Revolve

The Revolve command creates solid or surface features having radial symmetry such as stepped shafts and enclosures.

Revolve creates features by sweeping sketch and model geometry around an axis. The selection can be revolved through any angle measuring between zero and 360 degrees.

The axis can be a line in the profile, or a separate entity. An offset axis results in an axial hole in the feature. The axis cannot cross the region.

Create a revolved solid

1. Click the drop-down arrow under Extrude, and then click Revolve.
2. Select one or more sketch profiles or model faces. Multiple selections must be coplanar and in the same component. Sketch profiles must be in the same sketch.
3. Select the axis for the revolution. If the selected axis is not on the sketch plane, the axis is temporarily projected to the plane.
4. Select the Limit type. Use the manipulator to set the rotation angle, or enter the value.
   • Distance A numeric value for the angle.
   • To Determines the angle when select a face or work plane.
   • Full Determines the angle by the furthest face in the model.
5. Select the Direction
   • One DirectionCreates the revolve feature in one direction.
   • Two Directions Creates the revolve feature in both directions. Each direction can have a different angle.
   • Symmetric Creates the revolve feature in both directions. Each direction has the same angle.
6. Select the Boolean Option
   • Join Adds material.
   • Cut Removes material.
   • Intersect Removes all material from the solid that does not overlap the new feature.
   • New Component Creates a child component in the active component.

Create a revolved surface

1. Click the drop-down arrow under Extrude, and then click Revolve.
2. Select one or more sketch profiles, sketch entities, model faces, or model edges. Multiple selections must be coplanar and in the same component. Sketch profiles and entities must be in the same sketch.
3. Select the axis for the revolution. If the selected axis is not on the sketch plane, the axis is temporarily projected to the plane.
4. Select the Limit type. Use the manipulator to set the rotation angle, or enter the value.
   • Distance A numeric value for the angle.
   • To Determines the angle when select a face or work plane.
   • Full Determines the angle by the furthest face in the model.
5. Select the Direction
   • One DirectionCreates the revolve feature in one direction.
   • Two Directions Creates the revolve feature in both directions. Each direction can have a different angle.
   • Symmetric Creates the revolve feature in both directions. Each direction has the same angle.
6. Set the Creation Option to New Surface or New Component.