mec_mod_interfaces¶

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o Property AxisRotationAngle() As Angle (Read Only)

Returns the rotation angle of an axis system. Succeeds only if the axis

system is defined by a rotation around an axis, wich means that its type is

catAxisSystemAxisRotation.

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o Property AxisRotationReference() As Reference

Returns the reference for the axis rotation. Succeeds only if the axis

system is defined by a rotation around an axis, wich means that its type is

catAxisSystemAxisRotation.

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o Sub GetEulerAngles(Angle oFirstAngle,

Angle oSecondAngle,

Angle ThirdAngle)

Returns the Euler Angles of an axis system. Succeeds only if the axis

system is defined by Euler angles, wich means its type is

catAxisSystemEulerAngles.

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o Sub GetOrigin(CATSafeArrayVariant oOrigin)

Returns the coordinates X,Y,Z of the origin point of the axis

system.

Parameters:

oOrigin

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the origin point of the axis system.

Example:

The following example retrieves in originCoord the coordinates of the

origin point of the axisSystem axis system:

Dim originCoord(2)

axisSystem.GetOrigin originCoord

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o Sub GetVectors(CATSafeArrayVariant oVectorX,

CATSafeArrayVariant oVectorY)

Returns the coordinates X,Y,Z of the axes X and Y of the axis

system.

Parameters:

oVectorX

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the X axis vector of the axis system.

oVectorY

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Y axis vector of the axis system.

Example:

The following example retrieves in vectorXCoord and vectorYCoord the

coordinates of the vectors of the axisSystem axis

system:

Dim vectorXCoord(2)

Dim vectorYCoord(2)

axisSystem.GetVectors vectorXCoord, vectorYCoord

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o Sub GetXAxis(CATSafeArrayVariant oXAxis)

Returns the coordinates X,Y,Z of the X axis of the axis

system.

Parameters:

oXAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the X axis of the axis system.

Example:

The following example retrieves in XAxisCoord the coordinates of the X

axis of the axisSystem axis system:

Dim XAxisCoord(2)

axisSystem.GetXAxis XAxisCoord

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o Sub GetYAxis(CATSafeArrayVariant oYAxis)

Returns the coordinates X,Y,Z of the Y axis of the axis

system.

Parameters:

oYAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Y axis of the axis system.

Example:

The following example retrieves in YAxisCoord the coordinates of the Y

axis of the axisSystem axis system:

Dim YAxisCoord(2)

axisSystem.GetYAxis XAxisCoord

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o Sub GetZAxis(CATSafeArrayVariant oZAxis)

Returns the coordinates X,Y,Z of the Z axis of the axis

system.

Parameters:

oZAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Z axis of the axis system.

Example:

The following example retrieves in ZAxisCoord the coordinates of the Z

axis of the axisSystem axis system:

Dim ZAxisCoord(2)

axisSystem.GetZAxis ZAxisCoord

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o Property IsCurrent() As boolean

Returns True if the axis system is the current one, else returns False.

Sets the axis system as the current one or not.

Example:

The following example returns in isCurrent True if the axis system

axisSystem is the current one :

isCurrent = axisSystem.IsCurrent

The following example sets the axis system axisSystem as the current

one :

axisSystem.IsCurrent = 1

The following example sets the axis system axisSystem as not the

current one :

axisSystem.IsCurrent = 0

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o Property OriginPoint() As Reference

Returns or sets the geometric point which defines the origin of the axis

system.

OriginPoint is and must be a reference on a geometric 3D

point.

Example:

The following example sets the point Point.1 of the Geometrical Set

Geometrical Set.1 as the origin point of the axis system

AxisSystem0:

Dim HybridBody4 As AnyObject

Set HybridBody4 = Body1.HybridBodies.Item ( “Geometrical Set.1” )

Dim HybridShapePointCoord5 As AnyObject

Set HybridShapePointCoord5 = HybridBody4.HybridShapes.Item ( “Point.1” )

Dim Reference6 As Reference

Set Reference6 = CATIA.ActiveDocument.Part.CreateReferenceFromGeometry ( HybridShapePointCoord5 )

AxisSystem0.OriginPoint = Reference6

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o Property OriginType() As CATAxisSystemOriginType

Returns or sets the way the origin point is defined.

The origin point can be not specified, or be defined by coordinates or by a

geometric point.

CATAxisSystemOriginType is the enumeration which describes how the origin

point is defined :

If OriginType=0, the origin point is defined by a geometric point. If no

point si selected, the origin will be automatically put at the intersection of

the lines or planes defining the axes.

If OriginType=1, the origin is defined by three coordinates x,y,z. Then,

the origin will allways stays at the position defined by the

coordinates.

Example:

The following example prints the origin type :

Catia.SystemService.Print ” OriginType = ” & axisSystem.OriginType

The following example sets the origin type to 1 :

axisSystem.OriginType = 1

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o Sub PutOrigin(CATSafeArrayVariant iOrigin)

Defines the coordinates X,Y,Z of the origin point of the axis

system.

Parameters:

iOrigin

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the origin point of the axis system.

Example:

The following example puts in originCoord the new coordinates of the

origin point of the axisSystem axis system:

Dim originCoord(2)

originCoord ( 0 ) = 100.000000

originCoord ( 1 ) = 200.000000

originCoord ( 2 ) = 10.000000

axisSystem.PutOrigin originCoord

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o Sub PutVectors(CATSafeArrayVariant iVectorX,

CATSafeArrayVariant iVectorY)

Defines the coordinates X,Y,Z of the axes X and Y of the axis

system.

Parameters:

iVectorX

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the X axis vector of the axis system.

iVectorY

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Y axis vector of the axis system.

Example:

The following example modifies in vectorXCoord and vectorYCoord the

coordinates of the vectors of the axisSystem axis

system:

Dim vectorXCoord(2)

vectorYCoord ( 0 ) = 1.000000

vectorYCoord ( 1 ) = -1.000000

vectorYCoord ( 2 ) = 0.000000

Dim vectorYCoord(2)

vectorYCoord ( 0 ) = 0.000000

vectorYCoord ( 1 ) = 0.000000

vectorYCoord ( 2 ) = 1.000000

axisSystem.PutVectors vectorXCoord, vectorYCoord

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o Sub PutXAxis(CATSafeArrayVariant iXAxis)

Defines the coordinates X,Y,Z of the X axis of the axis

system.

Parameters:

iXAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the X axis of the axis system.

Example:

The following example puts in XAxisCoord the new coordinates of the X

axis of the axisSystem axis system:

Dim XAxis(2)

XAxis ( 0 ) = 100.000000

XAxis ( 1 ) = 200.000000

XAxis ( 2 ) = 10.000000

axisSystem.PutXAxis XAxis

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o Sub PutYAxis(CATSafeArrayVariant iYAxis)

Defines the coordinates X,Y,Z of the Y axis of the axis

system.

Parameters:

iYAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Y axis of the axis system.

Example:

The following example puts in XAxisCoord the new coordinates of the Y

axis of the axisSystem axis system:

Dim YAxis(2)

YAxis ( 0 ) = 100.000000

YAxis ( 1 ) = 200.000000

YAxis ( 2 ) = 10.000000

axisSystem.PutYAxis YAxis

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o Sub PutZAxis(CATSafeArrayVariant iZAxis)

Defines the coordinates X,Y,Z of the Z axis of the axis

system.

Parameters:

iZAxis

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the Z axis of the axis system.

Example:

The following example puts in ZAxisCoord the new coordinates of the Z

axis of the axisSystem axis system:

Dim ZAxis(2)

ZAxis ( 0 ) = 100.000000

ZAxis ( 1 ) = 200.000000

ZAxis ( 2 ) = 10.000000

axisSystem.PutZAxis ZAxis

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o Property Type() As CATAxisSystemMainType

Returns or sets the type of the axis system. Sets the axis system

type.

Example:

The following example returns in type1 the type of the axis system

axisSystem1:

type1 = axisSystem1.Type

The following example sets the type of the axis system axisSystem1 as

standard:

axisSystem1.Type = 0

The following example sets the type of the axis system axisSystem1 as

axis rotation:

axisSystem1.Type = 1

The following example sets the type of the axis system axisSystem1 as datum

(explicit):

axisSystem1.Type = 3

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o Property XAxisDirection() As Reference

Reads or sets the geometric point, line or plane which defines the

direction of the X axis.

AxisDirection is and must be a reference on a 3D point or 3D line or

plane.

Example:

The following example sets the point Point.1 of the Geometrical Set

Geometrical Set.1 as the direction of the X axis of the axis system

AxisSystem0:

Dim HybridBody4 As AnyObject

Set HybridBody4 = Body1.HybridBodies.Item ( “Geometrical Set.1” )

Dim HybridShapePointCoord5 As AnyObject

Set HybridShapePointCoord5 = HybridBody4.HybridShapes.Item ( “Point.1” )

Dim Reference6 As Reference

Set Reference6 = CATIA.ActiveDocument.Part.CreateReferenceFromGeometry ( HybridShapePointCoord5 )

AxisSystem0.XAxisDirection = Reference6

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o Property XAxisType() As CATAxisSystemAxisType

Reads or sets the way the X axis is specified.

An axis X,Y, or Z of the axis system can be defined by a geometric point,

line or plane, or by coordinates.

AxisType = 0 : The axis is defined by a geometric point, line or plane and with the same direction.

AxisType = 1 : The axis direction is defined by the three coordinates x,y,z, of a vector, to which the axis will allways stay parallel.

AxisType = 2 : the axis is defined by a geometric point, line or plane and with the opposite direction. Notice : If the X axis is neither defined by coordinates nor by a point,line or plane, the axis will be automatically computed in order to build an orthogonal axis sytem with the other specified axes.

Example:

The following example prints the X axis type :

Catia.SystemService.Print ” XAxisType = ” & axisSystem.XAxisType

The following example sets the X axis type to 1 :

axisSystem.XAxisType = 1

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o Property YAxisDirection() As Reference

Reads or sets the geometric point, line or plane which defines the

direction of the Y axis.

AxisDirection is and must be a reference on a 3D point or 3D line or

plane.

Example:

The following example sets the point Point.1 of the Geometrical Set

Geometrical Set.1 as the direction of the Y axis of the axis system

AxisSystem0:

Dim HybridBody4 As AnyObject

Set HybridBody4 = Body1.HybridBodies.Item ( “Geometrical Set.1” )

Dim HybridShapePointCoord5 As AnyObject

Set HybridShapePointCoord5 = HybridBody4.HybridShapes.Item ( “Point.1” )

Dim Reference6 As Reference

Set Reference6 = CATIA.ActiveDocument.Part.CreateReferenceFromGeometry ( HybridShapePointCoord5 )

AxisSystem0.YAxisDirection = Reference6

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o Property YAxisType() As CATAxisSystemAxisType

Reads or sets the way the Y axis is specified.

An axis X,Y, or Z of the axis system can be defined by a geometric point,

line or plane, or by coordinates.

AxisType = 0 : The axis is defined by a geometric point, line or plane and with the same direction.

AxisType = 1 : The axis direction is defined by the three coordinates x,y,z, of a vector, to which the axis will allways stay parallel.

AxisType = 2 : the axis is defined by a geometric point, line or plane and with the opposite direction. Notice : If the Y axis is neither defined by coordinates nor by a point,line or plane, the axis will be automatically computed in order to build an orthogonal axis sytem with the other specified axes.

Example:

The following example prints the Y axis type :

Catia.SystemService.Print ” YAxisType = ” & axisSystem.YAxisType

The following example sets the Y axis type to 1 :

axisSystem.YAxisType = 1

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o Property ZAxisDirection() As Reference

Reads or sets the geometric point, line or plane which defines the

direction of the Z axis.

AxisDirection is and must be a reference on a 3D point or 3D line or

plane.

Example:

The following example sets the point Point.1 of the Geometrical Set

Geometrical Set.1 as the direction of the Z axis of the axis system

AxisSystem0:

Dim HybridBody4 As AnyObject

Set HybridBody4 = Body1.HybridBodies.Item ( “Geometrical Set.1” )

Dim HybridShapePointCoord5 As AnyObject

Set HybridShapePointCoord5 = HybridBody4.HybridShapes.Item ( “Point.1” )

Dim Reference6 As Reference

Set Reference6 = CATIA.ActiveDocument.Part.CreateReferenceFromGeometry ( HybridShapePointCoord5 )

AxisSystem0.ZAxisDirection = Reference6

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o Property ZAxisType() As CATAxisSystemAxisType

Reads or sets the way the Z axis is specified.

An axis X,Y, or Z of the axis system can be defined by a geometric point,

line or plane, or by coordinates.

AxisType = 0 : The axis is defined by a geometric point, line or plane and with the same direction.

AxisType = 1 : The axis direction is defined by the three coordinates x,y,z, of a vector, to which the axis will allways stay parallel.

AxisType = 2 : the axis is defined by a geometric point, line or plane and with the opposite direction. Notice : If the Z axis is neither defined by coordinates nor by a point,line or plane, the axis will be automatically computed in order to build an orthogonal axis sytem with the other specified axes.

Example:

The following example prints the Z axis type :

Catia.SystemService.Print ” ZAxisType = ” & axisSystem.ZAxisType

The following example sets the Z axis type to 1 :

axisSystem.ZAxisType = 1

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o Func Add() As AxisSystem

Creates a new AxisSystem and adds it to the AxisSystems

collection.

Returns:

The created AxisSystem

Example:

The following example creates a AxisSystem names NewAxisSystem in the

AxisSystem collection of the rootPart part in the partDoc part

document.

Set rootPart = partDoc.Part

Set NewAxisSystem = rootPart.AxisSystems.Add()

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o Func Item(CATVariant iIndex) As AxisSystem

Returns an Axis System using its index or its name from the AxisSystems

collection.

Parameters:

iIndex

The index or the name of the AxisSystem to retrieve from the

collection of AxisSystems. As a numerics, this index is the rank of the

AxisSystem in the collection. The index of the first AxisSystem in the

collection is 1, and the index of the last AxisSystem is Count. As a string, it

is the name you assigned to the AxisSystem using the

AnyObject.Name property.

Returns:

The retrieved AxisSystem

Example:

This example retrieves in ThisAxisSystem the fifth AxisSystem in the

collection and in ThatAxisSystem the AxisSystem named MyAxisSystem in the

AxisSystem collection of the partDoc part document.

Set AxisSystemColl = partDoc.Part.AxisSystems

Set ThisAxisSystem = AxisSystemColl.Item(5)

Set ThatAxisSystem = AxisSystemColl.Item(“MyAxisSystem”)

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o Func Add() As Body

Creates a new body and adds it to the Bodies collection. This body becomes

the current one

Returns:

The created body

Example:

The following example creates a body names NewBody in the body

collection of the rootPart part in the partDoc part document. NewBody becomes

the current body in partDoc.

Set rootPart = partDoc.Part

Set NewBody = rootPart.Bodies.Add()

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o Func Item(CATVariant iIndex) As Body

Returns a body using its index or its name from the Bodies

collection.

Parameters:

iIndex

The index or the name of the body to retrieve from the collection

of bodies. As a numerics, this index is the rank of the body in the collection.

The index of the first body in the collection is 1, and the index of the last

body is Count. As a string, it is the name you assigned to the body using the

AnyObject.Name property.

Returns:

The retrieved body

Example:

This example retrieves in ThisBody the fifth body in the collection and

in ThatBody the body named MyBody in the body collection of the partDoc part

document.

Set BodyColl = partDoc.Part.Bodies

Set ThisBody = BodyColl.Item(5)

Set ThatBody = BodyColl.Item(“MyBody”)

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o Property HybridBodies() As HybridBodies (Read Only)

Returns the body’s HybridBodies collection.

Example:

The following example returns in hybridBodyColl the collection of

hybrid bodies of the main body of partDoc part

document:

Dim body As Body

Set body = partDoc.Part.Bodies.MainBody

Set hybridBodyColl = body.HybridBodies

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o Property HybridShapes() As HybridShapes (Read Only)

Returns the list of hybrid shapes included in the body.

Returns:

oHybridShapes The list of hybrid shapes in the body (@see

CATIAHybridShapes

for more information).

Example:

The following example returns in HybridShapes1 the list

of

hybrid shapes in the body Body1:

Dim HybridShapes1 As HybridShapes

Set HybridShapes1 = Body1.HybridShapes

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o Property InBooleanOperation() As boolean (Read Only)

Returns True if the body is involved in a boolean operation, else returns

False.

Example:

The following example returns in operated True if the body body1belongs

to a boolean operation.

operated = body1.InBooleanOperation

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o Sub InsertHybridShape(HybridShape iHybridShape)

Insert a hybrid shape to the body.

Parameters:

iHybriShape

The hybrid shape to insert.

Example:

This example inserts the hybrid shape HybridShape1 to the body

Body1:

Body1.InsertHybridShape (HybridShape1)

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o Property OrderedGeometricalSets() As OrderedGeometricalSets (Read

Only)

Returns the body’s OrderedGeometricalSets collection.

ometricalSetColl = Body1.OrderedGeometricalSets Example:

The following example returns in OrderedGeometricalSetColl the

collection of ordered geometrical set of the body Body1

:

Set OrderedGe

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o Property Shapes() As Shapes (Read Only)

Returns the body’s Shapes collection. These shapes make up the sequence of

shapes that will produce an intermediate result for the part, or the final

result in the case of the main body.

Example:

The following example returns in shapColl the collection of shapes

managed by the main body of the partDoc part document:

Dim body As Body

Set body = partDoc.Part.Bodies.MainBody

Set shapColl = body.Shapes

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o Property Sketches() As Sketches (Read Only)

Returns the body’s Sketches collection. These sketches are those inside the

body at all levels.

Example:

The following example returns in skColl the collection of sketches of

the main body of partDoc part document:

Dim body As Body

Set body = partDoc.Part.Bodies.MainBody

Set skColl = body.Sketches

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o Sub Activate()

Unsuppresses a constraint for the update process. An activated constraint

is again taken into account for the calculation of the part or product.

Example:

The following example es the pad1 pad:

Example:

The following example activates the tangencyCst constraint

:

tangencyCst.Activate

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o Property AngleSector() As CatConstraintAngleSector

Returns or sets the constraint angle (or angular) sector. The geometric elements of an angle

constraint (e.g. : 2 lines or 2 planes) divide the sketch or the space in 4 regions which are

called angle or angular sectors, numbered from 0 to 3. 1 / 0 —/— 2/ 3 By default, the

constraint is created in the sector number 0. One angle sector corresponds exactly to particular

values of the Dimension.Value, the Side and the Orientation. When changing the angle sector, the

Dimension.Value, Side and Orientation are also modified.

Parameters:

AngleSector=0

The default sector of a constraint.

Dimension.Value

= angle Orientation

= catCstOrientSame Side

= catCstSidePositive

AngleSector=1

Dimension.Value

= angle-180 if angle>180 abs(angle)+180 otherwise Orientation

= catCstOrientOpposite Side

= catCstSidePositive

AngleSector=2

Dimension.Value

= abs(540-angle) if angle>180 180-fabs(angle) otherwise Orientation

= catCstOrientOpposite Side

= catCstSideNegative

AngleSector=3

Dimension.Value

= 360-abs(angle) Orientation

= catCstOrientSame Side

= catCstSideNegative

Example:

The following example retrieves in angleSector the angle sector

of the angleCst angle constraint and then changes the angle

sector

angleSector = angleCst.AngleSector

angleCst.AngleSector = 2

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o Sub Deactivate()

Suppresses the constraint from being updated. A deactivated constraint is

not taken into account for the calculation of the part or of the product.

Example:

The following example deactivates the tangencyCst constraint from being

updated:

tangencyCst.Deactivate

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o Property Dimension() As Dimension (Read Only)

Returns the constraint dimension. The dimension may be meaningless for some

types of constraints such as tangency constraints, or if the constraint is not

currently satisfied. Use the Status property to check whether the constraint is

satisfied.

Example:

The following example returns in cstDimension the dimension of the

firstCst constraint:

Set cstDimension = firstCst.Dimension

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o Property DistanceConfig() As CatConstraintDistConfig

Returns or sets the distance constraint configuration. Distance constraints

between lines and cylinders offer often more degrees of freedom to geometry

than acually desired. This property allows to limit these degrees of freedom

without having to redefine additional constraints. This property is useless for

constraints whose type is not distance.

Example:

The following example retrieves in distCstConfig the configuration of

the distCst distance constraint:

distCstConfig = distCst.DistanceConfig

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o Property DistanceDirection() As CatConstraintDistDirection

Returns or sets the distance constraint direction. This property is useless for constraints whose

type is not Distance (1). Distance constraints may be measured along a particular direction.

This property will be used if the direction is a reference axis : In 2D, 1 means the horizontal

axis, 2 the vertical axis. In 3D, 1 stands for the X axis, 2 for the Y axis, 3 for the Z axis.

0 means that no direction is specified and the distance is measured as usual.

Example:

The following example retrieves in distCstDirection the configuration

of the distCst distance constraint:

distCstConfig = distCst.DistanceDirection

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o Func GetConstraintElement(long iElementNumber) As

Reference

Reads an element of a constraint.

Parameters:

iElementNumber

The number of the element of the constraint to be read. (1 for the first element,2 for

the second, 3 for the third). Notice it must not exceed the total number of elements of

the constraint. (eg : not allowed to read the third element of a tangency).

oCurrentElement

An element of the constraint.

Example:

The following example reads the first element of a

constraint

Dim reference1 As Reference

reference1=tangencyCst.GetConstraintElement( 1 )

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o Sub GetConstraintVisuLocation(CATSafeArrayVariant

oAnchorPoint,

CATSafeArrayVariant oAnchorVector)

Returns the constraint visualisation location. When displayed on screen,

the constraint is visualized as a dimension positioned close to the constrained

geometric element(s). This method retrieves the data used to position this

representation within the 3D space.

Parameters:

oAnchorPoint

A Safe Array made up of 3 doubles: X, Y, Z, representing the

coordinates in model space of the point where the constraint value is

displayed.

oAnchorVector

A Safe Array made up of 3 doubles : X, Y, Z, representing the vector normal to the plane

onto which the constraint value is displayed.

Example:

The following example retrieves in anchorPt the anchor point of the

tangencyCst tangency constraint:

Dim anchorPoint(2)

Dim anchorVector(2)

tangencyCst.ConstraintVisuLocation

anchorPoint,vectorPoint

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o Func IsInactive() As boolean

Indicates whether a constraint is suppressed from the update process. A

suppressed constraint is not taken into account for the calculation of part or

the product. The method returns True if the constraint is not active, False if

the constraint is active.

Example:

The following example returns in isInactive whether the tangencyCst

constraint is suppressed from the update process:

Set isInactive = tangencyCst.IsInactive

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o Property Mode() As CatConstraintMode

Returns or sets the constraint driving mode. For constraint types

supporting the concept of value, such as distance constraints, the driving mode

tells whether the constraint value actually drives the geometry position, or,

conversely, is driven by it.

Example:

The following example retrieves in currentMode the driving mode for the

distCst distance constraint:

currentMode = distCst.Mode

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o Property Orientation() As CatConstraintOrientation

Returns or sets the constraint orientation. This is used for constraints

that involve two geometric elements and specifies the orientation for the

second geometric element with regard to the first one, when several possible

orientations are all satisfying the constraint.

Example:

The following example retrieves the in distCstOrient the orientation of

the distCst distance constraint:

distCstOrient = distCst.Orientation

Note

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o Property ReferenceAxis() As CatConstraintRefAxis

Returns or sets the constraint reference axis. AxisParallel or

AxisPerpendicular constraint types define which axis they relate to through

this property, which makes no sense for constraints of another

type.

Example:

The following example retrieves in refAxis the reference axis for the

axisPerpCst AxisPerpendicular constraint:

refAxis = axisPerpCst.ReferenceAxis

Note

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o Property ReferenceType() As CatConstraintRefType

Returns or sets the constraint reference type. This property is used only

for Reference constraints in the Assembly context.

Example:

The following example applies to the reference constraint refCst2 the

reference type of the constraint refCst1.

refCst2.ReferenceType = refCst1.ReferenceType

Note

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o Sub SetConstraintElement(long iElementNumber,

Reference iNewElement)

Replaces an element of a constraint.

Parameters:

iElementNumber

The number of the element of the constraint to replace. (1 for the

first element,2 for the second, 3 for the third).

iNewElement

A new element of the constraint.

Example:

The following example changes the second element of a

constraint

Dim reference1 As Reference

tangencyCst.SetConstraintElement ( 2, reference1)

Note

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o Sub SetConstraintVisuLocation(double iNewX,

double iNewY,

double iNewZ)

Sets a new location for the constraint visualization.

Parameters:

iNewX

The new value for the constraint anchor point X coordinate

iNewY

The new value for the constraint anchor point Y coordinate

iNewZ

The new value for the constraint anchor point Z coordinate

Example:

The following example changes the anchor point coordinates to

10,0,0

tangencyCst.SetConstraintVisuLocation 10,0,0

Note

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o Property Side() As CatConstraintSide

Returns or sets the constraint side. Some constraint types need to

relatively position the constrained geometries, when several possible

configurations are all satisfying the constraint.

Example:

The following example retrieves in distCstSide the side of the distCst

distance constraint:

distCstSide = distCst.Side

Note

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o Property Status() As CatConstraintStatus (Read Only)

Returns the constraint status. The constraint status is a diagnosis on

whether the constraint is satisfied.

Example:

The following example retrieves the status of the distCst distance

constraint.

distCstSts = distCst.Status

Note

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o Property Type() As CatConstraintType (Read Only)

Returns the constraint type.

Example:

The following example returns in cstType the type of the firstCst

constraint:

cstType = firstCst.Type

Note

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o Func AddBiEltCst(CatConstraintType iCstType,

Reference iFirstElem,

Reference iSecondElem) As Constraint

Creates a new constraint applying to two geometric elements and adds it to

the Constraints collection.

Parameters:

iCstType

The constraint type

iFirstElem

The first constrained geometric element

The following

Boundary object is supported: Boundary.

iSecondElem

The second constrained geometric element

The following Boundary object is supported: Boundary.

Example:

This example adds the NewCst tangency constraint in a sketch, between the

two circles c1 and c2 using the value 4 for

catCstTypeTangency.

Set newCst = skCstList.AddBiEltCst(4, c1, c2)

Note

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o Func AddMonoEltCst(CatConstraintType iCstType,

Reference iElem) As Constraint

Creates a new constraint applying to a single geometric element and adds it

to the Constraints collection.

Parameters:

iCstType

The constraint type

iElem

The constrained geometric element

The following

Boundary object is supported: Boundary.

Example:

This example creates the reference constraint NewCst to a part, stating

that the P1 point should remain fixed with respect to the part’s origin

elements using the value 0 for catCstTypeReference, and adds it to the cstList

collection.

Set NewCst = cstList.AddMonoEltCst(0, P1)

Note

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o Func AddTriEltCst(CatConstraintType iCstType,

Reference iFirstElem,

Reference iSecondElem,

Reference iThirdElem) As Constraint

Creates a new constraint applying to three geometric elements and adds it

to the Constraints collection.

Parameters:

iCstType

The constraint type

iFirstElem

The first constrained geometric element

The following

Boundary object is supported: Boundary.

iSecondElem

The second constrained geometric element

The following Boundary object is supported: Boundary.

iThirdElem

The third constrained geometric element

The following Boundary object is supported: Boundary.

Example:

This example adds symCst symmetry constraint in a part, stating that the

cylinders cyl1 and cyl2 are symmetric with respect to the plane symPlane using

the value 15 for catCstTypeSymmetry.

Set symCst = prtCstList.AddTriEltCst(15, cyl1, cyl2, symPlane)

Note

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o Property BrokenConstraintsCount() As long (Read Only)

Returns the number of broken constraints from the Constraints

collection.

Example:

The following example retrieves in BknCstNum the number of broken

constraints from the myListofConstraints collection of

constraints:

BknCstNum = myListofConstraints.BrokenConstraintsCount

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o Func Item(CATVariant iIndex) As Constraint

Returns a constraint using its index or its name from the Constraints

collection.

Parameters:

iIndex

The index or the name of the constraint to retrieve frm the

collection of constraints. As a numerics, this index is the rank of the

constraint in the collection. The index of the first constraint in the

collection is 1, and the index of the last constraint is Count. As a string, it

is the name you assigned to the constraint using the

AnyObject.Name property.

Returns:

The retrieved constraint

Example:

This example retrieves in cst1 the first constraint in the collection

and in cst2 the constraint Constraint.2.

Set cst1 = cstList.Item(1)

Set cst2 = cstList.Item(“Constraint.2”)

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o Sub Remove(CATVariant iIndex)

Removes a constraint from the Constraints collection.

Parameters:

iIndex

The index or the name of the constraint to remove from the

Constraints collection. As a numerics, this index is the rank of the constraint

in the collection. The index of the first constraint in the collection is 1,

and the index of the last constraint is Count. As a string, it is the name you

assigned to the constraint using the

AnyObject.Name property.

Example:

This example removes the last constraint in the

collection.

cstList.Remove(cstList.Count)

Note

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o Property UnUpdatedConstraintsCount() As long (Read Only)

Returns the number of unupdated constraints from the Constraints

collection.

Example:

The following example retrieves in UnUpdCstNum the number of unupdated

constraints from the myListofConstraints collection of

constraints:

UnUpdCstNum = myListofConstraints.UnUpdatedConstraintsCount

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o Sub GetDirection(CATSafeArrayVariant oDirection)

Returns the direction of the cylindrical face axis

Parameters:

oDirection[0]

The X Coordinate of the axis direction

oDirection[1]

The Y Coordinate of the axis direction

oDirection[2]

The Z Coordinate of the axis direction

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o Sub GetOrigin(CATSafeArrayVariant oOrigin)

Returns the origin of the cylindrical face axis.

Parameters:

oOrigin[0]

The X Coordinate of the axis origin

oOrigin[1]

The Y Coordinate of the axis origin

oOrigin[2]

The Z Coordinate of the axis origin

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o Sub AddFixTogether(FixTogether iFixTogether)

Add a fixTogether to a FixTogether. The fixTogether is fixed together with

the products or fixTogethers already contained in the FixTogether.

Example:

The following example adds a FixTogether fixTogether in a FixTogether

myFixTogether.

myFixTogether.AddFixTogether(fixTogether)

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o Sub AddProduct(Product iProduct)

Add a product to a FixTogether. The product is fixed together with the

products and fixTogethers already contained in the FixTogether.

Example:

The following example adds a Product myProduct in a

FixTogether.

myFixTogether.AddProduct(myProduct)

Note

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o Property FixTogethersCount() As long (Read Only)

Returns the number of FixTogether entities in the

FixTogether.

Example:

The following example retrieves in fixTogethersCount the number of

FixTogethers of the myFixTogether FixTogether :

fixTogethersCount = myFixTogether.FixTogethersCount

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o Func GetFixTogether(CATVariant iIndex) As FixTogether

Returns a FixTogether using its index or its name in the

FixTogether.

Parameters:

iIndex

The index or the name of the FixTogether to retrieve. As a

numerics, this index is the rank of the FixTogether in the FixTogethers of the

FixTogether. The index of the first FixTogether is 1, and the index of the last

FixTogether is FixTogethersCount. As a string, it is the name you assigned to

the FixTogether using the

AnyObject.Name property.

Returns:

The retrieved FixTogether

Example:

This example retrieves in thisFixTogether the fifth FixTogether and in

thatFixTogether the FixTogether named myFixTogether in the FixTogethers of the

FixTogether.

Dim thisFixTogether As FixTogether

Set thisFixTogether = myFixTogether.GetFixTogether(5)

Dim thatFixTogether As FixTogether

Set thatFixTogether = myFixTogether.GetFixTogether(“myFixTogether”)

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o Func GetProduct(CATVariant iIndex) As Product

Returns a Product using its index or its name in the

FixTogether.

Parameters:

iIndex

The index or the name of the Product to retrieve. As a numerics,

this index is the rank of the Product in the products of the FixTogether. The

index of the first Product is 1, and the index of the last Product is

ProductsCount. As a string, it is the name you assigned to the Product using

the

AnyObject.Name property.

Returns:

The retrieved Product

Example:

This example retrieves in thisProduct the fifth Product and in

thatProduct the Product named myProduct in the products of the

FixTogether.

Dim thisProduct As Product

Set thisProduct = myFixTogether.GetProduct(5)

Dim thatProduct As Product

Set thatProduct = myFixTogether.GetProduct(“myProduct”)

Note

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o Property ProductsCount() As long (Read Only)

Returns the number of products fixed together in the

FixTogether.

Example:

The following example retrieves in productsCount the number of products

of the myFixTogether FixTogether :

productsCount = myFixTogether.ProductsCount

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o Sub RemoveFixTogether(CATVariant iIndex)

Removes a FixTogether from the FixTogether.

Parameters:

iIndex

The index or the name of the FixTogether to remove from the

FixTogether. As a numerics, this index is the rank of the FixTogether in the

FixTogethers of the FixTogether. The index of the first FixTogether is 1, and

the index of the last FixTogether is FixTogethersCount. As a string, it is the

name you assigned to the FixTogether using the

AnyObject.Name property.

Example:

This example removes the last FixTogether of the

FixTogether.

fixTogether.RemoveFixTogether(fixTogether.FixTogethersCount)

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o Sub RemoveProduct(CATVariant iIndex)

Removes a Product from the FixTogether.

Parameters:

iIndex

The index or the name of the Product to remove from the

FixTogether. As a numerics, this index is the rank of the Product in the

products of the FixTogether. The index of the first Product is 1, and the index

of the last Product is ProductsCount. As a string, it is the name you assigned

to the FixTogether using the

AnyObject.Name property.

Example:

This example removes the last Product of the FixTogether.

fixTogether.RemoveProduct(fixTogether.ProductsCount)

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o Func Add() As FixTogether

Creates a new FixTogether and adds it to the FixTogethers

collection.

Returns:

The created FixTogether

Example:

The following example creates a FixTogether newFixTogether in the

FixTogether collection.

Set newFixTogether = fixTogethers.Add

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o Func Item(CATVariant iIndex) As FixTogether

Returns a FixTogether using its index or its name from the FixTogethers

collection.

Parameters:

iIndex

The index or the name of the FixTogether to retrieve from the

collection of FixTogether. As a numerics, this index is the rank of the

FixTogether in the collection. The index of the first FixTogether in the

collection is 1, and the index of the last FixTogether is Count. As a string,

it is the name you assigned to the FixTogether using the

AnyObject.Name property.

Returns:

The retrieved FixTogether

Example:

This example retrieves in thisFixTogether the fifth FixTogether in the

collection and in thatFixTogether the FixTogether named MyFixTogether in the

FixTogether collection of the product product.

Set fixTogetherColl = product.FixTogethers

Set thisFixTogether = fixTogetherColl.Item(5)

Set thatFixTogether = fixTogetherColl.Item(“MyFixTogether”)

Note

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o Sub Remove(CATVariant iIndex)

Removes a FixTogether from the FixTogethers collection.

Parameters:

iIndex

The index or the name of the FixTogether to remove from the

FixTogethers collection. As a numerics, this index is the rank of the

FixTogether in the collection. The index of the first FixTogether in the

collection is 1, and the index of the last FixTogether is Count. As a string,

it is the name you assigned to the FixTogether using the

AnyObject.Name property.

Example:

This example removes the last FixTogether in the

collection.

fixTogetherColl.Remove(fixTogetherColl.Count)

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o Func Item(CATVariant iIndex) As GeometricElement

Returns a geometric element using its index or its name from the

GeometricElements collection.

Parameters:

iIndex

The index or the name of the geometric element to retrieve from the

collection of geometric elements. As a numerics, this index is the rank of the

geometric element in the collection. The index of the first geometric element

in the collection is 1, and the index of the last geometric element is Count.

As a string, it is the name you assigned to the geometric element using the

AnyObject.Name property.

Returns:

The retrieved geometric element

Example:

This example retrieves the last item in the geometric element

collection.

Set lastCst = cstList.Item(cstList.Count)

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o Func Add() As HybridBody

Creates a new hybrid body and adds it to the HybridBodies collection. This

body becomes the current one

Returns:

The created body

Example:

The following example creates a body named newHybridBody in the hybrid

body collection of the rootPart part in the partDoc part document. NewPartBody

becomes the current body in partDoc.

Set NewPartBody = rootPart.Bodies.AddPartBody()

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o Func Item(CATVariant iIndex) As HybridBody

Returns a body using its index or its name from the Bodies

collection.

Parameters:

iIndex

The index or the name of the hybrid body to retrieve from the

collection of hybrid bodies. As a numerics, this index is the rank of the

hybrid body in the collection. The index of the first hybrid body in the

collection is 1, and the index of the last hybrid body is Count. As a string,

it is the name you assigned to the hybrid body using the

AnyObject.Name property.

Returns:

The retrieved hybrid body

Example:

This example retrieves in ThisHybridBody the fifth hybrid body in the

collection and in ThatHybridBody the hybrid body named MyHybridBody in the

hybrid body collection of the partDoc part document.

Set hybridBodyColl = partDoc.Part.HybridBodies

Set ThisHybridBody = hybridBodyColl.Item(5)

Set ThatHybridBody = hybridBodyColl.Item(“MyHybridBody”)

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o Sub AppendHybridShape(HybridShape iHybridShape)

Appends a hybrid shape to the hybrid body.

Parameters:

iHybriShape

The hybrid shape to append.

Example:

This example appends the hybrid shape hybridShape to the hybrid body

hybridBody:

hybridBody.AppendHybridShape (hybridShape)

Note

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o Property Bodies() As Bodies (Read Only)

Returns the hybrid body’s Bodies collection.

Example:

The following example returns in bodyColl the collection of bodies of

the hybrid body hybridBody :

Set bodyColl = hybridBody.Bodies

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o Property GeometricElements() As GeometricElements (Read

Only)

Returns the list of geometrical elements included in the hybrid

body.

Returns:

oGeometricElements The list of geometric elements in the hybrid body

(@see CATIAGeometricElements

for more information).

Example:

The following example returns in geometricElements the list

of

geometrical elements in the Hybrid body

hybridBody:

Dim geometricElements As GeometricElements

Set geometricElements = hybridBody.GeometricElements

Note

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o Property HybridBodies() As HybridBodies (Read Only)

Returns the hybrid body’s HybridBodies collection.

Example:

The following example returns in hybridBodyColl the collection of

hybrid bodies of the hybrid body hybridBody :

Set hybridBodyColl = hybridBody.HybridBodies

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o Property HybridShapes() As HybridShapes (Read Only)

Returns the list of hybrid shapes included in the hybrid

body.

Returns:

oHybridShapes The list of hybrid shapes in the hybrid body (@see

CATIAHybridShapes

for more information).

Example:

The following example returns in hybridShapes the list

of

hybrid shapes in the hybrid body hybridBody:

Dim hybridShapes As HybridShapes

Set hybridShapes = hybridBody.HybridShapes

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o Property HybridSketches() As Sketches (Read Only)

Returns the hybrid body’s Sketches collection. These sketches are those

inside the hybrid body at all levels.

Example:

The following example returns in skColl the collection of sketches of a

hybrid body :

Set skColl = hybridBody.HybridSketches

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o Sub AppendHybridShape(HybridShape iHybridShape)

Appends a hybrid shape to another hybrid shape.

Parameters:

iHybridShape

The hybrid shape to append.

Example:

This example appends the hybrid shape newHybridShape to the hybrid

shape oldHybridShape:

oldHybridShape.AppendHybridShape (newHybridShape)

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o Sub Compute()

Computes the result of the hybrid shape.

Note

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o Property Thickness() As HybridShape (Read Only)

Returns the thickness of the hybrid shape.

The thickness is a CATIAHybridShapeThickness.

Example:

The following example returns the thickness ExtrudeThickness of the

extrude Extrude.1 as the origin point of the axis system

AxisSystem0:

Dim Extrude1 As AnyObject

Set Extrude1 = HybridBody1.HybridShapes.Item ( “Extrude.1” )

Dim Thickness1 As HybridShapeThickness

Set Thickness1 = Extrude1.Thickness

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o Func GetInput(CATBSTR iIndex) As AnyObject

Gets an input of a hybrid shape instance by its name.

Parameters:

iName

The name of the input of the hybrid shape instance

Returns:

The input, if found

Example:

The following example tests if the input was found:

Set input = hybridShapeInstance.GetInput(“Input1”)

If TypeName(input)=”Nothing” Then

MsgBox “Input not found”

End If

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o Func GetInputData(CATBSTR iName) As CATBaseDispatch

Gets an input of a shape instance by its name. Use this method if you want

to retrieve a Reference.

Parameters:

iName

The name of the input of the shape instance

Returns:

The input, if found

Example:

The following example tests if the input was found:

Set input = shapeInstance.GetInput(“Input1”)

If TypeName(input)=”Nothing” Then

MsgBox “Input not found”

End If

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o Func GetInputDataFromPosition(long iPosition) As

CATBaseDispatch

Gets an input of a hybrid shape instance from its position. Use this method

if you want to retrieve a Reference.

Parameters:

iPosition

The position

Returns:

The input, if found

Example:

The following example tests if the input was found:

Set input = hybridShapeInstance.GetInputFromPosition(2)

If TypeName(input)=”Nothing” Then

MsgBox “Input not found”

End If

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o Func GetInputFromPosition(long iPosition) As AnyObject

Gets an input of a hybrid shape instance from its

position.

Parameters:

iPosition

The position

Returns:

The input, if found

Example:

The following example tests if the input was found:

Set input = hybridShapeInstance.GetInputFromPosition(2)

If TypeName(input)=”Nothing” Then

MsgBox “Input not found”

End If

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o Func GetOutput(CATBSTR iName) As AnyObject

Gets a Ouput by its name.

Parameters:

iName

The name of the output of the shape instance

Returns:

The output, if found

Example:

The following example tests if the output was found:

Set output = shapeInstance.GetOuput(“Output1”)

If TypeName(output)=”Nothing” Then

MsgBox “Output not found”

End If

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o Func GetOutputFromPosition(long iPosition) As AnyObject

Gets a Ouput from its position.

Parameters:

iPosition

The position

Returns:

The output, if found

Example:

The following example tests if the output was found:

Set output = shapeInstance.GetOuputFromPosition(2)

If TypeName(output)=”Nothing” Then

MsgBox “Output not found”

End If

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o Func GetParameter(CATBSTR iName) As AnyObject

Gets a parameter of a hybrid shape instance by its name.

Parameters:

iName

The name of the parameter of the hybrid shape instance

Returns:

The parameter, if found

Example:

The following example tests if the parameter was

found:

Set parameter = hybridShapeInstance.GetParameter(“Parameter1”)

If TypeName(parameter)=”Nothing” Then

MsgBox “Parameter not found”

End If

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o Func GetParameterFromPosition(long iPosition) As AnyObject

Gets a parameter of a hybrid shape instance from its

position.

Parameters:

iPosition

The position

Returns:

The parameter, if found

Example:

The following example tests if the parameter was

found:

Set parameter = hybridShapeInstance.GetParameterFromPosition(2)

If TypeName(input)=”Nothing” Then

MsgBox “Parameter not found”

End If

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o Property InputsCount() As long (Read Only)

Returns the number of Inputs.

Example:

The following example retrieves in inputsCount the number of Inputs of

hybridShapeInstance:

inputsCount = hybridShapeInstance.InputsCount

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o Property OutputsCount() As long (Read Only)

Returns the number of Outputs.

Example:

The following example retrieves in outputsCount the number of Outputs

of hybridShapeInstance:

outputsCount = hybridShapeInstance.OutputsCount

Note

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o Property ParametersCount() As long (Read Only)

Returns the number of Parameters.

Example:

The following example retrieves in parametersCount the number of

parameters of hybridShapeInstance:

parametersCount = hybridShapeInstance.ParametersCount

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o Sub PutInput(CATBSTR iIndex,

AnyObject iInput)

Defines an input of a hybrid shape instance.

Parameters:

iName

The input name

iInput

The element wich will be input of the hybrid shape

instance

All types of

Boundary object are possibly supported.

Example:

The following example defines the input of a hybrid shape instance The

input will be a point and its name will be Input1.

hybridShapeInstance.PutInput “Input1”,point

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o Sub PutInputData(CATBSTR iName,

CATBaseDispatch iInput)

Defines an input of a shape instance. Use this method if you want to set as

input a Reference.

Parameters:

iName

The input name

iInput

The element wich will be input of the shape

instance

All types of

Boundary object are possibly supported.

Example:

The following example defines the input of a shape instance The input

will be a point and its name will be Input1.

shapeInstance.PutInput “Input1”,point

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o Func GetBoundary(CATBSTR iLabel) As Boundary

Returns a boundary using its label.

Parameters:

iLabel

Identification of the

Boundary object. See Reference.DisplayName.

Returns:

The retrieved boundary

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o Func Item(CATVariant iIndex) As HybridShape

Returns a HybridShape using its index or its name from the HybridShapes

collection.

Parameters:

iIndex

The index or the name of the HybridShape to retrieve from the

collection of HybridShapes. As a numerics, this index is the rank of the

HybridShape in the collection. The index of the first HybridShape in the

collection is 1, and the index of the last HybridShape is

Collection.Count. As a string, it is the name you assigned to the

HybridShape using the AnyObject.Name property.

Returns:

The retrieved HybridShape

Example:

This example retrieves in ThisHybridShape the third HybridShape, and in

ThatHybridShape the HybridShape named MyHybridShape in the HybridShape

collection of the active document, supposed to be a part

document.

Set ThisHybridShape = CATIA.ActiveDocument.HybridShapes.Item(3)

Set ThatHybridShape = CATIA.ActiveDocument.HybridShapes.Item(“MyHybridShape”)

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o Func AddInstance(AnyObject iReference) As AnyObject

Creates a new instance of a shape or hybrid shape.

Parameters:

iReference

The reference shape or hybrid shape.

Example:

This example creates the instance NewInstance in the

part.

Set NewInstance = instanceFactory.AddInstance(reference)

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o Sub BeginInstanceFactory(CATBSTR iNameOfReference,

CATBSTR iNameOfDocument)

Initializes the instantiation process with the document containing the

reference.

Role: Use this method to start instantiating a reference in the current

document.

In that method, the document containing the reference is locked in

session.

It will be unlocked in the last step EndInstanceFactory .

Parameters:

iNameOfReference

The name of the reference to be instantiated.

iDocumentFileName

The name of the file containing the document where to find the

reference to be instantiated.

Example:

The following example initializes the factory with a document and a

reference:

InstanceFactory.BeginInstanceFactory”NameOfReference”,”c:tmpNameOfDocument.CATPart”

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o Sub BeginInstantiate()

Initializes the data of the reference.

Role: This is the first method of the second step of

instantiation.

It is used to initialize all data of the reference in the

factory.

Example:

The following example shows how to initialize the

factory:

InstanceFactory.BeginInstantiate

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o Sub EndInstanceFactory()

Ends the instantiation process.

Role: Use this method to end the instantiation process.

In that method the document containing the reference is unlocked and

released from the session.

Example:

The following example shows how to end the

instantiation:

InstanceFactory.EndInstanceFactory

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o Sub EndInstantiate()

Ends the instantiation of the reference.

Role: This is the fifth and last method of the second step of

instantiation.

It is used to end the instantiation: after this step, all the links to the

reference are broken.

Example:

The following example shows how to end the

instantiation:

InstanceFactory.EndInstantiate

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o Func GetParameter(CATBSTR iName) As AnyObject

Retrieves a parameter of the reference by its name.

Role: This is the third method of the second step of

instantiation.

This step is optional.

It is used to retrieve a parameter of the reference in order to change its

value, using the ValuateFromString method of the Parameter

interface.

It has to be called on each parameter whose value has to be

changed.

Parameters:

iName

The name of the parameter.

Example:

The following example retrieves a parameter on the

reference:

Set parameter = InstanceFactory.GetParameter(“Parameter1”)

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o Func Instantiate() As AnyObject

Instantiates the reference in the current document.

Role: This is the fourth method of the second step of

instantiation.

It is used to duplicate or instantiate the data of the

reference.

In case of Power Copy instantiation, the data are duplicated and there

is no created instance.

In case of User Feature instantiation, the data are instantiated and an

instance is created and returned.

Example:

The following example instantiates the reference:

Set Instance = InstanceFactory.Instantiate

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o Property InstantiationMode(CATBSTR iInstantiationModeBSTR) (Write

Only)

Sets the mode of instantiation to “Inside” or “After”.

Role: This method should be called BEFORE the method BeginInstantiate to

take into account the desired instantiation mode.

It is used to set the destination path of insertion of the template

reference.

Example:

The following example shows how to determine the instantiation mode

(Mode’s value is “Inside” or “After”):

InstanceFactory.InstantationMode = Mode

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o Sub PutInputData(CATBSTR iName,

CATBaseDispatch iInput)

Sets a value to an input of the reference.

Role: This is the second method of the second step of

instantiation.

It is used to set a value to any input of the reference.

It has to be called on each input of the reference.

Parameters:

iName

The name of the input.

iInput

The element to set as the new value of the input.

All types of

Boundary object are possibly supported.

Example:

The following example sets a value to an input of the reference: The input

is a point and its name is Input1.

InstanceFactory.PutInputData “Input1”,point1

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o Property Bodies() As Bodies (Read Only)

Returns the ordered geometrical set’s Bodies collection.

Example:

The following example returns in bodyColl the collection of bodies of

the ordered geometrical set OrderedGeometricalSet1 :

Set bodyColl = OrderedGeometricalSet1.Bodies

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o Property HybridShapes() As HybridShapes (Read Only)

Returns the list of hybrid shapes included in the ordered geometrical

set.

Returns:

oHybridShapes The list of hybrid shapes in the ordered geometrical set

(@see CATIAHybridShapes

for more information).

Example:

The following example returns in HybridShapes1 the list

of

hybrid shapes in the ordered geometrical

setOrderedGeometricalSet1:

Dim HybridShapes1 As HybridShapes

Set HybridShapes1 = OrderedGeometricalSet1.HybridShapes

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o Sub InsertHybridShape(HybridShape iHybridShape)

Inserts a hybrid shape to the ordered geometrical set.

Parameters:

iHybridShape

The hybrid shape to insert.

Example:

This example inserts the hybrid shape HybridShape1 to the ordered

geometrical set OrderedGeometricalSet1:

OrderedGeometricalSet1.InsertHybridShape

(HybridShape1)

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o Property OrderedGeometricalSets() As OrderedGeometricalSets (Read

Only)

Returns the ordered geometrical set’s OrderedGeometricalSets

collection.

Example:

The following example returns in OrderedGeometricalSetColl the

collection of ordered geometrical set of the ordered geometrical set

OrderedGeometricalSet1 :

Set OrderedGeometricalSetColl = OrderedGeometricalSet1.OrderedGeometricalSets

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o Property OrderedSketches() As Sketches (Read Only)

Returns the ordered geometrical set’s Sketches collection. These sketches

are those inside the ordered geometrical set at all

levels.

Example:

The following example returns in sketchesCollection the collection of

sketches of an ordered geometrical set :

Set sketchesCollection = OrderedGeometricalSet1.OrderedSketches

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o Func Add() As OrderedGeometricalSet

Creates a new ordered geometrical set and adds it to the

OrderedGeometricalSets collection. Thisordered geometrical set becomes the

current one

Returns:

The created ordered geometrical set

Example:

The following example creates a ordered geometrical set named

newOrderedGeometricalSet in the ordered geometrical set collection of the

rootPart part in the partDoc part document. NewPartBody becomes the in work

object of partDoc.

Set NewPartBody = rootPart.OrderedGeometricalSets.Add()

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o Func Item(CATVariant iIndex) As OrderedGeometricalSet

Returns a ordered geometrical set using its index or its name from the

ordered geometrical set collection.

Parameters:

iIndex

The index or the name of the ordered geometrical set to retrieve

from the collection of ordered geometrical sets. As a numerics, this index is

the rank of the ordered geometrical set in the collection. The index of the

first ordered geometrical set in the collection is 1, and the index of the last

ordered geometrical set is Count. As a string, it is the name you assigned to

the ordered geometrical set using the

AnyObject.Name property.

Returns:

The retrieved ordered geometrical set

Example:

This example retrieves in ThisOrderedGeometricalSet the fifth ordered

geometrical set in the collection and in ThatOrderedGeometricalSet the ordered

geometrical set named MyOrderedGeometricalSet in the ordered geometrical set

collection of the partDoc part document.

Set orderedGeometricalSetColl = partDoc.Part.OrderedGeometricalSets

Set ThisOrderedGeometricalSet = orderedGeometricalSetColl.Item(5)

Set ThatOrderedGeometricalSet = orderedGeometricalSetColl.Item(“MyOrderedGeometricalSet”)

Note

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o Property PlaneXY() As AnyObject (Read Only)

Returns the XY plane of the part 3D reference axis system.

Example:

The following example returns in plnXY the XY plane of the partRoot

part from the partDoc part document:

Set partRoot = partDoc.Part

Set plnXY = partRoot.originElements.PlaneXY

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o Property PlaneYZ() As AnyObject (Read Only)

Returns the YZ plane of the part 3D reference axis system.

Example:

The following example returns in plnYZ the YZ plane of the partRoot

part from the partDoc part document:

Set partRoot = partDoc.Part

Set plnYZ = partRoot.originElements.PlaneYZ

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o Property PlaneZX() As AnyObject (Read Only)

Returns the ZX plane of the part 3D reference axis system.

Example:

The following example returns in plnZX the ZX plane of the partRoot

part from the partDoc part document:

Set partRoot = partDoc.Part

Set plnZX = partRoot.originElements.PlaneZX

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o Sub Activate(AnyObject iObject)

Unsuppresses an object for the update process. A unsuppressed object is

again taken into account for the calculation of the part.

Parameters:

iObject

The object to unsuppress for the update process

Example:

The following example unsuppresses the pad1 pad:

Set partRoot = partDoc.Part

Set pad1 = partRoot.FindObjectByName(“Pad.1”)

partRoot.Activate(pad1)

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o Property AnnotationSets() As Collection (Read Only)

Returns the collection object containing the annotation sets. All the

annotation sets that are aggregated in the part might be accessed thru that

collection.

Example:

The following example returns in annotationSets the annotation sets of

the partRoot part from the partDoc part document:

Set partRoot = partDoc.Part

Dim annotationSets As AnnotationSets

Set annotationSets = partRoot.AnnotationSets

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o Property AxisSystems() As AxisSystems (Read Only)

Returns the collection object containing the coordinate systems. All the

coordinate systems that are aggregated in the part might be accessed thru that

collection.

Example:

The following example returns in axisSystems the coordinate systems of

the partRoot part from the partDoc part document:

Set partRoot = partDoc.Part

Dim axisSystems As AxisSystems

Set axisSystems = partRoot.AxisSystems

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o Property Bodies() As Bodies (Read Only)

Returns the collection object containing the bodies that are direct

children of the part.

It does not return all the bodies of the part, particularly the bodies in a

boolean operation.

Example:

The following example returns in bodiesColl the collection of the

bodies of the partRoot part from the partDoc part

document:

Set partRoot = partDoc.Part

Set bodiesColl = partRoot.Bodies

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o Property Constraints() As Constraints (Read Only)

Returns the collection object containing the part constraints. Only 3D

constraints are concerned here, 2D constraints are managed in

sketches.

Example:

The following example returns in csts the constraints of the partRoot

part from the partDoc part document:

Set partRoot = partDoc.Part

Set csts = partRoot.Constraints

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o Func CreateReferenceFromBRepName(CATBSTR iLabel,

AnyObject iObjectContext) As Reference

Creates a reference from a GenericNaming label. This allows manipulation of

B-Rep (Type Functinal and Relimited) that are not easy to

access.

Parameters:

iLabel

The GenericNaming identification for an object. This is a cryptic

form for “the edge surrounded by the face extruded from line.12 of sketch.4 and

the face…”)

iObjectContext

The Object Context of Resolution This is the feature used for label

GenericNaming resolution

Returns:

The reference to a B-Rep sub-element such a face or an edge

Note

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o Func CreateReferenceFromName(CATBSTR iLabel) As Reference

Creates a reference from a GenericNaming label. This allows manipulation of

B-Rep (type Functional Only) that are not easy to access.

Parameters:

iLabel

The GenericNaming identification for an object. This is a cryptic

form for “the edge surrounded by the face extruded from line.12 of sketch.4 and

the face…”)

Returns:

The reference to a B-Rep sub-element such a face or an edge

Note

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o Func CreateReferenceFromObject(AnyObject iObject) As

Reference

Creates a reference from a operator. Use of reference allows a uniform

handling of B-Rep and non B-Rep objects.

Parameters:

iObject

The geometric object to be referenced. It can be a plane, a line or

a point.

Returns:

The reference to the object. This way, a direction can be either an

edge of a pad or a 3D line.

Note

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o Property Density() As double (Read Only)

Returns the part density.

Example:

The following example displays the density of the

part:

Set partRoot = partDoc.Part

MsgBox “The density is ” & partRoot.Density

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o Func FindObjectByName(CATBSTR iObjName) As AnyObject

Finds an object that is not a collection by its name. Scan in depth among

all the direct and indirect children (expensive, but hard to

escape).

Parameters:

iObjName

The name to be searched

Returns:

The object, if found

Example:

The following example tests if the object was found:

Set partRoot = partDoc.Part

Set obj = partRoot.FindObjectByName(“Wrong name”)

If TypeName(obj)=”Nothing” Then

MsgBox “Object not found”

End If

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o Property GeometricElements() As GeometricElements (Read

Only)

Returns the collection object containing the part geometrical elements.

Only 3D elements are concerned here, 2D elements are managed in sketches. The

origin elements are also accessible thru that collection.

Example:

The following example returns in geomElts the 3D elements of the

partRoot part from the partDoc part document:

Set partRoot = partDoc.Part

Set geomElts = partRoot.GeometricElements

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o Func GetCustomerFactory(CATBSTR iFactoryIID) As Factory

Returns a customer factory from a code string defined by the customer. It

allows a customer to define its own factory to create its own

objects.

Parameters:

iFactoryIID

The code name of the factory

Note

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o Property HybridBodies() As HybridBodies (Read Only)

Returns the collection object containing the hybrid bodies that are direct

children of the part.

Example:

The following example returns in hybridBodiesColl the collection of

hybrid bodies of the partRoot part from the partDoc part

document:

Set partRoot = partDoc.Part

Set hybridBodiesColl = partRoot.HybridBodies

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o Property HybridShapeFactory() As Factory (Read Only)

Returns the part hybrid shape factory. It allows the creation of hybrid

shapes in the part.

Example:

The following example returns in hybridShapeFact the hybrid shape

factory of the partRoot part from the partDoc part

document:

Set partRoot = partDoc.Part

Dim hybridShapeFact As Factory

Set hybridShapeFact = partRoot.HybridShapeFactory

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o Property InWorkObject() As AnyObject

Returns or sets the in work object of the part. The in work object is the

object after which a new object is added.

Example:

Set partRoot = partDoc.Part

Set partRoot.InWorkObject = cylindricPad

If ( partRoot.InWorkObject <> cylindricPad ) Then

MsgBox “There is a big problem”

End If

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o Sub Inactivate(AnyObject iObject)

Suppresses an object from being updated. A suppressed object is not taken

into account for the calculation of the part.

Parameters:

iObject

The object to suppress from being updated

Example:

The following example suppresses the pad1 pad from being

updated:

Set partRoot = partDoc.Part

Set pad1 = partRoot.FindObjectByName(“Pad.1”)

partRoot.Inactivate(pad1)

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o Func IsInactive(AnyObject iObject) As boolean

Indicates whether an object is deactivated. A deactivated object is not

taken into account for the calculation of the part.

Parameters:

iObject

The object to examine

Example:

The following example returns in isInactive whether the pad1 pad is

deactivated:

Set partRoot = partDoc.Part

Set pad1 = partRoot.FindObjectByName(“Pad.1”)

isInactive = partRoot.IsInactive(pad1)

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o Func IsUpToDate(AnyObject iObject) As boolean

Indicates whether an object needs to be updated. An object which is not

up-to-date has not be calculated with the last

specifications.

Parameters:

iObject

The object to examine

Example:

The following example returns in isuptodate whether the pad1 pad is

up-to-date:

Set partRoot = partDoc.Part

Set pad1 = partRoot.FindObjectByName(“Pad.1”)

isuptodate = partRoot.IsUpToDate(pad1)