Part Modeling > Base Features > Revolve > Basics of the Revolve Feature > About the Revolve Feature
About the Revolve Feature
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.