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 revolved 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. This 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.  The extent options are 360 Degrees and Finite. When you set the Finite option, you can also specify whether the extent is applied to one side of the profile plane, both sides of the profile plane symmetrically, or both sides of the profile plane non-symmetrically.

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.

Axis of Revolution

Specifies the axis of revolution for the profile.

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 type an Angle value of 60 degrees for Direction 1, and an Angle value of 20 degrees for Direction 2.

Applies half the extent distance to each side of the profile when the Finite Extent option is set.

Sets the extent options you want for Direction 1.

Sets the extent options you want for Direction 2.

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.

Sets the feature extent so that the profile is revolved 360 degrees about the revolution axis.

Sets the feature extent so that the profile is revolved a finite distance to either side of the profile plane, symmetrically to both sides of the profile plane, or non-symmetrically to both sides of the profile plane. Type the extent value into the Angle box on the command bar.

Sets the radial extent of the revolution.

Sets the radial angle value to increase or decrease in set increments when you move the cursor. For example, typing a step value of 10 degrees and moving the cursor away from the profile plane would increment the revolved extent from 0 to 10 degrees, then to 20 degrees, and so forth.

Specifies that planar faces are not added to 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.