This feature wraps a sketch onto a planar or non-planar face. You can create a planar face from cylindrical, conical, or extruded models. You can also select a planar profile to add multiple, closed spline sketches. The wrap feature supports contour selection and sketch reuse. You can project a wrap feature onto multiple faces.
The sketch plane must be tangent to the face, allowing the face normal and the sketch normal to be parallel at the closest point.
To create a wrap feature:
- Select the sketch you want to wrap from the FeatureManager design tree.
The sketch to wrap can contain multiple, closed contours only. You cannot create a wrap feature from a sketch that contains any open contours.
- Click Wrap on the Features toolbar, or click .
- In the PropertyManager, under Wrap Parameters:
- Select an option:
||Creates a raised feature on the face.
||Creates an indented feature on the face.
||Creates an imprint of the sketch contours on the face.
- Select a non-planar face in the graphics area for Face for Wrap Sketch .
- Set a value for Thickness .
- Select Reverse direction, if necessary.
- If you select Emboss or Deboss, you can select a line, linear edge, or plane to set a Pull Direction . For a line or linear edge, the pull direction is the direction of the selected entity. For a plane, the pull direction is normal to the plane.
|Pull direction - Plane A
||Pull direction - Plane B
To wrap the sketch normal to the sketch plane, leave Pull Direction
- Click OK .