Creating a Sweep Surface

You can use a sweep feature to add or remove material as the profile moves along a path. Before you create a sweep feature, first create the profile and the path.

Before you begin:
Profile
  • You can define the profile from sketch entities, sketch regions, or planar faces.
  • Solid sweep features require closed profiles.
  • Profiles can be open or closed for thin and surface sweep features.
Path You can define an open or closed sweep path from sketched curves contained in a sketch, or from model edges.
  1. From the Surfaces section of the action bar, click Sweep Surface .

    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 Sweep 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 set the wall thickness, drag the handle, or enter a value in Thickness. You can reverse the wall direction inward or outward by clicking .

    You can set 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. In the dialog box, click Path, and select the path to sweep along.

    To remove material with the sweep, select Cut.

  4. Select profiles to sweep.
  5. Select the Path options.
    • Follow Path. Keeps the profile at the same angle with respect to the path.
    • Keep Normal Constant. Keeps the profile parallel to the plane of the profile sketch.
    • Twist With Angle. Twists the profile along the path. Specify the twist angle by entering a positive or negative value in the callout in the work area.
    • Keep Alignment. Keeps the profile aligned to a selected direction vector. To define the direction vector, select a plane, planar face, or line for Select alignment direction.
  6. Optional: To extend the sweep along a path of tangent edges, select Tangent Propagation.
  7. Optional: To extend the sweep along a curve when you add an offset to a curved path, click Curvature Extension. The resulting sweep feature is curvature continuous at the junction with the extension.

    No offset

    Offset without Curvature Extension

    Offset with Curvature Extension

  8. To apply an optional offset to the sweep, expand Start Offset and End Offset and select the following.
    • Percentage. Offsets the start or end of the sweep by the specified percentage of the length of the path.
    • Length. Offsets the start or end of the sweep by the specified distance.
    • Up to Geometry. Extends the start or end of the feature to the selected plane, feature, or sketch entity.
  9. Optional: Select a merge option:
    1. Click Auto Merge to merge the sweep feature with all other possible bodies.
    2. If Auto Merge is not selected, select the bodies to merge with the sweep feature.
  10. Click .

 

See Also
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