To Create a Toroidal Bend
Create a toroidal bend for the following part:
1. With a part file open, click Model > Engineering > Toroidal Bend. The Toroidal Bend tab opens.
2. To define the profile sketch, perform one of these actions:
Select an external sketch:
With the collector active on the Toroidal Bend tab, or the Profile Section active on the References tab, select an external sketch.
Sketch an internal sketch:
Click the References tab, click the Profile Section collector, click Define, and then sketch an internal section in Sketcher.
Sketch plane:
Profile sketch:
1. Bend profile
2. Geometry coordinate system
* 
The sketch must be open.
The sketch must contain a geometry coordinate system.
3. To define the geometry to bend, on the References tab, click the Quilts and/or a solid body collector, and select one body, any number of quilts, or a combination of these to bend. The referenced surface is highlighted.
4. On the Toroidal Bend tab, from the list of bending methods, select one of the following options:
Bend Radius, and then type a radius value. The radius defines the distance between the origin of the geometry coordinate system, and the bend axis that the system generates.
Radius 20:
Radius 30:
1. Origin of the profile sketch
2. Axis of the bend
3. Radius
Bend Axis, and then select an axis around which to bend the geometry. The axis must lie on the profile section plane, parallel to the x-axis of the geometry coordinate system.
1. Axis
360 degrees Bend, and then select two planes, one at each end of the geometry to bend. The two planes must be parallel to each other, and perpendicular to the neutral plane. The neutral plane is coincident with the xz-plane of the geometry coordinate system.
1. Planes define bend length
5. To add curves to the toroidal bend feature, on the References tab:
a. Click the Curves collector, and select a curve or a composite curve.
b. Click Details to activate the Chain dialog box, and then select the appropriate Rule check box. The chain features are highlighted.
6. Optionally, to change the curve bend option, on the Options tab, select a curve bend option.
7. Optionally, to set the normal direction for bending geometry outside the neutral plane:
a. Click the References tab, and select the Normals Reference Section check box. A collector becomes active.
b. Click the collector, and then perform one of these actions:
Select an external sketch.
Click Define, and sketch an internal sketch.
8. Click OK.