Creating Walls from a Sketch

This task shows how to create a wall from a sketch.

You must be in the Sheet Metal Workbench, with a .CATPart document open, and you must have defined the sheet metal parameters. 
Set the sketcher grid to H = 100mm and V = 100mm, using the Tools -> Options, Mechanical Design -> Sketcher, Sketcher tab.

  1. Click Sketcher then select the xy plane.

  2. Click Profile .

  3. Sketch the profile as shown below:

  4. Click Exit workbench to return to the 3D world.

  5. Click Wall .

    The Wall Definition dialog box opens.

    By default, the Material Side is set to the top.

  6. Select the desired profile positioning option:

    • Click to set the sketch at middle position of the wall thickness
    • Click to set the sketch at extreme position of the wall thickness
    The Invert Material Side button is only available when the sketch is set at extreme position.

  1. Click OK.

    The Wall.1 feature is added in the specification tree.
    The first wall of the Generative Sheetmetal Design Part is known as the Reference wall.
    • Click Sketcher from the Wall Definition dialog box, if you wish to directly edit the selected sketch. When exiting the sketcher, you then go back to the wall creation step, without having to reactivate the Wall icon.
      This is also very useful if you have selected an edge from a wall and clicked Wall .
      In this case, the sketcher is automatically activated displaying a square sketch constrained to the plane perpendicular to the support of the selected edge.
      You can then directly draw a sketch, then exit the sketcher and return to the wall creation step.
    • You can directly create a wall with a hole, by selecting a sketch with an inner profile (the profiles must not intersect):

      Sketch with inner profile

      Resulting wall
      Note however, that the emptied area is part of the wall and is not a separate cutout that can be edited.