Allows you to specify 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.

Allows you to edit the profile for an existing feature. A profile is a 2D curve that defines the shape and location of the feature. To create a base feature by protrusion, the profile must be closed. This step is available only when you are editing an existing feature.

Defines the side of the profile 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 profile is closed.

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

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.

• 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 Normal to Curve—Specifies that you want to define a plane that is perpendicular to a curve you select. This is the default option when constructing a helix using the Perpendicular option.

• Plane By 3 Points—Specifies that you want to define a plane by three keypoints you select.

• 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

Sets the method of selecting a sketch element.

• Single—Allows you to select one or more individual elements.

• Chain—Allows you to select 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.

Specifies that the feature extent is to be applied non-symmetrically about the profile 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 profile 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 profile is extruded through all faces of the part, starting at the profile plane. You can extrude the profile to either side of the profile plane, or to both sides.

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

Sets the feature extent so that the profile is projected from a specified face or reference plane to another specified face or reference plane. You can use the profile plane as one of the extents. Select the profile plane handle or click the right mouse button.

"From" Surface

Sets the face to extend the feature from when the From/To Extent option is set.

"To" Surface

Sets the face to extend the feature to when the From/To Extent option is set.

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.

Sets the type of keypoint you can select to define a feature extent or to position a new reference plane. This allows you 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.

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 profile plane would increment the distance from 10 millimeters to 20 millimeters, then to 30 millimeters, and so forth.

Displays the Treatment Options dialog box so you can specify whether you are prompted for treatment parameters while you are constructing the feature. When you specify that you want to be prompted for treatment parameters, the Treatment Step on the command bar is activated so you can specify the draft angle and crowning options you want.

Removes any draft or crowning you have defined for the feature. If you want to apply the treatment options later, you will have to redefine the treatment options you want.

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

Adds crown parameters to the feature.

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 click the Preview button. If the draft angle is applied in the correct direction, click Finish. 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 Finish.

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

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

Specifies that planar faces are not added to the ends of the feature. This option is available when the profile you are extruding is closed.

Specifies that planar faces are added to the ends of the feature to create a closed volume. This option is available when the profile you are extruding is closed.

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.