Sweep and Sweep Cut

Context:

Profile: You can define the profile from sketch entities, sketch regions, or planar faces. Profiles must be closed for solid sweep features. 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.

From the Features section of the action bar, click Sweep or Sweep Cut .

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

Select the feature options in the Sweep dialog box.

Option	Description
	Add. Creates a feature by adding multiple profiles.
	Cut. Creates a feature by subtracting one profile from another. Note: You cannot apply cut feature to a sheet metal geometry.
	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.

In the dialog box, click Path, and select the path to sweep along.
To remove material with the sweep, select Cut.
Select profiles to sweep.

Note: You cannot apply sweep feature to a sheet metal geometry.
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 typing 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.
Optional: To extend the sweep along a path of tangent edges, select Tangent Propagation.

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

To apply an optional offset to the sweep, expand Start Offset and End Offset and select from 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.
  Note: You can select a face from a sheetmetal geometry for the sweep feature.
Note:
The Dimension Edit Box is displayed as you sketch. Type the value for the dimension and press Enter.
Click .