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.
![](doc1292868040210.image)
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.
![](doc1292868039084.image)
- Click Wrap
on the Features toolbar, or click .
- In the PropertyManager, under Wrap Parameters:
- Select an option:
Option |
Description |
Emboss |
Creates a raised feature on the face. |
Deboss |
Creates an indented feature on the face. |
Scribe |
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.
![](doc1292868039928.image)
- 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.
![](doc1292868037834.image) |
![](doc1292868038584.image) |
Pull direction - Plane A |
Pull direction - Plane B |
To wrap the sketch normal to the sketch plane, leave
Pull Direction ![](doc1292867501019.image)
blank.
![](doc1292868039506.image)
- Click OK
.![](doc1292868040710.image)