Revolve is a method of defining three-dimensional geometry by revolving a sketched section around a centerline. Use the Revolve tool to create a solid or surface feature, and to add or remove material. You can create the following revolve types:
• Revolved protrusion—Solid, Thickened
• Revolved cut—Solid, Thickened
• Revolved surface
• Revolved surface trim—Regular, Thickened
A revolved section requires an axis of revolution that can be created either with the section or defined by selecting model geometry.
Legacy revolved features that were defined using the Constant angle option are automatically converted to Variable.
Activating the Revolve Tool
There are several ways to activate the Revolve tool:
• Click Model > Revolve and create a sketch to revolve. This method is referred to as action-object.
• Select an existing sketch and then click Model > Revolve. This method is referred to as object-action.
• Select a datum plane or planar surface to use as the sketching plane and then click Model > Revolve.
A preview of the feature is displayed in the graphics window. You can adjust the feature as needed by changing the angle of revolution, switching between a solid or surface, switching between protrusion or cut, or assigning a thickness to the sketch to create a thickened feature.
Creating a Two-Sided Feature
You can create a two-sided feature that is constructed on both sides of the sketching plane, with an angle option defined for each side.
To create a two-sided feature, start creating a revolved feature with an angle option defined for one side. Then click the Options tab, or right-click the graphics window or a drag handle, and define the angle of revolution for the second side.