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



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.

Create a line intended to be used as an inertia axis
afterwards.

To do so, click the Formulas icon , select the Line item
in New Parameter of type, then click New Parameter of type.

Click the Formulas icon. From the parameter list, select
the line you have created (Geometrical Set.1\Line.1).

Click Add Formula and add the formula below in the
editor:
Geometrical Set.1\Line.1
= inertiaAxis(3,PartBody)
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). Click OK in the Formulas dialog box. The
inertia axis is displayed in the geometry area.

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

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.1\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.

Check the value displayed in the specification tree as
well as in the Formulas dialog box.
The KwoGettingStarted.CATPart document used as a sample for
the Product Engineering Optimizer User's Guide illustrates this
scenario. 