that!
Next I used a cool technique by sweeping a circle to form nice constant fillet lines that stay constant and then boundary surfaced the openings shut, note the curvature combs on the boundary surfaces are so that they approximate the shape of a constant fillet cross section.
Near the bottom that changes but that's ok, I rather have the geometry change a little rather than having the physical edges doing silly crazy things.
elbow_loft.SLDPRT.zip 648.1 KB
You know what it looks like? It looks like the direction vectors for the two profiles have been switched, althought I don't know what to make of that tapering effect, although I've seen it if the profiles are twisted.
Thanks a lot for the tips. I actually managed to get a pretty good shape simply by tweaking with the connectors. So on how to explain why Solidworks doesn't build what's previewed in some cases only remains a mystery to me!
About the connectors, do you know a way to make them snap to reference or sketch points ?
If you need that level of control, you're better off either adding splits to your circular profile so that it has the same number of vertices as the rectangular profile or adding guid curves
It doesnt look to me like your centerline has any special path so i would be inclinded to create this by using end normal directions and "weight" to control the shape. Ive attached an example.
Your handles will snap to intersection points but unless the circle was created using half an arc and a mirror, you will not get a snap. In the second file my sketches have been created in "half" but i have kept the full profile. During sketch selection in the Loft dialog i simply select each one at a point of interest.