Accesses the Lofted Flange Options dialog box so you can set the flange construction options.

Cross Section Step

Defines one of the 2D cross sections the feature will be fitted to. You can define two cross section profiles for a lofted flange. You can use cross sections created from profiles, sketches, and part edges.

Side Step

Defines the side of the profile to which material should be added to construct the feature. This step is available when constructing a base feature.

Preview/Finish/Cancel

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.

Edit

Edits the profile of an existing cross section. This button is available only when editing a lofted feature.

Cross Section Order

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 re-order and then click the Up or Down button until it is in the correct position.

Note:

Use this dialog box to correct the order of cross sections that were created out-of-sequence. This can be especially helpful for adding a cross section to an existing lofted feature during an edit. You cannot use the re-ordering capability to create lofts that fold back on themselves.

Define Start Point

Defines 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.

Plane or Sketch Step

Specifies 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.

Draw Profile Step

Edits the profile for an existing feature. A profile is a 2D curve that defines the shape and location of the feature. This step is available only when you are editing an existing feature.

Finish/Cancel

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

Create-From Options

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 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 From Sketch Options

Select

Sets the method of selecting a sketch element.

• Single—Selects one or more individual elements.

• Chain—Selects 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.

Thickness

Specifies the thickness for the part. This option is only available during the initial creation of the base feature. You can change the default value for the thickness on the Gage tab of the Solid Edge Material Table dialog box.

Next

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

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 Feature command on the shortcut menu.