CATPartUseItf Interface CATIPdgUseChamfer

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

interface CATIPdgUseChamfer

Interface to represent the chamfer shape.
Role: A chamfer is made up of a list of elements to be chamfered, such as edges or faces, is defined with a pair of parameters, such as two lengthes, or a length and an angle.

Method Index


o AddObject(CATLISTV(CATBaseUnknown_var)&)
Adds elements to be chamfered.
o GetContext(int&)
Returns the context of the chamfer (0 for PartDesign, 1 for Surfaces, 4 for Volumes and 5 for Functional).
o GetCornerCapMode(CATBoolean&)
Returns the CornerCapMode of the chamfer.
o GetExtremities(CATPrtChamferExtremities&)
Returns the Extremities of the chamfer.
o GetLength1()
Returns the first value of the chamfer.
o GetLength2()
Returns the second length value or the angle value of the chamfer.
o GetMode()
Returns the chamfer parameter mode.
o GetObject()
Returns the list of chamfered edges or faces.
o GetPropagation()
Returns the propagation mode of the elements to be chamfered.
o GetReferenceFace()
Returns the chamfer orientation.
o GetSupport(CATBaseUnknown_var&)
Returns the Support of the chamfer.
o GetSymmetricalExtent(CATBoolean&)
Returns the SymmetricalExtent button status.
o GetTrimSupportMode(CATPrtTrimSupportMode&)
Returns the TrimSupportMode of the chamfer.
o ModifyCornerCapMode(CATBoolean&)
Sets the CornerCapMode of the chamfer.
o ModifyExtremities(CATPrtChamferExtremities)
Sets the Extremities of the chamfer.
o ModifyLength1(double)
Sets the first value of the chamfer.
o ModifyLength2(double)
Sets the second length value or the angle value of the chamfer.
o ModifyMode(CATPrtChamferMode)
Sets the chamfer parameter mode.
o ModifyPropagation(CATPrtChamferPropagation)
Sets the propagation mode of the elements to be chamfered.
o ModifyReferenceFace(CATPrtChamferReferenceFace)
Sets the chamfer orientation.
o ModifySupport(CATBaseUnknown_var)
Sets the Support of the chamfer.
o ModifySymmetricalExtent(CATBoolean&)
Set the SymmetricalExtent button status.
o ModifyTrimSupportMode(CATPrtTrimSupportMode)
Sets the TrimSupportMode of the chamfer.
o RemoveObject(CATLISTV(CATBaseUnknown_var)&)
Removes elements from those to be chamfered.
o SetContext(int&)
Sets the context of the chamfer (0 for PartDesign, 1 for Surfaces, 4 for Volumes and 5 for Functional).

Methods


o AddObject
public virtual void AddObject( const CATLISTV(CATBaseUnknown_var)& iObjectList_input) = 0
Adds elements to be chamfered.
Parameters:
iObjectList
Specifies the list of sharp edges or faces 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 chamfer. This edge or face should belong to the same mechanical body.
o GetContext
public virtual void GetContext(int& oContext) = 0
Returns the context of the chamfer (0 for PartDesign, 1 for Surfaces, 4 for Volumes and 5 for Functional).
o GetCornerCapMode
public virtual HRESULT GetCornerCapMode(CATBoolean& OCornerCap) = 0
Returns the CornerCapMode of the chamfer.
o GetExtremities
public virtual HRESULT GetExtremities(CATPrtChamferExtremities& oExtremities) = 0
Returns the Extremities of the chamfer.
o GetLength1
public virtual double GetLength1()const = 0
Returns the first value of the chamfer. 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. This returns ChordalLength if the chamfer is defined with Chordal length and an angle. This returns Height if the chamfer is defined with Height and an angle.
Legal values: The first length value must be greater than 0 but not equal to 0.
o GetLength2
public virtual double GetLength2()const = 0
Returns the second length value or the angle value of the chamfer. This is the second length value if the chamfer is defined with two lengthes, or the angle value if the chamfer is defined with other modes.
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.
o GetMode
public virtual CATPrtChamferMode GetMode()const= 0
Returns the chamfer parameter mode.
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.
o GetObject
public virtual CATLISTV(CATIMmiMechanicalFeature_var) * GetObject()const = 0
Returns the list of chamfered edges or faces. The CATISpecObject_var is a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature.
o GetPropagation
public virtual CATPrtChamferPropagation GetPropagation()const = 0
Returns the propagation mode of the elements to be chamfered. 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.
o GetReferenceFace
public virtual CATPrtChamferReferenceFace GetReferenceFace()const= 0
Returns the chamfer orientation.
The first length, or the single length, depending on the way the chamfer is defined, is measured on the reference face from the edge to chamfer.
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).
o GetSupport
public virtual HRESULT GetSupport(CATBaseUnknown_var& ohsupport) = 0
Returns the Support of the chamfer.
o GetSymmetricalExtent
public virtual HRESULT GetSymmetricalExtent(CATBoolean& oSym) = 0
Returns the SymmetricalExtent button status.
o GetTrimSupportMode
public virtual HRESULT GetTrimSupportMode(CATPrtTrimSupportMode& oTrimSupportMode) = 0
Returns the TrimSupportMode of the chamfer.
o ModifyCornerCapMode
public virtual HRESULT ModifyCornerCapMode( const CATBoolean& iCornerCap) = 0
Sets the CornerCapMode of the chamfer.
o ModifyExtremities
public virtual HRESULT ModifyExtremities(CATPrtChamferExtremities iExtremities) = 0
Sets the Extremities of the chamfer.
o ModifyLength1
public virtual void ModifyLength1(double iLength1) = 0
Sets the first value of the chamfer.
Parameters:
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. This is ChordalLength if the chamfer is defined with Chordal length and an angle. This is Height if the chamfer is defined with Height and an angle.
Legal values: The first length value must be greater than 0 but not equal to 0.
o ModifyLength2
public virtual void ModifyLength2(double iLength2) = 0
Sets the second length value or the angle value of the chamfer.
Parameters:
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.
o ModifyMode
public virtual void ModifyMode(CATPrtChamferMode iParameterMode) = 0
Sets the chamfer parameter mode.
Parameters:
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.
o ModifyPropagation
public virtual void ModifyPropagation(CATPrtChamferPropagation iPropagation) = 0
Sets the propagation mode of the elements to be chamfered.
Parameters:
iPropagation
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.
o ModifyReferenceFace
public virtual void ModifyReferenceFace(CATPrtChamferReferenceFace iReferenceFace) = 0
Sets the chamfer orientation.
Parameters:
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 chamfer.
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).
o ModifySupport
public virtual HRESULT ModifySupport(CATBaseUnknown_var ihsupport) = 0
Sets the Support of the chamfer.
o ModifySymmetricalExtent
public virtual HRESULT ModifySymmetricalExtent( const CATBoolean& iSym) = 0
Set the SymmetricalExtent button status.
o ModifyTrimSupportMode
public virtual HRESULT ModifyTrimSupportMode(CATPrtTrimSupportMode iTrimSupportMode) = 0
Sets the TrimSupportMode of the chamfer.
o RemoveObject
public virtual void RemoveObject( const CATLISTV(CATBaseUnknown_var)& iObjectList_input) = 0
Removes elements from those to be chamfered.
Parameters:
iObjectList
Specifies the list of edges or faces to be removed. The CATISpecObject_var should be a Redge (CATIMfRedge) or Rsur (CATIMfRsur) feature . This edge or face should belong to the chamfer.
o SetContext
public virtual void SetContext(int& iContext) = 0
Sets the context of the chamfer (0 for PartDesign, 1 for Surfaces, 4 for Volumes and 5 for Functional).
This object is included in the file: CATIPdgUseChamfer.h
If needed, your Imakefile.mk should include the module: CATPartUseItf

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