Creating a Revolve

You can create a revolve by a rotational sweep of an open or closed profile. The rotation is based on a desired sweep angle around an axis.

This task shows you how to define a revolve.

Before you begin: Open a 2D sketch or surface.
See Also
Creating a Shellable Feature
  1. Launch any capability requiring a shape definition. For example, from the Create section of the action bar, click Shellable Feature , then click Revolve in the Shellable Feature dialog box that appears.

    All the shape features require a Profile/Surface as a part of the revolve geometry definition. You can select an existing sketch or surface in Profile/Surface field.

    Tips:
    • If no profile is defined, click Positioned Sketch to sketch the profile you need.
    • You can also select:
      • Any face originated by functional features of any solid functional set. In this case, the face needs to be the original untrimmed (unmerged) of the feature.
      • Any topological (trimmed) face of any Part Design body that is not the Part Body containing the active solid functional set.

    You can also select any face originated by functional features of any functional body. In this case, the face needs to be the original untrimmed (unmerged) of the feature.

    You can also select any topological (trimmed) face of any Part Design body that is not the PartBody containing the active solid functional set.

  2. Select the profile or surface you want to revolve.

    By default, the app specifies the length of your revolve feature and previews limits as Limit 1 and Limit 2.

  3. By default, the first angle value is 360 degrees. In the Limits tab, enter the required values in the First angle and the Second angle boxes as per the requirement.
  4. In the Axis selection box, select the axis for the revolve.
  5. Click to reverse the direction of the revolve.

    Tip: You can also reverse the revolve direction using handles in the work area.

  6. In the Fillet tab,
    • Select the Lateral radius check box to fillet lateral edges and set the radius value.

    • Select the First radius check box to fillet top edges and set the radius value

    • Select the Second radius check box to fillet the opposite bottom edges and set the radius value.

    • From the Type list under Intersection Fillet, select a type and specify the required parameters.
  7. Under Thin Properties,
    1. Select the Use param for thin feature check box to specify the thin feature parameters.
    2. In the Reference list in the Thin Properties tab, select the required reference.

    Following reference options are available:

    • Neutral Fiber to apply lateral fillet radius at neutral fiber.
    • Outside Thickness to apply lateral fillet radius at outside thickness face.
    • Inside Thickness to apply lateral fillet radius at inside thickness face.
    • If you enter a value in Inside Thickness, thickness is evenly distributed to both sides of the profile.

    • If you select Outside Thickness from the Reference list and enter a value, thickness outside the profile can be varied and the thickness you defined for Inside Thickness is added to the inside of the profile.

    Important: The Core command enables you to define a core body (offset) for a shellable feature.