Represents a sketch
Use the SketchCollection class to create 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. 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	AddEllipseOption { AddEllipseOptionTreatAsEllipse, AddEllipseOptionTreatAsConic }
	Used by AddGeometry to determine whether to treat an ellipse as an ellipse or generic conic when adding the curve to a sketch. More...

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

enum	AssocType { AssocTypeNone, AssocTypeStartPoint, AssocTypeEndPoint, AssocTypeArcCenter, AssocTypeTangency, AssocTypeCurvePoint, AssocTypeAnchorPoint, AssocTypeMidpoint }
	Used in Sketch::DimensionGeometry to indicate what type of geometry to use. More...

enum	AutoDimensioningRule { AutoDimensioningRuleSymmetric = 1, AutoDimensioningRuleAdjacentAngle, AutoDimensioningRuleLength, AutoDimensioningRuleHorizontalVertical, AutoDimensioningRuleReferenceAxes }
	Type of Auto Dimensioning rules. More...

enum	ConstraintClass { ConstraintClassNotConstraint, ConstraintClassAny, ConstraintClassGeometric, ConstraintClassDimension }
	Represents the class of the constraint. More...

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

enum	ConstraintPointType { ConstraintPointTypeNone, ConstraintPointTypeStartVertex, ConstraintPointTypeEndVertex, ConstraintPointTypeArcCenter, ConstraintPointTypeSplineDefiningPoint, ConstraintPointTypeAnchor }
	Used in ConstraintGeometry to indicate what type of point, if any, the geometry is. More...

enum	ConstraintType { ConstraintTypeNoCon, ConstraintTypeFixed, ConstraintTypeHorizontal, ConstraintTypeVertical, ConstraintTypeParallel, ConstraintTypePerpendicular, ConstraintTypeCollinear, ConstraintTypeEqualLength, ConstraintTypeEqualRadius, ConstraintTypeConstantLength, ConstraintTypeConstantAngle, ConstraintTypeCoincident, ConstraintTypeConcentric, ConstraintTypeMirror, ConstraintTypePointOnCurve, ConstraintTypeMidpoint, ConstraintTypeTangent, ConstraintTypeRadiusDim, ConstraintTypeDiameterDim, ConstraintTypeHorizontalDim, ConstraintTypeVerticalDim, ConstraintTypeParallelDim, ConstraintTypePerpendicularDim, ConstraintTypeAngularDim, ConstraintTypeReservedCon1, ConstraintTypeReservedCon2, ConstraintTypeReservedCon3, ConstraintTypeReservedCon4, ConstraintTypeReservedCon5, ConstraintTypeReservedCon6, ConstraintTypePointOnString, ConstraintTypeSlope, ConstraintTypeUniformScaled, ConstraintTypeNonUniformScaled, ConstraintTypeAssocTrim, ConstraintTypeAssocOffset, ConstraintTypePerimeterDim, ConstraintTypeOffset, ConstraintTypeNormal, ConstraintTypePointOnLoop, ConstraintTypeRecipeTrim, ConstraintTypePattern, ConstraintTypeMinorAngularDim, ConstraintTypeMajorAngularDim, ConstraintTypeLastConType }
	Represents the type of constraint. More...

enum	ConstraintVisibility { ConstraintVisibilityNone, ConstraintVisibilitySome, ConstraintVisibilityAll }
	Indicates the visibility of the constraints The APIs that use this enum are deprecated in NX85 The Sketch::ConstraintVisibilitySome option will behave the same as the Sketch::ConstraintVisibilityAll option. More...

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

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

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

enum	DimensionOption { DimensionOptionCreateAsDriving, DimensionOptionCreateAsReference, DimensionOptionCreateAsAutomatic }
	Used by CreateDimension , CreateRadialDimension CreateDiameterDimension and CreatePerimeterDimension to determine whether to create driving or reference dimension. More...

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

enum	PlaneOption { PlaneOptionInferred, PlaneOptionExistingPlane, PlaneOptionNewPlane, PlaneOptionNewCsys }
	Specifies the plane type used for a Sketch. More...

enum	Status { StatusUnknown, StatusNotEvaluated, StatusUnderConstrained, StatusWellConstrained, StatusOverConstrained, StatusInconsistentlyConstrained }
	Represents the status of the sketch. More...

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

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

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

Public Types inherited from NXOpen::DisplayableObject
enum	ObjectFont { ObjectFontSolid = 1, ObjectFontDashed, ObjectFontPhantom, ObjectFontCenterline, ObjectFontDotted, ObjectFontLongDashed, ObjectFontDottedDashed }
	specifies the object font for objects such as lines Created in NX3.0.0. More...

enum	ObjectWidth { ObjectWidthNormal, ObjectWidthThick, ObjectWidthThin, ObjectWidthOne = 5, ObjectWidthTwo, ObjectWidthThree, ObjectWidthFour, ObjectWidthFive, ObjectWidthSix, ObjectWidthSeven, ObjectWidthEight, ObjectWidthNine }
	specifies object width for objects such as lines and text Created in NX3.0.0. More...

Public Types inherited from NXOpen::NXObject
enum	AttributeType { AttributeTypeInvalid, AttributeTypeNull, AttributeTypeBoolean, AttributeTypeInteger, AttributeTypeReal, AttributeTypeString, AttributeTypeTime, AttributeTypeReference, AttributeTypeAny = 100 }
	Specifies attribute type. More...

enum	DateAndTimeFormat { DateAndTimeFormatNumeric, DateAndTimeFormatTextual }
	Specifies the format of the date and time attribute. More...

Public Member Functions
void	Activate (NXOpen::Sketch::ViewReorient orientView)
	Activates the sketch Created in NX3.0.0.

void	AddGeometry (NXOpen::DisplayableObject *crv, NXOpen::Sketch::InferConstraintsOption inferCoincidentConstraints)
	Adds a curve or point to the sketch Created in NX3.0.0.

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

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

void	AddGeometry (NXOpen::Sketch::InferConstraintsOption inferCoincidentConstraints, NXOpen::Sketch::AddEllipseOption ellipseOption, const std::vector< NXOpen::SmartObject * > &curvesOrPoints)
	Adds an array of curves or points to a sketch.

NXOpen::ISurface *	AttachPlane ()
	Returns the plane that the sketch is attached to Created in NX3.0.0.

std::vector < NXOpen::SketchConstraint * >	AutoConstrain (double linearTolerance, double angularTolerance, bool allowRemoteConstraints, const std::vector< NXOpen::SmartObject * > &geometries, const std::vector< NXOpen::Sketch::ConstraintType > &autoconstraintTypes)
	Creates Automatic Constraints on input set of geometries.

std::vector< NXOpen::NXObject * >	CopyObjects (const std::vector< NXOpen::NXObject * > &inputObjects)
	Creates copies of input objects and constraints between these objects.

void	CopyObjectsWithDimensionOutput (const std::vector< NXOpen::NXObject * > &inputObjects, std::vector< NXOpen::NXObject * > &outputObjects, std::vector< NXOpen::NXObject * > &outputDims)
	Creates copies of input objects and constraints between these objects.

std::vector < NXOpen::Sketch::CopyObjectData >	CopyObjectsWithTracking (const std::vector< NXOpen::DisplayableObject * > &inputObjects)
	Creates copies of input objects and constraints between these objects.

NXOpen::SketchGeometricConstraint *	CreateCoincidentConstraint (const NXOpen::Sketch::ConstraintGeometry &geom1, const NXOpen::Sketch::ConstraintGeometry &geom2)
	Creates a coincident constraint.

NXOpen::SketchGeometricConstraint *	CreateCollinearConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a collinear constraint.

NXOpen::SketchGeometricConstraint *	CreateConcentricConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a concentric constraint.

NXOpen::SketchGeometricConstraint *	CreateConstantAngleConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
	Creates a constant angle constraint.

NXOpen::SketchGeometricConstraint *	CreateConstantLengthConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
	Creates a constant length constraint.

NXOpen::SketchDimensionalConstraint *	CreateDiameterDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
	Creates a diameter dimension constraint.

NXOpen::SketchDimensionalConstraint *	CreateDiameterDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression, NXOpen::Sketch::DimensionOption refDim)
	Creates a diameter dimension constraint.

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

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

NXOpen::SketchGeometricConstraint *	CreateEqualLengthConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates an equal length constraint.

NXOpen::SketchGeometricConstraint *	CreateEqualRadiusConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates an equal radius constraint.

NXOpen::SketchGeometricConstraint *	CreateFixedConstraint (const NXOpen::Sketch::ConstraintGeometry &geom)
	Creates a fixed constraint.

std::vector < NXOpen::SketchGeometricConstraint * >	CreateFullyFixedConstraints (const 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.

NXOpen::SketchGeometricConstraint *	CreateHorizontalConstraint (const NXOpen::Sketch::ConstraintGeometry &geom)
	Creates a horizontal constraint.

NXOpen::Sketch::CreateInferConstraintSetting	CreateInferConstraintsSetting ()
	Returns the toggle that controls the creation of infer constraints in sketch Created in NX4.0.0.

NXOpen::SketchGeometricConstraint *	CreateMidpointConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a midpoint constraint.

NXOpen::SketchGeometricConstraint *	CreateNonUniformScaledConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
	Creates a non-uniform scale constraint.

NXOpen::SketchGeometricConstraint *	CreateNormalConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometryHelp &geom1Help, const NXOpen::Sketch::ConstraintGeometry &conGeom2, const NXOpen::Sketch::ConstraintGeometryHelp &geom2Help)
	Creates a normal constraint.

NXOpen::SketchGeometricConstraint *	CreateParallelConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a parallel constraint.

NXOpen::SketchDimensionalConstraint *	CreatePerimeterDimension (const std::vector< NXOpen::Curve * > &curves, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
	Creates a perimeter dimension constraint.

NXOpen::SketchGeometricConstraint *	CreatePerpendicularConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a perpendicular constraint.

NXOpen::SketchHelpedGeometricConstraint *	CreatePointOnCurveConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2, const NXOpen::Sketch::ConstraintGeometryHelp &help)
	Creates a point on curve constraint.

NXOpen::SketchHelpedGeometricConstraint *	CreatePointOnStringConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const std::vector< NXOpen::Curve * > &curvesInString, const NXOpen::Sketch::ConstraintGeometryHelp &helpData, int curveWhichHelpParamAppliesTo)
	Creates a point on string constraint.

NXOpen::SketchHelpedGeometricConstraint *	CreatePointOnStringConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, NXOpen::Curve *curveInString, const NXOpen::Sketch::ConstraintGeometryHelp &helpData)
	Creates a point on string constraint.

NXOpen::SketchDimensionalConstraint *	CreateRadialDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
	Creates a radial dimension constraint.

NXOpen::SketchDimensionalConstraint *	CreateRadialDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression, NXOpen::Sketch::DimensionOption refDim)
	Creates a radial dimension constraint.

NXOpen::SketchGeometricConstraint *	CreateSlopeConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
	Creates a slope constraint.

NXOpen::SketchTangentConstraint *	CreateTangentConstraint (const NXOpen::Sketch::ConstraintGeometry &geom1, const NXOpen::Sketch::ConstraintGeometryHelp &geom1Help, const NXOpen::Sketch::ConstraintGeometry &geom2, const NXOpen::Sketch::ConstraintGeometryHelp &geom2Help)
	Creates a tangent constraint.

NXOpen::SketchGeometricConstraint *	CreateUniformScaledConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
	Creates a uniform scale constraint.

NXOpen::SketchGeometricConstraint *	CreateVerticalConstraint (const NXOpen::Sketch::ConstraintGeometry &geom)
	Creates a vertical constraint.

void	Deactivate (NXOpen::Sketch::ViewReorient orientView, NXOpen::Sketch::UpdateLevel updateLevel)
	Deactivates the sketch Created in NX3.0.0.

void	DeleteConstraintsOnGeometries (const std::vector< NXOpen::NXObject * > &objects)
	Deletes all geometric constraints associated with the object and all of its vertices.

void	DeleteConstraintsOnGeometries (const std::vector< NXOpen::Sketch::ConstraintGeometry > &objects)
	Deletes all geometric constraints associated with the object and all of its vertices.

NXOpen::ErrorList *	DeleteObjects (const std::vector< NXOpen::NXObject * > &objects)
	Deletes objects from the sketch.

bool	DOFDisplay ()
	Returns a flag indicating whether the degree of freedom arrows are currently being displayed Created in NX3.0.0.

NXOpen::Features::Feature *	Feature ()
	Returns the feature associated with this sketch Created in NX3.0.0.

std::vector< NXOpen::Arc * >	Fillet (NXOpen::Curve curve1, NXOpen::Curve curve2, const NXOpen::Point3d &helpPoint1, const NXOpen::Point3d &helpPoint2, double radius, NXOpen::Sketch::TrimInputOption doTrim, NXOpen::Sketch::CreateDimensionOption createRadiusDim, NXOpen::Sketch::AlternateSolutionOption alternateSolution, std::vector< NXOpen::SketchConstraint * > &constraints)
	Fillets curves and creates appropriate constraints.

std::vector< NXOpen::Arc * >	Fillet (NXOpen::Curve curve1, NXOpen::Curve curve2, const NXOpen::Point3d &helpPoint1, const NXOpen::Point3d &helpPoint2, const NXOpen::Point3d &pointOnArc, double radius, NXOpen::Sketch::TrimInputOption doTrim, NXOpen::Sketch::CreateDimensionOption createRadiusDim, NXOpen::Sketch::AlternateSolutionOption alternateSolution, std::vector< NXOpen::SketchConstraint * > &constraints)
	Fillets curves and creates appropriate constraints.

std::vector< NXOpen::Arc * >	Fillet (NXOpen::Curve curve1, NXOpen::Curve curve2, NXOpen::Curve curve3, const NXOpen::Point3d &helpPoint1, const NXOpen::Point3d &helpPoint2, const NXOpen::Point3d &helpPoint3, double radius, NXOpen::Sketch::TrimInputOption doTrim, NXOpen::Sketch::DeleteThirdCurveOption doDelete, NXOpen::Sketch::CreateDimensionOption createRadiusDim, NXOpen::Sketch::AlternateSolutionOption alternateSolution, std::vector< NXOpen::SketchConstraint > &constraints)
	Fillets curves and creates appropriate constraints.

std::vector< NXOpen::Arc * >	Fillet (NXOpen::Curve curve1, NXOpen::Curve curve2, NXOpen::Curve curve3, const NXOpen::Point3d &helpPoint1, const NXOpen::Point3d &helpPoint2, const NXOpen::Point3d &helpPoint3, const NXOpen::Point3d &pointOnArc, double radius, NXOpen::Sketch::TrimInputOption doTrim, NXOpen::Sketch::DeleteThirdCurveOption doDelete, NXOpen::Sketch::CreateDimensionOption createRadiusDim, NXOpen::Sketch::AlternateSolutionOption alternateSolution, std::vector< NXOpen::SketchConstraint > &constraints)
	Fillets curves and creates appropriate constraints.

void	FlipNormal ()
	Flips the outward normal vector of the sketch Created in NX3.0.0.

void	FlipReferenceDirection ()
	Flips the reference direction of the sketch Created in NX3.0.0.

std::vector < NXOpen::SketchConstraint * >	GetAllConstraintsOfType (NXOpen::Sketch::ConstraintClass conClass, NXOpen::Sketch::ConstraintType conType)
	Gets all constraints in the sketch of a particular type.

std::vector< NXOpen::Expression * >	GetAllExpressions ()
	Returns all the expressions in the sketch.

std::vector< NXOpen::NXObject * >	GetAllGeometry ()
	Returns all the curves and points in the sketch.

std::vector < NXOpen::SketchConstraint * >	GetConstraintsForGeometry (NXOpen::SmartObject *geometry, NXOpen::Sketch::ConstraintClass conClass)
	Gets all the constraints associated with a particular geometric item.

NXOpen::Vector3d	GetReferenceDirection (NXOpen::IReferenceAxis *referenceAxis, NXOpen::AxisOrientation referenceAxisOrientation, NXOpen::Sense *referenceAxisSense)
	Gets the reference direction of the sketch.

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

void	HideDimensions (const std::vector< NXOpen::DisplayableObject * > &inputObjects)
	Blanks dimensions in the active sketch associated with the input sketch geometry.

void	HideDimensions ()
	Blanks all the dimensions of input sketch Created in NX6.0.1.

void	HideDimensions (const std::vector< NXOpen::Sketch::ConstraintGeometry > &objects)
	Blanks dimensions in the active sketch associated with the input sketch geometry.

bool	IsActive ()
	Returns true if the sketch is active Created in NX3.0.0.

bool	IsDraftingSketch ()
	Returns true if drafting sketch Created in NX6.0.0.

bool	IsInternal ()
	Returns true if the sketch is internal.

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

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

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

std::vector < NXOpen::SmartObject * >	MirrorObjects (NXOpen::DisplayableObject centerline, const std::vector< NXOpen::SmartObject > &objectsToMirror)
	Creates a reflection of the input geometry.

NXOpen::NXMatrix *	Orientation ()
	Returns the orientation matrix of the local coordinate system of the sketch Created in NX3.0.0.

NXOpen::Point3d	Origin ()
	Returns the location of the origin of the local coordinate system for the sketch Created in NX3.0.0.

NXOpen::Preferences::SketchPreferences *	Preferences ()
	Contains preferences for the sketch Created in NX3.0.0.

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

void	RunAutoDimension ()
	Run auto dimensioning.

void	SetCreateInferConstraintsSetting (NXOpen::Sketch::CreateInferConstraintSetting createInferCon)
	Sets the toggle that controls the creation of infer constraints in sketch Created in NX4.0.0.

void	SetDOFDisplay (bool displayDof)
	Sets a flag indicating whether the degree of freedom arrows are currently being displayed Created in NX3.0.0.

void	SetReferenceDirection (NXOpen::IReferenceAxis *referenceAxis, const NXOpen::Vector3d &referenceDirection, NXOpen::AxisOrientation referenceAxisOrientation, NXOpen::Sense referenceAxisSense)
	Sets the reference direction of the sketch.

void	SetUpdateScope (NXOpen::Sketch::UpdateLevel updateScope)
	Sets the current update scope.

void	SetVisibilityOfConstraints (NXOpen::Sketch::ConstraintVisibility visibility)
	Sets the visibility of the constraints in the sketch

void	ShowDimensions (const std::vector< NXOpen::DisplayableObject * > &inputObjects)
	Unblanks dimensions in the active sketch associated with the input sketch geometry Created in NX4.0.0.

void	ShowDimensions ()
	Unblanks all the dimensions of input sketch Created in NX6.0.1.

void	ShowDimensions (const std::vector< NXOpen::Sketch::ConstraintGeometry > &objects)
	Unblanks dimensions in the active sketch associated with the input sketch geometry.

void	Update ()
	Updates the sketch Created in NX3.0.0.

void	Update (const std::vector< NXOpen::NXObject * > &geoms)
	Updates the given set of geometries in the sketch Created in NX4.0.0.

void	UpdateConstraintDisplay ()
	Updates the constraint display without updating the sketch Created in NX3.0.0.

void	UpdateConstraintDisplay (const std::vector< NXOpen::SmartObject * > &geoms)
	Updates the constraint display of given set of geoms without updating the sketch Created in NX4.0.0.

void	UpdateDimensionDisplay ()
	Updates the dimension display without updating the sketch Created in NX4.0.0.

void	UpdateDimensionDisplay (const std::vector< NXOpen::SmartObject * > &geoms)
	Updates the dimension display of given set of geoms without updating the sketch Created in NX4.0.0.

void	UpdateDimensionDisplay (const std::vector< NXOpen::NXObject * > &dims)
	Updates the dimension display of given set of dims without updating the sketch Created in NX4.0.0.

void	UpdateGeometryDisplay ()
	Updates the geometry display without updating the sketch Created in NX4.0.0.

void	UpdateGeometryDisplay (const std::vector< NXOpen::SmartObject * > &geoms)
	Updates the geometry display of given set of geoms without updating the sketch Created in NX4.0.0.

NXOpen::Sketch::UpdateLevel	UpdateScope ()
	Returns the current update scope.

NXOpen::View *	View ()
	Returns the view corresponding to sketch Created in NX6.0.0.

NXOpen::Sketch::ConstraintVisibility	VisibilityOfConstraints ()
	Returns the visibility of the constraints in the sketch

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

int	Color ()
	Returns the color of the object.

void	Highlight ()
	Highlights the object.

bool	IsBlanked ()
	Returns the blank status of this object.

int	Layer ()
	Returns the layer that the object is in.

NXOpen::DisplayableObject::ObjectFont	LineFont ()
	Returns the line font of the object.

NXOpen::DisplayableObject::ObjectWidth	LineWidth ()
	Returns the line width of the object.

NXOpen::Point3d	NameLocation ()
	Returns the location of the object's name.

void	RedisplayObject ()
	Redisplays the object in all views.

void	SetColor (int color)
	Sets the color of the object.

void	SetLayer (int layer)
	Sets the layer that the object is in.

void	SetLineFont (NXOpen::DisplayableObject::ObjectFont font)
	Sets the line font of the object.

void	SetLineWidth (NXOpen::DisplayableObject::ObjectWidth width)
	Sets the line width of the object.

void	SetNameLocation (const NXOpen::Point3d &location)
	Sets the location of the object's name.

void	Unblank ()
	Unblanks the object.

void	Unhighlight ()
	Unhighlights the object.

Public Member Functions inherited from NXOpen::NXObject
void	DeleteAllAttributesByType (NXOpen::NXObject::AttributeType type)
	Deletes all attributes of a specific type.

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

void	DeleteAttributeByTypeAndTitle (NXOpen::NXObject::AttributeType type, const NXString &title)
	Deletes an attribute by type and title.

void	DeleteAttributeByTypeAndTitle (NXOpen::NXObject::AttributeType type, const char *title)
	Deletes an attribute by type and title.

void	DeleteAttributeByTypeAndTitle (NXOpen::NXObject::AttributeType type, const NXString &title, NXOpen::Update::Option option)
	Deletes an attribute by type and title with the option to update or not.

void	DeleteAttributeByTypeAndTitle (NXOpen::NXObject::AttributeType type, const char *title, NXOpen::Update::Option option)
	Deletes an attribute by type and title with the option to update or not.

void	DeleteUserAttribute (NXOpen::NXObject::AttributeType type, const NXString &title, bool deleteEntireArray, NXOpen::Update::Option option)
	Deletes the first attribute encountered with the given Type, Title and Index.

void	DeleteUserAttribute (NXOpen::NXObject::AttributeType type, const char *title, bool deleteEntireArray, NXOpen::Update::Option option)
	Deletes the first attribute encountered with the given Type, Title and Index.

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

virtual NXOpen::INXObject *	FindObject (const NXString &journalIdentifier)
	Finds the NXObject with the given identifier as recorded in a journal.

NXOpen::INXObject *	FindObject (const char *journalIdentifier)
	Finds the NXObject with the given identifier as recorded in a journal.

std::vector < NXOpen::NXObject::AttributeInformation >	GetAttributeTitlesByType (NXOpen::NXObject::AttributeType type)
	Gets all the attribute titles of a specific type.

bool	GetBooleanUserAttribute (const NXString &title, int index)
	Gets a boolean attribute by Title and array Index.

bool	GetBooleanUserAttribute (const char *title, int index)
	Gets a boolean attribute by Title and array Index.

NXOpen::NXObject::ComputationalTime	GetComputationalTimeUserAttribute (const NXString &title, int index)
	Gets a time attribute by Title and array Index.

NXOpen::NXObject::ComputationalTime	GetComputationalTimeUserAttribute (const char *title, int index)
	Gets a time attribute by Title and array Index.

int	GetIntegerAttribute (const NXString &title)
	Gets an integer attribute by title.

int	GetIntegerAttribute (const char *title)
	Gets an integer attribute by title.

int	GetIntegerUserAttribute (const NXString &title, int index)
	Gets an integer attribute by Title and array Index.

int	GetIntegerUserAttribute (const char *title, int index)
	Gets an integer attribute by Title and array Index.

double	GetRealAttribute (const NXString &title)
	Gets a real attribute by title.

double	GetRealAttribute (const char *title)
	Gets a real attribute by title.

double	GetRealUserAttribute (const NXString &title, int index)
	Gets a real attribute by Title and array Index.

double	GetRealUserAttribute (const char *title, int index)
	Gets a real attribute by Title and array Index.

NXString	GetReferenceAttribute (const NXString &title)
	Gets the reference string (not the calculated value) of a string attribute that uses a reference string.

NXString	GetReferenceAttribute (const char *title)
	Gets the reference string (not the calculated value) of a string attribute that uses a reference string.

NXString	GetStringAttribute (const NXString &title)
	Gets a string attribute value by title.

NXString	GetStringAttribute (const char *title)
	Gets a string attribute value by title.

NXString	GetStringUserAttribute (const NXString &title, int index)
	Gets a string attribute by Title and array Index.

NXString	GetStringUserAttribute (const char *title, int index)
	Gets a string attribute by Title and array Index.

NXString	GetTimeAttribute (NXOpen::NXObject::DateAndTimeFormat format, const NXString &title)
	Gets a time attribute by title.

NXString	GetTimeAttribute (NXOpen::NXObject::DateAndTimeFormat format, const char *title)
	Gets a time attribute by title.

NXString	GetTimeUserAttribute (const NXString &title, int index)
	Gets a time attribute by Title and array Index.

NXString	GetTimeUserAttribute (const char *title, int index)
	Gets a time attribute by Title and array Index.

NXOpen::NXObject::AttributeInformation	GetUserAttribute (const NXString &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.

NXOpen::NXObject::AttributeInformation	GetUserAttribute (const char *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.

NXString	GetUserAttributeAsString (const NXString &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.

NXString	GetUserAttributeAsString (const char *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.

bool	GetUserAttributeLock (const NXString &title, NXOpen::NXObject::AttributeType type)
	Determine the lock of the given attribute.

bool	GetUserAttributeLock (const char *title, NXOpen::NXObject::AttributeType type)
	Determine the lock of the given attribute.

std::vector < NXOpen::NXObject::AttributeInformation >	GetUserAttributes ()
	Gets all the attributes that have been set on the given object.

std::vector < NXOpen::NXObject::AttributeInformation >	GetUserAttributes (bool includeUnset)
	Gets all the attributes that have been set on the given object.

std::vector < NXOpen::NXObject::AttributeInformation >	GetUserAttributes (bool includeUnset, bool addStringValues)
	Gets all the attributes that have been set on the given object.

std::vector< NXString >	GetUserAttributesAsStrings ()
	Gets all the attributes that have been set on the given object.

std::vector< NXOpen::NXObject * >	GetUserAttributeSourceObjects ()
	Returns an array of objects from which this object presents attributes.

bool	HasUserAttribute (const NXString &title, NXOpen::NXObject::AttributeType type, int index)
	Determines if an attribute with the given Title, Type and array Index is present on the object If the attribute is not an array, the Index is ignored (if this is known beforehand, we recommend setting the Index to -1 to save time).

bool	HasUserAttribute (const char *title, NXOpen::NXObject::AttributeType type, int index)
	Determines if an attribute with the given Title, Type and array Index is present on the object If the attribute is not an array, the Index is ignored (if this is known beforehand, we recommend setting the Index to -1 to save time).

virtual bool	IsOccurrence ()
	Returns whether this object is an occurrence or not.

virtual NXString	JournalIdentifier ()
	Returns the identifier that would be recorded in a journal for this object.

virtual NXString	Name ()
	Returns the custom name of the object.

virtual NXOpen::Assemblies::Component *	OwningComponent ()
	Returns the owning component, if this object is an occurrence.

virtual NXOpen::BasePart *	OwningPart ()
	Returns the owning part of this object Created in NX3.0.0.

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

virtual NXOpen::INXObject *	Prototype ()
	Returns the prototype of this object if it is an occurrence.

void	SetAttribute (const NXString &title, int value)
	Creates or modifies an integer attribute.

void	SetAttribute (const char *title, int value)
	Creates or modifies an integer attribute.

void	SetAttribute (const NXString &title, int value, NXOpen::Update::Option option)
	Creates or modifies an integer attribute with the option to update or not.

void	SetAttribute (const char *title, int value, NXOpen::Update::Option option)
	Creates or modifies an integer attribute with the option to update or not.

void	SetAttribute (const NXString &title, double value)
	Creates or modifies a real attribute.

void	SetAttribute (const char *title, double value)
	Creates or modifies a real attribute.

void	SetAttribute (const NXString &title, double value, NXOpen::Update::Option option)
	Creates or modifies a real attribute with the option to update or not.

void	SetAttribute (const char *title, double value, NXOpen::Update::Option option)
	Creates or modifies a real attribute with the option to update or not.

void	SetAttribute (const NXString &title, const NXString &value)
	Creates or modifies a string attribute.

void	SetAttribute (const char title, const char value)
	Creates or modifies a string attribute.

void	SetAttribute (const NXString &title, const NXString &value, NXOpen::Update::Option option)
	Creates or modifies a string attribute with the option to update or not.

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

void	SetAttribute (const NXString &title)
	Creates or modifies a null attribute which is an attribute with a title and no value.

void	SetAttribute (const char *title)
	Creates or modifies a null attribute which is an attribute with a title and no value.

void	SetAttribute (const NXString &title, NXOpen::Update::Option option)
	Creates or modifies a null attribute with the option to update or not.

void	SetAttribute (const char *title, NXOpen::Update::Option option)
	Creates or modifies a null attribute with the option to update or not.

void	SetBooleanUserAttribute (const NXString &title, int index, bool value, NXOpen::Update::Option option)
	Creates or modifies a boolean attribute with the option to update or not.

void	SetBooleanUserAttribute (const char *title, int index, bool value, NXOpen::Update::Option option)
	Creates or modifies a boolean attribute with the option to update or not.

virtual void	SetName (const NXString &name)
	Sets the custom name of the object.

void	SetName (const char *name)
	Sets the custom name of the object.

void	SetReferenceAttribute (const NXString &title, const NXString &value)
	Creates or modifies a string attribute which uses a reference string.

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

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

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

void	SetTimeAttribute (const NXString &title, const NXString &value)
	Creates or modifies a time attribute.

void	SetTimeAttribute (const char title, const char value)
	Creates or modifies a time attribute.

void	SetTimeAttribute (const NXString &title, const NXString &value, NXOpen::Update::Option option)
	Creates or modifies a time attribute with the option to update or not.

void	SetTimeAttribute (const char title, const char value, NXOpen::Update::Option option)
	Creates or modifies a time attribute with the option to update or not.

void	SetTimeUserAttribute (const NXString &title, int index, const NXString &value, NXOpen::Update::Option option)
	Creates or modifies a time attribute with the option to update or not.

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

void	SetTimeUserAttribute (const NXString &title, int index, const NXOpen::NXObject::ComputationalTime &value, NXOpen::Update::Option option)
	Creates or modifies a time attribute with the option to update or not.

void	SetTimeUserAttribute (const char *title, int index, const NXOpen::NXObject::ComputationalTime &value, NXOpen::Update::Option option)
	Creates or modifies a time attribute with the option to update or not.

void	SetUserAttribute (const NXOpen::NXObject::AttributeInformation &info, NXOpen::Update::Option option)
	Creates or modifies an attribute with the option to update or not.

void	SetUserAttribute (const NXString &title, int index, int value, NXOpen::Update::Option option)
	Creates or modifies an integer attribute with the option to update or not.

void	SetUserAttribute (const char *title, int index, int value, NXOpen::Update::Option option)
	Creates or modifies an integer attribute with the option to update or not.

void	SetUserAttribute (const NXString &title, int index, double value, NXOpen::Update::Option option)
	Creates or modifies a real attribute with the option to update or not.

void	SetUserAttribute (const char *title, int index, double value, NXOpen::Update::Option option)
	Creates or modifies a real attribute with the option to update or not.

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

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

void	SetUserAttribute (const NXString &title, int index, NXOpen::Update::Option option)
	Creates or modifies a null attribute with the option to update or not.

void	SetUserAttribute (const char *title, int index, NXOpen::Update::Option option)
	Creates or modifies a null attribute with the option to update or not.

void	SetUserAttributeLock (const NXString &title, NXOpen::NXObject::AttributeType type, bool lock)
	Lock or unlock the given attribute.

void	SetUserAttributeLock (const char *title, NXOpen::NXObject::AttributeType type, bool lock)
	Lock or unlock the given attribute.

Public Member Functions inherited from NXOpen::TaggedObject
tag_t	GetTag () const
	<b>Deprecated</b>:<br> Use Tag instead.

tag_t	Tag () const
	Returns the tag of this object.

Public Member Functions inherited from NXOpen::INXObject
NXOpen::INXObject *	FindObject (const char *journalIdentifier)
	Finds the NXObject with the given identifier as recorded in a journal.

void	SetName (const char *name)
	Sets the custom name of the object.

Detailed Description

Represents a sketch
Use the SketchCollection class to create a sketch.

Created in NX3.0.0.

Member Enumeration Documentation

enum NXOpen::Sketch::AddEllipseOption

Used by 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:

AddEllipseOptionTreatAsEllipse	treat as ellipse
AddEllipseOptionTreatAsConic	treat as conic

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:

AlternateSolutionOptionFalse	Use the regular solution.
AlternateSolutionOptionTrue	Use the alternate solution.

enum NXOpen::Sketch::AssocType

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

Enumerator:

AssocTypeNone	Use the entire geometric item, as opposed to a point.
AssocTypeStartPoint	Start point. E.g. the start point of a line
AssocTypeEndPoint	End point. E.g. the start point of a line
AssocTypeArcCenter	Center of an arc, circle, or ellipse.
AssocTypeTangency	Create the dimension tangent to the geometric item.
AssocTypeCurvePoint	A point on a spline.
AssocTypeAnchorPoint	The anchor of a conic.
AssocTypeMidpoint	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. Sketch::AutoDimensioningRuleSymmetric : create symmetric dimensions if the curves are symmetric Sketch::AutoDimensioningRuleAdjacentAngle : create angles between adjacent lines Sketch::AutoDimensioningRuleLength : create length dimension for lines Sketch::AutoDimensioningRuleHorizontalVertical : create horizontal and vertical dimensions Sketch::AutoDimensioningRuleReferenceAxes : create dimensions between curves and reference axes

Enumerator:

AutoDimensioningRuleAdjacentAngle	Create Adjacent Angles.
AutoDimensioningRuleLength	Create Length Dimension.
AutoDimensioningRuleHorizontalVertical	Create Horizontal and Vertical Dimensions.
AutoDimensioningRuleReferenceAxes	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:

ConstraintClassNotConstraint	not constraint
ConstraintClassAny	Used in query methods that filter by constraint class to select both types of constraints.
ConstraintClassGeometric	A non-dimension constraint.
ConstraintClassDimension	A dimensional constraint.

enum NXOpen::Sketch::ConstraintGeometryHelpType

Used in ConstraintHelp to indicate what type of help it is.

Enumerator:

ConstraintGeometryHelpTypePoint	point
ConstraintGeometryHelpTypeParameter	parameter

enum NXOpen::Sketch::ConstraintPointType

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

Enumerator:

ConstraintPointTypeNone	The geometry is not a point.
ConstraintPointTypeStartVertex	Start vertex (e.g. the start point of a line)
ConstraintPointTypeEndVertex	End vertex (e.g. the end point of a line)
ConstraintPointTypeArcCenter	Center of a circle, arc, or ellipse.
ConstraintPointTypeSplineDefiningPoint	A defining point of a spline.
ConstraintPointTypeAnchor	The anchor point of a conic.

enum NXOpen::Sketch::ConstraintType

Represents the type of constraint.

Enumerator:

ConstraintTypeNoCon	Used in query methods that filter by constraint type to select any type of constraint.
ConstraintTypeFixed	fixed
ConstraintTypeHorizontal	horizontal
ConstraintTypeVertical	vertical
ConstraintTypeParallel	parallel
ConstraintTypePerpendicular	perpendicular
ConstraintTypeCollinear	collinear
ConstraintTypeEqualLength	equal length
ConstraintTypeEqualRadius	equal radius
ConstraintTypeConstantLength	constant length
ConstraintTypeConstantAngle	constant angle
ConstraintTypeCoincident	coincident
ConstraintTypeConcentric	concentric
ConstraintTypeMirror	mirror
ConstraintTypePointOnCurve	point on curve
ConstraintTypeMidpoint	midpoint
ConstraintTypeTangent	tangent
ConstraintTypeRadiusDim	radius dim
ConstraintTypeDiameterDim	diameter dim
ConstraintTypeHorizontalDim	horizontal dim
ConstraintTypeVerticalDim	vertical dim
ConstraintTypeParallelDim	parallel dim
ConstraintTypePerpendicularDim	perpendicular dim
ConstraintTypeAngularDim	system will decide if it is major or minor
ConstraintTypeReservedCon1	Do not use.
ConstraintTypeReservedCon2	Do not use.
ConstraintTypeReservedCon3	Do not use.
ConstraintTypeReservedCon4	Do not use.
ConstraintTypeReservedCon5	Do not use.
ConstraintTypeReservedCon6	Do not use.
ConstraintTypePointOnString	point on string
ConstraintTypeSlope	slope
ConstraintTypeUniformScaled	uniform scaled
ConstraintTypeNonUniformScaled	non uniform scaled
ConstraintTypeAssocTrim	Limited support.
ConstraintTypeAssocOffset	Limited support.
ConstraintTypePerimeterDim	perimeter dim
ConstraintTypeOffset	offset
ConstraintTypeNormal	normal
ConstraintTypePointOnLoop	point on loop
ConstraintTypeRecipeTrim	recipe trim
ConstraintTypePattern	pattern
ConstraintTypeMinorAngularDim	minor angular dim
ConstraintTypeMajorAngularDim	major angular dim
ConstraintTypeLastConType	The last constraint type indicator; NOT to be used.

enum NXOpen::Sketch::ConstraintVisibility

Indicates the visibility of the constraints The APIs that use this enum are deprecated in NX85 The Sketch::ConstraintVisibilitySome option will behave the same as the Sketch::ConstraintVisibilityAll option.

   Please use @link NXOpen::Preferences::SessionSketch::DisplayConstraintSymbols NXOpen::Preferences::SessionSketch::DisplayConstraintSymbols@endlink  and
   @link NXOpen::Preferences::SessionSketch::SetDisplayConstraintSymbols NXOpen::Preferences::SessionSketch::SetDisplayConstraintSymbols@endlink  instead.

Deprecated:: Deprecated in NX8.5.0. Please use NXOpen::Preferences::SessionSketch::DisplayConstraintSymbols and NXOpen::Preferences::SessionSketch::SetDisplayConstraintSymbols

Enumerator:

ConstraintVisibilityNone

No constraints visible.

ConstraintVisibilitySome

Certain constraints are visible.

Equivalent to having the UI show-all-constraints and show-no-constraints toggles off

ConstraintVisibilityAll

All constraints are visible.

enum NXOpen::Sketch::CreateDimensionOption

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

Enumerator:

CreateDimensionOptionFalse	Do not create a radius dimension.
CreateDimensionOptionTrue	Create a radius dimension.

enum NXOpen::Sketch::CreateInferConstraintSetting

Indicates if the infer constraints will be created or not.

Enumerator:

CreateInferConstraintSettingOn	Create infer constraints.
CreateInferConstraintSettingOff	Dont create infer constraints.

enum NXOpen::Sketch::DeleteThirdCurveOption

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

Enumerator:

DeleteThirdCurveOptionFalse	Do not delete the 3rd curve.
DeleteThirdCurveOptionTrue	Delete the 3rd curve.

enum NXOpen::Sketch::DimensionOption

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

Enumerator:

DimensionOptionCreateAsDriving	Create dimension as driving.
DimensionOptionCreateAsReference	Create dimension as reference.
DimensionOptionCreateAsAutomatic	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:

InferConstraintsOptionInferNoConstraints	Do not infer constraints.
InferConstraintsOptionInferCoincidentConstraints	Infer constraints.

enum NXOpen::Sketch::PlaneOption

Specifies the plane type used for a Sketch.

Enumerator:

PlaneOptionInferred	Use inferred plane.
PlaneOptionExistingPlane	Use existing plane.
PlaneOptionNewPlane	Use new plane.
PlaneOptionNewCsys	Use new CSYS.

enum NXOpen::Sketch::Status

Represents the status of the sketch.

Enumerator:

StatusUnknown	unknown
StatusNotEvaluated	not evaluated
StatusUnderConstrained	More constraints are needed to fully constrain the sketch.
StatusWellConstrained	The sketch is fully constrained.
StatusOverConstrained	The sketch has more constraints than is needed.
StatusInconsistentlyConstrained	The sketch has conflicting constraints.

enum NXOpen::Sketch::TrimInputOption

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

Enumerator:

TrimInputOptionFalse	Do not trim the input curves.
TrimInputOptionTrue	Trim the input curves.

enum NXOpen::Sketch::UpdateLevel

Used to indicate how much the updating should occur.

Enumerator:

UpdateLevelSketchOnly	Only update the sketch.
UpdateLevelModel	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:

ViewReorientFalse	Do not reorient view to sketch.
ViewReorientTrue	Reorient view to sketch.

Member Function Documentation

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")

Parameters

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

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")

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

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")

Parameters

crv	Must be a curve or point

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")

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 Sketch::AddEllipseOption for more details. The default value is Sketch::AddEllipseOptionTreatAsEllipse . In order to treat an ellipse as a conic, its end angle minus its start angle must be less than 180 degrees.

void NXOpen::Sketch::AddGeometry	(	NXOpen::Sketch::InferConstraintsOption	inferCoincidentConstraints,
		NXOpen::Sketch::AddEllipseOption	ellipseOption,
		const std::vector< 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")

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 Sketch::AddEllipseOption for more details. The default value is Sketch::AddEllipseOptionTreatAsEllipse . 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

NXOpen::ISurface* NXOpen::Sketch::AttachPlane ( )

Returns the plane that the sketch is attached to
Created in NX3.0.0.

License requirements : None

std::vector<NXOpen::SketchConstraint *> NXOpen::Sketch::AutoConstrain	(	double	linearTolerance,
		double	angularTolerance,
		bool	allowRemoteConstraints,
		const std::vector< NXOpen::SmartObject * > &	geometries,
		const std::vector< NXOpen::Sketch::ConstraintType > &	autoconstraintTypes
	)

Creates Automatic Constraints on input set of geometries.

Returns: Array of deduced constraints
Created in NX4.0.0.

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

Parameters

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

std::vector<NXOpen::NXObject *> NXOpen::Sketch::CopyObjects ( const std::vector< NXOpen::NXObject * > & inputObjects )

Creates copies of input objects and constraints between these objects.

Returns: Copies of objects
Created in NX4.0.0.

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

Parameters

inputObjects Objects to be copied

void NXOpen::Sketch::CopyObjectsWithDimensionOutput	(	const std::vector< NXOpen::NXObject * > &	inputObjects,
		std::vector< NXOpen::NXObject * > &	outputObjects,
		std::vector< NXOpen::NXObject * > &	outputDims
	)

Creates copies of input objects and constraints between these objects.

This function is same as 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")

Parameters

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

std::vector<NXOpen::Sketch::CopyObjectData> NXOpen::Sketch::CopyObjectsWithTracking ( const std::vector< 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.

Returns: Map between the original input object and the corresponding copied object
Created in NX7.5.0.

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

Parameters

inputObjects Objects to be copied

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateCoincidentConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	geom1,
		const NXOpen::Sketch::ConstraintGeometry &	geom2
	)

Creates a coincident constraint.

Returns: The coincident constraint
Created in NX3.0.0.

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

Parameters

geom1	Must be a vertex
geom2	Must be a vertex

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateCollinearConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2
	)

Creates a collinear constraint.

One of the input constraint geometries must be a line.

Returns: The collinear constraint
Created in NX3.0.0.

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

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateConcentricConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2
	)

Creates a concentric constraint.

One of the input constraint geometries must be a curve.

Returns: The concentric constraint
Created in NX3.0.0.

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

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateConstantAngleConstraint ( const NXOpen::Sketch::ConstraintGeometry & conGeom )

Creates a constant angle constraint.

Returns: The constant angle constraint
Created in NX3.0.0.

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

Parameters

conGeom Must be a line

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateConstantLengthConstraint ( const NXOpen::Sketch::ConstraintGeometry & conGeom )

Creates a constant length constraint.

Returns: The constant length constraint
Created in NX3.0.0.

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

Parameters

conGeom Must be a line

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateDiameterDimension	(	const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const NXOpen::Point3d &	dimOrigin,
		NXOpen::Expression *	expression
	)

Creates a diameter dimension constraint.

Returns: The diametral dimension constraint
Created in NX3.0.0.

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be NULL

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateDiameterDimension	(	const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const 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

Returns: The diametral dimension constraint
Created in NX4.0.0.

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be NULL
refDim	option for creating driving or reference dimension

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateDimension	(	NXOpen::Sketch::ConstraintType	dimType,
		const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const NXOpen::Sketch::DimensionGeometry &	dimObject2,
		const 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 CreateRadialDimension or CreateDiameterDimension . To create a perimeter dimension, use CreatePerimeterDimension

Returns: The dimensional constraint
Created in NX3.0.0.

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

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 NULL

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateDimension	(	NXOpen::Sketch::ConstraintType	dimType,
		const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const NXOpen::Sketch::DimensionGeometry &	dimObject2,
		const 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 CreateRadialDimension or CreateDiameterDimension . To create a perimeter dimension, use CreatePerimeterDimension . This function takes in an argument to create the dimension as driving or reference.

Returns: The dimensional constraint
Created in NX4.0.0.

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

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 NULL
refDim	option for creating driving or reference dimension

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateEqualLengthConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2
	)

Creates an equal length constraint.

One of the input constraint geometries must be a line.

Returns: The equal length constraint
Created in NX3.0.0.

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

Parameters

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateEqualRadiusConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2
	)

Creates an equal radius constraint.

One of the input constraint geometries must be a curve.

Returns: The equal radius constraint
Created in NX3.0.0.

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

Parameters

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateFixedConstraint ( const NXOpen::Sketch::ConstraintGeometry & geom )

Creates a fixed constraint.

Returns: The fixed constraint
Created in NX3.0.0.

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

Parameters

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

std::vector<NXOpen::SketchGeometricConstraint *> NXOpen::Sketch::CreateFullyFixedConstraints ( const 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.

Returns: The fixed constraints
Created in NX5.0.0.

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

Parameters

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateHorizontalConstraint ( const NXOpen::Sketch::ConstraintGeometry & geom )

Creates a horizontal constraint.

Returns: The horizontal constraint
Created in NX3.0.0.

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

Parameters

geom	Must be a line

NXOpen::Sketch::CreateInferConstraintSetting NXOpen::Sketch::CreateInferConstraintsSetting ( )

Returns the toggle that controls the creation of infer constraints in sketch
Created in NX4.0.0.

License requirements : None

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateMidpointConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const 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.

Returns: The midpoint constraint
Created in NX3.0.0.

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

Parameters

conGeom1	con geom1
conGeom2	con geom2

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateNonUniformScaledConstraint ( const NXOpen::Sketch::ConstraintGeometry & conGeom )

Creates a non-uniform scale constraint.

Returns: The non-uniform scale constraint
Created in NX3.0.0.

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

Parameters

conGeom Must be a spline

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateNormalConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometryHelp &	geom1Help,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2,
		const 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

Returns: The normal constraint
Created in NX3.0.0.

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

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateParallelConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const 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).

Returns: The parallel constraint
Created in NX3.0.0.

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

Parameters

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

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreatePerimeterDimension	(	const std::vector< NXOpen::Curve * > &	curves,
		const NXOpen::Point3d &	dimOrigin,
		NXOpen::Expression *	expression
	)

Creates a perimeter dimension constraint.

Returns: The perimeter dimensional constraint
Created in NX3.0.0.

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

Parameters

curves	The curves that form the perimeter
dimOrigin	Not currently used
expression	Defining expression for the dimension. Can be NULL

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreatePerpendicularConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const 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).

Returns: The perpendicular constraint
Created in NX3.0.0.

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

Parameters

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

NXOpen::SketchHelpedGeometricConstraint* NXOpen::Sketch::CreatePointOnCurveConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const NXOpen::Sketch::ConstraintGeometry &	conGeom2,
		const 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.

Returns: The point on curve constraint
Created in NX3.0.0.

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

Parameters

conGeom1	con geom1
conGeom2	con geom2
help	help

NXOpen::SketchHelpedGeometricConstraint* NXOpen::Sketch::CreatePointOnStringConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const std::vector< NXOpen::Curve * > &	curvesInString,
		const NXOpen::Sketch::ConstraintGeometryHelp &	helpData,
		int	curveWhichHelpParamAppliesTo
	)

Creates a point on string constraint.

@return  The point on string constraint

Created in NX3.0.0.

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

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	help data
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

NXOpen::SketchHelpedGeometricConstraint* NXOpen::Sketch::CreatePointOnStringConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		NXOpen::Curve *	curveInString,
		const 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.

Returns: The point on string constraint
Created in NX3.0.0.

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

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	help data

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateRadialDimension	(	const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const NXOpen::Point3d &	dimOrigin,
		NXOpen::Expression *	expression
	)

Creates a radial dimension constraint.

Returns: The radial dimension constraint
Created in NX3.0.0.

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be NULL

NXOpen::SketchDimensionalConstraint* NXOpen::Sketch::CreateRadialDimension	(	const NXOpen::Sketch::DimensionGeometry &	dimObject1,
		const 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

Returns: The radial dimension constraint
Created in NX4.0.0.

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

Parameters

dimObject1	Should be an arc
dimOrigin	The location where the dimension should be placed
expression	Defining expression for the dimension. Can be NULL
refDim	option for creating driving or reference dimension

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateSlopeConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	conGeom1,
		const 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.

Returns: The slope constraint
Created in NX3.0.0.

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

Parameters

conGeom1	con geom1
conGeom2	con geom2

NXOpen::SketchTangentConstraint* NXOpen::Sketch::CreateTangentConstraint	(	const NXOpen::Sketch::ConstraintGeometry &	geom1,
		const NXOpen::Sketch::ConstraintGeometryHelp &	geom1Help,
		const NXOpen::Sketch::ConstraintGeometry &	geom2,
		const NXOpen::Sketch::ConstraintGeometryHelp &	geom2Help
	)

Creates a tangent constraint.

Note: the input constraint geometries cannot both be linear.

Returns: The tangent constraint
Created in NX3.0.0.

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

Parameters

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

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateUniformScaledConstraint ( const NXOpen::Sketch::ConstraintGeometry & conGeom )

Creates a uniform scale constraint.

Returns: The uniform scale constraint
Created in NX3.0.0.

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

Parameters

conGeom Must be a spline

NXOpen::SketchGeometricConstraint* NXOpen::Sketch::CreateVerticalConstraint ( const NXOpen::Sketch::ConstraintGeometry & geom )

Creates a vertical constraint.

Returns: The vertical constraint
Created in NX3.0.0.

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

Parameters

geom	Must be a line

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")

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

void NXOpen::Sketch::DeleteConstraintsOnGeometries ( const std::vector< 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")

Parameters

objects Objects whose constraints needs to be deleted

void NXOpen::Sketch::DeleteConstraintsOnGeometries ( const std::vector< 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")

Parameters

objects Objects whose constraints needs to be deleted

NXOpen::ErrorList* NXOpen::Sketch::DeleteObjects ( const std::vector< NXOpen::NXObject * > & objects )

Deletes objects from the sketch.

Returns: List of errors encountered during the delete
Created in NX3.0.0.

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

Parameters

objects Objects to be deleted

bool NXOpen::Sketch::DOFDisplay ( )

Returns a flag indicating whether the degree of freedom arrows are currently being displayed
Created in NX3.0.0.

License requirements : None

NXOpen::Features::Feature* NXOpen::Sketch::Feature ( )

Returns the feature associated with this sketch
Created in NX3.0.0.

License requirements : None

std::vector<NXOpen::Arc *> NXOpen::Sketch::Fillet	(	NXOpen::Curve *	curve1,
		NXOpen::Curve *	curve2,
		const NXOpen::Point3d &	helpPoint1,
		const NXOpen::Point3d &	helpPoint2,
		double	radius,
		NXOpen::Sketch::TrimInputOption	doTrim,
		NXOpen::Sketch::CreateDimensionOption	createRadiusDim,
		NXOpen::Sketch::AlternateSolutionOption	alternateSolution,
		std::vector< 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.

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
Created in NX3.0.0.

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

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.
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.

std::vector<NXOpen::Arc *> NXOpen::Sketch::Fillet	(	NXOpen::Curve *	curve1,
		NXOpen::Curve *	curve2,
		const NXOpen::Point3d &	helpPoint1,
		const NXOpen::Point3d &	helpPoint2,
		const NXOpen::Point3d &	pointOnArc,
		double	radius,
		NXOpen::Sketch::TrimInputOption	doTrim,
		NXOpen::Sketch::CreateDimensionOption	createRadiusDim,
		NXOpen::Sketch::AlternateSolutionOption	alternateSolution,
		std::vector< 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.

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
Created in NX7.5.0.

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

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.
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.

std::vector<NXOpen::Arc *> NXOpen::Sketch::Fillet	(	NXOpen::Curve *	curve1,
		NXOpen::Curve *	curve2,
		NXOpen::Curve *	curve3,
		const NXOpen::Point3d &	helpPoint1,
		const NXOpen::Point3d &	helpPoint2,
		const NXOpen::Point3d &	helpPoint3,
		double	radius,
		NXOpen::Sketch::TrimInputOption	doTrim,
		NXOpen::Sketch::DeleteThirdCurveOption	doDelete,
		NXOpen::Sketch::CreateDimensionOption	createRadiusDim,
		NXOpen::Sketch::AlternateSolutionOption	alternateSolution,
		std::vector< 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.

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
Created in NX3.0.0.

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

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.
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.

std::vector<NXOpen::Arc *> NXOpen::Sketch::Fillet	(	NXOpen::Curve *	curve1,
		NXOpen::Curve *	curve2,
		NXOpen::Curve *	curve3,
		const NXOpen::Point3d &	helpPoint1,
		const NXOpen::Point3d &	helpPoint2,
		const NXOpen::Point3d &	helpPoint3,
		const NXOpen::Point3d &	pointOnArc,
		double	radius,
		NXOpen::Sketch::TrimInputOption	doTrim,
		NXOpen::Sketch::DeleteThirdCurveOption	doDelete,
		NXOpen::Sketch::CreateDimensionOption	createRadiusDim,
		NXOpen::Sketch::AlternateSolutionOption	alternateSolution,
		std::vector< 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.

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
Created in NX7.5.0.

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

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.
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.

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")

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")

std::vector<NXOpen::SketchConstraint *> NXOpen::Sketch::GetAllConstraintsOfType	(	NXOpen::Sketch::ConstraintClass	conClass,
		NXOpen::Sketch::ConstraintType	conType
	)

Gets all constraints in the sketch of a particular type.

Returns: All the constraints in the sketch of the specified type
Created in NX3.0.0.

License requirements : None

Parameters

conClass	Optional filter. Use Sketch::ConstraintClassAny if you do not want to filter by constraint class
conType	Optional filter. Use Sketch::ConstraintTypeNoCon if you do not want to filter by constraint type

std::vector<NXOpen::Expression *> NXOpen::Sketch::GetAllExpressions ( )

Returns all the expressions in the sketch.

Returns: All the expressions in the sketch
Created in NX3.0.0.

License requirements : None

std::vector<NXOpen::NXObject *> NXOpen::Sketch::GetAllGeometry ( )

Returns all the curves and points in the sketch.

Returns: All the curves and points in the sketch
Created in NX3.0.0.

License requirements : None

std::vector<NXOpen::SketchConstraint *> NXOpen::Sketch::GetConstraintsForGeometry	(	NXOpen::SmartObject *	geometry,
		NXOpen::Sketch::ConstraintClass	conClass
	)

Gets all the constraints associated with a particular geometric item.

Returns: All the constraints associated with the geometry that is input
Created in NX3.0.0.

License requirements : None

Parameters

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

NXOpen::Vector3d NXOpen::Sketch::GetReferenceDirection	(	NXOpen::IReferenceAxis **	referenceAxis,
		NXOpen::AxisOrientation *	referenceAxisOrientation,
		NXOpen::Sense *	referenceAxisSense
	)

Gets the reference direction of the sketch.

Returns: Created in NX3.0.0.

License requirements : None

Parameters

referenceAxis	An edge, datum axis, datum plane, or face that the sketch uses as a reference. May be NULL.
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.

NXOpen::Sketch::Status NXOpen::Sketch::GetStatus ( 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.

Returns: The sketch's status, which indicates how well constrained the sketch is
Created in NX3.0.0.

License requirements : None

Parameters

dofNeeded The number of degrees of freedom left in the sketch

void NXOpen::Sketch::HideDimensions ( const std::vector< 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")

Parameters

inputObjects Geometry and groups in active sketch

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")

void NXOpen::Sketch::HideDimensions ( const std::vector< 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")

Parameters

objects Geometry and vertices in active sketch

bool NXOpen::Sketch::IsActive ( )

Returns true if the sketch is active
Created in NX3.0.0.

License requirements : None

bool NXOpen::Sketch::IsDraftingSketch ( )

Returns true if drafting sketch
Created in NX6.0.0.

License requirements : None

bool NXOpen::Sketch::IsInternal ( )

Returns true if the sketch is internal.

Created in NX6.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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")

void NXOpen::Sketch::MakeDatumsExternal ( )

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

Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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.

License requirements : solid_modeling ("SOLIDS MODELING")

std::vector<NXOpen::SmartObject *> NXOpen::Sketch::MirrorObjects	(	NXOpen::DisplayableObject *	centerline,
		const std::vector< NXOpen::SmartObject * > &	objectsToMirror
	)

Creates a reflection of the input geometry.

    <br> 
   This API is now deprecated.
   Please use @link SketchMirrorBuilder SketchMirrorBuilder@endlink  instead.
    <br> 
@return  The mirrored geometry that was created

Deprecated:: Deprecated in NX5.0.0. Please use SketchMirrorBuilder instead.

Created in NX4.0.0.

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

Parameters

centerline	Axis of reflection for the mirror. Must be a linear curve, edge, datum axis or datum plane
objectsToMirror	Points and curves to mirror. None of the curves may be used as a centerline for another mirror operation

NXOpen::NXMatrix* NXOpen::Sketch::Orientation ( )

Returns the orientation matrix of the local coordinate system of the sketch
Created in NX3.0.0.

License requirements : None

NXOpen::Point3d NXOpen::Sketch::Origin ( )

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 ( )

Contains preferences for the sketch
Created in NX3.0.0.

void NXOpen::Sketch::Reattach	(	NXOpen::ISurface *	attachmentPlane,
		NXOpen::IReferenceAxis *	referenceAxis,
		const NXOpen::Vector3d &	referenceDirection,
		NXOpen::AxisOrientation	referenceAxisOrientation,
		NXOpen::Sense	referenceAxisSense,
		NXOpen::PlaneNormalOrientation	normalOrientation,
		const NXOpen::Point3d &	localCoordinateSystemOrigin
	)

Reattaches a sketch.

For documentation for the parameters for this method, see the documentation for SketchCollection::CreateSketch

Created in NX3.0.0.

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

Parameters

attachmentPlane	attachment plane
referenceAxis	reference axis
referenceDirection	reference direction
referenceAxisOrientation	reference axis orientation
referenceAxisSense	reference axis sense
normalOrientation	normal orientation
localCoordinateSystemOrigin	Origin of the sketch's local coordinate system

void NXOpen::Sketch::RunAutoDimension ( )

Run auto dimensioning.

Created in NX7.5.0.

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

void NXOpen::Sketch::SetCreateInferConstraintsSetting ( NXOpen::Sketch::CreateInferConstraintSetting createInferCon )

Sets the toggle that controls the creation of infer constraints in sketch
Created in NX4.0.0.

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

Parameters

createInferCon create infer con

void NXOpen::Sketch::SetDOFDisplay ( bool displayDof )

Sets a flag indicating whether the degree of freedom arrows are currently being displayed
Created in NX3.0.0.

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

Parameters

displayDof display dof

void NXOpen::Sketch::SetReferenceDirection	(	NXOpen::IReferenceAxis *	referenceAxis,
		const 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 SketchCollection::CreateSketch .

Created in NX3.0.0.

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

Parameters

referenceAxis	reference axis
referenceDirection	reference direction
referenceAxisOrientation	reference axis orientation
referenceAxisSense	reference axis sense

void NXOpen::Sketch::SetUpdateScope ( NXOpen::Sketch::UpdateLevel updateScope )

Sets the current update scope.

Used in Direct Sketch to control update
Created in NX8.0.0.

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

Parameters

updateScope update scope

void NXOpen::Sketch::SetVisibilityOfConstraints ( NXOpen::Sketch::ConstraintVisibility visibility )

Sets the visibility of the constraints in the sketch

Deprecated:: Deprecated in NX8.5.0.

Use NXOpen::Preferences::SessionSketch::SetDisplayConstraintSymbols instead.

Created in NX3.0.0.

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

Parameters

visibility visibility

void NXOpen::Sketch::ShowDimensions ( const std::vector< 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")

Parameters

inputObjects Geometry and groups in active sketch

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")

void NXOpen::Sketch::ShowDimensions ( const std::vector< 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")

Parameters

objects Geometry and vertices in active sketch

void NXOpen::Sketch::Update ( )

Updates the sketch
Created in NX3.0.0.

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

void NXOpen::Sketch::Update ( const std::vector< 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")

Parameters

geoms Geoms that need to be updated

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")

void NXOpen::Sketch::UpdateConstraintDisplay ( const std::vector< 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")

Parameters

geoms Geoms for which cons must be re-displayed

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")

void NXOpen::Sketch::UpdateDimensionDisplay ( const std::vector< 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")

Parameters

geoms Geoms for which cons must be re-displayed

void NXOpen::Sketch::UpdateDimensionDisplay ( const std::vector< 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

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")

void NXOpen::Sketch::UpdateGeometryDisplay ( const std::vector< 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")

Parameters

geoms Geoms for which cons must be re-displayed

NXOpen::Sketch::UpdateLevel NXOpen::Sketch::UpdateScope ( )

Returns the current update scope.

Used in Direct Sketch to control update
Created in NX8.0.0.

License requirements : None

NXOpen::View* NXOpen::Sketch::View ( )

Returns the view corresponding to sketch
Created in NX6.0.0.

License requirements : None

NXOpen::Sketch::ConstraintVisibility NXOpen::Sketch::VisibilityOfConstraints ( )

Returns the visibility of the constraints in the sketch

Deprecated:: Deprecated in NX8.5.0.

Use NXOpen::Preferences::SessionSketch::DisplayConstraintSymbols instead.

Created in NX3.0.0.

License requirements : None

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

Sketch.hxx

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