NX11 "Swept" thinning between two identical sections

[vdim]

Hello, I've run into a problem using Swept command (shown in the attached file).
I need to sweep a constant circle section along a guide until the end of the second ark and then continue until the end of the guide resulting in the conical shape after the second ark. However, I get a non-linear thinning between the first two identical sections. I would appreciate any advice on this matter. Thanks!

 

[Toost]

This type of sweep in NX does not always do a good job when you have multiple sections. - One can see unexpected shapes.
One could probably use a area law for this particular model but in this case the method seems overly complicated.

The math on that "do it all sweep" will become quite heavy if we force it to do this simple model, its a better solution to build this model in two features. each simple.

You have 4 sections for a constant size cylindrical tube. I created a tube feature and deleted 3 of the sketches.
You want the size transition to happen only between the last two arcs (?). I created a sweep between these two. Linear transition.
I also changed the horizontal reference on the large circle sketch to "avoid" the need to handle the alignment between start and end section.
I created the datum coordinate system for this purpose.
( I forgot to unite the two bodies.)
Note that the solution is not tangent by design even if the deviation is very small.

Regards,
Tomas

 

[vdim]

Thank you Tomas!
Now, by "the alignment between start and end section" do you mean the sketch orientation mismatch?
(as a similar issue described in this thread:

http://www.eng-tips.com/viewthread.cfm?qid=349853

)

 

[Toost]

Yes, as discussed in the other thread, how the sections connect to each other, imagine a fishnet where the start edge of the net snaps to a point on section 1, and the same start edge snaps to a matching point on section 2.
I changed the horizontal direction of the large circle -sketch. It then looks like the attached image.

Regards,
Tomas