Revolve and Revolve Cut

You can add or remove material when you revolve profiles about an axis.

Before you begin: Create the profile and the revolve axis.
Profile
  • For a solid revolved feature, you can create a profile sketch from multiple intersecting profiles. You can select intersecting or nonintersecting sketches for the profile.
  • For a thin or surface revolved feature, you can create a profile sketch from multiple open or closed intersecting profiles.
  • Profiles cannot cross the axis.
Revolve Axis You can define the axis from the following:
  • A line, centerline, or construction line in a sketch
  • The edge of another feature
  1. From the Features section of the action bar, click Revolve or Revolve Cut .

    Tip: In the top menu of the dialog box, you can switch between Extrude , Revolve , and Sweep features.

  2. Select the feature options in the Revolve dialog box.
    OptionDescription
    Add. Creates a feature by adding multiple profiles.
    Cut. Creates a feature by subtracting one profile from another.
    New. Creates a feature from another feature.
    Solid. Creates a solid feature.
    Thin. Creates a feature with a constant wall thickness. To specify the wall thickness, drag the handle, or enter a value in the callout in the work area.

    You can specify the wall thickness to be equal in both directions from the profile's midplane by clicking Thin Midplane.

    Surface. Creates a feature with a zero-thickness wall.
  3. Select an edge, line, or axis for Revolve Axis.
  4. Select profiles to revolve.
  5. Select the revolve type and end condition.

    Not all end conditions are available in every situation.

    • Full Revolve. Extends the revolve 360º.

    • Blind. Extends the revolve to the specified angle. To specify the angle, enter a value in the callout, or drag the handle. To reverse the revolve direction, click the axis handle.

    • Midplane. Extends the revolve from the sketch plane the same amount in both directions. To specify the angle, enter a value in the callout or drag the handle.

    • Up To Geometry. Extends the revolve to the selected plane, feature, or sketch entity.

    • Up To Next. Extends the revolve to the next body.

    • Up To Body. Extends the revolve to the selected body.

  6. To specify the amount of rotation, specify an angle. To reverse the angle direction, click or double-click the rotation handle arrow.

    Note:

    The Dimension Edit Box is displayed as you revolve. Type the value for the angle and press Enter.

  7. Optional: To revolve in a second direction, expand Direction 2 and select one of the following options from the menu.
    • Off. Turns off Direction 2.
    • Blind. Extends the revolve for the specified distance.
    • Up to Geometry. Extends the revolve to the selected plane, feature, or sketch entity.
    • Up to Next. Extends the revolve to the next body.
    • Up to Body. Extends the revolve to the selected body.
    1. If Up to Geometry or Up to Body is selected, select an entity or body to which the revolve extends.
    2. If Offset is available, you can extrude the sketch profile an offset distance from the sketch plane's original position. To reverse the direction, click .
  8. To specify additional options, expand Advanced and select one of the following Start Conditions from the menu.

    Applies an optional offset for the revolve.

    • At Sketch. Revolves the sketch profile from the sketch's plane.
    • From Offset. Revolves the sketch profile an offset distance from the sketch plane's original position.
    • From Selected Geometry. Revolves the sketch profile an offset distance from the selected geometry.
  9. Optional: Select a merge option:
    1. Click Auto Merge to merge the revolve feature with all other possible bodies.
    2. If Auto Merge is not selected, select the bodies to merge with the revolve feature.
  10. Click .

 

See Also
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