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
Model >
Extrude.
Commands
• Extrusion options:
◦ 
—Creates a solid.
◦ 
—Creates a surface.
• Depth options:
◦ 
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.
• The following additional depth options are available only for a second unattached extruded wall:
◦ 
To Next—Extrudes a section in the first direction up to the next surface.
◦ 
Through All—Extrudes a section in the first direction to intersect with all surfaces.
◦ 
Through Until—Extrudes a section in the first direction to intersect with a selected surface.
• 
—Flips the depth direction of the extrude to the other side of the sketch.
• —Flips the
material direction.
• 
—Removes material, displaying cut options.
◦ 
—Toggles between sheet metal and solid cuts. Select it to make the following sheet metal cuts available:
◦ 
—Removes material normal to both driving and offset surfaces.
◦ 
—Removes material normal to the driving surface.
◦ 
—Removes material normal to the offset surface.
• 
—Thickens the sketch by a specified value.
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:
▪ 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.
◦ The following additional depth options are available only for a second unattached extruded wall:
▪ Through All—Extrudes a section in the first direction to intersect with all surfaces.
▪ To Next—Extrudes a section in the first direction up to the next surface.
▪ Through Until—Extrudes a section in the first direction to intersect with a selected surface.
◦ Capped ends—Available only for quilts. Caps the quilt on both sides.
◦ Add taper—Tapers the extruded wall or surface.
◦ 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.
▪ Set driving surface opposite sketch plane—Flips the driving surface of the sheet metal wall. Use this option when the wall is not a first wall.
▪ Merge to model—Merges the wall geometry to an existing wall in the design. Keep merged edges—Wall edges are not merged with existing wall edges.
• To set feature-specific bend allowance and calculate the developed length using a different method from that of the part, perform the following operations:
1. Click Bend Allowance. The Bend Allowance tab opens.
2. Click Use feature settings.
3. Perform one of the following operations:
▪ Click By K factor or By Y factor and type a new factor value or select one from the list.
▪ To use a bend table to calculate developed length for arcs, click By bend table. Use the default table, select a new one from the list, or click Browse to browse to a different table.
|  Only bend tables copied to the part are available. |
• Properties—Displays detailed feature information:
◦ Name—Shows a name for the wall.
◦ 
—Shows feature information in a browser.
Shortcut Menus
Right-click the selected wall to access the following shortcut commands:
• Edit Internal Sketch—Opens Sketcher to edit an existing sketch.
• Clear—Removes the reference in the active collector.
• Solid—Extrudes surface geometry as a solid.
• Flip Depth Direction—Flips the depth direction of the extrude to the other side of the sketch.
• Surface—Extrudes solid geometry as a surface.
• Add taper—Tapers the extruded wall or surface.
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 Next—Extrudes a section in the first direction up to the next surface.
• Through All—Extrudes a section in the first direction to intersect with all surfaces.
• Through Until—Extrudes a section in the first direction to intersect with a selected surface.
• 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.
Right-click the graphics window to access the following shortcut commands:
• Define Internal Sketch—Opens Sketcher to create a sketch.
• Remove Material—Creates a cut using the extruded volume.
• Sheetmetal Cut—Creates a sheet metal cut.
• Thicken Sketch—Assigns a thickness to the section outline.