Section Curve (Smart Curves)

[BABUGOUDA]

Hello All,

For Example, i have a sweep feature with circle as a section curve and the spline as the guide curve.
so if i cut the section (using intersect or section command ) normal to the guide... the section curve which i get is spline not a smart curve(like arc or circle).here as i m working in sealing systems , we always prefer the section with smart curves not the with splines.
but when i cut in catia V5 i will get the circle or arcs, for the same model.

It is important for me to have section with Smart curves for all general information as in catia V5.
Can anybody please answer me.
I am using NX8
Thx
BGD

 

[mathisudar2007]

Hello,

From NX Documentation,it says
•Analytic section curves (lines, arcs or conics) are created if the face is planar, analytic, or a bounded plane.

Thanks,
Mathi K

 

[OldCADPOPro]

One question that I would have is on your sweep. Is Preserve Shape turned on for the sections? It is located under settings and is available when the Alignment is set to Parameter or By Points. If this option is off, your section string is approximated using a tolerance defined in settings as well. I would check these out and see if this gets you back to an arc for a profile. If your alignment method is set to Arc Length, your section strings are always approximated and you will always get a b-surface as the face.

Richard

 

[mathisudar2007]

Hello,

Instead of using spline as guide curve,use 'simplify curve' then create the swept using lines/arcs.

Create section curve using 'planes perpendicular to curve' method. (Here you can use 'join curve' to get the single spline curve from Lines / Arcs).


Thanks,
Mathi K

 

[jerry1423]

That 'planes perpendicular to curve' method works nicely on splines too, but you need to pick a control point on the spline.