Represents a NXOpen::SketchProjectBuilder builder
To create a new instance of this class, use NXOpen::SketchCollection::CreateProjectBuilder
Default values. More...

Inheritance diagram for NXOpen::SketchProjectBuilder:

Public Types
enum	OutputCurve { OutputCurveOriginal, OutputCurveSplineSegment, OutputCurveSingleSpline }
	This enum represents the kind of output curves. More...

Public Member Functions
bool	Associativity ()
	Returns the associativity of projection. More...

NXOpen::SelectNXObjectList *	CurveList ()
	Returns the curve list. More...

NXOpen::SketchProjectBuilder::OutputCurve	CurveType ()
	Returns the output curve type generated by the projection. More...

bool	ProjectAsDumbFixedCurves ()
	Returns the flag to indicate if the projection output needs to be converted to dumb fully fixed curves in the sketch. More...

NXOpen::Section *	Section ()
	Returns the section. More...

void	SetAssociativity (bool associativity)
	Sets the associativity of projection. More...

void	SetCurveType (NXOpen::SketchProjectBuilder::OutputCurve curveType)
	Sets the output curve type generated by the projection. More...

void	SetProjectAsDumbFixedCurves (bool projectAsDumbFixed)
	Sets the flag to indicate if the projection output needs to be converted to dumb fully fixed curves in the sketch. More...

void	SetTolerance (double tolerance)
	Sets the tolerance value used for the projection. More...

double	Tolerance ()
	Returns the tolerance value used for the projection. More...

Public Member Functions inherited from NXOpen::Features::EmbeddedOperationBuilder
NXOpen::Features::Feature *	CommitOperation ()
	Commits the operation and creates the feature. More...

NXOpen::Features::Feature *	GetOperation ()
	Returns the feature currently being edited by this builder. 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::SketchProjectBuilder builder
To create a new instance of this class, use NXOpen::SketchCollection::CreateProjectBuilder
Default values.

Property

Value

Associativity

True

CurveType

Original

Created in NX5.0.0.

Member Enumeration Documentation

enum NXOpen::SketchProjectBuilder::OutputCurve

This enum represents the kind of output curves.

Enumerator
OutputCurveOriginal	original curve output
OutputCurveSplineSegment	spline segment output
OutputCurveSingleSpline	single spline output

Member Function Documentation

bool NXOpen::SketchProjectBuilder::Associativity ( )

Returns the associativity of projection.

If this variable is turned on, the output curves will always depend on the input curves. So that when the input curves change, the output curves will change accordingly. If this variable is set to false, the output curves derive their shape from current stage of the input curves and then become independent of the input curves. In drafting mode, one can not project curves in associative manner. Also if the curves belong to multiple parts, they can not be projected in associative manner.
Created in NX5.0.0.

License requirements : None

NXOpen::SelectNXObjectList* NXOpen::SketchProjectBuilder::CurveList ( )

Returns the curve list.

The curves to project should be added to this list only if they belong to multiple parts and they are to be projected in non associative manner. All the curves to be projected should either go to the section or the curve list depending on their owning parts.
Created in NX5.0.0.

License requirements : None

NXOpen::SketchProjectBuilder::OutputCurve NXOpen::SketchProjectBuilder::CurveType ( )

Returns the output curve type generated by the projection.

Depending on this value, the projected curve can have the same geometry as the input curves or it can be a single spline curve or a set of splines.
Created in NX5.0.0.

License requirements : None

bool NXOpen::SketchProjectBuilder::ProjectAsDumbFixedCurves ( )

Returns the flag to indicate if the projection output needs to be converted to dumb fully fixed curves in the sketch.

This flag overrides the associativity flag i.e. if both projectAsDumbFixed and associativity are set to true, the result will be dumb fixed curves and not an associative projection.
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

NXOpen::Section* NXOpen::SketchProjectBuilder::Section ( )

Returns the section.

The curves to project should be added to the section if they do not belong to multiple parts. All the curves to be projected should either go to the section or the curve list depending on their owning parts.
Created in NX5.0.0.

License requirements : None

void NXOpen::SketchProjectBuilder::SetAssociativity ( bool associativity )

Sets the associativity of projection.

If this variable is turned on, the output curves will always depend on the input curves. So that when the input curves change, the output curves will change accordingly. If this variable is set to false, the output curves derive their shape from current stage of the input curves and then become independent of the input curves. In drafting mode, one can not project curves in associative manner. Also if the curves belong to multiple parts, they can not be projected in associative manner.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

associativity associativity

void NXOpen::SketchProjectBuilder::SetCurveType ( NXOpen::SketchProjectBuilder::OutputCurve curveType )

Sets the output curve type generated by the projection.

Depending on this value, the projected curve can have the same geometry as the input curves or it can be a single spline curve or a set of splines.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

curveType curve type

void NXOpen::SketchProjectBuilder::SetProjectAsDumbFixedCurves ( bool projectAsDumbFixed )

Sets the flag to indicate if the projection output needs to be converted to dumb fully fixed curves in the sketch.

This flag overrides the associativity flag i.e. if both projectAsDumbFixed and associativity are set to true, the result will be dumb fixed curves and not an associative projection.
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

projectAsDumbFixed projectasdumbfixed

void NXOpen::SketchProjectBuilder::SetTolerance ( double tolerance )

Sets the tolerance value used for the projection.

The same value is used for the tolerances related to the section.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

tolerance tolerance

double NXOpen::SketchProjectBuilder::Tolerance ( )

Returns the tolerance value used for the projection.

The same value is used for the tolerances related to the section.
Created in NX5.0.0.

License requirements : None

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

SketchProjectBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation