Mapping Elements

This task shows how to map curves or points onto a Sheet Metal part. These curves or points can be wireframe or sketcher elements.
This is especially useful when:
  • you want to define an area for chemical milling,
  • you want to create a circular hole on the unfolded part at a given center point defined in the folded view,
  • you want to generate a logotype.
Open the Aero_Mapping.CATPart document.

This sample already contain a point pre-defined in a sketch that will be mapped onto the part.

  1. Make sure the sketch is selected, and click Point or Curve Mapping .

    The Unfold object definition dialog box is displayed, indicating which elements have been selected for mapping.
    To add elements in the object(s) list, click on Add Mode and select an element in the geometry or the specification tree.

    To remove elements in the object(s) list, click on Remove Mode and select an element in the geometry or the specification tree.

    The curve mapping is previewed as if the surfacic flange onto which it has been drawn was unfolded.
    You can manage the list of objects if several are available:
    • to remove an object, select it from the list and use the Clear selection contextual menu
    • to add an object, select it directly in the geometry.
      Order in the list does not matter. 
    The Support is not necessarily the support element on which the element to be mapped has been drawn. Indeed, by default, the Support  is the last Sheet Metal feature that has been created or modified, that is the current feature in the specification tree.
  2. Click OK.

    The curve mapping is created and added in the specification tree.
  3. Click Fold/Unfold .

  4. Click Hole .

  5. Select Unfolded point.1 as the center of the hole and the surfacic flange as the hole's support.

  6. Click OK to create the hole.

  7. Click again Fold/Unfold to display the 3D view of the part.

    You can select several sketches/curves/points to be mapped at a time.