Displays the Contour Flange Options dialog box so you can set the flange 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

Allows you to edit 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.

Side Step

Defines the side of the profile to which material should be added to construct the feature. The side step is disabled when adding a contour flange to an existing part or when editing an existing contour flange.

Extent Step

Defines the depth of the feature or the distance to extend the profile to construct the feature.

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 or part edges.

• Coincident Plane—Specifies that you want to define a plane that is coincident to an existing reference plane or a 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.

• Parallel Plane—Specifies that you want to define a plane that is parallel to an existing reference plane or a planar face on the part. When you set this option, you can specify the parallel offset distance. 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.

• Angled Plane—Specifies that you want to define a plane that is at an angle to an existing reference plane or planar face on the part. When you set this option, you can specify the angle value you want.

• Perpendicular Plane—Specifies that you want to define a plane that is perpendicular to an existing reference plane or planar face on the part.

• Coincident Plane By Axis—Specifies that you want to define a plane that is coincident to an existing reference plane or a planar face on the part. When you set this option, you define the X-axis and direction for the new reference plane using a linear edge, a planar face, or another reference plane.

• Plane At End—Specifies that you want to define a plane at the end of an edge you select.

• Plane At Distance—Specifies that you want to define a plane that is offset from the end of an edge you select.

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.

Thickness

Specifies the thickness for the part. This option is only available during the initial creation of the base feature. You can change the default value for the thickness on the Gage tab of the Solid Edge Material Table dialog box.

Finite Extent

Sets the feature extent so that the profile is projected a finite distance to either side of the profile plane, or symmetrically to both sides of the profile plane. Type the distance into the Distance box on the command bar. This button is displayed on the command bar when the extent step is active.

To End

Sets the feature extent so that the profile is projected to the end of the selected edge. This button is displayed on the command bar when the extent step is active.

Chain

Sets the feature extent so that the contour flange extends along a series of edges you select.

Keypoints

Sets the type of keypoint you can select to define a feature extent or to position a new reference plane. Use this option to define the feature extent or the location of the reference plane using a keypoint on other existing geometry. The available keypoint options are specific to the command and workflow you use.

	Selects any keypoint.
	Selects an end point.
	Selects a midpoint.
	Selects the center point of a circle or arc.
	Selects a tangency point on an analytic curved face such as a cylinder, sphere, torus, or cone.
	Selects a silhouette point.
	Selects an edit point on a curve.

Distance (Extent Step)

Sets the distance to extend the feature when the Finite Extent option is set. This option is displayed on the command bar when the extent step is active.

Step

Increments or decrements the value displayed in the Distance box. For example, typing a step value of 0.25 and moving the cursor away from the start point would increment the distance from 0.25 to 0.5, 0.75, and so forth. This option is displayed on the command bar when the plane and extent steps are active

Symmetric Extent

Applies half the extent distance to each side of the profile. This button is displayed on the command bar when the Extent step is active.

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.