Wrap

You can choose between two methods to create a wrap feature.

The Analytical method 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 sketch plane must be tangent to the face, allowing the face normal and the sketch normal to be parallel at the closest point.

The Spline Surface method wraps a sketch on any face type. A limitation with this method is that it cannot wrap around a model.

 
Analytical   Spline Surface

Both methods support sketch reuse.

To create a wrap feature using the Analytical method:

  1. 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.
  2. Click Wrap on the Features toolbar, or click Insert > Features > Wrap.
  3. In the PropertyManager, under Wrap Type:
    1. 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.
    2. Under Wrap Method, select Analytical .
    3. Select a non-planar face in the graphics area for Face for Wrap Sketch , under Wrap Parameters.
    4. Set a value for Thickness .
    5. Select Reverse direction, if necessary.
  4. 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 blank.
  5. Click OK .

Using Scribe to Imprint Single-Line Fonts

You can create wrap features from sketches that use single-line fonts, also called stick fonts.

To use Scribe to imprint single-line fonts:

  1. Open a model onto which you want to imprint some text using a single-line font.
  2. Click Insert > Features > Wrap .
  3. In the PropertyManager:
    1. Under Wrap Type, select Scribe .
    2. Under Wrap Parameters, for Source Sketch , select the sketch that contains a single-line font.
    3. For Face for Wrap Sketch, select a face.
    The software imprints the text on the face using the single-line font.

  4. If text or characters do not display properly, check if your stick font is an authentic, single-line font supported by the Wrap feature. To check:
    1. Open the sketch.
    2. Right-click the sketch text and select Dissolve Sketch Text.
    3. In the graphics area, select the text entities to display their properties.
      Unsupported characters show multiple entities for what appears to be a single line.

Creating Wrap Geometry on Any Face

This example uses the Spline Surface method to wrap a sketch along six faces of the model.

To create wrap geometry on any face:

  1. Click Wrap (Features toolbar) or Insert > Features > Wrap.
  2. In the graphics area, select the SOLIDWORKS sketch.
  3. In the PropertyManager:
    1. For Wrap Type, click Emboss .
    2. For Wrap Method, click Spline Surface .
  4. Select the faces along the top handle of the iron. There are a total of six.

  5. In the PropertyManager, under Wrap Parameters, set the Thickness to 2mm and click .