NX Open C++ Reference Guide
Classes | Public Types | Public Member Functions
NXOpen::Sketch Class Reference

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

Inheritance diagram for NXOpen::Sketch:
NXOpen::DisplayableObject NXOpen::IProfile NXOpen::NXObject NXOpen::IFitTo NXOpen::INXObject NXOpen::TaggedObject NXOpen::INXObject NXOpen::INXObject

List of all members.

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. 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 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 (const std::vector< NXOpen::Curve * > &curves, NXOpen::Sketch::InferConstraintsOption inferCoincidentConstraints, NXOpen::Sketch::AddEllipseOption ellipseOption)
 Adds an array of curves (not points) 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::ISurfaceAttachPlane ()
 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::SketchGeometricConstraintCreateCoincidentConstraint (const NXOpen::Sketch::ConstraintGeometry &geom1, const NXOpen::Sketch::ConstraintGeometry &geom2)
 Creates a coincident constraint.
NXOpen::SketchGeometricConstraintCreateCollinearConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a collinear constraint.
NXOpen::SketchGeometricConstraintCreateConcentricConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a concentric constraint.
NXOpen::SketchGeometricConstraintCreateConstantAngleConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
 Creates a constant angle constraint.
NXOpen::SketchGeometricConstraintCreateConstantLengthConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
 Creates a constant length constraint.
NXOpen::SketchDimensionalConstraintCreateDiameterDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
 Creates a diameter dimension constraint.
NXOpen::SketchDimensionalConstraintCreateDiameterDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression, NXOpen::Sketch::DimensionOption refDim)
 Creates a diameter dimension constraint.
NXOpen::SketchDimensionalConstraintCreateDimension (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::SketchDimensionalConstraintCreateDimension (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::SketchGeometricConstraintCreateEqualLengthConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates an equal length constraint.
NXOpen::SketchGeometricConstraintCreateEqualRadiusConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates an equal radius constraint.
NXOpen::SketchGeometricConstraintCreateFixedConstraint (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::SketchGeometricConstraintCreateHorizontalConstraint (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::SketchGeometricConstraintCreateMidpointConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a midpoint constraint.
NXOpen::SketchGeometricConstraintCreateNonUniformScaledConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
 Creates a non-uniform scale constraint.
NXOpen::SketchGeometricConstraintCreateNormalConstraint (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::SketchGeometricConstraintCreateParallelConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a parallel constraint.
NXOpen::SketchDimensionalConstraintCreatePerimeterDimension (const std::vector< NXOpen::Curve * > &curves, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
 Creates a perimeter dimension constraint.
NXOpen::SketchGeometricConstraintCreatePerpendicularConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a perpendicular constraint.
NXOpen::SketchHelpedGeometricConstraintCreatePointOnCurveConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2, const NXOpen::Sketch::ConstraintGeometryHelp &help)
 Creates a point on curve constraint.
NXOpen::SketchHelpedGeometricConstraintCreatePointOnStringConstraint (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::SketchHelpedGeometricConstraintCreatePointOnStringConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, NXOpen::Curve *curveInString, const NXOpen::Sketch::ConstraintGeometryHelp &helpData)
 Creates a point on string constraint.
NXOpen::SketchDimensionalConstraintCreateRadialDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression)
 Creates a radial dimension constraint.
NXOpen::SketchDimensionalConstraintCreateRadialDimension (const NXOpen::Sketch::DimensionGeometry &dimObject1, const NXOpen::Point3d &dimOrigin, NXOpen::Expression *expression, NXOpen::Sketch::DimensionOption refDim)
 Creates a radial dimension constraint.
NXOpen::SketchGeometricConstraintCreateSlopeConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom1, const NXOpen::Sketch::ConstraintGeometry &conGeom2)
 Creates a slope constraint.
NXOpen::SketchTangentConstraintCreateTangentConstraint (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::SketchGeometricConstraintCreateUniformScaledConstraint (const NXOpen::Sketch::ConstraintGeometry &conGeom)
 Creates a uniform scale constraint.
NXOpen::SketchGeometricConstraintCreateVerticalConstraint (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.
NXOpen::ErrorListDeleteObjects (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::FeatureFeature ()
 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.
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::NXMatrixOrientation ()
 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::SketchPreferencesPreferences ()
 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
Created in NX3.0.0.
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 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::ViewView ()
 Returns the view corresponding to sketch
Created in NX6.0.0.
NXOpen::Sketch::ConstraintVisibility VisibilityOfConstraints ()
 Returns the visibility of the constraints in the sketch
Created in NX3.0.0.

Detailed Description

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



Created in NX3.0.0.


Member Enumeration Documentation

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

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.

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.

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.

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.

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

Enumerator:
ConstraintGeometryHelpTypePoint 

point

ConstraintGeometryHelpTypeParameter 

parameter

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.

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.

Indicates the visibility of the constraints.

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.

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.

Indicates if the infer constraints will be created or not.

Enumerator:
CreateInferConstraintSettingOn 

Create infer constraints.

CreateInferConstraintSettingOff 

Dont create infer constraints.

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.

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.

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.

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.

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.

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.

Used to indicate how much the updating should occur.

Enumerator:
UpdateLevelSketchOnly 

Only update the sketch.

UpdateLevelModel 

Update the full model and the sketch.

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

Activates the sketch
Created in NX3.0.0.



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

Parameters:
orientViewIndicates whether to orient the view to the sketch during activation

Adds a curve or point to the sketch
Created in NX3.0.0.



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

Parameters:
crvMust be a curve or point
inferCoincidentConstraintsWhether 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

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:
crvMust be a curve or point

Adds a curve or point to a sketch.


Created in NX3.0.0.

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

Parameters:
crvMust be a curve or point
inferCoincidentConstraintsWhether 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
ellipseOptionIf 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 ( const std::vector< NXOpen::Curve * > &  curves,
NXOpen::Sketch::InferConstraintsOption  inferCoincidentConstraints,
NXOpen::Sketch::AddEllipseOption  ellipseOption 
)

Adds an array of curves (not points) to a sketch.

Deprecated: Instead use the version of AddGeometry that permits an array of curves and points as input.


Deprecated:
Deprecated in NX6.0.1.


Created in NX5.0.2.

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

Parameters:
curvesMust be a curve or point
inferCoincidentConstraintsWhether 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
ellipseOptionIf 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:
inferCoincidentConstraintsWhether 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
ellipseOptionIf 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.
curvesOrPointsMust be a curve or point

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:
linearToleranceCapture Distance
angularToleranceCapture Angle
allowRemoteConstraintsAllow remote constraints
geometriesArray of geometries
autoconstraintTypesConstraint 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:
inputObjectsObjects 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:
inputObjectsObjects to be copied
outputObjectsCopies of objects
outputDimsCopies of dims

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:
inputObjectsObjects to be copied

Creates a coincident constraint.

Returns:
The coincident constraint
Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
Parameters:
geom1Must be a vertex
geom2Must be a vertex

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:
conGeom1Must be a line, linear edge, datum axis, or datum plane
conGeom2Must be a line, linear edge, datum axis, or datum plane

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:
conGeom1Must be an arc or ellipse or edge shaped as an arc or ellipse
conGeom2Must be an arc or ellipse or edge shaped as an arc or ellipse

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:
conGeomMust be a line

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:
conGeomMust be a line

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:
dimObject1Should be an arc
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL

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:
dimObject1Should be an arc
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL
refDimoption for creating driving or reference dimension

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:
dimTypeMust be one of the dimension types and should not be a radial, diametral, or perimeter dimension
dimObject1First input geometry
dimObject2Second input geometry
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL

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:
dimTypeMust be one of the dimension types and should not be a radial, diametral, or perimeter dimension
dimObject1First input geometry
dimObject2Second input geometry
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL
refDimoption for creating driving or reference dimension

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:
conGeom1Must be a line or linear edge
conGeom2Must be a line or linear edge

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:
conGeom1Must be an arc or edge shaped as an arc
conGeom2Must be an arc or edge shaped as an arc

Creates a fixed constraint.

Returns:
The fixed constraint
Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
Parameters:
geomCan be any curve, point, or vertex in the sketch

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:
geomCan be any curve, point, or vertex in the sketch

Creates a horizontal constraint.

Returns:
The horizontal constraint
Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
Parameters:
geomMust be a line

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



License requirements : None

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:
conGeom1con geom1
conGeom2con geom2

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:
conGeomMust be a spline

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:
conGeom1First input geometry for the constraint
geom1HelpHelp data for first geom
conGeom2Second input geometry for the constraint
geom2HelpHelp data for second geom

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:
conGeom1First input geometry for the constraint
conGeom2Second 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:
curvesThe curves that form the perimeter
dimOriginNot currently used
expressionDefining expression for the dimension. Can be NULL

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:
conGeom1First input geometry for the constraint
conGeom2Second input geometry for the constraint

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:
conGeom1con geom1
conGeom2con geom2
helphelp
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.

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

License requirements : solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
Parameters:
conGeom1Must be a vertex
curvesInStringMust all be part of the same string. (You can create a string of curves through the UI through the Edit -> Project command.)
helpDatahelp data
curveWhichHelpParamAppliesToIf helpData is a parameter, this parameter indicates which curve in the curvesInString that the help parameter applies to. Otherwise, this parameter is not used

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:
conGeom1Must be a vertex
curveInStringA 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.)
helpDatahelp data

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:
dimObject1Should be an arc
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL

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:
dimObject1Should be an arc
dimOriginThe location where the dimension should be placed
expressionDefining expression for the dimension. Can be NULL
refDimoption for creating driving or reference dimension

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:
conGeom1con geom1
conGeom2con geom2

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:
geom1A curve, edge, or datum axis
geom1Helpgeom1 help
geom2A curve, edge, or datum axis
geom2Helpgeom2 help

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:
conGeomMust be a spline

Creates a vertical constraint.

Returns:
The vertical constraint
Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
Parameters:
geomMust be a line

Deactivates the sketch
Created in NX3.0.0.



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

Parameters:
orientViewIndicates whether to orient the view to the model during deactivation
updateLevelIndicates 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:
objectsObjects 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:
objectsObjects to be deleted

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



License requirements : None

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:
curve1First curve for the fillet
curve2Second curve for the fillet
helpPoint1Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2Should be a point on the second curve. Indicates where the fillet should be created
radiusRadius of the fillet
doTrimIndicates whether the input curves should get trimmed by the fillet
createRadiusDimIndicates whether a radius dimension should be created
alternateSolutionIndicates 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.
constraintsThe 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:
curve1First curve for the fillet
curve2Second curve for the fillet
helpPoint1Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2Should be a point on the second curve. Indicates where the fillet should be created
pointOnArcPoint on fillet arc
radiusRadius of the fillet
doTrimIndicates whether the input curves should get trimmed by the fillet
createRadiusDimIndicates whether a radius dimension should be created
alternateSolutionIndicates 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.
constraintsThe 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:
curve1First curve for the fillet
curve2Second curve for the fillet
curve3Third curve for the fillet
helpPoint1Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2Should be a point on the second curve. Indicates where the fillet should be created
helpPoint3Should be a point on the third curve. Indicates where the fillet should be created
radiusRadius of the fillet
doTrimIndicates whether the input curves should get trimmed by the fillet
doDeleteIndicates whether the third curve should be deleted
createRadiusDimIndicates whether a radius dimension should be created
alternateSolutionIndicates 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.
constraintsThe 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:
curve1First curve for the fillet
curve2Second curve for the fillet
curve3Third curve for the fillet
helpPoint1Should be a point on the first curve. Indicates where the fillet should be created
helpPoint2Should be a point on the second curve. Indicates where the fillet should be created
helpPoint3Should be a point on the third curve. Indicates where the fillet should be created
pointOnArcPoint on fillet arc
radiusRadius of the fillet
doTrimIndicates whether the input curves should get trimmed by the fillet
doDeleteIndicates whether the third curve should be deleted
createRadiusDimIndicates whether a radius dimension should be created
alternateSolutionIndicates 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.
constraintsThe 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.

Flips the outward normal vector of the sketch
Created in NX3.0.0.



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

Flips the reference direction of the sketch
Created in NX3.0.0.



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

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:
conClassOptional filter. Use Sketch::ConstraintClassAny if you do not want to filter by constraint class
conTypeOptional filter. Use Sketch::ConstraintTypeNoCon if you do not want to filter by constraint type

Returns all the expressions in the sketch.

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

License requirements : None

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

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:
geometryMust be a curve or point
conClassOptional 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:
referenceAxisAn edge, datum axis, datum plane, or face that the sketch uses as a reference. May be NULL.
referenceAxisOrientationIndicates whether the reference axis is horizontal or vertical
referenceAxisSenseIf 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.

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:
dofNeededThe 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:
inputObjectsGeometry and groups in active sketch

Blanks all the dimensions of input sketch
Created in NX6.0.1.



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

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



License requirements : None

Returns true if drafting sketch
Created in NX6.0.0.



License requirements : None

Returns true if the sketch is internal.


Created in NX6.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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")

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


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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.


This API is now deprecated. Please use SketchMirrorBuilder instead.

Returns:
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:
centerlineAxis of reflection for the mirror. Must be a linear curve, edge, datum axis or datum plane
objectsToMirrorPoints and curves to mirror. None of the curves may be used as a centerline for another mirror operation

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



License requirements : None

Returns the location of the origin of the local coordinate system for the sketch
Created in NX3.0.0.



License requirements : None

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:
attachmentPlaneattachment plane
referenceAxisreference axis
referenceDirectionreference direction
referenceAxisOrientationreference axis orientation
referenceAxisSensereference axis sense
normalOrientationnormal orientation
localCoordinateSystemOriginOrigin of the sketch's local coordinate system

Run auto dimensioning.


Created in NX7.5.0.

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

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:
createInferConcreate 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:
displayDofdisplay 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:
referenceAxisreference axis
referenceDirectionreference direction
referenceAxisOrientationreference axis orientation
referenceAxisSensereference axis sense

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:
updateScopeupdate scope

Sets the visibility of the constraints in the sketch
Created in NX3.0.0.



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

Parameters:
visibilityvisibility
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:
inputObjectsGeometry and groups in active sketch

Unblanks all the dimensions of input sketch
Created in NX6.0.1.



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

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:
geomsGeoms that need to be updated

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:
geomsGeoms for which cons must be re-displayed

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:
geomsGeoms 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:
dimsDims for which cons must be re-displayed

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:
geomsGeoms for which cons must be re-displayed

Returns the current update scope.

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

License requirements : None

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



License requirements : None

Returns the visibility of the constraints in the sketch
Created in NX3.0.0.



License requirements : None


The documentation for this class was generated from the following file:
Copyright 2011 Siemens Product Lifecycle Management Software Inc. All Rights Reserved.