Displays the Hole Options dialog box so you can set the hole construction options. To apply saved settings, click the arrow on this button and then select a name from the list.

Plane Step

Defines a plane for the profile to be drawn on. You can select an existing plane or create a new one. Plane creation and selection controls are added to the command bar when the plane step is active.

Hole Step

Allows you to place hole circles, which are the profiles that hole features are based upon.

Extent Step

Defines the depth of the feature or the distance to extend the profile to construct the feature. The extent options are: Through All, Through Next, From/To Extent, and Finite Extent.

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

• 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.

• 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.

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 hole is extended through only the next face on the selected side. The next face is defined as the closest face where the hole circle 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 hole is extended from one face or reference plane to another. You can use the profile plane as one of the extentsselect the profile plane handle or click the right mouse button.

Finite Extent

Sets the feature extent so that the hole 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.

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

From Surface

Specifies the surface on which the hole will begin. This option is available only when you use the From/To Extent option to construct or edit a simple hole.

To Surface

Specifies the surface on which the hole will end. This option is available only when you use the From/To Extent option to construct or edit a hole.

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.

Activate Part

Activates an inactive part. This option is available only in an assembly.