Creating a Base Flange

To create a sheet metal part, you sketch an open profile and use the base flange feature to create the thin feature and the bends.

When you develop a sheet metal part, you generally design the part in the folded state. This allows you to capture the design intent and the dimensions of the finished part.

  1. Open a new part.
  2. Click Base Flange/Tab (Sheet Metal tab).
  3. Select the Front Plane.
    A sketch opens on the Front Plane.
  4. Sketch and dimension the profile.
    To draw the line with its midpoint at the origin, click Line (Sketch tab). In the Insert Line PropertyManager, under Options, select Midpoint line. Click on the origin to place the midpoint, then click again to place an endpoint.
  5. Click Exit Sketch (Sketch tab).
  6. In the PropertyManager, under Direction 1:
    1. Select Blind in End Condition.
    2. Set Depth to 75.
  7. Under Sheet Metal Parameters:
    1. Set Thickness to 3.
    2. Set Bend Radius to 1.
  8. Click .
    The sketch is extruded and the bends are added.