Defines one of the 2D cross sections to which the feature will be fitted. You can define any number of cross section profiles for a lofted feature, using any combination of cross sections created from profiles and cross sections created from part edges.

Defines the guide curves for the loft to follow. The guide curves must touch all the cross sections. You are not required to define guide curves for a lofted feature.

Defines the depth of the feature or the distance to extend the profile to construct the feature. The extent options are Closed and Finite.

This button changes function as you move through the feature construction process. The Preview button shows what the constructed feature will look like, based on the input provided in the other steps. The Finish button constructs the feature. After previewing or finishing the feature, you can edit it by re-selecting the appropriate step on the command bar. The Cancel button discards all input and exits the command.

Allows you to edit the profile of an existing cross section. This button is available only when editing a lofted feature.

Displays the Cross Section Order dialog box. When you move the cursor over the name of a cross section listed on the dialog box, the cross section geometry highlights in the part window. Select the name of the cross section you want to reorder and then click the Up or Down button until it is in the correct position.

Allows you to define the cross section start point. The start point must be at a vertex. The start point of a closed, periodic element is automatically defined by the software. This option is available only when drawing a profile for a lofted feature.

Allows you to specify whether you construct the feature by drawing a new profile on a reference plane or by using an existing sketch or part edges. 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 or part edges, select the Select From Sketch/Part Edges 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.

Finishes or cancels the profile you are drawing. This option is available only when you draw the profile for cross section.

Allows you to specify whether you construct the feature by drawing a new profile on a reference plane or by using an existing sketch or part edges. 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 or part edges, select the Select From Sketch/Part Edges 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.

Finishes or cancels the profile you are drawing. This option is available only when you draw the profile for path.

Allows you to map points on the cross sections to control the loft.

Sets the feature extent so that the lofted feature begins with the first cross section and ends with the last.

Sets the feature extent so that the lofted feature closes on itself, using the first cross section as both the beginning and the end of the extrusion.

Defines the end condition for endpoint 1. The end condition options are available for each end of an open loft. If the loft is closed, the end condition options are available for the first cross section.

• Natural--There is no constraining condition enforced at the end. This is the default end condition and is valid for any cross section type.

• Curvature Continuous--End cross sections defined using part edges, construction curves, and construction surfaces support a curvature continuous condition. The tangent vector for the surface is determined by the cross section element. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Tangent Continuous--The end cross sections defined using part edges and construction curves support a tangent condition. The tangent vector for the loft is determined by the adjacent surfaces. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Tangent Interior--The end cross sections defined using part edges and construction surfaces support a tangent interior condition. Tangent Interior forces the loft to be tangent to the inside faces.

• Normal to Section--End cross sections that are planar support a normal to section end condition. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Parallel to Section--End cross sections defined using point support a parallel to section end condition. The loft is tangent to the reference plane of the sketched cross section. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

Defines the end condition for endpoint 2. The end condition options are available for each end of an open loft. If the loft is closed, the end condition options are available for the first cross section.

• Natural--There is no constraining condition enforced at the end. This is the default end condition and is valid for any cross section type.

• Curvature Continuous-End cross sections defined using part edges, construction curves, and construction surfaces support a curvature continuous condition. The tangent vector for the surface is determined by the cross section element. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Tangent Continuous--The end cross sections defined using part edges and construction curves support a tangent condition. The tangent vector for the loft is determined by the adjacent surfaces. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Tangent Interior--The end cross sections defined using part edges and construction surfaces support a tangent interior condition. Tangent Interior forces the loft to be tangent to the inside faces. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Normal to Section--End cross sections defined using a sketch that are planar support a normal to section end condition. The loft is perpendicular to the reference plane of the sketched cross section. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

• Parallel to Section--End cross sections defined using point support a parallel to section end condition. The loft is tangent to the reference plane of the sketched cross section. A variable is added to the Variable Table, which you can edit to control the shape of the lofted feature.

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/Part Edges--Specifies that you want to define the profile for the feature using an existing sketch or part edges.

• 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 or part edges.

• 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.

• Loop--Allows you to select all the edges of an individual loop on a face by first selecting the face and then selecting a loop on the face.

• Face--Allows you to select all the edges of a face by selecting the face.

Deselect (x)

Clears the selection.

Accept (check mark)

Accepts the selected sketch or part edges.

Specifies that you are finished defining cross sections and are ready to move on to the next step.

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.