Creating Points, Lines... as Parameters

You can create elements such as Points, Lines, Curves, Surfaces, Planes or Circles and use them in knowledgeware relations. This task shows you how to determine the position of the inertia axis of a pad.

This task shows you how to:

Related Topics
About Parameters
Creating a Parameter

Create a Line

You can create the line.

  1. Access the Part Design workbench, create any sketch in the yz plane, then extrude this sketch to create a pad. If need be, refer to the Part Design User's Guide.

  2. Create a line intended to be used as an inertia axis. To do so, click Formula , select Line in New Parameter of type scrolling list, then click New Parameter of type.

Determine the Inertia Axis of the Pad

You can determine the intertia axis.

  1. Select the line you have created (PartBody.1\Line.1).

  2. Click Add Formula and add the formula below in the editor: PartBody.1\Line.1 = inertiaAxis(3,PartBody)

    Important: The inertiaAxis function is accessible through the Line constructors. The axis number 3 is the one which is in the extrusion direction (normal to yz).

  3. Click OK in the Formulas dialog box. The inertia axis is displayed in the geometry area.

  4. Back to . Create three length type parameters: X, Y and Z.

Retrieve the Coordinates

You can retrieve the coordinates.

  1. Retrieve the coordinates of the point located at the intersection of the inertia axis and the 'yz plane'. To do so, create the formulas below:

    X=intersect(Geometrical Set.1\Line.1, 'yz plane').coord(1) Y=intersect(Geometrical Set.1\Line.1, 'yz plane').coord(2) Z=intersect(Geometrical Set.\Line.1, 'yz plane').coord(3)

    You get the intersect function from the Wireframe constructors and the point.coord method from the Measures item of the dictionary.

  2. Check the value displayed in the specification tree as well as in the Formulas dialog box.

    Important: To create elements such as Points, Lines, Curves, Surfaces, Planes or Circles and use them in knowledgeware relations, you can:

    • Create these elements as 'Isolate' elements in the Generative Shape Design workbench. 'Isolate' elements also called Datum are elements that have no link to the other entities that were used to create them. For information on 'Datum' type elements, see the Generative Shape Design User's Guide.

    • Create these elements by using the f(x) capabilities and select the right type of element from the New parameter of type list.