About the Extrude User Interface for Sheetmetal Design
The Extrude user interface in Sheetmetal Design consists of commands, tabs, and shortcut menus. To access the Extrude tool, click > 
Extrude.
Extrude.Commands
• Depth options:
◦ 
Variable—Extrudes a section from the sketch plane by a specified value.
Variable—Extrudes a section from the sketch plane by a specified value.◦ 
Symmetric—Extrudes a section on both sides of the sketch plane by half the specified depth value in each direction.
Symmetric—Extrudes a section on both sides of the sketch plane by half the specified depth value in each direction.◦ 
To Reference—Extrudes a section in the first direction of the specified reference to the selected point, curve, plane, or surface of a solid geometry.
To Reference—Extrudes a section in the first direction of the specified reference to the selected point, curve, plane, or surface of a solid geometry.◦ 
—Flips the depth direction of the extrude to the other side of the sketch.
—Flips the depth direction of the extrude to the other side of the sketch.• Thickness options:
◦ 
box—Sets the thickness of the extruded surface.
box—Sets the thickness of the extruded surface.◦ —Flips the material direction.
—Flips the material direction.Tabs
• Placement—Displays the selected section in the collector. Click Define to sketch a new section. Click Edit to change an existing section.
• Options—Displays the following options:
◦ Depth—Displays depth options for Side 1 and Side 2 as follows:
▪ Variable—Extrudes a section from the sketch plane by a specified value.
Variable—Extrudes a section from the sketch plane by a specified value.▪ Symmetric—Extrudes a section on both sides of the sketch plane by half the specified depth value in each direction.
Symmetric—Extrudes a section on both sides of the sketch plane by half the specified depth value in each direction.▪ To Reference—Extrudes a section in the first direction of the specified reference to the selected point, curve, plane, or surface of a solid geometry.
To Reference—Extrudes a section in the first direction of the specified reference to the selected point, curve, plane, or surface of a solid geometry.◦ Add taper—Tapers the geometry by value.
◦ Sheetmetal options—Available for unattached extruded walls. Options are as follows:
▪ Add bends on sharp edges—Rounds sharp edges. Set the value for the radius and the dimensioning scheme of the radius.
▪ Merge to model—Merges the wall geometry to an existing wall in the design.
Keep merged edges—Does not merge wall edges to existing wall edges.
Keep edges of bends—Keeps the edges between existing bend surfaces and new geometry being created.
▪ Do not merge to model—Does not merge the wall geometry to an existing wall in the design.
▪ Set driving surface opposite sketch plane—Sets driving surface opposite sketch plane.
• Bend Allowance—Displays the following options:
◦ Use part settings—Uses the developed length calculation set for the part.
◦ Use feature settings—Uses the developed length calculation defined below.
▪ By K factor—Calculates the developed length according to the K factor. To change the value for K factor, type a new factor value or select a value from the list.
▪ By Y factor—Calculates the developed length according to the Y factor. To change the value for Y factor, type a new factor value or select a value from the list.
▪ By bend table—Calculates the developed length using a bend table. To choose a different bend table, select one from the list.
◦ Developed length for arcs—Calculates developed length for arcs. To use a bend table to calculate developed length for arcs, click Use bend table. Use the default table or select another one from the list.
 | • Only bend tables copied to the part are available. • Use the Preference dialog box to copy a bend allowance table to the model. |
• Properties—Displays detailed feature information:
◦ Name—Shows a name for the wall.
◦ 
—Shows feature information in a browser.
—Shows feature information in a browser.Shortcut Menus
Click in the graphics window to access the mini toolbar commands. Right-click in the graphics window to access the shortcut commands.
• 
—Opens Sketcher to edit an existing sketch.
—Opens Sketcher to edit an existing sketch.• Add taper—Tapers the geometry by value.
• Clear—Removes the reference in the active collector.
• Flip Depth Direction—Flips the depth direction of the extrude to the other side of the sketch.
• Side 1 Depth—Specifies one of the depth types Blind, Symmetric, or To Selected.
• Side 2 Depth—Specifies one of the depth types Blind, To Selected, or None.
• Side 2—Selects side 2.
• Show Section Dimensions—Displays the dimensions of the section.
Right-click the handle to access the following shortcut commands. Selections change depending on the depth option chosen:
• Blind—Extrudes a section from the sketch plane by a specified value.
• Symmetric—Extrudes a section on both sides of the sketch plane by half the specified depth value in each direction.
• To Selected—Extrudes a section in the first direction of the specified reference to the selected point, curve, plane, or surface of a solid geometry.