The Three Bend Corner feature class. More...

Inheritance diagram for NXOpen::Features::SheetMetal::ThreeBendCornerBuilder:

Public Types
enum	OriginTypes { OriginTypesBendCenter, OriginTypesCornerPoint }
	This enum represents Origin type. More...

enum	TreatmentTypeOptions { TreatmentTypeOptionsOpen, TreatmentTypeOptionsClosed, TreatmentTypeOptionsCircularCutout, TreatmentTypeOptionsUCutout, TreatmentTypeOptionsVCutout }
	This enum represents the corner treatment type. More...

Public Member Functions
void	AddFacePair (NXOpen::Face firstFace, NXOpen::Face secondFace)
	Input a bend face pair for the three bend corner feature. More...

bool	BlendMiter ()
	Returns the option for smooth transition from miter to cutout edges. More...

NXOpen::Expression *	BlendMiterRadius ()
	Returns the blend miter radius used for three bend corner miter treatment. More...

NXOpen::Expression *	Diameter ()
	Returns the diameter used for circular, u and v cutout corner treatments. More...

NXOpen::Expression *	FlangeClearance ()
	Returns the flange clearance used for three bend corner miter treatment. More...

void	GetFacePair (int index, NXOpen::Face firstFace, NXOpen::Face secondFace)
	Gets the bend face pair at the given index. More...

bool	MiterCorner ()
	Returns whether the corner will be closed using miter. More...

NXOpen::Expression *	MiterRootRadius ()
	Returns the miter root radius used for three bend corner miter treatment. More...

int	NumberOfFacePairs ()
	Returns the number of face pairs already identified for the three bend corner feature. More...

NXOpen::Expression *	Offset ()
	Returns the offset used for circular, u and v cutout corner treatments. More...

NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginTypes	OriginType ()
	Returns the relief origin used for circular, u and v cutout corner treatments. More...

void	RemoveFacePair (NXOpen::Face firstFace, NXOpen::Face secondFace)
	Removes a face pair (that represents a unique corner) from the list of face pairs already added. More...

void	SetBlendMiter (bool blendMiter)
	Sets the option for smooth transition from miter to cutout edges. More...

void	SetDiameter (const NXString &diameter)
	The diameter used for the circular cutout corner treatment. More...

void	SetDiameter (const char *diameter)
	The diameter used for the circular cutout corner treatment. More...

void	SetMiterCorner (bool miterCorner)
	Sets whether the corner will be closed using miter. More...

void	SetOriginType (NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginTypes originType)
	Sets the relief origin used for circular, u and v cutout corner treatments. More...

void	SetTreatmentType (NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions treatmentType)
	Sets the corner treatment type. More...

NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions	TreatmentType ()
	Returns the corner treatment type. More...

int	ValidateBuilderData ()
	Verify that the builder data is valid for creation of a three bend corner. More...

NXOpen::Expression *	VCutoutAngle1 ()
	Returns the angle 1 used for the v cutout treatment. More...

NXOpen::Expression *	VCutoutAngle2 ()
	Returns the angle 2 used for the v cutout treatment. More...

Public Member Functions inherited from NXOpen::Features::FeatureBuilder
NXOpen::Features::Feature *	CommitFeature ()
	Commits the feature parameters and creates the feature. More...

NXOpen::Features::Feature *	GetFeature ()
	Returns the feature currently being edited by this builder. More...

void	HideInternalParentFeatureAfterEdit (NXOpen::Features::Feature *parentFeature)
	Re-suppress an internal parent feature (a slave feature) after it has been edited. More...

bool	ParentFeatureInternal ()
	Returns whether or not the latest timestamped parent feature of this feature should be made internal Created in NX5.0.0. More...

bool	PatchSolutionFlag ()
	Returns the patch solution flag Created in NX8.0.1. More...

NXString	PatchSurfaceFilename ()
	Returns the patch surface filename Created in NX8.0.1. More...

void	SetParentFeatureInternal (NXOpen::Features::Feature *parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited Created in NX6.0.0. More...

void	SetParentFeatureInternal (bool isInternal)
	Sets whether or not the latest timestamped parent feature of this feature should be made internal Created in NX5.0.0. More...

void	SetPatchSolutionFlag (bool optionValue)
	Sets the patch solution flag Created in NX8.0.1. More...

void	SetPatchSurfaceFilename (const NXString &surfaceFilename)
	Sets the patch surface filename Created in NX8.0.1. More...

void	SetPatchSurfaceFilename (const char *surfaceFilename)
	Sets the patch surface filename Created in NX8.0.1. More...

void	SetSurroundingPatchSurfaceFilename (const NXString &surroundingSurfaceFilename)
	Sets the surrounding patch surface filename Created in NX8.0.1. More...

void	SetSurroundingPatchSurfaceFilename (const char *surroundingSurfaceFilename)
	Sets the surrounding patch surface filename Created in NX8.0.1. More...

void	ShowInternalParentFeatureForEdit (NXOpen::Features::Feature *parentFeature)
	Unsuppress an internal parent feature (a slave feature) so it can be edited. More...

NXString	SurroundingPatchSurfaceFilename ()
	Returns the surrounding patch surface filename Created in NX8.0.1. More...

void	UnsetParentFeatureInternal (NXOpen::Features::Feature *parentFeature)
	Set the internal parent feature of the feature being edited to external Created in NX6.0.0. More...

Public Member Functions inherited from NXOpen::Builder
NXOpen::NXObject *	Commit ()
	Commits any edits that have been applied to the builder. More...

void	Destroy ()
	Deletes the builder, and cleans up any objects created by the builder. More...

std::vector< NXOpen::NXObject * >	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...

NXOpen::NXObject *	GetObject ()
	Returns the object currently being edited by this builder. More...

void	ShowResults ()
	Updates the model to reflect the result of an edit to the model for all builders that support showing results. More...

virtual bool	Validate ()
	Validate whether the inputs to the component are sufficient for commit to be called. More...

Public Member Functions inherited from NXOpen::TaggedObject
tag_t	Tag () const
	Returns the tag of this object. More...

Detailed Description

The Three Bend Corner feature class.

Users can identify multiple input face pairs for each three bend corner feature. Each pair is made up of one face each from adjacent bends. The bends must both have the same radius and sweep angle, and they must also be connected via another adjoining bend.
To create a new instance of this class, use NXOpen::Features::SheetMetal::SheetmetalManager::CreateThreeBendCornerFeatureBuilder

Created in NX4.0.0.

Member Enumeration Documentation

enum NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginTypes

This enum represents Origin type.

Enumerator
OriginTypesBendCenter	The relief origin will be at the intersection of first bend's centerline and bisector of corner angle.
OriginTypesCornerPoint	The relief origin will be at the corner point.

enum NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions

This enum represents the corner treatment type.

Enumerator
TreatmentTypeOptionsOpen	open
TreatmentTypeOptionsClosed	closed
TreatmentTypeOptionsCircularCutout	circular cutout
TreatmentTypeOptionsUCutout	ucutout
TreatmentTypeOptionsVCutout	vcutout

Member Function Documentation

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::AddFacePair	(	NXOpen::Face *	firstFace,
		NXOpen::Face *	secondFace
	)

Input a bend face pair for the three bend corner feature.

This method can be called multiple times for a feature, with each bend face pair representing a unique corner.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

firstFace	A bend face from a bend
secondFace	A bend face from an adjacent bend

bool NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::BlendMiter ( )

Returns the option for smooth transition from miter to cutout edges.

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::BlendMiterRadius ( )

Returns the blend miter radius used for three bend corner miter treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsClosed or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::Diameter ( )

Returns the diameter used for circular, u and v cutout corner treatments.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::FlangeClearance ( )

Returns the flange clearance used for three bend corner miter treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsOpen or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsClosed or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::GetFacePair	(	int	index,
		NXOpen::Face **	firstFace,
		NXOpen::Face **	secondFace
	)

Gets the bend face pair at the given index.

The index can vary between zero and one less than the value returned by NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::NumberOfFacePairs .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

index	Index of the desired face pair
firstFace	First face of the face pair
secondFace	Second face of the face pair

bool NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::MiterCorner ( )

Returns whether the corner will be closed using miter.

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::MiterRootRadius ( )

Returns the miter root radius used for three bend corner miter treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsClosed .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

int NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::NumberOfFacePairs ( )

Returns the number of face pairs already identified for the three bend corner feature.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::Offset ( )

Returns the offset used for circular, u and v cutout corner treatments.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginTypes NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginType ( )

Returns the relief origin used for circular, u and v cutout corner treatments.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::RemoveFacePair	(	NXOpen::Face *	firstFace,
		NXOpen::Face *	secondFace
	)

Removes a face pair (that represents a unique corner) from the list of face pairs already added.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

firstFace	A face from an already selected face pair
secondFace	The other face from the face pair

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetBlendMiter ( bool blendMiter )

Sets the option for smooth transition from miter to cutout edges.

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

blendMiter blendmiter

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetDiameter ( const NXString & diameter )

The diameter used for the circular cutout corner treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout . .

Deprecated:: Deprecated in NX10.0.0. Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::Diameter instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

diameter The diameter for the circular cutout corner treatment

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetDiameter ( const char * diameter )

The diameter used for the circular cutout corner treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout . .

Deprecated:: Deprecated in NX10.0.0. Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::Diameter instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

diameter The diameter for the circular cutout corner treatment

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetMiterCorner ( bool miterCorner )

Sets whether the corner will be closed using miter.

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

miterCorner mitercorner

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetOriginType ( NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::OriginTypes originType )

Sets the relief origin used for circular, u and v cutout corner treatments.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsCircularCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsUCutout or NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX9.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

originType The relief origin type

void NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetTreatmentType ( NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions treatmentType )

Sets the corner treatment type.

The NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentType and NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetTreatmentType ) specifies how the corner should be treated. Valid options are in NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

treatmentType The type of treatment specified for the corner

NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentType ( )

Returns the corner treatment type.

The NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentType and NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::SetTreatmentType ) specifies how the corner should be treated. Valid options are in NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptions .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

int NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::ValidateBuilderData ( )

Verify that the builder data is valid for creation of a three bend corner.

If the data in the builder is valid, the return value is 0

Returns: Returns 0 if the data in the builder is valid
Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::VCutoutAngle1 ( )

Returns the angle 1 used for the v cutout treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX8.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::Expression* NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::VCutoutAngle2 ( )

Returns the angle 2 used for the v cutout treatment.

This only applies when the treatment type is set to NXOpen::Features::SheetMetal::ThreeBendCornerBuilder::TreatmentTypeOptionsVCutout .

Created in NX8.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

The documentation for this class was generated from the following file:

Features_SheetMetal_ThreeBendCornerBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation