Displays the Bend Options dialog box so you can set the bend construction options.

Sketch Step

Specifies whether you construct the feature by drawing a new profile on a reference plane or by using an existing sketch. To construct the feature by drawing a new profile, on the Create-From Options List, select the reference plane option you want. To construct the feature using an existing sketch, select the Select From Sketch option.

Draw Profile Step

Edits the profile for an existing feature. A profile is a 2-D curve that defines the shape and location of the feature. This step is available only when you are editing an existing feature. The profile for this feature must be a single linear element.

Bend Location Step

Defines how the bend location is determined.

Moving Side Step

Specifies which portion of the part will be bent. Position your mouse cursor so that the dynamic arrow is pointing toward the side of the part you want to bend.

Bend Direction Step

Specifies the direction the material will be bent. Position your cursor so that the dynamic arrow points in the direction you want the material bent.

Finish/Cancel

This button changes function as you move through the feature construction process. The Finish button constructs the feature using input provided in the other steps. Once you construct the feature, you can edit it by re-selecting the appropriate step on the command bar. The Cancel button discards any input and exits the command.

Create-From Options

Sets the method of defining the profile plane or specifies that you want to construct the feature using an existing sketch. Depending on the model you are constructing, some of the options listed may not be available. For example, if no sketches exist in the model, the Select From Sketch option is not displayed.

• Select From Sketch--Specifies that you want to define the profile for the feature using an existing sketch.

• Planar Face--Specifies that you want to define a plane that is coincident to an existing planar face on the part. When you set this option, a default X-axis and direction is applied to the new reference plane. You can use keyboard accelerators to define a different X-axis and direction for the new reference plane.

• Feature's Plane--Specifies that you want to define a plane that is coincident to a reference plane used to define an earlier feature. You can select the feature you want using Feature PathFinder or in the graphic window. This option is not available when constructing the base feature.

• Last Plane--Automatically selects the reference plane used for the previous feature. This option is not available if the last feature was a pattern or when constructing the base feature.

Select From Sketch Options

Select

Sets the method of selecting a sketch element.

• Single--Selects one or more individual elements.

• Chain--Selects a endpoint connected set of elements by selecting one of the elements in the chain.

Deselect (x)

Clears the selection.

Accept (check mark)

Accepts the selection.

From Profile

Defines whether the profile line represents the left mold line, right mold line, or centerline of the bend. To specify that the profile line represents the left or right mold line, position your cursor to one side of the profile so that a single arrow is displayed. To specify that the profile line represents the centerline of the bend, position your cursor on the profile so that a double arrow is displayed.

Material Inside

Positions the flange on the inside of the profile plane. Overall part length remains the same.

Material Outside

Positions the flange on the outside of the profile plane. Overall part length increases by the material thickness.

Bend Radius

Specifies the bend radius value for the feature you are constructing.

Angle

Specifies the bend angle for the feature. The value must be greater than zero and less than 180 degrees.

Name

Displays the feature name. Feature names are assigned automatically. You can edit the name by typing a new name in the box on the command bar or by selecting the feature and using the Rename command on the shortcut menu.