Creating Walls from a Sketch

This task shows you 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, Grid area.

1. Click Sketch 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 in the Walls toolbar.

   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 available only when the sketch is set at extreme position.

7. Click OK.

   The feature Wall.1 is added in the specification tree.
   	The first wall of the Generative Sheetmetal Design part is known as the Reference wall.
   	Click Sketch from the Wall Definition dialog box, if you want 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 However, note that the emptied area is part of the wall and is not a separate cutout that can be edited.