Sketch Class¶
-
class
NXOpen.
Sketch
¶ Bases:
NXOpen.DisplayableObject
,NXOpen.IProfile
Represents a sketch
Use the
NXOpen.SketchCollection
class to create a sketch.New in version NX3.0.0.
Properties¶
Property | Description |
---|---|
AttachPlane | Returns the plane that the sketch is attached to |
Color | Returns or sets the color of the object. |
CreateInferConstraintsSetting | Returns or sets the toggle that controls the creation of infer constraints in sketch |
DOFDisplay | Returns or sets a flag indicating whether the degree of freedom arrows are currently being displayed |
Feature | Returns the feature associated with this sketch |
IsActive | Returns true if the sketch is active |
IsBlanked | Returns the blank status of this object. |
IsDraftingSketch | Returns true if drafting sketch |
IsInternal | Returns true if the sketch is internal. |
IsOccurrence | Returns whether this object is an occurrence or not. |
JournalIdentifier | Returns the identifier that would be recorded in a journal for this object. |
Layer | Returns or sets the layer that the object is in. |
LineFont | Returns or sets the line font of the object. |
LineWidth | Returns or sets the line width of the object. |
Name | Returns the custom name of the object. |
NameLocation | Returns the location of the object’s name. |
Orientation | Returns the orientation matrix of the local coordinate system of the sketch |
Origin | Returns the location of the origin of the local coordinate system for the sketch |
OwningComponent | Returns the owning component, if this object is an occurrence. |
OwningPart | Returns the owning part of this object |
Prototype | Returns the prototype of this object if it is an occurrence. |
Tag | Returns the Tag for this object. |
UpdateScope | Returns or sets the current update scope. |
View | Returns the view corresponding to sketch |
VisibilityOfConstraints | Returns or sets the visibility of the constraints in the sketch |
Methods¶
Method | Description |
---|---|
Activate | Activates the sketch |
AddGeometry | Adds a curve or point to the sketch |
AutoConstrain | Creates Automatic Constraints on input set of geometries. |
Blank | Blanks the object. |
ConvertToNx10Spline | Convert the legacy splines to new NX10 splines. |
CopyObjects | Creates copies of input objects and constraints between these objects. |
CopyObjectsWithDimensionOutput | Creates copies of input objects and constraints between these objects. |
CopyObjectsWithTracking | Creates copies of input objects and constraints between these objects. |
CreateCoincidentConstraint | Creates a coincident constraint @return The coincident constraint |
CreateCollinearConstraint | Creates a collinear constraint. |
CreateConcentricConstraint | Creates a concentric constraint. |
CreateConstantAngleConstraint | Creates a constant angle constraint @return The constant angle constraint |
CreateConstantLengthConstraint | Creates a constant length constraint @return The constant length constraint |
CreateDiameterDimension | Creates a diameter dimension constraint @return The diametral dimension constraint |
CreateDimension | Creates a dimension between two geometric objects. |
CreateEqualLengthConstraint | Creates an equal length constraint. |
CreateEqualRadiusConstraint | Creates an equal radius constraint. |
CreateFixedConstraint | Creates a fixed constraint @return The fixed constraint |
CreateFullyFixedConstraints | Creates enough fixed constraints on the curve and all of its vertices such that the geometry is fully fixed without any redundant fixed constraints. |
CreateHorizontalConstraint | Creates a horizontal constraint @return The horizontal constraint |
CreateMidpointConstraint | Creates a midpoint constraint. |
CreateNonUniformScaledConstraint | Creates a non-uniform scale constraint @return The non-uniform scale constraint |
CreateNormalConstraint | Creates a normal constraint. |
CreateParallelConstraint | Creates a parallel constraint. |
CreatePerimeterDimension | Creates a perimeter dimension constraint @return The perimeter dimensional constraint |
CreatePerpendicularConstraint | Creates a perpendicular constraint. |
CreatePointOnCurveConstraint | Creates a point on curve constraint. |
CreatePointOnStringConstraint | Creates a point on string constraint. |
CreateRadialDimension | Creates a radial dimension constraint @return The radial dimension constraint |
CreateSlopeConstraint | Creates a slope constraint. |
CreateTangentConstraint | Creates a tangent constraint. |
CreateUniformScaledConstraint | Creates a uniform scale constraint @return The uniform scale constraint |
CreateVerticalConstraint | Creates a vertical constraint @return The vertical constraint |
Deactivate | Deactivates the sketch |
DeleteAllAttributesByType | Deletes all attributes of a specific type. |
DeleteAttributeByTypeAndTitle | Deletes an attribute by type and title. |
DeleteConstraintsOnGeometries | Deletes all geometric constraints associated with the object and all of its vertices. |
DeleteObjects | Deletes objects from the sketch @return List of errors encountered during the delete |
DeleteUserAttribute | Deletes the first attribute encountered with the given Type, Title. |
DeleteUserAttributes | Deletes the attributes encountered with the given Type with option to update or not. |
EditSplineDefiningPoints | Changes the locations of the defining points of a spline. |
EditSplinePoles | Changes the locations of the control poles of a spline. |
Fillet | Fillets curves and creates appropriate constraints. |
FindObject | Finds the NXOpen.NXObject with the given identifier as recorded in a journal. |
FlipNormal | Flips the outward normal vector of the sketch |
FlipReferenceDirection | Flips the reference direction of the sketch |
GetAllConstraintsOfType | Gets all constraints in the sketch of a particular type @return All the constraints in the sketch of the specified type |
GetAllExpressions | Returns all the expressions in the sketch @return All the expressions in the sketch |
GetAllGeometry | Returns all the curves and points in the sketch @return All the curves and points in the sketch |
GetAttributeTitlesByType | Gets all the attribute titles of a specific type. |
GetBooleanUserAttribute | Gets a boolean attribute by Title and array Index. |
GetComputationalTimeUserAttribute | Gets a time attribute by Title and array Index. |
GetConstraintsForGeometry | Gets all the constraints associated with a particular geometric item @return All the constraints associated with the geometry that is input |
GetIntegerAttribute | Gets an integer attribute by title. |
GetIntegerUserAttribute | Gets an integer attribute by Title and array Index. |
GetRealAttribute | Gets a real attribute by title. |
GetRealUserAttribute | Gets a real attribute by Title and array Index. |
GetReferenceAttribute | Gets the reference string (not the calculated value) of a string attribute that uses a reference string. |
GetReferenceDirection | Gets the reference direction of the sketch @return |
GetStatus | Gets the status of the sketch and the number of degrees of freedom that remain in the sketch. |
GetStringAttribute | Gets a string attribute value by title. |
GetStringUserAttribute | Gets a string attribute by Title and array Index. |
GetTimeAttribute | Gets a time attribute by title. |
GetTimeUserAttribute | Gets a time attribute by Title and array Index. |
GetUserAttribute | Gets the first attribute encountered on the object, if any, with a given Title, Type and array Index. |
GetUserAttributeAsString | Gets the first attribute encountered on the object, if any, with a given title, type and array index. |
GetUserAttributeCount | Gets the count of set attributes on the object, if any, of the given type. |
GetUserAttributeLock | Determine the lock of the given attribute. |
GetUserAttributeSize | Gets the size of the first attribute encountered on the object, if any, with a given Title and Type. |
GetUserAttributeSourceObjects | Returns an array of objects from which this object presents attributes. |
GetUserAttributes | Gets all the attributes that have been set on the given object. |
GetUserAttributesAsStrings | Gets all the attributes that have been set on the given object. |
HasUserAttribute | Determines if an attribute with the given Title, Type and array Index is present on the object Unset attributes will not be detected by this function, as its purpose is to test for the actual presence of the attribute on the object. |
HideDimensions | Blanks dimensions in the active sketch associated with the input sketch geometry. |
Highlight | Highlights the object. |
LocalUpdate | Update the sketch and not the sketch children. |
MakeDatumsExternal | Makes the internal sketch placement face and directional reference datums external. |
MakeDatumsInternal | Makes the sketch placement face and directional reference internal to the sketch if they are both datums referenced only by the sketch. |
MirrorObjects | Creates a reflection of the input geometry. |
Prints a representation of this object to the system log file. | |
Reattach | Reattaches a sketch. |
RedisplayObject | Redisplays the object in all views. |
RemoveViewDependency | Remove dependency on all views from an object. |
RunAutoDimension | Run auto dimensioning. |
SetAttribute | Creates or modifies an integer attribute. |
SetBooleanUserAttribute | Creates or modifies a boolean attribute with the option to update or not. |
SetName | Sets the custom name of the object. |
SetNameLocation | Sets the location of the object’s name. |
SetReferenceAttribute | Creates or modifies a string attribute which uses a reference string. |
SetReferenceDirection | Sets the reference direction of the sketch. |
SetTimeAttribute | Creates or modifies a time attribute. |
SetTimeUserAttribute | Creates or modifies a time attribute with the option to update or not. |
SetUserAttribute | Creates or modifies an attribute with the option to update or not. |
SetUserAttributeLock | Lock or unlock the given attribute. |
ShowDimensions | Unblanks dimensions in the active sketch associated with the input sketch geometry |
Unblank | Unblanks the object. |
Unhighlight | Unhighlights the object. |
Update | Updates the sketch |
UpdateConstraintDisplay | Updates the constraint display without updating the sketch |
UpdateDimensionDisplay | Updates the dimension display without updating the sketch |
UpdateGeometryDisplay | Updates the geometry display without updating the sketch |
Enumerations¶
SketchAddEllipseOption Enumeration | Used by NXOpen.Sketch.AddGeometry to determine whether to treat an ellipse as an ellipse or generic conic when adding the curve to a sketch. |
SketchAlternateSolutionOption Enumeration | Indicates whether the alternate solution should be used instead of the regular solution. |
SketchAssocType Enumeration | Used in NXOpen.SketchDimensionGeometry_Struct to indicate what type of geometry to use |
SketchAutoDimensioningRule Enumeration | Type of Auto Dimensioning rules. |
SketchConstraintClass Enumeration | Represents the class of the constraint. |
SketchConstraintGeometryHelpType Enumeration | Used in ConstraintHelp to indicate what type of help it is |
SketchConstraintPointType Enumeration | Used in ConstraintGeometry to indicate what type of point, if any, the geometry is |
SketchConstraintType Enumeration | Represents the type of constraint |
SketchConstraintVisibility Enumeration | Indicates the visibility of the constraints The APIs that use this enum are deprecated in NX85 The NXOpen.SketchConstraintVisibility.Some option will behave the same as the NXOpen.SketchConstraintVisibility.All option. |
SketchCreateDimensionOption Enumeration | Used in fillet to indicate whether a radius dimension should be created by the fillet |
SketchCreateInferConstraintSetting Enumeration | Indicates if the infer constraints will be created or not |
SketchDeleteThirdCurveOption Enumeration | Indicates whether the 3rd curve should be deleted when doing a 3 curve fillet |
SketchDimensionOption Enumeration | Used by NXOpen.Sketch.CreateDimension , NXOpen.Sketch.CreateRadialDimension NXOpen.Sketch.CreateDiameterDimension and NXOpen.Sketch.CreatePerimeterDimension to determine whether to create driving or reference dimension |
SketchInferConstraintsOption Enumeration | Used when adding a point or curve to a sketch. |
SketchPlaneOption Enumeration | Specifies the plane type used for a Sketch |
SketchStatus Enumeration | Represents the status of the sketch |
SketchTrimInputOption Enumeration | Indicates whether the input curves should be trimmed when doing a fillet |
SketchUpdateLevel Enumeration | Used to indicate how much the updating should occur |
SketchViewReorient Enumeration | Used to indicate whether to reorient the view when the sketch is activated |
Structs¶
SketchConstraintGeometry_Struct Struct | Used by the create geometric constraint methods to indicate what geometry the constraint should be applied to. |
SketchConstraintGeometryHelp_Struct Struct | Used by several constraint creation methods that need a help point or parameter to indicate how to create the constraint. |
SketchCopyObjectData_Struct Struct | This structure represents a map between the original object to be copied and the corresponding copied object. |
SketchDimensionGeometry_Struct Struct | Used in the dimension creation methods to indicate what geometry to create the dimension on. |
Property Detail¶
AttachPlane¶
-
Sketch.
AttachPlane
¶ Returns the plane that the sketch is attached to
-------------------------------------
Getter Method
Signature
AttachPlane()
Returns: Return type: NXOpen.ISurface
New in version NX3.0.0.
License requirements: None.
CreateInferConstraintsSetting¶
-
Sketch.
CreateInferConstraintsSetting
¶ Returns or sets the toggle that controls the creation of infer constraints in sketch
-------------------------------------
Getter Method
Signature
CreateInferConstraintsSetting()
Returns: Return type: NXOpen.SketchCreateInferConstraintSetting
New in version NX4.0.0.
License requirements: None.
-------------------------------------
Setter Method
Signature
CreateInferConstraintsSetting(createInferCon)
Parameters: createInferCon ( NXOpen.SketchCreateInferConstraintSetting
) –New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
DOFDisplay¶
-
Sketch.
DOFDisplay
¶ Returns or sets a flag indicating whether the degree of freedom arrows are currently being displayed
-------------------------------------
Getter Method
Signature
DOFDisplay()
Returns: Return type: bool New in version NX3.0.0.
License requirements: None.
-------------------------------------
Setter Method
Signature
DOFDisplay(displayDof)
Parameters: displayDof (bool) – New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
Feature¶
-
Sketch.
Feature
¶ Returns the feature associated with this sketch
-------------------------------------
Getter Method
Signature
Feature()
Returns: Associated feature Return type: NXOpen.Features.Feature
New in version NX3.0.0.
License requirements: None.
IsActive¶
-
Sketch.
IsActive
¶ Returns true if the sketch is active
-------------------------------------
Getter Method
Signature
IsActive()
Returns: Return type: bool New in version NX3.0.0.
License requirements: None.
IsDraftingSketch¶
-
Sketch.
IsDraftingSketch
¶ Returns true if drafting sketch
-------------------------------------
Getter Method
Signature
IsDraftingSketch()
Returns: Return type: bool New in version NX6.0.0.
License requirements: None.
IsInternal¶
-
Sketch.
IsInternal
¶ Returns true if the sketch is internal.
-------------------------------------
Getter Method
Signature
IsInternal()
Returns: Return type: bool New in version NX6.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)
IsOccurrence¶
-
Sketch.
IsOccurrence
¶ Returns whether this object is an occurrence or not.
-------------------------------------
Getter Method
Signature
IsOccurrence()
Returns: This object is an occurrence Return type: bool New in version NX3.0.0.
License requirements: None.
JournalIdentifier¶
-
Sketch.
JournalIdentifier
¶ Returns the identifier that would be recorded in a journal for this object.
This may not be the same across different releases of the software.
-------------------------------------
Getter Method
Signature
JournalIdentifier()
Returns: Return type: str New in version NX3.0.0.
License requirements: None.
Name¶
-
Sketch.
Name
¶ Returns the custom name of the object.
-------------------------------------
Getter Method
Signature
Name()
Returns: Return type: str New in version NX3.0.0.
License requirements: None.
Orientation¶
-
Sketch.
Orientation
¶ Returns the orientation matrix of the local coordinate system of the sketch
-------------------------------------
Getter Method
Signature
Orientation()
Returns: Return type: NXOpen.NXMatrix
New in version NX3.0.0.
License requirements: None.
Origin¶
-
Sketch.
Origin
¶ Returns the location of the origin of the local coordinate system for the sketch
-------------------------------------
Getter Method
Signature
Origin()
Returns: Return type: NXOpen.Point3d
New in version NX3.0.0.
License requirements: None.
OwningComponent¶
-
Sketch.
OwningComponent
¶ Returns the owning component, if this object is an occurrence.
-------------------------------------
Getter Method
Signature
OwningComponent()
Returns: Return type: NXOpen.Assemblies.Component
New in version NX3.0.0.
License requirements: None.
OwningPart¶
-
Sketch.
OwningPart
¶ Returns the owning part of this object
-------------------------------------
Getter Method
Signature
OwningPart()
Returns: The owning part of this object or null if it does not have an owner Return type: NXOpen.BasePart
New in version NX3.0.0.
License requirements: None.
Prototype¶
-
Sketch.
Prototype
¶ Returns the prototype of this object if it is an occurrence.
-------------------------------------
Getter Method
Signature
Prototype()
Returns: The prototype of this object or null if this object is not an occurrence Return type: NXOpen.INXObject
New in version NX3.0.0.
License requirements: None.
UpdateScope¶
-
Sketch.
UpdateScope
¶ Returns or sets the current update scope.
Used in Direct Sketch to control update
-------------------------------------
Getter Method
Signature
UpdateScope()
Returns: Return type: NXOpen.SketchUpdateLevel
New in version NX8.0.0.
License requirements: None.
-------------------------------------
Setter Method
Signature
UpdateScope(updateScope)
Parameters: updateScope ( NXOpen.SketchUpdateLevel
) –New in version NX8.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
View¶
-
Sketch.
View
¶ Returns the view corresponding to sketch
-------------------------------------
Getter Method
Signature
View()
Returns: View corresponding to sketch Return type: NXOpen.View
New in version NX6.0.0.
License requirements: None.
VisibilityOfConstraints¶
-
Sketch.
VisibilityOfConstraints
¶ Returns or sets the visibility of the constraints in the sketch
-------------------------------------
Getter Method
Signature
VisibilityOfConstraints()
Returns: Return type: NXOpen.SketchConstraintVisibility
New in version NX3.0.0.
Deprecated since version NX8.5.0: Use
NXOpen.Preferences.SessionSketch.DisplayConstraintSymbols
instead.License requirements: None.
-------------------------------------
Setter Method
Signature
VisibilityOfConstraints(visibility)
Parameters: visibility ( NXOpen.SketchConstraintVisibility
) –New in version NX3.0.0.
Deprecated since version NX8.5.0: Use
NXOpen.Preferences.SessionSketch.DisplayConstraintSymbols
instead.License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
Method Detail¶
Activate¶
-
Sketch.
Activate
¶ Activates the sketch
Signature
Activate(orientView)
Parameters: orientView ( NXOpen.SketchViewReorient
) – Indicates whether to orient the view to the sketch during activationNew in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
AddGeometry¶
-
Sketch.
AddGeometry
¶ Overloaded method AddGeometry
AddGeometry(crv, inferCoincidentConstraints)
AddGeometry(crv)
AddGeometry(crv, inferCoincidentConstraints, ellipseOption)
AddGeometry(inferCoincidentConstraints, ellipseOption, curvesOrPoints)
-------------------------------------
Adds a curve or point to the sketch
Signature
AddGeometry(crv, inferCoincidentConstraints)
Parameters: - crv (
NXOpen.DisplayableObject
) – Must be a curve or point - inferCoincidentConstraints (
NXOpen.SketchInferConstraintsOption
) – Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Adds a curve or point to the sketch. Infers coincident constraints with other geometry in the sketch
Signature
AddGeometry(crv)
Parameters: crv ( NXOpen.DisplayableObject
) – Must be a curve or pointNew in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Adds a curve or point to a sketch.
Signature
AddGeometry(crv, inferCoincidentConstraints, ellipseOption)
Parameters: - crv (
NXOpen.Curve
) – Must be a curve or point - inferCoincidentConstraints (
NXOpen.SketchInferConstraintsOption
) – Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created - ellipseOption (
NXOpen.SketchAddEllipseOption
) – 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 forNXOpen.SketchAddEllipseOption
for more details. The default value isNXOpen.SketchAddEllipseOption.TreatAsEllipse
. In order to treat an ellipse as a conic, its end angle minus its start angle must be less than 180 degrees.
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Adds an array of curves or points to a sketch.
Signature
AddGeometry(inferCoincidentConstraints, ellipseOption, curvesOrPoints)
Parameters: - inferCoincidentConstraints (
NXOpen.SketchInferConstraintsOption
) – Whether to automatically create coincident constraints when adding the geometry. If this flag is true and there exists another curve or point in the sketch that has a vertex that is at the same location (within system tolerance) as one of the vertices for crv, a coincident constraint will be created - ellipseOption (
NXOpen.SketchAddEllipseOption
) – 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 forNXOpen.SketchAddEllipseOption
for more details. The default value isNXOpen.SketchAddEllipseOption.TreatAsEllipse
. In order to treat an ellipse as a conic, its end angle minus its start angle must be less than 180 degrees. - curvesOrPoints (list of
NXOpen.SmartObject
) – Must be a curve or point
New in version NX6.0.1.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
AutoConstrain¶
-
Sketch.
AutoConstrain
¶ Creates Automatic Constraints on input set of geometries.
Signature
AutoConstrain(linearTolerance, angularTolerance, allowRemoteConstraints, geometries, autoconstraintTypes)
Parameters: - linearTolerance (float) – Capture Distance
- angularTolerance (float) – Capture Angle
- allowRemoteConstraints (bool) – Allow remote constraints
- geometries (list of
NXOpen.SmartObject
) – Array of geometries - autoconstraintTypes (list of
NXOpen.SketchConstraintType
) – Constraint type array
Returns: Array of deduced constraints
Return type: list of
NXOpen.SketchConstraint
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
ConvertToNx10Spline¶
-
Sketch.
ConvertToNx10Spline
¶ Convert the legacy splines to new NX10 splines.
The input spline will be upgraded to NX10 spline. No new splines will be created to replace the input spline.
Signature
ConvertToNx10Spline(spline)
Parameters: spline ( NXOpen.Spline
) –New in version NX10.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CopyObjects¶
-
Sketch.
CopyObjects
¶ Creates copies of input objects and constraints between these objects.
Signature
CopyObjects(inputObjects)
Parameters: inputObjects (list of NXOpen.NXObject
) – Objects to be copiedReturns: Copies of objects Return type: list of NXOpen.NXObject
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CopyObjectsWithDimensionOutput¶
-
Sketch.
CopyObjectsWithDimensionOutput
¶ Creates copies of input objects and constraints between these objects.
This function is same as
NXOpen.Sketch.CopyObjects
except that it returns an array of newly created dimensionsSignature
CopyObjectsWithDimensionOutput(inputObjects)
Parameters: inputObjects (list of NXOpen.NXObject
) – Objects to be copiedReturns: a tuple Return type: A tuple consisting of (outputObjects, outputDims). outputObjects is a list of NXOpen.NXObject
. Copies of objects outputDims is a list ofNXOpen.NXObject
. Copies of dimsNew in version NX6.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CopyObjectsWithTracking¶
-
Sketch.
CopyObjectsWithTracking
¶ Creates copies of input objects and constraints between these objects.
Sketch dimensions are copied only if explicitly included in the input_objects array.
Signature
CopyObjectsWithTracking(inputObjects)
Parameters: inputObjects (list of NXOpen.DisplayableObject
) – Objects to be copiedReturns: Map between the original input object and the corresponding copied object Return type: list of NXOpen.SketchCopyObjectData_Struct
New in version NX7.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateCoincidentConstraint¶
-
Sketch.
CreateCoincidentConstraint
¶ Creates a coincident constraint
Signature
CreateCoincidentConstraint(geom1, geom2)
Parameters: - geom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a vertex - geom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a vertex
Returns: The coincident constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- geom1 (
CreateCollinearConstraint¶
-
Sketch.
CreateCollinearConstraint
¶ Creates a collinear constraint.
One of the input constraint geometries must be a line.
Signature
CreateCollinearConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a line, linear edge, datum axis, or datum plane - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a line, linear edge, datum axis, or datum plane
Returns: The collinear constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateConcentricConstraint¶
-
Sketch.
CreateConcentricConstraint
¶ Creates a concentric constraint.
One of the input constraint geometries must be a curve.
Signature
CreateConcentricConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be an arc or ellipse or edge shaped as an arc or ellipse - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be an arc or ellipse or edge shaped as an arc or ellipse
Returns: The concentric constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateConstantAngleConstraint¶
-
Sketch.
CreateConstantAngleConstraint
¶ Creates a constant angle constraint
Signature
CreateConstantAngleConstraint(conGeom)
Parameters: conGeom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a lineReturns: The constant angle constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateConstantLengthConstraint¶
-
Sketch.
CreateConstantLengthConstraint
¶ Creates a constant length constraint
Signature
CreateConstantLengthConstraint(conGeom)
Parameters: conGeom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a lineReturns: The constant length constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateDiameterDimension¶
-
Sketch.
CreateDiameterDimension
¶ Overloaded method CreateDiameterDimension
CreateDiameterDimension(dimObject1, dimOrigin, expression)
CreateDiameterDimension(dimObject1, dimOrigin, expression, refDim)
-------------------------------------
Creates a diameter dimension constraint
Signature
CreateDiameterDimension(dimObject1, dimOrigin, expression)
Parameters: - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – Should be an arc - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None
Returns: The diametral dimension constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Creates a diameter dimension constraint. Accepts a flag to create the dim as driving or reference
Signature
CreateDiameterDimension(dimObject1, dimOrigin, expression, refDim)
Parameters: - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – Should be an arc - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None - refDim (
NXOpen.SketchDimensionOption
) – option for creating driving or reference dimension
Returns: The diametral dimension constraint
Return type: New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
CreateDimension¶
-
Sketch.
CreateDimension
¶ Overloaded method CreateDimension
CreateDimension(dimType, dimObject1, dimObject2, dimOrigin, expression)
CreateDimension(dimType, dimObject1, dimObject2, dimOrigin, expression, refDim)
-------------------------------------
Creates a dimension between two geometric objects. Do not use for radial, diameter, or perimeter dimensions. To create a radial or diameter constraint, use
NXOpen.Sketch.CreateRadialDimension
orNXOpen.Sketch.CreateDiameterDimension
. To create a perimeter dimension, useNXOpen.Sketch.CreatePerimeterDimension
Signature
CreateDimension(dimType, dimObject1, dimObject2, dimOrigin, expression)
Parameters: - dimType (
NXOpen.SketchConstraintType
) – Must be one of the dimension types and should not be a radial, diametral, or perimeter dimension - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – First input geometry - dimObject2 (
NXOpen.SketchDimensionGeometry_Struct
) – Second input geometry - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None
Returns: The dimensional constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Creates a dimension between two geometric objects. Do not use for radial, diameter, or perimeter dimensions. To create a radial or diameter constraint, use
NXOpen.Sketch.CreateRadialDimension
orNXOpen.Sketch.CreateDiameterDimension
. To create a perimeter dimension, useNXOpen.Sketch.CreatePerimeterDimension
. This function takes in an argument to create the dimension as driving or reference.Signature
CreateDimension(dimType, dimObject1, dimObject2, dimOrigin, expression, refDim)
Parameters: - dimType (
NXOpen.SketchConstraintType
) – Must be one of the dimension types and should not be a radial, diametral, or perimeter dimension - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – First input geometry - dimObject2 (
NXOpen.SketchDimensionGeometry_Struct
) – Second input geometry - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None - refDim (
NXOpen.SketchDimensionOption
) – option for creating driving or reference dimension
Returns: The dimensional constraint
Return type: New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
CreateEqualLengthConstraint¶
-
Sketch.
CreateEqualLengthConstraint
¶ Creates an equal length constraint.
One of the input constraint geometries must be a line.
Signature
CreateEqualLengthConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a line or linear edge - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a line or linear edge
Returns: The equal length constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateEqualRadiusConstraint¶
-
Sketch.
CreateEqualRadiusConstraint
¶ Creates an equal radius constraint.
One of the input constraint geometries must be a curve.
Signature
CreateEqualRadiusConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be an arc or edge shaped as an arc - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be an arc or edge shaped as an arc
Returns: The equal radius constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateFixedConstraint¶
-
Sketch.
CreateFixedConstraint
¶ Creates a fixed constraint
Signature
CreateFixedConstraint(geom)
Parameters: geom ( NXOpen.SketchConstraintGeometry_Struct
) – Can be any curve, point, or vertex in the sketchReturns: The fixed constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateFullyFixedConstraints¶
-
Sketch.
CreateFullyFixedConstraints
¶ Creates enough fixed constraints on the curve and all of its vertices such that the geometry is fully fixed without any redundant fixed constraints.
Signature
CreateFullyFixedConstraints(geom)
Parameters: geom ( NXOpen.SketchConstraintGeometry_Struct
) – Can be any curve, point, or vertex in the sketchReturns: The fixed constraints Return type: list of NXOpen.SketchGeometricConstraint
New in version NX5.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateHorizontalConstraint¶
-
Sketch.
CreateHorizontalConstraint
¶ Creates a horizontal constraint
Signature
CreateHorizontalConstraint(geom)
Parameters: geom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a lineReturns: The horizontal constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateMidpointConstraint¶
-
Sketch.
CreateMidpointConstraint
¶ Creates a midpoint constraint.
One of the input constraint geometries must be a vertex and the other must be a curve or edge.
Signature
CreateMidpointConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) –
Returns: The midpoint constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateNonUniformScaledConstraint¶
-
Sketch.
CreateNonUniformScaledConstraint
¶ Creates a non-uniform scale constraint
Signature
CreateNonUniformScaledConstraint(conGeom)
Parameters: conGeom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a splineReturns: The non-uniform scale constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateNormalConstraint¶
-
Sketch.
CreateNormalConstraint
¶ 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
Signature
CreateNormalConstraint(conGeom1, geom1Help, conGeom2, geom2Help)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – First input geometry for the constraint - geom1Help (
NXOpen.SketchConstraintGeometryHelp_Struct
) – Help data for first geom - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Second input geometry for the constraint - geom2Help (
NXOpen.SketchConstraintGeometryHelp_Struct
) – Help data for second geom
Returns: The normal constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateParallelConstraint¶
-
Sketch.
CreateParallelConstraint
¶ 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).
Signature
CreateParallelConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – First input geometry for the constraint - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Second input geometry for the constraint
Returns: The parallel constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreatePerimeterDimension¶
-
Sketch.
CreatePerimeterDimension
¶ Creates a perimeter dimension constraint
Signature
CreatePerimeterDimension(curves, dimOrigin, expression)
Parameters: - curves (list of
NXOpen.Curve
) – The curves that form the perimeter - dimOrigin (
NXOpen.Point3d
) – Not currently used - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None
Returns: The perimeter dimensional constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- curves (list of
CreatePerpendicularConstraint¶
-
Sketch.
CreatePerpendicularConstraint
¶ 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).
Signature
CreatePerpendicularConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – First input geometry for the constraint - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – Second input geometry for the constraint
Returns: The perpendicular constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreatePointOnCurveConstraint¶
-
Sketch.
CreatePointOnCurveConstraint
¶ 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.
Signature
CreatePointOnCurveConstraint(conGeom1, conGeom2, help)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) – - help (
NXOpen.SketchConstraintGeometryHelp_Struct
) –
Returns: The point on curve constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreatePointOnStringConstraint¶
-
Sketch.
CreatePointOnStringConstraint
¶ Overloaded method CreatePointOnStringConstraint
CreatePointOnStringConstraint(conGeom1, curvesInString, helpData, curveWhichHelpParamAppliesTo)
CreatePointOnStringConstraint(conGeom1, curveInString, helpData)
-------------------------------------
Creates a point on string constraint.
Signature
CreatePointOnStringConstraint(conGeom1, curvesInString, helpData, curveWhichHelpParamAppliesTo)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a vertex - curvesInString (list of
NXOpen.Curve
) – Must all be part of the same string. (You can create a string of curves through the UI through the Edit -<ja_gt> Project command.) - helpData (
NXOpen.SketchConstraintGeometryHelp_Struct
) – - curveWhichHelpParamAppliesTo (int) – If helpData is a parameter, this parameter indicates which curve in the curvesInString that the help parameter applies to. Otherwise, this parameter is not used
Returns: The point on string constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
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.
Signature
CreatePointOnStringConstraint(conGeom1, curveInString, helpData)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – Must be a vertex - curveInString (
NXOpen.Curve
) – 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 -<ja_gt> Project command.) - helpData (
NXOpen.SketchConstraintGeometryHelp_Struct
) –
Returns: The point on string constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
CreateRadialDimension¶
-
Sketch.
CreateRadialDimension
¶ Overloaded method CreateRadialDimension
CreateRadialDimension(dimObject1, dimOrigin, expression)
CreateRadialDimension(dimObject1, dimOrigin, expression, refDim)
-------------------------------------
Creates a radial dimension constraint
Signature
CreateRadialDimension(dimObject1, dimOrigin, expression)
Parameters: - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – Should be an arc - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None
Returns: The radial dimension constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Creates a radial dimension constraint. Accepts a flag to create the dimension as driving or reference
Signature
CreateRadialDimension(dimObject1, dimOrigin, expression, refDim)
Parameters: - dimObject1 (
NXOpen.SketchDimensionGeometry_Struct
) – Should be an arc - dimOrigin (
NXOpen.Point3d
) – The location where the dimension should be placed - expression (
NXOpen.Expression
) – Defining expression for the dimension. Can be None - refDim (
NXOpen.SketchDimensionOption
) – option for creating driving or reference dimension
Returns: The radial dimension constraint
Return type: New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
CreateSlopeConstraint¶
-
Sketch.
CreateSlopeConstraint
¶ 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.
Signature
CreateSlopeConstraint(conGeom1, conGeom2)
Parameters: - conGeom1 (
NXOpen.SketchConstraintGeometry_Struct
) – - conGeom2 (
NXOpen.SketchConstraintGeometry_Struct
) –
Returns: The slope constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- conGeom1 (
CreateTangentConstraint¶
-
Sketch.
CreateTangentConstraint
¶ Creates a tangent constraint.
Note: the input constraint geometries cannot both be linear.
Signature
CreateTangentConstraint(geom1, geom1Help, geom2, geom2Help)
Parameters: - geom1 (
NXOpen.SketchConstraintGeometry_Struct
) – A curve, edge, or datum axis - geom1Help (
NXOpen.SketchConstraintGeometryHelp_Struct
) – - geom2 (
NXOpen.SketchConstraintGeometry_Struct
) – A curve, edge, or datum axis - geom2Help (
NXOpen.SketchConstraintGeometryHelp_Struct
) –
Returns: The tangent constraint
Return type: New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- geom1 (
CreateUniformScaledConstraint¶
-
Sketch.
CreateUniformScaledConstraint
¶ Creates a uniform scale constraint
Signature
CreateUniformScaledConstraint(conGeom)
Parameters: conGeom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a splineReturns: The uniform scale constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
CreateVerticalConstraint¶
-
Sketch.
CreateVerticalConstraint
¶ Creates a vertical constraint
Signature
CreateVerticalConstraint(geom)
Parameters: geom ( NXOpen.SketchConstraintGeometry_Struct
) – Must be a lineReturns: The vertical constraint Return type: NXOpen.SketchGeometricConstraint
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
Deactivate¶
-
Sketch.
Deactivate
¶ Deactivates the sketch
Signature
Deactivate(orientView, updateLevel)
Parameters: - orientView (
NXOpen.SketchViewReorient
) – Indicates whether to orient the view to the model during deactivation - updateLevel (
NXOpen.SketchUpdateLevel
) – Indicates whether just the sketch should be updated or the entire model
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- orientView (
DeleteConstraintsOnGeometries¶
-
Sketch.
DeleteConstraintsOnGeometries
¶ Overloaded method DeleteConstraintsOnGeometries
DeleteConstraintsOnGeometries(objects)
DeleteConstraintsOnGeometries(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.
Signature
DeleteConstraintsOnGeometries(objects)
Parameters: objects (list of NXOpen.NXObject
) – Objects whose constraints needs to be deletedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Deletes all geometric constraints associated with the object and all of its vertices. Converts all the driving dimensions associated with the object and its vertices to reference dimensions. The user can pass in a vertex to do the same on just the supplied vertex.
Signature
DeleteConstraintsOnGeometries(objects)
Parameters: objects (list of NXOpen.SketchConstraintGeometry_Struct
) – Objects whose constraints needs to be deletedNew in version NX8.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
DeleteObjects¶
-
Sketch.
DeleteObjects
¶ Deletes objects from the sketch
Signature
DeleteObjects(objects)
Parameters: objects (list of NXOpen.NXObject
) – Objects to be deletedReturns: List of errors encountered during the delete Return type: NXOpen.ErrorList
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
EditSplineDefiningPoints¶
-
Sketch.
EditSplineDefiningPoints
¶ Changes the locations of the defining points of a spline.
The length of point array should be enough to cover existing defining points. You cannot add/remove points nor change knot sequence via this call.
Signature
EditSplineDefiningPoints(spline, points)
Parameters: - spline (
NXOpen.Spline
) – - points (list of float) – point locations. Size is three times the number of points.
New in version NX10.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- spline (
EditSplinePoles¶
-
Sketch.
EditSplinePoles
¶ Changes the locations of the control poles of a spline.
The length of poles array should be enough to cover existing poles. You cannot add/remove poles nor change knot sequence via this call. The order of data in poles array is x, y, z, weight. You can edit any or all of these four values via this function.
Signature
EditSplinePoles(spline, poles)
Parameters: - spline (
NXOpen.Spline
) – - poles (list of float) – pole locations. Size is four times the number of poles.
New in version NX10.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- spline (
Fillet¶
-
Sketch.
Fillet
¶ Overloaded method Fillet
Fillet(curve1, curve2, helpPoint1, helpPoint2, radius, doTrim, createRadiusDim, alternateSolution)
Fillet(curve1, curve2, helpPoint1, helpPoint2, pointOnArc, radius, doTrim, createRadiusDim, alternateSolution)
Fillet(curve1, curve2, curve3, helpPoint1, helpPoint2, helpPoint3, radius, doTrim, doDelete, createRadiusDim, alternateSolution)
Fillet(curve1, curve2, curve3, helpPoint1, helpPoint2, helpPoint3, pointOnArc, radius, doTrim, doDelete, createRadiusDim, alternateSolution)
-------------------------------------
Fillets curves and creates appropriate constraints. If the input curves have mirror constraints, the fillet is also performed on the mirror curves.
Signature
Fillet(curve1, curve2, helpPoint1, helpPoint2, radius, doTrim, createRadiusDim, alternateSolution)
Parameters: - curve1 (
NXOpen.Curve
) – First curve for the fillet - curve2 (
NXOpen.Curve
) – Second curve for the fillet - helpPoint1 (
NXOpen.Point3d
) – Should be a point on the first curve. Indicates where the fillet should be created - helpPoint2 (
NXOpen.Point3d
) – Should be a point on the second curve. Indicates where the fillet should be created - radius (float) – Radius of the fillet
- doTrim (
NXOpen.SketchTrimInputOption
) – Indicates whether the input curves should get trimmed by the fillet - createRadiusDim (
NXOpen.SketchCreateDimensionOption
) – Indicates whether a radius dimension should be created - alternateSolution (
NXOpen.SketchAlternateSolutionOption
) – Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.
Returns: a tuple
Return type: A tuple consisting of (fillets, constraints). fillets is a list of
NXOpen.Arc
. 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 constraints is a list ofNXOpen.SketchConstraint
. The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Fillets curves and creates appropriate constraints. If the input curves have mirror constraints, the fillet is also performed on the mirror curves.
Signature
Fillet(curve1, curve2, helpPoint1, helpPoint2, pointOnArc, radius, doTrim, createRadiusDim, alternateSolution)
Parameters: - curve1 (
NXOpen.Curve
) – First curve for the fillet - curve2 (
NXOpen.Curve
) – Second curve for the fillet - helpPoint1 (
NXOpen.Point3d
) – Should be a point on the first curve. Indicates where the fillet should be created - helpPoint2 (
NXOpen.Point3d
) – Should be a point on the second curve. Indicates where the fillet should be created - pointOnArc (
NXOpen.Point3d
) – Point on fillet arc - radius (float) – Radius of the fillet
- doTrim (
NXOpen.SketchTrimInputOption
) – Indicates whether the input curves should get trimmed by the fillet - createRadiusDim (
NXOpen.SketchCreateDimensionOption
) – Indicates whether a radius dimension should be created - alternateSolution (
NXOpen.SketchAlternateSolutionOption
) – Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.
Returns: a tuple
Return type: A tuple consisting of (fillets, constraints). fillets is a list of
NXOpen.Arc
. 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 constraints is a list ofNXOpen.SketchConstraint
. The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.New in version NX7.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Fillets curves and creates appropriate constraints. If the input curves have mirror constraints, the fillet is also performed on the mirror curves.
Signature
Fillet(curve1, curve2, curve3, helpPoint1, helpPoint2, helpPoint3, radius, doTrim, doDelete, createRadiusDim, alternateSolution)
Parameters: - curve1 (
NXOpen.Curve
) – First curve for the fillet - curve2 (
NXOpen.Curve
) – Second curve for the fillet - curve3 (
NXOpen.Curve
) – Third curve for the fillet - helpPoint1 (
NXOpen.Point3d
) – Should be a point on the first curve. Indicates where the fillet should be created - helpPoint2 (
NXOpen.Point3d
) – Should be a point on the second curve. Indicates where the fillet should be created - helpPoint3 (
NXOpen.Point3d
) – Should be a point on the third curve. Indicates where the fillet should be created - radius (float) – Radius of the fillet
- doTrim (
NXOpen.SketchTrimInputOption
) – Indicates whether the input curves should get trimmed by the fillet - doDelete (
NXOpen.SketchDeleteThirdCurveOption
) – Indicates whether the third curve should be deleted - createRadiusDim (
NXOpen.SketchCreateDimensionOption
) – Indicates whether a radius dimension should be created - alternateSolution (
NXOpen.SketchAlternateSolutionOption
) – Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.
Returns: a tuple
Return type: A tuple consisting of (fillets, constraints). fillets is a list of
NXOpen.Arc
. 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 constraints is a list ofNXOpen.SketchConstraint
. The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Fillets curves and creates appropriate constraints. If the input curves have mirror constraints, the fillet is also performed on the mirror curves.
Signature
Fillet(curve1, curve2, curve3, helpPoint1, helpPoint2, helpPoint3, pointOnArc, radius, doTrim, doDelete, createRadiusDim, alternateSolution)
Parameters: - curve1 (
NXOpen.Curve
) – First curve for the fillet - curve2 (
NXOpen.Curve
) – Second curve for the fillet - curve3 (
NXOpen.Curve
) – Third curve for the fillet - helpPoint1 (
NXOpen.Point3d
) – Should be a point on the first curve. Indicates where the fillet should be created - helpPoint2 (
NXOpen.Point3d
) – Should be a point on the second curve. Indicates where the fillet should be created - helpPoint3 (
NXOpen.Point3d
) – Should be a point on the third curve. Indicates where the fillet should be created - pointOnArc (
NXOpen.Point3d
) – Point on fillet arc - radius (float) – Radius of the fillet
- doTrim (
NXOpen.SketchTrimInputOption
) – Indicates whether the input curves should get trimmed by the fillet - doDelete (
NXOpen.SketchDeleteThirdCurveOption
) – Indicates whether the third curve should be deleted - createRadiusDim (
NXOpen.SketchCreateDimensionOption
) – Indicates whether a radius dimension should be created - alternateSolution (
NXOpen.SketchAlternateSolutionOption
) – Indicates whether the alternate solution should be used instead of the regular solution. The alternate solution for an arc is the portion of the full circle that is left out of the regular solution.
Returns: a tuple
Return type: A tuple consisting of (fillets, constraints). fillets is a list of
NXOpen.Arc
. 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 constraints is a list ofNXOpen.SketchConstraint
. The constraints that were created by the fillet. If the input curves get trimmed, coincident and tangent constraints are created. If the input curves do not get trimmed, point on curve and tangent constraints are created.New in version NX7.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
FindObject¶
-
Sketch.
FindObject
¶ Finds the
NXOpen.NXObject
with the given identifier as recorded in a journal.An object may not return the same value as its JournalIdentifier in different versions of the software. However newer versions of the software should find the same object when FindObject is passed older versions of its journal identifier. In general, this method should not be used in handwritten code and exists to support record and playback of journals.
An exception will be thrown if no object can be found with the given journal identifier.
Signature
FindObject(journalIdentifier)
Parameters: journalIdentifier (str) – Journal identifier of the object Returns: Return type: NXOpen.INXObject
New in version NX3.0.0.
License requirements: None.
FlipNormal¶
-
Sketch.
FlipNormal
¶ Flips the outward normal vector of the sketch
Signature
FlipNormal()
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
FlipReferenceDirection¶
-
Sketch.
FlipReferenceDirection
¶ Flips the reference direction of the sketch
Signature
FlipReferenceDirection()
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
GetAllConstraintsOfType¶
-
Sketch.
GetAllConstraintsOfType
¶ Gets all constraints in the sketch of a particular type
Signature
GetAllConstraintsOfType(conClass, conType)
Parameters: - conClass (
NXOpen.SketchConstraintClass
) – Optional filter. UseNXOpen.SketchConstraintClass.Any
if you do not want to filter by constraint class - conType (
NXOpen.SketchConstraintType
) – Optional filter. UseNXOpen.SketchConstraintType.NoCon
if you do not want to filter by constraint type
Returns: All the constraints in the sketch of the specified type
Return type: list of
NXOpen.SketchConstraint
New in version NX3.0.0.
License requirements: None.
- conClass (
GetAllExpressions¶
-
Sketch.
GetAllExpressions
¶ Returns all the expressions in the sketch
Signature
GetAllExpressions()
Returns: All the expressions in the sketch Return type: list of NXOpen.Expression
New in version NX3.0.0.
License requirements: None.
GetAllGeometry¶
-
Sketch.
GetAllGeometry
¶ Returns all the curves and points in the sketch
Signature
GetAllGeometry()
Returns: All the curves and points in the sketch Return type: list of NXOpen.NXObject
New in version NX3.0.0.
License requirements: None.
GetConstraintsForGeometry¶
-
Sketch.
GetConstraintsForGeometry
¶ Gets all the constraints associated with a particular geometric item
Signature
GetConstraintsForGeometry(geometry, conClass)
Parameters: - geometry (
NXOpen.SmartObject
) – Must be a curve or point - conClass (
NXOpen.SketchConstraintClass
) – Optional filter. UseNXOpen.SketchConstraintClass.Any
if you do not want to filter by constraint class
Returns: All the constraints associated with the geometry that is input
Return type: list of
NXOpen.SketchConstraint
New in version NX3.0.0.
License requirements: None.
- geometry (
GetReferenceDirection¶
-
Sketch.
GetReferenceDirection
¶ Gets the reference direction of the sketch
Signature
GetReferenceDirection()
Returns: a tuple Return type: A tuple consisting of (referenceDirection, referenceAxis, referenceAxisOrientation, referenceAxisSense). referenceDirection is a NXOpen.Vector3d
. referenceAxis is aNXOpen.IReferenceAxis
. An edge, datum axis, datum plane, or face that the sketch uses as a reference. May be None. referenceAxisOrientation is aNXOpen.AxisOrientation
. Indicates whether the reference axis is horizontal or vertical referenceAxisSense is aNXOpen.Sense
. If reference axis is an edge or datum axis, this parameter indicates whether the reference axis is in the same direction as the edge or datum axis or in the opposite direction. If reference axis is not an edge or datum axis, this parameter is not used.New in version NX3.0.0.
License requirements: None.
GetStatus¶
-
Sketch.
GetStatus
¶ 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.
Signature
GetStatus()
Returns: a tuple Return type: A tuple consisting of (status, dofNeeded). status is a NXOpen.SketchStatus
. The sketch’s status, which indicates how well constrained the sketch is dofNeeded is a int. The number of degrees of freedom left in the sketchNew in version NX3.0.0.
License requirements: None.
HideDimensions¶
-
Sketch.
HideDimensions
¶ Overloaded method HideDimensions
HideDimensions(inputObjects)
HideDimensions()
HideDimensions(objects)
-------------------------------------
Blanks dimensions in the active sketch associated with the input sketch geometry.
Signature
HideDimensions(inputObjects)
Parameters: inputObjects (list of NXOpen.DisplayableObject
) – Geometry and groups in active sketchNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Blanks all the dimensions of input sketch
Signature
HideDimensions()
New in version NX6.0.1.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Blanks dimensions in the active sketch associated with the input sketch geometry. This function can accept vertices
Signature
HideDimensions(objects)
Parameters: objects (list of NXOpen.SketchConstraintGeometry_Struct
) – Geometry and vertices in active sketchNew in version NX8.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
LocalUpdate¶
-
Sketch.
LocalUpdate
¶ Update the sketch and not the sketch children.
If a different sketch is active the SKETCH_NOT_INITIALIZED error will return. The function works even if the sketch is not active.
Signature
LocalUpdate()
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
MakeDatumsExternal¶
-
Sketch.
MakeDatumsExternal
¶ Makes the internal sketch placement face and directional reference datums external.
Signature
MakeDatumsExternal()
New in version NX5.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)
MakeDatumsInternal¶
-
Sketch.
MakeDatumsInternal
¶ Makes the sketch placement face and directional reference internal to the sketch if they are both datums referenced only by the sketch.
Signature
MakeDatumsInternal()
New in version NX5.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)
MirrorObjects¶
-
Sketch.
MirrorObjects
¶ Creates a reflection of the input geometry.
This API is now deprecated. Please use
NXOpen.SketchMirrorBuilder
instead.Signature
MirrorObjects(centerline, objectsToMirror)
Parameters: - centerline (
NXOpen.DisplayableObject
) – Axis of reflection for the mirror. Must be a linear curve, edge, datum axis or datum plane - objectsToMirror (list of
NXOpen.SmartObject
) – Points and curves to mirror. None of the curves may be used as a centerline for another mirror operation
Returns: The mirrored geometry that was created
Return type: list of
NXOpen.SmartObject
New in version NX4.0.0.
Deprecated since version NX5.0.0: Please use
NXOpen.SketchMirrorBuilder
instead.License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)
- centerline (
Print¶
-
Sketch.
Print
¶ Prints a representation of this object to the system log file.
Signature
Print()
New in version NX3.0.0.
License requirements: None.
Reattach¶
-
Sketch.
Reattach
¶ Reattaches a sketch.
For documentation for the parameters for this method, see the documentation for
NXOpen.SketchCollection.CreateSketch
Signature
Reattach(attachmentPlane, referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense, normalOrientation, localCoordinateSystemOrigin)
Parameters: - attachmentPlane (
NXOpen.ISurface
) – - referenceAxis (
NXOpen.IReferenceAxis
) – - referenceDirection (
NXOpen.Vector3d
) – - referenceAxisOrientation (
NXOpen.AxisOrientation
) – - referenceAxisSense (
NXOpen.Sense
) – - normalOrientation (
NXOpen.PlaneNormalOrientation
) – - localCoordinateSystemOrigin (
NXOpen.Point3d
) – Origin of the sketch’s local coordinate system
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- attachmentPlane (
RunAutoDimension¶
-
Sketch.
RunAutoDimension
¶ Run auto dimensioning.
Signature
RunAutoDimension()
New in version NX7.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
SetName¶
-
Sketch.
SetName
¶ Sets the custom name of the object.
NOTE: This method should not be used to edit a read-only object such as a Mirrored PMI object. If it is, the changes will be overridden when the part is updated.
Signature
SetName(name)
Parameters: name (str) – New in version NX3.0.0.
License requirements: None.
SetReferenceDirection¶
-
Sketch.
SetReferenceDirection
¶ Sets the reference direction of the sketch.
For documentation for the parameters for this method, see the documentation for
NXOpen.SketchCollection.CreateSketch
.Signature
SetReferenceDirection(referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense)
Parameters: - referenceAxis (
NXOpen.IReferenceAxis
) – - referenceDirection (
NXOpen.Vector3d
) – - referenceAxisOrientation (
NXOpen.AxisOrientation
) – - referenceAxisSense (
NXOpen.Sense
) –
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
- referenceAxis (
ShowDimensions¶
-
Sketch.
ShowDimensions
¶ Overloaded method ShowDimensions
ShowDimensions(inputObjects)
ShowDimensions()
ShowDimensions(objects)
-------------------------------------
Unblanks dimensions in the active sketch associated with the input sketch geometry
Signature
ShowDimensions(inputObjects)
Parameters: inputObjects (list of NXOpen.DisplayableObject
) – Geometry and groups in active sketchNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Unblanks all the dimensions of input sketch
Signature
ShowDimensions()
New in version NX6.0.1.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Unblanks dimensions in the active sketch associated with the input sketch geometry. This function can accept vertices.
Signature
ShowDimensions(objects)
Parameters: objects (list of NXOpen.SketchConstraintGeometry_Struct
) – Geometry and vertices in active sketchNew in version NX8.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Update¶
-
Sketch.
Update
¶ Overloaded method Update
Update()
Update(geoms)
-------------------------------------
Updates the sketch
Signature
Update()
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Updates the given set of geometries in the sketch
Signature
Update(geoms)
Parameters: geoms (list of NXOpen.NXObject
) – Geoms that need to be updatedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
UpdateConstraintDisplay¶
-
Sketch.
UpdateConstraintDisplay
¶ Overloaded method UpdateConstraintDisplay
UpdateConstraintDisplay()
UpdateConstraintDisplay(geoms)
-------------------------------------
Updates the constraint display without updating the sketch
Signature
UpdateConstraintDisplay()
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Updates the constraint display of given set of geoms without updating the sketch
Signature
UpdateConstraintDisplay(geoms)
Parameters: geoms (list of NXOpen.SmartObject
) – Geoms for which cons must be re-displayedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
UpdateDimensionDisplay¶
-
Sketch.
UpdateDimensionDisplay
¶ Overloaded method UpdateDimensionDisplay
UpdateDimensionDisplay()
UpdateDimensionDisplay(geoms)
UpdateDimensionDisplay(dims)
-------------------------------------
Updates the dimension display without updating the sketch
Signature
UpdateDimensionDisplay()
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Updates the dimension display of given set of geoms without updating the sketch
Signature
UpdateDimensionDisplay(geoms)
Parameters: geoms (list of NXOpen.SmartObject
) – Geoms for which cons must be re-displayedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Updates the dimension display of given set of dims without updating the sketch
Signature
UpdateDimensionDisplay(dims)
Parameters: dims (list of NXOpen.NXObject
) – Dims for which cons must be re-displayedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)
-------------------------------------
UpdateGeometryDisplay¶
-
Sketch.
UpdateGeometryDisplay
¶ Overloaded method UpdateGeometryDisplay
UpdateGeometryDisplay()
UpdateGeometryDisplay(geoms)
-------------------------------------
Updates the geometry display without updating the sketch
Signature
UpdateGeometryDisplay()
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------
Updates the geometry display of given set of geoms without updating the sketch
Signature
UpdateGeometryDisplay(geoms)
Parameters: geoms (list of NXOpen.SmartObject
) – Geoms for which cons must be re-displayedNew in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)
-------------------------------------