Lists the options for selecting an existing sketch. You can select the sketch in the graphic window or from the list of sketches. If there is only one valid sketch, it is selected automatically.

Defines the side of the sketch to which material should be added or from which material should be removed to construct the feature.

The side step is not required when the sketch is closed.

Defines the depth of the feature or the distance to extend the sketch to construct the feature. You can specify that the feature extends in one direction only, two directions symmetrically, or two directions non-symmetrically. The extent options are: Through All, Through Next, From/To Extent, and Finite Extent.

Defines the draft and crowning options you want.

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. The Cancel button discards any input and exits the command.

Sets the method of defining the feature.

• Single--Specifies that you want to select one or more individual sketch elements.

• Chain--Specifies that you want to select a endpoint connected set of sketch elements by selecting one of the elements in the chain.

• Face--Specifies that you want to select a planar face or sketch region on the model.

Accepts the selection. You can also right-click to accept the selection.

Clears the selection.

Specifies that the feature extent is to be applied non-symmetrically about the sketch plane. When you set the Non-Symmetric Extent option, Direction 1 and Direction 2 options are added to the command bar so you can specify the extent options you want for each direction. For example, you can specify a Through All extent for Direction 1, and type a finite extent value of 20 millimeters for Direction 2.

Specifies that the feature extent is to be applied symmetrically about the sketch plane.

Sets the extent options you want for Direction 1.

Sets the extent options you want for Direction 2.

Sets the feature extent so that the sketch is extruded through all faces of the part, starting at the sketch plane. You can extrude the sketch to either side of the sketch plane, or to both sides.

Sets the feature extent so that the sketch is extruded through only the next closed intersection with the part on the selected side. You can extrude the sketch to either side of the sketch plane, or to both sides.

Sets the feature extent so that the sketch is projected from the sketch plane to another specified surface. The From extent is automatically set to the sketch plane. The To Surface can be any valid surface on the model.

Sets the feature extent so that the sketch is projected a finite distance to either side of the sketch plane, or symmetrically to both sides of the sketch plane. Type the distance into the Distance box on the command bar.

Sets the type of keypoint you can select to define a feature extent. You can define the feature extent using a keypoint on other existing geometry. The available keypoint options are specific to the command and workflow you use.

Specifies the distance to extend the feature when the Finite Extent option is set.

Specifies the distance to offset the feature extent when the From/To extent option is set. For example, you can select a face as the From element and then specify that the feature extent is offset 10 millimeters from the face you selected.

Sets the distance value to increase or decrease in set increments when you move the cursor. For example, typing a step value of 10 millimeters and moving the cursor away from the sketch plane would increment the distance from 10 millimeters to 20 millimeters, then to 30 millimeters, and so forth.

Lists the treatment options which are available. You can specify No Treatment, Draft, or Crown.

Specifies that you do not want drawn or crowning applied to the feature.

Displays the draft options on the command bar so you can define the draft options you want.

Adds crown parameters to the feature. You can use the Crown Parameters dialog box to specify the crown parameters.

Displays the Crown Parameters dialog box.

Sets the draft angle you want for the first extent direction.

Flips the draft angle direction for the first extent direction. To see how the draft is applied, specify the draft angle you want, then move the cursor in the graphic window. If the draft angle is applied in the correct direction, click to construct the feature. If the draft angle is applied in the wrong direction, click the Treatment Step button, then click the Flip button for the draft angle direction you want to change, then click to construct the feature.

Sets the draft angle you want for the second extent direction. This option is available only when you have specified a symmetric extent.

Flips the draft angle direction for the second extent direction. This option is available only when you have specified a symmetric extent.