Displays the Slot Options dialog box.

Sketch step

Specifies whether you want to 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

Accesses the drawing commands used to create the slot profile.

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 reselecting 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 reference plane. Depending on the model you are constructing, some of the options listed may not be available.

• 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.

• Tangent Plane—Specifies that you want to define a plane that is tangent to a curved face on the part. You can select a cylinder, cone, sphere, torus, or B-spline surface. When you set this option, you can also specify the angular rotation value. 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 graphics 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—Selects one or more individual elements.

• Chain—Selects an 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.

Non-Symmetric Extent

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.

Symmetric Extent

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

Direction 1

Sets the extent options you want for Direction 1.

Direction 2

Sets the extent options you want for Direction 2.

Through All

Sets the feature extent so that the hole is extended through all faces of the part, starting at the profile plane. You can extend the hole to either side of the profile plane, or to both sides.

Through Next

Sets the feature extent so that the slot is extended through only the next face on the selected side. The next face is defined as the closest face where the slot forms a closed intersection with the part. You can extend the hole to either side of the profile plane, or to both sides.

From/To Extent

Sets the feature extent so that the slot is extended from one face or reference plane to another. You can use the profile plane as one of the extents. To use the profile plane, select the profile plane handle or right-click.

"From" Surface

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

"To" Surface

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

Finite Extent

Sets the feature extent so that the slot is extended 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.

Keypoints

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.

	Selects the center and end points.
	Selects any keypoint.
	Selects an end point.
	Selects the center point of a circle or arc.
	Selects a midpoint.
	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.
	Turns off the keypoint location.

Distance

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

Offset

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.

Step

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 increments the distance from 10 millimeters to 20 millimeters, then to 30 millimeters, and so forth.

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.