Wrap Feature
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 Insert,
Features, Wrap.
In the PropertyManager, under Wrap
Parameters:
Select an option:
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.
To wrap the sketch normal to the sketch plane, leave Pull Direction blank.
Click OK
.