public interface Sketch extends DisplayableObject, IProfile
Modifier and Type | Interface and Description |
---|---|
static class |
Sketch.AddEllipseOption
Used by
addGeometry(nxopen.DisplayableObject, nxopen.Sketch.InferConstraintsOption) to determine whether to treat an
ellipse as an ellipse or generic conic when adding the curve to
a sketch. |
static class |
Sketch.AlternateSolutionOption
Indicates whether the alternate solution should be used instead of the regular solution.
|
static class |
Sketch.AssocType
Used in
Sketch.DimensionGeometry to indicate what type of
geometry to use |
static class |
Sketch.AutoDimensioningRule
Type of Auto Dimensioning rules.
|
static class |
Sketch.ConstraintClass
Represents the class of the constraint.
|
static class |
Sketch.ConstraintGeometry
Used by the create geometric constraint methods to indicate what geometry
the constraint should be applied to.
|
static class |
Sketch.ConstraintGeometryHelp
Used by several constraint creation methods that need a help point or parameter
to indicate how to create the constraint.
|
static class |
Sketch.ConstraintGeometryHelpType
Used in ConstraintHelp to indicate what type of help it is
|
static class |
Sketch.ConstraintPointType
Used in ConstraintGeometry to indicate what type of point, if any, the geometry is
|
static class |
Sketch.ConstraintType
Represents the type of constraint
|
static class |
Sketch.ConstraintVisibility
Deprecated.
Deprecated in NX8.5.0. Please use
SessionSketch.displayConstraintSymbols() and SessionSketch.setDisplayConstraintSymbols(boolean)
|
static class |
Sketch.CopyObjectData
This structure represents a map between the original object to be copied
and the corresponding copied object.
|
static class |
Sketch.CopyObjectsWithDimensionOutputData
This class holds the data returned from
copyObjectsWithDimensionOutput(nxopen.NXObject[]) |
static class |
Sketch.CreateDimensionOption
Used in fillet to indicate whether a radius dimension should be created
by the fillet
|
static class |
Sketch.CreateInferConstraintSetting
Indicates if the infer constraints will be created or not
|
static class |
Sketch.DeleteThirdCurveOption
Indicates whether the 3rd curve should be deleted when doing a 3 curve fillet
|
static class |
Sketch.DimensionGeometry
Used in the dimension creation methods to indicate what geometry to
create the dimension on.
|
static class |
Sketch.DimensionOption
Used by
createDimension(nxopen.Sketch.ConstraintType, nxopen.Sketch.DimensionGeometry, nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression) , createRadialDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression)
createDiameterDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression) and createPerimeterDimension(nxopen.Curve[], nxopen.Point3d, nxopen.Expression)
to determine whether to create driving or reference dimension |
static class |
Sketch.FilletData
|
static class |
Sketch.InferConstraintsOption
Used when adding a point or curve to a sketch.
|
static class |
Sketch.PlaneOption
Specifies the plane type used for a Sketch
|
static class |
Sketch.ReferenceDirectionData
This class holds the data returned from
getReferenceDirection() |
static class |
Sketch.Status
Represents the status of the sketch
|
static class |
Sketch.StatusData
This class holds the data returned from
getStatus() |
static class |
Sketch.TrimInputOption
Indicates whether the input curves should be trimmed when doing a fillet
|
static class |
Sketch.UpdateLevel
Used to indicate how much the updating should occur
|
static class |
Sketch.ViewReorient
Used to indicate whether to reorient the view when the sketch is activated
|
DisplayableObject.ObjectFont, DisplayableObject.ObjectWidth
NXObject.AttributeInformation, NXObject.AttributeType, NXObject.ComputationalTime, NXObject.DateAndTimeFormat
Modifier and Type | Method and Description |
---|---|
void |
activate(Sketch.ViewReorient orientView)
Activates the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
addGeometry(Curve crv,
Sketch.InferConstraintsOption inferCoincidentConstraints,
Sketch.AddEllipseOption ellipseOption)
Adds a curve or point to a sketch.
|
void |
addGeometry(DisplayableObject crv)
Adds a curve or point to the sketch.
|
void |
addGeometry(DisplayableObject crv,
Sketch.InferConstraintsOption inferCoincidentConstraints)
Adds a curve or point to the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
addGeometry(Sketch.InferConstraintsOption inferCoincidentConstraints,
Sketch.AddEllipseOption ellipseOption,
SmartObject[] curvesOrPoints)
Adds an array of curves or points to a sketch.
|
ISurface |
attachPlane()
Returns the plane that the sketch is attached to
License requirements: None. |
SketchConstraint[] |
autoConstrain(double linearTolerance,
double angularTolerance,
boolean allowRemoteConstraints,
SmartObject[] geometries,
Sketch.ConstraintType[] autoconstraintTypes)
Creates Automatic Constraints on input set of geometries.
|
void |
convertToNx10Spline(Spline spline)
Convert the legacy splines to new NX10 splines.
|
NXObject[] |
copyObjects(NXObject[] inputObjects)
Creates copies of input objects and constraints between these objects.
|
Sketch.CopyObjectsWithDimensionOutputData |
copyObjectsWithDimensionOutput(NXObject[] inputObjects)
Creates copies of input objects and constraints between these objects.
|
Sketch.CopyObjectData[] |
copyObjectsWithTracking(DisplayableObject[] inputObjects)
Creates copies of input objects and constraints between these objects.
|
SketchGeometricConstraint |
createCoincidentConstraint(Sketch.ConstraintGeometry geom1,
Sketch.ConstraintGeometry geom2)
Creates a coincident constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint |
createCollinearConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a collinear constraint.
|
SketchGeometricConstraint |
createConcentricConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a concentric constraint.
|
SketchGeometricConstraint |
createConstantAngleConstraint(Sketch.ConstraintGeometry conGeom)
Creates a constant angle constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint |
createConstantLengthConstraint(Sketch.ConstraintGeometry conGeom)
Creates a constant length constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchDimensionalConstraint |
createDiameterDimension(Sketch.DimensionGeometry dimObject1,
Point3d dimOrigin,
Expression expression)
Creates a diameter dimension constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchDimensionalConstraint |
createDiameterDimension(Sketch.DimensionGeometry dimObject1,
Point3d dimOrigin,
Expression expression,
Sketch.DimensionOption refDim)
Creates a diameter dimension constraint.
|
SketchDimensionalConstraint |
createDimension(Sketch.ConstraintType dimType,
Sketch.DimensionGeometry dimObject1,
Sketch.DimensionGeometry dimObject2,
Point3d dimOrigin,
Expression expression)
Creates a dimension between two geometric objects.
|
SketchDimensionalConstraint |
createDimension(Sketch.ConstraintType dimType,
Sketch.DimensionGeometry dimObject1,
Sketch.DimensionGeometry dimObject2,
Point3d dimOrigin,
Expression expression,
Sketch.DimensionOption refDim)
Creates a dimension between two geometric objects.
|
SketchGeometricConstraint |
createEqualLengthConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates an equal length constraint.
|
SketchGeometricConstraint |
createEqualRadiusConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates an equal radius constraint.
|
SketchGeometricConstraint |
createFixedConstraint(Sketch.ConstraintGeometry geom)
Creates a fixed constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint[] |
createFullyFixedConstraints(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.
|
SketchGeometricConstraint |
createHorizontalConstraint(Sketch.ConstraintGeometry geom)
Creates a horizontal constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
Sketch.CreateInferConstraintSetting |
createInferConstraintsSetting()
Returns the toggle that controls the creation of infer constraints in sketch
License requirements: None. |
SketchGeometricConstraint |
createMidpointConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a midpoint constraint.
|
SketchGeometricConstraint |
createNonUniformScaledConstraint(Sketch.ConstraintGeometry conGeom)
Creates a non-uniform scale constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint |
createNormalConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometryHelp geom1Help,
Sketch.ConstraintGeometry conGeom2,
Sketch.ConstraintGeometryHelp geom2Help)
Creates a normal constraint.
|
SketchGeometricConstraint |
createParallelConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a parallel constraint.
|
SketchDimensionalConstraint |
createPerimeterDimension(Curve[] curves,
Point3d dimOrigin,
Expression expression)
Creates a perimeter dimension constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint |
createPerpendicularConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a perpendicular constraint.
|
SketchHelpedGeometricConstraint |
createPointOnCurveConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2,
Sketch.ConstraintGeometryHelp help)
Creates a point on curve constraint.
|
SketchHelpedGeometricConstraint |
createPointOnStringConstraint(Sketch.ConstraintGeometry conGeom1,
Curve[] curvesInString,
Sketch.ConstraintGeometryHelp helpData,
int curveWhichHelpParamAppliesTo)
Creates a point on string constraint.
|
SketchHelpedGeometricConstraint |
createPointOnStringConstraint(Sketch.ConstraintGeometry conGeom1,
Curve curveInString,
Sketch.ConstraintGeometryHelp helpData)
Creates a point on string constraint.
|
SketchDimensionalConstraint |
createRadialDimension(Sketch.DimensionGeometry dimObject1,
Point3d dimOrigin,
Expression expression)
Creates a radial dimension constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchDimensionalConstraint |
createRadialDimension(Sketch.DimensionGeometry dimObject1,
Point3d dimOrigin,
Expression expression,
Sketch.DimensionOption refDim)
Creates a radial dimension constraint.
|
SketchGeometricConstraint |
createSlopeConstraint(Sketch.ConstraintGeometry conGeom1,
Sketch.ConstraintGeometry conGeom2)
Creates a slope constraint.
|
SketchTangentConstraint |
createTangentConstraint(Sketch.ConstraintGeometry geom1,
Sketch.ConstraintGeometryHelp geom1Help,
Sketch.ConstraintGeometry geom2,
Sketch.ConstraintGeometryHelp geom2Help)
Creates a tangent constraint.
|
SketchGeometricConstraint |
createUniformScaledConstraint(Sketch.ConstraintGeometry conGeom)
Creates a uniform scale constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchGeometricConstraint |
createVerticalConstraint(Sketch.ConstraintGeometry geom)
Creates a vertical constraint
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
deactivate(Sketch.ViewReorient orientView,
Sketch.UpdateLevel updateLevel)
Deactivates the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
deleteConstraintsOnGeometries(NXObject[] objects)
Deletes all geometric constraints associated with the object and all of its
vertices.
|
void |
deleteConstraintsOnGeometries(Sketch.ConstraintGeometry[] objects)
Deletes all geometric constraints associated with the object and all of its vertices.
|
ErrorList |
deleteObjects(NXObject[] objects)
Deletes objects from the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
boolean |
dofdisplay()
Returns a flag indicating whether the degree of freedom arrows are currently being
displayed
License requirements: None. |
void |
editSplineDefiningPoints(Spline spline,
double[] points)
Changes the locations of the defining points of a spline.
|
void |
editSplinePoles(Spline spline,
double[] poles)
Changes the locations of the control poles of a spline.
|
nxopen.features.Feature |
feature()
Returns the feature associated with this sketch
License requirements: None. |
Sketch.FilletData |
fillet(Curve curve1,
Curve curve2,
Curve curve3,
Point3d helpPoint1,
Point3d helpPoint2,
Point3d helpPoint3,
double radius,
Sketch.TrimInputOption doTrim,
Sketch.DeleteThirdCurveOption doDelete,
Sketch.CreateDimensionOption createRadiusDim,
Sketch.AlternateSolutionOption alternateSolution)
Fillets curves and creates appropriate constraints.
|
Sketch.FilletData |
fillet(Curve curve1,
Curve curve2,
Curve curve3,
Point3d helpPoint1,
Point3d helpPoint2,
Point3d helpPoint3,
Point3d pointOnArc,
double radius,
Sketch.TrimInputOption doTrim,
Sketch.DeleteThirdCurveOption doDelete,
Sketch.CreateDimensionOption createRadiusDim,
Sketch.AlternateSolutionOption alternateSolution)
Fillets curves and creates appropriate constraints.
|
Sketch.FilletData |
fillet(Curve curve1,
Curve curve2,
Point3d helpPoint1,
Point3d helpPoint2,
double radius,
Sketch.TrimInputOption doTrim,
Sketch.CreateDimensionOption createRadiusDim,
Sketch.AlternateSolutionOption alternateSolution)
Fillets curves and creates appropriate constraints.
|
Sketch.FilletData |
fillet(Curve curve1,
Curve curve2,
Point3d helpPoint1,
Point3d helpPoint2,
Point3d pointOnArc,
double radius,
Sketch.TrimInputOption doTrim,
Sketch.CreateDimensionOption createRadiusDim,
Sketch.AlternateSolutionOption alternateSolution)
Fillets curves and creates appropriate constraints.
|
void |
flipNormal()
Flips the outward normal vector of the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
flipReferenceDirection()
Flips the reference direction of the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
SketchConstraint[] |
getAllConstraintsOfType(Sketch.ConstraintClass conClass,
Sketch.ConstraintType conType)
Gets all constraints in the sketch of a particular type
License requirements: None. |
Expression[] |
getAllExpressions()
Returns all the expressions in the sketch
License requirements: None. |
NXObject[] |
getAllGeometry()
Returns all the curves and points in the sketch
License requirements: None. |
SketchConstraint[] |
getConstraintsForGeometry(SmartObject geometry,
Sketch.ConstraintClass conClass)
Gets all the constraints associated with a particular geometric item
License requirements: None. |
Sketch.ReferenceDirectionData |
getReferenceDirection()
Gets the reference direction of the sketch
License requirements: None. |
Sketch.StatusData |
getStatus()
Gets the status of the sketch and the number of degrees of freedom that remain in the sketch.
|
void |
hideDimensions()
Blanks all the dimensions of input sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
hideDimensions(DisplayableObject[] inputObjects)
Blanks dimensions in the active sketch associated with the input sketch geometry.
|
void |
hideDimensions(Sketch.ConstraintGeometry[] objects)
Blanks dimensions in the active sketch associated with the input sketch geometry.
|
boolean |
isActive()
Returns true if the sketch is active
License requirements: None. |
boolean |
isDraftingSketch()
Returns true if drafting sketch
License requirements: None. |
boolean |
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.
|
SmartObject[] |
mirrorObjects(DisplayableObject centerline,
SmartObject[] objectsToMirror)
Deprecated.
Deprecated in NX5.0.0. Please use
SketchMirrorBuilder instead.
|
NXMatrix |
orientation()
Returns the orientation matrix of the local coordinate system of the sketch
License requirements: None. |
Point3d |
origin()
Returns the location of the origin of the local coordinate system for the sketch
License requirements: None. |
SketchPreferences |
preferences()
Contains preferences for the sketch .
|
void |
reattach(ISurface attachmentPlane,
IReferenceAxis referenceAxis,
Vector3d referenceDirection,
AxisOrientation referenceAxisOrientation,
Sense referenceAxisSense,
PlaneNormalOrientation normalOrientation,
Point3d localCoordinateSystemOrigin)
Reattaches a sketch.
|
void |
runAutoDimension()
Run auto dimensioning.
|
void |
setCreateInferConstraintsSetting(Sketch.CreateInferConstraintSetting createInferCon)
Sets the toggle that controls the creation of infer constraints in sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
setDOFDisplay(boolean displayDof)
Sets a flag indicating whether the degree of freedom arrows are currently being
displayed
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
setReferenceDirection(IReferenceAxis referenceAxis,
Vector3d referenceDirection,
AxisOrientation referenceAxisOrientation,
Sense referenceAxisSense)
Sets the reference direction of the sketch.
|
void |
setUpdateScope(Sketch.UpdateLevel updateScope)
Sets the current update scope.
|
void |
setVisibilityOfConstraints(Sketch.ConstraintVisibility visibility)
Deprecated.
Deprecated in NX8.5.0. Use
SessionSketch.setDisplayConstraintSymbols(boolean) instead.
|
void |
showDimensions()
Unblanks all the dimensions of input sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
showDimensions(DisplayableObject[] inputObjects)
Unblanks dimensions in the active sketch associated with the input sketch geometry
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
showDimensions(Sketch.ConstraintGeometry[] objects)
Unblanks dimensions in the active sketch associated with the input sketch geometry.
|
void |
update()
Updates the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
update(NXObject[] geoms)
Updates the given set of geometries in the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateConstraintDisplay()
Updates the constraint display without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateConstraintDisplay(SmartObject[] geoms)
Updates the constraint display of given set of geoms without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateDimensionDisplay()
Updates the dimension display without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateDimensionDisplay(NXObject[] dims)
Updates the dimension display of given set of dims without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") . |
void |
updateDimensionDisplay(SmartObject[] geoms)
Updates the dimension display of given set of geoms without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateGeometryDisplay()
Updates the geometry display without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
void |
updateGeometryDisplay(SmartObject[] geoms)
Updates the geometry display of given set of geoms without updating the sketch
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT") . |
Sketch.UpdateLevel |
updateScope()
Returns the current update scope.
|
View |
view()
Returns the view corresponding to sketch
License requirements: None. |
Sketch.ConstraintVisibility |
visibilityOfConstraints()
Deprecated.
Deprecated in NX8.5.0. Use
SessionSketch.displayConstraintSymbols() instead.
|
blank, color, highlight, isBlanked, layer, lineFont, lineWidth, nameLocation, redisplayObject, removeViewDependency, setColor, setLayer, setLineFont, setLineWidth, setNameLocation, unblank, unhighlight
deleteAllAttributesByType, deleteAllAttributesByType, deleteAttributeByTypeAndTitle, deleteAttributeByTypeAndTitle, deleteUserAttribute, deleteUserAttributes, getAttributeTitlesByType, getBooleanUserAttribute, getComputationalTimeUserAttribute, getIntegerAttribute, getIntegerUserAttribute, getRealAttribute, getRealUserAttribute, getReferenceAttribute, getStringAttribute, getStringUserAttribute, getTimeAttribute, getTimeUserAttribute, getUserAttribute, getUserAttribute, getUserAttributeAsString, getUserAttributeCount, getUserAttributeCount, getUserAttributeLock, getUserAttributes, getUserAttributes, getUserAttributes, getUserAttributesAsStrings, getUserAttributeSize, getUserAttributeSourceObjects, hasUserAttribute, setAttribute, setAttribute, setAttribute, setAttribute, setAttribute, setAttribute, setAttribute, setAttribute, setBooleanUserAttribute, setReferenceAttribute, setReferenceAttribute, setTimeAttribute, setTimeAttribute, setTimeUserAttribute, setTimeUserAttribute, setUserAttribute, setUserAttribute, setUserAttribute, setUserAttribute, setUserAttribute, setUserAttributeLock
printTestData, printTestData, tag, tagValue
findObject, isOccurrence, journalIdentifier, name, owningComponent, owningPart, print, prototype, setName
SketchPreferences preferences() throws RemoteException
RemoteException
ErrorList deleteObjects(NXObject[] objects) throws NXException, RemoteException
objects
- Objects to be deletedNXException
RemoteException
void reattach(ISurface attachmentPlane, IReferenceAxis referenceAxis, Vector3d referenceDirection, AxisOrientation referenceAxisOrientation, Sense referenceAxisSense, PlaneNormalOrientation normalOrientation, Point3d localCoordinateSystemOrigin) throws NXException, RemoteException
SketchCollection.createSketch(java.lang.String, nxopen.ISurface, IReferenceAxis, nxopen.Vector3d, nxopen.AxisOrientation, nxopen.Sense, nxopen.PlaneNormalOrientation)
attachmentPlane
- referenceAxis
- referenceDirection
- referenceAxisOrientation
- referenceAxisSense
- normalOrientation
- localCoordinateSystemOrigin
- Origin of the sketch's local coordinate systemNXException
RemoteException
void activate(Sketch.ViewReorient orientView) throws NXException, RemoteException
orientView
- Indicates whether to orient the view to the sketch during activationNXException
RemoteException
void deactivate(Sketch.ViewReorient orientView, Sketch.UpdateLevel updateLevel) throws NXException, RemoteException
orientView
- Indicates whether to orient the view to the model during deactivationupdateLevel
- Indicates whether just the sketch should be updated or the entire modelNXException
RemoteException
boolean isActive() throws NXException, RemoteException
NXException
RemoteException
void setReferenceDirection(IReferenceAxis referenceAxis, Vector3d referenceDirection, AxisOrientation referenceAxisOrientation, Sense referenceAxisSense) throws NXException, RemoteException
SketchCollection.createSketch(java.lang.String, nxopen.ISurface, IReferenceAxis, nxopen.Vector3d, nxopen.AxisOrientation, nxopen.Sense, nxopen.PlaneNormalOrientation)
.
referenceAxis
- referenceDirection
- referenceAxisOrientation
- referenceAxisSense
- NXException
RemoteException
void flipReferenceDirection() throws NXException, RemoteException
NXException
RemoteException
void flipNormal() throws NXException, RemoteException
NXException
RemoteException
ISurface attachPlane() throws NXException, RemoteException
NXException
RemoteException
Sketch.ReferenceDirectionData getReferenceDirection() throws NXException, RemoteException
NXException
RemoteException
Point3d origin() throws NXException, RemoteException
NXException
RemoteException
NXMatrix orientation() throws NXException, RemoteException
NXException
RemoteException
Sketch.ConstraintVisibility visibilityOfConstraints() throws NXException, RemoteException
SessionSketch.displayConstraintSymbols()
instead.
NXException
RemoteException
void setVisibilityOfConstraints(Sketch.ConstraintVisibility visibility) throws NXException, RemoteException
SessionSketch.setDisplayConstraintSymbols(boolean)
instead.
visibility
- NXException
RemoteException
Sketch.CreateInferConstraintSetting createInferConstraintsSetting() throws NXException, RemoteException
NXException
RemoteException
void setCreateInferConstraintsSetting(Sketch.CreateInferConstraintSetting createInferCon) throws NXException, RemoteException
createInferCon
- NXException
RemoteException
void runAutoDimension() throws NXException, RemoteException
NXException
RemoteException
SketchGeometricConstraint createCoincidentConstraint(Sketch.ConstraintGeometry geom1, Sketch.ConstraintGeometry geom2) throws NXException, RemoteException
geom1
- Must be a vertexgeom2
- Must be a vertexNXException
RemoteException
SketchGeometricConstraint createFixedConstraint(Sketch.ConstraintGeometry geom) throws NXException, RemoteException
geom
- Can be any curve, point, or vertex in the sketchNXException
RemoteException
SketchGeometricConstraint[] createFullyFixedConstraints(Sketch.ConstraintGeometry geom) throws NXException, RemoteException
geom
- Can be any curve, point, or vertex in the sketchNXException
RemoteException
SketchGeometricConstraint createHorizontalConstraint(Sketch.ConstraintGeometry geom) throws NXException, RemoteException
geom
- Must be a lineNXException
RemoteException
SketchGeometricConstraint createVerticalConstraint(Sketch.ConstraintGeometry geom) throws NXException, RemoteException
geom
- Must be a lineNXException
RemoteException
SketchTangentConstraint createTangentConstraint(Sketch.ConstraintGeometry geom1, Sketch.ConstraintGeometryHelp geom1Help, Sketch.ConstraintGeometry geom2, Sketch.ConstraintGeometryHelp geom2Help) throws NXException, RemoteException
geom1
- A curve, edge, or datum axisgeom1Help
- geom2
- A curve, edge, or datum axisgeom2Help
- NXException
RemoteException
SketchGeometricConstraint createConstantLengthConstraint(Sketch.ConstraintGeometry conGeom) throws NXException, RemoteException
conGeom
- Must be a lineNXException
RemoteException
SketchGeometricConstraint createConstantAngleConstraint(Sketch.ConstraintGeometry conGeom) throws NXException, RemoteException
conGeom
- Must be a lineNXException
RemoteException
SketchGeometricConstraint createUniformScaledConstraint(Sketch.ConstraintGeometry conGeom) throws NXException, RemoteException
conGeom
- Must be a splineNXException
RemoteException
SketchGeometricConstraint createNonUniformScaledConstraint(Sketch.ConstraintGeometry conGeom) throws NXException, RemoteException
conGeom
- Must be a splineNXException
RemoteException
SketchGeometricConstraint createParallelConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- First input geometry for the constraintconGeom2
- Second input geometry for the constraintNXException
RemoteException
SketchGeometricConstraint createPerpendicularConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- First input geometry for the constraintconGeom2
- Second input geometry for the constraintNXException
RemoteException
SketchGeometricConstraint createNormalConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometryHelp geom1Help, Sketch.ConstraintGeometry conGeom2, Sketch.ConstraintGeometryHelp geom2Help) throws NXException, RemoteException
conGeom1
- First input geometry for the constraintgeom1Help
- Help data for first geomconGeom2
- Second input geometry for the constraintgeom2Help
- Help data for second geomNXException
RemoteException
SketchGeometricConstraint createCollinearConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- Must be a line, linear edge, datum axis, or datum planeconGeom2
- Must be a line, linear edge, datum axis, or datum planeNXException
RemoteException
SketchGeometricConstraint createEqualLengthConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- Must be a line or linear edgeconGeom2
- Must be a line or linear edgeNXException
RemoteException
SketchGeometricConstraint createEqualRadiusConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- Must be an arc or edge shaped as an arcconGeom2
- Must be an arc or edge shaped as an arcNXException
RemoteException
SketchGeometricConstraint createConcentricConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- Must be an arc or ellipse or edge shaped as an arc or ellipseconGeom2
- Must be an arc or ellipse or edge shaped as an arc or ellipseNXException
RemoteException
SketchGeometricConstraint createMidpointConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- conGeom2
- NXException
RemoteException
SketchGeometricConstraint createSlopeConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2) throws NXException, RemoteException
conGeom1
- conGeom2
- NXException
RemoteException
SketchHelpedGeometricConstraint createPointOnCurveConstraint(Sketch.ConstraintGeometry conGeom1, Sketch.ConstraintGeometry conGeom2, Sketch.ConstraintGeometryHelp help) throws NXException, RemoteException
conGeom1
- conGeom2
- help
- NXException
RemoteException
SketchHelpedGeometricConstraint createPointOnStringConstraint(Sketch.ConstraintGeometry conGeom1, Curve[] curvesInString, Sketch.ConstraintGeometryHelp helpData, int curveWhichHelpParamAppliesTo) throws NXException, RemoteException
conGeom1
- Must be a vertexcurvesInString
- Must all be part of the same string.
(You can create a string of curves through the UI
through the Edit -> Project command.)helpData
- curveWhichHelpParamAppliesTo
- If helpData is a parameter, this parameter indicates
which curve in the curvesInString that the help parameter applies to. Otherwise, this parameter is not usedNXException
RemoteException
SketchHelpedGeometricConstraint createPointOnStringConstraint(Sketch.ConstraintGeometry conGeom1, Curve curveInString, Sketch.ConstraintGeometryHelp helpData) throws NXException, RemoteException
conGeom1
- Must be a vertexcurveInString
- 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
- NXException
RemoteException
SketchDimensionalConstraint createDimension(Sketch.ConstraintType dimType, Sketch.DimensionGeometry dimObject1, Sketch.DimensionGeometry dimObject2, Point3d dimOrigin, Expression expression) throws NXException, RemoteException
createRadialDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression)
or createDiameterDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression)
.
To create a perimeter dimension, use createPerimeterDimension(nxopen.Curve[], nxopen.Point3d, nxopen.Expression)
dimType
- Must be one of the dimension types and should not
be a radial, diametral, or perimeter dimensiondimObject1
- First input geometrydimObject2
- Second input geometrydimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullNXException
RemoteException
SketchDimensionalConstraint createDimension(Sketch.ConstraintType dimType, Sketch.DimensionGeometry dimObject1, Sketch.DimensionGeometry dimObject2, Point3d dimOrigin, Expression expression, Sketch.DimensionOption refDim) throws NXException, RemoteException
createRadialDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression)
or createDiameterDimension(nxopen.Sketch.DimensionGeometry, nxopen.Point3d, nxopen.Expression)
.
To create a perimeter dimension, use createPerimeterDimension(nxopen.Curve[], nxopen.Point3d, nxopen.Expression)
. This function
takes in an argument to create the dimension as driving or reference.
dimType
- Must be one of the dimension types and should not
be a radial, diametral, or perimeter dimensiondimObject1
- First input geometrydimObject2
- Second input geometrydimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullrefDim
- option for creating driving or reference dimensionNXException
RemoteException
SketchDimensionalConstraint createRadialDimension(Sketch.DimensionGeometry dimObject1, Point3d dimOrigin, Expression expression) throws NXException, RemoteException
dimObject1
- Should be an arcdimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullNXException
RemoteException
SketchDimensionalConstraint createRadialDimension(Sketch.DimensionGeometry dimObject1, Point3d dimOrigin, Expression expression, Sketch.DimensionOption refDim) throws NXException, RemoteException
dimObject1
- Should be an arcdimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullrefDim
- option for creating driving or reference dimensionNXException
RemoteException
SketchDimensionalConstraint createDiameterDimension(Sketch.DimensionGeometry dimObject1, Point3d dimOrigin, Expression expression) throws NXException, RemoteException
dimObject1
- Should be an arcdimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullNXException
RemoteException
SketchDimensionalConstraint createDiameterDimension(Sketch.DimensionGeometry dimObject1, Point3d dimOrigin, Expression expression, Sketch.DimensionOption refDim) throws NXException, RemoteException
dimObject1
- Should be an arcdimOrigin
- The location where the dimension should be placedexpression
- Defining expression for the dimension. Can be nullrefDim
- option for creating driving or reference dimensionNXException
RemoteException
SketchDimensionalConstraint createPerimeterDimension(Curve[] curves, Point3d dimOrigin, Expression expression) throws NXException, RemoteException
curves
- The curves that form the perimeterdimOrigin
- Not currently usedexpression
- Defining expression for the dimension. Can be nullNXException
RemoteException
void localUpdate() throws NXException, RemoteException
NXException
RemoteException
void update() throws NXException, RemoteException
NXException
RemoteException
void update(NXObject[] geoms) throws NXException, RemoteException
geoms
- Geoms that need to be updatedNXException
RemoteException
void updateGeometryDisplay() throws NXException, RemoteException
NXException
RemoteException
void updateGeometryDisplay(SmartObject[] geoms) throws NXException, RemoteException
geoms
- Geoms for which cons must be re-displayedNXException
RemoteException
void updateDimensionDisplay() throws NXException, RemoteException
NXException
RemoteException
void updateDimensionDisplay(SmartObject[] geoms) throws NXException, RemoteException
geoms
- Geoms for which cons must be re-displayedNXException
RemoteException
void updateDimensionDisplay(NXObject[] dims) throws NXException, RemoteException
dims
- Dims for which cons must be re-displayedNXException
RemoteException
void updateConstraintDisplay() throws NXException, RemoteException
NXException
RemoteException
void updateConstraintDisplay(SmartObject[] geoms) throws NXException, RemoteException
geoms
- Geoms for which cons must be re-displayedNXException
RemoteException
void addGeometry(DisplayableObject crv, Sketch.InferConstraintsOption inferCoincidentConstraints) throws NXException, RemoteException
crv
- Must be a curve or pointinferCoincidentConstraints
- 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 createdNXException
RemoteException
void addGeometry(DisplayableObject crv) throws NXException, RemoteException
crv
- Must be a curve or pointNXException
RemoteException
void addGeometry(Curve crv, Sketch.InferConstraintsOption inferCoincidentConstraints, Sketch.AddEllipseOption ellipseOption) throws NXException, RemoteException
crv
- Must be a curve or pointinferCoincidentConstraints
- 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 createdellipseOption
- 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.AddEllipseOption.TREAT_AS_ELLIPSE
.
In order to treat an ellipse as a conic, its end angle minus its
start angle must be less than 180 degrees.NXException
RemoteException
void addGeometry(Sketch.InferConstraintsOption inferCoincidentConstraints, Sketch.AddEllipseOption ellipseOption, SmartObject[] curvesOrPoints) throws NXException, RemoteException
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 createdellipseOption
- 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.AddEllipseOption.TREAT_AS_ELLIPSE
.
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 pointNXException
RemoteException
Sketch.StatusData getStatus() throws NXException, RemoteException
NXException
RemoteException
SketchConstraint[] getAllConstraintsOfType(Sketch.ConstraintClass conClass, Sketch.ConstraintType conType) throws NXException, RemoteException
conClass
- Optional filter. Use Sketch.ConstraintClass.ANY
if you
do not want to filter by constraint classconType
- Optional filter. Use Sketch.ConstraintType.NO_CON
if you
do not want to filter by constraint typeNXException
RemoteException
SketchConstraint[] getConstraintsForGeometry(SmartObject geometry, Sketch.ConstraintClass conClass) throws NXException, RemoteException
geometry
- Must be a curve or pointconClass
- Optional filter. Use Sketch.ConstraintClass.ANY
if you
do not want to filter by constraint classNXException
RemoteException
Expression[] getAllExpressions() throws NXException, RemoteException
NXException
RemoteException
NXObject[] getAllGeometry() throws NXException, RemoteException
NXException
RemoteException
boolean dofdisplay() throws NXException, RemoteException
NXException
RemoteException
void setDOFDisplay(boolean displayDof) throws NXException, RemoteException
displayDof
- NXException
RemoteException
Sketch.FilletData fillet(Curve curve1, Curve curve2, Point3d helpPoint1, Point3d helpPoint2, double radius, Sketch.TrimInputOption doTrim, Sketch.CreateDimensionOption createRadiusDim, Sketch.AlternateSolutionOption alternateSolution) throws NXException, RemoteException
curve1
- First curve for the filletcurve2
- Second curve for the fillethelpPoint1
- Should be a point on the first curve. Indicates where the fillet should be createdhelpPoint2
- Should be a point on the second curve. Indicates where the fillet should be createdradius
- Radius of the filletdoTrim
- Indicates whether the input curves should get trimmed by the filletcreateRadiusDim
- Indicates whether a radius dimension should be createdalternateSolution
- 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.NXException
RemoteException
Sketch.FilletData fillet(Curve curve1, Curve curve2, Point3d helpPoint1, Point3d helpPoint2, Point3d pointOnArc, double radius, Sketch.TrimInputOption doTrim, Sketch.CreateDimensionOption createRadiusDim, Sketch.AlternateSolutionOption alternateSolution) throws NXException, RemoteException
curve1
- First curve for the filletcurve2
- Second curve for the fillethelpPoint1
- Should be a point on the first curve. Indicates where the fillet should be createdhelpPoint2
- Should be a point on the second curve. Indicates where the fillet should be createdpointOnArc
- Point on fillet arcradius
- Radius of the filletdoTrim
- Indicates whether the input curves should get trimmed by the filletcreateRadiusDim
- Indicates whether a radius dimension should be createdalternateSolution
- 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.NXException
RemoteException
Sketch.FilletData fillet(Curve curve1, Curve curve2, Curve curve3, Point3d helpPoint1, Point3d helpPoint2, Point3d helpPoint3, double radius, Sketch.TrimInputOption doTrim, Sketch.DeleteThirdCurveOption doDelete, Sketch.CreateDimensionOption createRadiusDim, Sketch.AlternateSolutionOption alternateSolution) throws NXException, RemoteException
curve1
- First curve for the filletcurve2
- Second curve for the filletcurve3
- Third curve for the fillethelpPoint1
- Should be a point on the first curve. Indicates where the fillet should be createdhelpPoint2
- Should be a point on the second curve. Indicates where the fillet should be createdhelpPoint3
- Should be a point on the third curve. Indicates where the fillet should be createdradius
- Radius of the filletdoTrim
- Indicates whether the input curves should get trimmed by the filletdoDelete
- Indicates whether the third curve should be deletedcreateRadiusDim
- Indicates whether a radius dimension should be createdalternateSolution
- 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.NXException
RemoteException
Sketch.FilletData fillet(Curve curve1, Curve curve2, Curve curve3, Point3d helpPoint1, Point3d helpPoint2, Point3d helpPoint3, Point3d pointOnArc, double radius, Sketch.TrimInputOption doTrim, Sketch.DeleteThirdCurveOption doDelete, Sketch.CreateDimensionOption createRadiusDim, Sketch.AlternateSolutionOption alternateSolution) throws NXException, RemoteException
curve1
- First curve for the filletcurve2
- Second curve for the filletcurve3
- Third curve for the fillethelpPoint1
- Should be a point on the first curve. Indicates where the fillet should be createdhelpPoint2
- Should be a point on the second curve. Indicates where the fillet should be createdhelpPoint3
- Should be a point on the third curve. Indicates where the fillet should be createdpointOnArc
- Point on fillet arcradius
- Radius of the filletdoTrim
- Indicates whether the input curves should get trimmed by the filletdoDelete
- Indicates whether the third curve should be deletedcreateRadiusDim
- Indicates whether a radius dimension should be createdalternateSolution
- 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.NXException
RemoteException
SmartObject[] mirrorObjects(DisplayableObject centerline, SmartObject[] objectsToMirror) throws NXException, RemoteException
SketchMirrorBuilder
instead.
SketchMirrorBuilder
instead.
centerline
- Axis of reflection for the mirror. Must be a linear curve, edge, datum axis or datum planeobjectsToMirror
- Points and curves to mirror. None of the curves may be used as a centerline for another mirror operationNXException
RemoteException
nxopen.features.Feature feature() throws NXException, RemoteException
NXException
RemoteException
View view() throws NXException, RemoteException
NXException
RemoteException
boolean isDraftingSketch() throws NXException, RemoteException
NXException
RemoteException
void deleteConstraintsOnGeometries(NXObject[] objects) throws NXException, RemoteException
objects
- Objects whose constraints needs to be deletedNXException
RemoteException
void deleteConstraintsOnGeometries(Sketch.ConstraintGeometry[] objects) throws NXException, RemoteException
objects
- Objects whose constraints needs to be deletedNXException
RemoteException
NXObject[] copyObjects(NXObject[] inputObjects) throws NXException, RemoteException
inputObjects
- Objects to be copiedNXException
RemoteException
Sketch.CopyObjectsWithDimensionOutputData copyObjectsWithDimensionOutput(NXObject[] inputObjects) throws NXException, RemoteException
copyObjects(nxopen.NXObject[])
except that it returns an array of newly created dimensions
inputObjects
- Objects to be copiedNXException
RemoteException
void showDimensions(DisplayableObject[] inputObjects) throws NXException, RemoteException
inputObjects
- Geometry and groups in active sketchNXException
RemoteException
void hideDimensions(DisplayableObject[] inputObjects) throws NXException, RemoteException
inputObjects
- Geometry and groups in active sketchNXException
RemoteException
void showDimensions() throws NXException, RemoteException
NXException
RemoteException
void showDimensions(Sketch.ConstraintGeometry[] objects) throws NXException, RemoteException
objects
- Geometry and vertices in active sketchNXException
RemoteException
void hideDimensions() throws NXException, RemoteException
NXException
RemoteException
void hideDimensions(Sketch.ConstraintGeometry[] objects) throws NXException, RemoteException
objects
- Geometry and vertices in active sketchNXException
RemoteException
SketchConstraint[] autoConstrain(double linearTolerance, double angularTolerance, boolean allowRemoteConstraints, SmartObject[] geometries, Sketch.ConstraintType[] autoconstraintTypes) throws NXException, RemoteException
linearTolerance
- Capture DistanceangularTolerance
- Capture AngleallowRemoteConstraints
- Allow remote constraintsgeometries
- Array of geometriesautoconstraintTypes
- Constraint type arrayNXException
RemoteException
void makeDatumsInternal() throws NXException, RemoteException
NXException
RemoteException
void makeDatumsExternal() throws NXException, RemoteException
NXException
RemoteException
boolean isInternal() throws NXException, RemoteException
NXException
RemoteException
Sketch.CopyObjectData[] copyObjectsWithTracking(DisplayableObject[] inputObjects) throws NXException, RemoteException
inputObjects
- Objects to be copiedNXException
RemoteException
Sketch.UpdateLevel updateScope() throws NXException, RemoteException
NXException
RemoteException
void setUpdateScope(Sketch.UpdateLevel updateScope) throws NXException, RemoteException
updateScope
- NXException
RemoteException
void editSplinePoles(Spline spline, double[] poles) throws NXException, RemoteException
spline
- poles
- pole locations. Size is four times the number of poles.NXException
RemoteException
void editSplineDefiningPoints(Spline spline, double[] points) throws NXException, RemoteException
spline
- points
- point locations. Size is three times the number of points.NXException
RemoteException
void convertToNx10Spline(Spline spline) throws NXException, RemoteException
spline
- NXException
RemoteException
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