Part Modeling > Engineering Features > Toroidal Bends > To Create a Toroidal Bend
To Create a Toroidal Bend
1. With a Part file open, click Model > Engineering > Toroidal Bend. The Toroidal Bend tab opens.
2. On the References tab, click Quilts and select a surface or a quilt to bend. The referenced surface is highlighted. If the object to bend is solid, select Solid Geometry.
3. Select an external Profile Section or create an internal Profile Section in Sketcher.
4. Set the Bend Radius on the Toroidal Bend tab in one of the following ways:
Enter a value for the default Bend Radius.
Select Bend Axis and select an axis to bend the geometry around.
Select 360 degrees Bend and select two planes that define the geometry.
5. To extend the bend feature to other objects, click the Curves collector and select either a curve or a composite curve.
6. On the References tab, click Details to activate the Chain dialog box. Select the appropriate Rule check box. The chain features are highlighted.
7. Select a curve bend option on the Options tab to define the bend curve option
8. Use Sketcher to create an internal Normals Reference Section or create an external Normals Reference Section to set the normal direction for bending geometry outside the neutral plane.
9. Click .