Represents a sketch More...

Inheritance diagram for NXOpen.Sketch:

Classes
struct	_ConstraintGeometry
	Used by the create geometric constraint methods to indicate what geometry the constraint should be applied to.

struct	_CopyObjectData
	This structure represents a map between the original object to be copied and the corresponding copied object.

struct	_DimensionGeometry
	Used in the dimension creation methods to indicate what geometry to create the dimension on.

struct	ConstraintGeometry
	Used by the create geometric constraint methods to indicate what geometry the constraint should be applied to. More...

struct	ConstraintGeometryHelp
	Used by several constraint creation methods that need a help point or parameter to indicate how to create the constraint. More...

struct	CopyObjectData
	This structure represents a map between the original object to be copied and the corresponding copied object. More...

struct	DimensionGeometry
	Used in the dimension creation methods to indicate what geometry to create the dimension on. More...

Public Types
enum	Status { Unknown, NotEvaluated, UnderConstrained, WellConstrained, OverConstrained, InconsistentlyConstrained }
	Represents the status of the sketch More...

enum	ViewReorient { False, True }
	Used to indicate whether to reorient the view when the sketch is activated More...

enum	UpdateLevel { SketchOnly, Model }
	Used to indicate how much the updating should occur More...

enum	CreateInferConstraintSetting { On, Off }
	Indicates if the infer constraints will be created or not More...

enum	ConstraintPointType { None, StartVertex, EndVertex, ArcCenter, SplineDefiningPoint, Anchor, SplinePole, MidVertex }
	Used in ConstraintGeometry to indicate what type of point, if any, the geometry is More...

enum	AssocType { None, StartPoint, EndPoint, ArcCenter, Tangency, CurvePoint, AnchorPoint, Midpoint }
	Used in NXOpen.Sketch.DimensionGeometry to indicate what type of geometry to use More...

enum	ConstraintGeometryHelpType { Point, Parameter }
	Used in ConstraintHelp to indicate what type of help it is More...

enum	ConstraintClass { NotConstraint, Any, Geometric, Dimension }
	Represents the class of the constraint. More...

enum	ConstraintType { NoCon, Fixed, Horizontal, Vertical, Parallel, Perpendicular, Collinear, EqualLength, EqualRadius, ConstantLength, ConstantAngle, Coincident, Concentric, Mirror, PointOnCurve, Midpoint, Tangent, RadiusDim, DiameterDim, HorizontalDim, VerticalDim, ParallelDim, PerpendicularDim, AngularDim, ReservedCon1, ReservedCon2, ReservedCon3, ReservedCon4, ReservedCon5, ReservedCon6, PointOnString, Slope, UniformScaled, NonUniformScaled, AssocTrim, AssocOffset, PerimeterDim, Offset, Normal, PointOnLoop, RecipeTrim, Pattern, MinorAngularDim, MajorAngularDim, LastConType }
	Represents the type of constraint More...

enum	DimensionOption { CreateAsDriving, CreateAsReference, CreateAsAutomatic }
	Used by NXOpen.Sketch.CreateDimension , NXOpen.Sketch.CreateRadialDimension NXOpen.Sketch.CreateDiameterDimension and NXOpen.Sketch.CreatePerimeterDimension to determine whether to create driving or reference dimension More...

enum	AutoDimensioningRule { Symmetric = 1, AdjacentAngle, Length, HorizontalVertical, ReferenceAxes }
	Type of Auto Dimensioning rules. More...

enum	AddEllipseOption { TreatAsEllipse, TreatAsConic }
	Used by NXOpen.Sketch.AddGeometry to determine whether to treat an ellipse as an ellipse or generic conic when adding the curve to a sketch. More...

enum	TrimInputOption { False, True }
	Indicates whether the input curves should be trimmed when doing a fillet More...

enum	DeleteThirdCurveOption { False, True }
	Indicates whether the 3rd curve should be deleted when doing a 3 curve fillet More...

enum	CreateDimensionOption { False, True }
	Used in fillet to indicate whether a radius dimension should be created by the fillet More...

enum	AlternateSolutionOption { False, True }
	Indicates whether the alternate solution should be used instead of the regular solution. More...

enum	PlaneOption { Inferred, ExistingPlane, NewPlane, NewCsys }
	Specifies the plane type used for a Sketch More...

enum	InferConstraintsOption { InferNoConstraints, InferCoincidentConstraints }
	Used when adding a point or curve to a sketch. More...

Public Types inherited from NXOpen.DisplayableObject
enum	ObjectWidth { Normal, Thick, Thin, One = 5, Two, Three, Four, Five, Six, Seven, Eight, Nine }
	specifies object width for objects such as lines and text More...

enum	ObjectFont { Solid = 1, Dashed, Phantom, Centerline, Dotted, LongDashed, DottedDashed }
	specifies the object font for objects such as lines More...

Public Types inherited from NXOpen.NXObject
enum	AttributeType { Invalid, Null, Boolean, Integer, Real, String, Time, Reference, Any = 100 }
	Specifies attribute type. More...

enum	DateAndTimeFormat { Numeric, Textual }
	Specifies the format of the date and time attribute. More...

Public Member Functions
unsafe NXOpen.ErrorList	DeleteObjects (NXOpen.NXObject[] objects)
	Deletes objects from the sketch More...

unsafe void	Reattach (NXOpen.ISurface attachmentPlane, NXOpen.IReferenceAxis referenceAxis, NXOpen.Vector3d referenceDirection, NXOpen.AxisOrientation referenceAxisOrientation, NXOpen.Sense referenceAxisSense, NXOpen.PlaneNormalOrientation normalOrientation, NXOpen.Point3d localCoordinateSystemOrigin)
	Reattaches a sketch. More...

unsafe void	Activate (NXOpen.Sketch.ViewReorient orientView)
	Activates the sketch More...

unsafe void	Deactivate (NXOpen.Sketch.ViewReorient orientView, NXOpen.Sketch.UpdateLevel updateLevel)
	Deactivates the sketch More...

unsafe void	SetReferenceDirection (NXOpen.IReferenceAxis referenceAxis, NXOpen.Vector3d referenceDirection, NXOpen.AxisOrientation referenceAxisOrientation, NXOpen.Sense referenceAxisSense)
	Sets the reference direction of the sketch. More...

unsafe void	FlipReferenceDirection ()
	Flips the reference direction of the sketch More...

unsafe void	FlipNormal ()
	Flips the outward normal vector of the sketch More...

unsafe NXOpen.Vector3d	GetReferenceDirection (out NXOpen.IReferenceAxis referenceAxis, out NXOpen.AxisOrientation referenceAxisOrientation, out NXOpen.Sense referenceAxisSense)
	Gets the reference direction of the sketch More...

unsafe void	RunAutoDimension ()
	Run auto dimensioning. More...

unsafe NXOpen.SketchGeometricConstraint	CreateCoincidentConstraint (NXOpen.Sketch.ConstraintGeometry geom1, NXOpen.Sketch.ConstraintGeometry geom2)
	Creates a coincident constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateFixedConstraint (NXOpen.Sketch.ConstraintGeometry geom)
	Creates a fixed constraint More...

unsafe NXOpen.SketchGeometricConstraint[]	CreateFullyFixedConstraints (NXOpen.Sketch.ConstraintGeometry geom)
	Creates enough fixed constraints on the curve and all of its vertices such that the geometry is fully fixed without any redundant fixed constraints. More...

unsafe NXOpen.SketchGeometricConstraint	CreateHorizontalConstraint (NXOpen.Sketch.ConstraintGeometry geom)
	Creates a horizontal constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateVerticalConstraint (NXOpen.Sketch.ConstraintGeometry geom)
	Creates a vertical constraint More...

unsafe NXOpen.SketchTangentConstraint	CreateTangentConstraint (NXOpen.Sketch.ConstraintGeometry geom1, NXOpen.Sketch.ConstraintGeometryHelp geom1Help, NXOpen.Sketch.ConstraintGeometry geom2, NXOpen.Sketch.ConstraintGeometryHelp geom2Help)
	Creates a tangent constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateConstantLengthConstraint (NXOpen.Sketch.ConstraintGeometry conGeom)
	Creates a constant length constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateConstantAngleConstraint (NXOpen.Sketch.ConstraintGeometry conGeom)
	Creates a constant angle constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateUniformScaledConstraint (NXOpen.Sketch.ConstraintGeometry conGeom)
	Creates a uniform scale constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateNonUniformScaledConstraint (NXOpen.Sketch.ConstraintGeometry conGeom)
	Creates a non-uniform scale constraint More...

unsafe NXOpen.SketchGeometricConstraint	CreateParallelConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a parallel constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreatePerpendicularConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a perpendicular constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateNormalConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometryHelp geom1Help, NXOpen.Sketch.ConstraintGeometry conGeom2, NXOpen.Sketch.ConstraintGeometryHelp geom2Help)
	Creates a normal constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateCollinearConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a collinear constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateEqualLengthConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates an equal length constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateEqualRadiusConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates an equal radius constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateConcentricConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a concentric constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateMidpointConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a midpoint constraint. More...

unsafe NXOpen.SketchGeometricConstraint	CreateSlopeConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2)
	Creates a slope constraint. More...

unsafe NXOpen.SketchHelpedGeometricConstraint	CreatePointOnCurveConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Sketch.ConstraintGeometry conGeom2, NXOpen.Sketch.ConstraintGeometryHelp help)
	Creates a point on curve constraint. More...

unsafe NXOpen.SketchHelpedGeometricConstraint	CreatePointOnStringConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Curve[] curvesInString, NXOpen.Sketch.ConstraintGeometryHelp helpData, int curveWhichHelpParamAppliesTo)
	Creates a point on string constraint. More...

unsafe NXOpen.SketchHelpedGeometricConstraint	CreatePointOnStringConstraint (NXOpen.Sketch.ConstraintGeometry conGeom1, NXOpen.Curve curveInString, NXOpen.Sketch.ConstraintGeometryHelp helpData)
	Creates a point on string constraint. More...

unsafe NXOpen.SketchDimensionalConstraint	CreateDimension (NXOpen.Sketch.ConstraintType dimType, NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Sketch.DimensionGeometry dimObject2, NXOpen.Point3d dimOrigin, NXOpen.Expression expression)
	Creates a dimension between two geometric objects. More...

unsafe NXOpen.SketchDimensionalConstraint	CreateDimension (NXOpen.Sketch.ConstraintType dimType, NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Sketch.DimensionGeometry dimObject2, NXOpen.Point3d dimOrigin, NXOpen.Expression expression, NXOpen.Sketch.DimensionOption refDim)
	Creates a dimension between two geometric objects. More...

unsafe NXOpen.SketchDimensionalConstraint	CreateRadialDimension (NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Point3d dimOrigin, NXOpen.Expression expression)
	Creates a radial dimension constraint More...

unsafe NXOpen.SketchDimensionalConstraint	CreateRadialDimension (NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Point3d dimOrigin, NXOpen.Expression expression, NXOpen.Sketch.DimensionOption refDim)
	Creates a radial dimension constraint. More...

unsafe NXOpen.SketchDimensionalConstraint	CreateDiameterDimension (NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Point3d dimOrigin, NXOpen.Expression expression)
	Creates a diameter dimension constraint More...

unsafe NXOpen.SketchDimensionalConstraint	CreateDiameterDimension (NXOpen.Sketch.DimensionGeometry dimObject1, NXOpen.Point3d dimOrigin, NXOpen.Expression expression, NXOpen.Sketch.DimensionOption refDim)
	Creates a diameter dimension constraint. More...

unsafe NXOpen.SketchDimensionalConstraint	CreatePerimeterDimension (NXOpen.Curve[] curves, NXOpen.Point3d dimOrigin, NXOpen.Expression expression)
	Creates a perimeter dimension constraint More...

unsafe void	LocalUpdate ()
	Update the sketch and not the sketch children. More...

unsafe void	Update ()
	Updates the sketch More...

unsafe void	Update (NXOpen.NXObject[] geoms)
	Updates the given set of geometries in the sketch More...

unsafe void	UpdateGeometryDisplay ()
	Updates the geometry display without updating the sketch More...

unsafe void	UpdateGeometryDisplay (NXOpen.SmartObject[] geoms)
	Updates the geometry display of given set of geoms without updating the sketch More...

unsafe void	UpdateDimensionDisplay ()
	Updates the dimension display without updating the sketch More...

unsafe void	UpdateDimensionDisplay (NXOpen.SmartObject[] geoms)
	Updates the dimension display of given set of geoms without updating the sketch More...

unsafe void	UpdateDimensionDisplay (NXOpen.NXObject[] dims)
	Updates the dimension display of given set of dims without updating the sketch More...

unsafe void	UpdateConstraintDisplay ()
	Updates the constraint display without updating the sketch More...

unsafe void	UpdateConstraintDisplay (NXOpen.SmartObject[] geoms)
	Updates the constraint display of given set of geoms without updating the sketch More...

unsafe void	AddGeometry (NXOpen.DisplayableObject crv, NXOpen.Sketch.InferConstraintsOption inferCoincidentConstraints)
	Adds a curve or point to the sketch More...

unsafe void	AddGeometry (NXOpen.DisplayableObject crv)
	Adds a curve or point to the sketch. More...

unsafe void	AddGeometry (NXOpen.Curve crv, NXOpen.Sketch.InferConstraintsOption inferCoincidentConstraints, NXOpen.Sketch.AddEllipseOption ellipseOption)
	Adds a curve or point to a sketch. More...

unsafe void	AddGeometry (NXOpen.Sketch.InferConstraintsOption inferCoincidentConstraints, NXOpen.Sketch.AddEllipseOption ellipseOption, NXOpen.SmartObject[] curvesOrPoints)
	Adds an array of curves or points to a sketch. More...

unsafe NXOpen.Sketch.Status	GetStatus (out int dofNeeded)
	Gets the status of the sketch and the number of degrees of freedom that remain in the sketch. More...

unsafe NXOpen.SketchConstraint[]	GetAllConstraintsOfType (NXOpen.Sketch.ConstraintClass conClass, NXOpen.Sketch.ConstraintType conType)
	Gets all constraints in the sketch of a particular type More...

unsafe NXOpen.SketchConstraint[]	GetConstraintsForGeometry (NXOpen.SmartObject geometry, NXOpen.Sketch.ConstraintClass conClass)
	Gets all the constraints associated with a particular geometric item More...

unsafe NXOpen.Expression[]	GetAllExpressions ()
	Returns all the expressions in the sketch More...

unsafe NXOpen.NXObject[]	GetAllGeometry ()
	Returns all the curves and points in the sketch More...

unsafe NXOpen.Arc[]	Fillet (NXOpen.Curve curve1, NXOpen.Curve curve2, NXOpen.Point3d helpPoint1, NXOpen.Point3d helpPoint2, double radius, NXOpen.Sketch.TrimInputOption doTrim, NXOpen.Sketch.CreateDimensionOption createRadiusDim, NXOpen.Sketch.AlternateSolutionOption alternateSolution, out NXOpen.SketchConstraint[] constraints)
	Fillets curves and creates appropriate constraints. More...

unsafe NXOpen.Arc[]	Fillet (NXOpen.Curve curve1, NXOpen.Curve curve2, NXOpen.Point3d helpPoint1, NXOpen.Point3d helpPoint2, NXOpen.Point3d pointOnArc, double radius, NXOpen.Sketch.TrimInputOption doTrim, NXOpen.Sketch.CreateDimensionOption createRadiusDim, NXOpen.Sketch.AlternateSolutionOption alternateSolution, out NXOpen.SketchConstraint[] constraints)
	Fillets curves and creates appropriate constraints. More...

unsafe NXOpen.Arc[]	Fillet (NXOpen.Curve curve1, NXOpen.Curve curve2, NXOpen.Curve curve3, NXOpen.Point3d helpPoint1, NXOpen.Point3d helpPoint2, NXOpen.Point3d helpPoint3, double radius, NXOpen.Sketch.TrimInputOption doTrim, NXOpen.Sketch.DeleteThirdCurveOption doDelete, NXOpen.Sketch.CreateDimensionOption createRadiusDim, NXOpen.Sketch.AlternateSolutionOption alternateSolution, out NXOpen.SketchConstraint[] constraints)
	Fillets curves and creates appropriate constraints. More...

unsafe NXOpen.Arc[]	Fillet (NXOpen.Curve curve1, NXOpen.Curve curve2, NXOpen.Curve curve3, NXOpen.Point3d helpPoint1, NXOpen.Point3d helpPoint2, NXOpen.Point3d helpPoint3, NXOpen.Point3d pointOnArc, double radius, NXOpen.Sketch.TrimInputOption doTrim, NXOpen.Sketch.DeleteThirdCurveOption doDelete, NXOpen.Sketch.CreateDimensionOption createRadiusDim, NXOpen.Sketch.AlternateSolutionOption alternateSolution, out NXOpen.SketchConstraint[] constraints)
	Fillets curves and creates appropriate constraints. More...

unsafe void	DeleteConstraintsOnGeometries (NXOpen.NXObject[] objects)
	Deletes all geometric constraints associated with the object and all of its vertices. More...

unsafe void	DeleteConstraintsOnGeometries (NXOpen.Sketch.ConstraintGeometry[] objects)
	Deletes all geometric constraints associated with the object and all of its vertices. More...

unsafe void	DeleteConstraintsOnGeometries (NXOpen.Sketch.ConstraintClass conClass, NXOpen.Sketch.ConstraintGeometry[] objects)
	Deletes constraints associated with the input sketch geometry and vertices according to the constraint class, e. More...

unsafe NXOpen.NXObject[]	CopyObjects (NXOpen.NXObject[] inputObjects)
	Creates copies of input objects and constraints between these objects. More...

unsafe void	CopyObjectsWithDimensionOutput (NXOpen.NXObject[] inputObjects, out NXOpen.NXObject[] outputObjects, out NXOpen.NXObject[] outputDims)
	Creates copies of input objects and constraints between these objects. More...

unsafe void	ShowDimensions (NXOpen.DisplayableObject[] inputObjects)
	Unblanks dimensions in the active sketch associated with the input sketch geometry More...

unsafe void	HideDimensions (NXOpen.DisplayableObject[] inputObjects)
	Blanks dimensions in the active sketch associated with the input sketch geometry. More...

unsafe void	ShowDimensions ()
	Unblanks all the dimensions of input sketch More...

unsafe void	ShowDimensions (NXOpen.Sketch.ConstraintGeometry[] objects)
	Unblanks dimensions in the active sketch associated with the input sketch geometry. More...

unsafe void	HideDimensions ()
	Blanks all the dimensions of input sketch More...

unsafe void	HideDimensions (NXOpen.Sketch.ConstraintGeometry[] objects)
	Blanks dimensions in the active sketch associated with the input sketch geometry. More...

unsafe NXOpen.SketchConstraint[]	AutoConstrain (double linearTolerance, double angularTolerance, bool allowRemoteConstraints, NXOpen.SmartObject[] geometries, NXOpen.Sketch.ConstraintType[] autoconstraintTypes)
	Creates Automatic Constraints on input set of geometries. More...

unsafe void	MakeDatumsInternal ()
	Makes the sketch placement face and directional reference internal to the sketch if they are both datums referenced only by the sketch. More...

unsafe void	MakeDatumsExternal ()
	Makes the internal sketch placement face and directional reference datums external. More...

unsafe void	MakeDatumsExternal2 ()
	Makes the internal sketch placement face and directional reference datums external. More...

unsafe NXOpen.Sketch.CopyObjectData[]	CopyObjectsWithTracking (NXOpen.DisplayableObject[] inputObjects)
	Creates copies of input objects and constraints between these objects. More...

unsafe void	EditSplinePoles (NXOpen.Spline spline, double[] poles)
	Changes the locations of the control poles of a spline. More...

unsafe void	EditSplineDefiningPoints (NXOpen.Spline spline, double[] points)
	Changes the locations of the defining points of a spline. More...

unsafe void	ConvertToNx10Spline (NXOpen.Spline spline)
	Convert the legacy splines to new NX10 splines. More...

unsafe void	RemoveRedundantVertices (NXOpen.NXObject[] geoms)
	Remove redundant vertices of the given sketch geometry More...

unsafe void	ManageConstraintsAfterEdit (NXOpen.NXObject[] sketchGeoms, bool preserveComplexConstraints)
	Deletes or adjusts constraints of the input geometry that are incompatible after geometry edit. More...

unsafe void	BreakAssociativity (NXOpen.NXObject[] sketchGeoms)
	Breaks associativity of recipe geometry (projected or intersection curves and points) in the sketch, making the curves regular sketch geometry. More...

unsafe void	Scale (double scaleFactor)
	Scale the sketch entities by the given scale factor. More...

Public Member Functions inherited from NXOpen.DisplayableObject
unsafe void	Blank ()
	Blanks the object. More...

unsafe void	Unblank ()
	Unblanks the object. More...

unsafe void	Highlight ()
	Highlights the object. More...

unsafe void	Unhighlight ()
	Unhighlights the object. More...

unsafe void	SetNameLocation (NXOpen.Point3d location)
	Sets the location of the object's name. More...

unsafe void	RedisplayObject ()
	Redisplays the object in all views. More...

unsafe void	RemoveViewDependency ()
	Remove dependency on all views from an object. More...

Public Member Functions inherited from NXOpen.NXObject
unsafe void	SetUserAttribute (NXOpen.NXObject.AttributeInformation info, NXOpen.Update.Option option)
	Creates or modifies an attribute with the option to update or not. More...

unsafe void	SetUserAttribute (string title, int index, int value, NXOpen.Update.Option option)
	Creates or modifies an integer attribute with the option to update or not. More...

unsafe void	SetUserAttribute (string title, int index, double value, NXOpen.Update.Option option)
	Creates or modifies a real attribute with the option to update or not. More...

unsafe void	SetUserAttribute (string title, int index, string value, NXOpen.Update.Option option)
	Creates or modifies a string attribute with the option to update or not. More...

unsafe void	SetUserAttribute (string title, int index, NXOpen.Update.Option option)
	Creates or modifies a null attribute with the option to update or not. More...

unsafe void	SetTimeUserAttribute (string title, int index, string value, NXOpen.Update.Option option)
	Creates or modifies a time attribute with the option to update or not. More...

unsafe void	SetTimeUserAttribute (string title, int index, NXOpen.NXObject.ComputationalTime value, NXOpen.Update.Option option)
	Creates or modifies a time attribute with the option to update or not. More...

unsafe void	SetBooleanUserAttribute (string title, int index, bool value, NXOpen.Update.Option option)
	Creates or modifies a boolean attribute with the option to update or not. More...

unsafe NXOpen.AttributeIterator	CreateAttributeIterator ()
	Create an attribute iterator More...

unsafe bool	HasUserAttribute (NXOpen.AttributeIterator iterator)
	Determines if an attribute exists on the object, that satisfies the given iterator More...

unsafe bool	HasUserAttribute (string title, NXOpen.NXObject.AttributeType type, int index)
	Determines if an attribute with the given Title, Type and array Index is present on the object Unset attributes will not be detected by this function, as its purpose is to test for the actual presence of the attribute on the object. More...

unsafe int	GetUserAttributeCount (NXOpen.AttributeIterator iterator)
	Gets the count of set attributes on the object, if any, that satisfy the given iterator. More...

unsafe int	GetUserAttributeCount (NXOpen.AttributeIterator iterator, bool countArrayAsOneAttribute)
	Gets the count of set attributes on the object, if any, that satisfy the given iterator. More...

unsafe int	GetUserAttributeCount (NXOpen.NXObject.AttributeType type)
	Gets the count of set attributes on the object, if any, of the given type. More...

unsafe int	GetUserAttributeCount (NXOpen.NXObject.AttributeType type, bool includeUnset, bool countArrayAsOneAttribute)
	Gets the count of attributes on the object, if any, of the given type. More...

unsafe int	GetUserAttributeSize (string title, NXOpen.NXObject.AttributeType type)
	Gets the size of the first attribute encountered on the object, if any, with a given Title and Type. More...

unsafe bool	GetNextUserAttribute (NXOpen.AttributeIterator iterator, out NXOpen.NXObject.AttributeInformation info)
	Gets the next attribute encountered on the object, if any, that satisfies the given iterator. More...

unsafe NXOpen.NXObject.AttributeInformation	GetUserAttribute (string title, NXOpen.NXObject.AttributeType type, int index)
	Gets the first attribute encountered on the object, if any, with a given Title, Type and array Index. More...

unsafe bool	GetBooleanUserAttribute (string title, int index)
	Gets a boolean attribute by Title and array Index. More...

unsafe int	GetIntegerUserAttribute (string title, int index)
	Gets an integer attribute by Title and array Index. More...

unsafe double	GetRealUserAttribute (string title, int index)
	Gets a real attribute by Title and array Index. More...

unsafe string	GetStringUserAttribute (string title, int index)
	Gets a string attribute by Title and array Index. More...

unsafe string	GetTimeUserAttribute (string title, int index)
	Gets a time attribute by Title and array Index. More...

unsafe NXOpen.NXObject.ComputationalTime	GetComputationalTimeUserAttribute (string title, int index)
	Gets a time attribute by Title and array Index. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetUserAttributes (NXOpen.AttributeIterator iterator)
	Gets all the attributes that have been set on the given object, if any, that satisfy the given iterator. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetUserAttributes ()
	Gets all the attributes that have been set on the given object. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetUserAttributes (bool includeUnset)
	Gets all the attributes of the given object. More...

unsafe string	GetUserAttributeAsString (string title, NXOpen.NXObject.AttributeType type, int index)
	Gets the first attribute encountered on the object, if any, with a given title, type and array index. More...

unsafe void	DeleteUserAttributes (NXOpen.AttributeIterator iterator, NXOpen.Update.Option option)
	Deletes the attributes on the object, if any, that satisfy the given iterator More...

unsafe void	DeleteUserAttribute (NXOpen.NXObject.AttributeType type, string title, bool deleteEntireArray, NXOpen.Update.Option option)
	Deletes the first attribute encountered with the given Type, Title. More...

unsafe void	DeleteUserAttributes (NXOpen.NXObject.AttributeType type, NXOpen.Update.Option option)
	Deletes the attributes encountered with the given Type with option to update or not. More...

unsafe void	SetUserAttributeLock (string title, NXOpen.NXObject.AttributeType type, bool @lock)
	Lock or unlock the given attribute. More...

unsafe bool	GetUserAttributeLock (string title, NXOpen.NXObject.AttributeType type)
	Determine the lock of the given attribute. More...

unsafe NXOpen.NXObject[]	GetUserAttributeSourceObjects ()
	Returns an array of objects from which this object presents attributes. More...

unsafe void	SetPdmReferenceAttribute (string attributeTitle, string attributeValue)
	Sets the value of PDM Reference attribute on the object. More...

unsafe string	GetPdmReferenceAttributeValue (string attributeTitle)
	Gets the value of PDM Reference attribute for given object. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetUserAttribute (string title, bool includeUnset, bool addStringValues, NXOpen.NXObject.AttributeType type)
	Gets the first attribute (or attribute array) encountered on the object, if any, with a given Title and Type. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetUserAttributes (bool includeUnset, bool addStringValues)
	Gets all the attributes of the given object. More...

unsafe void	DeleteAllAttributesByType (NXOpen.NXObject.AttributeType type)
	Deletes all attributes of a specific type. More...

unsafe void	DeleteAllAttributesByType (NXOpen.NXObject.AttributeType type, NXOpen.Update.Option option)
	Deletes all attributes of a specific type with the option to update or not. More...

unsafe void	SetAttribute (string title, int value)
	Creates or modifies an integer attribute. More...

unsafe void	SetAttribute (string title, int value, NXOpen.Update.Option option)
	Creates or modifies an integer attribute with the option to update or not. More...

unsafe void	SetAttribute (string title, double value)
	Creates or modifies a real attribute. More...

unsafe void	SetAttribute (string title, double value, NXOpen.Update.Option option)
	Creates or modifies a real attribute with the option to update or not. More...

unsafe void	SetAttribute (string title, string value)
	Creates or modifies a string attribute. More...

unsafe void	SetAttribute (string title, string value, NXOpen.Update.Option option)
	Creates or modifies a string attribute with the option to update or not. More...

unsafe void	SetAttribute (string title)
	Creates or modifies a null attribute which is an attribute with a title and no value. More...

unsafe void	SetAttribute (string title, NXOpen.Update.Option option)
	Creates or modifies a null attribute with the option to update or not. More...

unsafe void	SetTimeAttribute (string title, string value)
	Creates or modifies a time attribute. More...

unsafe void	SetTimeAttribute (string title, string value, NXOpen.Update.Option option)
	Creates or modifies a time attribute with the option to update or not. More...

unsafe int	GetIntegerAttribute (string title)
	Gets an integer attribute by title. More...

unsafe double	GetRealAttribute (string title)
	Gets a real attribute by title. More...

unsafe string	GetStringAttribute (string title)
	Gets a string attribute value by title. More...

unsafe string	GetTimeAttribute (NXOpen.NXObject.DateAndTimeFormat format, string title)
	Gets a time attribute by title. More...

unsafe string	GetReferenceAttribute (string title)
	Gets the reference string (not the calculated value) of a string attribute that uses a reference string. More...

unsafe void	DeleteAttributeByTypeAndTitle (NXOpen.NXObject.AttributeType type, string title)
	Deletes an attribute by type and title. More...

unsafe void	DeleteAttributeByTypeAndTitle (NXOpen.NXObject.AttributeType type, string title, NXOpen.Update.Option option)
	Deletes an attribute by type and title with the option to update or not. More...

unsafe void	SetReferenceAttribute (string title, string value)
	Creates or modifies a string attribute which uses a reference string. More...

unsafe void	SetReferenceAttribute (string title, string value, NXOpen.Update.Option option)
	Creates or modifies a string attribute which uses a reference string, with the option to update or not. More...

unsafe NXOpen.NXObject.AttributeInformation[]	GetAttributeTitlesByType (NXOpen.NXObject.AttributeType type)
	Gets all the attribute titles of a specific type. More...

unsafe string[]	GetUserAttributesAsStrings ()
	Gets all the attributes that have been set on the given object. More...

unsafe NXOpen.INXObject	FindObject (string journalIdentifier)
	Finds the NXOpen.NXObject with the given identifier as recorded in a journal. More...

unsafe void	Print ()
	Prints a representation of this object to the system log file. More...

unsafe void	SetName (string name)
	Sets the custom name of the object. More...

Properties
NXOpen.Preferences.SketchPreferences	Preferences `[get]`
	Contains preferences for the sketch More...

unsafe NXOpen.ISurface	AttachPlane `[get]`
	Returns the plane that the sketch is attached to More...

unsafe NXOpen.Sketch.CreateInferConstraintSetting	CreateInferConstraintsSetting `[get, set]`
	Returns or sets the toggle that controls the creation of infer constraints in sketch More...

unsafe bool	DOFDisplay `[get, set]`
	Returns or sets a flag indicating whether the degree of freedom arrows are currently being displayed More...

unsafe NXOpen.Features.Feature	Feature `[get]`
	Returns the feature associated with this sketch More...

unsafe bool	IsActive `[get]`
	Returns true if the sketch is active More...

unsafe bool	IsDraftingSketch `[get]`
	Returns true if drafting sketch More...

unsafe bool	IsInternal `[get]`
	Returns true if the sketch is internal. More...

unsafe NXOpen.NXMatrix	Orientation `[get]`
	Returns the orientation matrix of the local coordinate system of the sketch More...

unsafe NXOpen.Point3d	Origin `[get]`
	Returns the location of the origin of the local coordinate system for the sketch More...

unsafe NXOpen.Sketch.UpdateLevel	UpdateScope `[get, set]`
	Returns or sets the current update scope. More...

unsafe NXOpen.View	View `[get]`
	Returns the view corresponding to sketch More...

Properties inherited from NXOpen.DisplayableObject
unsafe int	Color `[get, set]`
	Returns or sets the color of the object. More...

unsafe bool	IsBlanked `[get]`
	Returns the blank status of this object. More...

unsafe int	Layer `[get, set]`
	Returns or sets the layer that the object is in. More...

unsafe NXOpen.DisplayableObject.ObjectFont	LineFont `[get, set]`
	Returns or sets the line font of the object. More...

unsafe NXOpen.DisplayableObject.ObjectWidth	LineWidth `[get, set]`
	Returns or sets the line width of the object. More...

unsafe NXOpen.Point3d	NameLocation `[get]`
	Returns the location of the object's name. More...

Properties inherited from NXOpen.NXObject
unsafe bool	IsOccurrence `[get]`
	Returns whether this object is an occurrence or not. More...

unsafe string	JournalIdentifier `[get]`
	Returns the identifier that would be recorded in a journal for this object. More...

unsafe string	Name `[get]`
	Returns the custom name of the object. More...

unsafe NXOpen.Assemblies.Component	OwningComponent `[get]`
	Returns the owning component, if this object is an occurrence. More...

unsafe NXOpen.BasePart	OwningPart `[get]`
	Returns the owning part of this object More...

unsafe NXOpen.INXObject	Prototype `[get]`
	Returns the prototype of this object if it is an occurrence. More...

Properties inherited from NXOpen.INXObject
bool	IsOccurrence `[get]`
	Returns whether this object is an occurrence or not. More...

string	JournalIdentifier `[get]`
	Returns the identifier that would be recorded in a journal for this object. More...

string	Name `[get]`
	Returns the custom name of the object. More...

NXOpen.Assemblies.Component	OwningComponent `[get]`
	Returns the owning component, if this object is an occurrence. More...

NXOpen.BasePart	OwningPart `[get]`
	Returns the owning part of this object More...

NXOpen.INXObject	Prototype `[get]`
	Returns the prototype of this object if it is an occurrence. More...

Detailed Description

Represents a sketch

Use the NXOpen.SketchCollection class to create a sketch.

Created in NX3.0.0

Member Enumeration Documentation

enum NXOpen.Sketch.AddEllipseOption

Used by NXOpen.Sketch.AddGeometry to determine whether to treat an ellipse as an ellipse or generic conic when adding the curve to a sketch.

Treating an ellipse as a conic means that the ellipse will be given an anchor point. This affects, among other things, how the ellipse behaves when it is dragged.

In order for an ellipse to be treated as a conic, its end angle minus its start angle must be less than 180 degrees.

Enumerator
TreatAsEllipse
TreatAsConic

enum NXOpen.Sketch.AlternateSolutionOption

Indicates whether the alternate solution should be used instead of the regular solution.

The alternate solution for an arc is the portion of the full circle that is left out of the regular solution. For example, if the regular solution is an arc that goes from 0 to 45 degrees, the alternate solution will be an arc with the same center and origin but that goes from 45 degrees to 360.

Enumerator
False	Use the regular solution
True	Use the alternate solution

enum NXOpen.Sketch.AssocType

Used in NXOpen.Sketch.DimensionGeometry to indicate what type of geometry to use

Enumerator
None	Use the entire geometric item, as opposed to a point
StartPoint	Start point. E.g. the start point of a line
EndPoint	End point. E.g. the start point of a line
ArcCenter	Center of an arc, circle, or ellipse
Tangency	Create the dimension tangent to the geometric item
CurvePoint	A point on a spline
AnchorPoint	The anchor of a conic
Midpoint	The midpoint of a curve

enum NXOpen.Sketch.AutoDimensioningRule

Type of Auto Dimensioning rules.

It should match the rule types defined in Auto Dimensioning engine. Auto Dimensioning rules affect how the dimensions are created by the Auto Dimensioner. The rules will be put in a list, the first the rule with the highest priority and the last rule with the lowest priority. The user can change the order of the rules in the list to persue the flavor of the dimensions he wants. NXOpen.Sketch.AutoDimensioningRule.Symmetric : create symmetric dimensions if the curves are symmetric NXOpen.Sketch.AutoDimensioningRule.AdjacentAngle : create angles between adjacent lines NXOpen.Sketch.AutoDimensioningRule.Length : create length dimension for lines NXOpen.Sketch.AutoDimensioningRule.HorizontalVertical : create horizontal and vertical dimensions NXOpen.Sketch.AutoDimensioningRule.ReferenceAxes : create dimensions between curves and reference axes

Enumerator
Symmetric	Create Symmetric Dimensions
AdjacentAngle	Create Adjacent Angles
Length	Create Length Dimension
HorizontalVertical	Create Horizontal and Vertical Dimensions
ReferenceAxes	Create Dimensions to Reference Axes

enum NXOpen.Sketch.ConstraintClass

Represents the class of the constraint.

There are two classes of constraints: geometric and dimension

Enumerator
NotConstraint
Any	Used in query methods that filter by constraint class to select both types of constraints
Geometric	A non-dimension constraint
Dimension	A dimensional constraint

enum NXOpen.Sketch.ConstraintGeometryHelpType

Used in ConstraintHelp to indicate what type of help it is

Enumerator
Point
Parameter

enum NXOpen.Sketch.ConstraintPointType

Used in ConstraintGeometry to indicate what type of point, if any, the geometry is

Enumerator
None	The geometry is not a point
StartVertex	Start vertex (e.g. the start point of a line)
EndVertex	End vertex (e.g. the end point of a line)
ArcCenter	Center of a circle, arc, or ellipse
SplineDefiningPoint	A defining point of a spline.
Anchor	The anchor point of a conic
SplinePole	The control pole of a spline
MidVertex	The mid vertex of a line or an arc

enum NXOpen.Sketch.ConstraintType

Represents the type of constraint

Enumerator
NoCon	Used in query methods that filter by constraint type to select any type of constraint
Fixed
Horizontal
Vertical
Parallel
Perpendicular
Collinear
EqualLength
EqualRadius
ConstantLength
ConstantAngle
Coincident
Concentric
Mirror
PointOnCurve
Midpoint
Tangent
RadiusDim
DiameterDim
HorizontalDim
VerticalDim
ParallelDim
PerpendicularDim
AngularDim	system will decide if it is major or minor
ReservedCon1	Do not use
ReservedCon2	Do not use
ReservedCon3	Do not use
ReservedCon4	Do not use
ReservedCon5	Do not use
ReservedCon6	Do not use
PointOnString
Slope
UniformScaled
NonUniformScaled
AssocTrim	Limited support
AssocOffset	Limited support
PerimeterDim
Offset
Normal
PointOnLoop
RecipeTrim
Pattern
MinorAngularDim
MajorAngularDim
LastConType	The last constraint type indicator; NOT to be used.

enum NXOpen.Sketch.CreateDimensionOption

Used in fillet to indicate whether a radius dimension should be created by the fillet

Enumerator
False	Do not create a radius dimension
True	Create a radius dimension

enum NXOpen.Sketch.CreateInferConstraintSetting

Indicates if the infer constraints will be created or not

Enumerator
On	Create infer constraints
Off	Dont create infer constraints

enum NXOpen.Sketch.DeleteThirdCurveOption

Indicates whether the 3rd curve should be deleted when doing a 3 curve fillet

Enumerator
False	Do not delete the 3rd curve
True	Delete the 3rd curve

enum NXOpen.Sketch.DimensionOption

Used by NXOpen.Sketch.CreateDimension , NXOpen.Sketch.CreateRadialDimension NXOpen.Sketch.CreateDiameterDimension and NXOpen.Sketch.CreatePerimeterDimension to determine whether to create driving or reference dimension

Enumerator
CreateAsDriving	Create dimension as driving
CreateAsReference	Create dimension as reference
CreateAsAutomatic	Create dimension as automatic

enum NXOpen.Sketch.InferConstraintsOption

Used when adding a point or curve to a sketch.

Specifies whether to infer coincident constraints between the geometry that already exists in the sketch and the geometry being added to the sketch. If you choose to infer constraints, coincident constraints will be created if an end point of the geometry being added is at the same location (within system tolerance) as another end point in the sketch.

Enumerator
InferNoConstraints	Do not infer constraints
InferCoincidentConstraints	Infer constraints

enum NXOpen.Sketch.PlaneOption

Specifies the plane type used for a Sketch

Enumerator
Inferred	Use inferred plane
ExistingPlane	Use existing plane
NewPlane	Use new plane
NewCsys	Use new CSYS

enum NXOpen.Sketch.Status

Represents the status of the sketch

Enumerator
Unknown
NotEvaluated
UnderConstrained	More constraints are needed to fully constrain the sketch
WellConstrained	The sketch is fully constrained
OverConstrained	The sketch has more constraints than is needed
InconsistentlyConstrained	The sketch has conflicting constraints

enum NXOpen.Sketch.TrimInputOption

Indicates whether the input curves should be trimmed when doing a fillet

Enumerator
False	Do not trim the input curves
True	Trim the input curves

enum NXOpen.Sketch.UpdateLevel

Used to indicate how much the updating should occur

Enumerator
SketchOnly	Only update the sketch
Model	Update the full model and the sketch

enum NXOpen.Sketch.ViewReorient

Used to indicate whether to reorient the view when the sketch is activated

Enumerator
False	Do not reorient view to sketch
True	Reorient view to sketch

Member Function Documentation

unsafe void NXOpen.Sketch.Activate ( NXOpen.Sketch.ViewReorient orientView )

Activates the sketch

Created in NX3.0.0

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

Parameters

orientView Indicates whether to orient the view to the sketch during activation

unsafe void NXOpen.Sketch.AddGeometry	(	NXOpen.DisplayableObject	crv,
		NXOpen.Sketch.InferConstraintsOption	inferCoincidentConstraints
	)

Adds a curve or point to the sketch

Created in NX3.0.0

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

Parameters

crv	Must be a curve or point
inferCoincidentConstraints	Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created

unsafe void NXOpen.Sketch.AddGeometry ( NXOpen.DisplayableObject crv )

Adds a curve or point to the sketch.

Infers coincident constraints with other geometry in the sketch

Created in NX3.0.0

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

Parameters

crv	Must be a curve or point

unsafe void NXOpen.Sketch.AddGeometry	(	NXOpen.Curve	crv,
		NXOpen.Sketch.InferConstraintsOption	inferCoincidentConstraints,
		NXOpen.Sketch.AddEllipseOption	ellipseOption
	)

Adds a curve or point to a sketch.

Created in NX3.0.0

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

Parameters

crv	Must be a curve or point
inferCoincidentConstraints	Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created
ellipseOption	If you are adding an ellipse to the sketch, this parameter indicates whether the ellipse should be treated as an ellipse or general conic. If you are not adding an ellipse, the option is ignored. See the documentation for NXOpen.Sketch.AddEllipseOption for more details. The default value is NXOpen.Sketch.AddEllipseOption.TreatAsEllipse . In order to treat an ellipse as a conic, its end angle minus its start angle must be less than 180 degrees.

unsafe void NXOpen.Sketch.AddGeometry	(	NXOpen.Sketch.InferConstraintsOption	inferCoincidentConstraints,
		NXOpen.Sketch.AddEllipseOption	ellipseOption,
		NXOpen.SmartObject[]	curvesOrPoints
	)

Adds an array of curves or points to a sketch.

Created in NX6.0.1

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

Parameters

inferCoincidentConstraints	Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created
ellipseOption	If you are adding an ellipse to the sketch, this parameter indicates whether the ellipse should be treated as an ellipse or general conic. If you are not adding an ellipse, the option is ignored. See the documentation for NXOpen.Sketch.AddEllipseOption for more details. The default value is NXOpen.Sketch.AddEllipseOption.TreatAsEllipse . In order to treat an ellipse as a conic, its end angle minus its start angle must be less than 180 degrees.
curvesOrPoints	Must be a curve or point

unsafe NXOpen.SketchConstraint [] NXOpen.Sketch.AutoConstrain	(	double	linearTolerance,
		double	angularTolerance,
		bool	allowRemoteConstraints,
		NXOpen.SmartObject[]	geometries,
		NXOpen.Sketch.ConstraintType[]	autoconstraintTypes
	)

Creates Automatic Constraints on input set of geometries.

Created in NX4.0.0

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

Parameters

linearTolerance	Capture Distance
angularTolerance	Capture Angle
allowRemoteConstraints	Allow remote constraints
geometries	Array of geometries
autoconstraintTypes	Constraint type array

Returns: Array of deduced constraints

unsafe void NXOpen.Sketch.BreakAssociativity ( NXOpen.NXObject[] sketchGeoms )

Breaks associativity of recipe geometry (projected or intersection curves and points) in the sketch, making the curves regular sketch geometry.

Any non-recipe geometry is ignored. Call this before sketch update.

Created in NX11.0.0

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

Parameters

sketchGeoms Recipe geometry in the active sketch

unsafe void NXOpen.Sketch.ConvertToNx10Spline ( NXOpen.Spline spline )

Convert the legacy splines to new NX10 splines.

The input spline will be upgraded to NX10 spline. No new splines will be created to replace the input spline.

Created in NX10.0.0

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

Parameters

spline

unsafe NXOpen.NXObject [] NXOpen.Sketch.CopyObjects ( NXOpen.NXObject[] inputObjects )

Creates copies of input objects and constraints between these objects.

Created in NX4.0.0

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

Parameters

inputObjects Objects to be copied

Returns: Copies of objects

unsafe void NXOpen.Sketch.CopyObjectsWithDimensionOutput	(	NXOpen.NXObject[]	inputObjects,
		out NXOpen.NXObject[]	outputObjects,
		out NXOpen.NXObject[]	outputDims
	)

Creates copies of input objects and constraints between these objects.

This function is same as NXOpen.Sketch.CopyObjects except that it returns an array of newly created dimensions

Created in NX6.0.0

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

Parameters

inputObjects	Objects to be copied
outputObjects	Copies of objects
outputDims	Copies of dims

unsafe NXOpen.Sketch.CopyObjectData [] NXOpen.Sketch.CopyObjectsWithTracking ( NXOpen.DisplayableObject[] inputObjects )

Creates copies of input objects and constraints between these objects.

Sketch dimensions are copied only if explicitly included in the input_objects array.

Created in NX7.5.0

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

Parameters

inputObjects Objects to be copied

Returns: Map between the original input object and the corresponding copied object

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateCoincidentConstraint	(	NXOpen.Sketch.ConstraintGeometry	geom1,
		NXOpen.Sketch.ConstraintGeometry	geom2
	)

Creates a coincident constraint

Created in NX3.0.0

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

Parameters

geom1	Must be a vertex
geom2	Must be a vertex

Returns: The coincident constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateCollinearConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a collinear constraint.

One of the input constraint geometries must be a line.

Created in NX3.0.0

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

Parameters

conGeom1	Must be a line, linear edge, datum axis, or datum plane
conGeom2	Must be a line, linear edge, datum axis, or datum plane

Returns: The collinear constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateConcentricConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a concentric constraint.

One of the input constraint geometries must be a curve.

Created in NX3.0.0

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

Parameters

conGeom1	Must be an arc or ellipse or edge shaped as an arc or ellipse
conGeom2	Must be an arc or ellipse or edge shaped as an arc or ellipse

Returns: The concentric constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateConstantAngleConstraint ( NXOpen.Sketch.ConstraintGeometry conGeom )

Creates a constant angle constraint

Created in NX3.0.0

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

Parameters

conGeom Must be a line

Returns: The constant angle constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateConstantLengthConstraint ( NXOpen.Sketch.ConstraintGeometry conGeom )

Creates a constant length constraint

Created in NX3.0.0

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

Parameters

conGeom Must be a line

Returns: The constant length constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateDiameterDimension	(	NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression
	)

Creates a diameter dimension constraint

Created in NX3.0.0

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)

Returns: The diametral dimension constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateDiameterDimension	(	NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression,
		NXOpen.Sketch.DimensionOption	refDim
	)

Creates a diameter dimension constraint.

Accepts a flag to create the dim as driving or reference

Created in NX4.0.0

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)
refDim	option for creating driving or reference dimension

Returns: The diametral dimension constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateDimension	(	NXOpen.Sketch.ConstraintType	dimType,
		NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Sketch.DimensionGeometry	dimObject2,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression
	)

Creates a dimension between two geometric objects.

Do not use for radial, diameter, or perimeter dimensions. To create a radial or diameter constraint, use NXOpen.Sketch.CreateRadialDimension or NXOpen.Sketch.CreateDiameterDimension . To create a perimeter dimension, use NXOpen.Sketch.CreatePerimeterDimension

Created in NX3.0.0

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

Parameters

dimType	Must be one of the dimension types and should not be a radial, diametral, or perimeter dimension
dimObject1	First input geometry
dimObject2	Second input geometry
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)

Returns: The dimensional constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateDimension	(	NXOpen.Sketch.ConstraintType	dimType,
		NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Sketch.DimensionGeometry	dimObject2,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression,
		NXOpen.Sketch.DimensionOption	refDim
	)

Creates a dimension between two geometric objects.

Do not use for radial, diameter, or perimeter dimensions. To create a radial or diameter constraint, use NXOpen.Sketch.CreateRadialDimension or NXOpen.Sketch.CreateDiameterDimension . To create a perimeter dimension, use NXOpen.Sketch.CreatePerimeterDimension . This function takes in an argument to create the dimension as driving or reference.

Created in NX4.0.0

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

Parameters

dimType	Must be one of the dimension types and should not be a radial, diametral, or perimeter dimension
dimObject1	First input geometry
dimObject2	Second input geometry
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)
refDim	option for creating driving or reference dimension

Returns: The dimensional constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateEqualLengthConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates an equal length constraint.

One of the input constraint geometries must be a line.

Created in NX3.0.0

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

Parameters

conGeom1	Must be a line or linear edge
conGeom2	Must be a line or linear edge

Returns: The equal length constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateEqualRadiusConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates an equal radius constraint.

One of the input constraint geometries must be a curve.

Created in NX3.0.0

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

Parameters

conGeom1	Must be an arc or edge shaped as an arc
conGeom2	Must be an arc or edge shaped as an arc

Returns: The equal radius constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateFixedConstraint ( NXOpen.Sketch.ConstraintGeometry geom )

Creates a fixed constraint

Created in NX3.0.0

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

Parameters

geom	Can be any curve, point, or vertex in the sketch

Returns: The fixed constraint

unsafe NXOpen.SketchGeometricConstraint [] NXOpen.Sketch.CreateFullyFixedConstraints ( NXOpen.Sketch.ConstraintGeometry geom )

Creates enough fixed constraints on the curve and all of its vertices such that the geometry is fully fixed without any redundant fixed constraints.

Created in NX5.0.0

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

Parameters

geom	Can be any curve, point, or vertex in the sketch

Returns: The fixed constraints

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateHorizontalConstraint ( NXOpen.Sketch.ConstraintGeometry geom )

Creates a horizontal constraint

Created in NX3.0.0

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

Parameters

geom	Must be a line

Returns: The horizontal constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateMidpointConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a midpoint constraint.

One of the input constraint geometries must be a vertex and the other must be a curve or edge.

Created in NX3.0.0

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

Parameters

conGeom1
conGeom2

Returns: The midpoint constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateNonUniformScaledConstraint ( NXOpen.Sketch.ConstraintGeometry conGeom )

Creates a non-uniform scale constraint

Created in NX3.0.0

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

Parameters

conGeom Must be a spline

Returns: The non-uniform scale constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateNormalConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometryHelp	geom1Help,
		NXOpen.Sketch.ConstraintGeometry	conGeom2,
		NXOpen.Sketch.ConstraintGeometryHelp	geom2Help
	)

Creates a normal constraint.

A normal constraint can be created between any two curve/edge type except between two linear objects. For linear objects, create a perpendicular constraint

Created in NX3.0.0

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

Parameters

conGeom1	First input geometry for the constraint
geom1Help	Help data for first geom
conGeom2	Second input geometry for the constraint
geom2Help	Help data for second geom

Returns: The normal constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateParallelConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a parallel constraint.

A parallel constraint can only be created between one of the following pairs: (line, line or linear edge), (line, datum axis or datum plane), (line or linear edge, ellipse), (line, ellipse or elliptical edge), (ellipse, ellipse or elliptical edge).

Created in NX3.0.0

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

Parameters

conGeom1	First input geometry for the constraint
conGeom2	Second input geometry for the constraint

Returns: The parallel constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreatePerimeterDimension	(	NXOpen.Curve[]	curves,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression
	)

Creates a perimeter dimension constraint

Created in NX3.0.0

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

Parameters

curves	The curves that form the perimeter
dimOrigin	Not currently used
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)

Returns: The perimeter dimensional constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreatePerpendicularConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a perpendicular constraint.

A perpendicular constraint can only be created between one of the following pairs: (line, line or linear edge), (line, datum axis or datum plane), (line or linear edge, ellipse), (line, ellipse or elliptical edge), (ellipse, ellipse or elliptical edge).

Created in NX3.0.0

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

Parameters

conGeom1	First input geometry for the constraint
conGeom2	Second input geometry for the constraint

Returns: The perpendicular constraint

unsafe NXOpen.SketchHelpedGeometricConstraint NXOpen.Sketch.CreatePointOnCurveConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2,
		NXOpen.Sketch.ConstraintGeometryHelp	help
	)

Creates a point on curve constraint.

One of the input geometries must be a vertex and the other must be a curve, edge, datum axis, or datum plane.

Created in NX3.0.0

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

Parameters

conGeom1
conGeom2
help

Returns: The point on curve constraint

unsafe NXOpen.SketchHelpedGeometricConstraint NXOpen.Sketch.CreatePointOnStringConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Curve[]	curvesInString,
		NXOpen.Sketch.ConstraintGeometryHelp	helpData,
		int	curveWhichHelpParamAppliesTo
	)

Creates a point on string constraint.

Created in NX3.0.0

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

Parameters

conGeom1	Must be a vertex
curvesInString	Must all be part of the same string. (You can create a string of curves through the UI through the Edit -> Project command.)
helpData
curveWhichHelpParamAppliesTo	If helpData is a parameter, this parameter indicates which curve in the curvesInString that the help parameter applies to. Otherwise, this parameter is not used

Returns: The point on string constraint

unsafe NXOpen.SketchHelpedGeometricConstraint NXOpen.Sketch.CreatePointOnStringConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Curve	curveInString,
		NXOpen.Sketch.ConstraintGeometryHelp	helpData
	)

Creates a point on string constraint.

The string is specified using a single curve in the string. The constraint is created on the entire string that curveInString belongs to.

Created in NX3.0.0

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

Parameters

conGeom1	Must be a vertex
curveInString	A curve in the string that you want to create the constraint on. The constraint is created on the entire string that this curve belongs to. (You can create a string of curves through the UI through the Edit -> Project command.)
helpData

Returns: The point on string constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateRadialDimension	(	NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression
	)

Creates a radial dimension constraint

Created in NX3.0.0

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)

Returns: The radial dimension constraint

unsafe NXOpen.SketchDimensionalConstraint NXOpen.Sketch.CreateRadialDimension	(	NXOpen.Sketch.DimensionGeometry	dimObject1,
		NXOpen.Point3d	dimOrigin,
		NXOpen.Expression	expression,
		NXOpen.Sketch.DimensionOption	refDim
	)

Creates a radial dimension constraint.

Accepts a flag to create the dimension as driving or reference

Created in NX4.0.0

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be a null reference (Nothing in Visual Basic)
refDim	option for creating driving or reference dimension

Returns: The radial dimension constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateSlopeConstraint	(	NXOpen.Sketch.ConstraintGeometry	conGeom1,
		NXOpen.Sketch.ConstraintGeometry	conGeom2
	)

Creates a slope constraint.

One of the input constraint geometries must a spline defining point. The other must be datum axis, datum plane, or a curve or edge shaped as a line, arc, ellipse, conic, or spline.

Created in NX3.0.0

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

Parameters

conGeom1
conGeom2

Returns: The slope constraint

unsafe NXOpen.SketchTangentConstraint NXOpen.Sketch.CreateTangentConstraint	(	NXOpen.Sketch.ConstraintGeometry	geom1,
		NXOpen.Sketch.ConstraintGeometryHelp	geom1Help,
		NXOpen.Sketch.ConstraintGeometry	geom2,
		NXOpen.Sketch.ConstraintGeometryHelp	geom2Help
	)

Creates a tangent constraint.

Note: the input constraint geometries cannot both be linear.

Created in NX3.0.0

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

Parameters

geom1	A curve, edge, or datum axis
geom1Help
geom2	A curve, edge, or datum axis
geom2Help

Returns: The tangent constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateUniformScaledConstraint ( NXOpen.Sketch.ConstraintGeometry conGeom )

Creates a uniform scale constraint

Created in NX3.0.0

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

Parameters

conGeom Must be a spline

Returns: The uniform scale constraint

unsafe NXOpen.SketchGeometricConstraint NXOpen.Sketch.CreateVerticalConstraint ( NXOpen.Sketch.ConstraintGeometry geom )

Creates a vertical constraint

Created in NX3.0.0

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

Parameters

geom	Must be a line

Returns: The vertical constraint

unsafe void NXOpen.Sketch.Deactivate	(	NXOpen.Sketch.ViewReorient	orientView,
		NXOpen.Sketch.UpdateLevel	updateLevel
	)

Deactivates the sketch

Created in NX3.0.0

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

Parameters

orientView	Indicates whether to orient the view to the model during deactivation
updateLevel	Indicates whether just the sketch should be updated or the entire model

unsafe void NXOpen.Sketch.DeleteConstraintsOnGeometries ( NXOpen.NXObject[] objects )

Deletes all geometric constraints associated with the object and all of its vertices.

Converts all the driving dimensions associated with the object and its vertices to reference dimensions.

Created in NX4.0.0

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

Parameters

objects Objects whose constraints needs to be deleted

unsafe void NXOpen.Sketch.DeleteConstraintsOnGeometries ( NXOpen.Sketch.ConstraintGeometry[] objects )

Deletes all geometric constraints associated with the object and all of its vertices.

Converts all the driving dimensions associated with the object and its vertices to reference dimensions. The user can pass in a vertex to do the same on just the supplied vertex.

Created in NX8.5.0

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

Parameters

objects Objects whose constraints needs to be deleted

unsafe void NXOpen.Sketch.DeleteConstraintsOnGeometries	(	NXOpen.Sketch.ConstraintClass	conClass,
		NXOpen.Sketch.ConstraintGeometry[]	objects
	)

Deletes constraints associated with the input sketch geometry and vertices according to the constraint class, e.

g.,

NXOpen.Sketch.ConstraintClass.Any will remove all geometric constraints and convert driving dimensions to reference dimensions.
NXOpen.Sketch.ConstraintClass.Geometric will remove all geometric constraints.
NXOpen.Sketch.ConstraintClass.Dimension will remove all dimensions and not convert them to reference.
NXOpen.Sketch.ConstraintClass.NotConstraint will not remove any geometric constraints and dimensions.

Created in NX11.0.0

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

Parameters

conClass	Use NXOpen.Sketch.ConstraintClass.Any if you do not want to filter by constraint class
objects	Objects whose constraints needs to be deleted

unsafe NXOpen.ErrorList NXOpen.Sketch.DeleteObjects ( NXOpen.NXObject[] objects )

Deletes objects from the sketch

Created in NX3.0.0

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

Parameters

objects Objects to be deleted

Returns: List of errors encountered during the delete

unsafe void NXOpen.Sketch.EditSplineDefiningPoints	(	NXOpen.Spline	spline,
		double[]	points
	)

Changes the locations of the defining points of a spline.

The length of point array should be enough to cover existing defining points. You cannot add/remove points nor change knot sequence via this call.

Created in NX10.0.0

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

Parameters

spline
points	point locations. Size is three times the number of points.

unsafe void NXOpen.Sketch.EditSplinePoles	(	NXOpen.Spline	spline,
		double[]	poles
	)

Changes the locations of the control poles of a spline.

The length of poles array should be enough to cover existing poles. You cannot add/remove poles nor change knot sequence via this call. The order of data in poles array is x, y, z, weight. You can edit any or all of these four values via this function.

Created in NX10.0.0

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

Parameters

spline
poles	pole locations. Size is four times the number of poles.

unsafe NXOpen.Arc [] NXOpen.Sketch.Fillet	(	NXOpen.Curve	curve1,
		NXOpen.Curve	curve2,
		NXOpen.Point3d	helpPoint1,
		NXOpen.Point3d	helpPoint2,
		double	radius,
		NXOpen.Sketch.TrimInputOption	doTrim,
		NXOpen.Sketch.CreateDimensionOption	createRadiusDim,
		NXOpen.Sketch.AlternateSolutionOption	alternateSolution,
		out NXOpen.SketchConstraint[]	constraints
	)

Fillets curves and creates appropriate constraints.

If the input curves have mirror constraints, the fillet is also performed on the mirror curves.

Created in NX3.0.0

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

Parameters

curve1	First curve for the fillet
curve2	Second curve for the fillet
helpPoint1	Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2	Should be a point on the second curve. Indicates where the fillet should be created
radius	Radius of the fillet
doTrim	Indicates whether the input curves should get trimmed by the fillet
createRadiusDim	Indicates whether a radius dimension should be created
alternateSolution	Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.

Returns: The fillet arcs that are created. If the input curves do not have any mirror constraints, the number of fillet arcs will always be one. If the input curves have mirror constraints, fillets will be created on the mirrored curves, and all the fillet arcs that were created are returned

Parameters

constraints The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.

unsafe NXOpen.Arc [] NXOpen.Sketch.Fillet	(	NXOpen.Curve	curve1,
		NXOpen.Curve	curve2,
		NXOpen.Point3d	helpPoint1,
		NXOpen.Point3d	helpPoint2,
		NXOpen.Point3d	pointOnArc,
		double	radius,
		NXOpen.Sketch.TrimInputOption	doTrim,
		NXOpen.Sketch.CreateDimensionOption	createRadiusDim,
		NXOpen.Sketch.AlternateSolutionOption	alternateSolution,
		out NXOpen.SketchConstraint[]	constraints
	)

Fillets curves and creates appropriate constraints.

If the input curves have mirror constraints, the fillet is also performed on the mirror curves.

Created in NX7.5.0

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

Parameters

curve1	First curve for the fillet
curve2	Second curve for the fillet
helpPoint1	Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2	Should be a point on the second curve. Indicates where the fillet should be created
pointOnArc	Point on fillet arc
radius	Radius of the fillet
doTrim	Indicates whether the input curves should get trimmed by the fillet
createRadiusDim	Indicates whether a radius dimension should be created
alternateSolution	Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.

Returns: The fillet arcs that are created. If the input curves do not have any mirror constraints, the number of fillet arcs will always be one. If the input curves have mirror constraints, fillets will be created on the mirrored curves, and all the fillet arcs that were created are returned

Parameters

constraints The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.

unsafe NXOpen.Arc [] NXOpen.Sketch.Fillet	(	NXOpen.Curve	curve1,
		NXOpen.Curve	curve2,
		NXOpen.Curve	curve3,
		NXOpen.Point3d	helpPoint1,
		NXOpen.Point3d	helpPoint2,
		NXOpen.Point3d	helpPoint3,
		double	radius,
		NXOpen.Sketch.TrimInputOption	doTrim,
		NXOpen.Sketch.DeleteThirdCurveOption	doDelete,
		NXOpen.Sketch.CreateDimensionOption	createRadiusDim,
		NXOpen.Sketch.AlternateSolutionOption	alternateSolution,
		out NXOpen.SketchConstraint[]	constraints
	)

Fillets curves and creates appropriate constraints.

If the input curves have mirror constraints, the fillet is also performed on the mirror curves.

Created in NX3.0.0

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

Parameters

curve1	First curve for the fillet
curve2	Second curve for the fillet
curve3	Third curve for the fillet
helpPoint1	Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2	Should be a point on the second curve. Indicates where the fillet should be created
helpPoint3	Should be a point on the third curve. Indicates where the fillet should be created
radius	Radius of the fillet
doTrim	Indicates whether the input curves should get trimmed by the fillet
doDelete	Indicates whether the third curve should be deleted
createRadiusDim	Indicates whether a radius dimension should be created
alternateSolution	Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.

Returns: The fillet arcs that are created. If the input curves do not have any mirror constraints, the number of fillet arcs will always be one. If the input curves have mirror constraints, fillets will be created on the mirrored curves, and all the fillet arcs that were created are returned

Parameters

constraints The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.

unsafe NXOpen.Arc [] NXOpen.Sketch.Fillet	(	NXOpen.Curve	curve1,
		NXOpen.Curve	curve2,
		NXOpen.Curve	curve3,
		NXOpen.Point3d	helpPoint1,
		NXOpen.Point3d	helpPoint2,
		NXOpen.Point3d	helpPoint3,
		NXOpen.Point3d	pointOnArc,
		double	radius,
		NXOpen.Sketch.TrimInputOption	doTrim,
		NXOpen.Sketch.DeleteThirdCurveOption	doDelete,
		NXOpen.Sketch.CreateDimensionOption	createRadiusDim,
		NXOpen.Sketch.AlternateSolutionOption	alternateSolution,
		out NXOpen.SketchConstraint[]	constraints
	)

Fillets curves and creates appropriate constraints.

If the input curves have mirror constraints, the fillet is also performed on the mirror curves.

Created in NX7.5.0

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

Parameters

curve1	First curve for the fillet
curve2	Second curve for the fillet
curve3	Third curve for the fillet
helpPoint1	Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2	Should be a point on the second curve. Indicates where the fillet should be created
helpPoint3	Should be a point on the third curve. Indicates where the fillet should be created
pointOnArc	Point on fillet arc
radius	Radius of the fillet
doTrim	Indicates whether the input curves should get trimmed by the fillet
doDelete	Indicates whether the third curve should be deleted
createRadiusDim	Indicates whether a radius dimension should be created
alternateSolution	Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.

Returns: The fillet arcs that are created. If the input curves do not have any mirror constraints, the number of fillet arcs will always be one. If the input curves have mirror constraints, fillets will be created on the mirrored curves, and all the fillet arcs that were created are returned

Parameters

constraints The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.

unsafe void NXOpen.Sketch.FlipNormal ( )

Flips the outward normal vector of the sketch

Created in NX3.0.0

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

unsafe void NXOpen.Sketch.FlipReferenceDirection ( )

Flips the reference direction of the sketch

Created in NX3.0.0

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

unsafe NXOpen.SketchConstraint [] NXOpen.Sketch.GetAllConstraintsOfType	(	NXOpen.Sketch.ConstraintClass	conClass,
		NXOpen.Sketch.ConstraintType	conType
	)

Gets all constraints in the sketch of a particular type

Created in NX3.0.0

License requirements: None.

Parameters

conClass	Optional filter. Use NXOpen.Sketch.ConstraintClass.Any if you do not want to filter by constraint class
conType	Optional filter. Use NXOpen.Sketch.ConstraintType.NoCon if you do not want to filter by constraint type

Returns: All the constraints in the sketch of the specified type

unsafe NXOpen.Expression [] NXOpen.Sketch.GetAllExpressions ( )

Returns all the expressions in the sketch

Created in NX3.0.0

License requirements: None.

Returns: All the expressions in the sketch

unsafe NXOpen.NXObject [] NXOpen.Sketch.GetAllGeometry ( )

Returns all the curves and points in the sketch

Created in NX3.0.0

License requirements: None.

Returns: All the curves and points in the sketch

unsafe NXOpen.SketchConstraint [] NXOpen.Sketch.GetConstraintsForGeometry	(	NXOpen.SmartObject	geometry,
		NXOpen.Sketch.ConstraintClass	conClass
	)

Gets all the constraints associated with a particular geometric item

Created in NX3.0.0

License requirements: None.

Parameters

geometry	Must be a curve or point
conClass	Optional filter. Use NXOpen.Sketch.ConstraintClass.Any if you do not want to filter by constraint class

Returns: All the constraints associated with the geometry that is input

unsafe NXOpen.Vector3d NXOpen.Sketch.GetReferenceDirection	(	out NXOpen.IReferenceAxis	referenceAxis,
		out NXOpen.AxisOrientation	referenceAxisOrientation,
		out NXOpen.Sense	referenceAxisSense
	)

Gets the reference direction of the sketch

Created in NX3.0.0

License requirements: None.

Returns

Parameters

referenceAxis	An edge, datum axis, datum plane, or face that the sketch uses as a reference. May be a null reference (Nothing in Visual Basic).
referenceAxisOrientation	Indicates whether the reference axis is horizontal or vertical
referenceAxisSense	If reference axis is an edge or datum axis, this parameter indicates whether the reference axis is in the same direction as the edge or datum axis or in the opposite direction. If reference axis is not an edge or datum axis, this parameter is not used.

unsafe NXOpen.Sketch.Status NXOpen.Sketch.GetStatus ( out int dofNeeded )

Gets the status of the sketch and the number of degrees of freedom that remain in the sketch.

The status of the sketch indicates whether the sketch is fully constrained or under, over, or inconsistently constrained.

Created in NX3.0.0

License requirements: None.

Returns: The sketch's status, which indicates how well constrained the sketch is

Parameters

dofNeeded The number of degrees of freedom left in the sketch

unsafe void NXOpen.Sketch.HideDimensions ( NXOpen.DisplayableObject[] inputObjects )

Blanks dimensions in the active sketch associated with the input sketch geometry.

Created in NX4.0.0

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

Parameters

inputObjects Geometry and groups in active sketch

unsafe void NXOpen.Sketch.HideDimensions ( )

Blanks all the dimensions of input sketch

Created in NX6.0.1

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

unsafe void NXOpen.Sketch.HideDimensions ( NXOpen.Sketch.ConstraintGeometry[] objects )

Blanks dimensions in the active sketch associated with the input sketch geometry.

This function can accept vertices

Created in NX8.5.0

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

Parameters

objects Geometry and vertices in active sketch

unsafe void NXOpen.Sketch.LocalUpdate ( )

Update the sketch and not the sketch children.

If a different sketch is active the SKETCH_NOT_INITIALIZED error will return. The function works even if the sketch is not active.

Created in NX3.0.0

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

unsafe void NXOpen.Sketch.MakeDatumsExternal ( )

Makes the internal sketch placement face and directional reference datums external.

Created in NX5.0.0

Deprecated in NX11.0.0. Please use NXOpen.Sketch.MakeDatumsExternal2 instead.

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

unsafe void NXOpen.Sketch.MakeDatumsExternal2 ( )

Makes the internal sketch placement face and directional reference datums external.

It should be called only when the internal datum is not a datum CSYS or is not a PlaneAxisPoint type of datum CSYS.

Created in NX11.0.0

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

unsafe void NXOpen.Sketch.MakeDatumsInternal ( )

Makes the sketch placement face and directional reference internal to the sketch if they are both datums referenced only by the sketch.

Created in NX5.0.0

Deprecated in NX11.0.0. None.

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

unsafe void NXOpen.Sketch.ManageConstraintsAfterEdit	(	NXOpen.NXObject[]	sketchGeoms,
		bool	preserveComplexConstraints
	)

Deletes or adjusts constraints of the input geometry that are incompatible after geometry edit.

Call this before sketch update

Created in NX11.0.0

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

Parameters

sketchGeoms
preserveComplexConstraints	Complex constraints are Pattern, Mirror and Offset

unsafe void NXOpen.Sketch.Reattach	(	NXOpen.ISurface	attachmentPlane,
		NXOpen.IReferenceAxis	referenceAxis,
		NXOpen.Vector3d	referenceDirection,
		NXOpen.AxisOrientation	referenceAxisOrientation,
		NXOpen.Sense	referenceAxisSense,
		NXOpen.PlaneNormalOrientation	normalOrientation,
		NXOpen.Point3d	localCoordinateSystemOrigin
	)

Reattaches a sketch.

For documentation for the parameters for this method, see the documentation for NXOpen.SketchCollection.CreateSketch

Created in NX3.0.0

Deprecated in NX11.0.0. Use NXOpen.SketchInPlaceBuilder instead.

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

Parameters

attachmentPlane
referenceAxis
referenceDirection
referenceAxisOrientation
referenceAxisSense
normalOrientation
localCoordinateSystemOrigin	Origin of the sketch's local coordinate system

unsafe void NXOpen.Sketch.RemoveRedundantVertices ( NXOpen.NXObject[] geoms )

Remove redundant vertices of the given sketch geometry

Created in NX11.0.0

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

Parameters

geoms Array of geometries

unsafe void NXOpen.Sketch.RunAutoDimension ( )

Run auto dimensioning.

Created in NX7.5.0

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

unsafe void NXOpen.Sketch.Scale ( double scaleFactor )

Scale the sketch entities by the given scale factor.

The sketch cannot be scaled if there are recipe curves or external constraints/dimensions or constraints/dimensions that controls the size of one or more geometries in the sketch. The sketch can have at most one non-angular driving dimension and that dimension must have its expression value scaled by the scale factor.

Created in NX11.0.0

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

Parameters

scaleFactor the scaleFactor must be gerater than zero

unsafe void NXOpen.Sketch.SetReferenceDirection	(	NXOpen.IReferenceAxis	referenceAxis,
		NXOpen.Vector3d	referenceDirection,
		NXOpen.AxisOrientation	referenceAxisOrientation,
		NXOpen.Sense	referenceAxisSense
	)

Sets the reference direction of the sketch.

For documentation for the parameters for this method, see the documentation for NXOpen.SketchCollection.CreateSketch .

Created in NX3.0.0

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

Parameters

referenceAxis
referenceDirection
referenceAxisOrientation
referenceAxisSense

unsafe void NXOpen.Sketch.ShowDimensions ( NXOpen.DisplayableObject[] inputObjects )

Unblanks dimensions in the active sketch associated with the input sketch geometry

Created in NX4.0.0

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

Parameters

inputObjects Geometry and groups in active sketch

unsafe void NXOpen.Sketch.ShowDimensions ( )

Unblanks all the dimensions of input sketch

Created in NX6.0.1

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

unsafe void NXOpen.Sketch.ShowDimensions ( NXOpen.Sketch.ConstraintGeometry[] objects )

Unblanks dimensions in the active sketch associated with the input sketch geometry.

This function can accept vertices.

Created in NX8.5.0

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

Parameters

objects Geometry and vertices in active sketch

unsafe void NXOpen.Sketch.Update ( )

Updates the sketch

Created in NX3.0.0

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

unsafe void NXOpen.Sketch.Update ( NXOpen.NXObject[] geoms )

Updates the given set of geometries in the sketch

Created in NX4.0.0

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

Parameters

geoms Geoms that need to be updated

unsafe void NXOpen.Sketch.UpdateConstraintDisplay ( )

Updates the constraint display without updating the sketch

Created in NX3.0.0

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

unsafe void NXOpen.Sketch.UpdateConstraintDisplay ( NXOpen.SmartObject[] geoms )

Updates the constraint display of given set of geoms without updating the sketch

Created in NX4.0.0

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

Parameters

geoms Geoms for which cons must be re-displayed

unsafe void NXOpen.Sketch.UpdateDimensionDisplay ( )

Updates the dimension display without updating the sketch

Created in NX4.0.0

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

unsafe void NXOpen.Sketch.UpdateDimensionDisplay ( NXOpen.SmartObject[] geoms )

Updates the dimension display of given set of geoms without updating the sketch

Created in NX4.0.0

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

Parameters

geoms Geoms for which cons must be re-displayed

unsafe void NXOpen.Sketch.UpdateDimensionDisplay ( NXOpen.NXObject[] dims )

Updates the dimension display of given set of dims without updating the sketch

Created in NX4.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")

Parameters

dims	Dims for which cons must be re-displayed

unsafe void NXOpen.Sketch.UpdateGeometryDisplay ( )

Updates the geometry display without updating the sketch

Created in NX4.0.0

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

unsafe void NXOpen.Sketch.UpdateGeometryDisplay ( NXOpen.SmartObject[] geoms )

Updates the geometry display of given set of geoms without updating the sketch

Created in NX4.0.0

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

Parameters

geoms Geoms for which cons must be re-displayed

Property Documentation

unsafe NXOpen.ISurface NXOpen.Sketch.AttachPlane

get

Returns the plane that the sketch is attached to

Created in NX3.0.0

License requirements: None.

unsafe NXOpen.Sketch.CreateInferConstraintSetting NXOpen.Sketch.CreateInferConstraintsSetting

getset

Returns or sets the toggle that controls the creation of infer constraints in sketch

Created in NX4.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")

unsafe bool NXOpen.Sketch.DOFDisplay

getset

Returns or sets a flag indicating whether the degree of freedom arrows are currently being displayed

Created in NX3.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")

unsafe NXOpen.Features.Feature NXOpen.Sketch.Feature

get

Returns the feature associated with this sketch

Created in NX3.0.0

License requirements: None.

unsafe bool NXOpen.Sketch.IsActive

get

Returns true if the sketch is active

Created in NX3.0.0

License requirements: None.

unsafe bool NXOpen.Sketch.IsDraftingSketch

get

Returns true if drafting sketch

Created in NX6.0.0

License requirements: None.

unsafe bool NXOpen.Sketch.IsInternal

get

Returns true if the sketch is internal.

Created in NX6.0.0

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

unsafe NXOpen.NXMatrix NXOpen.Sketch.Orientation

get

Returns the orientation matrix of the local coordinate system of the sketch

Created in NX3.0.0

License requirements: None.

unsafe NXOpen.Point3d NXOpen.Sketch.Origin

get

Returns the location of the origin of the local coordinate system for the sketch

Created in NX3.0.0

License requirements: None.

NXOpen.Preferences.SketchPreferences NXOpen.Sketch.Preferences

get

Contains preferences for the sketch

Created in NX3.0.0

unsafe NXOpen.Sketch.UpdateLevel NXOpen.Sketch.UpdateScope

getset

Returns or sets the current update scope.

Used in Direct Sketch to control update

Created in NX8.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")

unsafe NXOpen.View NXOpen.Sketch.View

get

Returns the view corresponding to sketch

Created in NX6.0.0

License requirements: None.

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

dotnet_pool/Sketch.cs

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