=== enum_CatCDHoleMode_17692 ===
PartInterfaces CatCDHoleModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatCDHoleMode (Enumeration)
enum CatCDHoleMode {
catCDModeNoCountersunkDiameter,
catCDModeCountersunkDiameter
}
Counterdrilled hole mode.
It describes the chosen mode for Counterdrilled hole.
Values:
catCDModeNoCountersunkDiameter
Counterdrilled parameters are Diameter, Depth and Angle
catCDModeCountersunkDiameter
Counterdrilled parameters are Diameter, Depth, Angle and Countersunk Diameter
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatChamferMode_19322 ===
PartInterfaces CatChamferModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatChamferMode (Enumeration)
enum CatChamferMode {
catTwoLengthChamfer,
catLengthAngleChamfer
}
Chamfer definition mode.
A chamfer between two faces can be defined using two lengthes,
or a length and an angle.
The first length, or the single length, depending on the way the
chamfer is defined, is measured on the reference face from the
edge to chamfer
to determine the first edge the chamfer creates on the reference face.
This reference face is either the face selected or the face
determined by CATIA if the edge to be chamfered was selected.
The second length, or the angle, determines the second edge that the
chamfer creates on the second face.
Values:
catTwoLengthChamfer
The chamfer is defined using two lengthes
catLengthAngleChamfer
The chamfer is defined using a length and an angle
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatChamferOrientation_32438 ===
PartInterfaces CatChamferOrientationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatChamferOrientation (Enumeration)
enum CatChamferOrientation {
catNoReverseChamfer,
catReverseChamfer
}
Chamfer orientation.
Defines whether to keep the face selected or determined by CATIA
as the chamfer reference face.
Values:
catNoReverseChamfer
The chamfer reference face is the face selected or determined by CATIA
catReverseChamfer
The chamfer reference face is the other face
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatChamferPropagation_32286 ===
PartInterfaces CatChamferPropagationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatChamferPropagation (Enumeration)
enum CatChamferPropagation {
catTangencyChamfer,
catMinimalChamfer
}
Chamfer propagation mode.
Once running on an egde, a chamfer operation may propagate onto other
edges that extend the first one. This mode controls the chamfer ability
to do so.
Values:
catTangencyChamfer
The chamfer operation also chamfers any other edges
found at the first edge extremities, as long as they are tangent with
it. This process repeats until no more tangent edges to chamfer are
found at extremities of already chamfered ones.
catMinimalChamfer
The chamfer operation stops as soon as an edge to chamfer cuts
one or the two chamfer created edges
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatCircularPatternParameters_50079 ===
PartInterfaces CatCircularPatternParametersEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatCircularPatternParameters (Enumeration)
enum CatCircularPatternParameters {
catInstancesandAngularSpacing,
catCompleteCrown,
catUnequalAngularSpacing
}
Circular Pattern Parameters.
The Circular Pattern can apply parameters to the angular repartition.
Values:
catInstancesandAngularSpacing
The number of instances and the angular spacing are used to define the Pattern.
catCompleteCrown
Only the number of instances is used to define the Pattern, the total angle is set to 360 degrees.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatCSHoleMode_17752 ===
PartInterfaces CatCSHoleModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatCSHoleMode (Enumeration)
enum CatCSHoleMode {
catCSModeDepthAngle,
catCSModeDepthDiameter,
catCSModeAngleDiameter
}
Countersunk hole mode.
It describes the chosen mode for countersunk hole.
Values:
catCSModeDepthAngle
Countersunk parameters are depth and angle
catCSModeDepthDiameter
Countersunk parameters are depth and Diameter
catCSModeAngleDiameter
Countersunk parameters are angle and Diameter
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatDraftMode_16809 ===
PartInterfaces CatDraftModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatDraftMode (Enumeration)
enum CatDraftMode {
catStandardDraftMode,
catReflectKeepFaceDraftMode,
catReflectKeepEdgeDraftMode
}
Draft mode.
The draft consists in the envelope of a cone propagated along the
neutral edge.
Values:
catStandardDraftMode
The draft's neutral element must be input
catReflectKeepFaceDraftMode
The draft's neutral element is computed while maintaining
the adjacent faces
catReflectKeepEdgeDraftMode
The draft's neutral element is computed while maintaining
the adjacent edges
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatDraftMultiselectionMode_43981 ===
PartInterfaces CatDraftMultiselectionModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatDraftMultiselectionMode (Enumeration)
enum CatDraftMultiselectionMode {
catNoneDraftMultiselectionMode,
catDraftMultiselectionByNeutralMode
}
Multi Selection Mode.
The elements to be drafted can be selected explicitly
or can implicitly selected as neighbors of the neutral face
Values:
catNoneDraftMultiselectionMode
The elements to be drafted can be selected explicitly
catMultiselectionByNeutralMode
The elements to be drafted are the neighbors of the neutral face
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatDraftNeutralPropagationMode_55179 ===
PartInterfaces CatDraftNeutralPropagationModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatDraftNeutralPropagationMode (Enumeration)
enum CatDraftNeutralPropagationMode {
catNoneDraftNeutralPropagationMode,
catSmoothDraftNeutralPropagationMode
}
Draft neutral propagation.
The draft neutral element can consist in only the selected element
or can be propagated to all the tangent surfaces
Values:
catNoneDraftNeutralPropagationMode
The neutral element consists in only the selected surface
catSmoothDraftNeutralPropagationMode
The neutral element consists in the selected surface and all
its adjacent tangent surfaces
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatFilletBitangencyType_36649 ===
PartInterfaces CatFilletBitangencyTypeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatFilletBitangencyType (Enumeration)
enum CatFilletBitangencyType {
catSphereBitangencyType,
catCircleBitangencyType
}
Fillet Bitangency Type.
Defines the type of Bitangency
Values:
catCircleBitangencyType
Fillet type is circle. A Spine then
must be defined.
catSphereBitangencyType
Fillet type is sphere
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatFilletBoundaryRelimitation_53248 ===
PartInterfaces CatFilletBoundaryRelimitationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatFilletBoundaryRelimitation (Enumeration)
enum CatFilletBoundaryRelimitation {
catAutomaticFilletBoundaryRelimitation,
catUVFilletBoundaryRelimitation,
catConnectFilletBoundaryRelimitation,
catMinimumFilletBoundaryRelimitation,
catMaximumFilletBoundaryRelimitation
}
Fillet boundary relimitation.
Fillets can be created on open body, so you can choose
the relimitation mode on open boundaries.
Values:
catAutomaticFilletBoundaryRelimitation
for PartDesign Fillet
catUVFilletBoundaryRelimitation
catConnectFilletBoundaryRelimitation
catMinimumFilletBoundaryRelimitation
Fillet expands up to the limits of the smallest shell
catMaximumFilletBoundaryRelimitation
Fillet expands up to the limits of the largest shell
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatFilletEdgePropagation_38869 ===
PartInterfaces CatFilletEdgePropagationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatFilletEdgePropagation (Enumeration)
enum CatFilletEdgePropagation {
catMinimalFilletEdgePropagation,
catTangencyFilletEdgePropagation
}
Fillet edge propagation.
The fillet can apply to the selected edge only or to all contiguous
edges that are tangent to the selected edge.
Values:
catMinimalFilletEdgePropagation
The fillet is applied only to the selected edge and propagated to the
first natural relimitation
catTangencyFilletEdgePropagation
The fillet is propagated to all the tangent contiguous edges
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatFilletTrimSupport_30658 ===
PartInterfaces CatFilletTrimSupportEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatFilletTrimSupport (Enumeration)
enum CatFilletTrimSupport {
catTrimFilletSupport,
catNoTrimFilletSupport
}
Fillet Trim Support.
Fillets can be created on open body, so you can choose
to trim of fillet support.
Values:
catTrimFilletSupport
Trim of fillet support
catNoTrimFilletSupport
No trim of fillet support
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatFilletVariation_26331 ===
PartInterfaces CatFilletVariationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatFilletVariation (Enumeration)
enum CatFilletVariation {
catLinearFilletVariation,
catCubicFilletVariation
}
Fillet edge variation.
Variable edge fillets can have their radius that varies in a
linear mode from vertex to vertex or in a cubic mode.
Values:
catLinearFilletVariation
The fillet radius varies in a linear mode
catCubicFilletVariation
The fillet radius varies in a cubic mode
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleAnchorMode_23846 ===
PartInterfaces CatHoleAnchorModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleAnchorMode (Enumeration)
enum CatHoleAnchorMode {
catExtremPointHoleAnchor,
catMiddlePointHoleAnchor
}
Hole anchoring mode.
It specifies the way the hole is anchored to its support.
This is valid with catCounterboredHole and
catCounterdrilledHole holes only.
Otherwise, holes are considered as anchored with the top of their head.
Values:
catExtremPointHoleAnchor
The hole is anchored with the top of its head
catCATMiddlePointHoleAnchor
The hole is anchored with the bottom of its head
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleBottomType_24485 ===
PartInterfaces CatHoleBottomTypeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleBottomType (Enumeration)
enum CatHoleBottomType {
catFlatHoleBottom,
catVHoleBottom,
catTrimmedHoleBottom
}
Hole bottom type.
It describes the shape the hole bottom can have.
Values:
catFlatHoleBottom
The hole bottom is flat
catVHoleBottom
The hole bottom has a V-Shape
catTrimmedHoleBottom
The hole bottom has a shape obtained by trimming of hole with surface/plane
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleThreadingMode_29331 ===
PartInterfaces CatHoleThreadingModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleThreadingMode (Enumeration)
enum CatHoleThreadingMode {
catThreadedHoleThreading,
catSmoothHoleThreading
}
Hole threading mode.
It describes the different threadings the hole may receive.
Values:
catThreadedHoleThreading
The hole is threaded
catSmoothHoleThreading
The hole is smooth threaded
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleThreadSide_23708 ===
PartInterfaces CatHoleThreadSideEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleThreadSide (Enumeration)
enum CatHoleThreadSide {
catRightThreadSide,
catLeftThreadSide
}
Hole threading .
side
It describes the side of hole thread.
Values:
catRightThreadSide
The hole is right-threaded
catLeftThreadSide
The hole is left-threaded
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleThreadStandard_31573 ===
PartInterfaces CatHoleThreadStandardEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleThreadStandard (Enumeration)
enum CatHoleThreadStandard {
catHoleMetricThinPitch,
catHoleMetricThickPitch
}
Hole Thread Standard
It describes the standard to be used for hole threads.
Values:
catHoleMetricThinPitch
The hole thread standard is Metric Thin Pitch
catHoleMetricThickPitch
The hole thread standard is Metric Thick Pitch
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatHoleType_15894 ===
PartInterfaces CatHoleTypeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatHoleType (Enumeration)
enum CatHoleType {
catSimpleHole,
catTaperedHole,
catCounterboredHole,
catCountersunkHole,
catCounterdrilledHole
}
Hole type.
Values:
catSimpleHole
Simple hole
catTaperedHole
Tapered hole
catCounterboredHole
Counterbored hole
catCountersunkHole
Countersunk hole
catCounterdrilledHole
Counterdrilled hole
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatLimitMode_16875 ===
PartInterfaces CatLimitModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatLimitMode (Enumeration)
enum CatLimitMode {
catOffsetLimit,
catUpToNextLimit,
catUpToLastLimit,
catUpToPlaneLimit,
catUpToSurfaceLimit,
catUpThruNextLimit,
catUntilLimit
}
Limit mode.
Prismatic elements and holes are limited by surfaces or offset values.
This enum lists appropriate values to set this property.
Values:
catOffsetLimit
The shape is limited by an offset value.
catUpToNextLimit
The shape is limited by the next boundary encountered.
catUpToLastLimit
The shape is limited by the last boundary encountered.
catUpToPlaneLimit
The shape is limited by a selected plane.
catUpToSurfaceLimit
The shape is limited by a selected surface.
catUpThruNextLimit
The shape is limited by the next boundary encountered.
catUntilLimit
The shape is limited by a selected relimited face.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatMergeMode_16770 ===
PartInterfaces CatMergeModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatMergeMode (Enumeration)
enum CatMergeMode {
catMergeOff,
catMergeOn
}
Merge mode.
Sweep elements can be limited by existing material.
This enum lists appropriate values to set this property.
Values:
catMergeOff
The shape is not limited by existing material.
catMergeOn
The shape is limited by existing material
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatPrismExtrusionDirection_44720 ===
PartInterfaces CatPrismExtrusionDirectionEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatPrismExtrusionDirection (Enumeration)
enum CatPrismExtrusionDirection {
catNormalToSketchDirection,
catNotNormalToSketchDirection
}
Prism extrusion type.
The prism shapes can be extruded using a default direction
normal to the sketch plane. Otherwise, the extrusion direction
should be specified.
Values:
catNormalToSketchDirection
The prism is extruded using the sketch normal direction
catNotNormalToSketchDirection
The prism is not extruded using the sketch normal direction.
The actual extrusion direction should be specified.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatPrismOrientation_28480 ===
PartInterfaces CatPrismOrientationEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatPrismOrientation (Enumeration)
enum CatPrismOrientation {
catRegularOrientation,
catInverseOrientation
}
Prism extrusion orientation mode.
Values:
catRegularOrientation
The prism is extruded with the same orientation as the one
given by its extrusion direction vector
catInverseOrientation
The prism is extruded in the reverse direction than its
extrusion direction vector orientation
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatRectangularPatternParameters_59263 ===
PartInterfaces CatRectangularPatternParametersEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatRectangularPatternParameters (Enumeration)
enum CatRectangularPatternParameters {
catInstancesandSpacing,
catUnequalSpacing
}
Rectangular Pattern Parameters.
The Rectangular Pattern can apply parameters to the repartition.
Values:
catInstancesandSpacing
The number of instances and the length spacing are used to define the Pattern.
catUnequalSpacing
Only the number of instances is used to define the Pattern.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatSewingIntersectionMode_41376 ===
PartInterfaces CatSewingIntersectionModeEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatSewingIntersectionMode (Enumeration)
enum CatSewingIntersectionMode {
catSewingNoIntersect,
catSewingIntersect
}
Sewing Intersection mode.
The sewing operation parameter for specifying which algorithm is used to
perform sewing operation
Values:
catSewingNoIntersect
No intersection is computed to perform the operation.
catSewingIntersect
Intersection is computed to perform the operation
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatSplitSide_16913 ===
PartInterfaces CatSplitSideEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatSplitSide (Enumeration)
enum CatSplitSide {
catPositiveSide,
catNegativeSide
}
Split side.
The split operation parameter for specifying on which side
of the splitting element material in splitted element should be
removed.
Values:
catPositiveSide
Material in the splitted element should be removed in the direction
indicated by the splitting element normal vector. This vector is
oriented towards the outside of the material when a face is selected.
catNegativeSide
Material in the splitted element should be removed in the direction
opposite to the one indicated by the splitting element normal vector
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatThreadPolarity_24647 ===
PartInterfaces CatThreadPolarityEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatThreadPolarity (Enumeration)
enum CatThreadPolarity {
catThread,
catTap
}
Thread/Tap Polarity Management
It describes the thread polarity.
Values:
catThread
The thread/tap polarity is explicitly set to Thread
catTap
The thread/tap polarity is explicitly set to Tap
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatThreadSide_17946 ===
PartInterfaces CatThreadSideEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatThreadSide (Enumeration)
enum CatThreadSide {
catRightSide,
catLeftSide
}
Threading/Tapping side
It describes the side of thread/tap.
Values:
catRightSide
The Thread/tap is right-threaded
catLeftSide
The Thread/tap is left-threaded
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== enum_CatThreadStandard_24099 ===
PartInterfaces CatThreadStandardEnumeration
All Frameworks
Class Hierarchy
This Framework
Indexes
CatThreadStandard (Enumeration)
enum CatThreadStandard {
catMetricThinPitch,
catMetricThickPitch
}
Thread/Tap Standard
It describes the standard to be used for thread/tap.
Values:
catMetricThinPitch
The thread/tap standard is Metric Thin Pitch
catMetricThickPitch
The thread/tap standard is Metric Thick Pitch
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Add_13508 ===
PartInterfaces Add (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
Add (Object)
Represents the add, or union boolean operation.
It is performed between a body and the current shape.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Affinity_16337 ===
PartInterfaces Affinity (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
Affinity (Object)
Represents the hybrid shape Affinity feature object.
This solid feature is
created from an underlying HybridShapeAffinity aggregated by the Affinity.
Role: To access the data of the hybrid shape Affinity feature object.
This data includes:
The element to Affinity
Origin for the Affinity
Plane for the Affinity
Direction for the Affinity
XRatio Value for the Affinity
YRatio Value for the Affinity
ZRatio Value for the Affinity
The translation distance and its value
Use the CATIAHybridShapeFactory to create HybridShapeFeature object.
See also:
Property Index
HybridShape
Gets the underlying HybridShapeAffinity.
Properties
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeAffinity.
Example:
The following example explains how to retrieve the underlying HybridShape Affinity
Dim oHybridShape as AnyObject
Set oHybridShape=oAffinity.HybridShape
oHybridShape.ElemToAffinity = reference1
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AngularRepartition_29692 ===
PartInterfaces AngularRepartition (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
AngularRepartition (Object)
Represents the angular repartition.
It is used by the circular pattern.
It is made up of a number of times the shape is copied and of
an angular spacing between two consecutive copies
of the shape along a crown.
The number of times the shape is copied is accessible using
the  property.
See also:
Property Index
AngularSpacing
Returns the angle between two consecutive copies of a shape
along the repartition crown.
InstanceSpacing
Returns the angle at which the pattern spacing is done for unequal angular spacing mode.
Properties
Property AngularSpacing() As   (Read Only)
Returns the angle between two consecutive copies of a shape
along the repartition crown.
Example:
The following example returns in AngSpace1
the angular spacing of the
angular repartition firstRepartition:
Set AngSpace1 = firstRepartition.AngularSpacing
Property InstanceSpacing() As   (Read Only)
Returns the angle at which the pattern spacing is done for unequal angular spacing mode.
Example:
The following example returns in AngSpace1
the angular spacing of the
angular repartition firstRepartition:
Set AngSpace1 = firstRepartition.AngularSpacing
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Assemble_16137 ===
PartInterfaces Assemble (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
Assemble (Object)
Represents the assemble boolean operation.
It is performed between a body and the current shape.
An assemble operation adds material if the body is "positive"
and remove material if the body is "negative".
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AutoDraft_16956 ===
PartInterfaces AutoDraft (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
AutoDraft (Object)
Represents the AutoDraft shape.
Property Index
FunctionalFace
FunctionalFaces
Returns or sets the functional faces.
MainDraftAngle
Returns or sets the main draft angle.
Mode
Returns or sets the draft mode.
PartingElement
Returns or sets the parting element.
PullingDirection
Returns or sets the pulling direction.
Properties
Property FunctionalFace( iFace) (Write Only)
Property FunctionalFaces() As   (Read Only)
Returns or sets the functional faces.
Example:
The following example returns in FunctionalFaces the list
functional faces of the
AutoDraft AutoDraft,
and then sets NewFunctionalFace as a functional face:
Set FunctionalFaces = AutoDraft.FunctionalFace
AutoDraft.FunctionalFace = NewFunctionalFace
Property MainDraftAngle() As
Returns or sets the main draft angle.
Example:
The following example returns in MainDraftAngle the
main draft angle of the
AutoDraft AutoDraft,
and then sets it to NewMainDraftAngle.:
Set MainDraftAngle = AutoDraft.MainDraftAngle
AutoDraft.MainDraftAngle = NewMainDraftAngle
Property Mode() As
Returns or sets the draft mode.
Example:
The following example returns in Mode the
mode of the draft
AutoDraft AutoDraft,
and then sets it to NewMode:
Set Mode = AutoDraft.Mode
AutoDraft.Mode = NewMode
Property PartingElement() As
Returns or sets the parting element.
Example:
The following example returns in PartingElement the
parting element of the
AutoDraft AutoDraft,
and then sets it to NewpartingElement:
Set PartingElement = AutoDraft.PartingElement
AutoDraft.PartingElement = NewPartingElement
Property PullingDirection() As
Returns or sets the pulling direction.
Example:
The following example returns in PullingDirection the
pulling direction of the
AutoDraft AutoDraft,
and then sets it to NewPullingDirection.:
Set PullingDirection = AutoDraft.PullingDirection
AutoDraft.PullingDirection = NewPullingDirection
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AutoFillet_17951 ===
PartInterfaces AutoFillet (Object)
All Frameworks
Class Hierarchy
This Framework
Indexes
Previous
Next
AutoFillet (Object)
Represents the AutoFillet shape.
A AutoFillet fillets all the edges of Solid
Property Index
CurvatureRadius
Returns the Curvature radius.
FacesToFillet
Returns or sets the faces to fillet.
FacesToFillets
FilletRadius
Returns the Fillet radius.
FunctionalFace
FunctionalFaces
Returns or sets the functional face.
PartingElement
Returns or sets the parting element.
RoundRadius
Returns the Round radius.
RoundRadiusActivation
Returns the AutoFillet RoundRadiusActivation flag (for AutoFillet only).
SliversAndCrack
SliversAndCracks
Returns or sets the slivers face.
SupportSurface
Returns or sets the support surface.
Properties
Property CurvatureRadius() As   (Read Only)
Returns the Curvature radius.
Example:
The following example returns in Curvature radius the Curvature radius
of the AutoFillet Autofillet:
Set Curvatureradius = Autofillet.Radius
Property FacesToFillet() As   (Read Only)
Returns or sets the faces to fillet.
Example:
The following example returns in facestofillet the
faces required for
autofillet autoFillet,
and then sets it to NewFacestofillet:
Set Facestofillet = autoFillet.Facestofillet
autofillet.Facestofillet = NewFacestofillet
Property FacesToFillets( iFace) (Write Only)
Property FilletRadius() As   (Read Only)
Returns the Fillet radius.
Example:
The following example returns in fillet radius the fillet radius
of the AutoFillet Autofillet:
Set Filletradius = Autofillet.Radius
Property FunctionalFace( iFace) (Write Only)
Property FunctionalFaces() As   (Read Only)
Returns or sets the functional face.
Example:
The following example returns in functionalface the
functional face of the
autofillet autoFillet,
and then sets it to NewfunctionalFace:
Set functionalFace = autoFillet.FunctionalFace
autofillet.FunctionalFace = NewfunctionalFace
Property PartingElement() As
Returns or sets the parting element.
Example:
The following example returns in partingelement the
parting element of the
autofillet autoFillet,
and then sets it to Newparting element:
Set Parting element = autoFillet.PartingElement
autofillet.PartingElement = NewPartingElement
Property RoundRadius() As   (Read Only)
Returns the Round radius.
Example:
The following example returns in round radius the round radius
of the AutoFillet Autofillet:
Set roundradius = Autofillet.Radius
Property RoundRadiusActivation() As
Returns the AutoFillet RoundRadiusActivation flag (for AutoFillet only).
It returns 1 if RoundRadius is activated, 0 if not.
Returns:
oRoundRadActivation   The RoundRadActivation flag as an int
Example:
Property SliversAndCrack( iSlivers) (Write Only)
Property SliversAndCracks() As   (Read Only)
Returns or sets the slivers face.
Example:
The following example returns in slivers the
sliver face of the
autofillet autoFillet,
and then sets it to Newsliver:
Set sliversFace = autoFillet.SliversFace
autofillet.SliversFace = NewsliversFace
Property SupportSurface() As
Returns or sets the support surface.
Example:
The following example returns in SupportSurface the
support surface required for
autofillet autoFillet,
and then sets it to NewSupportSurface:
Set SupportSurface = autoFillet.SupportSurface
autofillet.SupportSurface = NewSupportSurface
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_AxisToAxis_17879 ===
PartInterfaces AxisToAxis (Object)
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AxisToAxis (Object)
Represents the hybrid shape AxisToAxis feature object.
This solid feature is
created from an underlying HybridShapeAxisToAxis aggregated by the AxisToAxis.
Role: To access the data of the hybrid shape AxisToAxis feature object.
This data includes:
The element to AxisToAxis
Origin for the AxisToAxis
Plane for the AxisToAxis
Direction for the AxisToAxis
XRatio Value for the AxisToAxis
YRatio Value for the AxisToAxis
ZRatio Value for the AxisToAxis
The translation distance and its value
Use the CATIAHybridShapeFactory to create HybridShapeFeature object.
See also:
Property Index
HybridShape
Gets the underlying HybridShapeAxisToAxis.
Properties
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeAxisToAxis.
Example:
The following example explains how to retrieve the underlying HybridShape AxisToAxis
Dim oHybridShape as AnyObject
Set oHybridShape=oAxisToAxis.HybridShape
oHybridShape.ElemToAxisToAxis = reference1
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_BooleanShape_19931 ===
PartInterfaces BooleanShape (Object)
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BooleanShape (Object)
Represents the shapes based on boolean operations on other shapes.
It is the base object for add, assemble, intersect, remove, and split shapes.
See also:
, , , , ,
Property Index
Body
Returns the inserted body.
Method Index
SetOperatedObject
Modifies the Second Operand.
SetOperatingVolume
Swaps the operands.
Properties
Property Body() As   (Read Only)
Returns the inserted body.
Methods
Sub SetOperatedObject( iReferenceObject)
Modifies the Second Operand.
input object to replace with Body or Volume
Sub SetOperatingVolume( iReferenceObject)
Swaps the operands. Both the Operands must be Volume.
This is available only for Volume Add and Volume UnionTrim Operations
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Chamfer_15430 ===
PartInterfaces Chamfer (Object)
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Chamfer (Object)
Represents the chamfer shape.
A chamfer is made up of a list of geometrical elements
to process, such as faces, and is defined using a couple of parameters,
such as two lengthes, or a length and an angle.
Property Index
Angle
Returns the chamfer angle.
ElementsToChamfer
Returns the collection of geometrical elements to be chamfered.
Length1
Returns the chamfer first length.
Length2
Returns the chamfer second length.
Mode
Returns or sets the chamfer definition mode.
Orientation
Returns or sets the chamfer orientation.
Propagation
Returns or sets the propagation mode of the geometrical elements
to be chamfered.
Method Index
AddElementToChamfer
Adds a new geometrical element to be chamfered.
WithdrawElementToChamfer
Withdraws a geometrical element from those to be chamfered.
Properties
Property Angle() As   (Read Only)
Returns the chamfer angle.
This is valid only if the chamfer is defined using a length and an angle,
that is if the chamfer definition mode
is set to catLengthAngleChamfer.
Example:
The following example returns in angle the angle of
the firstChamfer chamfer:
Set angle = firstChamfer.Angle
Property ElementsToChamfer() As   (Read Only)
Returns the collection of geometrical elements to be chamfered.
Example:
The following example returns in list the list of elements
of the firstChamfer chamfer:
Set list = firstChamfer.ElementsToChamfer
Property Length1() As   (Read Only)
Returns the chamfer first length.
This is the first length if the chamfer is defined by two lengthes,
or the chamfer if the chamfer is defined by a length and an angle.
Example:
The following example returns in length1 the first length of
the firstChamfer chamfer:
Set length1 = firstChamfer.Length1
Property Length2() As   (Read Only)
Returns the chamfer second length.
This is valid only if the chamfer is defined using two lengthes,
that is if the chamfer definition mode
is set to catTwoLengthChamfer.
Example:
The following example returns in length2 the second length
of the firstChamfer chamfer:
Set length2 = firstChamfer.Length2
Property Mode() As
Returns or sets the chamfer definition mode.
The chamfer definition mode enables the chamfer to be defined
using either two lengthes or a length and an angle.
Example:
The following example returns in mode how the parameters
of the firstChamfer chamfer are defined, and then sets it
to catTwoLengthChamfer:
Set mode = firstChamfer.Mode
firstChamfer.Mode = catTwoLengthChamfer
Property Orientation() As
Returns or sets the chamfer orientation.
Example:
The following example returns in orient the orientation mode
of the firstChamfer chamfer, and then sets it to
catReverseChamfer:
Set orient = firstChamfer.Orientation
firstChamfer.Orientation = catReverseChamfer
Property Propagation() As
Returns or sets the propagation mode of the geometrical elements
to be chamfered.
Example:
The following example returns in prop the propagation mode
of the firstChamfer chamfer, and then sets it to
catMinimalChamfer:
Set prop = firstChamfer.Propagation
firstChamfer.Propagation = catMinimalChamfer
Methods
Sub AddElementToChamfer( iElementToChamfer)
Adds a new geometrical element to be chamfered.
Parameters:
iElementToChamfer
The new element to be chamfered
The following
object is supported:
.
Example:
The following example adds the new element element
to be chamfered for the firstChamfer chamfer:
firstChamfer.AddElementToChamfer(element)
Sub WithdrawElementToChamfer( iElementToWithdraw)
Withdraws a geometrical element from those to be chamfered.
Parameters:
iElementToWithdraw
The existing element to withdraw
The following
object is supported:
.
Example:
The following example withdraws an existing element element
to be chamfered from the firstChamfer chamfer:
firstChamfer.WithdrawElementToChamfer(element)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_CircPattern_19085 ===
PartInterfaces CircPattern (Object)
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CircPattern (Object)
Represents the circular pattern.
The shape is duplicated along concentric circles to build crowns.
A linear repartition object defines the duplication along radial
directions, thus determining the number of crowns.
An angular repartition object defines the duplication on the crowns.
See also:
,
Property Index
AngularDirectionRow
Returns the position of the shape to be copied along the
angular direction.
AngularRepartition
Returns the angular repartition.
CircularPatternParameters
Returns or sets the circular pattern parameters required to define the pattern.
RadialAlignment
Returns or sets whether the copied shapes
should be rotated or radial aligned
with respect to the original one.
RadialDirectionRow
Returns the position of the shape to be copied along the
radial direction.
RadialRepartition
Returns the radial repartition.
RotationOrientation
Returns or sets whether the shapes are copied clockwise
on the crowns with respect to the rotation axis direction.
Method Index
GetRotationAxis
Returns the rotation axis.
GetRotationCenter
Returns the rotation center if the user defined it.
SetInstanceAngularSpacing
Sets the InstanceAngularSpacing.
SetRotationAxis
Sets the rotation axis.
SetRotationCenter
Sets the rotation center.
SetUnequalInstanceNumber
Sets the Instance Number.
SetUnequalStep
This method is deprecated
Sets the UnequalStep.
Properties
Property AngularDirectionRow() As   (Read Only)
Returns the position of the shape to be copied along the
angular direction.
Example:
The following example returns in AngularDirPos the
position of the shape to be copied along the angular direction.
Set AngularDirPos = firstPattern.AngularDirectionRow
Property AngularRepartition() As   (Read Only)
Returns the angular repartition.
The angular repartition is the repartition on a crown.
Example:
The following example returns in repartA
the angular repartition of the
circular pattern firstPattern:
Set repartA = firstPattern.AngularRepartition
Property CircularPatternParameters() As
Returns or sets the circular pattern parameters required to define the pattern.
These parameters are used when reading the CATIAAngularRepartition properties.
Example:
The following example returns in parameters the circular pattern parameters
of the firstPattern circular pattern,
and then sets it to catCompleteCrown,
so that only the number of instances is used to define the Pattern:
Set parameters = firstPattern.CircularPatternParameters
Set firstPattern.CircularPatternParameters = catCompleteCrown
Property RadialAlignment() As
Returns or sets whether the copied shapes
should be rotated or radial aligned
with respect to the original one.
True if the copied shapes are rotated.
Example:
The following example returns in alignedR
the radial alignment of the
circular pattern firstPattern,
and then sets it to False:
Set alignedR = firstPattern.RadialAlignment
firstPattern.RadialAlignment = False
Property RadialDirectionRow() As   (Read Only)
Returns the position of the shape to be copied along the
radial direction.
Example:
The following example returns in RadialDirPos the
position of the shape to be copied along the
radial direction.
Set RadialDirPos = firstPattern.RadialDirectionRow
Property RadialRepartition() As   (Read Only)
Returns the radial repartition.
The radial repartition is the repartition along a radius.
Example:
The following example returns in repartR
the radial repartition of the
circular pattern firstPattern:
Set repartR = firstPattern.RadialRepartition
Property RotationOrientation() As
Returns or sets whether the shapes are copied clockwise
on the crowns with respect to the rotation axis direction.
True if the shapes are copied counterclockwise
when the rotation axis direction goes towards you when
you look at the crown.
Example:
The following example returns in alignedAxis
whether the circular pattern firstPattern is built
clockwise, and then sets it to True:
alignedAxis = firstPattern.RotationOrientation
firstPattern.RotationOrientation = True
Methods
Sub GetRotationAxis( ioRotationAxis)
Returns the rotation axis.
The rotation axis is returned as an array containing
the rotation axis vector components.
Assume this array is oRotationAxis. It contains:
oRotationAxis[0],oRotationAxis[1],oRotationAxis[2]
The X, Y, and Z rotation axis vector components
Example:
The following example returns in axisArray the rotation axis
components of the circular pattern firstPattern:
Call firstPattern.GetRotationAxis(axisArray)
Set x = axisArray[0]
Set y = axisArray[1]
Set z = axisArray[2]
Sub GetRotationCenter( ioRotationCenter)
Returns the rotation center if the user defined it.
Returns E_FAIL if no rotation center has been defined
The rotation center is returned as an array containing
the rotation center coordinates.
Assume this array is oRotationCenter. It contains:
oRotationCenter[0],oRotationCenter[1],oRotationCenter[2]
The X, Y, and Z rotation center coordinates
Example:
The following example returns in centerArray
the rotation center
coordinates of the circular pattern firstPattern,
and saves them in variables:
Call firstPattern.GetRotationCenter(centerArray)
x = centerArray[0]
y = centerArray[1]
z = centerArray[2]
Sub SetInstanceAngularSpacing( iInstanceNumber, iAngularSpacing)
Sets the InstanceAngularSpacing.
Parameters:
iInstanceNumber
The Instance Number
iAngularSpacing
The Angular Spacing
Example:
The following example sets the InstanceAngularSpacing of the circular pattern
Sub SetRotationAxis( iRotationAxis)
Sets the rotation axis.
Parameters:
iRotationAxis
The rotation axis.
It is passed as reference and can
be valuated with a line, an edge or a plane reference: in this
case the plane normal is taken into account.
The following
objects are supported:
,
and
.
Example:
The following example sets the rotation axis of the circular pattern
firstPattern with the refLine1 reference:
firstPattern.SetRotationAxis refLine1
Sub SetRotationCenter( iRotationCenter)
Sets the rotation center.
Parameters:
iRotationCenter
The rotation center
Example:
The following example sets the rotation center of the circular pattern
firstPattern with point1Ref point:
firstPattern.SetRotationCenter point1Ref
Sub SetUnequalInstanceNumber( iInstanceNumber)
Sets the Instance Number.
Parameters:
iInstanceNumber
The Instance Number
Example:
The following example modifies the instance number for unequal angular spacing
Sub SetUnequalStep( iInstanceNumber)
This method is deprecated
Sets the UnequalStep.
Parameters:
iInstanceNumber
The Instance Number
Example:
The following example creates the number of pattern spacing objects in pattern object
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_CloseSurface_19992 ===
PartInterfaces CloseSurface (Object)
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CloseSurface (Object)
Represents the Close feature.
It Closes a skin .
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ConstRadEdgeFillet_28558 ===
PartInterfaces ConstRadEdgeFillet (Object)
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ConstRadEdgeFillet (Object)
Represents the edge fillet shape with a constant radius.
The resulting shape is made up of
edge fillets built with a constant radius.
Property Index
ObjectsToFillet
Returns the collection of reference elements to be filleted.
Radius
Returns the edge fillet constant radius.
Method Index
AddObjectToFillet
Adds a new sub-element to be filleted.
SwitchToVarFilletType
Changes the type of EdgeFillet to variable EdgeFillet and return it.
WithdrawObjectToFillet
Withdraws a sub-element from those to be filleted.
Properties
Property ObjectsToFillet() As   (Read Only)
Returns the collection of reference elements to be filleted.
Example:
The following example returns in elements
the reference elements to be filleted of the
constant radius edge fillet firstCstEdgeFillet:
Set elements = firstCstEdgeFillet.ObjectsToFillet
Property Radius() As   (Read Only)
Returns the edge fillet constant radius.
Example:
The following example returns in radius
the radius of the
constant radius edge fillet firstCstEdgeFillet:
Set radius = firstCstEdgeFillet.Radius
Methods
Sub AddObjectToFillet( iObjectToFillet)
Adds a new sub-element to be filleted.
This sub-element is usually an edge.
Parameters:
iObjectToFillet
The sub-element to be filleted
The following
object is supported:
.
Example:
The following example adds a new geometrical element
element
to be filleted by the constant radius edge fillet
firstCstEdgeFillet:
firstCstEdgeFillet.AddObjectToFillet(element)
Func SwitchToVarFilletType() As
Changes the type of EdgeFillet to variable EdgeFillet and return it.
Parameters:
opVarFillet
The opVarFillet is the variable edge fillet
Sub WithdrawObjectToFillet( iObjectToWithdraw)
Withdraws a sub-element from those to be filleted.
This sub-element is usually an edge.
Parameters:
iObjectToWithdraw
The sub-element to withdraw
The following
object is supported:
.
Example:
The following example withdraws the geometrical element
element from those to be
filleted by the constant radius edge fillet firstCstEdgeFillet:
firstCstEdgeFillet.WithdrawObjectToFillet(element)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Defeaturing_19144 ===
PartInterfaces Defeaturing (Object)
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Defeaturing (Object)
Represents the defeaturing.
Property Index
Filters
Returns the filter collection of the Defeaturing.
Properties
Property Filters() As   (Read Only)
Returns the filter collection of the Defeaturing.
The returned object is the filter collection associated to this Defeaturing object.
All changes applied to the returned collection will be automatically applied to the Defeaturing object.
As a consequence there is no need to affect the collection to the defeaturing after the change to update the property.
Returns:
oFilters   The filter collection (see
for list of possible actions)
Example:
The following example returns in myDefeaturingFiltersCollection the filter collection of the Defeaturing firstDefeaturing:
Set myDefeaturingFiltersCollection = firstDefeaturing.Filters
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DefeaturingFilletFilter_39542 ===
PartInterfaces DefeaturingFilletFilter (Object)
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DefeaturingFilletFilter (Object)
Represents the defeaturing fillet filter.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DefeaturingFilter_27541 ===
PartInterfaces DefeaturingFilter (Object)
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DefeaturingFilter (Object)
Represents the base object for defeaturing filters.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DefeaturingFilters_29496 ===
PartInterfaces DefeaturingFilters (Object)
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DefeaturingFilters (Object)
Represents the filter collection of a defeaturing object.
Method Index
Add
Creates a new filter and adds it to the Defeaturing filters collection.
Item
Returns the filter of the Defeaturing filters collection using its index or its name.
Remove
Removes a filter from the Defeaturing filters collection and deletes it, using its index or its name.
Methods
Func Add( iFilterTypeToAdd) As
Creates a new filter and adds it to the Defeaturing filters collection.
Parameters:
iFilterTypeToAdd
The type of the new filter to add among :
- "DefeaturingFilletFilter"
- "DefeaturingHoleFilter"
- or any user-defined filter's type
Returns:
oAddedFilterIndex   The added filter's index - equals to 0 if FAILED
Example:
The following example adds a new filter of type theFilterType to defeaturing colelction firstDefeaturingFilters and returns the index theIndex of the new filter
Set theIndex = firstDefeaturingFilters.Add(theFilterType)
Func Item( iFilterId) As
Returns the filter of the Defeaturing filters collection using its index or its name.
Parameters:
iFilterId
The index or the name of the filter to retrieve
As a numerics, must be in [1;Count])
Returns:
oFilter   The filter (see
for list of possible actions)
Example:
The following example returns in myFilter the filter number theIndex of Defeaturing collection firstDefeaturingFilters:
Set myFilter = firstDefeaturingFilters.Item(theIndex)
Sub Remove( iFilterId)
Removes a filter from the Defeaturing filters collection and deletes it, using its index or its name.
Parameters:
iFilterId
The index or the name of the filter to retrieve
As a numerics, must be in [1;Count])
Example:
The two following examples remove the filter number theIndex from Defeaturing collection firstDefeaturingFilters:
Call firstDefeaturingFilters.Remove(theIndex)
firstDefeaturingFilters.Remove theIndex
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DefeaturingFilterWithRange_46577 ===
PartInterfaces DefeaturingFilterWithRange (Object)
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DefeaturingFilterWithRange (Object)
Represents the base object for defeaturing filters which uses range(s) of values
Method Index
getMaximumActivity
getMaximumAngle
getMaximumLength
getMaximumValue
getMinimumActivity
Returns the minimum or maximum value activity of the filter for the given range id.
getMinimumAngle
getMinimumLength
getMinimumValue
Returns the minimum or maximum value of the filter for the given range id, if defined and active.
setMaximumActivity
setMaximumValue
setMinimumActivity
Sets the defeaturing minimum or maximum value activity of the filter for the given range id.
setMinimumValue
Sets the minimum or maximum value of the filter for the given range id.
Methods
Func getMaximumActivity( iRangeId) As
Func getMaximumAngle( iRangeId) As
Func getMaximumLength( iRangeId) As
Func getMaximumValue( iRangeId) As
Func getMinimumActivity( iRangeId) As
Returns the minimum or maximum value activity of the filter for the given range id.
Parameters:
iRangeId
The identificator of the range on which the minimum/maximum should be read
- if iRangeId is empty or equal to "Default", takes the default range as defined by the filter ("RibbonRadius" for FilletFilter, "MainDiameter" for HoleFilter)
- else iRangeId should be chosen among:
* {"RibbonRadius","RibbonAngle","RibbonLength"} for FilletFilter
* {"MainDiameter"} for HoleFilter
* any defined and supported range id in case of a user-defined filter
Returns:
oValue   The filter minimum/maximum activity for the specified range
Example:
The following example returns in theMinActivity the minimum value activity of filter myFilter for the range myRange:
Set theMinActivity = myFilter.getMinimumActivity(myRange)
Func getMinimumAngle( iRangeId) As
Func getMinimumLength( iRangeId) As
Func getMinimumValue( iRangeId) As
Returns the minimum or maximum value of the filter for the given range id, if defined and active.
Parameters:
iRangeId
The identificator of the range on which the minimum/maximum should be read
- if iRangeId is empty or equal to "Default", takes the default range as defined by the filter ("RibbonRadius" for FilletFilter, "MainDiameter" for HoleFilter)
- else iRangeId should be chosen among:
* {"RibbonRadius","RibbonAngle","RibbonLength"} for FilletFilter
* {"MainDiameter"} for HoleFilter
* any defined and supported range id in case of a user-defined filter
Returns:
oValue   The filter minimum/maximum value for the specified range if defined and active
ELSE the method FAILS (to avoid this, getMinimumValueActivity/getMaximumValueActivity can be called prior to calling getMinimumValue/getMaximumValue)
Signature with double works for angles as well as for lengthes / EXPRESSED in MODEL UNIT (mm/deg)
Signatures with CATIALength or CATIAAngle must be used with care and will fail if the range nature and the expected type are incompatible
Example:
The following example returns in theMinValue the minimum value of filter myFilter for the range myRange:
theMinValue = myFilter.getMinimumValue(myRange)
The following example returns in theMinAngle the minimum value as an angle of filter myFilter for the range myRange:
Set theMinAngle = myFilter.getMinimumAngle(myRange)
The following example returns in theMaxLength the maximum value as a length of filter myFilter for the range myRange:
Set theMaxLength = myFilter.getMaximumLength(myRange)
Sub setMaximumActivity( iRangeId, iValue)
Sub setMaximumValue( iRangeId, iValue)
Sub setMinimumActivity( iRangeId, iValue)
Sets the defeaturing minimum or maximum value activity of the filter for the given range id.
Parameters:
iRangeId
The identificator of the range on which the minimum/maximum should be read
- if iRangeId is empty or equal to "Default", takes the default range as defined by the filter ("RibbonRadius" for FilletFilter, "MainDiameter" for HoleFilter)
- else iRangeId should be chosen among:
* {"RibbonRadius","RibbonAngle","RibbonLength"} for FilletFilter
* {"MainDiameter"} for HoleFilter
* any defined and supported range id in case of a user-defined filter
iValue
The filter minimum/maximum activity for the specified range
Example:
The two following examples set theMaxActivity as the maximum value activity of filter myFilter for the range myRange:
Call myFilter.setMaximumActivity(myRange,theMaxActivity)
myFilter.setMaximumActivity myRange theMaxActivity
Sub setMinimumValue( iRangeId, iValue)
Sets the minimum or maximum value of the filter for the given range id.
Forces the activation of the minimum or maximum value if not the case yet.
Parameters:
iRangeId
The identificator of the range on which the minimum/maximum should be read
- if iRangeId is empty or equal to "Default", takes the default range as defined by the filter ("RibbonRadius" for FilletFilter, "MainDiameter" for HoleFilter)
- else iRangeId should be chosen among:
* {"RibbonRadius","RibbonAngle","RibbonLength"} for FilletFilter
* {"MainDiameter"} for HoleFilter
* any defined and supported range id in case of a user-defined filter
iValue
The filter minimum/maximum value for the specified range / MUST BE EXPRESSED in MODEL UNIT (mm/deg)
iValue must be consistent with the other value if defined and active
- new minimum iValue must be smaller than existing active maximum value if any
- new maximum iValue must be larger than existing active minimum value if any
ELSE the method FAILS
Example:
The two following examples set theMaxValue as the maximum value of filter myFilter for the range myRange:
Call myFilter.setMaximumValue(myRange,theMaxValue)
myFilter.setMaximumValue myRange theMaxValue
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DefeaturingHoleFilter_34939 ===
PartInterfaces DefeaturingHoleFilter (Object)
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DefeaturingHoleFilter (Object)
Represents the defeaturing hole filter.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Draft_14286 ===
PartInterfaces Draft (Object)
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Draft (Object)
Represents the draft shape.
A draft shape is made up of draft domains (at least one)
and of a parting element.
Property Index
DraftDomains
Returns the collection of draft domains.
Mode
Returns or sets the draft mode.
PartingElement
Returns or sets the draft parting element.
Properties
Property DraftDomains() As   (Read Only)
Returns the collection of draft domains.
Example:
The following example returns in list the collection of
draft domains of the firstDraft draft:
Set list = firstDraft.DraftDomains
Property Mode() As
Returns or sets the draft mode.
Example:
The following example returns in mode the draft mode of
the firstDraft draft, and then sets it
to CatReflectKeepFaceDraftMode:
Set mode = firstDraft.Mode
Set firstDraft.Mode = CatReflectKeepFaceDraftMode
Property PartingElement() As
Returns or sets the draft parting element.
To set the property, you can use the following
object:
.
Example:
The following example returns in element
the parting element of the firstDraft draft, and then sets
it to the element2 geometrical element:
Set element = firstDraft.PartingElement
Set firstDraft.PartingElement = element2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DraftDomain_18876 ===
PartInterfaces DraftDomain (Object)
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DraftDomain (Object)
Represents the draft domain.
A draft domain is a basic object used by a draft shape.
It contains objects such as an angle, a pulling direction,
and a collection of faces to be drafted.
Property Index
DraftAngle
Returns the draft angle.
FacesToDraft
Returns the faces to be drafted.
MultiselectionMode
Changes the multiselection mode.
NeutralElement
Returns or sets the draft neutral element.
NeutralPropagationMode
Returns or sets the neutral element propagation mode.
PullingDirectionElement
Returns or sets the draft pulling direction element.
Method Index
AddFaceToDraft
Adds a face to those to be drafted.
GetPullingDirection
Returns the draft pulling direction.
RemoveFaceToDraft
Removes a face from those to be drafted.
SetPullingDirection
Sets the draft pulling direction.
SetVolumeSupport
Value the support of draft.
Properties
Property DraftAngle() As   (Read Only)
Returns the draft angle.
Example:
The following example returns in angle
the draft angle of the draft domain firstDraftDomain:
Set angle = firstDraftDomain.DraftAngle
Property FacesToDraft() As   (Read Only)
Returns the faces to be drafted.
They are returned as a collection of reference geometric elements.
Example:
The following example returns the collection of faces to be drafted
of the draft domain firstDraftDomain in list:
Set list = firstDraftDomain.FacesToDraft
Property MultiselectionMode() As
Changes the multiselection mode.
Parameters:
iMultiselectionMode.
The elements to be drafted can be selected explicitly (CATNoneDraftMultiselectionMode)
or can implicitly selected as neighbors of the neutral face (CATMultiselectionByNeutralMode)
Example:
The following example returns in MultiselMode
the multiselection mode of the
draft domain firstDraftDomain, and then sets it to
CATMultiselectionByNeutralMode
Set MultiselMode = firstDraftDomain.MultiselectionMode
firstDraftDomain.MultiselectionMode = CATMultiselectionByNeutralMode
Property NeutralElement() As
Returns or sets the draft neutral element.
To set the property, you can use the following
object:
.
Example:
The following example returns in neutral
the neutral element of the draft domain firstDraftDomain,
and then sets it to newNeutral:
Set neutral = firstDraftDomain.NeutralElement
firstDraftDomain.NeutralElement = newNeutral
Property NeutralPropagationMode() As
Returns or sets the neutral element propagation mode.
This mode is used when computing the needed neutral elements.
Example:
The following example returns in propMode
the neutral propagation mode of the
draft domain firstDraftDomain, and then sets it to
CATSmoothDraftNeutralPropagationMode so that
the neutral propagation will now be smooth:
Set propMode = firstDraftDomain.NeutralPropagationMode
firstDraftDomain.NeutralPropagationMode = CATSmoothDraftNeutralPropagationMode
Property PullingDirectionElement() As
Returns or sets the draft pulling direction element.
To set the property, you can use one of the following
objects:
or
.
Example:
The following example returns in pullingdirection
the pulling direction element of the draft domain firstDraftDomain,
and then sets it to newPullingDirection:
Set pullingdirection = firstDraftDomain.NeutralElement
firstDraftDomain.PullingDirectionElement = newPullingDirection
Methods
Sub AddFaceToDraft( iFace)
Adds a face to those to be drafted.
Parameters:
iFace
The face to add to those to be drafted
The following
object is supported:  ScFace.
Example:
The following example adds the face NewFaceToDraft
to the draft domain CurrentDraftDomain:
CurrentDraftDomain.AddFaceToDraft(NewFaceToDraft)
Sub GetPullingDirection( ioPullingDirection)
Returns the draft pulling direction.
The pulling direction is returned as an array containing
the pulling direction vector components.
Assume this array is PullDir. It contains:
PullDir[0],PullDir[1],PullDir[2]
The X, Y, and Z pulling direction vector components
Example:
The following example returns in PullDir
the pulling direction vector components of the
draft domain firstDraftDomain:
Set PullDir = firstDraftDomain.PullingDirection
Set x = PullDir[0]
Set y = PullDir[1]
Set z = PullDir[2]
Sub RemoveFaceToDraft( iFace)
Removes a face from those to be drafted.
Parameters:
iFace
The face to be removed from those to be drafted
The following
object is supported:
.
Example:
The following example removes the face FaceToRemove
from the draft domain CurrentDraftDomain:
CurrentDraftDomain.RemoveFaceToDraft(FaceToRemove)
Sub SetPullingDirection( iX, iY, iZ)
Sets the draft pulling direction.
Parameters:
iX,iY,iZ
The X, Y, and Z pulling direction vector components
Example:
The following example sets the draft pulling direction of
the draft domain firstDraftDomain to the direction
with the vector components 10, -5, 10:
firstDraftDomain.PullingDirection 10, -5, 10
Sub SetVolumeSupport( iVolumeSupport)
Value the support of draft.
Parameters:
iVolumeSupport
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DraftDomains_20141 ===
PartInterfaces DraftDomains (Object)
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DraftDomains (Object)
The collection of draft domains used by the draft shape.
Method Index
Item
Returns a draft domain using its index or its name from the
DraftDomains collection.
Methods
Func Item( iIndex) As
Returns a draft domain using its index or its name from the
DraftDomains collection.
Parameters:
iIndex
The index or the name of the draft domain to retrieve from
the collection of draft domains.
As a numerics, this index is the rank of the draft domain
in the collection.
The index of the first draft domain in the collection is 1, and
the index of the last draft domain is Count.
As a string, it is the name you assigned to the draft domain using
the
property.
Returns:
The retrieved draft domain
Example:
The following example returns in domain the third
draft domain of the firstDraftDomains collection:
Set domain = firstDraftDomains.Item(3)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_DressUpShape_19943 ===
PartInterfaces DressUpShape (Object)
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DressUpShape (Object)
Represents the shapes built with other shape sub-elements such as
faces or  edges.
It is the base object for chamfers, drafts, fillets, scalings, shells,
and thickness objects.
See also:
, , , , ,
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_EdgeFillet_17878 ===
PartInterfaces EdgeFillet (Object)
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EdgeFillet (Object)
Represents the edges-based fillet shape.
It is the base object for constant radius edge fillets and
variable radius edge fillets.
See also:
,
Property Index
EdgePropagation
Returns or sets the edge fillet propagation mode.
EdgesToKeep
Returns the collection of edges to keep by the edge fillet.
Method Index
AddEdgeToKeep
Adds a new edge to keep by the filleting operation.
WithdrawEdgeToKeep
Withdraws an edge from those kept by a filleting operation.
Properties
Property EdgePropagation() As
Returns or sets the edge fillet propagation mode.
This propagation mode is used when computing the edges to be filleted.
Example:
The following example returns in mode the edge fillet
propagation mode of the firstEdgeFillet edge fillet,
and then sets it to CATMinimalFilletEdgePropagation,
so that a minimum numbers of edges will be filleted:
Set mode = firstEdgeFillet.EdgePropagation
Set firstEdgeFillet.EdgePropagation = CATMinimalFilletEdgePropagation
Property EdgesToKeep() As   (Read Only)
Returns the collection of edges to keep by the edge fillet.
Example:
The following example returns in edges
the edges to keep of the
constant radius edge fillet firstCstEdgeFillet:
Set edges = firstCstEdgeFillet.EdgesToKeep
Methods
Sub AddEdgeToKeep( iEdgeToKeep)
Adds a new edge to keep by the filleting operation.
The edge to keep is not modified by the fillet.
Parameters:
iEdgeToKeep
The edge to keep by the filleting operation
The following
object is supported:
.
Example:
The following example adds the new edge edge
to be kept from filleting by the constant radius edge fillet
firstCstEdgeFillet:
firstCstEdgeFillet.AddEdgeToKeep(edge)
Sub WithdrawEdgeToKeep( iEdgeToWithdraw)
Withdraws an edge from those kept by a filleting operation.
Parameters:
iEdgeToWithdraw
The edge to withdraw
The following
object is supported:
.
Example:
The following example withdraws the edge edge
from those kept from filleting by the constant radius edge fillet
firstCstEdgeFillet:
firstCstEdgeFillet.WithdrawEdgeToKeep(edge)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_FaceFillet_17867 ===
PartInterfaces FaceFillet (Object)
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FaceFillet (Object)
Represents the face fillet shape.
A face fillet shape is built between two faces with a fillet radius.
Property Index
FirstFace
Returns or sets the first limiting face.
Radius
Returns the face fillet radius.
SecondFace
Returns or sets the second limiting face.
Properties
Property FirstFace() As
Returns or sets the first limiting face.
To set the property, you can use the following
object:
.
Example:
The following example returns in face1 the first
limiting face of the
face fillet firstFaceFillet,
and then sets it to NewFace1:
Set face1 = firstFaceFillet.FirstFace
firstFaceFillet.FirstFace = NewFace1
Property Radius() As   (Read Only)
Returns the face fillet radius.
Example:
The following example returns in radius the fillet radius
of the face fillet firstFaceFillet:
Set radius = firstFaceFillet.Radius
Property SecondFace() As
Returns or sets the second limiting face.
To set the property, you can use the following
object:
.
Example:
The following example returns in face2 the second
limiting face of the
face fillet firstFaceFillet,
and then sets it to NewFace2:
Set face2 = firstFaceFillet.SecondFace
firstFaceFillet.SecondFace = NewFace2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Fillet_14837 ===
PartInterfaces Fillet (Object)
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Fillet (Object)
Represents the fillet shape.
It is the base object for face fillets and edge fillets.
See also:
,
Property Index
FilletBoundaryRelimitation
Returns or sets the fillet boundary relimitation mode.
FilletTrimSupport
Returns or sets the fillet Trim Support mode.
Properties
Property FilletBoundaryRelimitation() As
Returns or sets the fillet boundary relimitation mode.
This boundary relimitation mode is used when computing the fillet.
Example:
The following example returns in mode the fillet
boundary relimitation mode of the firstFillet fillet,
and then sets it to catMinimumFilletBoundaryRelimitation,
so that the fillet expands up to the limits of the smallest shell:
Set mode = firstFillet.FilletBoundaryRelimitation
Set FirstFillet.FilletBoundaryRelimitation = catMinimumFilletBoundaryRelimitation
Property FilletTrimSupport() As
Returns or sets the fillet Trim Support mode.
This Trim Support mode is used when computing the fillet.
Example:
The following example returns in mode the fillet
Trim Support mode of the firstFillet fillet,
and then sets it to catMinimumFilletTrimSupport,
so that the fillet expands up to the limits of the smallest shell:
Set mode = firstFillet.FilletTrimSupport
Set FirstFillet.FilletTrimSupport = catNoTrimFilletSupport
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Groove_14854 ===
PartInterfaces Groove (Object)
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Groove (Object)
Represents the groove shape.
A groove is made up of a sketch, used as the groove profile, containing
an axis, used as the revolution axis, and two limiting angles around
this axis.
This is a "negative" shape: it removes material from the body it
belongs to.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Hole_13838 ===
PartInterfaces Hole (Object)
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Hole (Object)
Hole Feature in Part Design.
Property Index
AnchorMode
Returns the hole anchor mode.
BottomAngle
Returns the hole bottom angle.
BottomLimit
Returns the bottom limit.
BottomType
Returns the hole bottom type.
CounterDrilledMode
Returns the mode of a counterdrilled hole .
CounterSunkMode
Returns the mode of a countersunk hole .
Diameter
Returns the hole diameter.
HeadAngle
Returns the hole head angle.
HeadDepth
Returns the hole head depth.
HeadDiameter
Returns the hole head diameter.
HoleThreadDescription
Returns the hole thread description parameter.
ThreadDepth
Returns the hole thread depth.
ThreadDiameter
Returns the hole thread diameter.
ThreadPitch
Returns the hole thread pitch.
ThreadSide
Returns the hole thread side.
ThreadingMode
Returns the hole threading mode.
Type
Returns the hole type.
Method Index
CreateStandardThreadDesignTable
Creates a Standard Thread design table .
CreateUserStandardDesignTable
Creates a UserStandard Thread design table .
GetDirection
Returns the hole direction with absolute coordinates.
GetOrigin
Returns the origin point which the hole is anchored to.
Reverse
Reverses the hole direction .
SetDirection
Sets the hole associative direction.
SetOrigin
Sets the origin point which the hole is anchored to.
Properties
Property AnchorMode() As
Returns the hole anchor mode.
This information is pertinent when hole type is Counterbored or Counterdrilled only.
Returns:
oMode   The hole anchor mode (see
for list of possible types)
Example:
The following example returns in holeAnchorMode the anchor mode of
hole firstHole:
Set holeAnchorMode = firstHole.AnchorMode
Property BottomAngle() As   (Read Only)
Returns the hole bottom angle.
This call is valid when the hole bottom type is : VBottom.
Returns:
oBottomAngle    An Angle object controlling the hole bottom angle  (see
for more information)
Example:
The following example returns in holeBottomAngle the bottom angle of
hole firstHole:
Set holeBottomAngle = firstHole.BottomAngle
Property BottomLimit() As   (Read Only)
Returns the bottom limit.
This call is valid when the hole bottom type is : BlindHole or ThruHole.
Returns:
oBottomLimit    A Limit object controlling the hole bottom limit (see
for more information)
Example:
The following example returns in holeBottomLimit the bottom limit of
hole firstHole:
Set holeBottomLimit = firstHole.BottomLimit
Property BottomType() As
Returns the hole bottom type.
Returns:
oBottomType   The hole bottom type (see
for list of possible types)
Example:
The following example returns in holeBottomType the bottom type of
hole firstHole:
Set holeBottomType = firstHole.BottomType
Property CounterDrilledMode() As
Returns the mode of a counterdrilled hole .
Returns:
CDMode    Value of the counterdrilled mode (see
for list of possible types)
Example:
The following example returns in CDMode the CDMode of
hole firsthole:
Set CDMode = firsthole.CounterDrilledMode
Property CounterSunkMode() As
Returns the mode of a countersunk hole .
Returns:
CSMode    Value of the countersunk mode (see
for list of possible types)
Example:
The following example returns in CSMode the CSMode of
hole firsthole:
Set CSMode = firsthole.CounterSunkMode
Property Diameter() As   (Read Only)
Returns the hole diameter.
Returns:
oDiameter    A Length object controlling the hole diameter (see
for more information)
Example:
The following example returns in holeDiam the diameter of
hole firstHole:
Set holeDiam = firstHole.Diameter
Property HeadAngle() As   (Read Only)
Returns the hole head angle.
This call is valid when the hole type is : Tapered or Counterdrilled or Countersunk.
Returns:
oHeadAngle    An Angle object controlling the hole head angle (see
for more information)
Example:
The following example returns in holeHeadAngle the head angle of
hole firstHole:
Set holeHeadAngle = firstHole.HeadAngle
Property HeadDepth() As   (Read Only)
Returns the hole head depth.
This call is valid when the hole type is : Counterbored or Counterdrilled or Countersunk.
Returns:
oHeadDepth    A Length object controlling the hole head depth (see
for more information)
Example:
The following example returns in holeHeadDepth the head depth of
hole firstHole:
Set holeHeadDepth = firstHole.HeadDepth
Property HeadDiameter() As   (Read Only)
Returns the hole head diameter.
This call is valid when the hole type is : Counterbored or Counterdrilled or Countersunk.
Returns:
oHeadDiameter    A Length object controlling the hole head diameter (see
for more information)
Example:
The following example returns in holeHeadDiam the head diameter of
hole firstHole:
Set holeHeadDiam = firstHole.HeadDiameter
Property HoleThreadDescription() As   (Read Only)
Returns the hole thread description parameter.
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
This call is valid only when a standard/user design table exists
Returns:
oThreadDescParam    A Parameter object controlling the hole thread description (see
for more information)
Example:
The following example returns in holeThreadDescription the thread description (M12 etc) of
hole firstHole:
Set holeThreadDescription = firstHole.HoleThreadDescription
Property ThreadDepth() As   (Read Only)
Returns the hole thread depth.
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
Returns:
oThreadDepth    A Length object controlling the hole thread depth (see
for more information)
Example:
The following example returns in holeThreadDepth the thread depth of
hole firstHole:
Set holeThreadDepth = firstHole.ThreadDepth
Property ThreadDiameter() As   (Read Only)
Returns the hole thread diameter.
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
Returns:
oThreadDiameter    A Length object controlling the hole thread diameter (see
for more information)
Example:
The following example returns in holeThreadDiameter the thread diameter of
hole firstHole:
Set holeThreadDiameter = firstHole.ThreadDiameter
Property ThreadPitch() As   (Read Only)
Returns the hole thread pitch.
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
Returns:
oThreadPitch    A Length object controlling the hole thread pitch (see
for more information)
Example:
The following example returns in holeThreadPitch the thread pitch of
hole firstHole:
Set holeThreadPitch = firstHole.ThreadPitch
Property ThreadSide() As
Returns the hole thread side.
Returns:
oThreadSide   The hole thread side (see
for list of possible sides)
Example:
The following example returns in holeThreadSide the thread side of
hole firstHole:
Set holeThreadSide = firstHole.ThreadSide
Property ThreadingMode() As
Returns the hole threading mode.
Returns:
oThreadingMode   The hole threading mode (see
for list of possible types)
Example:
The following example returns in holeThreadingMode the threading mode of
hole firstHole:
Set holeThreadingMode = firstHole.ThreadingMode
Property Type() As
Returns the hole type.
Returns:
oType   The hole type (see
for list of possible types)
Example:
The following example returns in holeType the type of
hole firstHole:
Set holeType = firstHole.Type
Methods
Sub CreateStandardThreadDesignTable( iStandardType)
Creates a Standard Thread design table .
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
Parameters:
iStandardType
Standard type for thread (see
for list of possible types)
Example:
The following example creates a standard table for MetricThinPitch for
hole firstHole:
firstHole.CreateStandardThreadDesignTable catHoleMetricThinPitch
Sub CreateUserStandardDesignTable( iStandardName, iPath)
Creates a UserStandard Thread design table .
This call is valid when the hole threading mode is : CATThreadedHoleThreading.
Parameters:
iStandardName
Name of the UserStandard thread. iStandardName should be empty if filepath is to be defined.
iPath
Path of the UserStandard file. iPath is empty if the filepath is already defined through CATReffilesPath.
Example1:
The following example creates a standard table for UserStandard for
hole firstHole. The file path is already defined thru CATReffilesPath:
firstHole.CreateUserStandardDesignTable "UserStandard",""
Example2:
The following example creates a standard table for UserStandard for
hole firstHole when file path is not defined thru CATReffilesPath:
firstHole.CreateUserStandardDesignTable "","E:\user\standard\UserStandard.txt"
Sub GetDirection( ioDirection)
Returns the hole direction with absolute coordinates.
It provides a safe array with 3 elements : X, Y, Z direction coordinates
Returns:
oDirection   The direction coordinates
Example:
The following example returns in dirArray the direction coordinates
of hole firstHole:
Call firstHole.GetDirection dirArray
Set x = dirArray[1]
Set y = dirArray[2]
Set z = dirArray[3]
Sub GetOrigin( ioOrigin)
Returns the origin point which the hole is anchored to.
This point belongs to a tangent plane.
Returns:
oOrigin   A Safe Array made up of 3 doubles : X, Y, Z - Hole origin point coordinates
Example:
The following example returns in coordArray the coordinates of
hole firstHole:
Call firstHole.GetOrigin coordArray
Set x = coordArray[1]
Set y = coordArray[2]
Set z = coordArray[3]
Sub Reverse()
Reverses the hole direction .
Example:
The following example reverses the current direction of
hole firstHole:
firstHole.Reverse()
Sub SetDirection( iDirection)
Sets the hole associative direction.
Parameters:
iDirection
A Reference object to an edge or a line (see
for more information)
The following
objects are supported:
,
and
.
Example:
The following example sets the support direction of
hole firstHole with holeDirRef direction reference :
firstHole.SetDirection holeDirref
Sub SetOrigin( iX, iY, iZ)
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
Parameters:
iX
Origin point x absolute coordinate
iY
Origin point y absolute coordinate
iZ
Origin point z absolute coordinate
Example:
The following example sets the coordinates of
hole firstHole to 10., 20., -5. :
firstHole.SetOrigin 10., 20., 5.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Intersect_17111 ===
PartInterfaces Intersect (Object)
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Intersect (Object)
Represents the intersect boolean operation.
It is performed between a body and the current shape.
Example
The following example shows how to create a
new shape by intersecting two existing pads Pad1 and Pad2,
created in two different bodies Body1 and Body2
respectively,
using the existing shape factory named shapeFactory.
' Make Pad1 the current shape
CATIA.ActiveDocument.Part.CurrentShape = Pad1
'
' Create the intersection between Pad1 and Body2
Set NewShape      = shapeFactory.AddNewIntersect(Body2)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Limit_14310 ===
PartInterfaces Limit (Object)
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Limit (Object)
Represents the limit of a prism or a hole shape.
See also:
,
Property Index
Dimension
Returns or sets the limit dimension.
LimitMode
Returns or sets the limit mode.
LimitingElement
Returns or sets the limiting element.
Properties
Property Dimension() As   (Read Only)
Returns or sets the limit dimension.
This property is valid for the offset limit mode only,
that is when
is set to catOffsetLimit .
Property LimitMode() As
Returns or sets the limit mode.
Property LimitingElement() As
Returns or sets the limiting element.
This property is valid when the limiting object is a surface or a plane,
that is when
is set to catUpToSurfaceLimit and catUpToPlaneLimit.
To set the property, you can use the following
object:
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_LinearRepartition_27841 ===
PartInterfaces LinearRepartition (Object)
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LinearRepartition (Object)
Represents the linear repartition.
It is used by the rectangular and circular patterns.
It is made up of a number of times the shape is copied
and of a spacing distance between two consecutive copies of this
shape along a direction.
The number of times the shape is copied is accessible using
the  property.
See also:
,
Property Index
Spacing
Returns the distance between two consecutive shapes
along the repartition direction.
Properties
Property Spacing() As   (Read Only)
Returns the distance between two consecutive shapes
along the repartition direction.
Example:
The following example returns in space1
the spacing distance of the
linear repartition firstRepartition:
Set space1 = firstRepartition.Spacing
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Loft_13871 ===
PartInterfaces Loft (Object)
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Loft (Object)
Loft feature.
Manipulation of solid Loft feature.
Allows to access data of the Loft feature created by the CATIAShapeFactory.
This solid feature is created from an underlying
HybridShapeLoft aggregated by the Loft.
See also:
Property Index
HybridShape
Gets the underlying HybridShapeLoft.
Properties
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeLoft.
Example:
The following example explains how to retrieve the underlying HybridShape Loft
Dim oHybridShape as AnyObject
Set oHybridShape=oLoft.HybridShape
oHybridShape.SectionCoupling = 2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Mirror_14897 ===
PartInterfaces Mirror (Object)
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Mirror (Object)
Represents the mirror shape.
It duplicates a shape with respect
to a planar mirroring element, such as a planar face or a plane.
Property Index
MirroringObject
Returns the mirroring Object.
MirroringPlane
Returns or sets the mirroring reference plane.
Properties
Property MirroringObject() As   (Read Only)
Returns the mirroring Object.
Property MirroringPlane() As
Returns or sets the mirroring reference plane.
It can be a plane, or a plane face.
To set the property, you can use the following
object:
.
Example:
The following example returns in ref the mirroring
reference plane of the mirroring firstMirroring,
and then sets it to the created MyRef:
Set ref = firstMirroring.MirroringPlane
Set MyRef = part.CreateReferenceFromGeometry (plane)
firstMirroring.MirroringPlane = MyRef
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Pad_13505 ===
PartInterfaces Pad (Object)
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Pad (Object)
Represents the pad shape.
A pad is created by extruding a profile represented by a sketch
in one or two opposite directions.
It is a "positive" shape: it adds material to the body it belongs to.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Pattern_15519 ===
PartInterfaces Pattern (Object)
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Pattern (Object)
Represents the pattern shape.
It is the base object for rectangular and circular patterns.
A pattern shape is a set of copies of the same shape.
The copy is done according to linear and angular repartitions.
See also:
, , , ,
Property Index
ItemToCopy
Returns or sets the shape to be copied.
RotationAngle
Returns the pattern global rotation angle.
Method Index
ActivatePosition
Allows user to activate an instance of the pattern.
DesactivatePosition
Allows user to desactivate an instance of the pattern.
Properties
Property ItemToCopy() As
Returns or sets the shape to be copied.
Example:
The following example returns in shape the copied shape
of the pattern firstPattern, and then sets it to pad1:
Set shape = firstPattern.ItemToCopy
firstPattern.ItemToCopy = pad1
Property RotationAngle() As   (Read Only)
Returns the pattern global rotation angle.
The rotation is applied to the whole pattern, but not to the shapes
themselves.
The shape to be copied is used as the rotation center.
Example:
The following example returns in globAng the rotation of
pattern firstPattern:
Set globAng = firstPattern.RotationAngle
Methods
Sub ActivatePosition( iPosU, iPosV)
Allows user to activate an instance of the pattern.
Parameters:
iPosU
The position of the instance in the U direction
iPosV
The position of the instance in the V direction
Sub DesactivatePosition( iPosU, iPosV)
Allows user to desactivate an instance of the pattern.
Parameters:
iPosU
The position of the instance in the U direction
iPosV
The position of the instance in the V direction
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Pocket_14822 ===
PartInterfaces Pocket (Object)
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Pocket (Object)
Represents the pocket shape.
A pocket is created by extruding a profile represented by a sketch
in one or two opposite directions.
It is a "negative" shape: it removes material from the body it
belongs to.
The sketch is usually drawn on another shape face.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Prism_14313 ===
PartInterfaces Prism (Object)
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Prism (Object)
Prism-based features in Part Design : base for pad or pocket.
Property Index
DirectionOrientation
Returns the prism direction orientation.
DirectionType
Returns the prism direction type.
FirstLimit
Returns the first prism limit (one of the two).
IsSymmetric
Returns the prism symmetry flag.
IsThin
Returns the prism thin flag.
MergeEnd
Returns the prism merge end flag (for thin prism only).
NeutralFiber
Returns the prism neutral fiber flag (for thin prism only).
SecondLimit
Returns the second prism limit (one of the two).
Method Index
GetDirection
Returns the prism direction with absolute coordinates.
ReverseInnerSide
Reverses the prism inner side when the profile is open.
SetDirection
Sets the prism associative direction.
Properties
Property DirectionOrientation() As
Returns the prism direction orientation.
Returns:
oOrientation   The direction orientation (see
for list of possible types)
Example:
The following example saves in dirOrientation the direction orientation of
prism firstPrism, and then sets it so that the direction will be now inversed :
Set dirOrientation = firstPrism.DirectionOrientation
firstPrism.DirectionOrientation = catInverseOrientation
Property DirectionType() As
Returns the prism direction type.
Returns:
oDirType   The direction type (see
for list of possible types)
Example:
The following example saves in dirType the direction type of
prism firstPrism, and then sets it so that the direction
will be now normal to the sketch :
Set dirType = firstPrism.DirectionType
firstPrism.DirectionType = catNormalToSketchDirection
Property FirstLimit() As   (Read Only)
Returns the first prism limit (one of the two).
This limit manages the way the prism is ended.
Returns:
oFirstLimit   The first limit (see
for more information)
Example:
The following example returns in firstLimit the first limit of
prism firstPrism:
Set firstLimit = firstPrism.FirstLimit
Property IsSymmetric() As
Returns the prism symmetry flag.
It returns TRUE if the prism is symmetric (from the base sketch), FALSE if not.
Returns:
oIsSymmetric   The symmetry flag as a boolean
Example:
The following example saves in symFlag the symmetry flag of
prism firstPrism, and then sets it so that it will be now symmetric (from the base sketch) :
Set symFlag = firstPrism.IsSymmetric
firstPrism.IsSymmetric = TRUE
Property IsThin() As
Returns the prism thin flag.
It returns TRUE if the prism is a thin prism , FALSE if not.
Returns:
oIsThin   The thin flag as a boolean
Example:
The following example saves in thinFlag the thin flag of
prism firstPrism, and then sets it so that it will be now thin :
Set thinFlag = firstPrism.IsThin
firstPrism.IsThin = TRUE
Property MergeEnd() As
Returns the prism merge end flag (for thin prism only).
It returns TRUE if merge ends is required , FALSE if not.
Returns:
oIsMergeEnd   The merge end flag as a boolean
Example:
The following example saves in MergeEndFlag the merge end flag of
prism firstPrism, and then sets it so that merge end will be required :
Set MergeEndFlag = firstPrism.IsMergeEnd
firstPrism.IsMergeEnd = TRUE
Property NeutralFiber() As
Returns the prism neutral fiber flag (for thin prism only).
It returns TRUE if the prism is a neutral fiber prism , FALSE if not.
Returns:
oIsNeutralFiber   The neutral fiber flag as a boolean
Example:
The following example saves in NeutralFiberFlag the neutral fiber flag of
prism firstPrism, and then sets it so that it will be now neutral fiber :
Set NeutralFiberFlag = firstPrism.IsNeutralFiber
firstPrism.IsNeutralFiber = TRUE
Property SecondLimit() As   (Read Only)
Returns the second prism limit (one of the two).
This limit manages the way the prism is ended.
Returns:
oSecondLimit   The second limit (see
for more information)
Example:
The following example returns in secondLimit the second limit of
prism firstPrism:
Set secondLimit = firstPrism.SecondLimit
Methods
Sub GetDirection( ioDirection)
Returns the prism direction with absolute coordinates.
It needs a safe array with 3 elements : X, Y, Z direction coordinates
The array must be previously initialized
Returns:
ioDirection   The direction coordinates
Example:
The following example returns in dirArray the direction coordinates of
prism firstPrism:
Dim dirArray(2)
Call firstPrism.GetDirection(dirArray)
Set x = dirArray[1]
Set y = dirArray[2]
Set z = dirArray[3]
Sub ReverseInnerSide()
Reverses the prism inner side when the profile is open.
This is useful for finding the shape to reach.
Example:
The following example reverses the current inner side of
prism firstPrism :
firstPrism.ReverseInnerSide
Sub SetDirection( iLine)
Sets the prism associative direction.
Parameters:
iLine
The support direction reference (see
for more information)
This reference can be valuated with a reference to a line or an edge.
The following
objects are supported:
,
and
.
Example:
The following example sets the prism direction reference of
prism firstPrism with prismDirRef line :
firstPrism.SetDirection prismDirRef
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_RectPattern_19102 ===
PartInterfaces RectPattern (Object)
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RectPattern (Object)
Represents the rectangular pattern.
The shape is copied along two directions.
Two linear repartitions control the shape copy.
See also:
Property Index
FirstDirectionRepartition
Returns the linear repartition along the first direction.
FirstDirectionRow
Returns the position of the shape to be copied along the
first linear direction.
FirstOrientation
Returns or sets whether the pattern is built towards
the first direction orientation.
FirstRectangularPatternParameters
Returns or sets the rectangular pattern parameters required to define the pattern.
SecondDirectionRepartition
Returns the linear repartition along the second direction.
SecondDirectionRow
Returns the position of the shape to be copied along the
second linear direction.
SecondOrientation
Returns or sets whether the pattern is built towards
the second direction orientation.
SecondRectangularPatternParameters
Returns or sets the rectangular pattern parameters required to define the pattern.
Method Index
GetFirstDirection
Returns the first repartition direction.
GetSecondDirection
Returns the second repartition direction.
SetFirstDirection
Sets the first repartition direction.
SetInstanceSpacing
Sets the InstanceSpacing.
SetSecondDirection
Sets the second repartition direction.
SetUnequalInstanceNumber
Sets the Instance Number.
Properties
Property FirstDirectionRepartition() As   (Read Only)
Returns the linear repartition along the first direction.
Example:
The following example returns in repart1
the first linear repartition of the
rectangular pattern firstPattern:
Set repart1 = firstPattern.FirstDirectionRepartition
Property FirstDirectionRow() As   (Read Only)
Returns the position of the shape to be copied along the
first linear direction.
Example:
The following example returns in FirstDirPos the
position of the shape to be copied along the
first linear direction
in the rectangular pattern firstPattern:
Set FirstDirPos = firstPattern.FirstDirectionRow
Property FirstOrientation() As
Returns or sets whether the pattern is built towards
the first direction orientation.
True if the pattern is built towards
the first direction orientation.
Example:
The following example returns in aligned1 whether the
rectangular pattern firstPattern is built towards the
first direction orientation, and then sets its to True:
Set aligned1 = firstPattern.FirstOrientation
firstPattern.FirstOrientation = True
Property FirstRectangularPatternParameters() As
Returns or sets the rectangular pattern parameters required to define the pattern.
These parameters are used when reading the CATIALinearRepartition properties.
Example:
The following example returns in parameters the rectangular pattern parameters
of the firstPattern rectangular pattern,
and then sets it to catUnequalSpacing,
so that the unqual spacing will be defined in first direction:
Set parameters = firstPattern.FirstCircularPatternParameters
Set firstPattern.FirstCircularPatternParameters = catUnequalSpacing
Property SecondDirectionRepartition() As   (Read Only)
Returns the linear repartition along the second direction.
Example:
The following example returns in repart2
the second linear repartition of the
rectangular pattern firstPattern:
Set repart2 = firstPattern.SecondDirectionRepartition
Property SecondDirectionRow() As   (Read Only)
Returns the position of the shape to be copied along the
second linear direction.
Example:
The following example returns in SecondDirPos the
position of the shape to be copied along the
second linear direction
in the rectangular pattern firstPattern:
Set SecondDirPos = firstPattern.SecondDirectionRow
Property SecondOrientation() As
Returns or sets whether the pattern is built towards
the second direction orientation.
True if the pattern is built towards
the second direction orientation.
Example:
The following example returns in aligned2 whether the
rectangular pattern firstPattern is built towards the
second direction orientation, and then sets its to False,
meaning the pattern is built in the opposite direction:
Set aligned2 = firstPattern.SecondOrientation
firstPattern.SecondOrientation = False
Property SecondRectangularPatternParameters() As
Returns or sets the rectangular pattern parameters required to define the pattern.
These parameters are used when reading the CATIALinearRepartition properties.
Example:
The following example returns in parameters the rectangular pattern parameters
of the secondPattern rectangular pattern,
and then sets it to catUnequalSpacing,
so that the unqual spacing will be defined in second direction:
Set parameters = secondPattern.SecondCircularPatternParameters
Set secondPattern.SecondCircularPatternParameters = catUnequalSpacing
Methods
Sub GetFirstDirection( ioFirstDirection)
Returns the first repartition direction.
The first repartition direction is returned as an array containing
the direction vector components.
Assume this array is o1stDirRep. It contains:
o1stDirRep[0],o1stDirRep[1],o1stDirRep[2]
The X, Y, and Z direction vector components
Example:
The following example returns in FirstDir
the first repartition direction vector
components of the rectangular pattern firstPattern
and saves them in variables:
Dim FirstDir()
Call firstPattern.GetFirstDirection(FirstDir)
x = FirstDir(0)
y = FirstDir(1)
z = FirstDir(2)
Sub GetSecondDirection( ioSecondDirection)
Returns the second repartition direction.
The second repartition direction is returned as an array containing
the direction vector components.
Assume this array is o2ndDirRep. It contains:
o2ndDirRep[0],o2ndDirRep[1],o2ndDirRep[2]
The X, Y, and Z direction vector components
Example:
The following example returns in SecondDir
the second repartition direction vector
components of the rectangular pattern firstPattern
and saves them in variables:
Call firstPattern.GetSecondDirection(SecondDir)
x = SecondDir[0]
y = SecondDir[1]
z = SecondDir[2]
Sub SetFirstDirection( iFirstDirection)
Sets the first repartition direction.
Parameters:
iFirstDirection
The first repartition direction.
It is passed as a
and can be valuated   with a reference to a line or an edge.
The following
objects are supported:
,
and
.
Example:
The following example sets the first repartition direction
of the rectangular pattern
firstPattern with the refToLine1 reference :
firstPattern.SetFirstDirection refToLine1
Sub SetInstanceSpacing( iInstanceNumber, iSpacing, iDirection)
Sets the InstanceSpacing.
Parameters:
iInstanceNumber
The Instance Number
iSpacing
The Spacing
iDirection
The Instance direction
Example:
The following example sets the InstanceSpacing in a direction for unequal spacing
Sub SetSecondDirection( iSecondDirection)
Sets the second repartition direction.
Parameters:
iSecondDirection
The second repartition direction.
It is passed as a
and can be valuated   with a reference to a line or an edge.
The following
objects are supported:
,
and
.
Example:
The following example sets the second repartition direction
of the rectangular pattern
firstPattern with the refToLine2 reference :
firstPattern.SetSecondDirection refToLine2
Sub SetUnequalInstanceNumber( iInstanceNumber, iDirection)
Sets the Instance Number.
Parameters:
iInstanceNumber
The Instance Number
iDirection
The Instance direction
Example:
The following example modifies the instance number for unequal spacing
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Remove_14837 ===
PartInterfaces Remove (Object)
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Remove (Object)
Represents the remove, or substract boolean operation.
It is performed between a body and the current shape.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_RemoveFace_17637 ===
PartInterfaces RemoveFace (Object)
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RemoveFace (Object)
Represents the Remove Face operation.
It removes a face or a set of faces.
Property Index
KeepFace
Adds a new face to be Kept.
KeepFaces
Get the specified faces to be kept.
Propagation
Get the faces that will be removed.
RemoveFace
Adds a new face to be removed.
RemoveFaces
Get the specified faces to be removed.
Method Index
remove_KeepFace
Removes a face to be Kept.
remove_RemoveFace
Removes a face to be removed.
Properties
Property KeepFace( iKeepFace) (Write Only)
Adds a new face to be Kept.
Parameters:
iKeepFace
The new face to process
The following
object is supported:
.
Property KeepFaces() As   (Read Only)
Get the specified faces to be kept.
Property Propagation() As   (Read Only)
Get the faces that will be removed.
Property RemoveFace( iRemoveFace) (Write Only)
Adds a new face to be removed.
Parameters:
iRemoveFace
The new face to process
The following
object is supported:
.
Property RemoveFaces() As   (Read Only)
Get the specified faces to be removed.
Methods
Sub remove_KeepFace( iKeepFace)
Removes a face to be Kept.
Parameters:
iKeepFace
The new face to process
The following
object is supported:
.
Sub remove_RemoveFace( iRemoveFace)
Removes a face to be removed.
Parameters:
iRemoveFace
The new face to process
The following
object is supported:
.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Repartition_19241 ===
PartInterfaces Repartition (Object)
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Repartition (Object)
Represents the repartition.
A repartition is a set of objects used by the pattern shapes.
It is the base object for linear and angular repartitions.
See also:
,
Property Index
InstancesCount
Returns the total number of copied shapes.
Properties
Property InstancesCount() As   (Read Only)
Returns the total number of copied shapes.
Example:
The following example returns in Nb the number
of shapes of the repartition firstRepartition:
Set Nb = firstRepartition.InstancesCount
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ReplaceFace_18513 ===
PartInterfaces ReplaceFace (Object)
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ReplaceFace (Object)
Represents the Replace Face operation.
It replaces a face or a set of faces obtained by tangency continuity
by a replacing element, such as a surface or a face or a skin.
Property Index
RemoveFace
Returns the face to be removed.
SplittingSide
Returns or sets the splitting side .
Method Index
AddRemoveFace
Sets the face to be removed.
AddSplitPlane
Sets the replacing element.
DeleteRemoveFace
Remove the face to be removed.
Properties
Property RemoveFace() As   (Read Only)
Returns the face to be removed.
Property SplittingSide() As
Returns or sets the splitting side .
The splitting side is the side of the body
kept after the splitting.
A positive side refers to the same orientation
than the splitting element normal vector.
Methods
Sub AddRemoveFace( iRemoveFace)
Sets the face to be removed.
Sub AddSplitPlane( iSplitPlane)
Sets the replacing element.
Sub DeleteRemoveFace( iRemoveFace)
Remove the face to be removed.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Revolution_18204 ===
PartInterfaces Revolution (Object)
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Revolution (Object)
Represents the revolution-based shapes.
It is the base objects for shaft and grooves.
See also:
,
Property Index
FirstAngle
Returns the revolution first angle.
IsThin
Returns the Revol thin flag.
MergeEnd
Returns the Revol merge end flag (for thin Revol only).
NeutralFiber
Returns the Revol neutral fiber flag (for thin Revol only).
RevoluteAxis
Returns or sets the rotation axis for Revol.
SecondAngle
Returns the revolution second angle.
Properties
Property FirstAngle() As   (Read Only)
Returns the revolution first angle.
This angle is computed around the revolution axis, starting from
the sketch plane trace on the plane perpendicular to the revolution
axis, and is counted positive clockwise when looking at this
plane in the revolution axis direction.
Example:
The following example returns in firstAngle
the first angle of the MyRevolution revolution object:
Set firstAngle = MyRevolution.FirstAngle
Property IsThin() As
Returns the Revol thin flag.
It returns TRUE if the Revol is a thin Revol , FALSE if not.
Returns:
oIsThin   The thin flag as a boolean
Example:
The following example saves in thinFlag the thin flag of
Revol firstRevol, and then sets it so that it will be now thin :
Set thinFlag = firstRevol.IsThin
firstRevol.IsThin = TRUE
Property MergeEnd() As
Returns the Revol merge end flag (for thin Revol only).
It returns TRUE if merge ends is required , FALSE if not.
Returns:
oIsMergeEnd   The merge end flag as a boolean
Example:
The following example saves in MergeEndFlag the merge end flag of
Revol firstRevol, and then sets it so that merge end will be required :
Set MergeEndFlag = firstRevol.IsMergeEnd
firstRevol.IsMergeEnd = TRUE
Property NeutralFiber() As
Returns the Revol neutral fiber flag (for thin Revol only).
It returns TRUE if the Revol is a neutral fiber Revol , FALSE if not.
Returns:
oIsNeutralFiber   The neutral fiber flag as a boolean
Example:
The following example saves in NeutralFiberFlag the neutral fiber flag of
Revol firstRevol, and then sets it so that it will be now neutral fiber :
Set NeutralFiberFlag = firstRevol.IsNeutralFiber
firstRevol.IsNeutralFiber = TRUE
Property RevoluteAxis() As
Returns or sets the rotation axis for Revol.
To set the property, you can use one of the following
objects:
,
or
.
Example:
This example retrieves in RevoluteAxis the rotation axis for the Rotate axis of the Revol feature
Dim RevoluteAxis As Reference
Set RevoluteAxis = Rotate.Axis
Property SecondAngle() As   (Read Only)
Returns the revolution second angle.
This angle is computed around the revolution axis, starting from
the sketch plane trace on the plane perpendicular to the revolution
axis, and is counted positive counterclockwise when looking at this
plane in the revolution axis direction.
Its default value is 0.
Example:
The following example returns in secondAngle
the second angle of the MyRevolution revolution object:
Set secondAngle = MyRevolution.SecondAngle
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Rib_13509 ===
PartInterfaces Rib (Object)
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Rib (Object)
Represents the rib shape.
The rib shape is made up of a profile represented by a sketch
swept along a center curve represented by another sketch.
This is a "positive" shape: it adds material to the body it belongs to.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Rotate_14811 ===
PartInterfaces Rotate (Object)
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Rotate (Object)
Represents the shape rotate feature object.
This solid feature is created from
an underlying HybridShapeRotate aggregated by the Rotate.
Role: To access the data of the hybrid shape rotate feature object.
This data includes:
The element to be rotated
The rotation axis
The angle and its value
Use the CATIAShapeFactory to create ShapeFeature object.
See also:
Property Index
Angle
Returns the rotation angle.
AngleValue
Returns or sets the rotation angle value.
Axis
Returns or sets the rotation axis.
HybridShape
Gets the underlying HybridShapeRotate.
Properties
Property Angle() As   (Read Only)
Returns the rotation angle.
Property AngleValue() As
Returns or sets the rotation angle value.
Example:
This example retrieves in AngleValue the angle value for the Rotate hybrid shape feature.
Dim AngleValue As double
Set AngleValue = Rotate.AngleValue
Property Axis() As
Returns or sets the rotation axis.
To set the property, you can use one of the following
objects:
,
or
.
Example:
This example retrieves in RotationAxis the rotation axis for the Rotate hybrid shape feature.
Dim RotationAxis As Reference
Set RotationAxis = Rotate.Axis
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeRotate.
Example:
The following example explains how to retrieve the underlying HybridShape Rotate
Dim oHybridShape as AnyObject
Set oHybridShape=oRotate.HybridShape
oHybridShape.SectionCoupling = 2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Scaling2_15763 ===
PartInterfaces Scaling2 (Object)
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Scaling2 (Object)
Represents the Scaling2 feature object.
This solid feature is created from  an underlying HybridShapeScaling
aggregated by the Scaling.
Role: To access the data of the feature object.
This data includes:
The element to be transformed using the Scaling2
The reference element for the Scaling2 which is a point or a plane
The ratio and its value
Use the CATIAShapeFactory to create Part object.
See also:
Property Index
Center
Returns or sets the reference element.
Ratio
Returns the scaling ratio.
RatioValue
Returns or sets the scaling ratio value.
Properties
Property Center() As
Returns or sets the reference element.This element can be a point or a plane.
To set the property, you can use one of the following
objects:
or
.
Example:
This example retrieves in RefElem the reference element for the Scaling2 hybrid shape feature.
Dim RefElem As Reference
Set RefElem = Scaling2.Center
Property Ratio() As   (Read Only)
Returns the scaling ratio.
Property RatioValue() As
Returns or sets the scaling ratio value.
Example:
This example retrieves in Value the ratio value for the Scaling hybrid shape feature.
Dim Value As double
Set Value = Scaling2.RatioValue
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Scaling_15413 ===
PartInterfaces Scaling (Object)
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Scaling (Object)
Represents the scaling shape.
The scaling shape is made up of a scaling reference
element, such as a point, and a scaling factor.
Property Index
Factor
Returns the scaling factor.
ScalingReference
Returns or sets the scaling reference element.
Properties
Property Factor() As   (Read Only)
Returns the scaling factor.
Example:
The following example returns in factor
the scaling factor of the scaling firstScaling:
Set factor = firstScaling.Factor
Property ScalingReference() As
Returns or sets the scaling reference element.
It can be a  point.
To set the property, you can use one of the following
objects:
or
.
Example:
The following example returns in ref the scaling
reference element of the scaling firstScaling,
and then sets it to the created MyRef:
Set ref = firstScaling.ScalingSupport
Set MyRef = part.CreateReferenceFromGeometry (Point)
firstScaling.ScalingSupport = MyRef
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_SewSurface_17826 ===
PartInterfaces SewSurface (Object)
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SewSurface (Object)
Represents the sewing  operation.
It sews a shape using a sewing element,
such as a surface or a face
Property Index
Deviation
Sets or Gets the maximum deviation allowed for smoothing operation in sewing command.
DeviationMode
Returns or sets the Deviation mode taken into account during Sew construction.
SewingIntersectionMode
Returns or sets the sewing mode .
SewingSide
Returns or sets the sewing side .
Method Index
SetSurfaceSupport
Sets the surface support for surfacic sew surface.
SetVolumeSupport
Sets the volume support for volume sew surface.
Properties
Property Deviation() As
Sets or Gets the maximum deviation allowed for smoothing operation in sewing command.
This value must be set in SI unit (m).
Example:
This example retrieves in DeviationValue the maximum deviation value for the
Sewfeature.
Dim DeviationValue As double
Set DeviationValue = Sew.MaximumDeviationValue
Property DeviationMode() As
Returns or sets the Deviation mode taken into account during Sew construction.
Legal values:
0
Unknown Deviation mode.
1
None Deviation mode. Error thrown if maximum deviation exceeds CATIA resolution.
2
Automatic Deviation mode. Error thrown if maximum deviation exceeds 100 times CATIA resolution.
3
Manual Deviation mode. Error thrown if maximum deviation exceeds input user deviation.
Example:
This example retrieves in oMode the Deviation mode
for the Sew feature.
Dim oMode
Set oMode = Sew.DeviationMode
Property SewingIntersectionMode() As
Returns or sets the sewing mode .
The sewing side is the side of the body
kept after the sewing.
A positive side refers to the same orientation
than the sewing element normal vector.
Example:
The following example returns in sptSide the sewing side
of the sew shape mySew, and then sets it to
catPositiveSide:
Set sptSide = mySew.SewingSide
mySew.SewingSide = catPositiveSide
Property SewingSide() As
Returns or sets the sewing side .
The sewing side is the side of the body
kept after the sewing.
A positive side refers to the same orientation
than the sewing element normal vector.
Example:
The following example returns in sptSide the sewing side
of the sew shape mySew, and then sets it to
catPositiveSide:
Set sptSide = mySew.SewingSide
mySew.SewingSide = catPositiveSide
Methods
Sub SetSurfaceSupport( iSupportSurface)
Sets the surface support for surfacic sew surface.
Parameters:
iSupportSurface
A Reference object to a surface (see
for more information)
Sub SetVolumeSupport( iVolume)
Sets the volume support for volume sew surface.
Parameters:
iVolume
A Reference object to a volume (see
for more information)
Example:
The following example sets the volume support of
SewSurface firstSewSurface to volumeExtrude volume reference :
firstSewSurface.SetVolumeSupport volumeExtrudeRef
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Shaft_14276 ===
PartInterfaces Shaft (Object)
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Shaft (Object)
Represents the shaft shape.
A shaft is made up of a sketch, used as the shaft profile, and containing
an axis, used as the revolution axis, and two limiting angles around
this axis.
This is a "positive" shape: it adds material to the body it
belongs to.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ShapeFactory_20269 ===
PartInterfaces ShapeFactory (Object)
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ShapeFactory (Object)
Represents the factory for shapes to create all kinds of shapes
that may be needed for part design.
The Shapefactory mission is to build from scratch shapes that
will be used within the design process of parts. Those shapes have a
strong mechanical built-in knowledge, such as chamfer or hole, and in
most cases apply contextually to the part being designed. When created,
they become part of the definition of whichever body or
shape that is current at that time. After they are created, they
become in turn the current body or shape.
In most cases, shapes are created from a factory with a minimum number
of parametersr. Other shapes parameters may be set further on by using
methods offered by the shape itself.
Method Index
AddNewAdd
Creates and returns a new add operation within the current body.
AddNewAffinity2
Creates and returns a Affinity feature.
AddNewAssemble
Creates and returns a new assembly operation within the current body.
AddNewAutoDraft
Creates and returns a new solid autodraft.
AddNewAutoFillet
Creates and returns a new solid autofillet.
AddNewAxisToAxis2
Creates and returns an AxisToAxis transformation feature.
AddNewBlend
Creates and returns a new Blend feature.
AddNewChamfer
Creates and returns a new chamfer within the current body.
AddNewCircPattern
Creates and returns a new circular pattern within the current body.
AddNewCircPatternofList
V5R8 Only: Creates and returns a new circular pattern within the current body using a list of shapes.
AddNewCloseSurface
Creates and returns a new CloseSurface feature.
AddNewDefeaturing
Creates and returns a new defeaturing operation within the current container.
AddNewDraft
Creates and returns a new draft within the current body.
AddNewEdgeFilletWithConstantRadius
AddNewEdgeFilletWithVaryingRadius
AddNewFaceFillet
AddNewGSDCircPattern
AddNewGSDRectPattern
AddNewGroove
Creates and returns a new groove within the current body.
AddNewGrooveFromRef
Creates and returns a new groove within the current body.
AddNewHole
Creates and returns a new hole within the current shape.
AddNewHoleFromPoint
Creates and returns a new hole within the current shape.
AddNewHoleFromRefPoint
Creates and returns a new hole within the current shape.
AddNewHoleFromSketch
Creates and returns a new hole within the current shape.
AddNewHoleWith2Constraints
Creates and returns a new hole within the current shape.
AddNewHoleWithConstraint
Creates and returns a new hole within the current shape.
AddNewIntersect
Creates and returns a new intersect operation within the current body.
AddNewLoft
Creates and returns a new Loft feature.
AddNewMirror
Creates and returns a new mirror within the current body.
AddNewPad
Creates and returns a new pad within the current body.
AddNewPadFromRef
Creates and returns a new pad within the current body.
AddNewPocket
Creates and returns a new pocket within the current shape.
AddNewPocketFromRef
Creates and returns a new pocket within the current shape.
AddNewRectPattern
Creates and returns a new rectangular pattern within the current body.
AddNewRectPatternofList
V5R8 Only: Creates and returns a new rectangular pattern within the current body using a list of shapes.
AddNewRemove
Creates and returns a new remove operation within the current body.
AddNewRemoveFace
Creates and returns a new RemoveFace feature.
AddNewRemovedBlend
Creates and returns a new Removed Blend feature.
AddNewRemovedLoft
Creates and returns a new Removed Loft feature.
AddNewReplaceFace
Creates and returns a new Align/ ReplaceFace feature.
AddNewRib
Creates and returns a new rib within the current body.
AddNewRibFromRef
Creates and returns a new rib within the current body.
AddNewScaling
Creates and returns a new scaling within the current body.
AddNewSewSurface
Creates and returns a new sewing operation within the current body.
AddNewShaft
Creates and returns a new shaft within the current body.
AddNewShaftFromRef
Creates and returns a new shaft within the current body.
AddNewShell
Creates and returns a new shell within the current body.
AddNewSlot
Creates and returns a new slot within the current shape.
AddNewSlotFromRef
Creates and returns a new slot within the current shape.
AddNewSolidCombine
Creates and returns a new SolidCombine feature.
AddNewSolidEdgeFilletWithConstantRadius
Creates and returns a new solid edge fillet with a constant radius.
AddNewSolidEdgeFilletWithVaryingRadius
Creates and returns a new solid edge fillet with a varying radius.
AddNewSolidFaceFillet
Creates and returns a new solid face-to-face fillet.
AddNewSolidTritangentFillet
Creates and returns a new solid tritangent fillet within the current body.
AddNewSplit
Creates and returns a new split operation within the current body.
AddNewStiffener
Creates and returns a new stiffener within the current body.
AddNewStiffenerFromRef
Creates and returns a new stiffener within the current body.
AddNewSurfaceEdgeFilletWithConstantRadius
Creates and returns a new surface edge fillet with a constant radius.
AddNewSurfaceEdgeFilletWithVaryingRadius
Creates and returns a new surface edge fillet with a varying radius.
AddNewSurfaceFaceFillet
Creates and returns a new surface face-to-face fillet.
AddNewSurfaceTritangentFillet
Creates and returns a new surface tritangent fillet within the current body.
AddNewSurfacicAutoFillet
Creates and returns a new Surfacic autofillet.
AddNewSurfacicCircPattern
Creates and returns a new gsd circular pattern within the current body.
AddNewSurfacicRectPattern
Creates and returns a new GSD rectangular pattern within the current body.
AddNewSurfacicSewSurface
Creates and returns a new volume sewing operation within the current OGS/GS.
AddNewSurfacicUserPattern
Creates and returns a new GSD user pattern within the current body.
AddNewThickSurface
Creates and returns a new ThickSurface feature.
AddNewThickness
Creates and returns a new thickness within the current body.
AddNewThreadWithOutRef
Creates and returns a new thread\tap within the current body.
AddNewThreadWithRef
Creates and returns a new thread\tap within the current body.
AddNewTrim
Creates and returns a new Trim operation within the current body.
AddNewTritangentFillet
AddNewUserPattern
Creates and returns a new user pattern within the current body.
AddNewUserPatternofList
V5R8 Only: Creates and returns a new user pattern within the current body using a list of shapes.
AddNewVolumeAdd
Creates and returns a Volumic Add feature.
AddNewVolumeCloseSurface
Creates and returns a new VolumeCloseSurface feature.
AddNewVolumeIntersect
Creates and returns a Volumic Intersect feature.
AddNewVolumeRemove
Creates and returns a Volumic Remove feature.
AddNewVolumeSewSurface
Creates and returns a new volume sewing operation within the current OGS/GS.
AddNewVolumeShell
Creates and returns a Volumic Shell feature.
AddNewVolumeThickSurface
Creates and returns a new VolumeThickSurface feature.
AddNewVolumeThickness
Creates and returns a volume new thickness within the current GS or OGS.
AddNewVolumeTrim
Creates and returns a new Volume Trim operation within the GS/OGS.
AddNewVolumicDraft
Creates and returns a new volume draft within the current body.
Methods
Func AddNewAdd( iBodyToAdd) As
Creates and returns a new add operation within the current body.
Parameters:
iBodyToAdd
The body to add to the current body
Returns:
The created add operation
Func AddNewAffinity2( XRatio, YRatio, ZRatio) As
Creates and returns a Affinity feature.
Parameters:
XRatio
Value for the XRatio.
YRatio
Value for the YRatio.
ZRatio
Value for the ZRatio.
Returns:
the created Affinity feature.
Func AddNewAssemble( iBodyToAssemble) As
Creates and returns a new assembly operation within the current body.
Parameters:
iBodyToAssemble
The body to assemble with the current body
Returns:
The created assembly operation
Func AddNewAutoDraft( iDraftAngle) As
Creates and returns a new solid autodraft.
Use this method to create autodraft by providing draft angle.
Parameters:
iDraftAngle
The draft angle.
Returns:
The created autodraft.
Func AddNewAutoFillet( iFilletRadius, iRoundRadius) As
Creates and returns a new solid autofillet.
Use this method to create autofillet by providing fillet and round radius values.
Parameters:
iFilletRadius
The fillet radius
iRoundRadius
The round radius
Returns:
The created autofillet
Func AddNewAxisToAxis2( iReference, iTarget) As
Creates and returns an AxisToAxis transformation feature.
Parameters:
iReference
The refrence axis.
iTarget
The target axis.
Returns:
The created AxisToAxis transformation feature.
Func AddNewBlend() As
Creates and returns a new Blend feature.
Returns:
The created Blend feature
Func AddNewChamfer( iObjectToChamfer, iPropagation, iMode, iOrientation, iLength1, iLength2OrAngle) As
Creates and returns a new chamfer within the current body.
Parameters:
iObjectToChamfer
The first edge or face to chamfer
The following
object is supported:
.
iPropagation
Controls if and how the chamfering operation should propagate beyond the
first chamfer element iObjectToChamfer, when it is an edge
iMode
Controls if the chamfer is defined by two lengthes, or by an angle and a
length
The value of this argument changes the way the arguments iLength1
and iLength2OrAngle should be interpreted.
iOrientation
Defines the relative meaning of arguments iLength1 and
iLength2OrAngle when defining a chamfer by two lengthes
iLength1
The first value for chamfer dimensioning. It represents the chamfer
first length if the chamfer is defined by two lengthes, or the chamfer
length if the chamfer is defined by a length and an angle.
iLength2OrAngle
The second value for chamfer dimensioning. It represents the chamfer
second length if the chamfer is defined by two lengthes, or the chamfer
angle if the chamfer is defined by a length and an angle.
Returns:
The created chamfer
Func AddNewCircPattern( iShapeToCopy, iNbOfCopiesInRadialDir, iNbOfCopiesInAngularDir, iStepInRadialDir, iStepInAngularDir, iShapeToCopyPositionAlongRadialDir, iShapeToCopyPositionAlongAngularDir, iRotationCenter, iRotationAxis, iIsReversedRotationAxis, iRotationAngle, iIsRadiusAligned) As
Creates and returns a new circular pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the circular pattern
iNbOfInstancesInRadialDir
The number of times iShapeToCopy will be copied along
pattern radial direction
iNbOfInstancesInAngularDir
The number of times iShapeToCopy will be copied along
pattern angular direction
iStepInRadialDir
The distance that will separate two consecutive copies in the pattern
along its radial direction
iStepInAngularDir
The angle that will separate two consecutive copies in the pattern
along its angular direction
iShapeToCopyPositionAlongRadialDir
Specifies the position of the original shape iShapeToCopy
among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir
Specifies the position of the original shape iShapeToCopy
among its copies along the angular direction
iRotationCenter
The point or vertex that specifies the pattern center of rotation
iRotationAxis
The line or linear edge that specifies the axis around which instances
will be rotated relative to each other
The following
objects are supported:
,
,
and
.
iIsReversedRotationAxis
The boolean flag indicating wether the natural orientation of
iRotationAxis should be used to orient the pattern operation.
A value
of true indicates that iItemToDuplicate are copied in the
direction of the natural orientation of iRotationAxis.
iRotationAngle
The angle applied to the direction iRotationAxis
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a circular pattern
relatively to existing geometry, but not necessarily parallel to it.
iIsRadiusAligned
The boolean flag that specifies whether the instances
of iItemToDuplicate
copied by the pattern should be kept parallel to each other (True)
or if they should
be aligned with the radial direction they lie upon (False).
Returns:
The created circular pattern
Func AddNewCircPatternofList( iShapeToCopy, iNbOfCopiesInRadialDir, iNbOfCopiesInAngularDir, iStepInRadialDir, iStepInAngularDir, iShapeToCopyPositionAlongRadialDir, iShapeToCopyPositionAlongAngularDir, iRotationCenter, iRotationAxis, iIsReversedRotationAxis, iRotationAngle, iIsRadiusAligned) As
V5R8 Only: Creates and returns a new circular pattern within the current body using a list of shapes.
Parameters:
iShapeToCopy
The shape to be copied by the circular pattern.
Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfInstancesInRadialDir
The number of times iShapeToCopy will be copied along
pattern radial direction
iNbOfInstancesInAngularDir
The number of times iShapeToCopy will be copied along
pattern angular direction
iStepInRadialDir
The distance that will separate two consecutive copies in the pattern
along its radial direction
iStepInAngularDir
The angle that will separate two consecutive copies in the pattern
along its angular direction
iShapeToCopyPositionAlongRadialDir
Specifies the position of the original shape iShapeToCopy
among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir
Specifies the position of the original shape iShapeToCopy
among its copies along the angular direction
iRotationCenter
The point or vertex that specifies the pattern center of rotation
iRotationAxis
The line or linear edge that specifies the axis around which instances
will be rotated relative to each other
iIsReversedRotationAxis
The boolean flag indicating wether the natural orientation of
iRotationAxis should be used to orient the pattern operation.
A value
of true indicates that iItemToDuplicate are copied in the
direction of the natural orientation of iRotationAxis.
iRotationAngle
The angle applied to the direction iRotationAxis
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a circular pattern
relatively to existing geometry, but not necessarily parallel to it.
iIsRadiusAligned
The boolean flag that specifies whether the instances
of iItemToDuplicate
copied by the pattern should be kept parallel to each other (True)
or if they should
be aligned with the radial direction they lie upon (False).
Returns:
The created circular pattern
Func AddNewCloseSurface( iCloseElement) As
Creates and returns a new CloseSurface feature.
Parameters:
iCloseElement
The skin that will be closed and add with the current body
Returns:
The created CloseSurface feature
Func AddNewDefeaturing() As
Creates and returns a new defeaturing operation within the current container.
Returns:
The created defeaturing operation
Func AddNewDraft( iFaceToDraft, iNeutral, iNeutralMode, iParting, iDirX, iDirY, iDirZ, iMode, iAngle, iMultiselectionMode) As
Creates and returns a new draft within the current body.
The draft needs a reference face on the body. This face will remain
unchanged in the draft operation, while faces adjacent to it
and specified for drafting will be rotated by the draft angle.
Parameters:
iFaceToDraft
The first face to draft in the body. This face should be adjacent to the
iFaceToDraft face. If several faces are to be drafted, only the
first one is specified here, the others being inferred by propagating the
draft operation onto faces adjacent to this first face. This is
controlled by the iNeutralMode argument.
The following
object is supported:
.
iNeutral
The reference face for the draft. The draft needs a reference face on
the body, that will remain unchanged in the draft operation, while faces
adjacent to it and specified for drafting will be rotated according
to the draft angle iAngle.
The following
object is supported:
.
iNeutralMode
Controls if and how the drafting operation should be propagated beyond the
first face to draft iFaceToDraft to other adjacent faces.
iParting
The draft parting plane, face or surface.
It specifies the element within the body to draft
that represents the bottom of the mold. This element can be located either
somewhere in the middle of the body or be one of its boundary faces.
When located in the middle of the body, it crosses the faces to draft,
and as a result, those faces are drafted with a positive angle on one
side of the parting surface, and with a negative angle on the other side.
The following
object is supported:
.
iDirX,iDirY,iDirZ
The X, Y, and Z components of the absolute vector representing the drafting
direction (i.e. the mold extraction direction).
iMode
The draft connecting mode to its reference face iFaceToDraft
iAngle
The draft angle
iMultiselectionMode.
The elements to be drafted can be selected explicitly
or can implicitly selected as neighbors of the neutral face
Returns:
The created draft
Func AddNewEdgeFilletWithConstantRadius( iEdgeToFillet, iPropagMode, iRadius) As
Deprecated:
V5R14 #AddNewEdgeFilletWithConstantRadius
use AddNewSolidEdgeFilletWithConstantRadius or AddNewSurfaceEdgeFilletWithConstantRadius
depending on the type of fillet you want to create
Func AddNewEdgeFilletWithVaryingRadius( iEdgeToFillet, iPropagMode, iVariationMode, iDefaultRadius) As
Deprecated:
V5R14 #AddNewEdgeFilletWithVaryingRadius
use AddNewSolidEdgeFilletWithVaryingRadius or AddNewSurfaceEdgeFilletWithVaryingRadius
depending on the type of fillet you want to create
Func AddNewFaceFillet( iF1, iF2, iRadius) As
Deprecated:
V5R14 #AddNewFaceFillet
use AddNewSolidFaceFillet or AddNewSurfaceFaceFillet
depending on the type of fillet you want to create
Func AddNewGSDCircPattern( iShapeToCopy, iNbOfCopiesInRadialDir, iNbOfCopiesInAngularDir, iStepInRadialDir, iStepInAngularDir, iShapeToCopyPositionAlongRadialDir, iShapeToCopyPositionAlongAngularDir, iRotationCenter, iRotationAxis, iIsReversedRotationAxis, iRotationAngle, iIsRadiusAligned, iCompleteCrown, iType) As
Deprecated:
V5R15 #AddNewSurfacicCircPattern
Func AddNewGSDRectPattern( iShapeToCopy, iNbOfCopiesInDir1, iNbOfCopiesInDir2, iStepInDir1, iStepInDir2, iShapeToCopyPositionAlongDir1, iShapeToCopyPositionAlongDir2, iDir1, iDir2, iIsReversedDir1, iIsReversedDir2, iRotationAngle, iType) As
Deprecated:
V5R15 #AddNewSurfacicRectPattern
Func AddNewGroove( iSketch) As
Creates and returns a new groove within the current body.
The
, as a supertype for grooves, provides starting and ending angles
for the groove definition.
Parameters:
iSketch
The sketch defining the groove section.
The sketch must contain
a contour and an axis that will be used to rotate
the contour in the space, thus defining the groove. The contour has to
penetrate in 3D space the current shape.
Returns:
The created groove
Func AddNewGrooveFromRef( iProfileElt) As
Creates and returns a new groove within the current body.
Parameters:
iProfileElt
The reference on the element defining the groove base
Returns:
The created groove
Func AddNewHole( iSupport, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iSupport
The support defining the hole reference plane.
Anchor point is located at the barycenter of the support.
The hole axis in 3D passes through that point and is normal to the plane.
The following
object is supported:
.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewHoleFromPoint( iX, iY, iZ, iSupport, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iX
Origin point x absolute coordinate
iY
Origin point y absolute coordinate
iZ
Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iSupport
The support defining the hole reference plane.
The following
object is supported:
.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewHoleFromRefPoint( iOrigin, iSupport, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iOrigin
The origin point which the hole is anchored to.
iSupport
The support defining the hole reference plane.
The following
object is supported:
.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewHoleFromSketch( iSketch, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iSketch
The sketch defining the hole reference plane and anchor point.
This sketch must contain a single point that defines the hole axis:
the hole axis in 3D passes through that point and is normal to the
sketch plane.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewHoleWith2Constraints( iX, iY, iZ, iEdge1, iEdge2, iSupport, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iX
Origin point x absolute coordinate
iY
Origin point y absolute coordinate
iZ
Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iEdge
The edge which the hole is constrained to.
The origin of the hole will have a length constraint with
each edge.
The following
object is supported:
.
iSupport
The support defining the hole reference plane.
The following
object is supported:
.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewHoleWithConstraint( iX, iY, iZ, iEdge, iSupport, iDepth) As
Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its
creation.
Parameters:
iX
Origin point x absolute coordinate
iY
Origin point y absolute coordinate
iZ
Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iEdge
The edge which the hole is constrained to.
If edge is circular, the origin of the hole will be concentric
to the edge (iX, iY, iZ will be overridden).
if not, the origin of the hole will have a length constraint with
the edge.
The following
object is supported:
.
iSupport
The support defining the hole reference plane.
The following
object is supported:
.
iDepth
The hole depth.
Returns:
The created hole
Func AddNewIntersect( iBodyToIntersect) As
Creates and returns a new intersect operation within the current body.
Parameters:
iBodyToIntersect
The body to intersect with the current body
Returns:
The created intersect operation
Func AddNewLoft() As
Creates and returns a new Loft feature.
Returns:
The created Loft feature
Func AddNewMirror( iMirroringElement) As
Creates and returns a new mirror within the current body.
A mirror allows for transforming existing shapes by a symmetry
with respect to an existing plane.
Parameters:
iMirroringElement
The plane used by the mirror as the symmetry plane.
The following
object is supported:
.
Returns:
The created mirror
Func AddNewPad( iSketch, iHeight) As
Creates and returns a new pad within the current body.
Parameters:
iSketch
The sketch defining the pad base
iHeight
The pad height
Returns:
The created pad
Func AddNewPadFromRef( iProfileElt, iHeight) As
Creates and returns a new pad within the current body.
Parameters:
iProfileElt
The reference on the element defining the pad base
iHeight
The pad height
Returns:
The created pad
Func AddNewPocket( iSketch, iHeight) As
Creates and returns a new pocket within the current shape.
Parameters:
iSketch
The sketch defining the pocket base
iDepth
The pocket depth
Returns:
The created pocket
Func AddNewPocketFromRef( iProfileElt, iHeight) As
Creates and returns a new pocket within the current shape.
Parameters:
iProfileElt
The reference on the element defining the pocket base
iDepth
The pocket depth
Returns:
The created pocket
Func AddNewRectPattern( iShapeToCopy, iNbOfCopiesInDir1, iNbOfCopiesInDir2, iStepInDir1, iStepInDir2, iShapeToCopyPositionAlongDir1, iShapeToCopyPositionAlongDir2, iDir1, iDir2, iIsReversedDir1, iIsReversedDir2, iRotationAngle) As
Creates and returns a new rectangular pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the rectangular pattern
iNbOfCopiesInDir1
The number of times iShapeToCopy will be copied along
the pattern first direction
iNbOfCopiesInDir2
The number of times iShapeToCopy will be copied along
the pattern second direction
iStepInDir1
The distance that will separate two consecutive copies in the pattern
along its first direction
iStepInDir2
The distance that will separate two consecutive copies in the pattern
along its second direction
iShapeToCopyPositionAlongDir1
Specifies the position of the original shape iShapeToCopy
among its copies along iDir1
iShapeToCopyPositionAlongDir2
Specifies the position of the original shape iShapeToCopy
among its copies along iDir2
iDir1
The line or linear edge that specifies the pattern first repartition
direction
The following
objects are supported:
,
,
.
iDir2
The line or linear edge that specifies the pattern second repartition
direction
The following
objects are supported:
,
,
.
iIsReversedDir1
The boolean flag indicating whether the natural orientation of
iDir1 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir1.
iIsReversedDir2
The boolean flag indicating whether the natural orientation of
iDir2 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir2.
iRotationAngle
The angle applied to both directions iDir1 and iDir2
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a rectangular pattern
relatively to existing geometry, but not necessarily parallel to it.
Returns:
The created rectangular pattern
Func AddNewRectPatternofList( iShapeToCopy, iNbOfCopiesInDir1, iNbOfCopiesInDir2, iStepInDir1, iStepInDir2, iShapeToCopyPositionAlongDir1, iShapeToCopyPositionAlongDir2, iDir1, iDir2, iIsReversedDir1, iIsReversedDir2, iRotationAngle) As
V5R8 Only: Creates and returns a new rectangular pattern within the current body using a list of shapes.
Parameters:
iShapeToCopy
The shape to be copied by the rectangular pattern
Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfCopiesInDir1
The number of times iShapeToCopy will be copied along
the pattern first direction
iNbOfCopiesInDir2
The number of times iShapeToCopy will be copied along
the pattern second direction
iStepInDir1
The distance that will separate two consecutive copies in the pattern
along its first direction
iStepInDir2
The distance that will separate two consecutive copies in the pattern
along its second direction
iShapeToCopyPositionAlongDir1
Specifies the position of the original shape iShapeToCopy
among its copies along iDir1
iShapeToCopyPositionAlongDir2
Specifies the position of the original shape iShapeToCopy
among its copies along iDir2
iDir1
The line or linear edge that specifies the pattern first repartition
direction
iDir2
The line or linear edge that specifies the pattern second repartition
direction
iIsReversedDir1
The boolean flag indicating whether the natural orientation of
iDir1 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir1.
iIsReversedDir2
The boolean flag indicating whether the natural orientation of
iDir2 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir2.
iRotationAngle
The angle applied to both directions iDir1 and iDir2
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a rectangular pattern
relatively to existing geometry, but not necessarily parallel to it.
Returns:
The created rectangular pattern
Func AddNewRemove( iBodyToRemove) As
Creates and returns a new remove operation within the current body.
Parameters:
iBodyToRemove
The body to remove from the current body
Returns:
The created remove operation
Func AddNewRemoveFace( iKeepFaces, iRemoveFaces) As
Creates and returns a new RemoveFace feature.
Parameters:
iKeepFaces
The reference of the face to Keep.
iRemoveFaces
The reference of the face to Remove.
Returns:
The created RemoveFace feature.
Func AddNewRemovedBlend() As
Creates and returns a new Removed Blend feature.
Returns:
The created Removed Blend feature
Func AddNewRemovedLoft() As
Creates and returns a new Removed Loft feature.
Returns:
The created Removed Loft feature
Func AddNewReplaceFace( iSplitPlane, iRemoveFace, iSplittingSide) As
Creates and returns a new Align/ ReplaceFace feature.
Parameters:
iSplitPlane
The reference of the element defining the Splitting Plane.
iRemoveFace
The reference of the Face to Remove.
iSplittingSide
The specification for which side of the current body should be Align
Returns:
The created Align/ ReplaceFace feature.
Func AddNewRib( iSketch, iCenterCurve) As
Creates and returns a new rib within the current body.
Parameters:
iSketch
The sketch defining the rib section
iCenterCurve
The sketched curve that defines the rib center curve. It must cross the
section definition sketch iSketch within the inner part of
its contour.
Returns:
The created rib
Func AddNewRibFromRef( iProfile, iCenterCurve) As
Creates and returns a new rib within the current body.
Parameters:
iProfile
The Profile defining the rib section
iCenterCurve
The curve that defines the rib center curve.
The following
object is supported:
.
Returns:
The created rib
Func AddNewScaling( iScalingReference, iFactor) As
Creates and returns a new scaling within the current body.
Parameters:
iScalingReference
The point, plane or  face of the current body  that will remain
fixed during the
scaling process: even if the face itself shrinks or expands during the
scaling, its supporting plane will remain unchanged after the scaling.
The following
objects are supported:
and
.
iFactor
The scaling factor
Returns:
The created scaling
Func AddNewSewSurface( iSewingElement, iSewingSide) As
Creates and returns a new sewing operation within the current body.
Parameters:
iSewingElement
The face or skin or surface that will be sewn on the current body
iSewingSide
The specification for which side of the current body should be kept
at the end of the sewing operation
Returns:
The created sewing operation
Func AddNewShaft( iSketch) As
Creates and returns a new shaft within the current body.
The
, as a supertype for shafts, provides starting and ending angles for the shaft definition.
Parameters:
iSketch
The sketch defining the shaft section.
If the shaft applies to the current body,
then the sketch must contain
a contour and an axis that will be used to rotate
the contour in the space, thus defining the shaft.
If the shaft is the first shape defined, there is not current
body to apply to. In such a case, the sketch must contain a curve
whose end points are linked by an axis. By rotating the
curve in the space around the axis, the shaft operation will define
a revolution shape.
This also works if the sketch contains a closed contour and
an axis outside of this contour: in that case a revolution
shape will be created, for example a torus.
Returns:
The created shaft
Func AddNewShaftFromRef( iProfileElt) As
Creates and returns a new shaft within the current body.
Parameters:
iProfileElt
The reference on the element defining the shaft base
Returns:
The created shaft
Func AddNewShell( iFaceToRemove, iInternalThickness, iExternalThickness) As
Creates and returns a new shell within the current body.
Parameters:
iFaceToRemove
The first face to be removed in the shell process.
The following
object is supported:
.
iInternalThickness
The thickness of material to be added on the internal side of all the faces
during the shell process, except for those to be removed
iExternaThickness
The thickness of material to be added on the external side of all the faces
during the shell process, except for those to be removed
Returns:
The created shell
Func AddNewSlot( iSketch, iCenterCurve) As
Creates and returns a new slot within the current shape.
Parameters:
iSketch
The sketch defining the slot section
iCenterCurve
The sketched curve that defines the slot center curve. It must cross the
section definition sketch iSketch within the inner part of
its contour.
Returns:
The created slot
Func AddNewSlotFromRef( iProfile, iCenterCurve) As
Creates and returns a new slot within the current shape.
Parameters:
iProfile
The sketch defining the slot section
iCenterCurve
The curve that defines the slot center curve.
The following
object is supported:
.
Returns:
The created slot
Func AddNewSolidCombine( iProfileEltFirst, iProfileEltSecond) As
Creates and returns a new SolidCombine feature.
Parameters:
iProfileEltFirst
The reference of the element defining the profile for first component.
iProfileEltSecond
The reference of the element defining the profile for second component.
Returns:
The created SolidCombine feature.
Func AddNewSolidEdgeFilletWithConstantRadius( iEdgeToFillet, iPropagMode, iRadius) As
Creates and returns a new solid edge fillet with a constant radius.
within the current body.
Parameters:
iEdgeToFillet
The edge that will be filleted first
The following
object is supported:
.
iPropagMode
Controls whether other edges found adjacent to the
first one should also be filleted in the same operation
iRadius
The fillet radius
Returns:
The created edge fillet
Func AddNewSolidEdgeFilletWithVaryingRadius( iEdgeToFillet, iPropagMode, iVariationMode, iDefaultRadius) As
Creates and returns a new solid edge fillet with a varying radius.
within the current body.
Parameters:
iEdgeToFillet
The edge that will be filleted first
The following
object is supported:
.
iPropagMode
Controls whether other edges found adjacent to the
first one should also be filleted in the same operation
iVariationMode
Controls the law of evolution for the fillet radius
between specified control points, such as edges extremities
iDefaultRadius
The fillet default radius, that will apply when no other radius can
be inferred from the iVariationMode parameter
Returns:
The created edge fillet
Func AddNewSolidFaceFillet( iF1, iF2, iRadius) As
Creates and returns a new solid face-to-face fillet.
Use this method to created face-to-face fillets with varying fillet radii,
by editing fillet attributes driving its radius after its creation.
Parameters:
iF1
The first face that will support the fillet
The following
object is supported:
.
iF2
The second face that will support the fillet
The following
object is supported:
.
iRadius
The fillet radius
Returns:
The created face-to-face fillet
Func AddNewSolidTritangentFillet( iF1, iF2, iRemovedFace) As
Creates and returns a new solid tritangent fillet within the current body.
This kind of fillet begins with tangency on a first face iF1,
gets tangent to a second one iRemovedFace
and ends with tangency to a third one iF2.
During the process the
second face iRemovedFace is removed.
Parameters:
iF1
The starting face for the fillet
The following
object is supported:
.
iF2
The ending face for the fillet
The following
object is supported:
.
iRemovedFace
The face used as an intermediate tangent support for the fillet
during its course from iF1 to iF2. This face will be
removed at the end of the filleting operation.
The following
object is supported:
Returns:
The created tritangent fillet
Func AddNewSplit( iSplittingElement, iSplitSide) As
Creates and returns a new split operation within the current body.
Parameters:
iSplittingElement
The face or plane that will split the current body
The following
object is supported:
.
iSplitSide
The specification for which side of the current body should be kept
at the end of the split operation
Returns:
The created split operation
Func AddNewStiffener( iSketch) As
Creates and returns a new stiffener within the current body.
A stiffener is made up of a sketch used as the stiffener profile,
that is extruded (offset) and that fills the nearest shape.
Parameters:
iSketch
The sketch defining the stiffener border. It must contain a
line or a curve that does not cross in 3D space the face(s) to stiffen.
Returns:
The created stiffener
Func AddNewStiffenerFromRef( iProfileElt) As
Creates and returns a new stiffener within the current body.
Parameters:
iProfileElt
The reference on the element defining the stiffener profile
Returns:
The created stiffener
Func AddNewSurfaceEdgeFilletWithConstantRadius( iEdgeToFillet, iPropagMode, iRadius) As
Creates and returns a new surface edge fillet with a constant radius.
within the current body.
Parameters:
iEdgeToFillet
The edge that will be filleted first
The following
object is supported:
.
iPropagMode
Controls whether other edges found adjacent to the
first one should also be filleted in the same operation
iRadius
The fillet radius
Returns:
The created edge fillet
Func AddNewSurfaceEdgeFilletWithVaryingRadius( iEdgeToFillet, iPropagMode, iVariationMode, iDefaultRadius) As
Creates and returns a new surface edge fillet with a varying radius.
within the current body.
Parameters:
iEdgeToFillet
The edge that will be filleted first
The following
object is supported:
.
iPropagMode
Controls whether other edges found adjacent to the
first one should also be filleted in the same operation
iVariationMode
Controls the law of evolution for the fillet radius
between specified control points, such as edges extremities
iDefaultRadius
The fillet default radius, that will apply when no other radius can
be inferred from the iVariationMode parameter
Returns:
The created edge fillet
Func AddNewSurfaceFaceFillet( iF1, iF2, iRadius) As
Creates and returns a new surface face-to-face fillet.
Use this method to created face-to-face fillets with varying fillet radii,
by editing fillet attributes driving its radius after its creation.
Parameters:
iF1
The first face that will support the fillet
The following
object is supported:
.
iF2
The second face that will support the fillet
The following
object is supported:
.
iRadius
The fillet radius
Returns:
The created face-to-face fillet
Func AddNewSurfaceTritangentFillet( iF1, iF2, iRemovedFace) As
Creates and returns a new surface tritangent fillet within the current body.
This kind of fillet begins with tangency on a first face iF1,
gets tangent to a second one iRemovedFace
and ends with tangency to a third one iF2.
During the process the
second face iRemovedFace is removed.
Parameters:
iF1
The starting face for the fillet
The following
object is supported:
.
iF2
The ending face for the fillet
The following
object is supported:
.
iRemovedFace
The face used as an intermediate tangent support for the fillet
during its course from iF1 to iF2. This face will be
removed at the end of the filleting operation.
The following
object is supported:
Returns:
The created tritangent fillet
Func AddNewSurfacicAutoFillet( iFilletRadius) As
Creates and returns a new Surfacic autofillet.
Use this method to create autofillet by providing fillet radius value.
Parameters:
iFilletRadius
The fillet radius
Returns:
The created autofillet
Func AddNewSurfacicCircPattern( iShapeToCopy, iNbOfCopiesInRadialDir, iNbOfCopiesInAngularDir, iStepInRadialDir, iStepInAngularDir, iShapeToCopyPositionAlongRadialDir, iShapeToCopyPositionAlongAngularDir, iRotationCenter, iRotationAxis, iIsReversedRotationAxis, iRotationAngle, iIsRadiusAligned, iCompleteCrown) As
Creates and returns a new gsd circular pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the circular pattern
iNbOfInstancesInRadialDir
The number of times iShapeToCopy will be copied along
pattern radial direction
iNbOfInstancesInAngularDir
The number of times iShapeToCopy will be copied along
pattern angular direction
iStepInRadialDir
The distance that will separate two consecutive copies in the pattern
along its radial direction
iStepInAngularDir
The angle that will separate two consecutive copies in the pattern
along its angular direction
iShapeToCopyPositionAlongRadialDir
Specifies the position of the original shape iShapeToCopy
among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir
Specifies the position of the original shape iShapeToCopy
among its copies along the angular direction
iRotationCenter
The point or vertex that specifies the pattern center of rotation
iRotationAxis
The line or linear edge that specifies the axis around which instances
will be rotated relative to each other
The following
objects are supported:
,
,
and
.
iIsReversedRotationAxis
The boolean flag indicating wether the natural orientation of
iRotationAxis should be used to orient the pattern operation.
A value
of true indicates that iItemToDuplicate are copied in the
direction of the natural orientation of iRotationAxis.
iRotationAngle
The angle applied to the direction iRotationAxis
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a circular pattern
relatively to existing geometry, but not necessarily parallel to it.
iIsRadiusAligned
The boolean flag that specifies whether the instances
of iItemToDuplicate
copied by the pattern should be kept parallel to each other (True)
or if they should
be aligned with the radial direction they lie upon (False).
iCompleteCrown
The boolean flag specifies the mode of angular distribution.
True indicates that the angular step will be equal to 360 degrees iNba.
Returns:
The created circular pattern
Func AddNewSurfacicRectPattern( iShapeToCopy, iNbOfCopiesInDir1, iNbOfCopiesInDir2, iStepInDir1, iStepInDir2, iShapeToCopyPositionAlongDir1, iShapeToCopyPositionAlongDir2, iDir1, iDir2, iIsReversedDir1, iIsReversedDir2, iRotationAngle) As
Creates and returns a new GSD rectangular pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the rectangular pattern
iNbOfCopiesInDir1
The number of times iShapeToCopy will be copied along
the pattern first direction
iNbOfCopiesInDir2
The number of times iShapeToCopy will be copied along
the pattern second direction
iStepInDir1
The distance that will separate two consecutive copies in the pattern
along its first direction
iStepInDir2
The distance that will separate two consecutive copies in the pattern
along its second direction
iShapeToCopyPositionAlongDir1
Specifies the position of the original shape iShapeToCopy
among its copies along iDir1
iShapeToCopyPositionAlongDir2
Specifies the position of the original shape iShapeToCopy
among its copies along iDir2
iDir1
The line or linear edge that specifies the pattern first repartition
direction
The following
objects are supported:
,
,
.
iDir2
The line or linear edge that specifies the pattern second repartition
direction
The following
objects are supported:
,
,
.
iIsReversedDir1
The boolean flag indicating whether the natural orientation of
iDir1 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir1.
iIsReversedDir2
The boolean flag indicating whether the natural orientation of
iDir2 should be used to orient the pattern operation.
True indicates that iShapeToCopy is copied in the
direction of the natural orientation of iDir2.
iRotationAngle
The angle applied to both directions iDir1 and iDir2
prior to applying the pattern.
The original shape iShapeToCopy is used as the rotation center.
Nevertheless, the copied shapes themselves are not rotated.
This allows the definition of a rectangular pattern
relatively to existing geometry, but not necessarily parallel to it.
Returns:
The created rectangular pattern
Func AddNewSurfacicSewSurface( iType, iSupportSurface, iSewingElement, iSewingSide) As
Creates and returns a new volume sewing operation within the current OGS/GS.
Parameters:
iType
Parameter to determine the sewing type. For Volume sewing Type = 4
iSupportSurface
The surfacic support on which sew operation will be performed
iSewingElement
The face or skin or surface that will be sewn on the current volume support
iSewingSide
The specification for which side of the current volume should be kept
at the end of the sewing operation
Returns:
The created sewing operation
Func AddNewSurfacicUserPattern( iShapeToCopy, iNbOfCopies) As
Creates and returns a new GSD user pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the user pattern
iNbOfCopies
The number of times iShapeToCopy will be copied
Returns:
The created user pattern
Func AddNewThickSurface( iOffsetElement, iIsensOffset, iTopOffset, iBotOffset) As
Creates and returns a new ThickSurface feature.
Parameters:
iOffsetElement
The skin that will be thicken and added with the current body
iIsensOffset
The direction of the offset in regard to the direction of the normal
iTopOffset
The Offset between the iOffsetElement and the upper skin of the
resulting feature
iBotOffset
The Offset between the iOffsetElement and the lower skin of the
resulting feature
Returns:
The created ThickSurface feature
Func AddNewThickness( iFaceToThicken, iOffset) As
Creates and returns a new thickness within the current body.
Parameters:
iFaceToThicken
The first face to thicken in the thickening process.
New faces to thicken can be added to the thickness afterwards by using
methods offered by the created thickness
The following
object is supported:
.
iOffset
The thickness of material to be added on the external side of the face
iFaceToThicken during the thickening process
Returns:
The created thickness
Func AddNewThreadWithOutRef() As
Creates and returns a new thread\tap within the current body.
Returns:
The created Thread
Func AddNewThreadWithRef( iLateralFace, iLimitFace) As
Creates and returns a new thread\tap within the current body.
Parameters:
iLateralFace
The Face defining the support of thread\tap
The following
object is supported:
.
iLimitFacee
The Face defining the origin of the thread.
The following
object is supported:
.
Returns:
The created Thread
Func AddNewTrim( iBodyToTrim) As
Creates and returns a new Trim operation within the current body.
Parameters:
iBodyToTrim
The body to Trim with current body.
Returns:
The created Trim operation
Func AddNewTritangentFillet( iF1, iF2, iRemovedFace) As
Deprecated:
V5R14 #AddNewTritangentFillet
use AddNewSolidTritangentFillet or AddNewSurfaceTritangentFillet
depending on the type of fillet you want to create
Func AddNewUserPattern( iShapeToCopy, iNbOfCopies) As
Creates and returns a new user pattern within the current body.
Parameters:
iShapeToCopy
The shape to be copied by the user pattern
iNbOfCopies
The number of times iShapeToCopy will be copied
Returns:
The created user pattern
Func AddNewUserPatternofList( iShapeToCopy, iNbOfCopies) As
V5R8 Only: Creates and returns a new user pattern within the current body using a list of shapes.
Parameters:
iShapeToCopy
The shape to be copied by the user pattern
Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfCopies
The number of times iShapeToCopy will be copied
Returns:
The created user pattern
Func AddNewVolumeAdd( iBody1, iBody2, iType) As
Creates and returns a Volumic Add feature.
Parameters:
iBody1
The volume or body to be modified.
iBody2
The volume or body to be operated.
iType
iType = 0 if Part Design, = 4 if GSD.
Returns:
The created Volumic Add feature.
Func AddNewVolumeCloseSurface( iCloseElement) As
Creates and returns a new VolumeCloseSurface feature.
Parameters:
iCloseElement
The skin that will be closed and add with the current body
Returns:
The created CloseSurface feature
Func AddNewVolumeIntersect( iBody1, iBody2, iType) As
Creates and returns a Volumic Intersect feature.
Parameters:
iBody1
The volume or body to be modified.
iBody2
The volume or body to be operated.
iType
iType = 0 if Part Design, = 4 if GSD.
Returns:
The created Volumic Intersect feature.
Func AddNewVolumeRemove( iBody1, iBody2, iType) As
Creates and returns a Volumic Remove feature.
Parameters:
iBody1
The volume or body to be modified.
iBody2
The volume or body to be operated.
iType
iType = 0 if Part Design, = 4 if GSD.
Returns:
The created Volumic Remove feature.
Func AddNewVolumeSewSurface( iType, iSupportVolume, iSewingElement, iSewingSide) As
Creates and returns a new volume sewing operation within the current OGS/GS.
Parameters:
iType
Parameter to determine the sewing type. For Volume sewing Type = 4
iSupportVolume
The volume support on which sew operation will be performed
iSewingElement
The face or skin or surface that will be sewn on the current volume support
iSewingSide
The specification for which side of the current volume should be kept
at the end of the sewing operation
Returns:
The created sewing operation
Func AddNewVolumeShell( iFaceToRemove, iInternalThickness, iExternalThickness, iVolumeSupport) As
Creates and returns a Volumic Shell feature.
Parameters:
iFacesToRemove
The Faces of the Volume
iFacesToThicken
The Faces of the Volume
iInternalThickness
The thickness of material to be added on the internal side of all the faces
during the shell process, except for those to be removed
iExternaThickness
The thickness of material to be added on the external side of all the faces
during the shell process, except for those to be removed
iVolumeSupport
The Volume related the faces to remove and faces to thicken
Returns:
The created Volumic Shell.
Func AddNewVolumeThickSurface( iOffsetElement, iIsensOffset, iTopOffset, iBotOffset) As
Creates and returns a new VolumeThickSurface feature.
Parameters:
iOffsetElement
The skin that will be thicken and added with the current OGS/GS
iIsensOffset
The direction of the offset in regard to the direction of the normal
iTopOffset
The Offset between the iOffsetElement and the upper skin of the
resulting feature
iBotOffset
The Offset between the iOffsetElement and the lower skin of the
resulting feature
Returns:
The created ThickSurface feature
Func AddNewVolumeThickness( iFaceToThicken, iOffset, iType, iVolumeSupport) As
Creates and returns a volume new thickness within the current GS or OGS.
Parameters:
iFaceToThicken
The first face to thicken in the thickening process.
New faces to thicken can be added to the thickness afterwards by using
methods offered by the created thickness
The following
object is supported:
.
iOffset
The thickness of material to be added on the external side of the face
iFaceToThicken during the thickening process
iType
The mode of thickness creation (4=Volume)
iVolumeSupport
The support volume for volumic draft
Returns:
The created thickness
Func AddNewVolumeTrim( iSupportVolume, iCuttingVolume) As
Creates and returns a new Volume Trim operation within the GS/OGS.
Parameters:
iSupportVolume
The Support Volume
iCutttingVolume
The trimming Volume
Returns:
The created Trim operation
Func AddNewVolumicDraft( iFaceToDraft, iNeutral, iNeutralMode, iParting, iDirX, iDirY, iDirZ, iMode, iAngle, iMultiselectionMode, iType, iVolumeSupport) As
Creates and returns a new volume draft within the current body.
The draft needs a reference face on the body. This face will remain
unchanged in the draft operation, while faces adjacent to it
and specified for drafting will be rotated by the draft angle.
Parameters:
iFaceToDraft
The first face to draft in the body. This face should be adjacent to the
iFaceToDraft face. If several faces are to be drafted, only the
first one is specified here, the others being inferred by propagating the
draft operation onto faces adjacent to this first face. This is
controlled by the iNeutralMode argument.
The following
object is supported:
.
iNeutral
The reference face for the draft. The draft needs a reference face on
the body, that will remain unchanged in the draft operation, while faces
adjacent to it and specified for drafting will be rotated according
to the draft angle iAngle.
The following
object is supported:
.
iNeutralMode
Controls if and how the drafting operation should be propagated beyond the
first face to draft iFaceToDraft to other adjacent faces.
iParting
The draft parting plane, face or surface.
It specifies the element within the body to draft
that represents the bottom of the mold. This element can be located either
somewhere in the middle of the body or be one of its boundary faces.
When located in the middle of the body, it crosses the faces to draft,
and as a result, those faces are drafted with a positive angle on one
side of the parting surface, and with a negative angle on the other side.
The following
object is supported:
.
iDirX,iDirY,iDirZ
The X, Y, and Z components of the absolute vector representing the drafting
direction (i.e. the mold extraction direction).
iMode
The draft connecting mode to its reference face iFaceToDraft
iAngle
The draft angle
iMultiselectionMode.
The elements to be drafted can be selected explicitly
or can implicitly selected as neighbors of the neutral face
iType
The mode of draft creation (4=Volume)
iVolumeSupport
The support volume for volumic draft
Returns:
The created draft
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Shell_14270 ===
PartInterfaces Shell (Object)
All Frameworks
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Shell (Object)
Represents the shell shape.
A shell shape is made up of a list of faces to process
and two thickness parameters.
Property Index
ExternalThickness
Returns the shell external thickness.
FacesToRemove
Returns the collection of faces to be removed by the shell process.
InternalThickness
Returns the shell internal thickness.
Method Index
AddFaceToRemove
Adds a new face to those to be removed by the shell process.
AddFaceWithDifferentThickness
Adds a new face to be thicken with different offset values.
RemoveFaceWithDifferentThickness
Removes an existing face from those to be thicken with different
offset values by the shell process.
SetVolumeSupport
Set the Support Volume of the faces to modify during Shell operation.
WithdrawFaceToRemove
Withdraws an existing face from those to be removed
by the shell process.
Properties
Property ExternalThickness() As   (Read Only)
Returns the shell external thickness.
Example:
The following example returns in extThick
the external thickness of the shell firstShell:
Set extThick = firstShell.ExternalThickness
Property FacesToRemove() As   (Read Only)
Returns the collection of faces to be removed by the shell process.
Example:
The following example returns in list the faces
to be removed from the shell firstShell:
Set list = firstShell.FacesToRemove
Property InternalThickness() As   (Read Only)
Returns the shell internal thickness.
Example:
The following example returns in intThick
the internal thickness of the shell firstShell:
Set intThick = firstShell.InternalThickness
Methods
Sub AddFaceToRemove( iFaceToRemove)
Adds a new face to those to be removed by the shell process.
Parameters:
iFaceToRemove
The face to be removed
The following
object is supported:
.
Example:
The following example adds the new face face
to be removed in the shell firstShell:
call firstShell.AddFaceToRemove(face)
Sub AddFaceWithDifferentThickness( iFaceToThicken)
Adds a new face to be thicken with different offset values.
Parameters:
iFaceToThicken
The face to be thicken with different offset values
The following
object is supported:
.
Example:
The following example adds the new face face
to be thicken with different offset values
in the shell firstShell:
call firstShell.AddFaceWithDifferentThickness(face)
Sub RemoveFaceWithDifferentThickness( iFaceToRemove)
Removes an existing face from those to be thicken with different
offset values by the shell process.
Parameters:
iFaceToRemove
The face to be removed from the shell specifications
The following
object is supported:
.
Example:
The following example removes the face face from the list
of faces in the shell firstShell:
call firstShell.RemoveFaceWithDifferentThickness(face)
Sub SetVolumeSupport( iVolumeSupport)
Set the Support Volume of the faces to modify during Shell operation.
Sub WithdrawFaceToRemove( iFaceToWithdraw)
Withdraws an existing face from those to be removed
by the shell process.
Parameters:
iFaceToWithdraw
The face to be withdrawn from the shell
The following
object is supported:
.
Example:
The following example removes the face face from the list of
faces in the shell firstShell:
call firstShell.WithdrawFaceToRemove(face)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_SketchBasedShape_25190 ===
PartInterfaces SketchBasedShape (Object)
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SketchBasedShape (Object)
Represents the shapes based on sketched 2D geometry.
It is the base object for prisms, holes, revolutions, stiffeners, and sweeps.
See also:
, , , ,
Property Index
Sketch
Returns the sketch the shape is based on.
Method Index
SetProfileElement
Returns or sets a profile element.
Properties
Property Sketch() As   (Read Only)
Returns the sketch the shape is based on.
Example:
The following example returns the sketch a pad
named firstPad is based on:
Set sketchPad = firstPad.Sketch
Methods
Sub SetProfileElement( iProfileElement)
Returns or sets a profile element.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Slot_13886 ===
PartInterfaces Slot (Object)
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Slot (Object)
Represents the slot shape.
The slot shape is made up of a profile represented by a sketch
swept along a center curve represented by another sketch.
This is a "negative" shape: it removes material from the body it
belongs to.
The profile sketch is usually drawn on another shape face.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_SolidCombine_19954 ===
PartInterfaces SolidCombine (Object)
All Frameworks
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SolidCombine (Object)
The interface to access a CATIASolidCombine.
Property Index
FirstComponentDirection
Returns or sets the direction of first component of SolidCombine.
FirstComponentProfile
Returns or sets the profile of first component of SolidCombine.
SecondComponentDirection
Returns or sets the direction of second component of SolidCombine.
SecondComponentProfile
Returns or sets the profile of second component of SolidCombine.
Properties
Property FirstComponentDirection() As
Returns or sets the direction of first component of SolidCombine.
Example:
The following example returns in firstDirection the direction of
first component of firstSolidCombine SolidCombine feature, and then sets
it to the firstDirection2 direction element.
Set firstDirection = firstSolidCombine.FirstComponentDirection
Set firstSolidCombine.FirstComponentDirection = firstDirection2
Property FirstComponentProfile() As
Returns or sets the profile of first component of SolidCombine.
Example:
The following example returns in firstProfile the profile of
first component of firstSolidCombine SolidCombine feature, and then sets
it to the firstProfile2 profile element:
Set firstProfile = firstSolidCombine.FirstComponentProfile
Set firstSolidCombine.FirstComponentProfile = firstProfile2
Property SecondComponentDirection() As
Returns or sets the direction of second component of SolidCombine.
Example:
The following example returns in secondDirection the direction of
second component of firstSolidCombine SolidCombine feature, and then sets
it to the secondDirection2 direction element.
Set secondDirection = firstSolidCombine.SecondComponentDirection
Set firstSolidCombine.SecondComponentDirection = secondDirection2
Property SecondComponentProfile() As
Returns or sets the profile of second component of SolidCombine.
Example:
The following example returns in secondProfile the profile of
second component of firstSolidCombine SolidCombine feature, and then sets
it to the secondProfile2 profile element:
Set secondProfile = firstSolidCombine.SecondComponentProfile
Set firstSolidCombine.SecondComponentProfile = secondProfile2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Split_14315 ===
PartInterfaces Split (Object)
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Split (Object)
Represents the split operation.
It splits a shape using a splitting element,
such as a surface, a face or a plane.
Property Index
SplittingSide
Returns or sets the splitting side .
Properties
Property SplittingSide() As
Returns or sets the splitting side .
The splitting side is the side of the splitting element
kept after the split.
A positive side refers to the same orientation
than the splitting element normal vector.
Example:
The following example returns in sptSide the splitting side
of the split shape mySplit, and then sets it to
catPositiveSide:
Set sptSide = mySplit.SplittingSide
mySplit.SplittingSide = catPositiveSide
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Stiffener_17032 ===
PartInterfaces Stiffener (Object)
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Stiffener (Object)
Represents the stiffener shape.
A stiffener is made up of a sketch used as the stiffener profile,
that is extruded (offset) and that fills the nearest shape.
This is a "positive" shape: it adds material to the body it
belongs to.
Property Index
IsFromTop
Returns or sets whether the stiffener is From Side or From Top.
IsSymmetric
Returns or sets whether the stiffener is symmetric.
Thickness
Returns the stiffener thickness.
ThicknessFromTop
Returns the stiffener thickness top in case of From Top stiffener.
Method Index
ReverseDepth
Reverses the stiffener direction.
ReverseThickness
Reverses the stiffener thickness direction.
Properties
Property IsFromTop() As
Returns or sets whether the stiffener is From Side or From Top.
True if the stiffener is From Top stiffener with respect to
the base sketch.
False if the stiffener is From Side stiffener with respect to
the base sketch.
Example:
The following example returns in FromTopFlag
whether the firstStiffener stiffener is From Top,
and then sets it as From Top stiffener with respect to its base sketch:
Set FromTopFlag = firstStiffener.IsFromTop
firstStiffener.IsFromTop  = True
Property IsSymmetric() As
Returns or sets whether the stiffener is symmetric.
True if the stiffener is symmetric with respect to
the base sketch.
Example:
The following example returns in symFlag
whether the firstStiffener stiffener is symmetric,
and then sets it as symmetric with respect to its base sketch:
Set symFlag = firstStiffener.IsSymmetric
firstStiffener.IsSymmetric  = True
Property Thickness() As   (Read Only)
Returns the stiffener thickness.
This is half of the thickness if the stiffener is symmetrical,
and the thickness otherwise.
Example:
The following example returns in thickness the thickness
of the firstStiffener stiffener:
Set thickness = firstStiffener.Thickness
Property ThicknessFromTop() As   (Read Only)
Returns the stiffener thickness top in case of From Top stiffener.
This is equal to first thickness if the stiffener is symmetrical,
Example:
The following example returns in thicknessfromtop the thickness
of the firstStiffener stiffener:
Set thicknessfromtop = firstStiffener.ThicknessFromTop
Methods
Sub ReverseDepth()
Reverses the stiffener direction.
This is useful for finding the shape to reach.
Example:
The following example reverses the current direction of
the firstStiffener stiffener:
firstStiffener.ReverseDepth
Sub ReverseThickness()
Reverses the stiffener thickness direction.
The stiffener thickness is swapped with respect to
the base sketch.
Example:
The following example reverses the current direction of
the firstStiffener stiffener:
firstStiffener.ReverseThickness
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_SurfaceBasedShape_26733 ===
PartInterfaces SurfaceBasedShape (Object)
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SurfaceBasedShape (Object)
Represents the shapes based on Surface.
It is the base object for Split , SewSurface , CloseSurface and
ThickSurface shapes.
See also:
, , ,
Property Index
Surface
Returns or sets the surface.
Properties
Property Surface() As
Returns or sets the surface.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Sweep_14280 ===
PartInterfaces Sweep (Object)
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Sweep (Object)
Represents the sweep shape.
It is the base object for ribs and slots.
Property Index
AnchorDirReverse
Returns the Sweep AnchorDirReverse flag (for Sweep Move Profile only).
CenterCurve
Returns the sketch used as the sweep center curve.
CenterCurveElement
Returns or sets the center curve .
IsThin
Returns the Sweep thin flag.
MergeEnd
Returns the Sweep merge end flag (for thin Sweep only).
MergeMode
Returns or sets the end mode .
MoveProfileToPath
Returns the Sweep MoveProfileToPath flag (for Sweep Move Profile only).
NeutralFiber
Returns the Sweep neutral fiber flag (for thin Sweep only).
NormalAxisDirReverse
Returns the Sweep NormalAxisDirReverse flag (for Sweep Move Profile only).
PullingDirElement
Returns or sets the pulling direction .
ReferenceSurfaceElement
Returns or sets the reference surface .
Method Index
SetKeepAngleOption
Actives KeepAngleOption.
Properties
Property AnchorDirReverse() As
Returns the Sweep AnchorDirReverse flag (for Sweep Move Profile only).
It returns TRUE if Anchor direction is reversed , FALSE if not.
Returns:
oAnchorDirReverse   The oAnchorDirReverse flag as a boolean
Example:
Property CenterCurve() As   (Read Only)
Returns the sketch used as the sweep center curve.
The sweep is built along this sketch.
Example:
The following example returns in centerCurve
the sketch used as center curve by the
firstSweep sweep object:
Set centerCurve = firstSweep.CenterCurve
Property CenterCurveElement() As
Returns or sets the center curve .
To set the property, you can use the following
object:
.
Property IsThin() As
Returns the Sweep thin flag.
It returns TRUE if the Sweep is a thin Sweep , FALSE if not.
Returns:
oIsThin   The thin flag as a boolean
Example:
The following example saves in thinFlag the thin flag of
Sweep firstSweep, and then sets it so that it will be now thin :
Set thinFlag = firstSweep.IsThin
firstSweep.IsThin = TRUE
Property MergeEnd() As
Returns the Sweep merge end flag (for thin Sweep only).
It returns TRUE if merge ends is required , FALSE if not.
Returns:
oIsMergeEnd   The merge end flag as a boolean
Example:
The following example saves in MergeEndFlag the merge end flag of
Sweep firstSweep, and then sets it so that merge end will be required :
Set MergeEndFlag = firstSweep.IsMergeEnd
firstSweep.IsMergeEnd = TRUE
Property MergeMode() As
Returns or sets the end mode .
Property MoveProfileToPath() As
Returns the Sweep MoveProfileToPath flag (for Sweep Move Profile only).
It returns TRUE if move profile is required , FALSE if not.
Returns:
oIsMoveProfileToPath   The MoveProfileToPath flag as a boolean
Example:
Property NeutralFiber() As
Returns the Sweep neutral fiber flag (for thin Sweep only).
It returns TRUE if the Sweep is a neutral fiber Sweep , FALSE if not.
Returns:
oIsNeutralFiber   The neutral fiber flag as a boolean
Example:
The following example saves in NeutralFiberFlag the neutral fiber flag of
Sweep firstSweep, and then sets it so that it will be now neutral fiber :
Set NeutralFiberFlag = firstSweep.IsNeutralFiber
firstSweep.IsNeutralFiber = TRUE
Property NormalAxisDirReverse() As
Returns the Sweep NormalAxisDirReverse flag (for Sweep Move Profile only).
It returns TRUE if Normal Axis direction is reversed , FALSE if not.
Returns:
oNormalAxisDirReverse   The oNormalAxisDirReverse flag as a boolean
Example:
Property PullingDirElement() As
Returns or sets the pulling direction .
To set the property, you can use one of the following
objects:
,
,
,
.
Property ReferenceSurfaceElement() As
Returns or sets the reference surface .
To set the property, you can use the following
object:
.
Methods
Sub SetKeepAngleOption()
Actives KeepAngleOption.
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Symmetry_16389 ===
PartInterfaces Symmetry (Object)
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Symmetry (Object)
Represents the shape symmetry feature object.
This solid feature is created from
an underlying HybridShapeSymmetry aggregated by the Symmetry.
Role: To access the data of the symmetry shape feature object.
The data includes:
The element to be transformed
The reference element which can be a point, a line or a plane
Use the CATIAShapeFactory to create ShapeFeature object.
See also:
Property Index
HybridShape
Gets the underlying HybridShapeSymmetry.
Properties
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeSymmetry.
Example:
The following example explains how to retrieve the underlying HybridShape Symmetry
Dim oHybridShape as AnyObject
Set oHybridShape=oSymmetry.HybridShape
oHybridShape.SectionCoupling = 2
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Thickness_17128 ===
PartInterfaces Thickness (Object)
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Thickness (Object)
Represents the thickness shape.
The thickness shape is made up of a collection of faces to process
and an offset parameter.
Property Index
FacesToThicken
Returns the collection of faces to be thickened.
Offset
Returns the thickness offset.
Method Index
AddFaceToThicken
Adds a new face to be thickened.
AddFaceWithDifferentThickness
Adds a new face to thicken with a different offset value.
RemoveFaceWithDifferentThickness
Removes an existing thickened face.
SetVolumeSupport
Set support of Thickness feature.
WithdrawFaceToThicken
Withdraws an existing thickened face.
Properties
Property FacesToThicken() As   (Read Only)
Returns the collection of faces to be thickened.
Example:
The following example returns in list the list of faces of
the thickness firstThickness:
Set list = firstThickness.FacesToThicken
Property Offset() As   (Read Only)
Returns the thickness offset.
Example:
The following example returns in offset the offset of
the thickness firstThickness:
Set offset = firstThickness.Offset
Methods
Sub AddFaceToThicken( iFaceToThicken)
Adds a new face to be thickened.
Parameters:
iFaceToThicken
The new face to process
The following
object is supported:
.
Example:
The following example adds the new face face
to thicken for the thickness firstThickness:
call firstThickness.AddFaceToThicken(face)
Sub AddFaceWithDifferentThickness( iFaceToThicken)
Adds a new face to thicken with a different offset value.
Parameters:
iFaceToThicken
The new face to process
The following
object is supported:
.
Example:
The following example adds the new face face
to thicken with a different offset value
for the thickness firstThickness:
call firstThickness.AddFaceWithDifferentThickness(face)
Sub RemoveFaceWithDifferentThickness( iFaceToRemove)
Removes an existing thickened face.
Parameters:
iFaceToRemove
The face to remove
The following
object is supported:
.
Example:
The following example removes the existing face thickened
face from the thickness firstThickness:
call firstThickness.RemoveFaceWithDifferentThickness(face)(face)
Sub SetVolumeSupport( iVolumeSupport)
Set support of Thickness feature.
Sub WithdrawFaceToThicken( iFaceToWithdraw)
Withdraws an existing thickened face.
Parameters:
iFaceToWithdraw
The face to withdraw
The following
object is supported:
.
Example:
The following example withdraws the existing face thickened
face from the thickness firstThickness:
call firstThickness.WithdrawFaceToThicken(face)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_ThickSurface_19952 ===
PartInterfaces ThickSurface (Object)
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ThickSurface (Object)
Represents the ThickSurface feature.
It thicks surface using an offset element
(such as a surface or a skin) and two offset values
TopOffset and Botoffset.
TopOffset is the offset between the offset element and the
top skin of the feature.
BotOffset is the offset between the offset element and the
bottom skin of the feature.
Property Index
BotOffset
Returns the value of the bottom offset.
OffsetSide
Returns the offset direction (defines in regards of the normal
direction) .
TopOffset
Returns the value of the top offset.
Method Index
swap_OffsetSide
Swap the side of the offset.
Properties
Property BotOffset() As   (Read Only)
Returns the value of the bottom offset.
Example:
The following example returns in botoffset the bottom
offset of the thicksurface firstThickSurface:
Set botoffset = firstThickSurface.BotOffset
Property OffsetSide() As   (Read Only)
Returns the offset direction (defines in regards of the normal
direction) .
Example:
The following example returns in offsetside the side
of the ThickSurface firstThickSurface:
Set offsetside = firstThickSurface.OffsetSide
Property TopOffset() As   (Read Only)
Returns the value of the top offset.
Example:
The following example returns in topoffset the top offset
of the ThickSurface firstThickSurface:
Set topoffset = firstThickSurface.TopOffset
Methods
Sub swap_OffsetSide()
Swap the side of the offset.
Example:
The following example changes the side of the
ThickSurface firstThickSurface:
call firstThickSurface.swap_OffsetSide()
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Thread_14731 ===
PartInterfaces Thread (Object)
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Thread (Object)
Represents the Thread feature.
It threads or taps cylindrical surface .
Property Index
Depth
Returns the thread/tap depth.
Diameter
Returns the thread/tap diameter.
LateralFaceElement
Returns or sets the lateral face (must be cylindrical) .
LimitFaceElement
Returns or sets the limit face (must be planar ) .
Pitch
Returns the thread/tap pitch.
Side
Returns the  thread or tap side.
SupportDepth
Returns the depth of thread/tap support.
SupportDiameter
Returns the diameter of thread/tap support.
ThreadDescription
Returns the thread/tap description parameter.
Method Index
CreateStandardThreadDesignTable
Creates a Standard Thread design table .
CreateUserStandardDesignTable
Creates a UserStandard Thread design table .
ReverseDirection
Swap the direction of the thread or the tap.
SetExplicitPolarity
Sets the thread polarity explicit.
Properties
Property Depth() As
Returns the thread/tap depth.
Returns:
oDepth    Value of the thread/tap depth
Example:
The following example returns in Depth the depth of
thread firstthread:
Set Depth = firstthread.Depth
Property Diameter() As
Returns the thread/tap diameter.
Returns:
oDiameter    Value of the thread/tap diameter
Example:
The following example returns in ThreadDiameter the diameter of
thread firstthread:
Set ThreadDiameter = firstthread.Diameter
Property LateralFaceElement() As
Returns or sets the lateral face (must be cylindrical) .
To set the property, you can use the following
object:
.
Property LimitFaceElement() As
Returns or sets the limit face (must be planar ) .
To set the property, you can use the following
object:
.
Property Pitch() As
Returns the thread/tap pitch.
Returns:
oPitch    Value of the thread/tap pitch
Example:
The following example returns in ThreadPitch the thread pitch of
thread firstthread:
Set ThreadPitch = firstthread.ThreadPitch
Property Side() As
Returns the  thread or tap side.
Returns:
oThreadSide   The thread/tap side (see
for list of possible sides)
Example:
The following example returns in ThreadSide the thread/tap side of
thread firstthread:
Set ThreadSide = firstthreadoThreadSide
Property SupportDepth() As   (Read Only)
Returns the depth of thread/tap support.
Returns:
oSupportDepth    Value of the depth of thread/tap support
Example:
The following example returns in SupportDepth the support depth of
thread firstthread:
Set SupportDepth = firstthread.SupportDepth
Property SupportDiameter() As   (Read Only)
Returns the diameter of thread/tap support.
Returns:
oSupportDiameter    Value of the diameter of thread/tap support
Example:
The following example returns in SupportDiameter the support diameter of
thread firstthread:
Set SupportDiameter = firstthread.SupportDiameter
Property ThreadDescription() As   (Read Only)
Returns the thread/tap description parameter.
This call is valid only when a standard/user design table created
Returns:
oThreadDescParam    A Parameter object controlling the thread/tap description (see
for more information)
Example:
The following example returns in threadDescription the thread description (M12 etc) of
thread firstthread:
Set threadDescription = firstthread.ThreadDescription
Methods
Sub CreateStandardThreadDesignTable( iStandardType)
Creates a Standard Thread design table .
Parameters:
iStandardType
Standard type for thread (see
for list of possible types)
Example:
The following example creates a standard table for MetricThinPitch for
thread firstthread:
firstthread.CreateStandardThreadDesignTable catMetricThinPitch
Sub CreateUserStandardDesignTable( iStandardName, iPath)
Creates a UserStandard Thread design table .
Parameters:
iStandardName
Name of the UserStandard thread. iStandardName should be empty if filepath is to be defined.
iPath
Path of the UserStandard file. iPath is empty if the filepath is already defined through CATReffilesPath.
Example1:
The following example creates a standard table for UserStandard for
thread firstThread. The file path is already defined thru CATReffilesPath:
firstThread.CreateUserStandardDesignTable "UserStandard",""
Example2:
The following example creates a standard table for UserStandard for
thread firstThread when file path is not defined thru CATReffilesPath:
firstThread.CreateUserStandardDesignTable "","E:\user\standard\UserStandard.txt"
Sub ReverseDirection()
Swap the direction of the thread or the tap.
Sub SetExplicitPolarity( iThreadPolarity)
Sets the thread polarity explicit. Thread polarity is no more evaluated
implicitly on basis of support face polarity
Parameters:
iThreadPolarity
Standard type for thread (see
for list of possible types)
Example:
The following example sets the thread polarity to Tap explicitly
thread firstthread:
firstthread.SetExplicitPolarity catTap
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_TransformationShape_31098 ===
PartInterfaces TransformationShape (Object)
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TransformationShape (Object)
Represents the shapes based on a transformation of another shape.
It is the base object for mirrors and patterns.
See also:
, , ,
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Translate_17048 ===
PartInterfaces Translate (Object)
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Translate (Object)
Represents the hybrid shape translate feature object.
This solid feature is
created from an underlying HybridShapeTranslate aggregated by the Translate.
Role: To access the data of the hybrid shape translate feature object.
This data includes:
The element to translate
The translation direction
The translation distance and its value
Use the CATIAHybridShapeFactory to create HybridShapeFeature object.
See also:
Property Index
HybridShape
Gets the underlying HybridShapeTranslate.
Properties
Property HybridShape() As   (Read Only)
Gets the underlying HybridShapeTranslate.
Example:
The following example explains how to retrieve the underlying HybridShape Translate
Dim oHybridShape as AnyObject
Set oHybridShape=oTranslate.HybridShape
oHybridShape.ElemToTranslate = reference1
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_Trim_13859 ===
PartInterfaces Trim (Object)
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Trim (Object)
Represents the Trim, or union trim boolean operation.
It is performed between a body and the current shape.
Method Index
AddFaceToKeep
Adds a new face to be kept (if face is not divided by operation).
AddFaceToKeep2
Adds a new face to be kept (if face is divided by operation).
AddFaceToRemove
Adds a new face to be Removed (if face not divided by operation).
AddFaceToRemove2
Adds a new face to be Removed (if face is divided by operation).
WithdrawFaceToKeep
Withdraws an existing Kept face (if face is not divided by operation) .
WithdrawFaceToKeep2
Withdraws an existing Kept face (if face is divided by operation).
WithdrawFaceToRemove
Withdraws an existing Removed face (if face not divided by operation).
WithdrawFaceToRemove2
Withdraws an existing Removed face (if face is divided by operation).
Methods
Sub AddFaceToKeep( iFaceToKeep)
Adds a new face to be kept (if face is not divided by operation).
Parameters:
iFaceToKeep
The new face to process
The following
object is supported:
.
Example:
The following example adds the new face face
to Keep for the Trim firstTrim:
call firstTrim.AddFaceToKeep(face)
Sub AddFaceToKeep2( iFaceToKeep, iFaceAdjacentForKeep)
Adds a new face to be kept (if face is divided by operation).
Parameters:
iFaceToKeep
The new face to process
The following
object is supported:
.
iFaceAdjacentForKeep
An adjacent face of iFaceToKeep belonging to the other operand
The following
object is supported:
.
Example:
The following example adds the new face face
to Keep for the Trim firstTrim:
call firstTrim.AddFaceToKeep(face)
Sub AddFaceToRemove( iFaceToRemove)
Adds a new face to be Removed (if face not divided by operation).
Parameters:
iFaceToRemove
The new face to process
The following
object is supported:
.
Example:
The following example adds the new face face
to Remove for the Trim firstTrim:
call firstTrim.AddFaceToRemove(face)
Sub AddFaceToRemove2( iFaceToRemove, iFaceAdjacentForRemove)
Adds a new face to be Removed (if face is divided by operation).
Parameters:
iFaceToRemove
The new face to process
The following
object is supported:
.
iFaceAdjacentForRemove
An adjacent face of iFaceToRemove belonging to the other operand
The following
object is supported:
.
Example:
The following example adds the new face face
to Remove for the Trim firstTrim:
call firstTrim.AddFaceToRemove(face)
Sub WithdrawFaceToKeep( iFaceToWithdraw)
Withdraws an existing Kept face (if face is not divided by operation) .
Parameters:
iFaceToWithdraw
The face to withdraw
The following
object is supported:
.
Example:
The following example withdraws the existing face Kept
face from the Trim firstTrim:
call firstTrim.WithdrawFaceToKeep(face)
Sub WithdrawFaceToKeep2( iFaceToWithdraw, iFaceAdjacentForKeep)
Withdraws an existing Kept face (if face is divided by operation).
Parameters:
iFaceToWithdraw
The face to withdraw
The following
object is supported:
.
iFaceAdjacentForKeep
An adjacent face of iFaceToKeep belonging to the other operand
The following
object is supported:
.
Example:
The following example withdraws the existing face Kept
face from the Trim firstTrim:
call firstTrim.WithdrawFaceToKeep(face)
Sub WithdrawFaceToRemove( iFaceToWithdraw)
Withdraws an existing Removed face (if face not divided by operation).
Parameters:
iFaceToWithdraw
The face to withdraw
The following
object is supported:
.
Example:
The following example withdraws the existing face Removed
face from the Trim firstTrim:
call firstTrim.WithdrawFaceToRemove(face)
Sub WithdrawFaceToRemove2( iFaceToWithdraw, iFaceAdjacentForRemove)
Withdraws an existing Removed face (if face is divided by operation).
Parameters:
iFaceToWithdraw
The face to withdraw
The following
object is supported:
.
iFaceAdjacentForRemove
An adjacent face of iFaceToRemove belonging to the other operand
The following
object is supported:
.
Example:
The following example withdraws the existing face Removed
face from the Trim firstTrim:
call firstTrim.WithdrawFaceToRemove(face)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_TritangentFillet_25776 ===
PartInterfaces TritangentFillet (Object)
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TritangentFillet (Object)
The Tritangent Fillet feature : a fillet is built between 3 faces,
2 faces will be relimited, the third one ("face to remove") will
be used for fillet tangency ; this face will disappear within the resulting shape.
Property Index
FaceToRemove
Returns the face to be removed by the tritangent fillet.
FirstFace
Returns the first face limiting the tritangent fillet.
SecondFace
Returns the second face limiting the tritangent fillet.
Properties
Property FaceToRemove() As
Returns the face to be removed by the tritangent fillet.
Returns:
oFaceToRemove   The face to be removed by the fillet (@see CATIAReference for more information)
Example:
The following example returns in removedFace the face to be removed of
tritangent fillet firstTritangentFillet:
Set removedFace = firstTritangentFillet.FaceToRemove
Property FirstFace() As
Returns the first face limiting the tritangent fillet.
Returns:
oFirstFace   The limiting face (@see CATIAReference for more information)
Example:
The following example returns in face1 the first limiting face of
tritangent fillet firstTritangentFillet:
Set face1 = firstTritangentFillet.FirstFace
Property SecondFace() As
Returns the second face limiting the tritangent fillet.
Returns:
oSecondFace   The limiting face (@see CATIAReference for more information)
Example:
The following example returns in face2 the second limiting face of
tritangent fillet firstTritangentFillet:
Set face2 = firstTritangentFillet.SecondFace
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_UserPattern_19114 ===
PartInterfaces UserPattern (Object)
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UserPattern (Object)
Represents the user pattern.
The shape is copied along user's positions.
Property Index
AnchorPoint
Returns the anchor point of the user pattern.
FeatureToLocatePositions
Returns the collection of feature to locate instances.
Method Index
AddFeatureToLocatePositions
Adds a new feature to locate instances.
Properties
Property AnchorPoint() As
Returns the anchor point of the user pattern.
Example:
The following example returns in anchor the anchor point
of the Pattern firstPattern:
Set anchor = firstPattern.AnchorPoint
Property FeatureToLocatePositions() As   (Read Only)
Returns the collection of feature to locate instances.
Example:
The following example returns in list the list of feature
to locate instances of the Pattern firstPattern:
Set list = firstPattern.FeatureToLocatePositions
Methods
Sub AddFeatureToLocatePositions( iFeatureToLocatePositions)
Adds a new feature to locate instances.
Parameters:
iFeatureToLocatePositions
The new object containing points of positioning
Example:
The following example adds the new feature feature
to locate instances of the Pattern firstPattern:
call firstPattern.AddFeatureToLocatePositions(object)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_UserRepartition_24576 ===
PartInterfaces UserRepartition (Object)
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UserRepartition (Object)
Represents the User Pattern  repartition.
It is made up of a number of times the shape is copied and
the location of instances.
The number of times the shape is copied is accessible using
the  property.
Property Index
FeatureToLocatePositions
Returns the collection of feature to locate instances.
Method Index
AddFeatureToLocatePositions
Adds a new feature to locate instances.
Properties
Property FeatureToLocatePositions() As   (Read Only)
Returns the collection of feature to locate instances.
Example:
The following example returns in list the list of feature
to locate instances of the Pattern firstPattern:
Set list = firstPattern.FeatureToLocatePositions
Methods
Sub AddFeatureToLocatePositions( iFeatureToLocatePositions)
Adds a new feature to locate instances.
Parameters:
iFeatureToLocatePositions
The new face to process
Example:
The following example adds the new feature feature
to locate instances of the Pattern firstPattern:
call firstPattern.AddFeatureToLocatePositions(face)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.

=== interface_VarRadEdgeFillet_25223 ===
PartInterfaces VarRadEdgeFillet (Object)
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VarRadEdgeFillet (Object)
Represents the edge fillet shape with a variable radius.
The resulting shape is made up of
edges fillets controlled by couples of radius/vertex.
Property Index
BitangencyType
Returns or set the fillet bitangency type.
EdgesToFillet
Returns the collection of edges to be filleted.
FilletSpine
Returns or set the spine for circle bitangency fillet.
FilletVariation
Returns or sets the edge fillet radius variation mode.
ImposedVertices
Returns the collection of vertices where a radius has been imposed.
SharpEdgeRemovalMode
Returns or set the sharp edge removal mode for variable edge fillet.
Method Index
AddEdgeToFillet
Adds a new edge to the variable radius edge fillet.
AddImposedVertex
Adds a new control couple.
ImposedVertexRadius
Returns the fillet radius on an imposed vertex.
SwitchToConstFilletType
Changes the type of EdgeFillet to constant EdgeFillet and return it.
WithdrawEdgeToFillet
Withdraws an edge from the variable radius edge fillet.
WithdrawImposedVertex
Withdraws a control couple.
Properties
Property BitangencyType() As
Returns or set the fillet bitangency type.
Parameters:
iType
The type used to perform the fillet :
catSphereBitangencyType or catCircleBitangencyType
Property EdgesToFillet() As   (Read Only)
Returns the collection of edges to be filleted.
Example:
The following example returns in edges
the edges to fillet of
variable radius edge filletfirstVarEdgeFillet:
Set edges = firstVarEdgeFillet.EdgesToFillet
Property FilletSpine() As
Returns or set the spine for circle bitangency fillet.
Parameters:
iSpin
The spine to be used for a circle bitangency fillet
Property FilletVariation() As
Returns or sets the edge fillet radius variation mode.
Example:
The following example returns in mode the radius variation
mode of the variable radius edge filletfirstVarEdgeFillet,
and then sets it to CATLinearFilletVariation
so that the radius variation is linear between two control vertices:
mode = firstVarEdgeFillet.FilletVariation
firstVarEdgeFillet.FilletVariation = CATLinearFilletVariation
Property ImposedVertices() As   (Read Only)
Returns the collection of vertices where a radius has been imposed.
Example:
The following example returns in vertices
the collection of imposed vertices of the
variable radius edge filletfirstVarEdgeFillet:
Set vertices = firstVarEdgeFillet.ImposedVertices
Property SharpEdgeRemovalMode() As
Returns or set the sharp edge removal mode for variable edge fillet.
Parameters:
iMode
The mode to be used for variable edge fillet
Methods
Sub AddEdgeToFillet( iEdge, iRadius)
Adds a new edge to the variable radius edge fillet.
Parameters:
iEdge
The edge to be filleted
The following
object is supported:
.
iRadius
The radius to impose along the edge.
This radius is imposed at both end points of the edge.
Example:
The following example adds the new edge edge
to be filleted to the
variable radius edge fillet firstVarEdgeFillet:
call firstVarEdgeFillet.AddEdgeToFillet(edge, 5.)
Sub AddImposedVertex( iVertex, iRadius)
Adds a new control couple.
A control couple is made up of a vertex and a radius.
Parameters:
iVertex
The vertex where to impose the radius
iRadius
The radius to impose at the given vertex
Example:
The following example adds a new control couple (vertex, radius) to
the variable radius edge fillet firstVarEdgeFillet set
with the vertex vertex and a radius of 50.
call firstVarEdgeFillet.AddImposedVertex(vertex, 50.)
Func ImposedVertexRadius( iImposedVertex) As
Returns the fillet radius on an imposed vertex.
Parameters:
iImposedVertex
The vertex where to retrieve the fillet radius
Returns:
The fillet radius
Example:
The following example returns in radius
the fillet radius of the
variable radius edge fillet firstVarEdgeFillet
at the vertex vertex:
Set radius = firstVarEdgeFillet.ImposedVertexRadius(vertex)
Func SwitchToConstFilletType() As
Changes the type of EdgeFillet to constant EdgeFillet and return it.
Parameters:
opConstFillet
The opConstFillet is the variable edge fillet
Sub WithdrawEdgeToFillet( iEdge)
Withdraws an edge from the variable radius edge fillet.
Parameters:
iEdge
The edge to be withdrawn
The following
object is supported:
.
Example:
The following example withdraws the edge edge
from those to be filleted of the
variable radius edge fillet firstVarEdgeFillet:
call firstVarEdgeFillet.WithdrawEdgeToFillet(edge)
Sub WithdrawImposedVertex( iVertex)
Withdraws a control couple.
Parameters:
iVertex
The vertex where the radius is imposed
Example:
The following example withdraws the imposed radius on the vertex
vertex for the variable radius edge fillet
firstVarEdgeFillet:
call firstVarEdgeFillet.WithdrawImposedVertex(vertex)
Copyright © 1999-2019, Dassault Systèmes. All rights reserved.