Part Modeling > Engineering Features > Toroidal Bends > About the Toroidal Bend User Interface
  
About the Toroidal Bend User Interface
The Toroidal Bend tab consists of commands, tabs, and shortcut menus. Click Model > Engineering > Toroidal Bend to open the Toroidal Bend tab.
Commands
Profile Section collector—Displays an internal sketch or an external section to determine the profile section. The profile section must contain a rotatable geometry coordinate system to indicate the location of the neutral plane. For internal profile sections, you cannot exit Sketcher and continue without creating a valid coordinate system.
Bend Radius list—Specifies the bend radius of the neutral plane in one of three ways:
Bend Radius—Sets the distance between the origin of the coordinate system and the bend axis.
Bend Axis—Lies on the profile section plane.
360 degrees Bend—Sets a full bend (360°). Specify two planes that define the geometry to bend. The bend radius is the distance between the two planes divided by 2π.
Bend options collector—When you select a bend radius option, one of the following data collectors appears:
Bend Radius—Sets the value of the bend radius.
Bend Axis—Sets an the axis to bend around.
Bounding Planes—Sets two planes to define the geometry and the length of the bend.
Tabs
References
Solid Geometry check box—Sets the toroidal bend functionality to solid bend geometry. Available when the model contains solid geometry.
Quilts collector—Displays quilts to bend. These can be a combination of any number of quilts within the model.
Curves collector—Displays all the curves that belong to the bending geometry feature. The bending geometry can include any combination of the following items:
Solid geometry
Any number of quilts
Any number of curve chains
Connected or disconnected entities
Profile Section collector—Displays an internal or an external sketch for the profile section.
Profile Section Unlink—Edits the selected profile section sketch.
Normals Reference Section check box—Activates the Normals Reference Section collector.
Normals Reference Section collector—Displays an external sketch as the reference for the normal vector direction of the toroidal bend. When a normals reference section is applied, it references the profile section. Place it as close to the profile section as possible. Avoid the area where the profile section is not tangent or has high curvature. The normals reference section must be long enough for all points in the profile section to have a projection on it. Preferably the two sections either coincide where the curvature is low, or one is an offset of the other. There are two ways to create this dependency:
Create both sections as external sketch features.
Create the profile section as an external sketch feature and the normals reference section as an internal sketch of the toroidal bend feature.
To implement a feature containing multiple internal cross-referencing sketches, first create the profiles section and then the normals reference section. The Sketcher setup for the normals reference section is then automatically selected to be the same as the profile section and cannot be modified within the normals reference section sketch.
Normals Reference Section Unlink—Activates Sketcher to edit the normals reference section sketch.
Options
Curve Bend—Defines the bending options for all curves in the curves collector.
Standard—Bends the chains according to the standard algorithm for toroidal bends.
Preserve length in angular direction—Bends curve chains so the distance from points on the curves to the plane of the profile section is maintained along the angular direction.
Keep flat and contract—Keeps the curve chains flat and in the neutral plane. The distance from points on the curves to the plane of the profile section is shortened. If a second toroidal bend is created with the Preserve length in angular direction option, the result is equivalent to creating a single toroidal bend with the Standard option.
Keep flat and expand—Keeps the curve chains flat and in the neutral plane. The distance from points on the curves to the plane of the profile section is increased. If a second toroidal bend is created with the Standard option, the result is equivalent to creating a single toroidal bend with the Preserve length in angular direction option.
 
* You can apply the nonstandard options only if the curves to bend lie on the neutral plane.
Properties
Name box—Sets a name for a feature.
—Displays detailed component information in a browser.
Handles
The Bend Radius handle displays and modifies the bend radius dimensions when the Bend Radius option is selected. Enter a new value into the input panel.
Shortcut Menu
Right-click the graphics window to access shortcut menu commands.