NXOpen.Features.PointSetBuilder Class Reference

Represents a NXOpen.Features.PointSetBuilder . More...

Inheritance diagram for NXOpen.Features.PointSetBuilder:

Public Types
enum	CurvePointsType {   EqualArcLength, EqualParameters, GeometricProgression, ChordalTolerance,   IncrementalArcLength, SpecifiedProjectionPoints, CurvePercentage }
	The settings for the curve points definition. More...
enum	FacePointsType { Pattern, FacePercentage, BSurfacePoles }
	The settings for the face points definition. More...
enum	PatternLimitsType { DiagonalPoints, Percentages }
	The settings for the pattern limit definition. More...
enum	SplinePointsType { DefiningPoints, Knots, Poles }
	The settings for the spline points definition. More...
enum	Types { CurvePoints, SplinePoints, FacePoints, IntersectionPoints }
	The settings for the type of Point Set feature. More...

Public Member Functions
unsafe NXOpen.Features.PointSetFacePercentageBuilder	CreateFacePercentageListItem ()
	Create an entry for the face percentage list. More...
Public Member Functions inherited from NXOpen.Features.FeatureBuilder
unsafe NXOpen.Features.Feature	CommitFeature ()
	Commits the feature parameters and creates the feature More...
unsafe NXOpen.Features.Feature	GetFeature ()
	Returns the feature currently being edited by this builder. More...
unsafe void	HideInternalParentFeatureAfterEdit (NXOpen.Features.Feature parentFeature)
	Re-suppress an internal parent feature (a slave feature) after it has been edited. More...
unsafe void	SetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited More...
unsafe void	ShowInternalParentFeatureForEdit (NXOpen.Features.Feature parentFeature)
	Unsuppress an internal parent feature (a slave feature) so it can be edited. More...
unsafe void	UnsetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the internal parent feature of the feature being edited to external More...
Public Member Functions inherited from NXOpen.Builder
unsafe NXOpen.NXObject	Commit ()
	Commits any edits that have been applied to the builder. More...
unsafe void	Destroy ()
	Deletes the builder, and cleans up any objects created by the builder. More...
unsafe NXOpen.NXObject[]	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...
unsafe NXOpen.NXObject	GetObject ()
	Returns the object currently being edited by this builder. More...
unsafe void	ShowResults ()
	Updates the model to reflect the result of an edit to the model for all builders that support showing results. More...
unsafe bool	Validate ()
	Validate whether the inputs to the component are sufficient for commit to be called. More...
Public Member Functions inherited from NXOpen.TaggedObject
void	PrintTestData (String variableName)
	<exclude> More...
void	PrintTestData (String variableName, int lineNumber)
	<exclude> More...
override string	ToString ()
	Returns a String that represents the current Object. More...
Public Member Functions inherited from NXOpen.Utilities.NXRemotableObject
IMessageCtrl	AsyncProcessMessage (IMessage msg, IMessageSink replySink)
	Asynchronously processes the given message. More...
IMessage	SyncProcessMessage (IMessage msg)
	Synchronously processes the given message. More...

Properties
unsafe double	AngleTolerance [get, set]
	Returns or sets the angle tolerance. More...
unsafe NXOpen.Expression	ArcLength [get]
	Returns the arc length of the curve at which a point is to be created. More...
unsafe bool	Associative [get, set]
	Returns or sets the associative setting. More...
unsafe NXOpen.Expression	ChordalTolerance [get]
	Returns the chordal tolerance used in creating points. More...
unsafe NXOpen.NXObjectList	CurvePercentageList [get]
	Returns the curve percentage list. More...
unsafe NXOpen.Features.PointSetBuilder.CurvePointsType	CurvePointsBy [get, set]
	Returns or sets the curve points definition setting. More...
unsafe double	DistanceTolerance [get, set]
	Returns or sets the distance tolerance. More...
unsafe NXOpen.Expression	EndPercentage [get]
	Returns the percentage of the curve at which to stop creating points. More...
unsafe NXOpen.Section	EndPercentageSection [get]
	Returns a section containing an object (curve, edge, or point) that will be used to determine an intersection with the curves/edges selected for setting the EndPercentage Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression . More...
unsafe NXOpen.Features.PointSetFacePercentageBuilderList	FacePercentageList [get]
	Returns the face percentage list. More...
unsafe NXOpen.Features.PointSetBuilder.FacePointsType	FacePointsBy [get, set]
	Returns or sets the face points definition setting. More...
unsafe bool	GroupPoints [get, set]
	Returns or sets the group points setting. More...
unsafe NXOpen.Section	IntersectionSection [get]
	Returns the intersection Section. More...
unsafe NXOpen.SelectDisplayableObjectList	IntersectionSelectedObjects [get]
	Returns the intersection selected objects. More...
unsafe NXOpen.SelectDisplayableObjectList	IntersectionSelectedObjectsSecond [get]
	Returns the intersection selected objects second. More...
unsafe NXOpen.Section	MultipleCurveOrEdgeCollector [get]
	Returns the collector that is used to hold multiple curves or edges. More...
unsafe NXOpen.ScCollector	MultipleFaceCollector [get]
	Returns the collector that is used to hold faces. More...
unsafe NXOpen.Expression	NumberOfPointsExpression [get]
	Returns the number of points that will be created along curve. More...
unsafe NXOpen.Expression	NumberOfPointsInUDirectionExpression [get]
	Returns the number of points to be created in the u direction. More...
unsafe NXOpen.Expression	NumberOfPointsInVDirectionExpression [get]
	Returns the number of points to be created in the v direction. More...
unsafe NXOpen.Features.PointSetBuilder.PatternLimitsType	PatternLimitsBy [get, set]
	Returns or sets the pattern limits definition setting. More...
unsafe NXOpen.Expression	PatternLimitsEndingUValue [get]
	Returns the ending u value of the pattern. More...
unsafe NXOpen.Expression	PatternLimitsEndingVValue [get]
	Returns the ending v value of the pattern. More...
unsafe NXOpen.Point	PatternLimitsEndPoint [get, set]
	Returns or sets the ending diagonal point of the pattern. More...
unsafe NXOpen.Expression	PatternLimitsStartingUValue [get]
	Returns the starting u value of the pattern. More...
unsafe NXOpen.Expression	PatternLimitsStartingVValue [get]
	Returns the starting v value of the pattern. More...
unsafe NXOpen.Point	PatternLimitsStartPoint [get, set]
	Returns or sets the starting diagonal point of the pattern. More...
unsafe NXOpen.PointList	ProjectionPointList [get]
	Returns the projection point list. More...
unsafe NXOpen.Expression	Ratio [get]
	Returns the ratio of geometric progression. More...
unsafe NXOpen.Section	SingleCurveOrEdgeCollector [get]
	Returns the collector that is used to hold a single curve or edge definition. More...
unsafe NXOpen.SelectFace	SingleFaceObject [get]
	Returns the select object that is used to hold the face. More...
unsafe NXOpen.ScCollector	SplineCollector [get]
	Returns the collector that is used to hold a spline. More...
unsafe NXOpen.Features.PointSetBuilder.SplinePointsType	SplinePointsBy [get, set]
	Returns or sets the spline points definition setting. More...
unsafe NXOpen.Expression	StartPercentage [get]
	Returns the percentage of the curve at which to start creating points. More...
unsafe NXOpen.Section	StartPercentageSection [get]
	Returns a section containing an object (curve, edge, or point) that will be used to determine an intersection with the curves/edges selected for setting the StartPercentage Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression . More...
unsafe NXOpen.Features.PointSetBuilder.Types	Type [get, set]
	Returns or sets the type setting. More...
Properties inherited from NXOpen.Features.FeatureBuilder
unsafe bool	ParentFeatureInternal [get, set]
	Returns or sets whether or not the latest timestamped parent feature of this feature should be made internal More...
Properties inherited from NXOpen.Builder
unsafe NXOpen.PreviewBuilder	PreviewBuilder [get]
	Returns the preview builder subobject. More...
Properties inherited from NXOpen.TaggedObject
Tag	Tag [get]
	Returns the tag of this object. More...
Properties inherited from NXOpen.Utilities.NXRemotableObject
IMessageSink	NextSink [get]
	Gets the next message sink in the sink chain. More...

Additional Inherited Members
Protected Member Functions inherited from NXOpen.TaggedObject
new void	initialize ()
	<exclude> More...

Detailed Description

Represents a NXOpen.Features.PointSetBuilder .

This builder is used to create and edit Point Set features. The Point Set feature allows you to create points on curves, edges or faces.

To create a new instance of this class, use NXOpen.Features.FeatureCollection.CreatePointSetBuilder

Default values.

Property	Value
ArcLength.Value	1 (millimeters part), 0.01 (inches part)
Associative	1
ChordalTolerance.Value	2.54 (millimeters part), 0.1 (inches part)
CurvePointsBy	EqualArcLength
EndPercentage.Value	100
FacePointsBy	Pattern
NumberOfPointsExpression.Value	2
NumberOfPointsInUDirectionExpression.Value	10
NumberOfPointsInVDirectionExpression.Value	10
PatternLimitsBy	Percentages
PatternLimitsEndingUValue.Value	100
PatternLimitsEndingVValue.Value	100
PatternLimitsStartingUValue.Value	0
PatternLimitsStartingVValue.Value	0
Ratio.Value	1
SplinePointsBy	DefiningPoints
StartPercentage.Value	0

Created in NX6.0.0

Member Enumeration Documentation

enum NXOpen.Features.PointSetBuilder.CurvePointsType

The settings for the curve points definition.

Enumerator
EqualArcLength	Points will be created at equal arc length along curve.
EqualParameters	Points will be created at equal parameter spacing along curve.
GeometricProgression	Points will be created with a geometric progression along curve.
ChordalTolerance	Points will be created based on the chordal deviation of curve.
IncrementalArcLength	A point will be created at the arc length spacing input.
SpecifiedProjectionPoints	Points will be created at minimum distance to curve.
CurvePercentage	A point will be created at given curve percentage.

enum NXOpen.Features.PointSetBuilder.FacePointsType

The settings for the face points definition.

Enumerator
Pattern	Points will be created based on a defined pattern.
FacePercentage	A point will be created at given face percentages.
BSurfacePoles	Points will be created at surface poles.

enum NXOpen.Features.PointSetBuilder.PatternLimitsType

The settings for the pattern limit definition.

Enumerator
DiagonalPoints	The pattern limit is defined by two points.
Percentages	The pattern limit is defined by surface U and V values.

enum NXOpen.Features.PointSetBuilder.SplinePointsType

The settings for the spline points definition.

Enumerator
DefiningPoints	Points will be created at spline defining points.
Knots	Points will be created at spline knot points.
Poles	Points will be created at spline pole points.

enum NXOpen.Features.PointSetBuilder.Types

The settings for the type of Point Set feature.

Enumerator
CurvePoints	Create points along curve.
SplinePoints	Create points along spline.
FacePoints	Create points on face
IntersectionPoints	Create intersection points

Member Function Documentation

unsafe NXOpen.Features.PointSetFacePercentageBuilder NXOpen.Features.PointSetBuilder.CreateFacePercentageListItem ( )

inline

Create an entry for the face percentage list.

Created in NX6.0.0

License requirements: solid_modeling ("SOLIDS MODELING")

Returns

Property Documentation

unsafe double NXOpen.Features.PointSetBuilder.AngleTolerance

getset

Returns or sets the angle tolerance.

Used in determining curve tangency when needed.

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.ArcLength

get

Returns the arc length of the curve at which a point is to be created.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.IncrementalArcLength .

Created in NX6.0.0

License requirements: None.

unsafe bool NXOpen.Features.PointSetBuilder.Associative

getset

Returns or sets the associative setting.

true indicates a feature will be created, false indicates just points will be created

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.ChordalTolerance

get

Returns the chordal tolerance used in creating points.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.ChordalTolerance .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.NXObjectList NXOpen.Features.PointSetBuilder.CurvePercentageList

get

Returns the curve percentage list.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.CurvePercentage .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Features.PointSetBuilder.CurvePointsType NXOpen.Features.PointSetBuilder.CurvePointsBy

getset

Returns or sets the curve points definition setting.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe double NXOpen.Features.PointSetBuilder.DistanceTolerance

getset

Returns or sets the distance tolerance.

Used in combining curves when needed.

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.EndPercentage

get

Returns the percentage of the curve at which to stop creating points.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Section NXOpen.Features.PointSetBuilder.EndPercentageSection

get

Returns a section containing an object (curve, edge, or point) that will be used to determine an intersection with the curves/edges selected for setting the EndPercentage Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Features.PointSetFacePercentageBuilderList NXOpen.Features.PointSetBuilder.FacePercentageList

get

Returns the face percentage list.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.FacePercentage .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Features.PointSetBuilder.FacePointsType NXOpen.Features.PointSetBuilder.FacePointsBy

getset

Returns or sets the face points definition setting.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe bool NXOpen.Features.PointSetBuilder.GroupPoints

getset

Returns or sets the group points setting.

true indicates a points will be grouped together. This setting is applicable only when associative is false.

Created in NX7.5.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Section NXOpen.Features.PointSetBuilder.IntersectionSection

get

Returns the intersection Section.

This is used only, when NXOpen.Features.PointSetBuilder.Types is NXOpen.Features.PointSetBuilder.Types.IntersectionPoints

Created in NX8.5.0

Deprecated in NX9.0.0. Please use NXOpen.Features.PointSetBuilder.IntersectionSelectedObjectsSecond instead.

License requirements: None.

unsafe NXOpen.SelectDisplayableObjectList NXOpen.Features.PointSetBuilder.IntersectionSelectedObjects

get

Returns the intersection selected objects.

This is used only, when NXOpen.Features.PointSetBuilder.Types is NXOpen.Features.PointSetBuilder.Types.IntersectionPoints . Only NXOpen.Section or NXOpen.ScCollector are allowed as intersection selected objects.

Created in NX8.5.0

License requirements: None.

unsafe NXOpen.SelectDisplayableObjectList NXOpen.Features.PointSetBuilder.IntersectionSelectedObjectsSecond

get

Returns the intersection selected objects second.

This is used only, when NXOpen.Features.PointSetBuilder.Types is NXOpen.Features.PointSetBuilder.Types.IntersectionPoints

Created in NX9.0.0

License requirements: None.

unsafe NXOpen.Section NXOpen.Features.PointSetBuilder.MultipleCurveOrEdgeCollector

get

Returns the collector that is used to hold multiple curves or edges.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.SpecifiedProjectionPoints , or NXOpen.Features.PointSetBuilder.CurvePointsType.IncrementalArcLength .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.ScCollector NXOpen.Features.PointSetBuilder.MultipleFaceCollector

get

Returns the collector that is used to hold faces.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.FacePercentage , or NXOpen.Features.PointSetBuilder.FacePointsType.BSurfacePoles .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.NumberOfPointsExpression

get

Returns the number of points that will be created along curve.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX7.5.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.NumberOfPointsInUDirectionExpression

get

Returns the number of points to be created in the u direction.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern .

Created in NX7.5.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.NumberOfPointsInVDirectionExpression

get

Returns the number of points to be created in the v direction.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern .

Created in NX7.5.0

License requirements: None.

unsafe NXOpen.Features.PointSetBuilder.PatternLimitsType NXOpen.Features.PointSetBuilder.PatternLimitsBy

getset

Returns or sets the pattern limits definition setting.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.PatternLimitsEndingUValue

get

Returns the ending u value of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.Percentages .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.PatternLimitsEndingVValue

get

Returns the ending v value of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.Percentages .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Point NXOpen.Features.PointSetBuilder.PatternLimitsEndPoint

getset

Returns or sets the ending diagonal point of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.DiagonalPoints .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.PatternLimitsStartingUValue

get

Returns the starting u value of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.Percentages .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.PatternLimitsStartingVValue

get

Returns the starting v value of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.Percentages .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Point NXOpen.Features.PointSetBuilder.PatternLimitsStartPoint

getset

Returns or sets the starting diagonal point of the pattern.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern , and when NXOpen.Features.PointSetBuilder.PatternLimitsBy is NXOpen.Features.PointSetBuilder.PatternLimitsType.DiagonalPoints .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.PointList NXOpen.Features.PointSetBuilder.ProjectionPointList

get

Returns the projection point list.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.SpecifiedProjectionPoints .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.Ratio

get

Returns the ratio of geometric progression.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Section NXOpen.Features.PointSetBuilder.SingleCurveOrEdgeCollector

get

Returns the collector that is used to hold a single curve or edge definition.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression , NXOpen.Features.PointSetBuilder.CurvePointsType.ChordalTolerance , or NXOpen.Features.PointSetBuilder.CurvePointsType.IncrementalArcLength .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.SelectFace NXOpen.Features.PointSetBuilder.SingleFaceObject

get

Returns the select object that is used to hold the face.

Only used when type is NXOpen.Features.PointSetBuilder.Types.FacePoints , and when NXOpen.Features.PointSetBuilder.FacePointsBy is NXOpen.Features.PointSetBuilder.FacePointsType.Pattern .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.ScCollector NXOpen.Features.PointSetBuilder.SplineCollector

get

Returns the collector that is used to hold a spline.

Only used when type is NXOpen.Features.PointSetBuilder.Types.SplinePoints .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Features.PointSetBuilder.SplinePointsType NXOpen.Features.PointSetBuilder.SplinePointsBy

getset

Returns or sets the spline points definition setting.

Only used when type is NXOpen.Features.PointSetBuilder.Types.SplinePoints .

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Expression NXOpen.Features.PointSetBuilder.StartPercentage

get

Returns the percentage of the curve at which to start creating points.

Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Section NXOpen.Features.PointSetBuilder.StartPercentageSection

get

Returns a section containing an object (curve, edge, or point) that will be used to determine an intersection with the curves/edges selected for setting the StartPercentage Only used when type is NXOpen.Features.PointSetBuilder.Types.CurvePoints , and when NXOpen.Features.PointSetBuilder.CurvePointsBy is NXOpen.Features.PointSetBuilder.CurvePointsType.EqualArcLength , NXOpen.Features.PointSetBuilder.CurvePointsType.EqualParameters , or NXOpen.Features.PointSetBuilder.CurvePointsType.GeometricProgression .

Created in NX6.0.0

License requirements: None.

unsafe NXOpen.Features.PointSetBuilder.Types NXOpen.Features.PointSetBuilder.Type

getset

Returns or sets the type setting.

Created in NX6.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

---

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

• Features_PointSetBuilder.cs