About the Extrude User Interface
The Extrude tab consists of commands, tabs, and shortcut menus. Click > 
Extrude to open the Extrude tab.
Extrude to open the Extrude tab.Commands
• Type
◦ 
Solid—Creates a solid extrude.
Solid—Creates a solid extrude.◦ 
Surface—Creates a surface extrude.
Surface—Creates a surface extrude.• Depth
◦ Side 1 depth options:
▪ 
Variable—Extrudes a section from the sketching plane to the specified depth value.
Variable—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.
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.
To Next—Extrudes a section from the placement reference to the first surface that it reaches. | This option is not available in these cases: • Cut geometry from body is on the Body Options tab, and All is selected • Cut geometry from body is on the Body Options tab, and more than one body is in the Selected collector • In Assembly mode |
▪ 
Through All—Extrudes a section from the placement reference to the last surface it reaches.
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.
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 these cases: • Cut geometry from body is on the Body Options tab, and All is selected • Cut geometry from body is on the Body Options tab, and more than one body is in the Selected collector • In Assembly mode |
▪ 
To Reference—Extrudes a section to a selected point, curve, plane, surface, quilt, or body, or to an offset or a translation of a selected reference.
To Reference—Extrudes a section to a selected point, curve, plane, surface, quilt, or body, or to an offset or a translation of a selected reference.▪ Reference collector—Displays the point, curve, plane, surface, quilt, or body that defines the extrude depth.
◦ 
—Flips the extrude depth direction to the other side of the sketch.
—Flips the extrude depth direction to the other side of the sketch.◦ 
Capped Ends—Closes each end of the feature when it is created as a Surface feature and the section is closed.
Capped Ends—Closes each end of the feature when it is created as a Surface feature and the section is closed.• Settings
◦ 
—Flips the side of the sketch to which to add material. Available when adding material using an open sketch whose endpoints intersect geometry, creating a closed volume.
—Flips the side of the sketch to which to add material. Available when adding material using an open sketch whose endpoints intersect geometry, creating a closed volume.◦ 
Remove Material—Removes material along the extrude to create a cut for a solid feature, or a quilt trim for a surface feature.
Remove Material—Removes material along the extrude to create a cut for a solid feature, or a quilt trim for a surface feature.▪ 
Solid
Solid▪ —Flips the side from which to remove material from one side of the sketch to the opposite side.
—Flips the side from which to remove material from one side of the sketch to the opposite side.▪ 
Surface
Surface▪ 
—Switches the side from which to remove material from one side, the other side, or keep both sides of the sketch.
—Switches the side from which to remove material from one side, the other side, or keep both sides of the sketch.▪ Quilt collector—Collects a quilt from which to remove material.
▪ —Flips the side of the quilt that retains the identity of the original quilt when material is removed from both sides of the quilt.
—Flips the side of the quilt that retains the identity of the original quilt when material is removed from both sides of the quilt.◦ 
Thicken Sketch—Adds a thickness to a sketch to create a thickened solid, a thickened solid cut, or a thickened surface trim.
Thicken 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.
—Switches the thicken direction to one side, the other side, or both sides of the sketch.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 Variable or Symmetric.
Variable or Symmetric.▪ Reference collector—Displays a depth reference when the depth option is Through Until or To Reference.
Through Until or To Reference.▪ Extrude options when the depth option is To Reference
To Reference▪ 
—Extrudes to a selected point, curve, plane, surface, quilt, or body.
—Extrudes to a selected point, curve, plane, surface, quilt, or body.▪ 
—Extrudes to an offset of a selected point, curve, plane, surface, quilt, or body.
—Extrudes to an offset of a selected point, curve, plane, surface, quilt, or body.▪ 
—Extrudes to a translation of a selected point, curve, plane, surface, quilt, or body.
—Extrudes to a translation of a selected point, curve, plane, surface, quilt, or body.▪ Value box—Sets an offset or translation distance value when the extrude option is or .
or .▪ —Flips the direction of the offset or translation when or is selected.
—Flips the direction of the offset or translation when or is selected.◦ Capped ends check box—Closes each end of the feature when it is created as a Surface feature and the section is closed.
Surface feature and the section is closed.◦ 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.
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°.
• Body Options
Available when the feature is created as a solid. Not available for creating assembly-level features.
◦ Add geometry to body—Displayed when geometry is added.
▪ Create new body check box—Creates the feature in a new body.
▪ Body collector
▪ Selects the body to which geometry is added when you add the feature to an existing body. The default body is displayed, unless you select a different body.
▪ Shows the name of the new body when you create the feature in a new body.
◦ Cut geometry from body—Displayed when geometry is removed.
▪ All—Cuts geometry from all the bodies that the feature passes through.
▪ Selected—Cuts geometry from the selected bodies. The default body is displayed, unless you select a different body or bodies.
▪ Body collector—Selects the body from which geometry is removed.
| | The body that is selected in the collector on the Body Options tab cannot be used as a depth reference. |
• Properties
◦ Name box—Sets a name for a feature.
◦ 
—Displays detailed component information in a browser.
—Displays detailed component information in a browser.Shortcut Menus
Right-click the graphics window to access shortcut menu commands.
• Clear—Clears the active collector.
• Solid—Switches from surface geometry to solid.
Solid—Switches from surface geometry to solid.• Surface—Switches from solid geometry to surface.
Surface—Switches from solid geometry to surface.• 
Remove Material—Removes material along the extrude to create a cut for a solid feature or a quilt trim for a surface feature.
Remove Material—Removes material along the extrude to create a cut for a solid feature or a quilt trim for a surface feature.• Thicken Sketch—Adds a thickness to a sketch to create a thickened solid, a thickened solid cut, or a thickened surface trim.
Thicken Sketch—Adds a thickness to a sketch to create a thickened solid, a thickened solid cut, or a thickened surface trim.• 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.
• 
Define Internal Sketch—Opens Sketcher so you can create an internal sketch.
Define Internal Sketch—Opens Sketcher so you can create an internal sketch.• Edit Internal Sketch—Opens the internal sketch in Sketcher for editing.
Edit Internal Sketch—Opens the internal sketch in Sketcher for editing.• 
Add Taper—Toggles adding a taper off or on.
Add Taper—Toggles adding a taper off or on.• Capped Ends—Closes each end of the feature when it is created as a Surface feature and the section is closed.
Capped Ends—Closes each end of the feature when it is created as a Surface feature and the section is closed.• Select bodies—Activates the body collector so you can select bodies.
• Create new body—Creates the feature in a new body.
• All—Removes geometry from all the bodies that the feature passes through.
• Selected—Removes geometry from the selected bodies.
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.
• Depth1 Reference Collector—Activates the Side 1 reference collector when the depth option is To Reference or Through Until.
To Reference or Through Until.• Depth2 Reference Collector—Activates the Side 2 reference collector when the depth option is To Reference or Through Until.
To Reference 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.
• Variable—Sets the depth option to Variable.
Variable.• Symmetric—Sets the depth option to Symmetric.
Symmetric.• To Next—Sets the depth option to To Next.
To Next.• Through All—Sets the depth option to Through All.
Through All.• Through Until—Sets the depth option to Through Until.
Through Until.• To Reference—Sets the depth option to To Reference.
To Reference.• Other Side—Sets the depth option on the other side of the sketching plane.