Represents a NXOpen::Features::PatternFeature builder
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreatePatternFeatureBuilder
Default values. More...

Inheritance diagram for NXOpen::Features::PatternFeatureBuilder:

Public Types
enum	ExpressionTransferOptions { ExpressionTransferOptionsCreateNew, ExpressionTransferOptionsLinkToOriginal, ExpressionTransferOptionsOriginalInstance }
	the Expression transfer options. More...

enum	OutputOptions { OutputOptionsPatternFeature, OutputOptionsCopiesOfInputFeatures, OutputOptionsCopiesOfInputFeaturesInGroup }
	the Output options. More...

enum	PatternMethodOptions { PatternMethodOptionsVariational = 1, PatternMethodOptionsSimple }
	the Pattern method options. More...

Public Member Functions
void	ClearReferencesToReuse ()
	Clears all the existing references to reuse so that new references can be added Created in NX8.0.0. More...

bool	CreateReferencePattern ()
	Returns the Create Reference Pattern option Created in NX8.0.0. More...

NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions	ExpressionOption ()
	Returns the expression transfer option Created in NX7.5.0. More...

NXOpen::Features::SelectFeatureList *	FeatureList ()
	Returns the Features Created in NX7.5.0. More...

NXOpen::Features::PatternFeatureBuilder::OutputOptions	OutputOption ()
	Returns the output option Created in NX8.0.0. More...

NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions	PatternMethod ()
	Returns the Pattern method Created in NX7.5.0. More...

NXOpen::GeometricUtilities::PatternDefinition *	PatternService ()
	Returns the Pattern definition service Created in NX7.5.0. More...

NXOpen::Point *	ReferencePoint ()
	Returns the reference point More...

NXOpen::GeometricUtilities::PatternReferencePointServiceBuilder *	ReferencePointService ()
	Returns the reference point service Created in NX9.0.0. More...

void	RemoveAllClocking ()
	Removes clocking from (unclocks) all instances of the NXOpen::Features::PatternFeature . More...

void	SetCreateReferencePattern (bool createReferencePattern)
	Sets the Create Reference Pattern option Created in NX8.0.0. More...

void	SetExpressionOption (NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions expressionOption)
	Sets the expression transfer option Created in NX7.5.0. More...

void	SetOutputOption (NXOpen::Features::PatternFeatureBuilder::OutputOptions outputOption)
	Sets the output option Created in NX8.0.0. More...

void	SetPatternMethod (NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions methodOption)
	Sets the Pattern method Created in NX7.5.0. More...

void	SetReferencePoint (NXOpen::Point *referencePoint)
	Sets the reference point More...

void	SetReferencesToReuse (NXOpen::Features::Feature inputFeature, const std::vector< NXOpen::NXObject > &referencesFromInputFeatures)
	Sets the references or selections from the input features which are to be reused for all instances. More...

void	SetUseInferredReferencePoint (bool useInferredReferencePoint)
	Sets a flag to indicate whether to use reference point inferred from selected feature(s) or not. More...

bool	UseInferredReferencePoint ()
	Returns a flag to indicate whether to use reference point inferred from selected feature(s) or not. 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::PatternFeature builder
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreatePatternFeatureBuilder
Default values.

Property

Value

CreateReferencePattern

True

ExpressionOption

CreateNew

OutputOption

PatternFeature

PatternMethod

Variational

PatternService.AlongPathDefinition.XOnPathSpacing.NCopies.Value

2

PatternService.AlongPathDefinition.XOnPathSpacing.SpaceType

Offset

PatternService.AlongPathDefinition.XPathOption

Offset

PatternService.AlongPathDefinition.YDirectionOption

Section

PatternService.AlongPathDefinition.YOnPathSpacing.NCopies.Value

1

PatternService.AlongPathDefinition.YPathOption

Offset

PatternService.AlongPathDefinition.YSpacing.NCopies.Value

1

PatternService.AlongPathDefinition.YSpacing.PitchDistance.Value

10 (millimeters part), 1 (inches part)

PatternService.AlongPathDefinition.YSpacing.SpaceType

Offset

PatternService.AlongPathDefinition.YSpacing.SpanDistance.Value

100 (millimeters part), 10 (inches part)

PatternService.CircularDefinition.AngularSpacing.NCopies.Value

12

PatternService.CircularDefinition.AngularSpacing.PitchAngle.Value

30

PatternService.CircularDefinition.AngularSpacing.PitchDistance.Value

10 (millimeters part), 1 (inches part)

PatternService.CircularDefinition.AngularSpacing.SpaceType

Offset

PatternService.CircularDefinition.AngularSpacing.SpanAngle.Value

360 (millimeters part), 360 (inches part)

PatternService.CircularDefinition.AngularSpacing.UsePitchOption

Angle

PatternService.CircularDefinition.CreateLastStaggered

true

PatternService.CircularDefinition.HorizontalRef.RotationAngle.Value

0 (millimeters part), 0 (inches part)

PatternService.CircularDefinition.IncludeSeedToggle

true

PatternService.CircularDefinition.RadialSpacing.NCopies.Value

1

PatternService.CircularDefinition.StaggerType

None

PatternService.HelixDefinition.AnglePitch.Value

30

PatternService.HelixDefinition.CountOfInstances.Value

6

PatternService.HelixDefinition.DirectionType

Righthand

PatternService.HelixDefinition.DistancePitch.Value

10 (millimeters part), 0.4 (inches part)

PatternService.HelixDefinition.HelixPitch.Value

50 (millimeters part), 2 (inches part)

PatternService.HelixDefinition.HelixSpan.Value

100 (millimeters part), 4 (inches part)

PatternService.HelixDefinition.NumberOfTurns.Value

2

PatternService.HelixDefinition.SizeOption

CountAngleDistance

PatternService.PatternFill.FillMargin.Value

0 (millimeters part), 0 (inches part)

PatternService.PatternFill.FillOptions

None

PatternService.PatternFill.SimplifiedBoundaryToggle

False

PatternService.PatternOrientation.AlongOrientationOption

NormalToPath

PatternService.PatternOrientation.CircularOrientationOption

FollowPattern

PatternService.PatternOrientation.FollowFaceProjDirOption

PatternPlaneNormal

PatternService.PatternOrientation.GeneralOrientationOption

Fixed

PatternService.PatternOrientation.HelixOrientationOption

FollowPattern

PatternService.PatternOrientation.LinearOrientationOption

Fixed

PatternService.PatternOrientation.MirrorOrientationOption

FollowPattern

PatternService.PatternOrientation.OrientationOption

Fixed

PatternService.PatternOrientation.PolygonOrientationOption

FollowPattern

PatternService.PatternOrientation.SpiralOrientationOption

FollowPattern

PatternService.PatternType

Linear

PatternService.PolygonDefinition.NumberOfSides.Value

6

PatternService.PolygonDefinition.PolygonSizeOption

Inscribed

PatternService.PolygonDefinition.PolygonSpacing.NCopies.Value

4

PatternService.PolygonDefinition.PolygonSpacing.PitchDistance.Value

25 (millimeters part), 1 (inches part)

PatternService.PolygonDefinition.PolygonSpacing.SpaceType

Offset

PatternService.PolygonDefinition.PolygonSpacing.SpanAngle.Value

360

PatternService.PolygonDefinition.RadialSpacing.NCopies.Value

1

PatternService.PolygonDefinition.RadialSpacing.PitchDistance.Value

25 (millimeters part), 1 (inches part)

PatternService.PolygonDefinition.RadialSpacing.SpanDistance.Value

100 (millimeters part), 4 (inches part)

PatternService.RectangularDefinition.CreateLastStaggered

true

PatternService.RectangularDefinition.SimplifiedLayoutType

Square

PatternService.RectangularDefinition.StaggerType

None

PatternService.RectangularDefinition.XSpacing.NCopies.Value

2

PatternService.RectangularDefinition.YSpacing.NCopies.Value

1

PatternService.SpiralDefinition.DirectionType

Lefthand

PatternService.SpiralDefinition.NumberOfTurns.Value

1 (millimeters part), 1 (inches part)

PatternService.SpiralDefinition.RadialPitch.Value

50 (millimeters part), 2 (inches part)

PatternService.SpiralDefinition.SizeSpiralType

NumberOfTurns

PatternService.SpiralDefinition.TotalAngle.Value

360 (millimeters part), 360 (inches part)

UseInferredReferencePoint (deprecated)

True

Created in NX7.5.0.

Member Enumeration Documentation

enum NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions

the Expression transfer options.

Enumerator
ExpressionTransferOptionsCreateNew	New.
ExpressionTransferOptionsLinkToOriginal	Link to Original.
ExpressionTransferOptionsOriginalInstance	Instance of Original.

enum NXOpen::Features::PatternFeatureBuilder::OutputOptions

the Output options.

Enumerator
OutputOptionsPatternFeature	Pattern Feature.
OutputOptionsCopiesOfInputFeatures	Copies of Input features.
OutputOptionsCopiesOfInputFeaturesInGroup	Copies of Input features in Group.

enum NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions

the Pattern method options.

Enumerator
PatternMethodOptionsVariational	variational
PatternMethodOptionsSimple	simple

Member Function Documentation

void NXOpen::Features::PatternFeatureBuilder::ClearReferencesToReuse ( )

Clears all the existing references to reuse so that new references can be added
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

bool NXOpen::Features::PatternFeatureBuilder::CreateReferencePattern ( )

Returns the Create Reference Pattern option
Created in NX8.0.0.

License requirements : None

NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions NXOpen::Features::PatternFeatureBuilder::ExpressionOption ( )

Returns the expression transfer option
Created in NX7.5.0.

License requirements : None

NXOpen::Features::SelectFeatureList* NXOpen::Features::PatternFeatureBuilder::FeatureList ( )

Returns the Features
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

NXOpen::Features::PatternFeatureBuilder::OutputOptions NXOpen::Features::PatternFeatureBuilder::OutputOption ( )

Returns the output option
Created in NX8.0.0.

License requirements : None

NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions NXOpen::Features::PatternFeatureBuilder::PatternMethod ( )

Returns the Pattern method
Created in NX7.5.0.

License requirements : None

NXOpen::GeometricUtilities::PatternDefinition* NXOpen::Features::PatternFeatureBuilder::PatternService ( )

Returns the Pattern definition service
Created in NX7.5.0.

License requirements : None

NXOpen::Point* NXOpen::Features::PatternFeatureBuilder::ReferencePoint ( )

Returns the reference point

Deprecated:: Deprecated in NX9.0.0.

Use GeometricUtilities::PatternReferencePointServiceBuilder::Point instead.

Created in NX7.5.0.

License requirements : None

NXOpen::GeometricUtilities::PatternReferencePointServiceBuilder* NXOpen::Features::PatternFeatureBuilder::ReferencePointService ( )

Returns the reference point service
Created in NX9.0.0.

License requirements : None

void NXOpen::Features::PatternFeatureBuilder::RemoveAllClocking ( )

Removes clocking from (unclocks) all instances of the NXOpen::Features::PatternFeature .

Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

void NXOpen::Features::PatternFeatureBuilder::SetCreateReferencePattern ( bool createReferencePattern )

Sets the Create Reference Pattern option
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

createReferencePattern createreferencepattern

void NXOpen::Features::PatternFeatureBuilder::SetExpressionOption ( NXOpen::Features::PatternFeatureBuilder::ExpressionTransferOptions expressionOption )

Sets the expression transfer option
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

expressionOption expressionoption

void NXOpen::Features::PatternFeatureBuilder::SetOutputOption ( NXOpen::Features::PatternFeatureBuilder::OutputOptions outputOption )

Sets the output option
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

outputOption outputoption

void NXOpen::Features::PatternFeatureBuilder::SetPatternMethod ( NXOpen::Features::PatternFeatureBuilder::PatternMethodOptions methodOption )

Sets the Pattern method
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

methodOption methodoption

void NXOpen::Features::PatternFeatureBuilder::SetReferencePoint ( NXOpen::Point * referencePoint )

Sets the reference point

Deprecated:: Deprecated in NX9.0.0.

Use GeometricUtilities::PatternReferencePointServiceBuilder::SetPoint instead.

Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

referencePoint referencepoint

void NXOpen::Features::PatternFeatureBuilder::SetReferencesToReuse	(	NXOpen::Features::Feature *	inputFeature,
		const std::vector< NXOpen::NXObject * > &	referencesFromInputFeatures
	)

Sets the references or selections from the input features which are to be reused for all instances.

The references for reuse should belong to some input feature which needs to be specified while calling this API.
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

inputFeature	inputfeature
referencesFromInputFeatures	referencesfrominputfeatures

void NXOpen::Features::PatternFeatureBuilder::SetUseInferredReferencePoint ( bool useInferredReferencePoint )

Sets a flag to indicate whether to use reference point inferred from selected feature(s) or not.

If 'true', the reference point will be inferred every time the selected feature(s) get modified or updates. If 'false, the reference point provided will be independent of the selected feature(s) but will be associative to the rule by which it was created (e.g. End of Line, Center of Arc).

Deprecated:: Deprecated in NX9.0.0. Use GeometricUtilities::PatternReferencePointServiceBuilder::SetReferencePointInferred instead.

Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

useInferredReferencePoint useinferredreferencepoint

bool NXOpen::Features::PatternFeatureBuilder::UseInferredReferencePoint ( )

Returns a flag to indicate whether to use reference point inferred from selected feature(s) or not.

If 'true', the reference point will be inferred every time the selected feature(s) get modified or updates. If 'false, the reference point provided will be independent of the selected feature(s) but will be associative to the rule by which it was created (e.g. End of Line, Center of Arc).

Deprecated:: Deprecated in NX9.0.0. Use GeometricUtilities::PatternReferencePointServiceBuilder::IsReferencePointInferred instead.

Created in NX8.0.0.

License requirements : None

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

Features_PatternFeatureBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation