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PartInterfaces Interface CATIPrtFactory

CATIPrtFactory
 

Usage: an implementation of this interface is supplied and you must use it as is. You should not reimplement it.


interface CATIPrtFactory

Interface to create all types of Mechanical Design feature.
Role: The CATIPrtfactory role is to build from scratch features that will be used within the design process of parts. In most cases, features are created from a factory with a minimum number of parameters. Other feature parameters will be set by using methods offered by the feature itself.


Method Index


o CreateAffinity(CATISpecObject_var&,CATISpecObject_var&,CATISpecObject_var&,CATISpecObject_var&,CATICkeParm_var&,CATICkeParm_var&,CATICkeParm_var&)
Creates and returns an Affinity feature.
o CreateAlign(CATISpecObject_var,CATPrtSplitType)
Creates and returns a replace face feature.
o CreateAxisToAxis(CATISpecObject_var&,CATISpecObject_var&,CATISpecObject_var&)
Creates and returns an AxisToAxis transformation feature.
o CreateChamfer(CATLISTV(CATISpecObject_var)*,CATPrtChamferPropagation,CATPrtChamferMode,double,double,CATPrtChamferReferenceFace,CATISpecObject_var,int)
Creates and returns a chamfer feature.
o CreateCircPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,int,int,double,double,int,int,double,CATBoolean,CATBoolean)
Creates and returns a new solid circular pattern.
o CreateCircPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,int,int,double,double,int,int,double,CATBoolean,CATBoolean,int)
o CreateClose(CATISpecObject_var)
o CreateCloseSurface(CATISpecObject_var)
Creates and returns a close feature.
o CreateDraft(CATLISTV(CATISpecObject_var)*,int,CATISpecObject_var,int,CATISpecObject_var,CATMathDirection,CATISpecObject_var,int,double,int)
Creates and returns a new draft.
o CreateFillet(CATIMfBRepFeature_var,CATIMfBRepFeature_var,CATIMfBRepFeature_var,CATISpecObject_var,int)
o CreateFillet(CATIMfBRepFeature_var,CATIMfBRepFeature_var,double,CATISpecObject_var,int)
o CreateFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATISpecObject_var,int)
o CreateFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATLISTV(CATISpecObject_var)*,CATISpecObject_var,int)
o CreateFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATISpecObject_var,int)
o CreateFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATLISTV(CATISpecObject_var)*,CATISpecObject_var,int)
o CreateGroove(CATISpecObject_var&)
Creates a new groove.
o CreateHole(CATISpecObject_var,CATISpecObject_var)
Creates and returns a new hole feature.
o CreateHole(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,int)
Creates and returns a new hole feature.
o CreateHole(CATMathPoint,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates and returns a new hole feature.
o CreateHole(CATMathPoint,CATISpecObject_var,CATISpecObject_var,int)
Creates and returns a new hole feature.
o CreateLoft()
Creates and returns a new loft feature.
o CreateMirror(CATISpecObject_var)
Creates and returns a new mirror.
o CreateOffset(CATISpecObject_var,CATPrtOffsetSens,double,double)
o CreatePad(CATISpecObject_var&)
Creates a new pad.
o CreatePocket(CATISpecObject_var&)
Creates a new pocket.
o CreateRectPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATBoolean,int,int,double,double,int,int,double)
Creates and returns a new solid rectangular pattern.
o CreateRectPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATBoolean,int,int,double,double,int,int,double,int)
o CreateRemovedLoft()
Creates and returns a new removed loft feature.
o CreateRib()
Creates and returns a new rib feature.
o CreateRib(CATISpecObject_var&,CATISpecObject_var&)
Creates and returns a new rib feature.
o CreateRotate(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var)
Creates and returns a Rotate feature.
o CreateScaling(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var)
Creates and returns a Scaling feature.
o CreateSewing(CATISpecObject_var,CATPrtSplitType)
Creates and returns a sewing feature.
o CreateShaft(CATISpecObject_var&)
Creates a new shaft.
o CreateShell(CATLISTV(CATISpecObject_var)*,double,double)
Creates and returns a shell feature.
o CreateSlot()
Creates and returns a new slot feature.
o CreateSlot(CATISpecObject_var&,CATISpecObject_var&)
Creates and returns a new slot feature.
o CreateSolidFillet(CATIMfBRep_var,CATIMfBRep_var,CATIMfBRep_var,CATISpecObject_var)
Creates and returns a tritangent fillet feature.
o CreateSolidFillet(CATIMfBRep_var,CATIMfBRep_var,double,CATISpecObject_var)
Creates and returns a solid face fillet feature.
o CreateSolidFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATISpecObject_var)
Creates and returns a solid variable edge fillet feature.
o CreateSolidFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATLISTV(CATISpecObject_var)*,CATISpecObject_var)
Creates and returns a variable solid edge fillet feature with Keep Edge.
o CreateSolidFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATISpecObject_var)
Creates and returns a solid constant edge fillet feature.
o CreateSolidFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATLISTV(CATISpecObject_var)*,CATISpecObject_var)
Creates and returns a solid constant edge fillet feature with Keep Edge.
o CreateSolidOffset(CATISpecObject_var,CATPrtOffsetSens,double,double)
Creates and returns an offset feature.
o CreateSolidSplit(CATISpecObject_var,CATPrtSplitType)
Creates and returns a split feature.
o CreateSplit(CATISpecObject_var,CATPrtSplitType)
o CreateStiffener(CATISpecObject_var&)
Creates a new stiffener.
o CreateSurfaceFillet(CATIMfBRep_var,CATIMfBRep_var,CATIMfBRep_var,CATISpecObject_var)
Creates and returns a tritangent fillet feature.
o CreateSurfaceFillet(CATIMfBRep_var,CATIMfBRep_var,double,CATISpecObject_var)
Creates and returns a surface face fillet feature.
o CreateSurfaceFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATISpecObject_var)
Creates and returns a surface variable edge fillet feature.
o CreateSurfaceFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,CATPrtFilletVariation,CATLISTV(CATISpecObject_var)*,CATISpecObject_var)
Creates and returns a variable surfacic edge fillet feature with Keep Edge.
o CreateSurfaceFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATISpecObject_var)
Creates and returns a surface constant edge fillet feature.
o CreateSurfaceFillet(CATLISTV(CATISpecObject_var)*,CATPrtFilletPropagation,double,CATLISTV(CATISpecObject_var)*,CATISpecObject_var)
Creates and returns a surface constant edge fillet feature with Keep Edge.
o CreateSurfacicCircPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,int,int,double,double,int,int,double,CATBoolean,CATBoolean)
Creates and returns a new surfacic or volumic circular pattern.
o CreateSurfacicRectPatt(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATBoolean,int,int,double,double,int,int,double)
Creates and returns a new surfacic or volumic rectangular pattern.
o CreateSurfacicUserPatt(CATISpecObject_var,int,CATLISTV(CATISpecObject_var),CATISpecObject_var)
Creates and returns a new surfacic or volumic user pattern.
o CreateSymmetry(CATISpecObject_var,CATISpecObject_var)
Creates and returns a Symmetry feature.
o CreateThickness(CATLISTV(CATISpecObject_var)*,double)
Creates and returns a thickness feature.
o CreateThread()
Creates and returns a new thread feature.
o CreateThread(CATISpecObject_var,CATISpecObject_var)
Creates and returns a thread feature.
o CreateTranslate(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var)
Creates and returns a Translate feature.
o CreateUserPatt(CATISpecObject_var,int,CATLISTV(CATISpecObject_var),CATISpecObject_var)
Creates and returns a new solid user pattern.
o CreateVolumicCloseSurface(CATISpecObject_var)
Creates and returns a volumic close feature.
o CreateVolumicDraft(CATLISTV(CATISpecObject_var)*,int,CATISpecObject_var,int,CATISpecObject_var,CATMathDirection,CATISpecObject_var,int,double,int,CATISpecObject_var)
Creates and returns a volumic draft feature.
o CreateVolumicDraft(CATLISTV(CATISpecObject_var)*,int,CATISpecObject_var,int,CATISpecObject_var,CATMathDirection,CATISpecObject_var,int,double,int,int,CATISpecObject_var)
o CreateVolumicDraftAngle()
Creates and returns a Draft feature in volumic context.
o CreateVolumicDraftAngle(int&)
o CreateVolumicOffset(CATISpecObject_var,CATPrtOffsetSens,double,double)
Creates and returns a volumic offset feature.
o CreateVolumicSewing(int&,CATISpecObject_var&,CATISpecObject_var,CATPrtSplitType)
Creates and returns a volumic sewing feature.
o CreateVolumicShell(CATISpecObject_var,CATLISTV(CATISpecObject_var)*,double,double)
Creates and returns a volumic shell feature.
o CreateVolumicShell(int,CATISpecObject_var,CATLISTV(CATISpecObject_var)*,double,double)
o CreateVolumicThickness(CATLISTV(CATISpecObject_var)*,double,CATISpecObject_var)
Creates and returns a thickness feature.

Methods


o CreateAffinity
public virtual CATISpecObject_var CreateAffinity( const CATISpecObject_var& ihElemToTransfor,
const CATISpecObject_var& ihAxisOrigin,
const CATISpecObject_var& ihAxisPlane,
const CATISpecObject_var& ihAxisFirstDirection,
const CATICkeParm_var& ihRatioX,
const CATICkeParm_var& ihRatioY,
const CATICkeParm_var& ihRatioZ) = 0
Creates and returns an Affinity feature.
Parameters:
ihElemToTransfor
The object on which Affinity transformation will be applied.
ihAxisOrigin
Origin for the affinity.
ihAxisPlane
Plane for the affinity.
ihAxisFirstDirection
Direction for the affinity.
ihRatioX
XRatio Value for the affinity.
ihRatioY
YRatio Value for the affinity.
ihRatioZ
ZRatio Value for the affinity.
Returns:
The created Affinity feature.
o CreateAlign
public virtual CATISpecObject_var CreateAlign( const CATISpecObject_var ihAlignPlane,
const CATPrtSplitType iAlignType) = 0
Creates and returns a replace face feature.
Parameters:
ihAlignPlane
The surfacic feature to be used to perform the replace operation.
iAlignType
Represents the side to be kept after the replace operation.
Legal values: iAlignType equals PositiveSide or NegativeSide. The PositiveSide value refers to the same orientation as the replacing element normal vector. The NegativeSide value refers to the opposite orientation as the replacing element normal vector.
Returns:
the created replace face feature.
o CreateAxisToAxis
public virtual CATISpecObject_var CreateAxisToAxis( const CATISpecObject_var& ihToTransform,
const CATISpecObject_var& ihReferenceAxis,
const CATISpecObject_var& ihTargetAxis)= 0
Creates and returns an AxisToAxis transformation feature.
Parameters:
ihToTransform
The object on which AxisToAxis transformation will be applied.
ihReferenceAxis
The refrence axis.
ihTargetAxis
The target axis.
Returns:
The created AxisToAxis feature.
o CreateChamfer
public virtual CATISpecObject_var CreateChamfer( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtChamferPropagation iPropagationMode,
const CATPrtChamferMode iParameterMode,
const double iLength1,
const double iLength2,
const CATPrtChamferReferenceFace iReferenceFace= NO_REVERSE,
const CATISpecObject_var ihSupport=NULL_var,
const int iContext= -1) = 0
Creates and returns a chamfer feature.
Parameters:
iObjectList
Specifies the list of sharp edges or faces to be chamfered.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when chamfering.
The propagation can be performed in two ways:
Tangency: CATIA continues chamfering beyond the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtChamferPropagation propagation mode can be set to _TANGENCY or _MINIMAL.
iParameterMode
The chamfer parameter mode specifies both parameters required to define the chamfer: two lengthes (Length1/Length2) or a length and an angle (Length1/Angle).
Legal values: The CATPrtChamferMode parameter mode can be set to LENGTH or LENGTH_ANGLE.
iLength1
This is the first length value if the chamfer is defined with two lengthes, or if the chamfer is defined with a length and an angle.
Legal values: The first length value must be greater than 0 but not equal to 0.
iLength2
This is the second length value if the chamfer is defined with two lengthes, or the angle value if the chamfer is defined with a length and an angle.
Legal values: The second length value must be greater than 0 but not equal to 0 and the angle value must be greater than 0 but not equal to 0 and smaller than 90 but not equal to 90.
iReferenceFace
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 be chamfered.
This reference face is either the face selected or the face determined by CATIA if the edge to be chamfered was selected.
The chamfer orientation defines whether to keep the face selected or determined by CATIA as the chamfer reference face.
Legal values: The CATPrtChamferReferenceFace orientation can be set to NO_REVERSE (the chamfer reference face is the face selected or determined by CATIA) or REVERSE (the chamfer reference face is the other face).
ihSupport
Do not use this parameter.
iContext
Specifies the chamfer context. Set to 5 for Functional Chamfer.
Returns:
The created chamfer feature.
o CreateCircPatt
public virtual CATISpecObject_var CreateCircPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var iDir,
const CATISpecObject_var iPto,
const CATBoolean iSensa,
const int iNbr,
const int iNba,
const double iStepr,
const double iStepa,
const int iNr,
const int iNa,
const double iRotationAngle,
const CATBoolean iInstRot,
const CATBoolean iCompleteCrown) = 0
Creates and returns a new solid circular pattern.
Parameters:
ihMotif
The feature to be duplicated with the circular pattern.
iDir
The line or linear edge that specifies the axis around which duplications will be rotated relative to each other.
iPto
The point or vertex that specifies the pattern rotation center.
iSensa
The boolean flag indicating the natural orientation of iDir used to orientate the pattern operation. A value of true indicates that ihMotif are duplicated in the direction of the natural orientation of iDir.
iNbr
The number of times that ihMotif will be duplicated along pattern radial direction.
Legal values: iNbr must be greater or equal than 1.
iNba
The number of times that ihMotif will be duplicated along pattern angular direction.
Legal values: iNba must be greater or equal than 1.
iStepr
The distance that will separate two consecutive duplications in the pattern along its radial direction.
Legal values: iStepr must be greater than 0 but not equal to 0.
iStepa
The angle that will separate two consecutive duplications in the pattern along its angular direction.
Legal values: iStepa must be greater than 0 but not equal to 0.
iNr
Specifies the position of the original feature ihMotif among its duplications along the radial direction.
iNa
Specifies the position of the original feature ihMotif among its duplications along the angular direction.
iRotationAngle
Do not use, iRotationAngle must be already equal to 0.
iInstRot
The boolean flag that specifies:
True to keep the same orientation of ihMotif for its duplications.
False to orientate the duplications of ihMotif same according to the radial direction.
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.
o CreateCircPatt
public virtual CATISpecObject_var CreateCircPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var iDir,
const CATISpecObject_var iPto,
const CATBoolean iSensa,
const int iNbr,
const int iNba,
const double iStepr,
const double iStepa,
const int iNr,
const int iNa,
const double iRotationAngle,
const CATBoolean iInstRot,
const CATBoolean iCompleteCrown,
const int iContext) = 0
Deprecated:
V5R15 #CreateCircPatt(const CATISpecObject_var ihMotif, const CATISpecObject_var iDir, const CATISpecObject_var iPto, const CATBoolean iSensa, const int iNbr, const int iNba, const double iStepr, const double iStepa, const int iNr, const int iNa, const double iRotationAngle, const CATBoolean iInstRot, const CATBoolean iCompleteCrown)
o CreateClose
public virtual CATISpecObject_var CreateClose( const CATISpecObject_var ihCloseElement) = 0
Deprecated:
V5R15 #CreateClose use CreateCloseSurface
o CreateCloseSurface
public virtual CATISpecObject_var CreateCloseSurface( const CATISpecObject_var ihCloseElement) = 0
Creates and returns a close feature.
Parameters:
ihCloseElement
The surfacic feature to be closed.
Returns:
The created close feature.
o CreateDraft
public virtual CATISpecObject_var CreateDraft( const CATLISTV(CATISpecObject_var)* ihSupportToDraft,
const int iBid1,
const CATISpecObject_var ihNeutral,
const int iBid2,
const CATISpecObject_var ihParting,
const CATMathDirection iPullDir,
const CATISpecObject_var ihPullDirSpec,
const int iMode,
const double iAngle,
const int iBid4) = 0
Creates and returns a new draft. Drafts are defined on molded parts to make them easier to remove from molds.
Parameters:
ihSupportToDraft
The list of faces to be drafted.
Legal values: The CATISpecObject_var must be a face.
NULL_var value is not allowed.
iBid1
Not used. Must be set to 0.
ihNeutral
The neutral element. The intersection of this element and the faces to be drafted, defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft. The neutral element and parting element may be the same element.
Legal values: The CATISpecObject_var could be a plane, a face or a surface.
NULL_var value is not allowed.
iBid2
Not used. Must be set to 0.
ihParting
The parting element. This element cuts the faces to be drafted in two and one portion is drafted according to its previously defined pulling direction. The parting element and neutral element may be the same element.
Legal values: The CATISpecObject_var could be a plane, a face or a surface.
NULL_var value means the draft has no parting element.
iPullDir
The pulling direction. This is the direction in which the mold will be removed from the part.
ihPullDirSpec
The pulling direction reference.
Precondition: If you used a reference, you must set the pulling direction iPullDir with the CATMathDirection of the reference.
Legal values: The CATISpecObject_var is either a plane or a planar face or a planar surface the pulling direction is normal to this element, a line or a linear edge the pulling direction is the direction of the element. NULL_var there is no pulling direction reference.
iMode
The draft mode (standard or reflectline).
Legal values: The Draft mode is either 0 standard (the draft's neutral element must be input). 1 reflectline (the draft's neutral element is computed as the reflect line).
iAngle
The draft angle value.
Legal values: Angle between -90 degrees (not included) and +90 degrees (not included). The value should be set in degree.
iBid4
Not used. Must be set to 0.
Returns:
The created draft.
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATIMfBRepFeature_var ihRsur1,
const CATIMfBRepFeature_var ihRsur2,
const CATIMfBRepFeature_var ihRemoveRsur,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R15 #CreateFillet use CATISpecObject_var CreateSolidFillet (const CATIMfBRep_var ihRsur1, const CATIMfBRep_var ihRsur2, const CATIMfBRep_var ihRemoveRsur, const CATISpecObject_var ihSupport=NULL_var) = 0; or CATISpecObject_var CreateSurfaceFillet (const CATIMfBRep_var ihRsur1, const CATIMfBRep_var ihRsur2, const CATIMfBRep_var ihRemoveRsur, const CATISpecObject_var ihSupport=NULL_var) = 0; depending of the type of the fillet you want to create.
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATIMfBRepFeature_var ihRsur1,
const CATIMfBRepFeature_var ihRsur2,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R14 #CreateFillet use CreateSolidFillet (const CATIMfBRep_var ihRsur1, const CATIMfBRep_var ihRsur2, const double iRadius, const CATISpecObject_var ihSupport=NULL_var) = 0; or CreateSurfaceFillet (const CATIMfBRep_var ihRsur1, const CATIMfBRep_var ihRsur2, const double iRadius, const CATISpecObject_var ihSupport=NULL_var) = 0; depending on the type of fillet.
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R14 #CreateFillet use CATISpecObject_var CreateSolidFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const CATPrtFilletVariation iVariationMode, const CATISpecObject_var ihSupport=NULL_var) = 0; or CATISpecObject_var CreateSurfaceFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const CATPrtFilletVariation iVariationMode, const CATISpecObject_var ihSupport=NULL_var) = 0; depending of the type of the fillet you want to create
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R14 #CreateFillet use CATISpecObject_var CreateSolidFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const CATPrtFilletVariation iVariationMode, const CATLISTV(CATISpecObject_var)* iKeepEdgeList, const CATISpecObject_var ihSupport=NULL_var) = 0; or CATISpecObject_var CreateSurfaceFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const CATPrtFilletVariation iVariationMode, const CATLISTV(CATISpecObject_var)* iKeepEdgeList, const CATISpecObject_var ihSupport=NULL_var) = 0; depending on the type of the fillet
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R14 #CreateFillet use CATISpecObject_var CreateSolidFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const double iRadius, const CATISpecObject_var ihSupport=NULL_var) = 0; or CATISpecObject_var CreateSurfaceFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const double iRadius, const CATISpecObject_var ihSupport=NULL_var) = 0; depending of the type of the fillet you want to create
o CreateFillet
public virtual CATISpecObject_var CreateFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var,
const int iType= -1) = 0
Deprecated:
V5R14 #CreateFillet use CATISpecObject_var CreateSolidFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const double iRadius,const CATLISTV(CATISpecObject_var)* iKeepEdgeList, const CATISpecObject_var ihSupport=NULL_var) = 0; or CATISpecObject_var CreateSurfaceFillet (const CATLISTV(CATISpecObject_var)* iObjectList, const CATPrtFilletPropagation iPropagationMode ,const double iRadius,const CATLISTV(CATISpecObject_var)* iKeepEdgeList, const CATISpecObject_var ihSupport=NULL_var) = 0; depending of the type of fillet you want to create
o CreateGroove
public virtual CATISpecObject_var CreateGroove( const CATISpecObject_var& ihSketch= NULL_var) = 0
Creates a new groove.
Parameters:
ihSketch
The sketch defining the groove profile.
It must contain an axis used as revolution axis.
Returns:
The groove feature.
o CreateHole
public virtual CATISpecObject_var CreateHole( const CATISpecObject_var ihSurface,
const CATISpecObject_var ihDirection) = 0
Creates and returns a new hole feature.
Parameters:
ihSurface
Selected face or plane used as support for the hole feature.
ihDirection
Selected direction.
Returns:
The hole feature.
o CreateHole
public virtual CATISpecObject_var CreateHole( const CATISpecObject_var ihPoint,
const CATISpecObject_var ihSurface,
const CATISpecObject_var ihDirection,
const int IsPointOnSurface) = 0
Creates and returns a new hole feature.
Parameters:
ihPoint
Selected point uses to locate the hole feature on its support
ihSurface
Selected face used as support for the hole feature.
ihDirection
Selected direction.
IsPointOnSurface

= 0 if ihPoint does not lay down support (ihSurface).
= 1 if ihPoint lays down support (ihSurface).
Returns:
The Hole feature.
o CreateHole
public virtual CATISpecObject_var CreateHole( const CATMathPoint iMathPoint,
const CATISpecObject_var ihFirstEdge,
const CATISpecObject_var ihSecndEdge,
const CATISpecObject_var ihSurface,
const CATISpecObject_var iDirection) = 0
Creates and returns a new hole feature. This method creates a constraint in positionning sketch between hole origine and selected edge .
Parameters:
iMathPoint
Coordinates of the point uses to locate the hole feature on its support.
ihFirstEdge
First selected edge.
ihSecndEdge
Second selected edge.
ihSurface
Selected face used as support for the hole feature.
ihDirection
Selected direction.
Returns:
The hole feature.
o CreateHole
public virtual CATISpecObject_var CreateHole( const CATMathPoint iMathPoint,
const CATISpecObject_var ihSurface,
const CATISpecObject_var ihDirection,
const int IsPointOnSurface) = 0
Creates and returns a new hole feature.
Parameters:
iMathPoint
Coordinates of the point uses to locate the hole feature on its support.
ihSurface
Selected face used as support for the hole feature.
ihDirection
Selected direction.
IsPointOnSurface

= 0 if iMathPoint doesn't lay down support (ihSurface).
= 1 if iMathPoint lays down support (ihSurface).
Returns:
The hole feature.
o CreateLoft
public virtual CATISpecObject_var CreateLoft()= 0
Creates and returns a new loft feature.
Returns:
The loft feature.
o CreateMirror
public virtual CATISpecObject_var CreateMirror( const CATISpecObject_var ihSymPlane) = 0
Creates and returns a new mirror. A mirror allows users for transforming by duplication existing feature by a symmetry with respect to an existing plane.
Parameters:
ihSymPlane
The plane used by the mirror as the symmetry plane.
Returns:
The created mirror.
o CreateOffset
public virtual CATISpecObject_var CreateOffset( const CATISpecObject_var ihSurface,
const CATPrtOffsetSens iIsensOffset,
double iTopOffset,
double iBotOffset) = 0
Deprecated:
V5R15 #CreateOffset use CreateSolidOffset
o CreatePad
public virtual CATISpecObject_var CreatePad( const CATISpecObject_var& ihSketch= NULL_var) = 0
Creates a new pad.
Parameters:
ihSketch
The sketch defining the pad profile.
Returns:
The pad feature.
o CreatePocket
public virtual CATISpecObject_var CreatePocket( const CATISpecObject_var& ihSketch= NULL_var) = 0
Creates a new pocket.
Parameters:
ihSketch
The sketch defining the pocket profile.
Returns:
The pocket feature.
o CreateRectPatt
public virtual CATISpecObject_var CreateRectPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var ihLine1,
const CATISpecObject_var ihLine2,
const CATBoolean iDir1,
const CATBoolean iDir2,
const int iNb1,
const int iNb2,
const double iStep1,
const double iStep2,
const int iNu,
const int iNv,
const double iRotationAngle) = 0
Creates and returns a new solid rectangular pattern.
Parameters:
ihMotif
The feature to be duplicated with the rectangular pattern.
ihLine1
The line or linear edge that specifies the pattern first distribution direction.
iLine2
The line or linear edge that specifies the pattern second distribution direction.
iDir1
The boolean flag indicating if the natural orientation of iLine1 used to orientate the pattern operation. True indicates that ihMotif is duplicated in the direction of the natural orientation of iLine1.
iDir2
The boolean flag indicating if the natural orientation of iLine2 used to orientate the pattern operation. True indicates that ihMotif is duplicated in the direction of the natural orientation of iLine2.
iNb1
The number of times that ihMotif will be duplicated along the pattern first direction. ihMotif is the first instance.
Legal values: iNb1 must be greater or equal than 1.
iNb2
The number of times that ihMotif will be duplicated along the pattern second direction.
Legal values: iNb2 must be greater or equal than 1.
iStep1
The distance that will separate two consecutive duplications in the pattern along its first direction.
Legal values: iStep1 must be greater than 0 but not equal to 0.
iStep2
The distance that will separate two consecutive duplications in the pattern along its second direction.
Legal values: iStep2 must be greater than 0 but not equal to 0.
iNu
Specifies the position of the original feature ihMotif among its duplications along iLine1.
Legal values: iNu must be greater or equal than 1 and less or equal than iNb1.
iNv
Specifies the position of the original feature ihMotif among its duplications along iLine2.
Legal values: iNv must be greater or equal than 1 and less or equal than iNb2.
iRotationAngle
The angle between the real pattern directions and the two defined directions iLine1 and iLine2, in case of two defined directions only. The original feature ihMotif is used as the rotation center. Nevertheless the duplicated shapes are not own rotated.
Returns:
The created rectangular pattern.
o CreateRectPatt
public virtual CATISpecObject_var CreateRectPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var ihLine1,
const CATISpecObject_var ihLine2,
const CATBoolean iDir1,
const CATBoolean iDir2,
const int iNb1,
const int iNb2,
const double iStep1,
const double iStep2,
const int iNu,
const int iNv,
const double iRotationAngle,
const int iContext) = 0
Deprecated:
V5R15 #CreateRectPatt(const CATISpecObject_var ihMotif, const CATISpecObject_var ihLine1, const CATISpecObject_var ihLine2, const CATBoolean iDir1, const CATBoolean iDir2, const int iNb1, const int iNb2, const double iStep1, const double iStep2, const int iNu, const int iNv, const double iRotationAngle)
o CreateRemovedLoft
public virtual CATISpecObject_var CreateRemovedLoft()= 0
Creates and returns a new removed loft feature.
Returns:
The removed loft feature.
o CreateRib
public virtual CATISpecObject_var CreateRib()= 0
Creates and returns a new rib feature.
Returns:
The rib feature.
o CreateRib
public virtual CATISpecObject_var CreateRib( const CATISpecObject_var& ihSketch,
const CATISpecObject_var& ihCenterCrv) = 0
Creates and returns a new rib feature.
Parameters:
ihSketch
Selected profile.
ihCenterCrv
Selected center curve.
Returns:
The rib feature.
o CreateRotate
public virtual CATISpecObject_var CreateRotate( const CATISpecObject_var ihToRotate,
const CATISpecObject_var ihAxis,
const CATICkeParm_var ihAngle) = 0
Creates and returns a Rotate feature.
Parameters:
ihToRotate
The object on which rotate will be applied.
ihAxis
The rotation axis.
ihAngle
The rotation angle.
Returns:
The created Rotate feature.
o CreateScaling
public virtual CATISpecObject_var CreateScaling( const CATISpecObject_var ihToScale,
const CATISpecObject_var ihReference,
const CATICkeParm_var ihRatio) = 0
Creates and returns a Scaling feature.
Parameters:
ihToScale
The object on which scaling will be applied.
ihReference
The scaling reference element.
ihRatio
The scaling ratio.
Returns:
The created Scaling feature.
o CreateSewing
public virtual CATISpecObject_var CreateSewing( const CATISpecObject_var ihSewingPlane,
const CATPrtSplitType iSewingType) = 0
Creates and returns a sewing feature.
Parameters:
ihSewingPlane
The surfacic feature to be sewn to perform the sewing operation.
iSewingType
Represents the side to be kept after the sewing operation.
Legal values: iSewingType equals PositiveSide or NegativeSide. The PositiveSide value refers to the same orientation as the sewing element normal vector. The NegativeSide value refers to the opposite orientation as the sewing element normal vector.
Returns:
the created sewing feature.
o CreateShaft
public virtual CATISpecObject_var CreateShaft( const CATISpecObject_var& ihSketch= NULL_var) = 0
Creates a new shaft.
Parameters:
ihSketch
The sketch defining the shaft profile.
It must contain an axis used as revolution axis.
Returns:
The shaft feature.
o CreateShell
public virtual CATISpecObject_var CreateShell( const CATLISTV(CATISpecObject_var)* ihObjectList,
double iIntOffset,
double iExtOffset) = 0
Creates and returns a shell feature.
Parameters:
ihObjectList
The list of the faces which corresponds to the shell openings.
iIntOffset
The internal offset value.
iExtOffset
The external offset value.
Returns:
The created shell feature.
o CreateSlot
public virtual CATISpecObject_var CreateSlot()= 0
Creates and returns a new slot feature.
Returns:
The slot feature.
o CreateSlot
public virtual CATISpecObject_var CreateSlot( const CATISpecObject_var& ihSketch,
const CATISpecObject_var& ihCenterCrv) = 0
Creates and returns a new slot feature.
Parameters:
ihSketch
Selected profile.
ihCenterCrv
Selected center curve.
Returns:
The slot feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATIMfBRep_var ihRsur1,
const CATIMfBRep_var ihRsur2,
const CATIMfBRep_var ihRemoveRsur,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a tritangent fillet feature.
Parameters:
ihRsur1
Specifies the first face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRsur2
Specifies the second face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRemoveRsur
Specifies the face to be removed. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created tritangent fillet feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATIMfBRep_var ihRsur1,
const CATIMfBRep_var ihRsur2,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a solid face fillet feature.
Parameters:
ihRsur1
Specifies the first face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRsur2
Specifies the second face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
iRadius
Specifies the radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
ihSupport
Do not use this parameter.
Returns:
The created Face Fillet feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a solid variable edge fillet feature.
Postcondition: It just adds the edges to the fillet. So you have to use AddFilletRadius method of CATIEdgeFillet on the edge to add vertices for computing variable fillet.
Parameters:
iObjectList
Specifies the list of sharp edges to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iVariationMode
The variation mode specifies the way the fillet shape changes from one radius to another.
The variation can be performed in two ways:
Cubic: The fillet changes smoothly from one radius to another.
Linear: The fillet changes straight from one radius to another.
Legal values: The CATPrtFilletVariation variation mode can be set to CUBIC or LINEAR.
ihSupport
Do not use this parameter.
Returns:
The created variable edge fillet feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a variable solid edge fillet feature with Keep Edge.
Precondition: only for edge fillets with constant radius.
Postcondition: It just adds the edges to the fillet. So you have to use AddFilletRadius method of CATIEdgeFillet on the edge to add vertices for computing variable fillet.
Parameters:
iObjectList
Specifies the list of sharp edges to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iVariationMode
The variation mode specifies the way the fillet shape changes from one radius to another.
The variation can be performed in two ways:
Cubic: The fillet changes smoothly from one radius to another.
Linear: The fillet changes straight from one radius to another.
Legal values: The CATPrtFilletVariation variation mode can be set to CUBIC or LINEAR.
iKeepEdgeList
Specifies the list of sharp edges that must not be modified.
The CATISpecObject_var should be a Redge (CATIMfRedge) feature created with CATIMfBRepFactory. This edge should not be already used in the fillet. This edge should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created variable edge fillet feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a solid constant edge fillet feature.
Parameters:
iObjectList
Specifies the list of sharp edges or faces to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iRadius
Specifies the constant radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
ihSupport
Do not use this parameter.
Returns:
The created constant edge fillet feature.
o CreateSolidFillet
public virtual CATISpecObject_var CreateSolidFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a solid constant edge fillet feature with Keep Edge.
Parameters:
iObjectList
Specifies the list of sharp edges or faces to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iRadius
Specifies the constant radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
iKeepEdgeList
Specifies the list of sharp edges that must not be modified.
The CATISpecObject_var should be a Redge (CATIMfRedge) feature created with CATIMfBRepFactory. This edge should not be already used in the fillet. This edge should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created constant edge fillet feature.
o CreateSolidOffset
public virtual CATISpecObject_var CreateSolidOffset( const CATISpecObject_var ihSurface,
const CATPrtOffsetSens iIsensOffset,
double iTopOffset,
double iBotOffset) = 0
Creates and returns an offset feature.
Parameters:
ihSurface
The surfacic feature to be offseted to perform an offset operation.
iIsensOffset
Represents the orientation of the offset.
Legal values: iIsensOffset equals NormalSide or InverseNormalSide. The NormalSide value refers to the same orientation as the normal vector of the surfacic feature. The InverseNormalSide value refers to the opposite orientation as the normal vector of the surfacic feature.
iTopOffset
Represents the offset value between the surfacic feature to be offseted and the top skin of the offset feature.
iBotOffset
Represents the offset value between the surfacic feature to be offseted and the bottom skin of the offset feature.
Returns:
the created offset feature.
o CreateSolidSplit
public virtual CATISpecObject_var CreateSolidSplit( const CATISpecObject_var ihSplitPlane,
const CATPrtSplitType iSplitType) = 0
Creates and returns a split feature.
Parameters:
ihSplitPlane
The surfacic feature as splitting element to perform the split operation.
iSplitType
Represents the side to be kept after the split operation.
Legal values: iSplitType equals PositiveSide or NegativeSide. The PositiveSide value refers to the same orientation as the splitting element normal vector. The NegativeSide value refers to the opposite orientation as the splitting element normal vector.
Returns:
the created split feature.
o CreateSplit
public virtual CATISpecObject_var CreateSplit( const CATISpecObject_var ihSplitPlane,
const CATPrtSplitType iSplitType) = 0
Deprecated:
V5R15 #CreateSplit use CreateSplitSolid
o CreateStiffener
public virtual CATISpecObject_var CreateStiffener( const CATISpecObject_var& ihSketch= NULL_var) = 0
Creates a new stiffener.
Parameters:
ihSketch
The sketch defining the stiffener profile.
It must be an open profile.
Returns:
The stiffener feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATIMfBRep_var ihRsur1,
const CATIMfBRep_var ihRsur2,
const CATIMfBRep_var ihRemoveRsur,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a tritangent fillet feature.
Parameters:
ihRsur1
Specifies the first face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRsur2
Specifies the second face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRemoveRsur
Specifies the face to be removed. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created tritangent fillet feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATIMfBRep_var ihRsur1,
const CATIMfBRep_var ihRsur2,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a surface face fillet feature.
Parameters:
ihRsur1
Specifies the first face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
ihRsur2
Specifies the second face to be filleted. The CATIMfBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMfBRepFactory. This face should not be already used in the fillet. This face should belong to the same mechanical body.
iRadius
Specifies the radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
ihSupport
Do not use this parameter.
Returns:
The created Face Fillet feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a surface variable edge fillet feature.
Postcondition: It just adds the edges to the fillet. So you have to use AddFilletRadius method of CATIEdgeFillet on the edge to add vertices for computing variable fillet.
Parameters:
iObjectList
Specifies the list of sharp edges to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iVariationMode
The variation mode specifies the way the fillet shape changes from one radius to another.
The variation can be performed in two ways:
Cubic: The fillet changes smoothly from one radius to another.
Linear: The fillet changes straight from one radius to another.
Legal values: The CATPrtFilletVariation variation mode can be set to CUBIC or LINEAR.
ihSupport
Do not use this parameter.
Returns:
The created variable edge fillet feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const CATPrtFilletVariation iVariationMode,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a variable surfacic edge fillet feature with Keep Edge.
Precondition: only for edge fillets with constant radius.
Postcondition: It just adds the edges to the fillet. So you have to use AddFilletRadius method of CATIEdgeFillet on the edge to add vertices for computing variable fillet.
Parameters:
iObjectList
Specifies the list of sharp edges to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iVariationMode
The variation mode specifies the way the fillet shape changes from one radius to another.
The variation can be performed in two ways:
Cubic: The fillet changes smoothly from one radius to another.
Linear: The fillet changes straight from one radius to another.
Legal values: The CATPrtFilletVariation variation mode can be set to CUBIC or LINEAR.
iKeepEdgeList
Specifies the list of sharp edges that must not be modified.
The CATISpecObject_var should be a Redge (CATIMfRedge) feature created with CATIMfBRepFactory. This edge should not be already used in the fillet. This edge should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created variable edge fillet feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a surface constant edge fillet feature.
Parameters:
iObjectList
Specifies the list of sharp edges or faces to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iRadius
Specifies the constant radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
ihSupport
Do not use this parameter.
Returns:
The created constant edge fillet feature.
o CreateSurfaceFillet
public virtual CATISpecObject_var CreateSurfaceFillet( const CATLISTV(CATISpecObject_var)* iObjectList,
const CATPrtFilletPropagation iPropagationMode,
const double iRadius,
const CATLISTV(CATISpecObject_var)* iKeepEdgeList,
const CATISpecObject_var ihSupport=NULL_var) = 0
Creates and returns a surface constant edge fillet feature with Keep Edge.
Parameters:
iObjectList
Specifies the list of sharp edges or faces to be filleted.
The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature created with CATIMfBRepFactory. This edge or face should not be already used in the fillet. This edge or face should belong to the same mechanical body.
iPropagationMode
The propagation mode specifies the edges taken into account when filleting.
The propagation can be performed in two ways:
Tangency:CATIA continues filleting belong the selected edge until it encounters an edge that is non continuous in tangency.
Minimal: The propagation is done up to the first natural relimitation by the geometry.
Legal values: The CATPrtFilletPropagation propagation mode can be set to TANGENCY or MINIMAL.
iRadius
Specifies the constant radius value.
Legal values: The radius value must be greater than 0 but not equal to 0.
iKeepEdgeList
Specifies the list of sharp edges that must not be modified.
The CATISpecObject_var should be a Redge (CATIMfRedge) feature created with CATIMfBRepFactory. This edge should not be already used in the fillet. This edge should belong to the same mechanical body.
ihSupport
Do not use this parameter.
Returns:
The created constant edge fillet feature.
o CreateSurfacicCircPatt
public virtual CATISpecObject_var CreateSurfacicCircPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var iDir,
const CATISpecObject_var iPto,
const CATBoolean iSensa,
const int iNbr,
const int iNba,
const double iStepr,
const double iStepa,
const int iNr,
const int iNa,
const double iRotationAngle,
const CATBoolean iInstRot,
const CATBoolean iCompleteCrown) = 0
Creates and returns a new surfacic or volumic circular pattern.
Parameters:
ihMotif
The feature to be duplicated with the circular pattern.
iDir
The line or linear edge that specifies the axis around which duplications will be rotated relative to each other.
iPto
The point or vertex that specifies the pattern rotation center.
iSensa
The boolean flag indicating the natural orientation of iDir used to orientate the pattern operation. A value of true indicates that ihMotif are duplicated in the direction of the natural orientation of iDir.
iNbr
The number of times that ihMotif will be duplicated along pattern radial direction.
Legal values: iNbr must be greater or equal than 1.
iNba
The number of times that ihMotif will be duplicated along pattern angular direction.
Legal values: iNba must be greater or equal than 1.
iStepr
The distance that will separate two consecutive duplications in the pattern along its radial direction.
Legal values: iStepr must be greater than 0 but not equal to 0.
iStepa
The angle that will separate two consecutive duplications in the pattern along its angular direction.
Legal values: iStepa must be greater than 0 but not equal to 0.
iNr
Specifies the position of the original feature ihMotif among its duplications along the radial direction.
iNa
Specifies the position of the original feature ihMotif among its duplications along the angular direction.
iRotationAngle
Do not use, iRotationAngle must be already equal to 0.
iInstRot
The boolean flag that specifies:
True to keep the same orientation of ihMotif for its duplications.
False to orientate the duplications of ihMotif same according to the radial direction.
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.
o CreateSurfacicRectPatt
public virtual CATISpecObject_var CreateSurfacicRectPatt( const CATISpecObject_var ihMotif,
const CATISpecObject_var ihLine1,
const CATISpecObject_var ihLine2,
const CATBoolean iDir1,
const CATBoolean iDir2,
const int iNb1,
const int iNb2,
const double iStep1,
const double iStep2,
const int iNu,
const int iNv,
const double iRotationAngle) = 0
Creates and returns a new surfacic or volumic rectangular pattern.
Parameters:
ihMotif
The feature to be duplicated with the rectangular pattern.
ihLine1
The line or linear edge that specifies the pattern first distribution direction.
iLine2
The line or linear edge that specifies the pattern second distribution direction.
iDir1
The boolean flag indicating if the natural orientation of iLine1 used to orientate the pattern operation. True indicates that ihMotif is duplicated in the direction of the natural orientation of iLine1.
iDir2
The boolean flag indicating if the natural orientation of iLine2 used to orientate the pattern operation. True indicates that ihMotif is duplicated in the direction of the natural orientation of iLine2.
iNb1
The number of times that ihMotif will be duplicated along the pattern first direction. ihMotif is the first instance.
Legal values: iNb1 must be greater or equal than 1.
iNb2
The number of times that ihMotif will be duplicated along the pattern second direction.
Legal values: iNb2 must be greater or equal than 1.
iStep1
The distance that will separate two consecutive duplications in the pattern along its first direction.
Legal values: iStep1 must be greater than 0 but not equal to 0.
iStep2
The distance that will separate two consecutive duplications in the pattern along its second direction.
Legal values: iStep2 must be greater than 0 but not equal to 0.
iNu
Specifies the position of the original feature ihMotif among its duplications along iLine1.
Legal values: iNu must be greater or equal than 1 and less or equal than iNb1.
iNv
Specifies the position of the original feature ihMotif among its duplications along iLine2.
Legal values: iNv must be greater or equal than 1 and less or equal than iNb2.
iRotationAngle
The angle between the real pattern directions and the two defined directions iLine1 and iLine2, in case of two defined directions only. The original feature ihMotif is used as the rotation center. Nevertheless the duplicated shapes are not own rotated.
Returns:
The created rectangular pattern.
o CreateSurfacicUserPatt
public virtual CATISpecObject_var CreateSurfacicUserPatt( const CATISpecObject_var ihMotif,
const int iNbCopy,
const CATLISTV(CATISpecObject_var) iObjectList,
const CATISpecObject_var ihStepElt) = 0
Creates and returns a new surfacic or volumic user pattern.
Parameters:
ihMotif
The feature to be duplicated by the user pattern.
iNbCopy
The number of times that ihMotif will be duplicated.
iObjectList
The list must be composed of one sketch of points to locate duplications.
ihStepElt
Do not use, ihStepElt must be equal to NULL_var.
Returns:
The created user pattern.
o CreateSymmetry
public virtual CATISpecObject_var CreateSymmetry( const CATISpecObject_var ihSpec,
const CATISpecObject_var ihPlane)=0
Creates and returns a Symmetry feature.
Parameters:
ihSpec
The object on which symmetry will be applied.
ihPlane
The plane used as mirroring element.
Returns:
The created Symmetry feature.
o CreateThickness
public virtual CATISpecObject_var CreateThickness( const CATLISTV(CATISpecObject_var)* ihObjectList,
double iOffset) = 0
Creates and returns a thickness feature.
Parameters:
ihObjectList
The list of the faces which corresponds to the shell openings.
iOffset
The offset value.
Returns:
The created Thickness feature.
o CreateThread
public virtual CATISpecObject_var CreateThread()= 0
Creates and returns a new thread feature.
Returns:
The thread feature.
o CreateThread
public virtual CATISpecObject_var CreateThread( const CATISpecObject_var ihSupportElement,
const CATISpecObject_var ihLimitElement) = 0
Creates and returns a thread feature.
Parameters:
ihSupportElement
Face to thread or to tap.
ihLimitElement
Face to limit top of thread or tap.
Returns:
The created thread feature.
o CreateTranslate
public virtual CATISpecObject_var CreateTranslate( const CATISpecObject_var ihSpecToTranslate,
const CATIGSMDirection_var ihDirection,
const CATICkeParm_var ihDistance)=0
Creates and returns a Translate feature.
Parameters:
ihSpecToTranslate
The object on which translation will be applied.
ihDirection
The translation direction.
ihDistance
The translation length.
Returns:
The created Symmetry feature.
o CreateUserPatt
public virtual CATISpecObject_var CreateUserPatt( const CATISpecObject_var ihMotif,
const int iNbCopy,
const CATLISTV(CATISpecObject_var) iObjectList,
const CATISpecObject_var ihStepElt) = 0
Creates and returns a new solid user pattern.
Parameters:
ihMotif
The feature to be duplicated by the user pattern.
iNbCopy
The number of times that ihMotif will be duplicated.
iObjectList
The list must be composed of one sketch of points to locate duplications.
ihStepElt
Do not use, ihStepElt must be equal to NULL_var.
Returns:
The created user pattern.
o CreateVolumicCloseSurface
public virtual CATISpecObject_var CreateVolumicCloseSurface( const CATISpecObject_var ihCloseElement) = 0
Creates and returns a volumic close feature.
Parameters:
ihCloseElement
The surfacic feature to be closed.
Returns:
The created close feature.
o CreateVolumicDraft
public virtual CATISpecObject_var CreateVolumicDraft( const CATLISTV(CATISpecObject_var)* ihSupportToDraft,
const int iBid1,
const CATISpecObject_var ihNeutral,
const int iBid2,
const CATISpecObject_var ihParting,
const CATMathDirection iPullDir,
const CATISpecObject_var ihPullDirSpec,
const int iMode,
const double iAngle,
const int iBid4,
const CATISpecObject_var hSupport) = 0
Creates and returns a volumic draft feature. Drafts are defined on molded parts to make them easier to remove from molds.
Parameters:
ihSupportToDraft
The list of faces to be drafted.
Legal values: The CATISpecObject_var must be a face.
NULL_var value is not allowed.
iBid1
Not used. Must be set to 0.
ihNeutral
The neutral element. The intersection of this element and the faces to be drafted, defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft. The neutral element and parting element may be the same element.
Legal values: The CATISpecObject_var could be a plane, a face or a surface.
NULL_var value is not allowed.
iBid2
Not used. Must be set to 0.
ihParting
The parting element. This element cuts the faces to be drafted in two and one portion is drafted according to its previously defined pulling direction. The parting element and neutral element may be the same element.
Legal values: The CATISpecObject_var could be a plane, a face or a surface.
NULL_var value means the draft has no parting element.
iPullDir
The pulling direction. This is the direction in which the mold will be removed from the part.
ihPullDirSpec
The pulling direction reference.
Precondition: If you used a reference, you must set the pulling direction iPullDir with the CATMathDirection of the reference.
Legal values: The CATISpecObject_var is either a plane or a planar face or a planar surface the pulling direction is normal to this element, a line or a linear edge the pulling direction is the direction of the element. NULL_var there is no pulling direction reference.
iMode
The draft mode (standard or reflectline).
Legal values: The Draft mode is either 0 standard (the draft's neutral element must be input). 1 reflectline (the draft's neutral element is computed as the reflect line).
iAngle
The draft angle value.
Legal values: Angle between -90 degrees (not included) and +90 degrees (not included). The value should be set in degree.
iBid4
Not used. Must be set to 0.
hSupport
The volumic feature to be operated.
Returns:
The created volumic draft.
o CreateVolumicDraft
public virtual CATISpecObject_var CreateVolumicDraft( const CATLISTV(CATISpecObject_var)* ihSupportToDraft,
const int iBid1,
const CATISpecObject_var ihNeutral,
const int iBid2,
const CATISpecObject_var ihParting,
const CATMathDirection iPullDir,
const CATISpecObject_var ihPullDirSpec,
const int iMode,
const double iAngle,
const int iBid4,
const int iType,
const CATISpecObject_var hSupport) = 0
Deprecated:
V5R15 #CreateVolumicDraft use CreateVolumicDraft (const CATLISTV(CATISpecObject_var)* ihSupportToDraft, const int iBid1, const CATISpecObject_var ihNeutral,
o CreateVolumicDraftAngle
public virtual CATISpecObject_var CreateVolumicDraftAngle()=0
Creates and returns a Draft feature in volumic context.
o CreateVolumicDraftAngle
public virtual CATISpecObject_var CreateVolumicDraftAngle( const int& type) =0
Deprecated:
V5R15 #CreateVolumicDraftAngle use CreateVolumicDraftAngle() to create Draft feature in Volumic context.
o CreateVolumicOffset
public virtual CATISpecObject_var CreateVolumicOffset( const CATISpecObject_var ihSurface,
const CATPrtOffsetSens iIsensOffset,
double iTopOffset,
double iBotOffset) = 0
Creates and returns a volumic offset feature.
Parameters:
ihSurface
The surfacic feature to be offseted to perform an offset operation.
iIsensOffset
Represents the orientation of the offset.
Legal values: iIsensOffset equals NormalSide or InverseNormalSide. The NormalSide value refers to the same orientation as the normal vector of the surfacic feature. The InverseNormalSide value refers to the opposite orientation as the normal vector of the surfacic feature.
iTopOffset
Represents the offset value between the surfacic feature to be offseted and the top skin of the offset feature.
iBotOffset
Represents the offset value between the surfacic feature to be offseted and the bottom skin of the offset feature.
Returns:
the created offset feature.
o CreateVolumicSewing
public virtual CATISpecObject_var CreateVolumicSewing( const int& Type,
const CATISpecObject_var& hVolume,
const CATISpecObject_var ihSewingPlane,
const CATPrtSplitType iSewingType) = 0
Creates and returns a volumic sewing feature.
Parameters:
Type
Must be set to 4.
ihVolume
The volumic feature to be operated.
ihSewingPlane
The surfacic feature to be sewn to perform the sewing operation.
iSewingType
Represents the side to be kept after the sewing operation.
Legal values: iSewingType equals PositiveSide or NegativeSide. The PositiveSide value refers to the same orientation as the sewing element normal vector. The NegativeSide value refers to the opposite orientation as the sewing element normal vector.
Returns:
the created sewing feature.
o CreateVolumicShell
public virtual CATISpecObject_var CreateVolumicShell( const CATISpecObject_var ihVolume,
const CATLISTV(CATISpecObject_var)* ihObjectList,
double iIntOffset,
double iExtOffset) = 0
Creates and returns a volumic shell feature.
Parameters:
ihVolume
The volumic feature to be operated.
ihObjectList
The list of the faces which corresponds to the shell openings.
iIntOffset
The internal offset value.
iExtOffset
The external offset value.
Returns:
The created shell feature.
o CreateVolumicShell
public virtual CATISpecObject_var CreateVolumicShell( const int type,
const CATISpecObject_var ihVolume,
const CATLISTV(CATISpecObject_var)* ihObjectList,
double iIntOffset,
double iExtOffset) = 0
Deprecated:
V5R15 #CreateVolumicShell use CreateVolumicShell (const CATISpecObject_var ihVolume, const CATLISTV(CATISpecObject_var)* ihObjectList, double iIntOffset, double iExtOffset)
o CreateVolumicThickness
public virtual CATISpecObject_var CreateVolumicThickness( const CATLISTV(CATISpecObject_var)* ihObjectList,
double iOffset,
const CATISpecObject_var ihSupport) = 0
Creates and returns a thickness feature.
Parameters:
ihObjectList
The list of the faces which corresponds to the shell openings.
iOffset
The offset value.
hSupport
The volumic feature to be operated.
Returns:
The created Thickness feature.

This object is included in the file: CATIPrtFactory.h
If needed, your Imakefile.mk should include the module: CATPartInterfaces

Copyright © 2003, Dassault Systèmes. All rights reserved.