Represents a NXOpen::Features::ProjectCurve builder. More...

Inheritance diagram for NXOpen::Features::ProjectCurveBuilder:

Public Types
enum	ArcLengthType { ArcLengthTypeBothXY, ArcLengthTypeFirstXThenY, ArcLengthTypeFirstYThenX, ArcLengthTypeXOnly, ArcLengthTypeYOnly }
	Represents Equal Arc Length type. More...

enum	DirectionType { DirectionTypeAlongFaceNormal, DirectionTypeTowardPoint, DirectionTypeTowardLine, DirectionTypeAlongVector, DirectionTypeAngleToVector }
	Represents direction method. More...

enum	ProjectionOptionType { ProjectionOptionTypeNone, ProjectionOptionTypeProjectBothSides, ProjectionOptionTypeEqualArcLength }
	Represents projection option type used when direction type is along vector. More...

Public Member Functions
NXOpen::Expression *	AngleToProjectionVector ()
	Returns the angle to projection vector Created in NX5.0.0. More...

double	BridgedGapSize ()
	Returns the maximum bridged gap size. More...

NXOpen::GeometricUtilities::CurveFitData *	CurveFitData ()
	Returns the curve fit settings Created in NX8.0.0. More...

NXOpen::GeometricUtilities::CurveFitJoin *	CurveFitJoinData ()
	Returns the curve fit join method More...

NXOpen::Features::ProjectCurveBuilder::ArcLengthType	EqualArcLengthMethod ()
	Returns the equal arc length method Created in NX5.0.0. More...

NXOpen::SelectObjectList *	FaceToProjectTo ()
	Returns the face to project to Created in NX5.0.0. More...

bool	GapOption ()
	Returns the gap option whether to create curve to bridge gap or not Created in NX7.5.0. More...

NXOpen::GeometricUtilities::CurveOptions *	InputCurvesOption ()
	Returns the input curves option Created in NX5.0.0. More...

NXOpen::SelectDisplayableObject *	LineToProjectToward ()
	Returns the line to project toward Created in NX5.0.0. More...

bool	NearestPointOption ()
	Returns the nearest point option whether to project curve by nearest point or not. More...

NXOpen::Plane *	PlaneToProjectTo ()
	Returns the plane to project to Created in NX5.0.0. More...

NXOpen::Point *	PointToProjectToward ()
	Returns the point to project toward Created in NX5.0.0. More...

NXOpen::Features::ProjectCurveBuilder::DirectionType	ProjectionDirectionMethod ()
	Returns the projection direction method Created in NX5.0.0. More...

NXOpen::Features::ProjectCurveBuilder::ProjectionOptionType	ProjectionOption ()
	Returns the projection option type Created in NX5.0.0. More...

NXOpen::Direction *	ProjectionVector ()
	Returns the projection vector Created in NX5.0.0. More...

NXOpen::Point *	ReferencePointForEqualArcLength ()
	Returns the reference point for equal arc length Created in NX5.0.0. More...

NXOpen::Section *	SectionToProject ()
	Returns the section to project Created in NX5.0.0. More...

void	SetBridgedGapSize (double bridgedGapSize)
	Sets the maximum bridged gap size. More...

void	SetEqualArcLengthMethod (NXOpen::Features::ProjectCurveBuilder::ArcLengthType arcLengthMethod)
	Sets the equal arc length method Created in NX5.0.0. More...

void	SetGapOption (bool gapOption)
	Sets the gap option whether to create curve to bridge gap or not Created in NX7.5.0. More...

void	SetNearestPointOption (bool nearestPointOption)
	Sets the nearest point option whether to project curve by nearest point or not. More...

void	SetPlaneToProjectTo (NXOpen::Plane *projectedPlane)
	Sets the plane to project to Created in NX5.0.0. More...

void	SetPointToProjectToward (NXOpen::Point *towardPoint)
	Sets the point to project toward Created in NX5.0.0. More...

void	SetProjectionDirectionMethod (NXOpen::Features::ProjectCurveBuilder::DirectionType directionMethod)
	Sets the projection direction method Created in NX5.0.0. More...

void	SetProjectionOption (NXOpen::Features::ProjectCurveBuilder::ProjectionOptionType projectionOption)
	Sets the projection option type Created in NX5.0.0. More...

void	SetProjectionVector (NXOpen::Direction *alongVector)
	Sets the projection vector Created in NX5.0.0. More...

void	SetReferencePointForEqualArcLength (NXOpen::Point *referencePoint)
	Sets the reference point for equal arc length Created in NX5.0.0. More...

void	SetTolerance (double tolerance)
	Sets the tolerance Created in NX5.0.0. More...

void	SetXVectorForEqualArcLength (NXOpen::Direction *xVector)
	Sets the x vector for equal arc length Created in NX5.0.0. More...

double	Tolerance ()
	Returns the tolerance Created in NX5.0.0. More...

NXOpen::Direction *	XVectorForEqualArcLength ()
	Returns the x vector for equal arc length Created in NX5.0.0. 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 NXOpen::Features::ProjectCurve builder.

Inputs to this class can be convergent objects.
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreateProjectCurveBuilder
Default values.

Property

Value

AngleToProjectionVector.Value

0.0

BridgedGapSize

1.0 (millimeters part), 0.04 (inches part)

CurveFitData.CurveJoinMethod

No

CurveFitData.Degree

7

CurveFitData.FitMethod

DegreeAndSegments

CurveFitData.IsAdvancedFit

0

CurveFitData.IsAlignShape

0

CurveFitData.MaximumDegree

7

CurveFitData.MaximumSegments

1

CurveFitData.MinimumDegree

5

CurveFitData.Segments

1

CurveFitJoinData.CurveFitOptions.FitOption (deprecated)

Cubic

CurveFitJoinData.CurveFitOptions.MaximumDegree (deprecated)

7

CurveFitJoinData.CurveFitOptions.MaximumSegments (deprecated)

1

EqualArcLengthMethod

BothXY

GapOption

false

InputCurvesOption.Associative

True

NearestPointOption

false

ProjectionDirectionMethod

AlongFaceNormal

ProjectionOption

None

Created in NX5.0.0.

Member Enumeration Documentation

enum NXOpen::Features::ProjectCurveBuilder::ArcLengthType

Represents Equal Arc Length type.

Enumerator
ArcLengthTypeBothXY	Represents Both X and Y.
ArcLengthTypeFirstXThenY	Represents First X then Y.
ArcLengthTypeFirstYThenX	Represents First Y then X.
ArcLengthTypeXOnly	Represents X only.
ArcLengthTypeYOnly	Represents Y only.

enum NXOpen::Features::ProjectCurveBuilder::DirectionType

Represents direction method.

Enumerator
DirectionTypeAlongFaceNormal	Represents Along Face Normal.
DirectionTypeTowardPoint	Represents Towards Point.
DirectionTypeTowardLine	Represents Towards Line.
DirectionTypeAlongVector	Represents Along Vector.
DirectionTypeAngleToVector	Represents Angle To Vector.

enum NXOpen::Features::ProjectCurveBuilder::ProjectionOptionType

Represents projection option type used when direction type is along vector.

Enumerator
ProjectionOptionTypeNone	Represents None.
ProjectionOptionTypeProjectBothSides	Represents Project Both Sides.
ProjectionOptionTypeEqualArcLength	Represents Equal Arc Length.

Member Function Documentation

NXOpen::Expression* NXOpen::Features::ProjectCurveBuilder::AngleToProjectionVector ( )

Returns the angle to projection vector
Created in NX5.0.0.

License requirements : None

double NXOpen::Features::ProjectCurveBuilder::BridgedGapSize ( )

Returns the maximum bridged gap size.

When gap distance is less than maximum bridged gap size and bigger than the default modeling tolerance, NX project curve will add an internal bridge curve to close the gap between segments in projection curve. This option is only valid if NXOpen::Features::ProjectCurveBuilder::GapOption and NXOpen::Features::ProjectCurveBuilder::SetGapOption is true.

Created in NX7.5.0.

License requirements : None

NXOpen::GeometricUtilities::CurveFitData* NXOpen::Features::ProjectCurveBuilder::CurveFitData ( )

Returns the curve fit settings
Created in NX8.0.0.

License requirements : None

NXOpen::GeometricUtilities::CurveFitJoin* NXOpen::Features::ProjectCurveBuilder::CurveFitJoinData ( )

Returns the curve fit join method

Deprecated:: Deprecated in NX8.0.0.

Use NXOpen::Features::ProjectCurveBuilder::CurveFitData instead

Created in NX5.0.0.

License requirements : None

NXOpen::Features::ProjectCurveBuilder::ArcLengthType NXOpen::Features::ProjectCurveBuilder::EqualArcLengthMethod ( )

Returns the equal arc length method
Created in NX5.0.0.

License requirements : None

NXOpen::SelectObjectList* NXOpen::Features::ProjectCurveBuilder::FaceToProjectTo ( )

Returns the face to project to
Created in NX5.0.0.

License requirements : None

bool NXOpen::Features::ProjectCurveBuilder::GapOption ( )

Returns the gap option whether to create curve to bridge gap or not
Created in NX7.5.0.

License requirements : None

NXOpen::GeometricUtilities::CurveOptions* NXOpen::Features::ProjectCurveBuilder::InputCurvesOption ( )

Returns the input curves option
Created in NX5.0.0.

License requirements : None

NXOpen::SelectDisplayableObject* NXOpen::Features::ProjectCurveBuilder::LineToProjectToward ( )

Returns the line to project toward
Created in NX5.0.0.

License requirements : None

bool NXOpen::Features::ProjectCurveBuilder::NearestPointOption ( )

Returns the nearest point option whether to project curve by nearest point or not.

This option is only valid if NXOpen::Features::ProjectCurveBuilder::DirectionTypeAlongVector is used and NXOpen::Features::ProjectCurveBuilder::ProjectionOptionTypeNone or NXOpen::Features::ProjectCurveBuilder::ProjectionOptionTypeProjectBothSides is used.

Created in NX7.5.0.

License requirements : None

NXOpen::Plane* NXOpen::Features::ProjectCurveBuilder::PlaneToProjectTo ( )

Returns the plane to project to
Created in NX5.0.0.

License requirements : None

NXOpen::Point* NXOpen::Features::ProjectCurveBuilder::PointToProjectToward ( )

Returns the point to project toward
Created in NX5.0.0.

License requirements : None

NXOpen::Features::ProjectCurveBuilder::DirectionType NXOpen::Features::ProjectCurveBuilder::ProjectionDirectionMethod ( )

Returns the projection direction method
Created in NX5.0.0.

License requirements : None

NXOpen::Features::ProjectCurveBuilder::ProjectionOptionType NXOpen::Features::ProjectCurveBuilder::ProjectionOption ( )

Returns the projection option type
Created in NX5.0.0.

License requirements : None

NXOpen::Direction* NXOpen::Features::ProjectCurveBuilder::ProjectionVector ( )

Returns the projection vector
Created in NX5.0.0.

License requirements : None

NXOpen::Point* NXOpen::Features::ProjectCurveBuilder::ReferencePointForEqualArcLength ( )

Returns the reference point for equal arc length
Created in NX5.0.0.

License requirements : None

NXOpen::Section* NXOpen::Features::ProjectCurveBuilder::SectionToProject ( )

Returns the section to project
Created in NX5.0.0.

License requirements : None

void NXOpen::Features::ProjectCurveBuilder::SetBridgedGapSize ( double bridgedGapSize )

Sets the maximum bridged gap size.

When gap distance is less than maximum bridged gap size and bigger than the default modeling tolerance, NX project curve will add an internal bridge curve to close the gap between segments in projection curve. This option is only valid if NXOpen::Features::ProjectCurveBuilder::GapOption and NXOpen::Features::ProjectCurveBuilder::SetGapOption is true.

Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

bridgedGapSize bridgedgapsize

void NXOpen::Features::ProjectCurveBuilder::SetEqualArcLengthMethod ( NXOpen::Features::ProjectCurveBuilder::ArcLengthType arcLengthMethod )

Sets the equal arc length method
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

arcLengthMethod arclengthmethod

void NXOpen::Features::ProjectCurveBuilder::SetGapOption ( bool gapOption )

Sets the gap option whether to create curve to bridge gap or not
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

gapOption gapoption

void NXOpen::Features::ProjectCurveBuilder::SetNearestPointOption ( bool nearestPointOption )

Sets the nearest point option whether to project curve by nearest point or not.

This option is only valid if NXOpen::Features::ProjectCurveBuilder::DirectionTypeAlongVector is used and NXOpen::Features::ProjectCurveBuilder::ProjectionOptionTypeNone or NXOpen::Features::ProjectCurveBuilder::ProjectionOptionTypeProjectBothSides is used.

Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

nearestPointOption nearestpointoption

void NXOpen::Features::ProjectCurveBuilder::SetPlaneToProjectTo ( NXOpen::Plane * projectedPlane )

Sets the plane to project to
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

projectedPlane projectedplane

void NXOpen::Features::ProjectCurveBuilder::SetPointToProjectToward ( NXOpen::Point * towardPoint )

Sets the point to project toward
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

towardPoint towardpoint

void NXOpen::Features::ProjectCurveBuilder::SetProjectionDirectionMethod ( NXOpen::Features::ProjectCurveBuilder::DirectionType directionMethod )

Sets the projection direction method
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

directionMethod directionmethod

void NXOpen::Features::ProjectCurveBuilder::SetProjectionOption ( NXOpen::Features::ProjectCurveBuilder::ProjectionOptionType projectionOption )

Sets the projection option type
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

projectionOption projectionoption

void NXOpen::Features::ProjectCurveBuilder::SetProjectionVector ( NXOpen::Direction * alongVector )

Sets the projection vector
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

alongVector alongvector

void NXOpen::Features::ProjectCurveBuilder::SetReferencePointForEqualArcLength ( NXOpen::Point * referencePoint )

Sets the reference point for equal arc length
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

referencePoint referencepoint

void NXOpen::Features::ProjectCurveBuilder::SetTolerance ( double tolerance )

Sets the tolerance
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

tolerance tolerance

void NXOpen::Features::ProjectCurveBuilder::SetXVectorForEqualArcLength ( NXOpen::Direction * xVector )

Sets the x vector for equal arc length
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

xVector xvector

double NXOpen::Features::ProjectCurveBuilder::Tolerance ( )

Returns the tolerance
Created in NX5.0.0.

License requirements : None

NXOpen::Direction* NXOpen::Features::ProjectCurveBuilder::XVectorForEqualArcLength ( )

Returns the x vector for equal arc length
Created in NX5.0.0.

License requirements : None

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

Features_ProjectCurveBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation