=== enum_CATAxisSystemAxisType_35022 ===
MecModInterfaces CATAxisSystemAxisTypeEnumeration
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CATAxisSystemAxisType (Enumeration)
enum CATAxisSystemAxisType {
catAxisSystemAxisSameDirection,
catAxisSystemAxisByCoordinates,
catAxisSystemAxisOppositeDirection
}
Specification of the axes of the coordinate system.
Values:
catAxisSystemAxisSameDirection
= 0 Specifies that the axis direction is defined by a point, line, or plane.
If the axis is defined by a point, the axis has the direction of the vector
going from the origin of the coordinate system to the point.
If defined by a line, the axis has the same direction as the line.
If defined by a plane, the axis has the same direction as the normal vector of the plane.
catAxisSystemAxisByCoordinates
= 1 Specifies that the axis direction is defined by the three coordinates x,y,z of a vector.
catAxisSystemAxisOppositeDirection
= 2 Specifies that the axis direction is not specified or defined by a point, line, or plane.
If the axis is defined by a point, the axis has the direction of the vector
going from the point to the origin of the coordinate system.
If defined by a line, the axis has the opposite direction of the line.
If defined by a plane, the axis has the opposite direction of the normal vector of the plane.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CATAxisSystemMainType_34776 ===
MecModInterfaces CATAxisSystemMainTypeEnumeration
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CATAxisSystemMainType (Enumeration)
enum CATAxisSystemMainType {
catAxisSystemStandard,
catAxisSystemAxisRotation,
catAxisSystemEulerAngles,
catAxisSystemExplicit
}
Axis System type.
Values:
catAxisSystemStandard
= 0 Specifies that the axis system is defined by an origin point and three axes
catAxisSystemAxisRotation
= 1 Specifies that the axis system is defined by an origin point, and a rotation around one axis
catAxisSystemEulerAngles
= 2 Specifies that the axis system is defined by an origin point, and the three Euler angles
catAxisSystemExplicit=
30 Specifies that the axis system is a datum.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CATAxisSystemOriginType_39529 ===
MecModInterfaces CATAxisSystemOriginTypeEnumeration
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CATAxisSystemOriginType (Enumeration)
enum CATAxisSystemOriginType {
catAxisSystemOriginByPoint,
catAxisSystemOriginByCoordinates
}
Axis System Origin.
Values:
catAxisSystemOriginByPoint
= 0 Specifies that the origin point is put at the position 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.
catAxisSystemOriginByCoordinates
= 1 Specifies that the origin point must stay at the position defined by  three coordinates x,y,z.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintAngleSector_41773 ===
MecModInterfaces CatConstraintAngleSectorEnumeration
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CatConstraintAngleSector (Enumeration)
enum CatConstraintAngleSector {
catCstAngleSector0,
catCstAngleSector1,
catCstAngleSector2,
catCstAngleSector3
}
Special constraint property for angle constraints.
It only applies to the constraints of type Angle or PlanarAngle.
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 angular
sectors, numbered from 0 to 3.
By default, the constraint is created in the sector number 0.
One angular sector corresponds exactly to particular values
of the Dimension.Value, the Side and the Orientation.
When changing the angular sector, the Dimension.Value, Side and Orientation
are also modified.
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.
Values:
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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintDistConfig_39178 ===
MecModInterfaces CatConstraintDistConfigEnumeration
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CatConstraintDistConfig (Enumeration)
enum CatConstraintDistConfig {
catCstDCUnspec,
catCstDCParallel,
catCstDCParallelSameOrient,
catCstDCParallelOppOrient
}
Special constraint configurations for distance constraints.
When distance constraints involve lines or cylinders, the constrained
elements  can  rotate around the line on which the distance is
measured, while still respecting the distance constraint. This degree of
freedom is in most cases not wanted.
This enum is used to further qualify the distance constraint, so that
such  degree of freedom can be eliminated in case of need, without
requiring another distinct constraint to be defined.
Values:
catCstDCUnspec
No additional condition is set on the constraint.
catCstDCParallel
In addition to being positioned at a given distance, constrained
elements are required to be parallel. Their orientation can be
the same or opposite.
catCstDCParallelSameOrient
In addition to being positioned at a given distance, constrained
elements are required to be parallel, and their orientations
are required to be the same.
catCstDCParallelOppOrient
In addition to being positioned at a given distance, constrained
elements are required to be parallel, and their orientations
are required to be opposite.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintDistDirection_47132 ===
MecModInterfaces CatConstraintDistDirectionEnumeration
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CatConstraintDistDirection (Enumeration)
enum CatConstraintDistDirection {
catCstDistDirectionNone,
catCstDistDirection1,
catCstDistDirection2,
catCstDistDirection3
}
Constraint distance direction.
DistanceDirection. This enum lists the appropriate values to
set this property.
Values:
catCstDistDirectionNone
No direction has been specified.
The constraint is measured as usual.
catCstDistDirection1
2D : The constraint is measured along the horizontal axis.
3D : The constraint is measured along the X axis.
catCstDistDirection2
2D : The constraint is measured along the vertical axis.
3D : The constraint is measured along the Y axis.
catCstDistDirection3
3D : The constraint is measured along the Z axis.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintMode_27176 ===
MecModInterfaces CatConstraintModeEnumeration
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CatConstraintMode (Enumeration)
enum CatConstraintMode {
catCstModeDrivingDimension,
catCstModeDrivenDimension
}
Constraint working mode
Part constraints can work in two modes: as constraints or as measurements.
In constraint mode, the value assigned to the constraint
drives the  actual  position of the constrained geometry.
In measurement mode, the constraint value only reflects what
can be observed from the actual position of the constrained geometry.
Values:
catCstModeDrivingDimension
Specifies that a constraint should work as a constraint.
catCstModeDrivenDimension
Specifies that a constraint should work as a measurement.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintOrientation_42617 ===
MecModInterfaces CatConstraintOrientationEnumeration
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CatConstraintOrientation (Enumeration)
enum CatConstraintOrientation {
catCstOrientSame,
catCstOrientOpposite,
catCstOrientUndefined
}
Constraint elements relative orientation.
When two geometrical elements are constrained, there is often a variety
of relative positions and orientations of these elements that respect
the constraint. For instance,
if a distance constraint is placed on two planes,
the second plane can lie on both sides of first plane while maintaining
the requested distance: the constraint is respected, but
geometry remains unresolved. Furthermore, even if the side is fixed,
second plane still can be oriented so that its normal points towards the
first plane or in the opposite direction, without breaking the constraint.
Managing such indetermination requires control over two variables:
Side
determines, when relevant, on which side of each other constrained
elements should be positionned
Orientation
determines, when relevant, how to orient constrained elements,
whith respect to each other.
This enum deals with possibles options for dealing with the
Orientation variable (see  for possibles options for Side).
This enum is based on the notion of characteristic vector. A
characteristic vector is a vector which is associated with a constrained
element each time it can be assimilated to a line or a plane. The vector
represents the direction of the line, or the direction normal to the
plane.
Values:
catCstOrientSame
specifies that characteristic vectors associated to  constrained
elements have same orientation.
catCstOrientOpposite
specifies that characteristic vectors associated to constrained
elements have opposite orientation.
catCstOrientUndefined
specifies that the relative orientation of characteristic vectors
associated to constrained elements is not specified
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintRefAxis_32670 ===
MecModInterfaces CatConstraintRefAxisEnumeration
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CatConstraintRefAxis (Enumeration)
enum CatConstraintRefAxis {
catCstRefAxisX,
catCstRefAxisY,
catCstRefAxisZ
}
Constraint reference axis.
Constraints that specify parallelism or perpendicularity to an
axis in 3D are mono-element constraints. The axis to which the
constraint applies is determined by the constraint property
ReferenceAxis. This enum lists appropriate values to
set this property.
Values:
catCstRefAxisX
The constraint applies to the X axis.
catCstRefAxisY
The constraint applies to the Y axis.
catCstRefAxisZ
The constraint applies to the Z axis.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintRefType_32851 ===
MecModInterfaces CatConstraintRefTypeEnumeration
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CatConstraintRefType (Enumeration)
enum CatConstraintRefType {
catCstRefTypeRelative,
catCstRefTypeFixInSpace
}
Constraint reference type.
In the PartDesign context, an element having a Reference constraint
will not move during the update.
The Assembly context allows two behaviours :
Either the element will not move,
or the element will move to the position where it was when
the Reference type has been set to FixInSpace.
ReferenceType. This enum lists appropriate values to
set this property.
Values:
catCstRefTypeRelative
The element will not move during the update (the default mode).
catCstRefTypeFixInSpace
The element will move to its former position (Assembly context only).
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintSide_27170 ===
MecModInterfaces CatConstraintSideEnumeration
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CatConstraintSide (Enumeration)
enum CatConstraintSide {
catCstSidePositive,
catCstSideNegative,
catCstSideSameAsValue,
catCstSideOppositeToValue,
catCstSideUndefined
}
Constrained elements relative side.
When two geometrical elements are constrained, there is often a variety
of relative positions and orientations of these elements that respect
the constraint. For instance,
if a distance constraint is placed on two planes,
the second plane can lie on both sides of first plane while maintaining
the requested distance: the constraint is respected, but
geometry remains unresolved. Furthermore, even if the side is fixed,
second plane still can be oriented so that its normal points towards the
first plane or in the opposite direction, without breaking the constraint.
Managing such indetermination requires control over two variables:
Side
determines, when relevant, on which side of each other constrained
elements should be positionned
Orientation
determines, when relevant, how to orient constrained elements,
whith respect to each other.
This enum deals with possibles options for dealing with the Side
variable (see  for possibles options for Orientation).
This enum is based on the notion of characteristic vector. A
characteristic vector is a vector which is associated with a constrained
element each time it can be assimilated to a line or a plane. The vector
represents the direction of the line, or the direction normal to the
plane.
Values:
catCstSidePositive
First constrained element characteristic vector points towards
second constrained element.
Arithmetic sign of constraint value is ignored, only its absolute
value is taken into account.
catCstSideNegative
First constrained element characteristic vector points opposite to
second constrained element.
Arithmetic sign of constraint value is ignored, only its absolute
value is taken into account.
catCstSideSameAsValue
Arithmetic sign of constraint value specifies where second element
lies with regard to first one: a positive value means in the direction
of first constrained element characteristic vector, a negative value in
the opposite direction.
catCstSideOppositeToValue
Arithmetic sign of constraint value specifies where second element
lies with regard to first one: a negative value means in the direction
of first constrained element characteristic vector, a positive value in
the opposite direction.
catCstSideUndefined
Relative positionning of constrained elements is not defined.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintStatus_31578 ===
MecModInterfaces CatConstraintStatusEnumeration
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CatConstraintStatus (Enumeration)
enum CatConstraintStatus {
catCstStatusOK,
catCstStatusKOStronglyNotSatisfied,
catCstStatusKOWrongOrientOrSide,
catCstStatusKOWrongValue,
catCstStatusKOWrongGeomEltType,
catCstStatusKOBroken
}
Possible state of a constraint.
Indicates whether a constraint is
satisfied or not, along with a diagnosis when not satisfied.
Values:
catCstStatusOK
The constraint is satisfied.
catCstStatusKOStronglyNotSatisfied
The constraint is strongly not satisfied (e.g. distance constraint
between two planes, which are not currently parallel).
catCstStatusKOWrongOrientOrSide
The constraint is not satisfied because of the wrong orientation or
side of its geometric elements (e.g. planes are parallel and at
the specified distance, but their orientation is inverted with
respect to the one specified by the constraint).
catCstStatusKOWrongValue
The constraint is not satisfied because of its value
(e.g. planes are parallel and at the specified orientation and side
but not at the specified distance).
catCstStatusKOWrongGeomEltType
The constraint is not satisfied because of the wrong type of
its geometric elements (e.g.  angle between a point and a plane).
It can happen in an assembly when replacing a part by another.
catCstStatusKOBroken
The constraint is not satisfied because a geometric element is
missing. It can happen in an assembly when a part is missing.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatConstraintType_27587 ===
MecModInterfaces CatConstraintTypeEnumeration
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CatConstraintType (Enumeration)
enum CatConstraintType {
catCstTypeReference,
catCstTypeDistance,
catCstTypeOn,
catCstTypeConcentricity,
catCstTypeTangency,
catCstTypeLength,
catCstTypeAngle,
catCstTypePlanarAngle,
catCstTypeParallelism,
catCstTypeAxisParallelism,
catCstTypeHorizontality,
catCstTypePerpendicularity,
catCstTypeAxisPerpendicularity,
catCstTypeVerticality,
catCstTypeRadius,
catCstTypeSymmetry,
catCstTypeMidPoint,
catCstTypeEquidistance,
catCstTypeMajorRadius,
catCstTypeMinorRadius,
catCstTypeSurfContact,
catCstTypeLinContact,
catCstTypePoncContact,
catCstTypeChamfer,
catCstTypeChamferPerpend,
catCstTypeAnnulContact,
catCstTypeCylinderRadius,
catCstTypeStContinuity,
catCstTypeStDistance,
catCstTypeSdContinuity,
catCstTypeSdShape
}
Possible types of constraints.
According to their type, constraint may exist in 3D space (at the part
level), in 2D space (at the sketch level), or both.
The constraint type also determines the number of elements (from
1 to 3) that are necessary to define the constraint, plus the
type of those elements. Also, the constraint type defines the
valid combinations between those types, and the associated semantics.
These combinations plus usage notes are detailed in tables on a per-type
basis below.
Values:
catCstTypeReference
catCstTypeReference Definition
Constraint valid in
2D  & 3D
# of needed elements
1
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line, Circle or Arc, Ellipse or Arc, parabola, Hyperbola,
Polynomial curve, Spline
Possible configurations (2D)
1rst elt type
Definition
Notes
All types
The element support is not modifiable
--
Constraint definition in 3D space
Valid types for 1rst elt
Point, Line, Plane, Cylinder, Sphere, Cone
Possible configurations (3D)
1rst elt type
Definition
Notes
All types
The element cannot move with respect to the bloc that contains it
--
catCstTypeDistance
catCstTypeDistance between 2 elements Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line, Circle or Arc, Ellipse or Arc, Parabola,
Hyperbola, Polynomial curve, Spline
Valid types for 2nd elt
Same as 1rst elt
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Point
Point
Distance between points is equal to constraint value
--
Point
Curve
Constraint is measured between point and its closest projection onto
curve. Constraint value is equal to that distance.
"Curve" means every possible type except point
Curve
Curve
Constraint is measured at points on curves that mutually project onto the
other curve, and such as their distance is minimum. Constraint value is
this distance.
"Curve" means every possible type except point
Constraint definition in 3D space
Valid types for 1rst Elt
Point, Line, Plane, Cylinder, Sphere, Cone
Valid types for 2nd Elt
Same as 1rst elt
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
...with point
Point
Point
Distance between points is equal to constraint value.
--
Point
Line
Distance between point and its projection onto line support
is equal to constraint value.
--
Point
Plane
Distance between point and its projection onto plane
is equal to constraint value.
See
for managing the relative position of constrained elements
Point
Cylinder
Constraint is measured along the line, perpendicular to cylinder axis,
that contains point. Constraint value is equal to the distance between the
point and the cylinder surface, measured along this line.
See
for managing the placement of point relative to the normal to the
cylinder at projection point.
Point
Sphere
Constraint is measured along the line passing through
point and sphere center. Constraint value is equal to the distance between
point  and sphere surface, measured along this line.
See
for managing the placement of point relative to the normal to the
sphere at projection point.
...with line
Line
Line
Constraint is measured along the common perpendicular to both lines.
Constraint value is equal to the distance between both lines measures
on this perpendicular.
See
for further specifying parallelism conditions on lines.
Line
Plane
Line is parallel to plane, i.e. line lies within a plane parallel to plane.
Constraint value is equal to distance between those planes.
See
for managing the relative position of line and plane
Line
Cylinder
Same as Line/Line case, but  constraint value is measured
between line and cylinder surface.
See
for managing on which side of measurement point on first element
is second element located (relative to  the direction of normal to
element at that point).
See
for managing wether the distance to second element is measured on the
inside or on the outside of it: it mutually orients the normals
taken at measurement points on both elements.
Line
Sphere
Constraint is measured on the line by which sphere center projects
onto line.
Constraint value is equal to the distance between that projection
point and the sphere surface.
See
for managing the relative position of line regarding the normal to
sphere at constraint measurement point.
...with plane
Plane
Plane
Planes are parallel and constraint value is equal to their distance.
See
for managing on which side of measurement point on first element
is second element located (relative to  the direction of normal to
element at that point).
See
for managing wether the distance to second element is measured on the
inside or on the outside of it: it mutually orients the normals
Plane
Cylinder
Plane is parallel to cylinder axis (as in Plane/Line case) and
constraint value is measured between plane and cylinder surface.
See
for managing on which side of measurement point on first element
is second element located (relative to  the direction of normal to
element at that point).
See
for managing wether the distance to second element is measured on the
inside or on the outside of it: it mutually orients the normals
taken at measurement points on both elements.
Plane
Sphere
Constraint value is equal to distance between plane and sphere surface.
See
for managing the relative position of plane and sphere.
See
for managing the relative orientation of plane normal and
normal to sphere at constraint measurement point.
...with cylinder
Cylinder
Cylinder
Similar to a Line/Line distance constraint applied to
cylinder axis, but constraint value is
measured between cylinder surfaces.
See
for managing on which side of measurement point on first element
is second element located (relative to  the direction of normal to
element at that point).
See
for managing wether the distance to second element is measured on the
inside or on the outside of it: it mutually orients the normals
taken at measurement points on both elements.
See
for further specifying parallelism conditions on cylinders axes.
Cylinder
Sphere
Similar to a Line/Point distance constraint applied to
cylinder axis and sphere center, but constraint value is
measured between cylinder and sphere surfaces.
See
for managing on which side of measurement point on first element
is second element located (relative to  the direction of normal to
element at that point).
See
for managing wether the distance to second element is measured on the
inside or on the outside of it: it mutually orients the normals
taken at measurement points on both elements.
...with sphere
Sphere
Sphere
Similar to a Point/Point distance constraint applied between spheres
centers, but
constraint value is measured between spheres surfaces.
See
for managing where second measurement point is taken on second sphere:
normals to spheres at measurement points may be or not oriented in
the same direction, thus defining two possible measurement points.
See
for managing the direction of constraint measurement relative to
normal vector to first sphere.
Sphere
Cone
Similar to a Point/Cone distance constraint applied between sphere center and
cone, but constraint value is measured between sphere and cone surfaces.
--
catCstTypeDistance
catCstTypeDistance with 3 elements Definition
Constraint valid in
2D & 3D
# of needed elements
3
Constraint definition in 2D space
Valid types for 1rst elt
same as catCstTypeDistance
Valid types for 2nd elt
same as catCstTypeDistance
Valid types for 3rd elt
Line
Possible combinations (2D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Same as catCstTypeDistance
Same as catCstTypeDistance
Line
The difference with the distance between 2 elements is that
the third element is a projection direction.
The distance is measured after projection on the third element.
--
Constraint definition in 3D space
Valid types for 1rst elt
same as catCstTypeDistance
Valid types for 2nd elt
same as catCstTypeDistance
Valid types for 3rd elt
Line, plane
Possible combinations (2D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Same as catCstTypeDistance
Same as catCstTypeDistance
Line or plane
The distance is measured after projection on the third element.
--
catCstTypeOn
catCstTypeOn Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line, Circle or Arc, Ellipse or Arc
Valid types for 2nd elt
Same as 1rst elt
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
All Types
All Types
Constrained elements supports are identical.
Support mean the element considered without limitation (e.g.
the underlying infinite line for a line segment).
Constraint definition in 3D space
Valid types for 1rst elt
Point, Line, Plane, Cylinder, Sphere, Cone, Circle
Valid types for 2nd elt
Same as 1rst elt
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
Point
Point
Points lie at the same location.
--
Point
Line
Points lie on line support.
--
Point
Plane
Point lies within plane.
--
Point
Cylinder
Point lies on cylinder surface.
--
Point
Sphere
Point lies on sphere surface.
--
Line
Line
Lines supports are identical.
See
for managing the relative orientation of lines.
Line
Plane
Line lies within plane.
--
Line
Cylinder
One of the cylinder generating lines and line supports are the same.
See
for managing the relative orientation of line support and Cylinder
axis.
Line
Sphere
Line support contains sphere center.
--
Plane
Plane
Both planes are identical.
See
for managing the relative orientation of planes.
Sphere
Sphere
Spheres centers and radii are identical.
--
Cylinder
Cylinder
Both cylinder supports are identical.
Cylinder are considered infinite in length.
Cone
Cone
Both cones supports are identical.
Cones are considered infinite in heigth.
Cone
Circle
The circle lies on the cone.
See
for managing the relative orientation of the plane of the circle.
catCstTypeConcentricity
catCstTypeConcentricity Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Point, Circle or Arc, Ellipse or Arc
Valid types for 2nd elt
Same as 1rst elt
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Point
Circle
Circle center lies on point.
--
Circle
Circle
Circle centers lie on each other.
--
Point
Ellipse
Ellipse center lies on point.
--
Ellipse
Circle
Ellipse center lies on circle center.
--
Ellipse
Ellipse
Ellipse center lies on ellipse center.
--
Constraint definition in 3D space
Valid types for 1rst elt
Sphere
Valid types for 2nd elt
Sphere
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
Sphere
Sphere
Both spheres centers are the same.
--
catCstTypeTangency
catCstTypeTangency Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line, Circle or Arc, Ellipse or Arc, Parabola,
Hyperbola, Polynomial curve, Spline
Valid types for 2nd elt
Same as 1rst elt
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
All types
All types
A point exists, where both elements supports are tangent.
This constraint type cannot be defined between two lines.
Constraint definition in 3D space
Valid types for 1rst elt
Line, Plane, Cylinder, Sphere, Cone
Valid types for 2nd elt
Cylinder, Sphere, Cone
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
Line
Cylinder
Line is tangent to cylinder.
--
Line
Sphere
Line is tangent to sphere.
--
Plane
Cylinder
Plane is tangent to cylinder.
See
for managing the relative orientation of plane and cylinder normals.
Plane
Sphere
Plane is tangent to Sphere.
See
for managing the relative orientation of plane and sphere normals.
Cylinder
Cylinder
Both cylinders are tangent.
See
for managing the relative orientation of both cylinder normals at
tangency point. See
for       adding additional parallelism requirements on the constraint.
Cylinder
Sphere
Cylinders is tangent to sphere.
See
for managing the relative orientation of cylinder and sphere normals.
Sphere
Sphere
Both spheres are tangent.
See
for managing the relative orientation of both spheres normals.
Cone
Cone
Both cones are tangent through on of their gererating lines.
See
for managing the relative orientation of both generating lines.
catCstTypeLength
catCstTypeLength Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D space
Valid types for 1rst elt
Line
Possible combinations(2D)
1rst elt type
Definition
Notes
Line
Line length is equal to constraint value.
--
catCstTypeAngle
catCstTypeAngle Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Line
Line
Angle between lines supports is equal to constraint value.
The angle is measured in degrees, within the 0-360 range.
Constraint definition in 3D space
Valid types for 1rst elt
Line, Plane
Valid types for 2nd elt
Line, Plane
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
Line
Line
The common perpendicular to both lines defines the normal to the measuring
plane. Both lines direction vector is projected onto that plane. The
constraint value is equal to the angular difference between those two projected vectors.
Angle is measured in degree, in the 0-180 range.
Line
Plane
Constraint value is equal to the angular difference between the line
direction vector and its projection onto the plane.
Angle is measured in degree, in the 0-180 range.
Plane
Plane
Constraint value is equal to the angular difference between the normals to
both planes.
Angle is measured in degree, in the 0-180 range.
catCstTypePlanarAngle
catCstTypePlanarAngle Definition
Constraint valid in
3D
# of needed elements
3
Constraint definition in 3D space
Valid types for 1rst elt
Plane
Valid types for 2nd elt
Plane
Valid types for 3rd elt
Line
Possible combinations (3D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Plane
Plane
Line
Line lies at the intersection of both planes. Angle is measured in the normal
plane to line.
Angle is measured in degrees, in the 0-360 range, in the direct sense
of the measuring plane deduced for the line orientation.
catCstTypeParallelism
catCstTypeParallelism Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Line
Line
Both lines supports are parallel.
See
for managing the relative orientation of lines.
Constraint definition in 3D space
Valid types for 1rst elt
Line, Plane
Valid types for 2nd elt
Line, Plan
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
Line
Line
Both lines supports are parallel.
See
for managing the relative orientation of lines.
Line
Plane
Lines support is parallel to plane.
See
for managing the relative position of line and plane
Plane
Plane
Planes are parallel.
See
and
for managing the relative positioning and orientation of planes.
catCstTypeAxisParallelism
catCstTypeAxisParallelism Definition
Constraint valid in
3D
# of needed elements
1
Constraint definition in 3D space
Valid types for 1rst elt
Line, Plane, Cylinder
Possible combinations(3D)
1rst elt type
Definition
Notes
All types
Element is parallel to one of the 3D space axes.
See
for managing which axis the constraint applies to.
See
for managing the relative orientation of element and axis in the case
of line and cylinder.
catCstTypeHorizontality
catCstTypeHorizontality Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D space
Valid types for 1rst elt
Line
Possible combinations(2D)
1rst elt type
Definition
Notes
Line
Line is parallel to the horizontal component of the reference axis.
--
catCstTypePerpendicularity
catCstTypePerpendicularity Definition
Constraint valid in
2D  & 3D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Line
Line
Lines support are perpendicular.
--
Constraint definition in 3D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line, Plane, Cylinder
Possible combinations (3D)
1rst elt type
2nd  elt type
Definition
Notes
...with line
Line
Line
Lines support are perpendicular.
--
Line
Plane
Line is perpendicular to plane.
See
for managing the relative orientation of line direction vector
and normal to plane.
Line
Cylinder
Lines support is perpendicular to cylinder axis.
--
catCstTypeAxisPerpendicularity
catCstTypeAxisPerpendicularity Definition
Constraint valid in
3D
# of needed elements
1
Constraint definition in 3D space
Valid types for 1rst elt
Line, Plane, Cylinder
Possible combinations(3D)
1rst elt type
Definition
Notes
All types
Element is perpendicular to one of the 3D space axes.
See
for managing which axis the constraint applies to.
See
for managing the relative orientation of element and axis in the case
of line and cylinder.
catCstTypeVerticality
catCstTypeVerticality Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D space
Valid types for 1rst elt
Line
Possible combinations(2D)
1rst elt type
Definition
Notes
Line
Line is parallel to the vertical component of the reference axis.
--
catCstTypeRadius
catCstTypeRadius Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D space
Valid types for 1rst elt
Circle or Arc
Possible combinations(2D)
1rst elt type
Definition
Notes
Circle/Arc
Circle or arc radius is equal to constraint value.
--
catCstTypeSymmetry
catCstTypeSymmetry Definition
Constraint valid in
2D & 3D
# of needed elements
3
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line, Circle or Arc, Ellipse or Arc
Valid types for 2nd elt
Same as 1rst elt
Valid types for 3rd elt
Line
Possible combinations (3D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
All types
All types
Line
First element is symmetric to second one with respect to line.
Types of first and second elements are the same.
Constraint definition in 3D space
Valid types for 1rst elt
Point, Line, Plane, Cylinder, Sphere, Cone
Valid types for 2nd elt
Same as 1rst elt
Valid types for 3rd elt
Line, Plane
Possible combinations (3D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
All types
All types
Line
First element is symmetric to second one with respect to line.
Types of first and second elements are the same.
Characteristic vectors of symmetric elements are always opposite.
All types
All types
Plane
First element is symmetric to second one with respect to plane.
Types of first and second elements are the same.
Characteristic vectors of symmetric elements are always opposite.
catCstTypeMidPoint
catCstTypeMidPoint Definition
Constraint valid in
2D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Point
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Point
Line
Point is equally distant from both line extremities.
--
catCstTypeEquidistance
catCstTypeEquidistance Definition
Constraint valid in
2D
# of needed elements
3
Constraint definition in 2D space
Valid types for 1rst elt
Point, Line
Valid types for 2nd elt
Same as 1rst elt
Valid types for 3rd elt
Point
Possible combinations (3D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Point
Point
Point
Third point is equally distant from first and second one.
--
Line
Line
Point
Third point is equally distant from each of its projections onto
first and second line.
--
catCstTypeMajorRadius
catCstTypeMajorRadius Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D
space
Valid types for 1rst elt
Ellipse or Arc
Possible combinations(2D)
1rst elt type
Definition
Notes
Ellipse or Arc
The length of ellipse major axis is equal to constraint value.
Ellipse major axis is the largest of ellipse axes at creation time
catCstTypeMinorRadius
catCstTypeMinorRadius Definition
Constraint valid in
2D
# of needed elements
1
Constraint definition in 2D
space
Valid types for 1rst elt
Ellipse or Arc
Possible combinations(2D)
1rst elt type
Definition
Notes
Ellipse or Arc
The length of ellipse minor axis is equal to constraint value.
Ellipse minor axis is the smallest of ellipse axes at creation time
catCstTypeChamfer
catCstTypeChamfer Definition
Constraint valid in
2D & 3D
# of needed elements
3
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Valid types for 3rd elt
Line
Possible combinations (2D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Line
Line
Line
The chamfer is defined by two lengths and two angles.
The first line is between the second and the third lines.
The first and second lines intersect in one of their extremities.
Idem with the first and third lines.
Constraint definition in 3D space
Valid types for 1rst elt
Plane, Cone
Valid types for 2nd elt
Plane
Valid types for 3rd elt
Plane, Cylinder
Possible combinations (3D)
1rst elt type
2nd  elt type
3rd elt type
Definition
Notes
Plane
Plane
Plane
The chamfer is defined by two lengths and two angles.
The mode of the constraint is catCstModeDrivenDimension.
The first plane is between the second and the third planes.
The normal vectors of the planes are in a same plane.
Cone
Plane
Cylinder
The chamfer is defined by two lengths and two angles.
The cone and the cylinder have the same axis.
The plane is normal to that axis.
The cone is between the plane and the cylinder.
catCstTypeChamferPerpend
catCstTypeChamferPerpend Definition
Constraint valid in
2D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Line
Line
Chamfer is defined by one length and one angle.
The mode of the constraint is catCstModeDrivenDimension.
The third element is implicit because it is perpendicular to the second line
and it intersects the first line in one of their extremities.
catCstTypeCylinderRadius
catCstTypeChamferPerpend Definition
Constraint valid in
2D
# of needed elements
2
Constraint definition in 2D space
Valid types for 1rst elt
Line
Valid types for 2nd elt
Line
Possible combinations (2D)
1rst elt type
2nd elt type
Definition
Notes
Line
Line
The cylinder radius is defined by the distance beetween 2 the lines
which results of the projection of a cylinder on a drawing sheet.
--
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatPartElementsNamingMode_43558 ===
MecModInterfaces CatPartElementsNamingModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatPartElementsNamingMode (Enumeration)
enum CatPartElementsNamingMode {
catNoNamingCheck,
catNamingCheckUnderSameNode,
catNamingCheckWithinUIActiveObject
}
Naming mode parameter's possible values.
Role: This enumeration is used in the  interface.
Values:
catNoCheck
Naming is rule-free,
catNamingCheckUnderSameNode
Two elements cannot have the same name under the same node,
catNamingCheckWithinUIActiveObject
Two elements cannot have the same name within a defined UIActiveObject.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatPartSurfaceElementsLocation_58269 ===
MecModInterfaces CatPartSurfaceElementsLocationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatPartSurfaceElementsLocation (Enumeration)
enum CatPartSurfaceElementsLocation {
catPartBodyLocation,
catXGSLocation
}
Wireframe and surface elements location parameter's possible values.
Role: This enum is used in the  interface.
Values:
catPartBodyLocation
Wireframe and surface elements are created within a PartBody
catXGSLocation
Wireframe and surface elements are created within a G.S. or an O.G.S..
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatPartUpdateMode_26785 ===
MecModInterfaces CatPartUpdateModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatPartUpdateMode (Enumeration)
enum CatPartUpdateMode {
catManualUpdate,
catAutomaticUpdate
}
Update mode setting parameter's possible values.
Role: This enum is used in the  interface.
Values:
catManualUpdate
User has to manually launch update tasks.
catAutomaticUpdate
Update is automatically launched
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AxisSystem_20968 ===
MecModInterfaces AxisSystem (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
AxisSystem (Object)
The object Axis System
A axis system has got one origin point and three orthogonal axes,
crossing at the origin point.
Property Index
AxisRotationAngle
Returns the rotation angle of an axis system.
AxisRotationReference
Returns the reference for the axis rotation.
IsCurrent
Returns True if the axis system is the current one, else returns False.
OriginPoint
Returns or sets the geometric point which defines the origin of the axis system.
OriginType
Returns or sets the way the origin point is defined.
Type
Returns or sets the type of the axis system.
XAxisDirection
Reads or sets the geometric point, line or plane which defines the direction of the X axis.
XAxisType
Reads or sets the way the X axis is specified.
YAxisDirection
Reads or sets the geometric point, line or plane which defines the direction of the Y axis.
YAxisType
Reads or sets the way the Y axis is specified.
ZAxisDirection
Reads or sets the geometric point, line or plane which defines the direction of the Z axis.
ZAxisType
Reads or sets the way the Z axis is specified.
Method Index
GetEulerAngles
Returns the Euler Angles of an axis system.
GetOrigin
Returns the coordinates X,Y,Z of the origin point of the axis system.
GetVectors
Returns the coordinates X,Y,Z of the axes X and Y of the axis system.
GetXAxis
Returns the coordinates X,Y,Z of the X axis of the axis system.
GetYAxis
Returns the coordinates X,Y,Z of the Y axis of the axis system.
GetZAxis
Returns the coordinates X,Y,Z of the Z axis of the axis system.
PutOrigin
Defines the coordinates X,Y,Z of the origin point of the axis system.
PutVectors
Defines the coordinates X,Y,Z of the axes X and Y of the axis system.
PutXAxis
Defines the coordinates X,Y,Z of the X axis of the axis system.
PutYAxis
Defines the coordinates X,Y,Z of the Y axis of the axis system.
PutZAxis
Defines the coordinates X,Y,Z of the Z axis of the axis system.
Properties
Property AxisRotationAngle() As   (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.
Property AxisRotationReference() As
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.
Property IsCurrent() As
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
Property OriginPoint() As
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
Property OriginType() As
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
Property Type() As
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
Property XAxisDirection() As
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
Property XAxisType() As
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
Property YAxisDirection() As
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
Property YAxisType() As
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
Property ZAxisDirection() As
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
Property ZAxisType() As
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
Methods
Sub GetEulerAngles( oFirstAngle, oSecondAngle, 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.
Sub GetOrigin( 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
Sub GetVectors( oVectorX, 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
Sub GetXAxis( 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
Sub GetYAxis( 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
Sub GetZAxis( 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
Sub PutOrigin( 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
Sub PutVectors( iVectorX, 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
Sub PutXAxis( 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
Sub PutYAxis( 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
Sub PutZAxis( 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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AxisSystems_22118 ===
MecModInterfaces AxisSystems (Object)
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AxisSystems (Object)
A collection of all the AxisSystem objects contained in the part.
Method Index
Add
Creates a new AxisSystem and adds it to the AxisSystems collection.
Item
Returns an Axis System using its index or its name from the AxisSystems
collection.
Methods
Func Add() As
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()
Func Item( iIndex) As
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
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")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_BiDimFeatEdge_23586 ===
MecModInterfaces BiDimFeatEdge (Object)
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BiDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is two dimensional.
Role:
This  object may be, for example, the edge of a surface obtained through the extrusion of a spline.
You will create a BiDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a BiDimFeatEdge object is limited, see
.
Example:
This example asks the end user to select an edge, and creates a point on this edge. Here, both
TriDimFeatEdge and BiDimFeatEdge objects are proposed to the user.
Dim InputObjectType(1)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
Set HybridBodies = Document.Part.HybridBodies
Set HybridBody = HybridBodies.Item("Geometrical Set.1")
'We propose to the user that he select an edge
InputObjectType(0)="TriDimFeatEdge"
InputObjectType(1)="BiDimFeatEdge"
Status=Selection.SelectElement2(InputObjectType,"Select an edge",true)
if (Status = "cancel") then Exit Sub
Set Curve = Selection.Item(1).Value
Set HybridShapePointOnCurve = HybridShapeFactory.AddNewPointOnCurveFromDistance(Curve,18.0,False)
HybridBody.AppendHybridShape HybridShapePointOnCurve
Document.Part.InWorkObject = HybridShapePointOnCurve
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Bodies_17670 ===
MecModInterfaces Bodies (Object)
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Bodies (Object)
A collection of all the Body objects contained in the part.
Method Index
Add
Creates a new body and adds it to the Bodies collection.
Item
Returns a body using its index or its name from the Bodies
collection.
Methods
Func Add() As
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()
Func Item( iIndex) As
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
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")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Body_16739 ===
MecModInterfaces Body (Object)
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Body (Object)
The object that manages a sequence of shapes, a set of sketches,
a set of hybrid bodies, a set of ordered geometrical sets and a set of hybrid shapes.
It belongs to the  collection of a
or
object.
Property Index
HybridBodies
Returns the body's HybridBodies collection.
HybridShapes
Returns the list of hybrid shapes included in the body.
InBooleanOperation
Returns True if the body is involved in a boolean operation, else returns False.
OrderedGeometricalSets
Returns the body's OrderedGeometricalSets collection.
Shapes
Returns the body's Shapes collection.
Sketches
Returns the body's Sketches collection.
Method Index
InsertHybridShape
Insert a hybrid shape to the body.
Properties
Property HybridBodies() As   (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
Property HybridShapes() As   (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
Property InBooleanOperation() As   (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
Property OrderedGeometricalSets() As   (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
Property Shapes() As   (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
Property Sketches() As   (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
Methods
Sub InsertHybridShape( 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)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Boundary_19156 ===
MecModInterfaces Boundary (Object)
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Boundary (Object)
Topological cell, such as a face, an edge or a vertex.
Role:
The Boundary objects are basic topological objects, such as the edge of a Pad. Some of them posess
a geometrical feature (planar face, rectilinear edge).
You will create a Boundary object (such as the  object, which is derived, indirectly,  from the Boundary object) using the
,
,
or
method. Then, you pass it to the operator (such as
). Note that, regarding V4 sub-elements, once the data of a CATIA Version 4 Model has been copied to a .CATPart, the sub-elements of the resulting .CATPart are
supported by the
object.  The lifetime of a Boundary object is limited. In particular, after having call
, the Boundary objects are usually no more valid.
See also:
,
,
,
,
,
,
,
,
,
,
,
Note:
objects cannot be selected into the specification tree.
Note:For a
object, the object returned by the
property is the master shape. For example, if we have:
Pad.2
!
!
+                        V
!                      +---+
!                    /   / !
+-- Pad.1          /   /   !
!                /   / one +------+
!               +---+    /       /!
Example:
This example asks the end user to select an edge (using the
object), and creates an edge fillet on this edge:
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select an edge
InputObjectType(0)="TriDimFeatEdge"
Status=Selection.SelectElement2(InputObjectType,"Select an edge",true)
if (Status = "cancel") then Exit Sub
Set EdgeFillet = ShapeFactory.AddNewEdgeFilletWithConstantRadius(Selection.Item(1).Value,1,5.0)
EdgeFillet.EdgePropagation = 1
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Constraint_21016 ===
MecModInterfaces Constraint (Object)
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Constraint (Object)
A geometric constraint set for geometric elements of a part, a sketch,
or a product.
Property Index
AngleSector
Returns or sets the constraint angle (or angular) sector.
Dimension
Returns the constraint dimension.
DistanceConfig
Returns or sets the distance constraint configuration.
DistanceDirection
Returns or sets the distance constraint direction.
Mode
Returns or sets the constraint driving  mode.
Orientation
Returns or sets the constraint orientation.
ReferenceAxis
Returns or sets the constraint reference axis.
ReferenceType
Returns or sets the constraint reference type.
Side
Returns or sets the constraint side.
Status
Returns the constraint status.
Type
Returns the  constraint type.
Method Index
Activate
Unsuppresses a constraint for the update process.
Deactivate
Suppresses the constraint from being updated.
GetConstraintElement
Reads an element of a constraint.
GetConstraintVisuLocation
Returns the constraint visualisation location.
IsInactive
Indicates whether a constraint is suppressed from the update process.
SetConstraintElement
Replaces an element of a constraint.
SetConstraintVisuLocation
Sets a new location for the constraint visualization.
Properties
Property AngleSector() As
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
Property Dimension() As   (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
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
Property DistanceConfig() As
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
Property DistanceDirection() As
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
Property Mode() As
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
Property Orientation() As
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
Property ReferenceAxis() As
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
Property ReferenceType() As
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
Property Side() As
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
Property Status() As   (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
Property Type() As   (Read Only)
Returns the  constraint type.
Example:
The following example returns in cstType the type
of the firstCst constraint:
cstType = firstCst.Type
Methods
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
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
Func GetConstraintElement( iElementNumber) As
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 )
Sub GetConstraintVisuLocation( oAnchorPoint, 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
Func IsInactive() As
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
Sub SetConstraintElement( iElementNumber, 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)
Sub SetConstraintVisuLocation( iNewX, iNewY, 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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Constraints_22166 ===
MecModInterfaces Constraints (Object)
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Constraints (Object)
A collection of all geometric constraints set on a part, a sketch,
or a product.
A constraint collection is created with default values for its properties
(such as value, orientation, etc.). Use the constraint properties
edition services to set them to appropriate values after constraint
creation.
See also:
Property Index
BrokenConstraintsCount
Returns the number of broken constraints from the Constraints collection.
UnUpdatedConstraintsCount
Returns the number of unupdated constraints from the Constraints
collection.
Method Index
AddBiEltCst
Creates a new constraint applying to two geometric elements
and adds it to the Constraints collection.
AddMonoEltCst
Creates a new constraint applying to a single geometric element
and adds it to the Constraints collection.
AddTriEltCst
Creates a new constraint applying to three geometric elements
and adds it to the Constraints collection.
Item
Returns a constraint using its index or its name from the Constraints
collection.
Remove
Removes a constraint from the Constraints collection.
Properties
Property BrokenConstraintsCount() As   (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
Property UnUpdatedConstraintsCount() As   (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
Methods
Func AddBiEltCst( iCstType, iFirstElem, iSecondElem) As
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
object is supported:
.
iSecondElem
The second constrained geometric element
The following
object is supported:
.
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)
Func AddMonoEltCst( iCstType, iElem) As
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
object is supported:
.
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)
Func AddTriEltCst( iCstType, iFirstElem, iSecondElem, iThirdElem) As
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
object is supported:
.
iSecondElem
The second constrained geometric element
The following
object is supported:
.
iThirdElem
The third constrained geometric element
The following
object is supported:
.
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)
Func Item( iIndex) As
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
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")
Sub Remove( 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
property.
Example:
This example removes the last constraint in the collection.
cstList.Remove(cstList.Count)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_CylindricalFace_26456 ===
MecModInterfaces CylindricalFace (Object)
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CylindricalFace (Object)
2-D boundary with a cylindrical geometry.
Role:
This  object may be, for example, the lateral face of a cylinder. You will create a CylindricalFace object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a CylindricalFace object is limited, see
.
Example:
This example asks the end user to select a shape to pattern and a cylindrical face, and creates a circular
pattern of the shape. The cylindrical face specifies the rotation axis.
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select the shape to pattern
InputObjectType(0)="SketchBasedShape"
Status=Selection.SelectElement2(InputObjectType,"Select the shape to pattern",true)
if (Status = "cancel") then Exit Sub
Set Shape = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the cylindrical face
InputObjectType(0)="CylindricalFace"
Status=Selection.SelectElement2(InputObjectType,"Select the cylindrical face",true)
if (Status = "cancel") then Exit Sub
Set CylindricalFace = Selection.Item(1).Value
Set RotationCenter = Document.Part.CreateReferenceFromName("")
Set CircPattern = ShapeFactory.AddNewCircPattern(Shape,1,4,20.0,45.0,1,4,RotationCenter,CylindricalFace,True,0.0,True)
Document.Part.Update
Method Index
GetDirection
Returns the direction of the cylindrical face axis
GetOrigin
Returns the origin of the cylindrical face axis.
Methods
Sub GetDirection( 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
Sub GetOrigin( 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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Edge_16674 ===
MecModInterfaces Edge (Object)
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Edge (Object)
1-D boundary.
Role:
This  object may be, for example, the edge of a cylinder. You will create an Edge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of an Edge object is limited, see
.  See also:
,
,
,
,
,
.
Example:
This example asks the end user to select a planar curve, whose plane is parallel to the XY plane.
Then, it creates a point on the tangent to the curve in the X direction:
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
Set HybridBodies = Document.Part.HybridBodies
Set HybridBody = HybridBodies.Item("Geometrical Set.1")
'We propose to the user that he select a planar curve whose plane is parallel to the XY plane
InputObjectType(0)="Edge"
Status=Selection.SelectElement2(InputObjectType,"Select a planar curve whose plane is parallel to the XY plane",true)
if (Status = "cancel") then Exit Sub
Set PlanarCurve = Selection.Item(1).Value
Set HybridShapeDirection = HybridShapeFactory.AddNewDirectionByCoord(1.0,0.0,0.0)
Set HybridShapePointTangent = HybridShapeFactory.AddNewPointTangent(PlanarCurve,HybridShapeDirection)
HybridBody.AppendHybridShape HybridShapePointTangent
Document.Part.InWorkObject = HybridShapePointTangent
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Face_16663 ===
MecModInterfaces Face (Object)
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Face (Object)
2-D boundary.
Role:
This  object may be, for example, the lateral face of cylinder. You will create a Face object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a Face object is limited, see
.  See also:
,
.
Example:
This example asks the end user to select two faces, and creates a face-face fillet on these faces:
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select the first face
InputObjectType(0)="Face"
Status=Selection.SelectElement2(InputObjectType,"Select the first face",true)
if (Status = "cancel") then Exit Sub
Set FirstFace = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the second face
InputObjectType(0)="Face"
Status=Selection.SelectElement2(InputObjectType,"Select the second face",true)
if (Status = "cancel") then Exit Sub
Set SecondFace = Selection.Item(1).Value
Set FaceFillet = ShapeFactory.AddNewFaceFillet(FirstFace,SecondFace,5.0)
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Factory_18448 ===
MecModInterfaces Factory (Object)
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Factory (Object)
Abstract object gathering behaviours of all objects being a factory.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_FixTogether_21920 ===
MecModInterfaces FixTogether (Object)
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FixTogether (Object)
The object that manages a sequence of products or fixTogethers.
It belongs to the  collection of a
.
Property Index
FixTogethersCount
Returns the number of FixTogether entities in the FixTogether.
ProductsCount
Returns the number of products fixed together in the FixTogether.
Method Index
AddFixTogether
Add a fixTogether to a FixTogether.
AddProduct
Add a product to a FixTogether.
GetFixTogether
Returns a FixTogether using its index or its name in the FixTogether.
GetProduct
Returns a Product using its index or its name in the FixTogether.
RemoveFixTogether
Removes a FixTogether from the FixTogether.
RemoveProduct
Removes a Product from the FixTogether.
Properties
Property FixTogethersCount() As   (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
Property ProductsCount() As   (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
Methods
Sub AddFixTogether( 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)
Sub AddProduct( 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)
Func GetFixTogether( iIndex) As
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
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")
Func GetProduct( iIndex) As
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
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")
Sub RemoveFixTogether( 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
property.
Example:
This example removes the last FixTogether of the FixTogether.
fixTogether.RemoveFixTogether(fixTogether.FixTogethersCount)
Sub RemoveProduct( 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
property.
Example:
This example removes the last Product of the FixTogether.
fixTogether.RemoveProduct(fixTogether.ProductsCount)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_FixTogethers_23185 ===
MecModInterfaces FixTogethers (Object)
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FixTogethers (Object)
A collection of all the FixTogether objects contained in the product.
Method Index
Add
Creates a new FixTogether and adds it to the FixTogethers collection.
Item
Returns a FixTogether using its index or its name from the FixTogethers
collection.
Remove
Removes a FixTogether from the FixTogethers collection.
Methods
Func Add() As
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
Func Item( iIndex) As
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
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")
Sub Remove( 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
property.
Example:
This example removes the last FixTogether in the collection.
fixTogetherColl.Remove(fixTogetherColl.Count)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_GeometricElements_30463 ===
MecModInterfaces GeometricElements (Object)
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GeometricElements (Object)
A collection of all geometric elements contained in a part or a sketch.
Geometric elements are created with the 2D factory for the sketch and with
the 3D factory for the part. Geometric elements thus created are then
aggregated either in the sketch or as part of the geometric element
collection.
See also:
,
Method Index
Item
Returns a geometric element using its index or its name from the
GeometricElements collection.
Methods
Func Item( iIndex) As
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
property.
Returns:
The retrieved geometric element
Example:
This example retrieves the last item in the geometric element collection.
Set lastCst = cstList.Item(cstList.Count)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_HybridBodies_22837 ===
MecModInterfaces HybridBodies (Object)
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HybridBodies (Object)
A collection of the HybridBody objects.
Method Index
Add
Creates a new hybrid body and adds it to the HybridBodies collection.
Item
Returns a body using its index or its name from the Bodies
collection.
Methods
Func Add() As
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()
Func Item( iIndex) As
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
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")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_HybridBody_20706 ===
MecModInterfaces HybridBody (Object)
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HybridBody (Object)
The object is a hybrid body.
The hybrid body manages a set of geometric elements, a set of hybrid shapes,
a set of bodies and a set of hybrid bodies.
It belongs to the  collection of a
or @ref CATIABody  or
object.
Property Index
Bodies
Returns the hybrid body's Bodies collection.
GeometricElements
Returns the list of geometrical elements included in the hybrid body.
HybridBodies
Returns the hybrid body's HybridBodies collection.
HybridShapes
Returns the list of hybrid shapes included in the hybrid body.
HybridSketches
Returns the hybrid body's Sketches collection.
Method Index
AppendHybridShape
Appends a hybrid shape to the hybrid body.
Properties
Property Bodies() As   (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
Property GeometricElements() As   (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
Property HybridBodies() As   (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
Property HybridShapes() As   (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
Property HybridSketches() As   (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
Methods
Sub AppendHybridShape( 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)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_HybridShape_21664 ===
MecModInterfaces HybridShape (Object)
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HybridShape (Object)
Represents the hybrid shape object.
Property Index
Thickness
Returns the thickness of the hybrid shape.
Method Index
AppendHybridShape
Appends a hybrid shape to another hybrid shape.
Compute
Computes the result of the hybrid shape.
Properties
Property Thickness() As   (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
Methods
Sub AppendHybridShape( 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)
Sub Compute()
Computes the result of the hybrid shape.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_HybridShapeInstance_33622 ===
MecModInterfaces HybridShapeInstance (Object)
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HybridShapeInstance (Object)
The interface to access a CATIAHybridShapeInstance.
Property Index
InputsCount
Returns the number of Inputs.
OutputsCount
Returns the number of Outputs.
ParametersCount
Returns the number of Parameters.
Method Index
GetInput
Gets an input of a hybrid shape instance by its name.
GetInputData
Gets an input of a shape instance by its name.
GetInputDataFromPosition
Gets an input of a hybrid shape instance from its position.
GetInputFromPosition
Gets an input of a hybrid shape instance from its position.
GetOutput
Gets a Ouput by its name.
GetOutputFromPosition
Gets a Ouput from its position.
GetParameter
Gets a parameter of a hybrid shape instance by its name.
GetParameterFromPosition
Gets a parameter of a hybrid shape instance from its position.
PutInput
Defines an input of a hybrid shape instance.
PutInputData
Defines an input of a shape instance.
Properties
Property InputsCount() As   (Read Only)
Returns the number of Inputs.
Example:
The following example retrieves in inputsCount
the number of Inputs of hybridShapeInstance:
inputsCount = hybridShapeInstance.InputsCount
Property OutputsCount() As   (Read Only)
Returns the number of Outputs.
Example:
The following example retrieves in outputsCount
the number of Outputs of hybridShapeInstance:
outputsCount = hybridShapeInstance.OutputsCount
Property ParametersCount() As   (Read Only)
Returns the number of Parameters.
Example:
The following example retrieves in parametersCount
the number of parameters of hybridShapeInstance:
parametersCount = hybridShapeInstance.ParametersCount
Methods
Func GetInput( iIndex) As
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
Func GetInputData( iName) As
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
Func GetInputDataFromPosition( iPosition) As
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
Func GetInputFromPosition( iPosition) As
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
Func GetOutput( iName) As
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
Func GetOutputFromPosition( iPosition) As
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
Func GetParameter( iName) As
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
Func GetParameterFromPosition( iPosition) As
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
Sub PutInput( iIndex, 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
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
Sub PutInputData( iName, 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
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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_HybridShapes_22929 ===
MecModInterfaces HybridShapes (Object)
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HybridShapes (Object)
The collection of the HybridShapes making up a body.
Method Index
GetBoundary
Returns a boundary using its label.
Item
Returns a HybridShape using its index or its name from the HybridShapes collection.
Methods
Func GetBoundary( iLabel) As
Returns a boundary using its label.
Parameters:
iLabel
Identification of the
object.   See
.
Returns:
The retrieved boundary
Func Item( iIndex) As
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
.   As a string, it is the name you assigned to the HybridShape using
the
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")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_InstanceFactory_27199 ===
MecModInterfaces InstanceFactory (Object)
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Class Hierarchy
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InstanceFactory (Object)
Represents the CATIAInstanceFactory.
Role:
This interface is used to create a new instance of a shape reference ( ) or a hybrid shape reference (
) in case of the instantiation of a User Feature.
It is also used to instantiate a Power Copy reference.
This interface contains two protocols of instantiation:
The first protocol is dedicated to User Feature instantiation only.
It is defined by a single method:
. It creates a shape or hybrid shape instance depending on the result of the User Feature.
Use this method when you want to perform only one instantiation of the reference.
Read the document containing the User Feature reference and instantiate it.
As the document containing the reference is released from the session at the end of the instantiation,
it is not recommmended to use this method if you want to perform several instantiations of the same reference in a loop.
In that case, prefer the second protocol of instantiation.
The second protocol is dedicated to both User Feature and Power Copy instantiations.
It is defined by several methods that must be called in order.
For User Feature instantiation, these methods are an alternative way of the
method.
It is recommended to use the second protocol to perform several instantiations of the same reference in a loop.
For Power Copy instantiation, it is the only way of instantiating a reference.
The instantiation process is composed of three major steps:
The first step
consists in initializing the
with the reference and the document where it is stored.
This step must be called once at the beginning whatever the number of instantiations are done.
Optional step
allow the user to specify the mode of the instantiation, that is to say "After" or "Inside".
If this method is not called, the instantiation mode will be chosen according to the BeginInstantiate method.
The second step is the instantiation itself: it is composed of five methods that must be called in the order.
This set of five methods can be called in a loop in order to make several instantiations.
The method
is used to initialize all data of the reference.
The method
is used to set a value to any input of the reference.
The method
is used to retrieve any parameter of the reference in order to modify its value.
The method
is used to duplicate the reference. It returns the created instance when it does exist.
The method
is used to indicate that the instantiation is done.
The third step
consists in ending the instantiation and cleaning the
.
When doing several instantiations in a loop, this step must be called just once at the end of all instantiations.
Property Index
InstantiationMode
Sets the mode of instantiation to "Inside" or "After".
Method Index
AddInstance
Creates a new instance of a shape or hybrid shape.
BeginInstanceFactory
Initializes the instantiation process with the document containing the reference.
BeginInstantiate
Initializes the data of the reference.
EndInstanceFactory
Ends the instantiation process.
EndInstantiate
Ends the instantiation of the reference.
GetParameter
Retrieves a parameter of the reference by its name.
Instantiate
Instantiates the reference in the current document.
PutInputData
Sets a value to an input of the reference.
Properties
Property InstantiationMode( 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
Methods
Func AddInstance( iReference) As
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)
Sub BeginInstanceFactory( iNameOfReference, 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
.
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:\tmp\NameOfDocument.CATPart"
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
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
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
Func GetParameter( iName) As
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")
Func Instantiate() As
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
Sub PutInputData( iName, 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
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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_MonoDimFeatEdge_26223 ===
MecModInterfaces MonoDimFeatEdge (Object)
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MonoDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is one dimensional.
Role:
This  object may be, for example, in a part containing a Sketch which is made up of a circle arc and a spline, the circle arc.
You will create a MonoDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a MonoDimFeatEdge object is limited, see
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_NotWireBoundaryMonoDimFeatVertex_67048 ===
MecModInterfaces NotWireBoundaryMonoDimFeatVertex (Object)
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NotWireBoundaryMonoDimFeatVertex (Object)
0-D boundary belonging to a feature whose topological result is one dimensional, the boundary not beeing the extremity of the feature.
Role:
This  object may be, for example, in a part containing a Sketch which is made up of a circle arc and a spline, the vertex between the circle arc and the spline.
You will create a NotWireBoundaryMonoDimFeatVertex object using the
,
,
or
method. Then, you pass it to the operator.
The lifetime of a NotWireBoundaryMonoDimFeatVertex object is limited, see
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_OrderedGeometricalSet_37698 ===
MecModInterfaces OrderedGeometricalSet (Object)
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OrderedGeometricalSet (Object)
The object is an ordered geometrical set.
The ordered geometrical set manages a set of hybrid shapes,
a set of bodies and a set of ordered geometrical sets.
It belongs to the  collection of a
or
object.
Property Index
Bodies
Returns the ordered geometrical set's Bodies collection.
HybridShapes
Returns the list of hybrid shapes included in the ordered geometrical set.
OrderedGeometricalSets
Returns the ordered geometrical set's OrderedGeometricalSets collection.
OrderedSketches
Returns the ordered geometrical set's Sketches collection.
Method Index
InsertHybridShape
Inserts a hybrid shape to the ordered geometrical set.
Properties
Property Bodies() As   (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
Property HybridShapes() As   (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
Property OrderedGeometricalSets() As   (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
Property OrderedSketches() As   (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
Methods
Sub InsertHybridShape( 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)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_OrderedGeometricalSets_40113 ===
MecModInterfaces OrderedGeometricalSets (Object)
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OrderedGeometricalSets (Object)
A collection of the OrderedGeometricalSet objects.
Method Index
Add
Creates a new ordered geometrical set and adds it to the OrderedGeometricalSets collection.
Item
Returns a ordered geometrical set using its index or its name from the ordered geometrical set
collection.
Methods
Func Add() As
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()
Func Item( iIndex) As
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
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")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_OriginElements_25734 ===
MecModInterfaces OriginElements (Object)
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OriginElements (Object)
Represents the part's 3D reference axis system.
It allows an easy access to 3D reference axis system of a
Part object thru the three planes XY, YZ, and ZX.
See  for parent object.
Property Index
PlaneXY
Returns the XY plane of the part 3D reference axis system.
PlaneYZ
Returns the YZ plane of the part 3D reference axis system.
PlaneZX
Returns the ZX plane of the part 3D reference axis system.
Properties
Property PlaneXY() As   (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
Property PlaneYZ() As   (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
Property PlaneZX() As   (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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Part_16738 ===
MecModInterfaces Part (Object)
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Part (Object)
The root level object inside a PartDocument object.
Role: It aggregates all the objects making up the part document.
It provides many factories and collections. The collections list only the direct children of the part.
allows to get all objects of one type.
See also:
Property Index
AnnotationSets
Returns the collection object containing the annotation sets.
AxisSystems
Returns the collection object containing the coordinate systems.
Bodies
Returns the collection object containing the bodies that are direct children of the part.
Constraints
Returns the collection object containing the part constraints.
Density
Returns the part density.
GeometricElements
Returns the collection object containing the part geometrical elements.
HybridBodies
Returns the collection object containing the hybrid bodies that are direct children of the part.
HybridShapeFactory
Returns the part hybrid shape factory.
InWorkObject
Returns or sets the in work object of the part.
MainBody
Returns or sets the main body of the part.
OrderedGeometricalSets
Returns the collection object containing the ordered geometrical sets of the part.
OriginElements
Returns the object defining the part 3D reference axis system.
Parameters
Returns the collection object containing the part parameters.
Relations
Returns the collection object containing the part relations.
ShapeFactory
Returns the part shape factory.
SheetMetalFactory
Returns the sheet metal factory of the part.
SheetMetalParameters
Returns the sheet metal parameters of the part.
UserSurfaces
Returns the collection object containing the user surfaces.
Method Index
Activate
Unsuppresses an object for the update process.
CreateReferenceFromBRepName
Creates a reference from a GenericNaming label.
CreateReferenceFromName
Creates a reference from a GenericNaming label.
CreateReferenceFromObject
Creates a reference from a operator.
FindObjectByName
Finds an object that is not a collection by its name.
GetCustomerFactory
Returns a customer factory from a code string defined by the customer.
Inactivate
Suppresses an object from being updated.
IsInactive
Indicates whether an object is deactivated.
IsUpToDate
Indicates whether an object needs to be updated.
Update
Updates of the part result with respect to its specifications.
UpdateObject
Updates an object with respect to its specifications.
Properties
Property AnnotationSets() As   (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
Property AxisSystems() As   (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
Property Bodies() As   (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
Property Constraints() As   (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
Property Density() As   (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
Property GeometricElements() As   (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
Property HybridBodies() As   (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
Property HybridShapeFactory() As   (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
Property InWorkObject() As
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
Property MainBody() As
Returns or sets the main body of the part.
Example:
The following example returns the main body
of the part of the current document.
Dim mainBody As Body
Set mainBody=CATIA.ActiveDocument.Part.MainBody
Property OrderedGeometricalSets() As   (Read Only)
Returns the collection object containing the ordered geometrical sets of the part.
Example:
The following example returns in ogsColl the collection
of ordered geometrical sets of the partRoot part from the
partDoc part document:
Set partRoot = partDoc.Part
Set ogsColl = partRoot.OrderedGeometricalSets
Property OriginElements() As   (Read Only)
Returns the object defining the part 3D reference axis system.
Example:
The following example returns in originElts the origin
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Set originElts = partRoot.OriginElements
Property Parameters() As   (Read Only)
Returns the collection object containing the part parameters.
All the parameters that are aggregated in the different
objects of the part might be accessed thru that collection.
Example:
The following example returns in params the parameters
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Dim params As Parameters
Set params = partRoot.Parameters
Property Relations() As   (Read Only)
Returns the collection object containing the part relations.
All the relations that are used to valuate
the parameters of the part might be accessed thru that collection.
Example:
The following example returns in rels the relations
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Set rels = partRoot.Relations
Property ShapeFactory() As   (Read Only)
Returns the part shape factory.
It allows the creation of shapes in the part.
Example:
The following example returns in shapeFact the shape factory
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Dim shapeFact As Factory
Set shapeFact = partRoot.ShapeFactory
Property SheetMetalFactory() As   (Read Only)
Returns the sheet metal factory of the part.
It allows the creation of sheet metal elements in the part.
Example:
The following example returns in sheetMetalFact the sheet metal factory
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Dim sheetMetalFact As Factory
Set sheetMetalFact = partRoot.SheetMetalFactory
Property SheetMetalParameters() As   (Read Only)
Returns the sheet metal parameters of the part.
Example:
The following example returns in sheetMetalParm the sheet metal parameters
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Dim sheetMetalParm As SheetMetalParameters
Set sheetMetalFact = partRoot.SheetMetalParameters
Property UserSurfaces() As   (Read Only)
Returns the collection object containing the user surfaces.
All the user surfaces that are aggregated in the part
might be accessed thru that collection.
Example:
The following example returns in userSurfaces the user surfaces
of the partRoot part from the partDoc part document:
Set partRoot = partDoc.Part
Dim userSurfaces As UserSurfaces
Set userSurfaces = partRoot.UserSurfaces
Methods
Sub Activate( 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)
Func CreateReferenceFromBRepName( iLabel, iObjectContext) As
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
Func CreateReferenceFromName( iLabel) As
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
Func CreateReferenceFromObject( iObject) As
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.
Func FindObjectByName( iObjName) As
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
Func GetCustomerFactory( iFactoryIID) As
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
Sub Inactivate( 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)
Func IsInactive( iObject) As
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)
Func IsUpToDate( iObject) As
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)
Sub Update()
Updates of the part result with respect to its specifications.
Any composing specification that hasn't its result up-to-date will
recompute it, thus propagating changes to the whole part.
Example:
The following example update the part:
Set partRoot = partDoc.Part
partRoot.Update
Sub UpdateObject( iObject)
Updates an object with respect to its specifications.
Any composing specification of the object that hasn't
its result up-to-date will recompute it,
thus propagating changes to the object.
Parameters:
iObject
The object to be updated
Example:
The following example updates Pad.1:
Set partRoot = partDoc.Part
Set pad1 = partRoot.FindObjectByName("Pad.1")
partRoot.UpdateObject(pad1)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_PartDocument_23135 ===
MecModInterfaces PartDocument (Object)
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PartDocument (Object)
Represents the Document object for parts.
Role:
When a PartDocument object is created, a Part object is also created.
This Part object is the root object  of the Part structure.
A reference Product object is also created in each PartDocument. It is used to access Publications,
PartNumber.
See also:
,
Property Index
Part
Returns the root Part object from the current part document.
Product
Returns the root Product object from the current part document.
Properties
Property Part() As   (Read Only)
Returns the root Part object from the current part document.
Example:
The following example retrieves in RootPart the root Part
object of the active document, assumed to be a part document:
Set RootPart = CATIA.ActiveDocument.Part
Property Product() As   (Read Only)
Returns the root Product object from the current part document.
Example:
The following example retrieves in RootProd the root Product
object of the active document, assumed to be a part document:
Set RootProd = CATIA.ActiveDocument.Part
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_PartInfrastructureSettingAtt_56080 ===
MecModInterfaces PartInfrastructureSettingAtt (Object)
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PartInfrastructureSettingAtt (Object)
Setting controller for all the Part Infrastructure property tab pages.
Role: This interface is implemented by a component representing
the controller for the Part Infrastructure settings.
Property Index
AlsoDeleteExclusiveParents
Returns or sets the "AlsoDeleteExclusiveParents" parameter.
AxisSystemSize
Returns or sets the "AxisSystemSize" parameter.
BodiesUnderOperationsInTree
Returns or sets the "BodiesUnderOperationsInTree" parameter.
ColorSynchronizationEditability
Returns or sets the "ColorSynchronizationEditability" parameter.
ColorSynchronizationMode
Returns or sets the "ColorSynchronizationMode" parameter.
ColorSynchronizationModeManage
Returns or sets the "ColorSynchronizationModeManage" parameter.
ColorSynchronizationModeOnFeature
Returns or sets the "ColorSynchronizationModeOnFeature" parameter.
ColorSynchronizationModeOnSubElements
Returns or sets the "ColorSynchronizationModeOnSubElements" parameter.
Colors3DExperienceManagement
Returns or sets the "Colors3DExperienceManagement" parameter.
ConstraintsInGeometry
Returns or sets the "ConstraintsInGeometry" parameter.
ConstraintsNodeInTree
Returns or sets the "ConstraintsNodeInTree" parameter.
ContextualFeaturesSelectableAtCreation
Returns or sets the "ContextualFeaturesSelectableAtCreation" parameter.
DefaultColorsEditability
Returns or sets the "DefaultColorsEditability" parameter.
DeleteWarningBox
Returns or sets the "DeleteWarningBox" parameter.
DisplayGeometryAfterCurrent
Returns or sets the "DisplayGeometryAfterCurrent" parameter.
ExpandSketchBasedFeaturesNodeAtCreation
Returns or sets the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
ExternalReferencesAsVisible
Returns or sets the "ExternalReferencesAsVisible" parameter.
ExternalReferencesAssemblyRootContext
Returns or sets the "ExternalReferencesAssemblyRootContext" parameter.
ExternalReferencesNodeInTree
Returns or sets the "ExternalReferencesNodeInTree" parameter.
HybridDesignMode
Returns or sets the "HybridDesignMode" parameter.
KnowledgeInHybridDesignMode
Returns or sets the "KnowledgeInHybridDesignMode" parameter.
LinkedExternalReferences
Returns or sets the "LinkedExternalReferences" parameter.
LinkedExternalReferencesOnlyOnPublication
Returns or sets the "LinkedExternalReferencesOnlyOnPublication" parameter.
LinkedExternalReferencesWarningAtCreation
Returns or sets the "LinkedExternalReferencesWarningAtCreation" parameter.
NamingMode
Returns or sets the "NamingMode" parameter.
NewWith3DSupport
Returns or sets the "NewWith3DSupport" parameter.
NewWithAxisSystem
Returns or sets the "NewWithAxisSystem" parameter.
NewWithGS
Returns or sets the "NewWithGS" parameter.
NewWithOGS
Returns or sets the "NewWithOGS" parameter.
NewWithPanel
Returns or sets the "NewWithPanel" parameter.
OnlyCurrentOperatedSolidSetInGeometry
Returns or sets the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
OnlyCurrentSolidSetInGeometry
Returns or sets the "OnlyCurrentSolidSetInGeometry" parameter.
ParametersNodeInTree
Returns or sets the "ParametersNodeInTree" parameter.
PublishTopologicalElements
Returns or sets the "PublishTopologicalElements" parameter.
RelationsNodeInTree
Returns or sets the "RelationsNodeInTree" parameter.
ReplaceOnlyAfterCurrent
Returns or sets the "ReplaceOnlyAfterCurrent" parameter.
SurfaceElementsLocation
Returns or sets the "SurfaceElementsLocation" parameter.
TrueColorMode
Returns or sets the "ColorInheritanceMode" parameter.
UpdateElementsRefreshed
Returns or sets the "UpdateElementsRefreshed" parameter.
UpdateLinkedExternalReferences
Returns or sets the "UpdateLinkedExternalReferences" parameter.
UpdateMode
Returns or sets the "UpdateMode" parameter.
UpdateStoppedOnError
Returns or sets the "UpdateStoppedOnError" parameter.
Method Index
GetAlsoDeleteExclusiveParentsInfo
Retrieves environment informations for the "AlsoDeleteExclusiveParents" parameter.
GetAxisSystemSizeInfo
Retrieves environment informations for the "AxisSystemSize" parameter.
GetBodiesUnderOperationsInTreeInfo
Retrieves environment informations for the "BodiesUnderOperationsInTree" parameter.
GetColorSynchronizationEditabilityInfo
Retrieves environment informations for the "ColorSynchronizationEditability" parameter.
GetColorSynchronizationModeInfo
Retrieves environment informations for the "ColorSynchronizationMode" parameter.
GetColorSynchronizationModeManageInfo
Retrieves environment informations for the "ColorSynchronizationModeManage" parameter.
GetColorSynchronizationModeOnFeatureInfo
Retrieves environment informations for the "ColorSynchronizationModeOnFeature" parameter.
GetColorSynchronizationModeOnSubElementsInfo
Retrieves environment informations for the "ColorSynchronizationModeOnSubElements" parameter.
GetColors3DExperienceManagementInfo
Retrieves environment informations for the "Colors3DExperienceManagement" parameter.
GetConstraintsInGeometryInfo
Retrieves environment informations for the "ConstraintsInGeometry" parameter.
GetConstraintsNodeInTreeInfo
Retrieves environment informations for the "ConstraintsNodeInTree" parameter.
GetContextualFeaturesSelectableAtCreationInfo
Retrieves environment informations for the "ContextualFeaturesSelectableAtCreation" parameter.
GetDefaultColorsEditabilityInfo
Retrieves environment informations for the "DefaultColorsEditability" parameter.
GetDeleteWarningBoxInfo
Retrieves environment informations for the "DeleteWarningBox" parameter.
GetDisplayGeometryAfterCurrentInfo
Retrieves environment informations for the "DisplayGeometryAfterCurrent" parameter.
GetExpandSketchBasedFeaturesNodeAtCreationInfo
Retrieves environment informations for the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
GetExternalReferencesAsVisibleInfo
Retrieves environment informations for the "ExternalReferencesAsVisible" parameter.
GetExternalReferencesAssemblyRootContextInfo
Retrieves environment informations for the "ExternalReferencesAssemblyRootContext" parameter.
GetExternalReferencesNodeInTreeInfo
Retrieves environment informations for the "ExternalReferencesNodeInTree" parameter.
GetHybridDesignModeInfo
Retrieves environment informations for the "HybridDesignMode" parameter.
GetKnowledgeInHybridDesignModeInfo
Retrieves environment informations for the "KnowledgeInHybridDesignMode" parameter.
GetLinkedExternalReferencesInfo
Retrieves environment informations for the "LinkedExternalReferences" parameter.
GetLinkedExternalReferencesOnlyOnPublicationInfo
Retrieves environment informations for the "LinkedExternalReferencesOnlyOnPublication" parameter.
GetLinkedExternalReferencesWarningAtCreationInfo
Retrieves environment informations for the "LinkedExternalReferencesWarningAtCreation" parameter.
GetNamingModeInfo
Retrieves environment informations for the "NamingMode" parameter.
GetNewWith3DSupportInfo
Retrieves environment informations for the "NewWith3DSupport" parameter.
GetNewWithAxisSystemInfo
Retrieves environment informations for the "NewWithAxisSystem" parameter.
GetNewWithGSInfo
Retrieves environment informations for the "NewWithGS" parameter.
GetNewWithOGSInfo
Retrieves environment informations for the "NewWithOGS" parameter.
GetNewWithPanelInfo
Retrieves environment informations for the "NewWithPanel" parameter.
GetOnlyCurrentOperatedSolidSetInGeometryInfo
Retrieves environment informations for the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
GetOnlyCurrentSolidSetInGeometryInfo
Retrieves environment informations for the "OnlyCurrentSolidSetInGeometry" parameter.
GetParametersNodeInTreeInfo
Retrieves environment informations for the "ParametersNodeInTree" parameter.
GetPublishTopologicalElementsInfo
Retrieves environment informations for the "PublishTopologicalElements" parameter.
GetRelationsNodeInTreeInfo
Retrieves environment informations for the "RelationsNodeInTree" parameter.
GetReplaceOnlyAfterCurrentInfo
Retrieves environment informations for the "ReplaceOnlyAfterCurrent" parameter.
GetSurfaceElementsLocationInfo
Retrieves environment informations for the "SurfaceElementsLocation" parameter.
GetTrueColorModeInfo
Retrieves environment informations for the "ColorInheritanceMode" parameter.
GetUpdateElementsRefreshedInfo
Retrieves environment informations for the "UpdateElementsRefreshed" parameter.
GetUpdateLinkedExternalReferencesInfo
Retrieves environment informations for the "UpdateLinkedExternalReferences" parameter.
GetUpdateModeInfo
Retrieves environment informations for the "UpdateMode" parameter.
GetUpdateStoppedOnErrorInfo
Retrieves environment informations for the "UpdateStoppedOnError" parameter.
SetAlsoDeleteExclusiveParentsLock
Locks or unlocks the "AlsoDeleteExclusiveParents" parameter.
SetAxisSystemSizeLock
Locks or unlocks the "AxisSystemSize" parameter.
SetBodiesUnderOperationsInTreeLock
Locks or unlocks the "BodiesUnderOperationsInTree" parameter.
SetColorSynchronizationEditabilityLock
Locks or unlocks the "ColorSynchronizationEditability" parameter.
SetColorSynchronizationModeLock
Locks or unlocks the "ColorSynchronizationMode" parameter.
SetColorSynchronizationModeManageLock
Locks or unlocks the "ColorSynchronizationModeManage" parameter.
SetColorSynchronizationModeOnFeatureLock
Locks or unlocks the "ColorSynchronizationModeOnFeature" parameter.
SetColorSynchronizationModeOnSubElementsLock
Locks or unlocks the "ColorSynchronizationModeOnSubElements" parameter.
SetColors3DExperienceManagementLock
Locks or unlocks the "Colors3DExperienceManagement" parameter.
SetConstraintsInGeometryLock
Locks or unlocks the "ConstraintsInGeometry" parameter.
SetConstraintsNodeInTreeLock
Locks or unlocks the "ConstraintsNodeInTree" parameter.
SetContextualFeaturesSelectableAtCreationLock
Locks or unlocks the "ContextualFeaturesSelectableAtCreation" parameter.
SetDefaultColorsEditabilityLock
Locks or unlocks the "DefaultColorsEditability" parameter.
SetDeleteWarningBoxLock
Locks or unlocks the "DeleteWarningBox" parameter.
SetDisplayGeometryAfterCurrentLock
Locks or unlocks the "DisplayGeometryAfterCurrent" parameter.
SetExpandSketchBasedFeaturesNodeAtCreationLock
Locks or unlocks the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
SetExternalReferencesAsVisibleLock
Locks or unlocks the "ExternalReferencesAsVisible" parameter.
SetExternalReferencesAssemblyRootContextLock
Locks or unlocks the "ExternalReferencesAssemblyRootContext" parameter.
SetExternalReferencesNodeInTreeLock
Locks or unlocks the "ExternalReferencesNodeInTree" parameter.
SetHybridDesignModeLock
Locks or unlocks the "HybridDesignMode" parameter.
SetKnowledgeInHybridDesignModeLock
Locks or unlocks the "KnowledgeInHybridDesignMode" parameter.
SetLinkedExternalReferencesLock
Locks or unlocks the "LinkedExternalReferences" parameter.
SetLinkedExternalReferencesOnlyOnPublicationLock
Locks or unlocks the "LinkedExternalReferencesOnlyOnPublication" parameter.
SetLinkedExternalReferencesWarningAtCreationLock
Locks or unlocks the "LinkedExternalReferencesWarningAtCreation" parameter.
SetNamingModeLock
Locks or unlocks the "NamingMode" parameter.
SetNewWith3DSupportLock
Locks or unlocks the "NewWith3DSupport" parameter.
SetNewWithAxisSystemLock
Locks or unlocks the "NewWithAxisSystem" parameter.
SetNewWithGSLock
Locks or unlocks the "NewWithGS" parameter.
SetNewWithOGSLock
Locks or unlocks the "NewWithOGS" parameter.
SetNewWithPanelLock
Locks or unlocks the "NewWithPanel" parameter.
SetOnlyCurrentOperatedSolidSetInGeometryLock
Locks or unlocks the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
SetOnlyCurrentSolidSetInGeometryLock
Locks or unlocks the "OnlyCurrentSolidSetInGeometry" parameter.
SetParametersNodeInTreeLock
Locks or unlocks the "ParametersNodeInTree" parameter.
SetPublishTopologicalElementsLock
Locks or unlocks the "PublishTopologicalElements" parameter.
SetRelationsNodeInTreeLock
Locks or unlocks the "RelationsNodeInTree" parameter.
SetReplaceOnlyAfterCurrentLock
Locks or unlocks the "ReplaceOnlyAfterCurrent" parameter.
SetSurfaceElementsLocationLock
Locks or unlocks the "SurfaceElementsLocation" parameter.
SetUpdateElementsRefreshedLock
Locks or unlocks the "UpdateElementsRefreshed" parameter.
SetUpdateLinkedExternalReferencesLock
Locks or unlocks the "UpdateLinkedExternalReferences" parameter.
SetUpdateModeLock
Locks or unlocks the "UpdateMode" parameter.
SetUpdateStoppedOnErrorLock
Locks or unlocks the "UpdateStoppedOnError" parameter.
Properties
Property AlsoDeleteExclusiveParents() As
Returns or sets the "AlsoDeleteExclusiveParents" parameter.
Role: This parameter defines if a exclusive parents of an object will also be deleted when the object is deleted.
This option is effective only when the "Deletion warning box" is displayed.
Parameters:
oDeleted
Current "AlsoDeleteExclusiveParents" parameter's value:
TRUE or 1 if exclusive parents are also deleted,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property AxisSystemSize() As
Returns or sets the "AxisSystemSize" parameter.
Role: This parameter determines the size of axis systems.
Parameters:
oSize
Current size of axis systems
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property BodiesUnderOperationsInTree() As
Returns or sets the "BodiesUnderOperationsInTree" parameter.
Role: This parameter determines if a Body node is displayed when it is being aggregated under a boolean operation (Add, Assemble, Remove, Intersect, Union Trim).
Its value can be changed even after a boolean operation has been created. Simply collapse and expand the federating boolean operation node for the specification tree to be refreshed.
Parameters:
oNodeDisplayed
Current "BodiesUnderOperationsInTree" parameter's value:
TRUE or 1 if such a node is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ColorSynchronizationEditability() As
Returns or sets the "ColorSynchronizationEditability" parameter.
Role: This parameter determines whether color synchronization property on Part is editable or not.
Color synchronization editability defines whether the property of synchronization on Part can be interactively editable
If it is valuated to 1, user will be able to interactively modify the Part property of Color management tab for synchronization.
If it is defined to 0, user will not be able to interactively modify the Part property of Color management tab for synchronization.
This option cannot be changed after a document has been opened.
Parameters:
oActivated
Current "ColorSynchronizationEditability" parameter's value:
TRUE or 1, Part property option for synchronization is editable
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ColorSynchronizationMode() As
Returns or sets the "ColorSynchronizationMode" parameter.
Role: This parameter determines color synchronization mode for imported features in a part.
Color synchronization mode defines whether the imported feature, created through copy/paste as result with link mechanism, copies reference
feature colors on its faces or not. If it is valuated to 1, synchronization will be effective and referece feature colors will be reported.
If it is defined to 0, nothing will be copied(default mode).
This option cannot be changed after a document has been opened.
Parameters:
oActivated
Current "ColorSynchronizationMode" parameter's value:
TRUE or 1 if reference feature colors are reported on imported feature,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ColorSynchronizationModeManage() As
Returns or sets the "ColorSynchronizationModeManage" parameter.
Role: This parameter determines access to specific color synchronization mode for imported features in a part.
Color synchronization mode Manage defines if access is granted to color synchronization suboptions "on feature" and "on subelements". If it is valuated to 1, access will be granted.
If it is defined to 0, no acces to color on feature & color on subelements options
Parameters:
oActivated
Current "ColorSynchronizationModeManage" parameter's value:
TRUE or 1 if possibility to chose specific color copy parameters
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ColorSynchronizationModeOnFeature() As
Returns or sets the "ColorSynchronizationModeOnFeature" parameter.
Role: This parameter determines graphic properties synchronization mode on feature for imported features in a part.
Color synchronization mode defines whether the imported feature, created through copy/paste as result with link mechanism, copies reference
feature graphic properties or not. If it is valuated to 1, synchronization will be effective and referece feature graphic properties will be reported.
If it is defined to 0, nothing will be copied(default mode).
Parameters:
oActivated
Current "ColorSynchronizationModeOnFeature" parameter's value:
TRUE or 1 if reference feature graphic properties are reported on imported feature,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ColorSynchronizationModeOnSubElements() As
Returns or sets the "ColorSynchronizationModeOnSubElements" parameter.
Role: This parameter determines color synchronization mode for imported features in a part.
Color synchronization mode OnSubElements defines whether the imported feature, created through copy/paste as result with link mechanism, copies reference
feature colors on his overloaded faces or not. If it is valuated to 1, synchronization will be effective and reference subelements colors will be reported.
If it is defined to 0, nothing will be copied(default mode).
Parameters:
oActivated
Current "ColorSynchronizationModeOnSubElements" parameter's value:
TRUE or 1 if reference subelements colors are reported on imported feature,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property Colors3DExperienceManagement() As
Returns or sets the "Colors3DExperienceManagement" parameter.
Role: This parameter determines whether color synchronization property on Part is editable or not.
Color synchronization editability defines whether the property of synchronization on Part can be interactively editable
If it is valuated to 1, user will be able to interactively modify the Part property of Color management tab for synchronization.
If it is defined to 0, user will not be able to interactively modify the Part property of Color management tab for synchronization.
This option cannot be changed after a document has been opened.
Parameters:
oActivated
Current "Colors3DExperienceManagement" parameter's value:
TRUE or 1, Part property option for synchronization is editable
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ConstraintsInGeometry() As
Returns or sets the "ConstraintsInGeometry" parameter.
Role: This parameter enables constraints to be visualized in the 3D view.
Parameters:
oDisplayed
Current "Display constraints within 3D" parameter's value:
TRUE or 1 if constraints are displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ConstraintsNodeInTree() As
Returns or sets the "ConstraintsNodeInTree" parameter.
Role: This parameter determines if a node called "Constraints" is created to contain all constraints.
Its value can be changed even after constraints have been created. The result is that the specification tree node display status will be affected.
Parameters:
oNodeDisplayed
Current "ConstraintsNodeInTree" parameter's value:
TRUE or 1 if such a node is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ContextualFeaturesSelectableAtCreation() As
Returns or sets the "ContextualFeaturesSelectableAtCreation" parameter.
Role: This parameter determines if contextual features can be selected during the creation of an other feature.
Parameters:
oContextualFeaturesSelectable
Current "ContextualFeaturesSelectableAtCreation" parameter's value:
TRUE or 1 if contextual features can be selected,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property DefaultColorsEditability() As
Returns or sets the "DefaultColorsEditability" parameter.
Role: This parameter determines whether color synchronization property on Part is editable or not.
Color synchronization editability defines whether the property of synchronization on Part can be interactively editable
If it is valuated to 1, user will be able to interactively modify the Part property of Color management tab for synchronization.
If it is defined to 0, user will not be able to interactively modify the Part property of Color management tab for synchronization.
This option cannot be changed after a document has been opened.
Parameters:
oActivated
Current "DefaultColorsEditability" parameter's value:
TRUE or 1, Part property option for synchronization is editable
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property DeleteWarningBox() As
Returns or sets the "DeleteWarningBox" parameter.
Role: This parameter defines if a warning box is displayed when an element is deleted.
Parameters:
oDisplayed
Current "DeleteWarningBox" parameter's value:
TRUE or 1 if a warning box is displayed at deletion,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property DisplayGeometryAfterCurrent() As
Returns or sets the "DisplayGeometryAfterCurrent" parameter.
Role: This parameter enables to visualize in the 3D features after the current object in O.G.S. and "solid and surface set".
Parameters:
oDisplayed
Current "DisplayGeometryAfterCurrent" parameter's value:
TRUE or 1 if such is the visualization,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ExpandSketchBasedFeaturesNodeAtCreation() As
Returns or sets the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
Role: This parameter determines if specification tree nodes for sketch-based features are expanded when such elements are created. This will enable to view their sketch node.
Parameters:
oNodeExpanded
Current "ExpandSketchBasedFeaturesNodeAtCreation" parameter's value:
TRUE or 1 if such nodes are expanded,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ExternalReferencesAsVisible() As
Returns or sets the "ExternalReferencesAsVisible" parameter.
Role: This parameter defines if an external reference is visible when being created.
Parameters:
oVisible
Current "ExternalReferencesAsVisible" parameter's value:
TRUE or 1 if external references are visible when being created,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ExternalReferencesAssemblyRootContext() As
Returns or sets the "ExternalReferencesAssemblyRootContext" parameter.
Role: This parameter defines if external references are created using the root context of an assembly.
Parameters:
oRootContextUsed
Current "ExternalReferencesAssemblyRootContext" parameter's value:
TRUE or 1 if external references are created using the root context of an assembly,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ExternalReferencesNodeInTree() As
Returns or sets the "ExternalReferencesNodeInTree" parameter.
Role: This parameter determines if a node called "External Reference" is created to contain all linked external references.
Its value can be changed even after linked external references have been created. The result is that the specification tree node display status will be affected.
Parameters:
oNodeDisplayed
Current "ExternalReferencesNodeInTree" parameter's value:
TRUE or 1 if such a node is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property HybridDesignMode() As
Returns or sets the "HybridDesignMode" parameter.
Role: This parameter determines if hybrid design is possible inside Part Bodies and bodies.
This option can be changed even after a document has been opened.
Parameters:
oHybridDesign
Current "HybridDesignMode" parameter's value:
TRUE or 1 if hybrid design is enabled,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property KnowledgeInHybridDesignMode() As
Returns or sets the "KnowledgeInHybridDesignMode" parameter.
Role: This parameter determines if knowledge features (formulas, parameters, rules, ...)
can be located inside ordered sets.
This option can be changed even after a document has been opened.
Parameters:
oKnowledgeInHybridDesign
Current "KnowledgeInHybridDesignMode" parameter's value:
TRUE or 1 if hybrid design is enabled,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property LinkedExternalReferences() As
Returns or sets the "LinkedExternalReferences" parameter.
Role: This parameter enables creation of external references with links.
Parameters:
oWithLink
"LinkedExternalReferences" parameter's value:
TRUE or 1 if external references are created with links,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property LinkedExternalReferencesOnlyOnPublication() As
Returns or sets the "LinkedExternalReferencesOnlyOnPublication" parameter.
Role: This parameter restricts the creation of external references with links to only published elements.
This option is only used when external references are created with link.
Parameters:
oOnlyForPublishedElements
Current "LinkedExternalReferencesOnlyOnPublication" parameter's value:
TRUE or 1 if external references with link are only allowed on published elements,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property LinkedExternalReferencesWarningAtCreation() As
Returns or sets the "LinkedExternalReferencesWarningAtCreation" parameter.
Role: This parameter defines if a warning panel is displayed each time an external reference with llink is created. The panel enables the user to decide whether the link will be kept or not.
This option is only used when external references are created with link.
Parameters:
oWarningAtCreation
Current "LinkedExternalReferencesWarningAtCreation" parameter's value:
TRUE or 1 if a panel is displayed upon external references with link creation,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NamingMode() As
Returns or sets the "NamingMode" parameter.
Role: This parameter determines how an element can be named through Edit/Properties or any operation creating a feature (Copy-Paste, etc.).
When this option is being changed, it only affects elements whose name is modified afterwards.
Parameters:
oNamingMode
Current "NamingMode" parameter's value:
catNoCheck when naming is rule-free,
catNamingCheckUnderSameNode when 2 elements cannot have the same name under the same node,
catNamingCheckWithinUIActiveObject when 2 elements cannot have the same name within a defined UIActiveObject.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NewWith3DSupport() As
Returns or sets the "NewWith3DSupport" parameter.
Role: This parameter determines if a new .CATPart document will be created with 3D working support.
Parameters:
o3DSupportCreated
Current "NewWith3DSupport" parameter's value:
TRUE or 1 if a 3D support is created,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NewWithAxisSystem() As
Returns or sets the "NewWithAxisSystem" parameter.
Role: This parameter determines if a new .CATPart document will be created with an Axis System.
Parameters:
oAxisSystemCreated
Current "NewWithAxisSystem" parameter's value:
TRUE or 1 if an axis system is created,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NewWithGS() As
Returns or sets the "NewWithGS" parameter.
Role: This parameter determines if a new .CATPart document will be created with a Geometrical Set.
Parameters:
oGSCreated
Current "NewWithGS" parameter's value:
TRUE or 1 if a G.S. is created,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NewWithOGS() As
Returns or sets the "NewWithOGS" parameter.
Role: This parameter determines if a new .CATPart document will be created with an Ordered Geometrical Set.
Parameters:
oOGSCreated
Current "NewWithOGS" parameter's value:
TRUE or 1 if an O.G.S. is created,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property NewWithPanel() As
Returns or sets the "NewWithPanel" parameter.
Role: This parameter determines if a dedicated 'New Part' panel is displayed when createing a new .CATPart document.
Parameters:
oNewPartPanelDisplayed
Current "NewWithPanel" parameter's value:
TRUE or 1 if the 'New Part' panel is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property OnlyCurrentOperatedSolidSetInGeometry() As
Returns or sets the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
Role: This parameter enables to visualize in the 3D only the current operated body's feature (operated means being aggregated in a boolean operation), as well as all other bodies and sets direcly inserted under the Part feature.
Parameters:
oDisplayed
Current "Display in 3D only current operated solid set" parameter's value:
TRUE or 1 if such is the visualization,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property OnlyCurrentSolidSetInGeometry() As
Returns or sets the "OnlyCurrentSolidSetInGeometry" parameter.
Role: This parameter enables to visualize in the 3D only the current operated body's feature (operated means being aggregated in a boolean operation), as well as all other bodies and sets direcly inserted under the Part feature.
Parameters:
oDisplayed
Current "Display in 3D only current operated solid set" parameter's value:
TRUE or 1 if such is the visualization,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ParametersNodeInTree() As
Returns or sets the "ParametersNodeInTree" parameter.
Role: This parameter determines if a node called "Parameters" is created to contain all Knowledgeware parameters.
Its value can be changed even after parameters have been created. The result is that the specification tree node display status will be affected.
Parameters:
oNodeDisplayed
Current "ParametersNodeInTree" parameter's value:
TRUE or 1 if such a node is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property PublishTopologicalElements() As
Returns or sets the "PublishTopologicalElements" parameter.
Role: This parameter defines if topological elements (faces, edges, vertices, axes extremities) can be published.
Parameters:
oTopologyAllowed
Current "PublishTopologicalElements" parameter's value:
TRUE or 1 if topological elements can be used for publication,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property RelationsNodeInTree() As
Returns or sets the "RelationsNodeInTree" parameter.
Role: This parameter determines if a node called "Relations" is created to contain all Knowledgeware relations (for instance formulas).
Its value can be changed even after parameters have been created. The result is that the specification tree node display status will be affected.
Parameters:
oNodeDisplayed
Current "RelationsNodeInTree" parameter's value:
TRUE or 1 if such a node is displayed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property ReplaceOnlyAfterCurrent() As
Returns or sets the "ReplaceOnlyAfterCurrent" parameter.
Role: This parameter defines if the replace operation can only apply to components located after the current object.
Parameters:
oOnlyAfterCurrent
Current "ReplaceOnlyAfterCurrent" parameter's value:
TRUE or 1 if the replace operation can only apply to components located after the current object,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property SurfaceElementsLocation() As
Returns or sets the "SurfaceElementsLocation" parameter.
Role: This parameter determines where wireframe and surface elements are created when hybrid design is active.
This option can be changed when hybrid design mode is not active (but useless then), and also even after a document has been opened.
Parameters:
oLocation
Current "SurfaceElementsLocation" parameter's value:
catPartBodyLocation when elements are created within a PartBody,
catXGSLocation when elements are created within a G.S. or an O.G.S..
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property TrueColorMode() As
Returns or sets the "ColorInheritanceMode" parameter.
Role: This parameter determines color inheritance mode for absorbing features in a part.
Color inheritance mode defines which mode of propagation will be used to set color on an absorbing feature. If it is valuated to 1, absorbing feature
will inherit colors from all their input. If it is defined to 0, absorbing features will inherit colors from their main input only (default mode).
This option can be changed even after a document has been opened.
Parameters:
oActivated
Current "ColorInheritanceMode" parameter's value:
TRUE or 1 if absorbing features inherit from all their inputs,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property UpdateElementsRefreshed() As
Returns or sets the "UpdateElementsRefreshed" parameter.
Role: This parameter determines if elements visualization has to be refreshed individually during update tasks.
Parameters:
oElementsRefreshed
Current "UpdateElementsRefreshed" parameter's value:
TRUE or 1 if elements visualization is refreshed,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property UpdateLinkedExternalReferences() As
Returns or sets the "UpdateLinkedExternalReferences" parameter.
Role: This parameter determines if update tasks also apply to linked external references.
Parameters:
oExternalReferencesUpdated
Current "UpdateLinkedExternalReferences" parameter's value:
TRUE or 1 if the update tasks apply to linked external references,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property UpdateMode() As
Returns or sets the "UpdateMode" parameter.
Role: This parameter determines how the update of a .CATPart document is conducted.
Parameters:
oUpdateMode
Current update mode:
catAutomaticUpdate when update is automatically launched,
catManualUpdate when update has to be launched manually.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Property UpdateStoppedOnError() As
Returns or sets the "UpdateStoppedOnError" parameter.
Role: This parameter determines if update tasks stop on the first detected error.
Parameters:
oStoppedOnError
Current "UpdateStoppedOnError" parameter's value:
TRUE or 1 if update tasks stop,
FALSE or 0 otherwise.
Returns:
S_OK if the parameter is correctly retrieved, E_FAIL otherwise.
Methods
Func GetAlsoDeleteExclusiveParentsInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "AlsoDeleteExclusiveParents" parameter.
Role:Retrieves the state of the "AlsoDeleteExclusiveParents" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetAxisSystemSizeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "AxisSystemSize" parameter.
Role:Retrieves the state of the "AxisSystemSize" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetBodiesUnderOperationsInTreeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "BodiesUnderOperationsInTree" parameter.
Role:Retrieves the state of the "BodiesUnderOperationsInTree" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColorSynchronizationEditabilityInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorSynchronizationEditability" parameter.
Role:Retrieves the state of the "ColorSynchronizationEditability" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColorSynchronizationModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorSynchronizationMode" parameter.
Role:Retrieves the state of the "ColorSynchronizationMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColorSynchronizationModeManageInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorSynchronizationModeManage" parameter.
Role:Retrieves the state of the "ColorSynchronizationModeManage" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColorSynchronizationModeOnFeatureInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorSynchronizationModeOnFeature" parameter.
Role:Retrieves the state of the "ColorSynchronizationModeOnFeature" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColorSynchronizationModeOnSubElementsInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorSynchronizationModeOnSubElements" parameter.
Role:Retrieves the state of the "ColorSynchronizationModeOnSubElements" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetColors3DExperienceManagementInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "Colors3DExperienceManagement" parameter.
Role:Retrieves the state of the "Colors3DExperienceManagement" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetConstraintsInGeometryInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ConstraintsInGeometry" parameter.
Role:Retrieves the state of the "ConstraintsInGeometry" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetConstraintsNodeInTreeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ConstraintsNodeInTree" parameter.
Role:Retrieves the state of the "ConstraintsNodeInTree" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetContextualFeaturesSelectableAtCreationInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ContextualFeaturesSelectableAtCreation" parameter.
Role:Retrieves the state of the "ContextualFeaturesSelectableAtCreation" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetDefaultColorsEditabilityInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "DefaultColorsEditability" parameter.
Role:Retrieves the state of the "DefaultColorsEditability" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetDeleteWarningBoxInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "DeleteWarningBox" parameter.
Role:Retrieves the state of the "DeleteWarningBox" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetDisplayGeometryAfterCurrentInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "DisplayGeometryAfterCurrent" parameter.
Role:Retrieves the state of the "DisplayGeometryAfterCurrent" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetExpandSketchBasedFeaturesNodeAtCreationInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
Role:Retrieves the state of the "ExpandSketchBasedFeaturesNodeAtCreation" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetExternalReferencesAsVisibleInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ExternalReferencesAsVisible" parameter.
Role:Retrieves the state of the "ExternalReferencesAsVisible" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetExternalReferencesAssemblyRootContextInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ExternalReferencesAssemblyRootContext" parameter.
Role:Retrieves the state of the "ExternalReferencesAssemblyRootContext" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetExternalReferencesNodeInTreeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ExternalReferencesNodeInTree" parameter.
Role:Retrieves the state of the "ExternalReferencesNodeInTree" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetHybridDesignModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "HybridDesignMode" parameter.
Role:Retrieves the state of the "HybridDesignMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetKnowledgeInHybridDesignModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "KnowledgeInHybridDesignMode" parameter.
Role:Retrieves the state of the "KnowledgeInHybridDesignMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetLinkedExternalReferencesInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "LinkedExternalReferences" parameter.
Role:Retrieves the state of the "LinkedExternalReferences" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetLinkedExternalReferencesOnlyOnPublicationInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "LinkedExternalReferencesOnlyOnPublication" parameter.
Role:Retrieves the state of the "LinkedExternalReferencesOnlyOnPublication" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetLinkedExternalReferencesWarningAtCreationInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "LinkedExternalReferencesWarningAtCreation" parameter.
Role:Retrieves the state of the "LinkedExternalReferencesWarningAtCreation" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNamingModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NamingMode" parameter.
Role:Retrieves the state of the "NamingMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNewWith3DSupportInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NewWith3DSupport" parameter.
Role:Retrieves the state of the "NewWith3DSupport" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNewWithAxisSystemInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NewWithAxisSystem" parameter.
Role:Retrieves the state of the "NewWithAxisSystem" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNewWithGSInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NewWithGS" parameter.
Role:Retrieves the state of the "NewWithGS" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNewWithOGSInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NewWithOGS" parameter.
Role:Retrieves the state of the "NewWithOGS" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetNewWithPanelInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "NewWithPanel" parameter.
Role:Retrieves the state of the "NewWithPanel" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetOnlyCurrentOperatedSolidSetInGeometryInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
Role:Retrieves the state of the "OnlyCurrentOperatedSolidSetInGeometry" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetOnlyCurrentSolidSetInGeometryInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "OnlyCurrentSolidSetInGeometry" parameter.
Role:Retrieves the state of the "OnlyCurrentSolidSetInGeometry" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetParametersNodeInTreeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ParametersNodeInTree" parameter.
Role:Retrieves the state of the "ParametersNodeInTree" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetPublishTopologicalElementsInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "PublishTopologicalElements" parameter.
Role:Retrieves the state of the "PublishTopologicalElements" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetRelationsNodeInTreeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "RelationsNodeInTree" parameter.
Role:Retrieves the state of the "RelationsNodeInTree" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetReplaceOnlyAfterCurrentInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ReplaceOnlyAfterCurrent" parameter.
Role:Retrieves the state of the "ReplaceOnlyAfterCurrent" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetSurfaceElementsLocationInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "SurfaceElementsLocation" parameter.
Role:Retrieves the state of the "SurfaceElementsLocation" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetTrueColorModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "ColorInheritanceMode" parameter.
Role:Retrieves the state of the "ColorInheritanceMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetUpdateElementsRefreshedInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "UpdateElementsRefreshed" parameter.
Role:Retrieves the state of the "UpdateElementsRefreshed" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetUpdateLinkedExternalReferencesInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "UpdateLinkedExternalReferences" parameter.
Role:Retrieves the state of the "UpdateLinkedExternalReferences" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetUpdateModeInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "UpdateMode" parameter.
Role:Retrieves the state of the "UpdateMode" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Func GetUpdateStoppedOnErrorInfo( ioAdminLevel, ioLocked) As
Retrieves environment informations for the "UpdateStoppedOnError" parameter.
Role:Retrieves the state of the "UpdateStoppedOnError" parameter
in the current environment.
Parameters:
ioAdminLevel
If the parameter is locked, AdminLevel gives the administration
level that imposes the value of the parameter.
If the parameter is not locked, AdminLevel gives the administration
level that will give the value of the parameter after a reset.
ioLocked
Indicates if the parameter has been locked.
Returns:
Indicates if the parameter has been explicitly modified or remain
to the administrated value.
Sub SetAlsoDeleteExclusiveParentsLock( iLocked)
Locks or unlocks the "AlsoDeleteExclusiveParents" parameter.
Role:Locks or unlocks the "AlsoDeleteExclusiveParents" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetAxisSystemSizeLock( iLocked)
Locks or unlocks the "AxisSystemSize" parameter.
Role:Locks or unlocks the "AxisSystemSize" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetBodiesUnderOperationsInTreeLock( iLocked)
Locks or unlocks the "BodiesUnderOperationsInTree" parameter.
Role:Locks or unlocks the "BodiesUnderOperationsInTree" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColorSynchronizationEditabilityLock( iLocked)
Locks or unlocks the "ColorSynchronizationEditability" parameter.
Role:Locks or unlocks the "ColorSynchronizationEditability" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColorSynchronizationModeLock( iLocked)
Locks or unlocks the "ColorSynchronizationMode" parameter.
Role:Locks or unlocks the "ColorSynchronizationMode" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColorSynchronizationModeManageLock( iLocked)
Locks or unlocks the "ColorSynchronizationModeManage" parameter.
Role:Locks or unlocks the "ColorSynchronizationModeManage" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColorSynchronizationModeOnFeatureLock( iLocked)
Locks or unlocks the "ColorSynchronizationModeOnFeature" parameter.
Role:Locks or unlocks the "ColorSynchronizationModeOnFeature" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColorSynchronizationModeOnSubElementsLock( iLocked)
Locks or unlocks the "ColorSynchronizationModeOnSubElements" parameter.
Role:Locks or unlocks the "ColorSynchronizationModeOnSubElements" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetColors3DExperienceManagementLock( iLocked)
Locks or unlocks the "Colors3DExperienceManagement" parameter.
Role:Locks or unlocks the "Colors3DExperienceManagement" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetConstraintsInGeometryLock( iLocked)
Locks or unlocks the "ConstraintsInGeometry" parameter.
Role:Locks or unlocks the "ConstraintsInGeometry" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetConstraintsNodeInTreeLock( iLocked)
Locks or unlocks the "ConstraintsNodeInTree" parameter.
Role:Locks or unlocks the "ConstraintsNodeInTree" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetContextualFeaturesSelectableAtCreationLock( iLocked)
Locks or unlocks the "ContextualFeaturesSelectableAtCreation" parameter.
Role:Locks or unlocks the "ContextualFeaturesSelectableAtCreation" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetDefaultColorsEditabilityLock( iLocked)
Locks or unlocks the "DefaultColorsEditability" parameter.
Role:Locks or unlocks the "DefaultColorsEditability" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetDeleteWarningBoxLock( iLocked)
Locks or unlocks the "DeleteWarningBox" parameter.
Role:Locks or unlocks the "DeleteWarningBox" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetDisplayGeometryAfterCurrentLock( iLocked)
Locks or unlocks the "DisplayGeometryAfterCurrent" parameter.
Role:Locks or unlocks the "DisplayGeometryAfterCurrent" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetExpandSketchBasedFeaturesNodeAtCreationLock( iLocked)
Locks or unlocks the "ExpandSketchBasedFeaturesNodeAtCreation" parameter.
Role:Locks or unlocks the "ExpandSketchBasedFeaturesNodeAtCreation" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetExternalReferencesAsVisibleLock( iLocked)
Locks or unlocks the "ExternalReferencesAsVisible" parameter.
Role:Locks or unlocks the "ExternalReferencesAsVisible" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetExternalReferencesAssemblyRootContextLock( iLocked)
Locks or unlocks the "ExternalReferencesAssemblyRootContext" parameter.
Role:Locks or unlocks the "ExternalReferencesAssemblyRootContext" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetExternalReferencesNodeInTreeLock( iLocked)
Locks or unlocks the "ExternalReferencesNodeInTree" parameter.
Role:Locks or unlocks the "ExternalReferencesNodeInTree" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetHybridDesignModeLock( iLocked)
Locks or unlocks the "HybridDesignMode" parameter.
Role:Locks or unlocks the "HybridDesignMode" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetKnowledgeInHybridDesignModeLock( iLocked)
Locks or unlocks the "KnowledgeInHybridDesignMode" parameter.
Role:Locks or unlocks the "KnowledgeInHybridDesignMode" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetLinkedExternalReferencesLock( iLocked)
Locks or unlocks the "LinkedExternalReferences" parameter.
Role:Locks or unlocks the "LinkedExternalReferences" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetLinkedExternalReferencesOnlyOnPublicationLock( iLocked)
Locks or unlocks the "LinkedExternalReferencesOnlyOnPublication" parameter.
Role:Locks or unlocks the "LinkedExternalReferencesOnlyOnPublication" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetLinkedExternalReferencesWarningAtCreationLock( iLocked)
Locks or unlocks the "LinkedExternalReferencesWarningAtCreation" parameter.
Role:Locks or unlocks the "LinkedExternalReferencesWarningAtCreation" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNamingModeLock( iLocked)
Locks or unlocks the "NamingMode" parameter.
Role:Locks or unlocks the "NamingMode" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNewWith3DSupportLock( iLocked)
Locks or unlocks the "NewWith3DSupport" parameter.
Role:Locks or unlocks the "NewWith3DSupport" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNewWithAxisSystemLock( iLocked)
Locks or unlocks the "NewWithAxisSystem" parameter.
Role:Locks or unlocks the "NewWithAxisSystem" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNewWithGSLock( iLocked)
Locks or unlocks the "NewWithGS" parameter.
Role:Locks or unlocks the "NewWithGS" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNewWithOGSLock( iLocked)
Locks or unlocks the "NewWithOGS" parameter.
Role:Locks or unlocks the "NewWithOGS" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetNewWithPanelLock( iLocked)
Locks or unlocks the "NewWithPanel" parameter.
Role:Locks or unlocks the "NewWithPanel" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetOnlyCurrentOperatedSolidSetInGeometryLock( iLocked)
Locks or unlocks the "OnlyCurrentOperatedSolidSetInGeometry" parameter.
Role:Locks or unlocks the "OnlyCurrentOperatedSolidSetInGeometry" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetOnlyCurrentSolidSetInGeometryLock( iLocked)
Locks or unlocks the "OnlyCurrentSolidSetInGeometry" parameter.
Role:Locks or unlocks the "OnlyCurrentSolidSetInGeometry" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetParametersNodeInTreeLock( iLocked)
Locks or unlocks the "ParametersNodeInTree" parameter.
Role:Locks or unlocks the "ParametersNodeInTree" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetPublishTopologicalElementsLock( iLocked)
Locks or unlocks the "PublishTopologicalElements" parameter.
Role:Locks or unlocks the "PublishTopologicalElements" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetRelationsNodeInTreeLock( iLocked)
Locks or unlocks the "RelationsNodeInTree" parameter.
Role:Locks or unlocks the "RelationsNodeInTree" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetReplaceOnlyAfterCurrentLock( iLocked)
Locks or unlocks the "ReplaceOnlyAfterCurrent" parameter.
Role:Locks or unlocks the "ReplaceOnlyAfterCurrent" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetSurfaceElementsLocationLock( iLocked)
Locks or unlocks the "SurfaceElementsLocation" parameter.
Role:Locks or unlocks the "SurfaceElementsLocation" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetUpdateElementsRefreshedLock( iLocked)
Locks or unlocks the "UpdateElementsRefreshed" parameter.
Role:Locks or unlocks the "UpdateElementsRefreshed" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetUpdateLinkedExternalReferencesLock( iLocked)
Locks or unlocks the "UpdateLinkedExternalReferences" parameter.
Role:Locks or unlocks the "UpdateLinkedExternalReferences" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetUpdateModeLock( iLocked)
Locks or unlocks the "UpdateMode" parameter.
Role:Locks or unlocks the "UpdateMode" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Sub SetUpdateStoppedOnErrorLock( iLocked)
Locks or unlocks the "UpdateStoppedOnError" parameter.
Role:Locks or unlocks the "UpdateStoppedOnError" parameter if it is possible
in the current administrative context. In user mode this method will always
return E_FAIL.
Parameters:
iLocked
the locking operation to be performed
Legal values:
TRUE :   to lock the parameter.
FALSE:   to unlock the parameter.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_PartServices_23091 ===
MecModInterfaces PartServices (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
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PartServices (Object)
The object exposes services for the part.
This object is available thanks to     Set myPart = CATIA.ActiveDocument.Part
' Get Service Object by querying on part - extension of CATIA Base
Set partServices = myPart.GetItem("CATPartServices")
Example:
Set part1 = CATIA.ActiveDocument.Part
Set partServices1 = myPart.GetItem("CATPartServices")
Method Index
GetNearSubElements
Get the sub elements of a geometric object or a body that are the closest to a geometric object or a body.
GetSubElements
Get the sub elements of a geometric object or a body.
Methods
Func GetNearSubElements( iObject, iSubElementDimension, iNearObject) As
Get the sub elements of a geometric object or a body that are the closest to a geometric object or a body.
Parameters:
iObject
A geometric object or a body
iSubElementDimension
The dimension of sub elements wanted: 0 for vertex, 1 for edge, 2 for face.
iNearObject
A geometric object or a body to be close to
oSubElements
List of the sub elements of iObject (without duplicates) closest to iNearObject.
Example:
The following example returns the vertices of a pad that are the closest to a point.
Set part1 = CATIA.ActiveDocument.Part
Set bodies1 = part1.Bodies
Set body1 = bodies1.Item("PartBody")
Set shapes1 = body1.Shapes
Set pad1 = shapes1.Item("Pad.1")
Set point1 = shapes1.Item("Point.1")
Set partServices1 = myPart.GetItem("CATPartServices")
Set references1 = partServices1.GetSubNearElements(pad1, 0, point1)
Func GetSubElements( iObject, iSubElementDimension, iDuplicates) As
Get the sub elements of a geometric object or a body.
Parameters:
iObject
A geometric object or a body
iSubElementDimension
The dimension of sub elements wanted: 0 for vertex, 1 for edge, 2 for face.
iDuplicates
Allow duplicate sub elements in the list. FALSE will remove duplicates (same label and selecting feature).
oSubElements
List of the sub elements
Example:
The following example returns the vertices of a pad
Set part1 = CATIA.ActiveDocument.Part
Set bodies1 = part1.Bodies
Set body1 = bodies1.Item("PartBody")
Set shapes1 = body1.Shapes
Set pad1 = shapes1.Item("Pad.1")
Set partServices1 = myPart.GetItem("CATPartServices")
Set references1 = partServices1.GetSubElements(pad1, 0, True)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_PlanarFace_20455 ===
MecModInterfaces PlanarFace (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
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PlanarFace (Object)
2-D boundary with a planar geometry.
Role:
This  object may be, for example, the face of a cube. You will create a PlanarFace object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a PlanarFace object is limited, see
.
Example:
This example asks the end user to select a face and two planar faces, and creates a draft on these faces:
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select the face to draft
InputObjectType(0)="Face"
Status=Selection.SelectElement2(InputObjectType,"Select the face to draft",true)
if (Status = "cancel") then Exit Sub
Set FaceToDraft = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the neutral face
InputObjectType(0)="PlanarFace"
Status=Selection.SelectElement2(InputObjectType,"Select the neutral face",true)
if (Status = "cancel") then Exit Sub
Set NeutralFace = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the parting element
InputObjectType(0)="PlanarFace"
Status=Selection.SelectElement2(InputObjectType,"Select the parting element",true)
if (Status = "cancel") then Exit Sub
Set PartingElement = Selection.Item(1).Value
Set Draft = ShapeFactory.AddNewDraft(FaceToDraft,NeutralFace,0,PartingElement,0.0,0.0,1.0,0,5.0,0)
Set DraftDomains = Draft.DraftDomains
Set DraftDomain = DraftDomains.Item(1)
DraftDomain.SetPullingDirection 0.0, 0.0,1.0
Document.Part.Update
Method Index
GetFirstAxis
Returns the planar face first axis
GetOrigin
Returns the origin of the planar face.
GetSecondAxis
Returns the planar face second axis.
Methods
Sub GetFirstAxis( oFirstAxis)
Returns the planar face first axis
Parameters:
oFirstAxis[0]
The X Coordinate of the planar face first axis
oFirstAxis[1]
The Y Coordinate of the planar face first axis
oFirstAxis[2]
The Z Coordinate of the planar face first axis
Sub GetOrigin( oOrigin)
Returns the origin of the planar face.
Parameters:
oOrigin[0]
The X Coordinate of the planar face origin
oOrigin[1]
The Y Coordinate of the planar face origin
oOrigin[2]
The Z Coordinate of the planar face origin
Sub GetSecondAxis( oSecondAxis)
Returns the planar face second axis.
Parameters:
oSecondAxis[0]
The X Coordinate of the planar face second axis
oSecondAxis[1]
The Y Coordinate of the planar face second axis
oSecondAxis[2]
The Z Coordinate of the planar face second axis
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_RectilinearBiDimFeatEdge_42724 ===
MecModInterfaces RectilinearBiDimFeatEdge (Object)
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This Framework
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RectilinearBiDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is two dimensional, the boundary having a rectilinear geometry.
Role:
This  object may be, for example, the edge of a surface obtained through the extrusion of a line.
You will create a RectilinearBiDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a RectilinearBiDimFeatEdge object is limited, see
.
Example: see the
example
Method Index
GetDirection
Returns the direction of the rectilinear edge.
GetOrigin
Returns the origin of the the rectilinear edge.
Methods
Sub GetDirection( oDirection)
Returns the direction of the rectilinear edge.
Parameters:
oDirection[0]
The X Coordinate of the direction
oDirection[1]
The Y Coordinate of the direction
oDirection[2]
The Z Coordinate of the direction
Sub GetOrigin( oOrigin)
Returns the origin of the the rectilinear edge.
Parameters:
oOrigin[0]
The X Coordinate of the rectilinear edge origin
oOrigin[1]
The Y Coordinate of the rectilinear edge origin
oOrigin[2]
The Z Coordinate of the rectilinear edge origin
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_RectilinearMonoDimFeatEdge_47979 ===
MecModInterfaces RectilinearMonoDimFeatEdge (Object)
All Frameworks
Class Hierarchy
This Framework
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RectilinearMonoDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is one dimensional, the boundary having a rectilinear geometry.
Role:
This  object may be, for example, in a part containing a Sketch which is made up of a line segment and a spline, the line segment.
You will create a RectilinearMonoDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a RectilinearMonoDimFeatEdge object is limited, see
.
Example: see the
example
Method Index
GetDirection
Returns the direction of the rectilinear edge
GetOrigin
Returns the origin of the the rectilinear edge.
Methods
Sub GetDirection( oDirection)
Returns the direction of the rectilinear edge
Parameters:
oDirection[0]
The X Coordinate of the direction
oDirection[1]
The Y Coordinate of the direction
oDirection[2]
The Z Coordinate of the direction
Sub GetOrigin( oOrigin)
Returns the origin of the the rectilinear edge.
Parameters:
oOrigin[0]
The X Coordinate of the rectilinear edge origin
oOrigin[1]
The Y Coordinate of the rectilinear edge origin
oOrigin[2]
The Z Coordinate of the rectilinear edge origin
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_RectilinearTriDimFeatEdge_45434 ===
MecModInterfaces RectilinearTriDimFeatEdge (Object)
All Frameworks
Class Hierarchy
This Framework
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RectilinearTriDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is three dimensional, the boundary having a rectilinear geometry.
Role:
This  object may be, for example, the edge of a Pad resulting from the extrusion of a square.  You will create a RectilinearTriDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a RectilinearTriDimFeatEdge object is limited, see
.
Example:
This example asks the end user to select a face, a rectilinear edge, and creates a hole.
The rectilinear edge specifies the hole direction. It may be a RectilinearTriDimFeatEdge, a RectilinearBiDimFeatEdge
or a RectilinearMonoDimFeatEdge.
Dim EnabledObjectSelection1(0)
Dim EnabledObjectSelection2(2)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select a face
EnabledObjectSelection1(0)="Face"
Status=Selection.SelectElement2(EnabledObjectSelection1,"Select a face",true)
if (Status = "cancel") then Exit Sub
Set Face = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the hole direction
EnabledObjectSelection2(0)="RectilinearTriDimFeatEdge"
EnabledObjectSelection2(1)="RectilinearBiDimFeatEdge"
EnabledObjectSelection2(2)="RectilinearMonoDimFeatEdge"
Status=Selection.SelectElement2(EnabledObjectSelection2,"Select the hole direction",true)
if (Status = "cancel") then Exit Sub
Set Hole = ShapeFactory.AddNewHoleFromPoint(20.0,-5.5, 1.07,Face,10.0)
Hole.ThreadingMode = 1
Hole.ThreadSide = 0
Hole.SetDirection Selection.Item(1).Value
Document.Part.Update
Method Index
GetDirection
Returns the direction of the rectilinear edge
GetOrigin
Returns the origin of the the rectilinear edge.
Methods
Sub GetDirection( oDirection)
Returns the direction of the rectilinear edge
Parameters:
oDirection[0]
The X Coordinate of the direction
oDirection[1]
The Y Coordinate of the direction
oDirection[2]
The Z Coordinate of the direction
Sub GetOrigin( oOrigin)
Returns the origin of the the rectilinear edge.
Parameters:
oOrigin[0]
The X Coordinate of the rectilinear edge origin
oOrigin[1]
The Y Coordinate of the rectilinear edge origin
oOrigin[2]
The Z Coordinate of the rectilinear edge origin
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Shape_17103 ===
MecModInterfaces Shape (Object)
All Frameworks
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This Framework
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Shape (Object)
Represents the Shape object.
It is an abstract object which is not intended to be created as such,
from which all objects having a shape representation derive.
See also:
, , ,
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ShapeInstance_24135 ===
MecModInterfaces ShapeInstance (Object)
All Frameworks
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ShapeInstance (Object)
The interface to access a CATIAShapeInstance.
Property Index
InputsCount
Returns the number of Inputs.
OutputsCount
Returns the number of Outputs.
ParametersCount
Returns the number of Parameters.
Method Index
GetInput
Gets an input of a shape instance by its name.
GetInputData
Gets an input of a shape instance by its name.
GetInputDataFromPosition
Gets an input of a hybrid shape instance from its position.
GetInputFromPosition
Gets an input of a hybrid shape instance from its position.
GetOutput
Gets a Ouput by its name.
GetOutputFromPosition
Gets a Ouput from its position.
GetParameter
Gets a parameter of a shape instance by its name.
GetParameterFromPosition
Gets a parameter of a hybrid shape instance from its position.
PutInput
Defines an input of a shape instance.
PutInputData
Defines an input of a shape instance.
Properties
Property InputsCount() As   (Read Only)
Returns the number of Inputs.
Example:
The following example retrieves in inputsCount
the number of Inputs of hybridShapeInstance:
inputsCount = hybridShapeInstance.InputsCount
Property OutputsCount() As   (Read Only)
Returns the number of Outputs.
Example:
The following example retrieves in outputsCount
the number of Outputs of hybridShapeInstance:
outputsCount = hybridShapeInstance.OutputsCount
Property ParametersCount() As   (Read Only)
Returns the number of Parameters.
Example:
The following example retrieves in parametersCount
the number of parameters of hybridShapeInstance:
parametersCount = hybridShapeInstance.ParametersCount
Methods
Func GetInput( iName) As
Gets an input of a shape instance by its name.
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
Func GetInputData( iName) As
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
Func GetInputDataFromPosition( iPosition) As
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
Func GetInputFromPosition( iPosition) As
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
Func GetOutput( iName) As
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
Func GetOutputFromPosition( iPosition) As
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
Func GetParameter( iName) As
Gets a parameter of a shape instance by its name.
Parameters:
iName
The name of the parameter of the shape instance
Returns:
The parameter, if found
Example:
The following example tests if the parameter was found:
Set parameter = shapeInstance.GetParameter("Parameter1")
If TypeName(parameter)="Nothing" Then
MsgBox "Parameter not found"
End If
Func GetParameterFromPosition( iPosition) As
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
Sub PutInput( iName, iInput)
Defines an input of a shape instance.
Parameters:
iName
The input name
iInput
The element wich will be input of the shape instance
All types of
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
Sub PutInputData( iName, 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
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
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Shapes_17678 ===
MecModInterfaces Shapes (Object)
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Shapes (Object)
The collection of the shapes making up a body.
Method Index
GetBoundary
Returns a boundary using its label.
Item
Returns a shape using its index or its name from the Shapes collection.
Methods
Func GetBoundary( iLabel) As
Returns a boundary using its label.
Parameters:
iLabel
Identification of the
object.   See
.
Returns:
The retrieved boundary
Func Item( iIndex) As
Returns a shape using its index or its name from the Shapes collection.
Parameters:
iIndex
The index or the name of the shape to retrieve from
the collection of shapes.
As a numerics, this index is the rank of the shape
in the collection.
The index of the first shape in the collection is 1, and
the index of the last shape is
.   As a string, it is the name you assigned to the shape using
the
property.
Returns:
The retrieved shape
Example:
This example retrieves in ThisShape the third shape,
and in ThatShape the shape named
MyShape in the shape collection of the active document,
supposed to be a part document.
Set ThisShape = CATIA.ActiveDocument.Shapes.Item(3)
Set ThatShape = CATIA.ActiveDocument.Shapes.Item("MyShape")
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Sketches_19049 ===
MecModInterfaces Sketches (Object)
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Sketches (Object)
The body's collection of sketches not yet used by any shape.
Method Index
Add
Creates a new sketch and adds it to the sketch collection.
GetBoundary
Returns a boundary using its label.
Item
Returns a sketch using its index or its name from the Sketches
collection.
Methods
Func Add( iPlane) As
Creates a new sketch and adds it to the sketch collection.
The sketch creation implies to specify a supporting plane.
Once created, the sketch exists, but is empty.
You must use the
method to begin to edit it.
Parameters:
iPlane
The sketch supporting plane
The following
object is supported:
.
Returns:
oNewSketch   The created sketch
Example:
This example creates the newSketch sketch on the XY plane
of the myPart part:
Set XYPlane = myPart.OriginElements.PlaneXY()
Set newSketch = myPart.Sketches.Add(XYPlane)
Func GetBoundary( iLabel) As
Returns a boundary using its label.
Parameters:
iLabel
Identification of the
object.   See
.
Returns:
The retrieved boundary
Func Item( iIndex) As
Returns a sketch using its index or its name from the Sketches
collection.
Parameters:
iIndex
The index or the name of the sketch to retrieve from
the collection of sketches.
As a numerics, this index is the rank of the sketch
in the collection.
The index of the first sketch in the collection is 1, and
the index of the last sketch is Count.
As a string, it is the name you assigned to the sketch using
the
property.
Returns:
The retrieved sketch
Example:
This example retrieves the last item in the collection sketches.
Set lastSketch = sketchList.Item(sketchList.Count)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Solid_17107 ===
MecModInterfaces Solid (Object)
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Solid (Object)
Represents an imported solid object.
Role: the imported solid is a solid obtained from copy/paste with link or design in context.
The solid object has a link to a source element obtained from  and a source product obtained from
.
Property Index
Move
Returns the move object of the solid.
SourceElement
Returns the source element of the imported solid.
SourceProduct
Returns the source product instance of the imported solid.
Properties
Property Move() As   (Read Only)
Returns the move object of the solid.
Role:
The move object is aggregated by the solid object
and itself aggregates a movable object
to which you can apply a move transformation
by means of an isometry matrix. It moves the solid
according to this isometry.
Example:
This example retrieves the move object EngineMoveObject for the
Engine product.
Dim EngineMoveObject As Move
Set EngineMoveObject = Engine.Move
See also:
Property SourceElement() As   (Read Only)
Returns the source element of the imported solid.
Role: returns the linked element in the source part.
Example:
The following example returns in element the source element
of the imported solid importedSolid:
Set element = importedSolid.SourceElement
Property SourceProduct() As   (Read Only)
Returns the source product instance of the imported solid.
Role: returns the product instance which was selected when the import was created.
Example:
The following example returns in prod1 the source product instance
of the imported solid importedSolid:
Set prod1 = importedSolid.SourceProduct
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_TriDimFeatEdge_24844 ===
MecModInterfaces TriDimFeatEdge (Object)
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TriDimFeatEdge (Object)
1-D boundary belonging to a feature whose topological result is three dimensional.
Role:
This  object may be, for example, the edge of a Pad.  You will create a TriDimFeatEdge object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a TriDimFeatEdge object is limited, see
.
Example:
This example asks the end user to select an edge, and creates an edge fillet on this edge:
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
'We propose to the user that he select an edge
InputObjectType(0)="TriDimFeatEdge"
Status=Selection.SelectElement2(InputObjectType,"Select an edge",true)
if (Status = "cancel") then Exit Sub
Set EdgeFillet = ShapeFactory.AddNewEdgeFilletWithConstantRadius(Selection.Item(1).Value,1,5.0)
EdgeFillet.EdgePropagation = 1
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_TriDimFeatVertexOrBiDimFeatVertex_69296 ===
MecModInterfaces TriDimFeatVertexOrBiDimFeatVertex (Object)
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TriDimFeatVertexOrBiDimFeatVertex (Object)
0-D boundary belonging to a feature whose topological result is three dimensional or two dimentional.
Role:
This  object may be, for example, the corner of a Pad resulting from the extrusion of a  square.
You will create a TriDimFeatVertexOrBiDimFeatVertex object using the
,
,
or
method. Then, you pass it to the operator.
The lifetime of a TriDimFeatVertexOrBiDimFeatVertex object is limited, see
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Vertex_17746 ===
MecModInterfaces Vertex (Object)
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Vertex (Object)
0-D boundary.
Role:
This  object may be, for example, the corner of a Pad resulting from the extrusion of a  square.
You will create an Vertex object using the
,
,
or
method. Then, you pass it to the operator (such as
).  The lifetime of a Vertex object is limited, see
.  See also:
,
,
.
Example:
This example asks the end user to select successively two vertices. Then, it creates a line between these
two vertices.
Dim InputObjectType(0)
Set Document = CATIA.ActiveDocument
Set Selection = Document.Selection
Set HybridBodies = Document.Part.HybridBodies
Set HybridBody = HybridBodies.Item("Geometrical Set.1")
'We propose to the user that he select the first vertex
InputObjectType(0)="Vertex"
Status=Selection.SelectElement2(InputObjectType,"Select the first vertex",true)
if (Status = "cancel") then Exit Sub
Set FirstVertex = Selection.Item(1).Value
Selection.Clear
'We propose to the user that he select the second vertex
InputObjectType(0)="Vertex"
Status=Selection.SelectElement2(InputObjectType,"Select the second vertex",true)
if (Status = "cancel") then Exit Sub
Set SecondVertex = Selection.Item(1).Value
Set hybridShapeLinePtPt = HybridShapeFactory.AddNewLinePtPt(FirstVertex,SecondVertex)
HybridBody.AppendHybridShape hybridShapeLinePtPt
Document.Part.InWorkObject = hybridShapeLinePtPt
Document.Part.Update
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ZeroDimFeatVertexOrWireBoundaryMonoDimFeatVertex_131539 ===
MecModInterfaces ZeroDimFeatVertexOrWireBoundaryMonoDimFeatVertex (Object)
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ZeroDimFeatVertexOrWireBoundaryMonoDimFeatVertex (Object)
0-D boundary beeing either an isolated point or the extremity of a feature whose topological result is one dimensional.
Role:
This  object may be, for example, the extremity of a line segment.  You will create a ZeroDimFeatVertexOrWireBoundaryMonoDimFeatVertex object using the
,
,
or
method.  Then, you pass it to the operator.
The lifetime of a ZeroDimFeatVertexOrWireBoundaryMonoDimFeatVertex object is limited, see
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.