Revolve a solid body

Learn how to use the Revolve tool to create a solid body in Fusion.

1. On the toolbar, click Solid > Create > Revolve .

   The Revolve dialog displays.

2. In the canvas, select a coplanar sketch profile or face to revolve.

3. In the canvas, select a linear sketch curve, edge, cylindrical face, or axis to revolve around.

4. In the dialog, select an Extent Type setting, and adjust its associated settings:

   • Partial: Revolves the profile around the axis to an angle value that you specify.
     • Direction: Select a direction setting.
       • One Side: Revolves profile on one side of the profile plane.
       • Two Sides: Revolves profile on each side of the profile plane.
       • Symmetric: Revolves profile symmetrically on each side of the profile plane.
     • Angle: Drag the manipulator handle or type a value to specify the angle of revolution.
   • To Object: Revolves to a body, face, or plane that you select.
     • Direction: Select One Side or Two Sides .
     • Angle: (To) Select body, face, plane, or vertex to revolve to.
   • Full: Revolves the profile 360 degrees around the axis.

5. Select an Operation type, and adjust its associated settings:

   • Join: Combines the new body with an existing body.
   • Cut: Removes an area from an existing body.
     • Objects to Cut: Check or uncheck objects to cut.
   • Intersect: Creates a body at the intersection of an existing body and the new body.
     • Objects to Cut: Check or uncheck objects to cut.
   • New Body: Creates a new body in the active component.
   • New Component: Creates a new body in a new component.

6. Click OK.

The revolved solid body displays in the canvas.

Tips

• Use Project Axis to project the axis to the same plane that the revolved profile is on. Uncheck to keep the axis in its original location.

Left: Check Project axis	Right: Uncheck Project Axis