Part Modeling > Base Features > Extrude > Basics of the Extrude Feature > About the Extrude User Interface
  
About the Extrude User Interface
The Extrude tab consists of commands, tabs, and shortcut menus. Click Model > Extrude to open the Extrude tab.
Commands
—Creates a solid extrude.
—Creates a surface extrude.
Side 1 depth options:
Blind—Extrudes a section from the sketching plane to the specified depth value.
Value box—Sets the depth value for Side 1.
Symmetric—Extrudes a section on each side of the sketching plane by half of the specified depth value in each direction.
Value box—Sets the depth value for Side 1.
To Next—Extrudes a section from the placement reference to the first surface that it reaches.
 
* This option is not available in Assembly mode.
Through All—Extrudes a section from the placement reference to the last surface it reaches.
Through Until—Extrudes a section to intersect with a selected surface.
Reference collector—Displays the surface that defines the extrude depth.
 
* This option is not available in Assembly mode.
To Selected—Extrudes a section to a selected point, curve, plane, or surface, or to an offset or a translation of a selected reference.
Reference collector—Displays the point, curve, plane, or surface that defines the extrude depth.
—Flips the extrude depth direction to the other side of the sketch.
—Removes material along the extrude to create a cut for a solid feature or a quilt trim for a surface feature.
—Flips the remove functionality to remove material from the opposite side of the sketch.
—Adds a thickness to a sketch to create a thickened solid, a thickened solid cut, or a thickened surface trim.
Value box—Sets a thickness value.
—Switches the thicken direction to one side, the other side, or both sides of the sketch.
Quilt collector—Displays a quilt to trim when and are selected.
(to the left of the Quilt collector)—Switches the side of the quilt to remove to one side, the other side, or keep both sides of the quilt.
(to the right of the Quilt collector)—Toggles the side of a quilt to retain the ID of the original quilt if you keep both sides of the quilt.
Tabs
Placement
Sketch collector—Displays the sketch that defines the extrude feature.
Define—Opens Sketcher so you can create an internal sketch.
Edit—Opens the internal sketch in Sketcher for editing.
Unlink—Breaks the association with the selected sketch and copies the sketch as an internal sketch.
Options
Side 1 and Side 2—Sets the depth option on Side 1 or Side 2 of the reference.
Value box—Sets a depth value when the depth option is Blind or Symmetric.
Reference collector—Displays a depth reference when the depth option is Through Until or To Selected.
Extrude options when the depth option is To Selected
—Extrudes to a selected point, curve, plane, or surface.
—Extrudes to an offset of a selected point, curve, plane, or surface.
—Extrudes to a translation of a selected point, curve, plane, or surface.
Value box—Sets an offset or translation distance value when the extrude option is or .
—Flips the direction of the offset or translation when or is selected.
Capped Ends check box—Closes each end of an extrude feature when is selected.
Section end point 1 and Section end point 2—Highlights the corresponding end point in the graphics window when you point to the label. Available when thicken sketch is selected, the sketch is open, one or both sketch end points intersect the model solid geometry, and at least one surface can be used for capping and attaching the extrude feature.
Cap with model geometry check box—Caps and attaches thickened extruded geometry to the model.
Previous and Next—Switches between the surfaces that can be used to cap and attach the extruded geometry.
Add taper check box—Tapers the geometry by a value.
Value box—Sets the taper angle from -89.9° to 89.9°.
Properties
Name box—Sets a name for a feature.
—Displays detailed component information in a browser.
Shortcut Menus
Right-click the graphics window to access shortcut menu commands.
Define Internal Sketch—Opens Sketcher so you can create an internal sketch.
Edit Internal Sketch—Opens the internal sketch in Sketcher for editing.
Clear—Clears the active collector.
Surface—Switches from solid geometry to surface.
Solid—Switches from surface geometry to solid.
Remove Material—Toggles off and on.
Thicken Sketch—Toggles off and on.
Flip Depth Direction—Switches the direction of the feature creation to the other side of the sketching plane.
Flip Material Side—Switches the side of the sketch from which to remove material when creating a cut, or the side to which to add material when creating a protrusion.
Side 2—Toggles the Side 2 depth option on the Options tab.
Add taper—Toggles adding a taper off or on.
Right-click an extruded feature to access shortcut commands.
Placement Collector—Activates the Sketch collector.
Trim Quilt Collector—Activates the Quilt collector.
Intersection Components Collector—Defines the feature visibility and select the components that the feature will intersect in Assembly mode.
To Selected Depth1 Collector—Activates the Side 1 reference collector when the depth option is To Selected or Through Until.
To Selected Depth2 Collector—Activates the Side 2 reference collector when the depth option is To Selected or Through Until.
Right-click a directional arrow to access shortcut command.
Flip—Switches the direction of feature creation.
Right-click a drag handle to access shortcut commands.
Flip Depth Direction—Switches the direction of the feature creation in relation to the sketching plane.
Blind—Sets the depth option to .
Symmetric—Sets the depth option to .
To Next—Sets the depth option to .
Through All—Sets the depth option to .
Through Until—Sets the depth option to .
To Selected—Sets the depth option to .
Other Side—Sets the depth option on the other side of the sketching plane.