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CATPartUseItf Interface CATIPdgUsePrtFactory

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

interface CATIPdgUsePrtFactory

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

Methods

o CreateAffinity

public virtual CreateAffinity(	const	`ihElemToTransfor_input`,
	const	`ihAxisOrigin_input`,
	const	`ihAxisPlane_input`,
	const	`ihAxisFirstDirection_input`,
	const	`ihRatioX`,
	const	`ihRatioY`,
	const	`ihRatioZ`)

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 CreateAlign(	const	`ihAlignPlane_input`,
	const	`iAlignType`)

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 CreateAxisToAxis(	const	`ihToTransform_input`,
	const	`ihReferenceAxis_input`,
	const	`ihTargetAxis_input`)

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 CreateChamfer(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iParameterMode`,
	const	`iLength1`,
	const	`iLength2`,
	const	`iReferenceFace`	`= NO_REVERSE`,
	const	`ihSupport_input`	`=NULL_var`,
	const	`iContext`	`= -1`)

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 CATIMmiBRepFactory. 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 CreateCircPatt(	const	`ihMotif_input`,
	const	`iDir_input`,
	const	`iPto_input`,
	const	`iSensa`,
	const	`iNbr`,
	const	`iNba`,
	const	`iStepr`,
	const	`iStepa`,
	const	`iNr`,
	const	`iNa`,
	const	`iRotationAngle`,
	const	`iInstRot`,
	const	`iCompleteCrown`)

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 CreateCloseSurface

public virtual CreateCloseSurface( const ihCloseElement_input)

Creates and returns a close feature.

Parameters:

ihCloseElement: The surfacic feature to be closed.

Returns:

The created close feature.

o CreateDraft

public virtual CreateDraft(	const	`ihSupportToDraft_input`,
	const	`iBid1`,
	const	`ihNeutral_input`,
	const	`iBid2`,
	const	`ihParting_input`,
	const	`iPullDir`,
	const	`ihPullDirSpec_input`,
	const	`iMode`,
	const	`iAngle`,
	const	`iBid4`)

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 CreateGroove

public virtual CreateGroove( const ihSketch_input = NULL_var)

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 CreateHole(	const	`ihSurface_input`,
	const	`ihDirection_input`)

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 CreateHole(	const	`iMathPoint`,
	const	`ihSurface_input`,
	const	`ihDirection_input`,
	const	`IsPointOnSurface`)

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 CreateHole

public virtual CreateHole(	const	`ihPoint_input`,
	const	`ihSurface_input`,
	const	`ihDirection_input`,
	const	`IsPointOnSurface`)

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 CreateHole(	const	`iMathPoint`,
	const	`ihFirstEdge_input`,
	const	`ihSecndEdge_input`,
	const	`ihSurface_input`,
	const	`iDirection_input`)

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 CreateLoft

public virtual CreateLoft(

)

Creates and returns a new loft feature.

Returns:: The loft feature.

o CreateMirror

public virtual CreateMirror( const ihSymPlane_input)

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 CreatePad

public virtual CreatePad( const ihSketch_input = NULL_var)

Creates a new pad.

Parameters:

ihSketch: The sketch defining the pad profile.

Returns:

The pad feature.

o CreatePocket

public virtual CreatePocket( const ihSketch_input = NULL_var)

Creates a new pocket.

Parameters:

ihSketch: The sketch defining the pocket profile.

Returns:

The pocket feature.

o CreateRectPatt

public virtual CreateRectPatt(	const	`ihMotif_input`,
	const	`ihLine1_input`,
	const	`ihLine2_input`,
	const	`iDir1`,
	const	`iDir2`,
	const	`iNb1`,
	const	`iNb2`,
	const	`iStep1`,
	const	`iStep2`,
	const	`iNu`,
	const	`iNv`,
	const	`iRotationAngle`)

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 CreateRemovedLoft

public virtual CreateRemovedLoft(

)

Creates and returns a new removed loft feature.

Returns:: The removed loft feature.

o CreateRib

public virtual CreateRib(

)

Creates and returns a new rib feature.

Returns:: The rib feature.

o CreateRib

public virtual CreateRib(	const	`ihSketch_input`,
	const	`ihCenterCrv_input`)

Creates and returns a new rib feature.

Parameters:

ihSketch: Selected profile.
ihCenterCrv: Selected center curve.

Returns:

The rib feature.

o CreateRotate

public virtual CreateRotate(	const	`ihToRotate_input`,
	const	`ihAxis_input`,
	const	`ihAngle`)

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 CreateScaling(	const	`ihToScale_input`,
	const	`ihReference_input`,
	const	`ihRatio`)

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 CreateSewing(	const	`ihSewingPlane_input`,
	const	`iSewingType`)

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 CreateShaft( const ihSketch_input = NULL_var)

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 CreateShell(	const	`ihObjectList_input`,
		`iIntOffset`,
		`iExtOffset`)

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 CreateSlot(

)

Creates and returns a new slot feature.

Returns:: The slot feature.

o CreateSlot

public virtual CreateSlot(	const	`ihSketch_input`,
	const	`ihCenterCrv_input`)

Creates and returns a new slot feature.

Parameters:

ihSketch: Selected profile.
ihCenterCrv: Selected center curve.

Returns:

The slot feature.

o CreateSolidFillet

public virtual CreateSolidFillet(	const	`ihRsur1`,
	const	`ihRsur2`,
	const	`iRadius`,
	const	`ihSupport_input`	`=NULL_var`)

Creates and returns a solid face fillet feature.

Parameters:

ihRsur1: Specifies the first face to be filleted. The CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CreateSolidFillet(	const	`ihRsur1`,
	const	`ihRsur2`,
	const	`ihRemoveRsur`,
	const	`ihSupport_input`	`=NULL_var`)

Creates and returns a tritangent fillet feature.

Parameters:

ihRsur1: Specifies the first face to be filleted. The CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CreateSolidFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iRadius`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIMmiBRepFactory. 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 CreateSolidFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iVariationMode`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIPdgUseEdgeFillet 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 CATIMmiBRepFactory. 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 CreateSolidFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iRadius`,
	const	`iKeepEdgeList_input`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIMmiBRepFactory. 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 CATIMmiBRepFactory. 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 CreateSolidFillet

public virtual CreateSolidFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iVariationMode`,
	const	`iKeepEdgeList_input`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIPdgUseEdgeFillet 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 CATIMmiBRepFactory. 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 CATIMmiBRepFactory. 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 CreateSolidOffset

public virtual CreateSolidOffset(	const	`ihSurface_input`,
	const	`iIsensOffset`,
		`iTopOffset`,
		`iBotOffset`)

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 CreateSolidSplit(	const	`ihSplitPlane_input`,
	const	`iSplitType`)

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 CreateStiffener

public virtual CreateStiffener( const ihSketch_input = NULL_var)

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 CreateSurfaceFillet(	const	`ihRsur1`,
	const	`ihRsur2`,
	const	`iRadius`,
	const	`ihSupport_input`	`=NULL_var`)

Creates and returns a surface face fillet feature.

Parameters:

ihRsur1: Specifies the first face to be filleted. The CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CreateSurfaceFillet(	const	`ihRsur1`,
	const	`ihRsur2`,
	const	`ihRemoveRsur`,
	const	`ihSupport_input`	`=NULL_var`)

Creates and returns a tritangent fillet feature.

Parameters:

ihRsur1: Specifies the first face to be filleted. The CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CATIMmiUseBRep_var should be a Rsur feature (CATIMfRsur) created with CATIMmiBRepFactory. 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 CreateSurfaceFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iRadius`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIMmiBRepFactory. 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 CreateSurfaceFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iVariationMode`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIPdgUseEdgeFillet 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 CATIMmiBRepFactory. 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 CreateSurfaceFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iRadius`,
	const	`iKeepEdgeList_input`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIMmiBRepFactory. 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 CATIMmiBRepFactory. 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 CreateSurfaceFillet

public virtual CreateSurfaceFillet(	const	`iObjectList_input`,
	const	`iPropagationMode`,
	const	`iVariationMode`,
	const	`iKeepEdgeList_input`,
	const	`ihSupport_input`	`=NULL_var`)

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 CATIPdgUseEdgeFillet 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 CATIMmiBRepFactory. 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 CATIMmiBRepFactory. 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 CreateSurfacicCircPatt

public virtual CreateSurfacicCircPatt(	const	`ihMotif_input`,
	const	`iDir_input`,
	const	`iPto_input`,
	const	`iSensa`,
	const	`iNbr`,
	const	`iNba`,
	const	`iStepr`,
	const	`iStepa`,
	const	`iNr`,
	const	`iNa`,
	const	`iRotationAngle`,
	const	`iInstRot`,
	const	`iCompleteCrown`)

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 CreateSurfacicRectPatt(	const	`ihMotif_input`,
	const	`ihLine1_input`,
	const	`ihLine2_input`,
	const	`iDir1`,
	const	`iDir2`,
	const	`iNb1`,
	const	`iNb2`,
	const	`iStep1`,
	const	`iStep2`,
	const	`iNu`,
	const	`iNv`,
	const	`iRotationAngle`)

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 CreateSurfacicUserPatt(	const	`ihMotif_input`,
	const	`iNbCopy`,
	const	`iObjectList_input`,
	const	`ihStepElt_input`)

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 CreateSymmetry(	const	`ihSpec_input`,
	const	`ihPlane_input`)

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 CreateThickness(	const	`ihObjectList_input`,
		`iOffset`)

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 CreateThread(

)

Creates and returns a new thread feature.

Returns:: The thread feature.

o CreateThread

public virtual CreateThread(	const	`ihSupportElement_input`,
	const	`ihLimitElement_input`)

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 CreateTranslate(	const	`ihSpecToTranslate_input`,
	const	`ihDirection`,
	const	`ihDistance`)

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 CreateUserPatt(	const	`ihMotif_input`,
	const	`iNbCopy`,
	const	`iObjectList_input`,
	const	`ihStepElt_input`)

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 CreateVolumicCloseSurface( const ihCloseElement_input)

Creates and returns a volumic close feature.

Parameters:

ihCloseElement: The surfacic feature to be closed.

Returns:

The created close feature.

o CreateVolumicDraft

public virtual CreateVolumicDraft(	const	`ihSupportToDraft_input`,
	const	`iBid1`,
	const	`ihNeutral_input`,
	const	`iBid2`,
	const	`ihParting_input`,
	const	`iPullDir`,
	const	`ihPullDirSpec_input`,
	const	`iMode`,
	const	`iAngle`,
	const	`iBid4`,
	const	`hSupport_input`)

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 CreateVolumicDraftAngle

public virtual CreateVolumicDraftAngle(

)

Creates and returns a Draft feature in volumic context.

o CreateVolumicOffset

public virtual CreateVolumicOffset(	const	`ihSurface_input`,
	const	`iIsensOffset`,
		`iTopOffset`,
		`iBotOffset`)

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 CreateVolumicSewing(	const	`Type`,
	const	`ihVolume_input`,
	const	`ihSewingPlane_input`,
	const	`iSewingType`)

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 CreateVolumicShell(	const	`ihVolume_input`,
	const	`ihObjectList_input`,
		`iIntOffset`,
		`iExtOffset`)

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 CreateVolumicThickness

public virtual CreateVolumicThickness(	const	`ihObjectList_input`,
		`iOffset`,
	const	`ihSupport_input`)

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: CATIPdgUsePrtFactory.h
If needed, your Imakefile.mk should include the module: CATPartUseItf