 |
distance(Body1, Body2) : Length
Returns the distance between two bodies of a part.
Example:
Length.1 =
distance(Body.3 , Body.1)
|
length(GSMCurve) :Length
Returns the total length of a curve.
|
length(GSMCurve, Point1, Point2) : Length
Returns the length of a curve segment delimited by Point1 and Point2.
|
length(GSMCurve,Point1,Boolean): Length
Returns the length of a curve segment located between Point1 and one of the curve
ends.
Modifying the boolean value allows you to retrieve the length from the specified point to the
other end.
|
area(Surface): Area
Returns the area of a surface generated by the Generative Shape Design product (an extruded
surface for example).
|
area(Curve) : Area
Returns the area delimited by a curve.
|
point.coord(Integer): Length
Returns the coordinate of a point. Returns X if 1 is specified, Y if 2 is specified, Z if
3 is specified.
|
point.coord(oX: Length, oY: Length, oZ: length):
Void
Assigns the point coordinates to the length parameters specified in the arguments. This method
can only be used in Knowledge Advisor rules.
Example:
if Open_body.1\Point.2.coord(1) > 0mm
Message("Point.2 abscissa is positive")
else
{
Open_body.1\Point.1.coord(Xout, Yout, Zout)
Message("Point.1 abscissa is: # ", Xout)
}
|
volume(closedSurface) : Volume
Returns the volume of a closed surface.
|
angle(C, Point1, Point2) : Angle
Returns the angle between the lines "C-Point1" and "C-Point2".
|
angle(Line1, Line2) : Angle
Returns the angle between the Line1 and Line2 lines.
|
angle(direction1,direction2) : Angle
Returns the angle between two directions.
|
body.centerofgravity(oX: Length, oY: Length, oZ:
length): Void
Assigns the values of the solid center of gravity coordinates to the parameters specified in
the arguments. Cannot be used in a formula.
Example:
if Xout==2mm
Body.3.centerofgravity(Xcog,Ycog,Zcog)
|
|
curvature(crv: Curve, pt: Point): Real
Returns the curvature of a curve in a given point.
Example:
Real.1
curvature(Open_body.1\Spline.1 ,Open_body.1\Point.2 )
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