Generating Final Holes and Pads

This chapter deals with the rules the Generate Final Holes and Pads tool must comply with. This tool allows you to:
  • use a simplified representation of holes/pads throughout the construction of your mold to improve performances,
  • and replace this simplified representation by the actual holes/pads when you are finished with the construction:
    • select the required plates and launch the tool,
    • the actual holes/pads are created and the simplified representations are removed.

The Generate Final Holes and Pads tool:

  • is proposed for a CATPart or a CATProduct (the command takes all the children CATParts of the CATProduct into account).
  • is available through the Tools menu or the contextual menu of the plates,
  • applies to Assemble or Add/Remove operations on drilling bodies named TapHole*, DrillHole*, Pocket*, Pad*
    (those names are compulsory),
  • is used at the end of the construction of the mold,
  • cannot be undone (once the actual holes/pads are created, you cannot revert to their simplified representation).

The simplified representation of holes and pads:

  • is managed only by the Drill from/To/Between From and To capability,

    and not by the Drill Component and the Distributed Drill Component tools,
  • is ignored if it is empty or missing,
  • appears in plates with the same visibility as they have in the component,
  • must be published to be taken into account,
  • a drilling body is compulsory for each simplified representation of holes and pads.

You must create this simplified representation:

  • in a Geometrical Set in the CATPart of the component,
  • the drilling bodies of the component must be named TapHole*or DrillHole*or Pocket* or Pad* (those names are compulsory),
  • the name of Geometrical Set containing the definition of the simplified representation is NameOfDrillingBody_S*,
    e.g. the Geometrical Set containing the simplified representation of DrillHole* is named DrillHole_S*, that of Pocket1 is named Pocket_S1.
  • the simplified representation is defined by points, sketch, lines and curves.
    At least one of those elements must be present in the Geometrical Set, otherwise the simplified representation is ignored.

The simplified representation will be used automatically whenever applicable.
Its position is defined with respect to the component.
The component does not know which plates are impacted, therefore the simplified representation may appear distant from the plate it will drill.

If the simplified representation is useful to understand the design quickly, it is useful to see the plates from the Z direction of the die or to create very long lines in the direction of the component axis.
If this visualization is not required, we recommend you create the simplified representation in NoShow in the component.

Specific behavior:

  • If the component is de-activated, the simplified representation is also de-activated,
  • Delete command: the simplified representation is deleted in the corresponding plates,
  • Replace/Add new instance/Add new reference/Isolate capabilities: the behavior of the simplified representation is that of the standard holes,
  • Edition: the simplified representation is managed as in creation.