Represents a Hole feature builder. More...

Inheritance diagram for NXOpen::Features::HoleFeatureBuilder:

Public Types
enum	HoleSubtype { HoleSubtypeSimple, HoleSubtypeCounterbore, HoleSubtypeCountersink }
	Represents the subtype of the hole. More...

Public Types inherited from NXOpen::Features::RPOBuilder
enum	AssociativityType { AssociativityTypeEndPoint, AssociativityTypeArcCenter, AssociativityTypeTangency, AssociativityTypeEndPoint1, AssociativityTypeEndPoint2, AssociativityTypeVerticalCenterline1, AssociativityTypeVerticalCenterline2, AssociativityTypeHorizontalCenterline1, AssociativityTypeHorizontalCenterline2 }
	Represents the associativity type for a dimension entity. More...

Public Member Functions
NXOpen::Expression *	CounterboreDepth ()
	Returns the depth of the counterbore for a hole. More...

NXOpen::Expression *	CounterboreDiameter ()
	Returns the diameter of the counterbore for a hole. More...

NXOpen::Expression *	CountersinkAngle ()
	Returns the angle of the countersink for a hole. More...

NXOpen::Expression *	CountersinkDiameter ()
	Returns the diameter of the countersink for a hole. More...

void	CreateHole ()
	Creates a hole body which can be positioned Created in NX3.0.0. More...

NXOpen::Expression *	Depth ()
	Returns the depth of the hole. More...

NXOpen::Expression *	Diameter ()
	Returns the diameter of the hole. More...

NXOpen::Body *	GetTargetBody ()
	Returns target body for the hole. More...

NXOpen::ISurface *	GetThruFace ()
	Returns thru face parameter for the hole. More...

NXOpen::Point3d	HoleLocation ()
	Returns the reference point of the hole. More...

NXOpen::ISurface *	PlacementFace ()
	Returns the placement face of the hole. More...

bool	ReverseDirection ()
	Returns the reverse direction flag of the hole. More...

void	SetCounterboreDepth (const NXString &depth)
	Sets the depth of the counterbore for a hole. More...

void	SetCounterboreDepth (const char *depth)
	Sets the depth of the counterbore for a hole. More...

void	SetCounterboreDiameter (const NXString &diameter)
	Sets the diameter of the counterbore for a hole. More...

void	SetCounterboreDiameter (const char *diameter)
	Sets the diameter of the counterbore for a hole. More...

void	SetCounterboreHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter, const NXString &counterboreDiameter, const NXString &counterboreDepth)
	Sets parameters for counterbore hole Created in NX3.0.0. More...

void	SetCounterboreHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface placementFace, const char diameter, const char counterboreDiameter, const char counterboreDepth)
	Sets parameters for counterbore hole Created in NX3.0.0. More...

void	SetCountersinkAngle (const NXString &angle)
	Sets the angle of the countersink for a hole. More...

void	SetCountersinkAngle (const char *angle)
	Sets the angle of the countersink for a hole. More...

void	SetCountersinkDiameter (const NXString &diameter)
	Sets the diameter of the countersink for a hole. More...

void	SetCountersinkDiameter (const char *diameter)
	Sets the diameter of the countersink for a hole. More...

void	SetCountersinkHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter, const NXString &countersinkDiameter, const NXString &countersinkAngle)
	Sets parameters for countersink hole Created in NX3.0.0. More...

void	SetCountersinkHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface placementFace, const char diameter, const char countersinkDiameter, const char countersinkAngle)
	Sets parameters for countersink hole Created in NX3.0.0. More...

void	SetDepth (const NXString &depth)
	Sets the depth of the hole. More...

void	SetDepth (const char *depth)
	Sets the depth of the hole. More...

void	SetDepthAndTipAngle (const NXString &depth, const NXString &tipAngle)
	Sets depth and tip angle parameters for the hole. More...

void	SetDepthAndTipAngle (const char depth, const char tipAngle)
	Sets depth and tip angle parameters for the hole. More...

void	SetDiameter (const NXString &diameter)
	Sets the diameter of the hole. More...

void	SetDiameter (const char *diameter)
	Sets the diameter of the hole. More...

void	SetHoleLocation (const NXOpen::Point3d &referencePoint)
	Sets the reference point of the hole. More...

void	SetPlacementFace (NXOpen::ISurface *placementFace)
	Sets the placement face of the hole. More...

void	SetReverseDirection (bool reverse)
	Sets the reverse direction flag of the hole. More...

void	SetSimpleHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter)
	Sets parameters for simple hole Created in NX3.0.0. More...

void	SetSimpleHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface placementFace, const char diameter)
	Sets parameters for simple hole Created in NX3.0.0. More...

void	SetSubtype (NXOpen::Features::HoleFeatureBuilder::HoleSubtype subtype)
	Sets the type of hole. More...

void	SetTargetBody (NXOpen::Body *targetBody)
	Sets target body for the hole. More...

void	SetThruFace (NXOpen::ISurface *thruFace)
	Sets thru face parameter for the hole. More...

void	SetTipAngle (const NXString &tipAngle)
	Sets the tip angle of the hole. More...

void	SetTipAngle (const char *tipAngle)
	Sets the tip angle of the hole. More...

NXOpen::Features::HoleFeatureBuilder::HoleSubtype	Subtype ()
	Returns the type of hole. More...

NXOpen::Expression *	TipAngle ()
	Returns the tip angle of the hole. More...

Public Member Functions inherited from NXOpen::Features::RPOBuilder
void	ApplyDimensions ()
	Transforms the feature by applying the positioning dimensions Created in NX3.0.0. More...

NXOpen::Features::RPODimension *	CreateDimension ()
	Creates a new empty RPODimension object. More...

void	CreatePositioningDimension ()
	Creates a positioning dimension. More...

void	GetReferenceDirection (NXOpen::IReferenceAxis *reference, NXOpen::AxisOrientation orientation)
	Query/Set a horizontal or vertical reference for the feature. More...

std::vector < NXOpen::Features::RPODimension * >	GetRpoDimensions ()
	Gets the list of RPO dimemsions. More...

void	HidePositioningDimensions ()
	Hides display of all the positioning dimensions Created in NX3.0.0. More...

void	SetExpression (const NXString &expression)
	Sets the expression value in order to constrain the target and tool entities which are set using NXOpen::Features::RPOBuilder::SetTargetAndTool . More...

void	SetExpression (const char *expression)
	Sets the expression value in order to constrain the target and tool entities which are set using NXOpen::Features::RPOBuilder::SetTargetAndTool . More...

void	SetReferenceDirection (NXOpen::IReferenceAxis *reference, NXOpen::AxisOrientation orientation)
	Sets a horizontal or vertical reference for the feature. More...

void	SetRpoDimensions (const std::vector< NXOpen::Features::RPODimension * > &dimensions)
	Sets the list of RPO dimemsions. More...

void	SetTargetAndTool (NXOpen::PositioningDimension::Subtype subtype, NXOpen::NXObject target, NXOpen::Features::RPOBuilder::AssociativityType targetAssociativity, const NXOpen::Point3d &targetHelpPoint, NXOpen::NXObject tool, NXOpen::Features::RPOBuilder::AssociativityType toolAssociativity, const NXOpen::Point3d &toolHelpPoint)
	Sets the target and tool entities. More...

void	ShowPositioningDimensions ()
	Displays all the positioning dimensions Created in NX3.0.0. More...

void	UndoLastDimension ()
	Undo the last positioning dimension Created in NX3.0.0. 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

Represents a Hole feature builder.

See NXOpen::Features::RPOBuilder for details on positioning the hole.
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreateHoleFeatureBuilder

Created in NX3.0.0.

Member Enumeration Documentation

enum NXOpen::Features::HoleFeatureBuilder::HoleSubtype

Represents the subtype of the hole.

Enumerator
HoleSubtypeSimple	Simple hole.
HoleSubtypeCounterbore	Counterbore hole.
HoleSubtypeCountersink	Countersink hole.

Member Function Documentation

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::CounterboreDepth ( )

Returns the depth of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::CounterboreDiameter ( )

Returns the diameter of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::CountersinkAngle ( )

Returns the angle of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::CountersinkDiameter ( )

Returns the diameter of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

void NXOpen::Features::HoleFeatureBuilder::CreateHole ( )

Creates a hole body which can be positioned
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::Depth ( )

Returns the depth of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::Diameter ( )

Returns the diameter of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Body* NXOpen::Features::HoleFeatureBuilder::GetTargetBody ( )

Returns target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.

Returns: Target Body
Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::ISurface* NXOpen::Features::HoleFeatureBuilder::GetThruFace ( )

Returns thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.

Returns: Thru face
Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Point3d NXOpen::Features::HoleFeatureBuilder::HoleLocation ( )

Returns the reference point of the hole.

This parameter will position the hole unless relative positioning dimensions are used

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::ISurface* NXOpen::Features::HoleFeatureBuilder::PlacementFace ( )

Returns the placement face of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

bool NXOpen::Features::HoleFeatureBuilder::ReverseDirection ( )

Returns the reverse direction flag of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreDepth ( const NXString & depth )

Sets the depth of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth counterbore depth

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreDepth ( const char * depth )

Sets the depth of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth counterbore depth

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreDiameter ( const NXString & diameter )

Sets the diameter of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreDiameter ( const char * diameter )

Sets the diameter of the counterbore for a hole.

Only used if the hole type is couterbore

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const NXString &	diameter,
		const NXString &	counterboreDiameter,
		const NXString &	counterboreDepth
	)

Sets parameters for counterbore hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter
counterboreDiameter	Counterbore diameter
counterboreDepth	Counterbore depth

void NXOpen::Features::HoleFeatureBuilder::SetCounterboreHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const char *	diameter,
		const char *	counterboreDiameter,
		const char *	counterboreDepth
	)

Sets parameters for counterbore hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter
counterboreDiameter	Counterbore diameter
counterboreDepth	Counterbore depth

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkAngle ( const NXString & angle )

Sets the angle of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

angle countersink angle

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkAngle ( const char * angle )

Sets the angle of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

angle countersink angle

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkDiameter ( const NXString & diameter )

Sets the diameter of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkDiameter ( const char * diameter )

Sets the diameter of the countersink for a hole.

Only used if the hole type is coutersink

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const NXString &	diameter,
		const NXString &	countersinkDiameter,
		const NXString &	countersinkAngle
	)

Sets parameters for countersink hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter
countersinkDiameter	Countersink diameter
countersinkAngle	Countersink angle

void NXOpen::Features::HoleFeatureBuilder::SetCountersinkHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const char *	diameter,
		const char *	countersinkDiameter,
		const char *	countersinkAngle
	)

Sets parameters for countersink hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter
countersinkDiameter	Countersink diameter
countersinkAngle	Countersink angle

void NXOpen::Features::HoleFeatureBuilder::SetDepth ( const NXString & depth )

Sets the depth of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth Hole depth

void NXOpen::Features::HoleFeatureBuilder::SetDepth ( const char * depth )

Sets the depth of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth Hole depth

void NXOpen::Features::HoleFeatureBuilder::SetDepthAndTipAngle	(	const NXString &	depth,
		const NXString &	tipAngle
	)

Sets depth and tip angle parameters for the hole.

Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth	Hole depth
tipAngle	Tip angle of the tool

void NXOpen::Features::HoleFeatureBuilder::SetDepthAndTipAngle	(	const char *	depth,
		const char *	tipAngle
	)

Sets depth and tip angle parameters for the hole.

Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

depth	Hole depth
tipAngle	Tip angle of the tool

void NXOpen::Features::HoleFeatureBuilder::SetDiameter ( const NXString & diameter )

Sets the diameter of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetDiameter ( const char * diameter )

Sets the diameter of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

diameter Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetHoleLocation ( const NXOpen::Point3d & referencePoint )

Sets the reference point of the hole.

This parameter will position the hole unless relative positioning dimensions are used

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint Reference point for the hole

void NXOpen::Features::HoleFeatureBuilder::SetPlacementFace ( NXOpen::ISurface * placementFace )

Sets the placement face of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

placementFace Placement face

void NXOpen::Features::HoleFeatureBuilder::SetReverseDirection ( bool reverse )

Sets the reverse direction flag of the hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

reverse reverse

void NXOpen::Features::HoleFeatureBuilder::SetSimpleHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const NXString &	diameter
	)

Sets parameters for simple hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetSimpleHole	(	const NXOpen::Point3d &	referencePoint,
		bool	reverseDirection,
		NXOpen::ISurface *	placementFace,
		const char *	diameter
	)

Sets parameters for simple hole
Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint	Reference point for the hole
reverseDirection	Reverse direction flag, applicable only if placement face is a datum plane
placementFace	Placement face
diameter	Hole diameter

void NXOpen::Features::HoleFeatureBuilder::SetSubtype ( NXOpen::Features::HoleFeatureBuilder::HoleSubtype subtype )

Sets the type of hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

subtype subtype

void NXOpen::Features::HoleFeatureBuilder::SetTargetBody ( NXOpen::Body * targetBody )

Sets target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

targetBody Target Body

void NXOpen::Features::HoleFeatureBuilder::SetThruFace ( NXOpen::ISurface * thruFace )

Sets thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.

Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

thruFace Thru face

void NXOpen::Features::HoleFeatureBuilder::SetTipAngle ( const NXString & tipAngle )

Sets the tip angle of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

tipAngle Tip angle

void NXOpen::Features::HoleFeatureBuilder::SetTipAngle ( const char * tipAngle )

Sets the tip angle of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters

tipAngle Tip angle

NXOpen::Features::HoleFeatureBuilder::HoleSubtype NXOpen::Features::HoleFeatureBuilder::Subtype ( )

Returns the type of hole.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

NXOpen::Expression* NXOpen::Features::HoleFeatureBuilder::TipAngle ( )

Returns the tip angle of the hole.

If this parameter is set then the thru face is ignored.

Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

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

Features_HoleFeatureBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation