Creating a Bead

This task shows you how to create a bead, that is a local deformation in the web.

If you use the Generative Sheetmetal Design workbench, open the NEWStamping6.CATPart document.
If you use the Aerospace SheetMetal Design workbench, open the Aero_Stamping6.CATPart document.

  1. Click Bead in the Cutting/Stamping toolbar (Stamping sub-toolbar).

  2. Select the spine profile where you want to place the bead.

    The Bead Definition dialog box is displayed, providing default values.
     

  3. Change the value in the different fields, if needed:

    • Section radius R1 (corresponding to the cross section value)

    • End radius R2

    • Height H

    • Radius R

    You can use 0 as the Radius value to deactivate the Radius R value, and to create the bead without a fillet.

    The Profile is automatically set to the sketch you chose.

    The vector for the direction of the bead is shown in the model and a preview of the bead appears. A vector shows its direction.

    The vector cannot be reverted until the bead spine is defined.

  4. Click Preview to visualize the bead.

  5. Click OK to validate.

    The bead (identified as Bead.xxx) is created and the specification tree is updated accordingly.
 

More about Beads

  • You can also create a bead using a 3D curve such as shown here:
  • You can also create a bead with a fillet on a profile whose edges intersect. When you select the intersecting profile, the Bead Definition dialog box is updated and a new Radius r option is added:



    Select the Radius r check box and define the radius value of the fillet in the field.

    Fillets are displayed on the intersecting edges as shown below:

  • Refer to Editing the Sheet and Tool Parameters to define the Standards Files.