FeatureCollection Class¶

class NXOpen.Features.FeatureCollection¶

Bases: object

Represents a collection of features

To obtain an instance of this class, refer to NXOpen.BasePart

New in version NX3.0.0.

Properties¶

Property	Description
ActiveGroup	Returns the active feature group.
SheetmetalManager	Returns the Straight Brake Sheetmetal Manager for this part
AeroSheetmetalManager	Returns the aerospace sheet metal manager for this part
Dies	Returns the DieCollection instance belonging to this part
WeldManager	Returns the WeldManager for this part
AutomotiveCollection	Returns the AutomotiveCollection instance belonging to this part
ShipCollection	Returns the ShipCollection instance belonging to this part
ToolingCollection	Returns the ToolingCollection instance belonging to this part
SynchronousEdgeCollection	Returns the SynchronousEdgeCollection instance belonging to this part
SweepFeatureCollection	Returns the Sweep-like features collection belonging to this part
SynchronousCurveCollection	Returns the SynchronousCurveCollection instance belonging to this part
VehicleDesignCollection	Returns the VehicleDesignCollection instance belonging to this part
DesignFeatureCollection	Returns the DesignfeatureCollection instance belonging to this part
FreeformCurveCollection	Returns the FreeformCurveCollection instance belonging to this part
FreeformSurfaceCollection	Returns the FreeformSurfaceCollection instance belonging to this part
TrimFeatureCollection	Returns the TrimfeatureCollection instance belonging to this part
ToolingFeatureCollection	Returns the ToolingFeatureCollection instance belonging to this part
CustomAttributeCollection	Returns the CustomAttributeCollection instance belonging to this part
AeroCollection	Returns the AeroCollection instance belonging to this part
CurveFeatureCollection	Returns the CurveFeatureCollection instance belonging to this part
GeodesicSketchCollection	Returns the GeodesicSketchCollection instance belonging to this part
CustomFeatureDataCollection	Returns the CustomFeatureDataCollection instance belonging to this part
LatticeFeatureCollection	Returns the LatticeFeatureCollection instance belonging to this part

Methods¶

Method	Description
ConvertToFloatingFeatureGroups	Converts sequential feature groups to floating feature groups
ConvertToNewFeatureGroups	Converts to new feature groups
ConvertToSequentialFeatureGroups	Converts floating feature groups to sequential feature groups
CreateAdaptiveShellBuilder	Creates a `NXOpen.Features.AdaptiveShellBuilder`
CreateAdmMoveFaceBuilder	Creates a `NXOpen.Features.AdmMoveFaceBuilder`
CreateAdmOffsetRegionBuilder	Creates a `NXOpen.Features.AdmOffsetRegionBuilder`
CreateAdmResizeFaceBuilder	Creates a `NXOpen.Features.AdmResizeFaceBuilder`
CreateAestheticFaceBlendBuilder	Creates a `NXOpen.Features.AestheticFaceBlendBuilder`
CreateAnalyzePocketBuilder	Creates a `NXOpen.Features.AnalyzePocketBuilder`
CreateAngularDimensionBuilder	Creates a `NXOpen.Features.AngularDimBuilder`
CreateAocsBuilder	Creates an Offset In Face builder
CreateAssemblyCutBuilder	Creates a `NXOpen.Features.AssemblyCutBuilder`
CreateBlendPocketBuilder	Creates a `NXOpen.Features.BlendPocketBuilder`
CreateBlockFeatureBuilder	Creates a Block feature builder
CreateBodyByEquationBuilder	Creates a `NXOpen.Features.BodyByEquationBuilder`
CreateBooleanBuilder	Creates a Boolean builder
CreateBooleanBuilderUsingCollector	Creates a Boolean builder.
CreateBoundedPlaneBuilder	Creates a `NXOpen.Features.BoundedPlaneBuilder`
CreateBridgeCurveBuilder	Creates a `NXOpen.Features.BridgeCurveBuilder`
CreateBridgeCurveBuilderEx	Creates a `NXOpen.Features.BridgeCurveBuilderEx`
CreateBridgeSurfaceBuilder	Creates a `NXOpen.Features.BridgeSurfaceBuilder`
CreateChamferBuilder	Creates a Chamfer feature builder
CreateChangeShellThicknessBuilder	Creates a `NXOpen.Features.ChangeShellThicknessBuilder`
CreateCircularBlendCurveBuilder	Creates a `NXOpen.Features.CircularBlendCurveBuilder`
CreateCoaxialBuilder	Creates a `NXOpen.Features.CoaxialBuilder`
CreateColorFaceBuilder	Creates a `NXOpen.Features.ColorFaceBuilder`
CreateColorFeatureBuilder	Creates a `NXOpen.Features.ColorFeatureBuilder`
CreateColorFeatureGroupBuilder	Creates a `NXOpen.Features.ColorFeatureGroupBuilder`
CreateCombinedProjectionBuilder	Creates a `NXOpen.Features.CombinedProjectionBuilder`
CreateCompositeCurveBuilder	Creates a `NXOpen.Features.CompositeCurveBuilder`
CreateConcaveFacesBuilder	Creates a `NXOpen.Features.ConcaveFacesBuilder`
CreateConeBuilder	Creates a `NXOpen.Features.ConeBuilder`
CreateConvertFeatureGroupsToModulesBuilder	Creates a `NXOpen.GeometricUtilities.ConvertFeatureGroupsToModulesBuilder`
CreateCoplanarBuilder	Creates a coplanar builder, don’t use it until nx6
CreateCopyFaceBuilder	Creates a copy face builder
CreateCopyPasteBuilder	Creates a `NXOpen.Features.CopyPasteBuilder`
CreateCopyPasteBuilder2	Creates a `NXOpen.Features.CopyPasteBuilder`
CreateCurveOnSurfaceBuilder	Creates a Curve On Surface feature builder
CreateCurvelengthBuilder	Creates a Curvelength builder
CreateCustomFeatureBuilder	Creates a `Features.CustomFeatureBuilder`
CreateCutFaceBuilder	Creates a cut face builder
CreateCylinderBuilder	Creates a `NXOpen.Features.CylinderBuilder`
CreateDatumAxisBuilder	Creates a Datum Axis feature builder
CreateDatumCsysBuilder	Creates a Datum CSYS feature builder
CreateDatumPlaneBuilder	Creates a Datum Plane feature builder
CreateDeformDefinitionBuilder	Creates a `NXOpen.Features.DeformDefinitionBuilder`
CreateDeleteBodyBuilder	Creates a `NXOpen.Features.DeleteBodyBuilder`
CreateDeleteEdgeBuilder	Creates a `NXOpen.Features.DeleteEdgeBuilder`
CreateDeleteFaceBuilder	Creates a delete face builder, don’t use it until nx502
CreateDividefaceBuilder	Creates a Divideface builder
CreateDraftBodyBuilder	Creates a `NXOpen.Features.DraftBodyBuilder`
CreateDraftBuilder	Creates a draft builder
CreateDraftingSplineBuilder	Creates a Studio Spline builder for drafting
CreateEdgeBlendBuilder	Creates a Edge Blend feature builder
CreateEdgeSymmetryBuilder	Creates a `NXOpen.Features.EdgeSymmetryBuilder`
CreateEditCrossSectionBuilder	Creates a `NXOpen.Features.EditCrossSectionBuilder`
CreateEditDimensionBuilder	Creates a `NXOpen.Features.EditDimensionBuilder`
CreateEmbedManagerBuilder	Creates a `NXOpen.Features.EmbedManagerBuilder`
CreateEmbossBodyBuilder	Creates a `NXOpen.Features.EmbossBodyBuilder`
CreateEmbossBuilder	Creates an Emboss builder
CreateEnlargeBuilder	Creates an Enlarge builder
CreateExtensionBuilder	Creates a `NXOpen.Features.ExtensionBuilder`
CreateExtractFaceBuilder	Creates a `NXOpen.Features.ExtractFaceBuilder`
CreateExtrudeBuilder	Creates a Extrude builder
CreateFaceBlendBuilder	Creates a Face Blend feature builder
CreateFeatureReplayBuilder	Creates a `NXOpen.Features.FeatureReplayBuilder`
CreateFitCurveBuilder	Creates a `NXOpen.Features.FitCurveBuilder`
CreateFitSurfaceBuilder	Creates a `NXOpen.Features.FitSurfaceBuilder`
CreateFixedBuilder	Creates a `NXOpen.Features.FixedBuilder`
CreateFlowBlendBuilder	Creates a `Features.FlowBlendBuilder`
CreateFreeTransformerBuilder	Creates a `NXOpen.Features.FreeTransformerBuilder`
CreateGeneralConicBuilder	Creates a `NXOpen.Features.GeneralConicBuilder`
CreateGeomcopyBuilder	Creates a `NXOpen.Features.GeomcopyBuilder`
CreateGlobalShapingBuilder	Creates a `NXOpen.Features.GlobalShapingBuilder`
CreateGroupFaceBuilder	Creates a `NXOpen.Features.GroupFaceBuilder`
CreateGuidedExtensionBuilderEx	Creates a `NXOpen.Features.GuidedExtensionBuilderEx`
CreateHelixBuilder	Creates a `NXOpen.Features.HelixBuilder`
CreateHoleFeatureBuilder	Creates a Hole feature builder
CreateHolePackageBuilder	Creates a `NXOpen.Features.HolePackageBuilder`
CreateHoodVisibilityBuilder	Creates a `NXOpen.Features.VehicleDesign.HoodVisibilityBuilder`
CreateHumanBuilder	Creates a human feature builder.
CreateHumanPosturePredictionBuilder	Creates a human posture prediction builder.
CreateIformBuilder	Creates a `NXOpen.Features.IFormBuilder`
CreateInstanceFeatureBuilder	Creates `NXOpen.Features.InstanceFeatureBuilder`
CreateIntersectFeature	Creates an intersect feature.
CreateIntersectionCurveBuilder	Creates a `NXOpen.Features.IntersectionCurveBuilder`
CreateIsolateFeatureBuilder	Creates a `NXOpen.Features.IsolateFeatureBuilder`
CreateIsoparametricCurvesBuilder	Creates a `NXOpen.Features.IsoparametricCurvesBuilder`
CreateJoinCurvesBuilder	Creates a `NXOpen.Features.JoinCurvesBuilder`
CreateLabelChamferBuilder	Creates a `NXOpen.Features.LabelChamferBuilder`
CreateLabelNotchBlendBuilder	Creates a `NXOpen.Features.LabelNotchBlendBuilder`
CreateLawCurveBuilder	Creates a `NXOpen.Features.LawCurveBuilder`
CreateLawExtensionBuilder	Creates a `NXOpen.Features.LawExtensionBuilder`
CreateLawExtensionBuilderEx	Creates a `NXOpen.Features.LawExtensionBuilderEx`
CreateLinearDimensionBuilder	Creates a `NXOpen.Features.LinearDimensionBuilder`
CreateLinkedFacetBuilder	Creates a `NXOpen.Features.LinkedFacetBuilder`
CreateMakeOffsetBuilder	Creates a `NXOpen.Features.MakeOffsetBuilder`
CreateMapleBuilder	Creates a `NXOpen.Features.MapleBuilder`
CreateMasterCutBuilder	Create a Master Cut builder
CreateMatchEdgeBuilder	Creates a `NXOpen.Features.MatchEdgeBuilder`
CreateMathIntegrationBuilder	Creates a `NXOpen.Features.MathIntegrationBuilder`
CreateMeshSurfaceBuilder	Creates a Mesh Surface feature builder
CreateMeshTransformerBuilder	Creates a `NXOpen.Features.MeshTransformerBuilder`
CreateMidSurfaceByFacePairsBuilder	Creates a `NXOpen.Features.MidSurfaceByFacePairsBuilder`
CreateMidSurfaceUserDefinedBuilder	Creates a `NXOpen.Features.MidSurfaceUserDefinedBuilder`
CreateMirrorBodyBuilder	Creates a `NXOpen.Features.MirrorBodyBuilder`
CreateMirrorBuilder	Creates `NXOpen.Features.MirrorBuilder`
CreateMirrorCurveBuilder	Creates a `NXOpen.Features.MirrorCurveBuilder`
CreateMirrorFaceBuilder	Creates a mirror face builder
CreateMirrorFeatureBuilder	Creates `NXOpen.Features.MirrorFeatureBuilder`
CreateMoveFaceBuilder	Create a move face builder, don’t use it until nx502
CreateNSidedSurfaceBuilder	Creates a `NXOpen.Features.NSidedSurfaceBuilder`
CreateNestModuleBuilder	Creates a `NXOpen.GeometricUtilities.NestModuleBuilder`
CreateOffsetCurveBuilder	Creates a `NXOpen.Features.OffsetCurveBuilder`
CreateOffsetEmbossBuilder	Creates a Offsetemboss builder
CreateOffsetFaceBuilder	Creates a `NXOpen.Features.OffsetFaceBuilder`
CreateOffsetRegionBuilder	Creates an offset region builder, don’t use it until nx502
CreateOffsetSurfaceBuilder	Creates an Offset Surface builder
CreateOptimizeCurveBuilder	Creates a `NXOpen.Features.OptimizeCurveBuilder`
CreateOptimizeFaceBuilder	Creates a `NXOpen.Features.OptimizeFaceBuilder`
CreateOvercrownFeatureBuilder	Creates a Overcrown feature builder
CreatePaintParametersBuilder	Creates a `NXOpen.Features.PaintParametersBuilder`
CreateParallelBuilder	Creates a `NXOpen.Features.ParallelBuilder`
CreatePartModuleBuilder	Creates a `NXOpen.Features.PartModuleBuilder`
CreatePartModuleRelationshipBuilder	Creates a `NXOpen.GeometricUtilities.PartModuleRelationshipBuilder`
CreatePasteFaceBuilder	Creates a paste face builder
CreatePatchBuilder	Creates a `NXOpen.Features.PatchBuilder`
CreatePatchOpeningsBuilder	Creates a `NXOpen.Features.PatchOpeningsBuilder`
CreatePatternFaceBuilder	Creates a pattern face builder, don’t use it until nx502
CreatePatternFaceFeatureBuilder	Creates a `NXOpen.Features.PatternFaceFeatureBuilder`
CreatePatternFeatureBuilder	Creates `NXOpen.Features.PatternFeatureBuilder`
CreatePatternGeometryBuilder	Creates a `NXOpen.Features.PatternGeometryBuilder`
CreatePedestrianProtectionBuilder	Creates a `NXOpen.Features.VehicleDesign.PedestrianProtectionBuilder`
CreatePerpendicularBuilder	Creates a `NXOpen.Features.PerpendicularBuilder`
CreatePointSetBuilder	Creates a `NXOpen.Features.PointSetBuilder`
CreatePoleSmoothingBuilder	Creates a `NXOpen.Features.PoleSmoothingBuilder`
CreateProjectCurveBuilder	Creates a `NXOpen.Features.ProjectCurveBuilder`
CreatePromotionBuilder	Creates a `NXOpen.Features.PromotionBuilder`
CreatePullFaceBuilder	Creates a `NXOpen.Features.PullFaceBuilder`
CreateRadialDimensionBuilder	Creates a `NXOpen.Features.RadialDimensionBuilder`
CreateRapidSurfaceBuilder	Creates a Rapid Surfacing feature builder
CreateRasterImage	Creates a raster image
CreateReferenceMapperBuilder	Creates a `NXOpen.Features.ReferenceMapperBuilder`
CreateRefitFaceBuilder	Creates a RefitFaceBuilder
CreateReflectionDataBuilder	Creates a `NXOpen.Features.VehicleDesign.ReflectionDataBuilder`
CreateRemoveParametersBuilder	Creates a `NXOpen.Features.RemoveParametersBuilder`
CreateRenameLinkedPartModulePartBuilder	Creates a `NXOpen.GeometricUtilities.RenameLinkedPartModulePartBuilder`
CreateRenewFeatureBuilder	Creates a `NXOpen.GeometricUtilities.RenewFeatureBuilder`
CreateReorderBlendsBuilder	Creates a `NXOpen.Features.ReorderBlendsBuilder`
CreateReplaceBlendBuilder	Creates a `NXOpen.Features.ReplaceBlendBuilder`
CreateReplaceFaceBuilder	Creates a replace face builder, don’t use it until nx502
CreateReplaceFeatureBuilder	Creates a `NXOpen.Features.ReplaceFeatureBuilder`
CreateResizeBlendBuilder	Creates a resize blend builder, don’t use it until nx502
CreateResizeChamferBuilder	Creates a `NXOpen.Features.ResizeChamferBuilder`
CreateResizeFaceBuilder	Creates a resize face builder, don’t use it until nx502
CreateResizePlaneBuilder	Creates a Resize Datum Plane feature builder
CreateRevolveBuilder	Creates a Revolve builder
CreateRibbonBuilder	Creates a ribbon builder
CreateRpoBuilder	Creates a Relative Positioning Object builder
CreateRuledBuilder	Creates a Ruled Surface builder
CreateScaleBuilder	Creates a `NXOpen.Features.ScaleBuilder`
CreateSeatBeltAnchorageBuilder	Creates a `NXOpen.Features.VehicleDesign.SeatBeltAnchorageBuilder`
CreateSectionCurveBuilder	Creates a `NXOpen.Features.SectionCurveBuilder`
CreateSectionEditBuilder	Creates a `NXOpen.Features.SectionEditBuilder`
CreateSectionInertiaAnalysisBuilder	Creates a `NXOpen.Features.SectionInertiaAnalysisBuilder`
CreateSectionSurfaceBuilder	Create a section surface
CreateSectionSurfaceBuilderEx	Creates a `NXOpen.Features.SectionSurfaceBuilderEx`
CreateSewBuilder	Creates a Sew feature builder
CreateShellBuilder	Creates an Shell builder
CreateShellFaceBuilder	Creates a `NXOpen.Features.ShellFaceBuilder`
CreateShowRelatedFacesBuilder	Creates a `NXOpen.Features.ShowRelatedFacesBuilder`
CreateSilhouetteFlangeBuilder	Creates a `NXOpen.Features.SilhouetteFlangeBuilder`
CreateSketchFitCurveBuilder	Creates a `NXOpen.Features.SketchFitCurveBuilder`
CreateSketchSplineBuilder	Creates a Studio Spline builder for sketcher
CreateSmoothSplineBuilder	Creates a `NXOpen.Features.SmoothSplineBuilder`
CreateSnipSurfaceBuilder	Creates a `NXOpen.Features.SnipSurfaceBuilder`
CreateSphereBuilder	Creates a `NXOpen.Features.SphereBuilder`
CreateSphericalCornerBuilder	Creates a `NXOpen.Features.SphericalCornerBuilder`
CreateSplitBodyBuilder	Creates a `NXOpen.Features.SplitBodyBuilder`
CreateSplitBodyBuilderUsingCollector	Creates a `NXOpen.Features.SplitBodyBuilder`.
CreateStudioSplineBuilder	Creates a Studio Spline builder
CreateStudioSplineBuilderEx	Creates a Studio Spline builder
CreateStudioSurfaceBuilder	Creates a Studio Surface Builder
CreateStudioXformBuilder	Creates a Features.
CreateStudioXformBuilderEx	Creates a Features.
CreateStyledBlendBuilder	Creates a `NXOpen.Features.StyledBlendBuilder`
CreateStyledCornerBuilder	Creates a `NXOpen.Features.StyledCornerBuilder`
CreateStyledSweepBuilder	Creates a `NXOpen.Features.StyledSweepBuilder`
CreateSubtractFeature	Creates a subtract feature.
CreateSweepAlongGuideBuilder	Creates a `NXOpen.Features.SweepAlongGuideBuilder`
CreateSweptBuilder	Creates a `NXOpen.Features.SweptBuilder`
CreateSymmetricBuilder	Creates a `NXOpen.Features.SymmetricBuilder`
CreateTangentBuilder	Creates a `NXOpen.Features.TangentBuilder`
CreateTextBuilder	Creates a `NXOpen.Features.TextBuilder`
CreateThickenBuilder	Creates a Thicken feature builder
CreateThroughCurveMeshBuilder	Creates a `NXOpen.Features.ThroughCurveMeshBuilder`
CreateThroughCurvesBuilder	Creates a `NXOpen.Features.ThroughCurvesBuilder`
CreateTrimBody2Builder	Creates a `NXOpen.Features.TrimBody2Builder` for Trim Body feature
CreateTrimBodyBuilder	Creates a trim body builder object.
CreateTrimCurve2FeatureBuilder	Creates a `NXOpen.Features.TrimCurve2Builder`
CreateTrimCurveBuilder	Creates a `NXOpen.Features.TrimCurveBuilder`
CreateTrimExtendBuilder	Creates a `NXOpen.Features.TrimExtendBuilder`
CreateTrimsheetBuilder	Creates a `NXOpen.Features.TrimSheetBuilder`
CreateTubeBuilder	Creates a `NXOpen.Features.TubeBuilder`
CreateUniteFeature	Creates a unite feature.
CreateUnnestModuleBuilder	Creates a `NXOpen.GeometricUtilities.UnnestModuleBuilder`
CreateUnsewBuilder	Creates a `NXOpen.Features.UnsewBuilder`
CreateUntrimBuilder	Creates a `NXOpen.Features.UntrimBuilder`
CreateUserDefinedObjectFeatureBuilder	Creates a UserDefinedObjectFeature builder
CreateVarOffsetFaceBuilder	Creates a `NXOpen.Features.VarOffsetFaceBuilder`
CreateVariableOffsetBuilder	Creates a `NXOpen.Features.VariableOffsetBuilder`
CreateVarsweepBuilder	Creates a Varsweep feature builder
CreateVehicleCoordinateSystemBuilder	Creates a `NXOpen.Features.VehicleDesign.VehicleCoordinateSystemBuilder`
CreateVirtualBlendEdgeBuilder	Creates a `NXOpen.Features.VirtualBlendEdgeBuilder`
CreateVirtualCurveBuilder	Creates a `NXOpen.Features.VirtualCurveBuilder`
CreateVisionPlaneBuilder	Creates a `NXOpen.Features.VehicleDesign.VisionPlaneBuilder`
CreateWaveDatumBuilder	Creates a Wavedatum Builder
CreateWavePointBuilder	Creates a `NXOpen.Features.WavePointBuilder`
CreateWaveRoutingBuilder	Creates a `NXOpen.Features.WaveRoutingBuilder`
CreateWaveSketchBuilder	Creates a Wavesketch Builder
CreateWindshieldDatumBuilder	Creates a `NXOpen.Features.VehicleDesign.WindshieldDatumBuilder`
CreateWrapBuilder	Creates a `NXOpen.Features.WrapBuilder`
CreateWrapGeometryBuilder	Creates a `NXOpen.Features.WrapGeometryBuilder`
DeleteAllPartInformationalFeatureAlerts	Delete all informational alerts from all the features in a given part
DeleteInformationalAlerts	Delete all informational alerts from the features and if numFrecs is 0 then delete informational alerts from all features in the part
DeleteWarningAlerts	Delete all warning alerts from the features and if numFrecs is 0 then delete warning alerts from all features in the part
FindObject	Finds the `NXOpen.Features` with the given identifier as recorded in a journal.
GetAllPartFeaturesWithAlerts	Returns a list of all features from a given part that have update alerts
GetAssociatedFeature	Get the feature associated with an object
GetAssociatedFeaturesOfBody	Returns all features that are associated with this body
GetAssociatedFeaturesOfEdge	Returns all features that are associated with the faces of this edge
GetAssociatedFeaturesOfFace	Returns all features associated with this face
GetFeatures	Returns all the features in the part.
GetIsMasterCutVisibleInView	Returns if a `NXOpen.Features.MasterCutBuilder` is visible in specified `NXOpen.CutView` .
GetParentFeatureOfBody	Returns the feature that created this body.
GetParentFeatureOfFace	Returns the feature that created this face
GetParentFeaturesOfEdge	Returns the features that created the faces of this edge.
GetPartFeaturesWithNewAlerts	Returns a list of features that generated update alerts during recent update
InsertNewDesignGroup	Creates a new empty design group after a specified referece design group
ReorderFeature	Reorders the Feature with respect to the given feature
ReorganizeFeature	Reorganizes the Feature with respect to the given feature across the part module
ReplaceWithIndependentSketch	Replace the given features with Independent Sketch
SetCanResetMcf	Sets whether mcf is allowed
SetEditWithRollbackFeature	Sets the feature being edited with rollback
StartEditWithRollbackManager	Creates a `NXOpen.Features.EditWithRollbackManager`
SuppressFeatures	Suppress the given features
UnsuppressFeatures	Unsuppress the given features

Enumerations¶

FeatureCollectionReorderType Enumeration

Reorder operation type.

Property Detail¶

ActiveGroup¶

FeatureCollection.ActiveGroup¶

Returns the active feature group.

-------------------------------------

Getter Method

Signature ActiveGroup

Returns:
Return type:	`NXOpen.Features.FeatureGroup`

New in version NX7.5.1.

License requirements: None.

SheetmetalManager¶

FeatureCollection.SheetmetalManager¶

Returns the Straight Brake Sheetmetal Manager for this part

Signature SheetmetalManager

New in version NX3.0.0.

Returns:
Return type:	`NXOpen.Features.SheetMetal.SheetmetalManager`

AeroSheetmetalManager¶

FeatureCollection.AeroSheetmetalManager¶

Returns the aerospace sheet metal manager for this part

Signature AeroSheetmetalManager

New in version NX3.0.0.

Returns:
Return type:	`NXOpen.Features.SheetMetal.AeroSheetmetalManager`

Dies¶

FeatureCollection.Dies¶

Returns the DieCollection instance belonging to this part

Signature Dies

New in version NX3.0.0.

Returns:
Return type:	`NXOpen.Die.DieCollection`

WeldManager¶

FeatureCollection.WeldManager¶

Returns the WeldManager for this part

Signature WeldManager

New in version NX3.0.0.

Returns:
Return type:	`NXOpen.Weld.WeldManager`

AutomotiveCollection¶

FeatureCollection.AutomotiveCollection¶

Returns the AutomotiveCollection instance belonging to this part

Signature AutomotiveCollection

New in version NX7.5.0.

Returns:
Return type:	`NXOpen.Features.AutomotiveCollection`

ShipCollection¶

FeatureCollection.ShipCollection¶

Returns the ShipCollection instance belonging to this part

Signature ShipCollection

New in version NX8.0.0.

Returns:
Return type:	`NXOpen.Features.ShipCollection`

ToolingCollection¶

FeatureCollection.ToolingCollection¶

Returns the ToolingCollection instance belonging to this part

Signature ToolingCollection

New in version NX8.5.0.

Returns:
Return type:	`NXOpen.Features.ToolingCollection`

SynchronousEdgeCollection¶

FeatureCollection.SynchronousEdgeCollection¶

Returns the SynchronousEdgeCollection instance belonging to this part

Signature SynchronousEdgeCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.SynchronousEdgeCollection`

SweepFeatureCollection¶

FeatureCollection.SweepFeatureCollection¶

Returns the Sweep-like features collection belonging to this part

Signature SweepFeatureCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.SweepFeatureCollection`

SynchronousCurveCollection¶

FeatureCollection.SynchronousCurveCollection¶

Returns the SynchronousCurveCollection instance belonging to this part

Signature SynchronousCurveCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.SynchronousCurveCollection`

VehicleDesignCollection¶

FeatureCollection.VehicleDesignCollection¶

Returns the VehicleDesignCollection instance belonging to this part

Signature VehicleDesignCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.VehicleDesignCollection`

DesignFeatureCollection¶

FeatureCollection.DesignFeatureCollection¶

Returns the DesignfeatureCollection instance belonging to this part

Signature DesignFeatureCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.DesignFeatureCollection`

FreeformCurveCollection¶

FeatureCollection.FreeformCurveCollection¶

Returns the FreeformCurveCollection instance belonging to this part

Signature FreeformCurveCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.FreeformCurveCollection`

FreeformSurfaceCollection¶

FeatureCollection.FreeformSurfaceCollection¶

Returns the FreeformSurfaceCollection instance belonging to this part

Signature FreeformSurfaceCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.FreeformSurfaceCollection`

TrimFeatureCollection¶

FeatureCollection.TrimFeatureCollection¶

Returns the TrimfeatureCollection instance belonging to this part

Signature TrimFeatureCollection

New in version NX9.0.0.

Returns:
Return type:	`NXOpen.Features.TrimFeatureCollection`

ToolingFeatureCollection¶

FeatureCollection.ToolingFeatureCollection¶

Returns the ToolingFeatureCollection instance belonging to this part

Signature ToolingFeatureCollection

New in version NX10.0.0.

Returns:
Return type:	`NXOpen.Features.ToolingFeatureCollection`

CustomAttributeCollection¶

FeatureCollection.CustomAttributeCollection¶

Returns the CustomAttributeCollection instance belonging to this part

Signature CustomAttributeCollection

New in version NX11.0.0.

Returns:
Return type:	`NXOpen.Features.CustomAttributeCollection`

AeroCollection¶

FeatureCollection.AeroCollection¶

Returns the AeroCollection instance belonging to this part

Signature AeroCollection

New in version NX10.0.0.

Returns:
Return type:	`NXOpen.Features.AeroCollection`

CurveFeatureCollection¶

FeatureCollection.CurveFeatureCollection¶

Returns the CurveFeatureCollection instance belonging to this part

Signature CurveFeatureCollection

New in version NX10.0.0.

Returns:
Return type:	`NXOpen.Features.CurveFeatureCollection`

GeodesicSketchCollection¶

FeatureCollection.GeodesicSketchCollection¶

Returns the GeodesicSketchCollection instance belonging to this part

Signature GeodesicSketchCollection

New in version NX10.0.0.

Returns:
Return type:	`NXOpen.Features.GeodesicSketchCollection`

CustomFeatureDataCollection¶

FeatureCollection.CustomFeatureDataCollection¶

Returns the CustomFeatureDataCollection instance belonging to this part

Signature CustomFeatureDataCollection

New in version NX11.0.0.

Returns:
Return type:	`NXOpen.Features.CustomFeatureDataCollection`

LatticeFeatureCollection¶

FeatureCollection.LatticeFeatureCollection¶

Returns the LatticeFeatureCollection instance belonging to this part

Signature LatticeFeatureCollection

New in version NX11.0.2.

Returns:
Return type:	`NXOpen.Features.LatticeFeatureCollection`

Method Detail¶

ConvertToFloatingFeatureGroups¶

FeatureCollection.ConvertToFloatingFeatureGroups¶

Converts sequential feature groups to floating feature groups

Signature ConvertToFloatingFeatureGroups()

New in version NX7.5.3.

License requirements: solid_modeling (“SOLIDS MODELING”)

ConvertToNewFeatureGroups¶

FeatureCollection.ConvertToNewFeatureGroups¶

Converts to new feature groups

Signature ConvertToNewFeatureGroups()

New in version NX7.5.1.

Deprecated since version NX8.0.0: Use NXOpen.Features.FeatureCollection.ConvertToSequentialFeatureGroups() or NXOpen.Features.FeatureCollection.ConvertToFloatingFeatureGroups() instead.

License requirements: solid_modeling (“SOLIDS MODELING”)

ConvertToSequentialFeatureGroups¶

FeatureCollection.ConvertToSequentialFeatureGroups¶

Converts floating feature groups to sequential feature groups

Signature ConvertToSequentialFeatureGroups()

New in version NX7.5.3.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateAdaptiveShellBuilder¶

FeatureCollection.CreateAdaptiveShellBuilder¶

Creates a NXOpen.Features.AdaptiveShellBuilder

Signature CreateAdaptiveShellBuilder(shellFace)

Parameters:	shellFace (`NXOpen.Features.AdaptiveShell`) – `NXOpen.Features.AdaptiveShell` to be edited
Returns:	`NXOpen.Features.AdaptiveShellBuilder` object
Return type:	`NXOpen.Features.AdaptiveShellBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAdmMoveFaceBuilder¶

FeatureCollection.CreateAdmMoveFaceBuilder¶

Creates a NXOpen.Features.AdmMoveFaceBuilder

Signature CreateAdmMoveFaceBuilder(admMoveFace)

Parameters:	admMoveFace (`NXOpen.Features.AdmMoveFace`) – `NXOpen.Features.AdmMoveFace` to be edited
Returns:
Return type:	`NXOpen.Features.AdmMoveFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAdmOffsetRegionBuilder¶

FeatureCollection.CreateAdmOffsetRegionBuilder¶

Creates a NXOpen.Features.AdmOffsetRegionBuilder

Signature CreateAdmOffsetRegionBuilder(offsetRegion)

Parameters:	offsetRegion (`NXOpen.Features.AdmOffsetRegion`) – `NXOpen.Features.AdmOffsetRegion` to be edited
Returns:	Features.

AdmOffsetRegionBuilder object :rtype: NXOpen.Features.AdmOffsetRegionBuilder

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAdmResizeFaceBuilder¶

FeatureCollection.CreateAdmResizeFaceBuilder¶

Creates a NXOpen.Features.AdmResizeFaceBuilder

Signature CreateAdmResizeFaceBuilder(admResizeFace)

Parameters:	admResizeFace (`NXOpen.Features.AdmResizeFace`) – `NXOpen.Features.AdmResizeFace` to be edited
Returns:
Return type:	`NXOpen.Features.AdmResizeFaceBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAestheticFaceBlendBuilder¶

FeatureCollection.CreateAestheticFaceBlendBuilder¶

Creates a NXOpen.Features.AestheticFaceBlendBuilder

Signature CreateAestheticFaceBlendBuilder(aestheticFaceBlend)

Parameters:	aestheticFaceBlend (`NXOpen.Features.AestheticFaceBlend`) – `NXOpen.Features.AestheticFaceBlend` to be edited
Returns:
Return type:	`NXOpen.Features.AestheticFaceBlendBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateAnalyzePocketBuilder¶

FeatureCollection.CreateAnalyzePocketBuilder¶

Creates a NXOpen.Features.AnalyzePocketBuilder

Signature CreateAnalyzePocketBuilder(analyzePocket)

Parameters:	analyzePocket (`NXOpen.Features.AnalyzePocket`) – `NXOpen.Features.AnalyzePocket` to be edited
Returns:	AnalyzePocketBuilder object
Return type:	`NXOpen.Features.AnalyzePocketBuilder`

New in version NX9.0.0.

License requirements: features_modeling (“FEATURES MODELING”)

CreateAngularDimensionBuilder¶

FeatureCollection.CreateAngularDimensionBuilder¶

Creates a NXOpen.Features.AngularDimBuilder

Signature CreateAngularDimensionBuilder(angularDimension)

Parameters:	angularDimension (`NXOpen.Features.AngularDim`) – `NXOpen.Features.AngularDim` to be edited
Returns:
Return type:	`NXOpen.Features.AngularDimBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAocsBuilder¶

FeatureCollection.CreateAocsBuilder¶

Creates an Offset In Face builder

Signature CreateAocsBuilder(aocs)

Parameters:	aocs (`NXOpen.Features.Feature`) – `NXOpen.Features.AOCSBuilder` to be edited
Returns:	AOCSBuilder object
Return type:	`NXOpen.Features.AOCSBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateAssemblyCutBuilder¶

FeatureCollection.CreateAssemblyCutBuilder¶

Creates a NXOpen.Features.AssemblyCutBuilder

Signature CreateAssemblyCutBuilder(assemblyCut)

Parameters:	assemblyCut (`NXOpen.Features.AssemblyCut`) – `NXOpen.Features.AssemblyCut` to be edited
Returns:	Features.

AssemblyCutBuilder object :rtype: NXOpen.Features.AssemblyCutBuilder

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateBlendPocketBuilder¶

FeatureCollection.CreateBlendPocketBuilder¶

Creates a NXOpen.Features.BlendPocketBuilder

Signature CreateBlendPocketBuilder(blendPocket)

Parameters:	blendPocket (`NXOpen.Features.BlendPocket`) – `NXOpen.Features.BlendPocket` to be edited
Returns:	BlendPocketBuilder object
Return type:	`NXOpen.Features.BlendPocketBuilder`

New in version NX9.0.0.

License requirements: features_modeling (“FEATURES MODELING”)

CreateBlockFeatureBuilder¶

FeatureCollection.CreateBlockFeatureBuilder¶

Creates a Block feature builder

Signature CreateBlockFeatureBuilder(block)

Parameters:	block (`NXOpen.Features.Feature`) – `NXOpen.Features.Block` to be edited
Returns:	BlockFeatureBuilder object
Return type:	`NXOpen.Features.BlockFeatureBuilder`

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateBodyByEquationBuilder¶

FeatureCollection.CreateBodyByEquationBuilder¶

Creates a NXOpen.Features.BodyByEquationBuilder

Signature CreateBodyByEquationBuilder(facetBodyByEquation)

Parameters:	facetBodyByEquation (`NXOpen.Features.BodyByEquation`) – `NXOpen.Features.BodyByEquation` to be edited
Returns:
Return type:	`NXOpen.Features.BodyByEquationBuilder`

New in version NX12.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateBooleanBuilder¶

FeatureCollection.CreateBooleanBuilder¶

Creates a Boolean builder

Signature CreateBooleanBuilder(booleanFeature)

Parameters:	booleanFeature (`NXOpen.Features.BooleanFeature`) – `NXOpen.Features.BooleanFeature` to be edited
Returns:	BooleanBuilder object
Return type:	`NXOpen.Features.BooleanBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateBooleanBuilderUsingCollector¶

FeatureCollection.CreateBooleanBuilderUsingCollector¶

Creates a Boolean builder.

Leverage body collectors if possible

Signature CreateBooleanBuilderUsingCollector(booleanFeature)

Parameters:	booleanFeature (`NXOpen.Features.BooleanFeature`) – `NXOpen.Features.BooleanFeature` to be edited
Returns:	BooleanBuilder object
Return type:	`NXOpen.Features.BooleanBuilder`

New in version NX7.5.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateBoundedPlaneBuilder¶

FeatureCollection.CreateBoundedPlaneBuilder¶

Creates a NXOpen.Features.BoundedPlaneBuilder

Signature CreateBoundedPlaneBuilder(boundedPlane)

Parameters:	boundedPlane (`NXOpen.Features.BoundedPlane`) – `NXOpen.Features.BoundedPlane` to be edited
Returns:	Features.

BoundedPlaneBuilder object :rtype: NXOpen.Features.BoundedPlaneBuilder

New in version NX6.0.0.

License requirements: nx_freeform_1 (“basic freeform modeling”)

CreateBridgeCurveBuilder¶

FeatureCollection.CreateBridgeCurveBuilder¶

Creates a NXOpen.Features.BridgeCurveBuilder

Signature CreateBridgeCurveBuilder(bridgeCurve)

Parameters:	bridgeCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.BridgeCurve` to be edited
Returns:
Return type:	`NXOpen.Features.BridgeCurveBuilder`

New in version NX5.0.0.

Deprecated since version NX8.5.0: Use NXOpen.Features.FeatureCollection.CreateBridgeCurveBuilderEx() instead.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateBridgeCurveBuilderEx¶

FeatureCollection.CreateBridgeCurveBuilderEx¶

Creates a NXOpen.Features.BridgeCurveBuilderEx

Signature CreateBridgeCurveBuilderEx(bridgeCurve)

Parameters:	bridgeCurve (`NXOpen.Features.BridgeCurve`) – `NXOpen.Features.BridgeCurve` to be edited
Returns:
Return type:	`NXOpen.Features.BridgeCurveBuilderEx`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR nx_freeform_1 (“basic freeform modeling”)

CreateBridgeSurfaceBuilder¶

FeatureCollection.CreateBridgeSurfaceBuilder¶

Creates a NXOpen.Features.BridgeSurfaceBuilder

Signature CreateBridgeSurfaceBuilder(bridgeSurface)

Parameters:	bridgeSurface (`NXOpen.Features.BridgeSurface`) – `NXOpen.Features.BridgeSurface` to be edited
Returns:
Return type:	`NXOpen.Features.BridgeSurfaceBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateChamferBuilder¶

FeatureCollection.CreateChamferBuilder¶

Creates a Chamfer feature builder

Signature CreateChamferBuilder(chamfer)

Parameters:	chamfer (`NXOpen.Features.Feature`) – Chamfer to be edited, if None then create a new one
Returns:	ChamferBuilder object
Return type:	`NXOpen.Features.ChamferBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateChangeShellThicknessBuilder¶

FeatureCollection.CreateChangeShellThicknessBuilder¶

Creates a NXOpen.Features.ChangeShellThicknessBuilder

Signature CreateChangeShellThicknessBuilder(shellFace)

Parameters:	shellFace (`NXOpen.Features.ChangeShellThickness`) – `NXOpen.Features.ChangeShellThickness` to be edited
Returns:	`NXOpen.Features.ChangeShellThicknessBuilder` object
Return type:	`NXOpen.Features.ChangeShellThicknessBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateCircularBlendCurveBuilder¶

FeatureCollection.CreateCircularBlendCurveBuilder¶

Creates a NXOpen.Features.CircularBlendCurveBuilder

Signature CreateCircularBlendCurveBuilder(circularBlendCurve)

Parameters:	circularBlendCurve (`NXOpen.Features.CircularBlendCurve`) – `NXOpen.Features.CircularBlendCurve` to be edited, , if None then create a new one
Returns:	CircularBlendCurveBuilder object
Return type:	`NXOpen.Features.CircularBlendCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCoaxialBuilder¶

FeatureCollection.CreateCoaxialBuilder¶

Creates a NXOpen.Features.CoaxialBuilder

Signature CreateCoaxialBuilder(coaxial)

Parameters:	coaxial (`NXOpen.Features.Coaxial`) – `NXOpen.Features.Coaxial` to be edited
Returns:	Features.

CoaxialBuilder object :rtype: NXOpen.Features.CoaxialBuilder

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateColorFaceBuilder¶

FeatureCollection.CreateColorFaceBuilder¶

Creates a NXOpen.Features.ColorFaceBuilder

Signature CreateColorFaceBuilder()

Returns:
Return type:	`NXOpen.Features.ColorFaceBuilder`

New in version NX7.0.0.

License requirements: None.

CreateColorFeatureBuilder¶

FeatureCollection.CreateColorFeatureBuilder¶

Creates a NXOpen.Features.ColorFeatureBuilder

Signature CreateColorFeatureBuilder()

Returns:
Return type:	`NXOpen.Features.ColorFeatureBuilder`

New in version NX8.5.0.

License requirements: None.

CreateColorFeatureGroupBuilder¶

FeatureCollection.CreateColorFeatureGroupBuilder¶

Creates a NXOpen.Features.ColorFeatureGroupBuilder

Signature CreateColorFeatureGroupBuilder()

Returns:
Return type:	`NXOpen.Features.ColorFeatureGroupBuilder`

New in version NX8.5.0.

License requirements: None.

CreateCombinedProjectionBuilder¶

FeatureCollection.CreateCombinedProjectionBuilder¶

Creates a NXOpen.Features.CombinedProjectionBuilder

Signature CreateCombinedProjectionBuilder(combinedProjection)

Parameters:	combinedProjection (`NXOpen.Features.CombinedProjection`) – `NXOpen.Features.CombinedProjection` to be edited
Returns:
Return type:	`NXOpen.Features.CombinedProjectionBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCompositeCurveBuilder¶

FeatureCollection.CreateCompositeCurveBuilder¶

Creates a NXOpen.Features.CompositeCurveBuilder

Signature CreateCompositeCurveBuilder(compositeCurve)

Parameters:	compositeCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.

CompositeCurveBuilder object :rtype: NXOpen.Features.CompositeCurveBuilder

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateConcaveFacesBuilder¶

FeatureCollection.CreateConcaveFacesBuilder¶

Creates a NXOpen.Features.ConcaveFacesBuilder

Signature CreateConcaveFacesBuilder(concaveFaces)

Parameters:	concaveFaces (`NXOpen.Features.ConcaveFaces`) – `NXOpen.Features.ConcaveFaces` to be edited
Returns:
Return type:	`NXOpen.Features.ConcaveFacesBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateConeBuilder¶

FeatureCollection.CreateConeBuilder¶

Creates a NXOpen.Features.ConeBuilder

Signature CreateConeBuilder(cone)

Parameters:	cone (`NXOpen.Features.Cone`) – `NXOpen.Features.Cone` to be edited
Returns:
Return type:	`NXOpen.Features.ConeBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateConvertFeatureGroupsToModulesBuilder¶

FeatureCollection.CreateConvertFeatureGroupsToModulesBuilder¶

Creates a NXOpen.GeometricUtilities.ConvertFeatureGroupsToModulesBuilder

Signature CreateConvertFeatureGroupsToModulesBuilder()

Returns:
Return type:	`NXOpen.GeometricUtilities.ConvertFeatureGroupsToModulesBuilder`

New in version NX9.0.0.

License requirements: usr_defined_features (“USER DEFINED FEATURES”)

CreateCoplanarBuilder¶

FeatureCollection.CreateCoplanarBuilder¶

Creates a coplanar builder, don’t use it until nx6

Signature CreateCoplanarBuilder(coplanar)

Parameters:	coplanar (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.CoplanarBuilder object
Return type:	`NXOpen.Features.CoplanarBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateCopyFaceBuilder¶

FeatureCollection.CreateCopyFaceBuilder¶

Creates a copy face builder

Signature CreateCopyFaceBuilder(copyFace)

Parameters:	copyFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.CopyFaceBuilder object
Return type:	`NXOpen.Features.CopyFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateCopyPasteBuilder¶

FeatureCollection.CreateCopyPasteBuilder¶

Creates a NXOpen.Features.CopyPasteBuilder

Signature CreateCopyPasteBuilder(features)

Parameters:	features (list of `NXOpen.NXObject`) – Features to be copy/paste
Returns:	CopyPasteBuilder
Return type:	`NXOpen.Features.CopyPasteBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCopyPasteBuilder2¶

FeatureCollection.CreateCopyPasteBuilder2¶

Creates a NXOpen.Features.CopyPasteBuilder

Signature CreateCopyPasteBuilder2(features)

Parameters:	features (list of `NXOpen.NXObject`) – Features to be copy/paste
Returns:	CopyPasteBuilder
Return type:	`NXOpen.Features.CopyPasteBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCurveOnSurfaceBuilder¶

FeatureCollection.CreateCurveOnSurfaceBuilder¶

Creates a Curve On Surface feature builder

Signature CreateCurveOnSurfaceBuilder(cosFeature)

Parameters:	cosFeature (`NXOpen.Features.CurveOnSurface`) – `NXOpen.Features.CurveOnSurface` to be edited
Returns:	CurveOnSurfaceBuilder object
Return type:	`NXOpen.Features.CurveOnSurfaceBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCurvelengthBuilder¶

FeatureCollection.CreateCurvelengthBuilder¶

Creates a Curvelength builder

Signature CreateCurvelengthBuilder(curvelength)

Parameters:	curvelength (`NXOpen.Features.Feature`) – `NXOpen.Features.CurveLengthBuilder` to be edited, if None then create a new one
Returns:	CurveLengthBuilder object
Return type:	`NXOpen.Features.CurveLengthBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCustomFeatureBuilder¶

FeatureCollection.CreateCustomFeatureBuilder¶

Creates a Features.CustomFeatureBuilder

Signature CreateCustomFeatureBuilder(customFeature)

Parameters:	customFeature (`NXOpen.Features.Feature`) – `Features.CustomFeature` to be edited
Returns:
Return type:	`NXOpen.Features.CustomFeatureBuilder`

New in version NX11.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateCutFaceBuilder¶

FeatureCollection.CreateCutFaceBuilder¶

Creates a cut face builder

Signature CreateCutFaceBuilder(cutFace)

Parameters:	cutFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.CutFaceBuilder object
Return type:	`NXOpen.Features.CutFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateCylinderBuilder¶

FeatureCollection.CreateCylinderBuilder¶

Creates a NXOpen.Features.CylinderBuilder

Signature CreateCylinderBuilder(cylinder)

Parameters:	cylinder (`NXOpen.Features.Feature`) – `NXOpen.Features.Cylinder` to be edited
Returns:
Return type:	`NXOpen.Features.CylinderBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateDatumAxisBuilder¶

FeatureCollection.CreateDatumAxisBuilder¶

Creates a Datum Axis feature builder

Signature CreateDatumAxisBuilder(datumAxis)

Parameters:	datumAxis (`NXOpen.Features.Feature`) – `NXOpen.Features.DatumAxisFeature` to be edited
Returns:	DatumAxisBuilder object
Return type:	`NXOpen.Features.DatumAxisBuilder`

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

CreateDatumCsysBuilder¶

FeatureCollection.CreateDatumCsysBuilder¶

Creates a Datum CSYS feature builder

Signature CreateDatumCsysBuilder(datumCsys)

Parameters:	datumCsys (`NXOpen.Features.Feature`) – `NXOpen.Features.DatumCsysBuilder` to be edited
Returns:	DatumCsysBuilder object
Return type:	`NXOpen.Features.DatumCsysBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateDatumPlaneBuilder¶

FeatureCollection.CreateDatumPlaneBuilder¶

Creates a Datum Plane feature builder

Signature CreateDatumPlaneBuilder(dplane)

Parameters:	dplane (`NXOpen.Features.Feature`) – `NXOpen.Features.DatumPlaneFeature` to be edited
Returns:	DatumPlaneBuilder object
Return type:	`NXOpen.Features.DatumPlaneBuilder`

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateDeformDefinitionBuilder¶

FeatureCollection.CreateDeformDefinitionBuilder¶

Creates a NXOpen.Features.DeformDefinitionBuilder

Signature CreateDeformDefinitionBuilder()

Returns:	The newly created deform definition builder.
Return type:	`NXOpen.Features.DeformDefinitionBuilder`

New in version NX12.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateDeleteBodyBuilder¶

FeatureCollection.CreateDeleteBodyBuilder¶

Creates a NXOpen.Features.DeleteBodyBuilder

Signature CreateDeleteBodyBuilder(deleteBody)

Parameters:	deleteBody (`NXOpen.Features.DeleteBody`) – `NXOpen.Features.DeleteBody` to be edited
Returns:	DeleteBodyBuilder object
Return type:	`NXOpen.Features.DeleteBodyBuilder`

New in version NX8.5.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateDeleteEdgeBuilder¶

FeatureCollection.CreateDeleteEdgeBuilder¶

Creates a NXOpen.Features.DeleteEdgeBuilder

Signature CreateDeleteEdgeBuilder(deleteEdge)

Parameters:	deleteEdge (`NXOpen.Features.DeleteEdge`) – `NXOpen.Features.DeleteEdge` to be edited
Returns:
Return type:	`NXOpen.Features.DeleteEdgeBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateDeleteFaceBuilder¶

FeatureCollection.CreateDeleteFaceBuilder¶

Creates a delete face builder, don’t use it until nx502

Signature CreateDeleteFaceBuilder(deleteFace)

Parameters:	deleteFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.DeleteFaceBuilder object
Return type:	`NXOpen.Features.DeleteFaceBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateDividefaceBuilder¶

FeatureCollection.CreateDividefaceBuilder¶

Creates a Divideface builder

Signature CreateDividefaceBuilder(divideface)

Parameters:	divideface (`NXOpen.Features.Feature`) – `NXOpen.Features.DividefaceBuilder` to be edited
Returns:	DividefaceBuilder object
Return type:	`NXOpen.Features.DividefaceBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateDraftBodyBuilder¶

FeatureCollection.CreateDraftBodyBuilder¶

Creates a NXOpen.Features.DraftBodyBuilder

Signature CreateDraftBodyBuilder(draftBody)

Parameters:	draftBody (`NXOpen.Features.Feature`) – `NXOpen.Features.DraftBody` to be edited
Returns:
Return type:	`NXOpen.Features.DraftBodyBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateDraftBuilder¶

FeatureCollection.CreateDraftBuilder¶

Creates a draft builder

Signature CreateDraftBuilder(draft)

Parameters:	draft (`NXOpen.Features.Feature`) – `NXOpen.Features.DraftBuilder` to be edited, if None then create a new one
Returns:	DraftBuilder object
Return type:	`NXOpen.Features.DraftBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateDraftingSplineBuilder¶

FeatureCollection.CreateDraftingSplineBuilder¶

Creates a Studio Spline builder for drafting

Signature CreateDraftingSplineBuilder(spline)

Parameters:	spline (`NXOpen.Spline`) – `NXOpen.Spline` to be edited
Returns:	DraftingSplineBuilder object
Return type:	`NXOpen.Features.DraftingSplineBuilder`

New in version NX8.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateEdgeBlendBuilder¶

FeatureCollection.CreateEdgeBlendBuilder¶

Creates a Edge Blend feature builder

Signature CreateEdgeBlendBuilder(edgeblend)

Parameters:	edgeblend (`NXOpen.Features.Feature`) – `NXOpen.Features.EdgeBlendBuilder` to be edited, if None then create a new one
Returns:	EdgeBlendBuilder object
Return type:	`NXOpen.Features.EdgeBlendBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateEdgeSymmetryBuilder¶

FeatureCollection.CreateEdgeSymmetryBuilder¶

Creates a NXOpen.Features.EdgeSymmetryBuilder

Signature CreateEdgeSymmetryBuilder(edgeSymmetry)

Parameters:	edgeSymmetry – `NXOpen.Features.EdgeSymmetry` to be edited.

Accepts NXOpen.Features.MatchEdge type if NXOpen.Features.MatchEdgeBuilderTypes is NXOpen.Features.MatchEdgeBuilderTypes.MatchEdgeToDatum. In that case converts NXOpen.Features.MatchEdge to NXOpen.Features.EdgeSymmetry feature. :type edgeSymmetry: NXOpen.Features.Feature :returns: :rtype: NXOpen.Features.EdgeSymmetryBuilder

New in version NX7.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateEditCrossSectionBuilder¶

FeatureCollection.CreateEditCrossSectionBuilder¶

Creates a NXOpen.Features.EditCrossSectionBuilder

Signature CreateEditCrossSectionBuilder(editCrossSection)

Parameters:	editCrossSection (`NXOpen.Features.EditCrossSection`) – `NXOpen.Features.EditCrossSection` to be edited
Returns:
Return type:	`NXOpen.Features.EditCrossSectionBuilder`

New in version NX8.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateEditDimensionBuilder¶

FeatureCollection.CreateEditDimensionBuilder¶

Creates a NXOpen.Features.EditDimensionBuilder

Signature CreateEditDimensionBuilder()

Returns:
Return type:	`NXOpen.Features.EditDimensionBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

CreateEmbedManagerBuilder¶

FeatureCollection.CreateEmbedManagerBuilder¶

Creates a NXOpen.Features.EmbedManagerBuilder

Signature CreateEmbedManagerBuilder()

Returns:
Return type:	`NXOpen.Features.EmbedManagerBuilder`

New in version NX12.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateEmbossBodyBuilder¶

FeatureCollection.CreateEmbossBodyBuilder¶

Creates a NXOpen.Features.EmbossBodyBuilder

Signature CreateEmbossBodyBuilder(embossBody)

Parameters:	embossBody (`NXOpen.Features.EmbossBody`) – `NXOpen.Features.EmbossBody` to be edited
Returns:
Return type:	`NXOpen.Features.EmbossBodyBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateEmbossBuilder¶

FeatureCollection.CreateEmbossBuilder¶

Creates an Emboss builder

Signature CreateEmbossBuilder(emboss)

Parameters:	emboss (`NXOpen.Features.Feature`) – `NXOpen.Features.EmbossBuilder` to be edited
Returns:	EmbossBuilder object
Return type:	`NXOpen.Features.EmbossBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateEnlargeBuilder¶

FeatureCollection.CreateEnlargeBuilder¶

Creates an Enlarge builder

Signature CreateEnlargeBuilder(enlargeFeature)

Parameters:	enlargeFeature (`NXOpen.Features.Enlarge`) – `NXOpen.Features.Enlarge` to be edited
Returns:	EnlargeBuilder object
Return type:	`NXOpen.Features.EnlargeBuilder`

New in version NX6.0.0.

License requirements: nx_freeform_2 (“advanced freeform modeling”)

CreateExtensionBuilder¶

FeatureCollection.CreateExtensionBuilder¶

Creates a NXOpen.Features.ExtensionBuilder

Signature CreateExtensionBuilder(extension)

Parameters:	extension (`NXOpen.Features.Extension`) – `NXOpen.Features.Extension` to be edited
Returns:
Return type:	`NXOpen.Features.ExtensionBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR free_form_modeling (“FREE-FORM MODELING”)

CreateExtractFaceBuilder¶

FeatureCollection.CreateExtractFaceBuilder¶

Creates a NXOpen.Features.ExtractFaceBuilder

Signature CreateExtractFaceBuilder(copyFace)

Parameters:	copyFace (`NXOpen.Features.Feature`) – CopyFace Feature to be edited
Returns:	Extract face builder object
Return type:	`NXOpen.Features.ExtractFaceBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateExtrudeBuilder¶

FeatureCollection.CreateExtrudeBuilder¶

Creates a Extrude builder

Signature CreateExtrudeBuilder(extrude)

Parameters:	extrude (`NXOpen.Features.Feature`) – `NXOpen.Features.Extrude` to be edited
Returns:	ExtrudeBuilder object
Return type:	`NXOpen.Features.ExtrudeBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateFaceBlendBuilder¶

FeatureCollection.CreateFaceBlendBuilder¶

Creates a Face Blend feature builder

Signature CreateFaceBlendBuilder(faceBlend)

Parameters:	faceBlend (`NXOpen.Features.Feature`) – `NXOpen.Features.FaceBlendBuilder` to be edited
Returns:	FaceBlendBuilder object
Return type:	`NXOpen.Features.FaceBlendBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateFeatureReplayBuilder¶

FeatureCollection.CreateFeatureReplayBuilder¶

Creates a NXOpen.Features.FeatureReplayBuilder

Signature CreateFeatureReplayBuilder()

Returns:	Features.

FeatureReplayBuilder object :rtype: NXOpen.Features.FeatureReplayBuilder

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateFitCurveBuilder¶

FeatureCollection.CreateFitCurveBuilder¶

Creates a NXOpen.Features.FitCurveBuilder

Signature CreateFitCurveBuilder(fitCurve)

Parameters:	fitCurve (`NXOpen.Features.FitCurve`) – `NXOpen.Features.FitCurve` to be edited
Returns:
Return type:	`NXOpen.Features.FitCurveBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateFitSurfaceBuilder¶

FeatureCollection.CreateFitSurfaceBuilder¶

Creates a NXOpen.Features.FitSurfaceBuilder

Signature CreateFitSurfaceBuilder(fitSurface)

Parameters:	fitSurface (`NXOpen.Features.FitSurface`) – `NXOpen.Features.FitSurface` to be edited
Returns:
Return type:	`NXOpen.Features.FitSurfaceBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateFixedBuilder¶

FeatureCollection.CreateFixedBuilder¶

Creates a NXOpen.Features.FixedBuilder

Signature CreateFixedBuilder(makeFix)

Parameters:	makeFix (`NXOpen.Features.Fixed`) – `NXOpen.Features.Fixed` to be edited
Returns:
Return type:	`NXOpen.Features.FixedBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateFlowBlendBuilder¶

FeatureCollection.CreateFlowBlendBuilder¶

Creates a Features.FlowBlendBuilder

Signature CreateFlowBlendBuilder(flowBlend)

Parameters:	flowBlend (`NXOpen.Features.FlowBlend`) – `Features.FlowBlend` to be edited
Returns:
Return type:	`NXOpen.Features.FlowBlendBuilder`

New in version NX10.0.0.

License requirements: flow_blend_for_nx (” Flow Blend”), solid_modeling (“SOLIDS MODELING”)

CreateFreeTransformerBuilder¶

FeatureCollection.CreateFreeTransformerBuilder¶

Creates a NXOpen.Features.FreeTransformerBuilder

Signature CreateFreeTransformerBuilder(freeTransformer)

Parameters:	freeTransformer (`NXOpen.Features.Feature`) – `NXOpen.Features.FreeTransformer` to be edited
Returns:
Return type:	`NXOpen.Features.FreeTransformerBuilder`

New in version NX10.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateGeneralConicBuilder¶

FeatureCollection.CreateGeneralConicBuilder¶

Creates a NXOpen.Features.GeneralConicBuilder

Signature CreateGeneralConicBuilder(generalConic)

Parameters:	generalConic (`NXOpen.Features.GeneralConic`) – `NXOpen.Features.GeneralConic` to be edited
Returns:
Return type:	`NXOpen.Features.GeneralConicBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

CreateGeomcopyBuilder¶

FeatureCollection.CreateGeomcopyBuilder¶

Creates a NXOpen.Features.GeomcopyBuilder

Signature CreateGeomcopyBuilder(geomcopy)

Parameters:	geomcopy (`NXOpen.Features.Feature`) – `NXOpen.Features.Geomcopy` to be edited
Returns:
Return type:	`NXOpen.Features.GeomcopyBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateGlobalShapingBuilder¶

FeatureCollection.CreateGlobalShapingBuilder¶

Creates a NXOpen.Features.GlobalShapingBuilder

Signature CreateGlobalShapingBuilder(globalShaping)

Parameters:	globalShaping (`NXOpen.Features.GlobalShaping`) – `NXOpen.Features.GlobalShaping` to be edited
Returns:
Return type:	`NXOpen.Features.GlobalShapingBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateGroupFaceBuilder¶

FeatureCollection.CreateGroupFaceBuilder¶

Creates a NXOpen.Features.GroupFaceBuilder

Signature CreateGroupFaceBuilder(groupFace)

Parameters:	groupFace (`NXOpen.Features.GroupFace`) – `NXOpen.Features.GroupFace` to be edited
Returns:
Return type:	`NXOpen.Features.GroupFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateGuidedExtensionBuilderEx¶

FeatureCollection.CreateGuidedExtensionBuilderEx¶

Creates a NXOpen.Features.GuidedExtensionBuilderEx

Signature CreateGuidedExtensionBuilderEx(guidedExtension)

Parameters:	guidedExtension (`NXOpen.Features.Feature`) – `NXOpen.Features.GuidedExtensionEx` to be edited
Returns:
Return type:	`NXOpen.Features.GuidedExtensionBuilderEx`

New in version NX10.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateHelixBuilder¶

FeatureCollection.CreateHelixBuilder¶

Creates a NXOpen.Features.HelixBuilder

Signature CreateHelixBuilder(helix)

Parameters:	helix (`NXOpen.Features.Helix`) – `NXOpen.Features.Helix` to be edited
Returns:
Return type:	`NXOpen.Features.HelixBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateHoleFeatureBuilder¶

FeatureCollection.CreateHoleFeatureBuilder¶

Creates a Hole feature builder

Signature CreateHoleFeatureBuilder(hole)

Parameters:	hole (`NXOpen.Features.Feature`) – `NXOpen.Features.Hole` to be edited
Returns:	HoleFeatureBuilder object
Return type:	`NXOpen.Features.HoleFeatureBuilder`

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateHolePackageBuilder¶

FeatureCollection.CreateHolePackageBuilder¶

Creates a NXOpen.Features.HolePackageBuilder

Signature CreateHolePackageBuilder(holePackage)

Parameters:	holePackage (`NXOpen.Features.HolePackage`) – `NXOpen.Features.HolePackage` to be edited
Returns:
Return type:	`NXOpen.Features.HolePackageBuilder`

New in version NX5.0.2.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateHoodVisibilityBuilder¶

FeatureCollection.CreateHoodVisibilityBuilder¶

Creates a NXOpen.Features.VehicleDesign.HoodVisibilityBuilder

Signature CreateHoodVisibilityBuilder(hoodVisibility)

Parameters:	hoodVisibility (`NXOpen.Features.Feature`) – feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.VehicleDesignCollection.CreateHoodVisibilityBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreateHumanBuilder¶

FeatureCollection.CreateHumanBuilder¶

Creates a human feature builder.

Signature CreateHumanBuilder(human)

Parameters:	human (`NXOpen.Features.Feature`) – `NXOpen.Features.Human` to be edited, if None then create a new one
Returns:	HumanBuilder object
Return type:	`NXOpen.Features.HumanBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”), ug_human (“Human Modelling”)

CreateHumanPosturePredictionBuilder¶

FeatureCollection.CreateHumanPosturePredictionBuilder¶

Creates a human posture prediction builder.

Signature CreateHumanPosturePredictionBuilder(posturePrediction)

Parameters:	posturePrediction (`NXOpen.HumanPosturePrediction`) – `NXOpen.HumanPosturePrediction` to be edited, if None then create a new one
Returns:	`NXOpen.HumanPosturePredictionBuilder` object
Return type:	`NXOpen.HumanPosturePredictionBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”), ug_human (“Human Modelling”)

CreateIformBuilder¶

FeatureCollection.CreateIformBuilder¶

Creates a NXOpen.Features.IFormBuilder

Signature CreateIformBuilder(iform)

Parameters:	iform (`NXOpen.Features.IForm`) – `NXOpen.Features.IForm` to be edited
Returns:
Return type:	`NXOpen.Features.IFormBuilder`

New in version NX7.5.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateInstanceFeatureBuilder¶

FeatureCollection.CreateInstanceFeatureBuilder¶

Overloaded method CreateInstanceFeatureBuilder

CreateInstanceFeatureBuilder(instanceFeature)
CreateInstanceFeatureBuilder(instanceFeatures, forClocking)

-------------------------------------

Creates NXOpen.Features.InstanceFeatureBuilder

Signature CreateInstanceFeatureBuilder(instanceFeature)

Parameters:	instanceFeature (`NXOpen.Features.InstanceFeature`) – `NXOpen.Features.InstanceFeature` to be edited
Returns:	`NXOpen.Features.InstanceFeatureBuilder` object
Return type:	`NXOpen.Features.InstanceFeatureBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

-------------------------------------

Creates NXOpen.Features.InstanceFeatureBuilder from multiple NXOpen.Features.InstanceFeature

Signature CreateInstanceFeatureBuilder(instanceFeatures, forClocking)

Parameters:	instanceFeatures (list of `NXOpen.Features.InstanceFeature`) – array of `NXOpen.Features.InstanceFeature` to be edited forClocking (bool) –
Returns:	`NXOpen.Features.InstanceFeatureBuilder` object
Return type:	`NXOpen.Features.InstanceFeatureBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

-------------------------------------

CreateIntersectFeature¶

FeatureCollection.CreateIntersectFeature¶

Creates an intersect feature.

Signature CreateIntersectFeature(targetBody, retainTargetBody, toolBodies, retainToolBodies, allowNonAssociativeBoolean)

Parameters:	targetBody (`NXOpen.Body`) – Target body retainTargetBody (bool) – Retain option for target body toolBodies (list of `NXOpen.Body`) – Tool bodies retainToolBodies (bool) – Retain option for tool bodies allowNonAssociativeBoolean (bool) – Allow boolean operation even if it results into non-associative boolean
Returns:	a tuple
Return type:	A tuple consisting of (features, nonAssociativeBoolean, unparameterizedSolids). features is a list of `NXOpen.Features.BooleanFeature`. Array of boolean features nonAssociativeBoolean is a bool. True if operation resulted in a non-associative boolean. False otherwise unparameterizedSolids is a bool. True if operation resulted in unparameterized solids. False otherwise

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateIntersectionCurveBuilder¶

FeatureCollection.CreateIntersectionCurveBuilder¶

Creates a NXOpen.Features.IntersectionCurveBuilder

Signature CreateIntersectionCurveBuilder(intersectionCurve)

Parameters:	intersectionCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.IntersectionCurveBuilder` to be edited
Returns:	IntersectionCurveBuilder object
Return type:	`NXOpen.Features.IntersectionCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateIsolateFeatureBuilder¶

FeatureCollection.CreateIsolateFeatureBuilder¶

Creates a NXOpen.Features.IsolateFeatureBuilder

Signature CreateIsolateFeatureBuilder(isolateFeature)

Parameters:	isolateFeature (`NXOpen.Features.IsolateFeature`) –
Returns:
Return type:	`NXOpen.Features.IsolateFeatureBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateIsoparametricCurvesBuilder¶

FeatureCollection.CreateIsoparametricCurvesBuilder¶

Creates a NXOpen.Features.IsoparametricCurvesBuilder

Signature CreateIsoparametricCurvesBuilder(isoparametricCurves)

Parameters:	isoparametricCurves (`NXOpen.Features.IsoparametricCurves`) – `NXOpen.Features.IsoparametricCurves` to be edited
Returns:
Return type:	`NXOpen.Features.IsoparametricCurvesBuilder`

New in version NX8.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateJoinCurvesBuilder¶

FeatureCollection.CreateJoinCurvesBuilder¶

Creates a NXOpen.Features.JoinCurvesBuilder

Signature CreateJoinCurvesBuilder(joinCurves)

Parameters:	joinCurves (`NXOpen.Features.Feature`) – `NXOpen.Features.JoinCurves` to be edited, if None then create a new one
Returns:	JoinCurvesBuilder object
Return type:	`NXOpen.Features.JoinCurvesBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateLabelChamferBuilder¶

FeatureCollection.CreateLabelChamferBuilder¶

Creates a NXOpen.Features.LabelChamferBuilder

Signature CreateLabelChamferBuilder(labelChamfer)

Parameters:	labelChamfer (`NXOpen.Features.LabelChamfer`) – `NXOpen.Features.LabelChamfer` to be edited
Returns:
Return type:	`NXOpen.Features.LabelChamferBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateLabelNotchBlendBuilder¶

FeatureCollection.CreateLabelNotchBlendBuilder¶

Creates a NXOpen.Features.LabelNotchBlendBuilder

Signature CreateLabelNotchBlendBuilder(labelNotchBlend)

Parameters:	labelNotchBlend (`NXOpen.Features.LabelNotchBlend`) – `NXOpen.Features.LabelNotchBlend` to be edited
Returns:
Return type:	`NXOpen.Features.LabelNotchBlendBuilder`

New in version NX8.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateLawCurveBuilder¶

FeatureCollection.CreateLawCurveBuilder¶

Creates a NXOpen.Features.LawCurveBuilder

Signature CreateLawCurveBuilder(lawCurve)

Parameters:	lawCurve (`NXOpen.Features.LawCurve`) – `NXOpen.Features.LawCurve` to be edited
Returns:
Return type:	`NXOpen.Features.LawCurveBuilder`

New in version NX7.5.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateLawExtensionBuilder¶

FeatureCollection.CreateLawExtensionBuilder¶

Creates a NXOpen.Features.LawExtensionBuilder

Signature CreateLawExtensionBuilder(lawExtension)

Parameters:	lawExtension (`NXOpen.Features.LawExtension`) – `NXOpen.Features.LawExtension` to be edited
Returns:
Return type:	`NXOpen.Features.LawExtensionBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateLawExtensionBuilderEx¶

FeatureCollection.CreateLawExtensionBuilderEx¶

Creates a NXOpen.Features.LawExtensionBuilderEx

Signature CreateLawExtensionBuilderEx(lawExtension)

Parameters:	lawExtension (`NXOpen.Features.Feature`) – `NXOpen.Features.LawExtensionEx` to be edited
Returns:
Return type:	`NXOpen.Features.LawExtensionBuilderEx`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateLinearDimensionBuilder¶

FeatureCollection.CreateLinearDimensionBuilder¶

Creates a NXOpen.Features.LinearDimensionBuilder

Signature CreateLinearDimensionBuilder(linearDimension)

Parameters:	linearDimension (`NXOpen.Features.LinearDimension`) – `NXOpen.Features.LinearDimension` to be edited
Returns:
Return type:	`NXOpen.Features.LinearDimensionBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateLinkedFacetBuilder¶

FeatureCollection.CreateLinkedFacetBuilder¶

Creates a NXOpen.Features.LinkedFacetBuilder

Signature CreateLinkedFacetBuilder(linkedFacet)

Parameters:	linkedFacet (`NXOpen.Features.LinkedFacet`) – `NXOpen.Features.LinkedFacet` to be edited
Returns:
Return type:	`NXOpen.Features.LinkedFacetBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMakeOffsetBuilder¶

FeatureCollection.CreateMakeOffsetBuilder¶

Creates a NXOpen.Features.MakeOffsetBuilder

Signature CreateMakeOffsetBuilder(makeOffset)

Parameters:	makeOffset (`NXOpen.Features.MakeOffset`) – `NXOpen.Features.MakeOffset` to be edited
Returns:
Return type:	`NXOpen.Features.MakeOffsetBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateMapleBuilder¶

FeatureCollection.CreateMapleBuilder¶

Creates a NXOpen.Features.MapleBuilder

Signature CreateMapleBuilder(maple)

Parameters:	maple (`NXOpen.Features.Maple`) – `NXOpen.Features.Maple` to be edited
Returns:
Return type:	`NXOpen.Features.MapleBuilder`

New in version NX7.5.0.

Deprecated since version NX12.0.0: Use NXOpen.Features.FeatureCollection.CreateMathIntegrationBuilder() instead.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMasterCutBuilder¶

FeatureCollection.CreateMasterCutBuilder¶

Create a Master Cut builder

Signature CreateMasterCutBuilder(masterCut)

Parameters:	masterCut (`NXOpen.Features.Feature`) – `NXOpen.Features.MasterCutBuilder` to be edited, if None then create a new one
Returns:
Return type:	`NXOpen.Features.MasterCutBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMatchEdgeBuilder¶

FeatureCollection.CreateMatchEdgeBuilder¶

Creates a NXOpen.Features.MatchEdgeBuilder

Signature CreateMatchEdgeBuilder(matchEdge)

Parameters:	matchEdge (`NXOpen.Features.MatchEdge`) – `NXOpen.Features.MatchEdge` to be edited
Returns:
Return type:	`NXOpen.Features.MatchEdgeBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”)

CreateMathIntegrationBuilder¶

FeatureCollection.CreateMathIntegrationBuilder¶

Creates a NXOpen.Features.MathIntegrationBuilder

Signature CreateMathIntegrationBuilder(mathIntegration)

Parameters:	mathIntegration (`NXOpen.Features.MathIntegration`) – `NXOpen.Features.MathIntegration` to be edited
Returns:
Return type:	`NXOpen.Features.MathIntegrationBuilder`

New in version NX12.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMeshSurfaceBuilder¶

FeatureCollection.CreateMeshSurfaceBuilder¶

Creates a Mesh Surface feature builder

Signature CreateMeshSurfaceBuilder(meshSurf)

Parameters:	meshSurf (`NXOpen.Features.Feature`) – `NXOpen.Features.Ruled`, `NXOpen.Features.ThroughCurves`, `NXOpen.Features.ThroughCurveMesh` to be edited
Returns:	MeshSurfaceBuilder object
Return type:	`NXOpen.Features.MeshSurfaceBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateMeshTransformerBuilder¶

FeatureCollection.CreateMeshTransformerBuilder¶

Creates a NXOpen.Features.MeshTransformerBuilder

Signature CreateMeshTransformerBuilder(meshTransformer)

Parameters:	meshTransformer (`NXOpen.Features.Feature`) – `NXOpen.Features.MeshTransformer` to be edited
Returns:
Return type:	`NXOpen.Features.MeshTransformerBuilder`

New in version NX10.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMidSurfaceByFacePairsBuilder¶

FeatureCollection.CreateMidSurfaceByFacePairsBuilder¶

Creates a NXOpen.Features.MidSurfaceByFacePairsBuilder

Signature CreateMidSurfaceByFacePairsBuilder(midSurfaceByFacePairs)

Parameters:	midSurfaceByFacePairs (`NXOpen.Features.Feature`) – `NXOpen.Features.MidSurfaceByFacePairs` to be edited or a `NXOpen.Features.MidSurfaceFacePair`
Returns:
Return type:	`NXOpen.Features.MidSurfaceByFacePairsBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMidSurfaceUserDefinedBuilder¶

FeatureCollection.CreateMidSurfaceUserDefinedBuilder¶

Creates a NXOpen.Features.MidSurfaceUserDefinedBuilder

Signature CreateMidSurfaceUserDefinedBuilder(midsurfaceUserDefined)

Parameters:	midsurfaceUserDefined (`NXOpen.Features.MidSurfaceUserDefined`) – `NXOpen.Features.MidSurfaceUserDefined` to be edited
Returns:
Return type:	`NXOpen.Features.MidSurfaceUserDefinedBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMirrorBodyBuilder¶

FeatureCollection.CreateMirrorBodyBuilder¶

Creates a NXOpen.Features.MirrorBodyBuilder

Signature CreateMirrorBodyBuilder(mirrorBody)

Parameters:	mirrorBody (`NXOpen.Features.Feature`) – `NXOpen.Features.MirrorBodyBuilder` to be edited
Returns:	MirrorBodyBuilder object
Return type:	`NXOpen.Features.MirrorBodyBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateMirrorBuilder¶

FeatureCollection.CreateMirrorBuilder¶

Creates NXOpen.Features.MirrorBuilder

Signature CreateMirrorBuilder(mirrorFeature)

Parameters:	mirrorFeature (`NXOpen.Features.Mirror`) – `NXOpen.Features.Mirror` to be edited
Returns:	`NXOpen.Features.MirrorBuilder` object
Return type:	`NXOpen.Features.MirrorBuilder`

New in version NX8.0.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMirrorCurveBuilder¶

FeatureCollection.CreateMirrorCurveBuilder¶

Creates a NXOpen.Features.MirrorCurveBuilder

Signature CreateMirrorCurveBuilder(mirrorCurve)

Parameters:	mirrorCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.MirrorCurve` to be edited
Returns:
Return type:	`NXOpen.Features.MirrorCurveBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMirrorFaceBuilder¶

FeatureCollection.CreateMirrorFaceBuilder¶

Creates a mirror face builder

Signature CreateMirrorFaceBuilder(mirrorFace)

Parameters:	mirrorFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.MirrorFaceBuilder object
Return type:	`NXOpen.Features.MirrorFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateMirrorFeatureBuilder¶

FeatureCollection.CreateMirrorFeatureBuilder¶

Creates NXOpen.Features.MirrorFeatureBuilder

Signature CreateMirrorFeatureBuilder(mirrorFea)

Parameters:	mirrorFea (`NXOpen.Features.Feature`) – `NXOpen.Features.MirrorFeatureBuilder` to be edited
Returns:	MirrorFeatureBuilder object
Return type:	`NXOpen.Features.MirrorFeatureBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateMoveFaceBuilder¶

FeatureCollection.CreateMoveFaceBuilder¶

Create a move face builder, don’t use it until nx502

Signature CreateMoveFaceBuilder(moveFace)

Parameters:	moveFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.MoveFaceBuilder object
Return type:	`NXOpen.Features.MoveFaceBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateNSidedSurfaceBuilder¶

FeatureCollection.CreateNSidedSurfaceBuilder¶

Creates a NXOpen.Features.NSidedSurfaceBuilder

Signature CreateNSidedSurfaceBuilder(nsidedSurface)

Parameters:	nsidedSurface (`NXOpen.Features.NSidedSurface`) – `NXOpen.Features.NSidedSurface` to be edited
Returns:
Return type:	`NXOpen.Features.NSidedSurfaceBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateNestModuleBuilder¶

FeatureCollection.CreateNestModuleBuilder¶

Creates a NXOpen.GeometricUtilities.NestModuleBuilder

This API is now deprecated. Please use NXOpen.Features.FeatureCollection instead.

Signature CreateNestModuleBuilder()

Returns:	Returns a `NXOpen.GeometricUtilities.NestModuleBuilder` builder
Return type:	`NXOpen.GeometricUtilities.NestModuleBuilder`

New in version NX9.0.0.

Deprecated since version NX10.0.0: Please use NXOpen.Features.FeatureCollection instead.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateOffsetCurveBuilder¶

FeatureCollection.CreateOffsetCurveBuilder¶

Creates a NXOpen.Features.OffsetCurveBuilder

Signature CreateOffsetCurveBuilder(offsetCurve)

Parameters:	offsetCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.OffsetCurve` to be edited
Returns:	Offset Curve Builder object
Return type:	`NXOpen.Features.OffsetCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

CreateOffsetEmbossBuilder¶

FeatureCollection.CreateOffsetEmbossBuilder¶

Creates a Offsetemboss builder

Signature CreateOffsetEmbossBuilder(offsetEmboss)

Parameters:	offsetEmboss (`NXOpen.Features.Feature`) – `NXOpen.Features.OffsetEmbossBuilder` to be edited
Returns:	OffsetEmbossBuilder object
Return type:	`NXOpen.Features.OffsetEmbossBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateOffsetFaceBuilder¶

FeatureCollection.CreateOffsetFaceBuilder¶

Creates a NXOpen.Features.OffsetFaceBuilder

Signature CreateOffsetFaceBuilder(offsetface)

Parameters:	offsetface (`NXOpen.Features.Feature`) – `NXOpen.Features.OffsetFace` to be edited, if None then create a new one
Returns:	OffsetFaceBuilder object
Return type:	`NXOpen.Features.OffsetFaceBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateOffsetRegionBuilder¶

FeatureCollection.CreateOffsetRegionBuilder¶

Creates an offset region builder, don’t use it until nx502

Signature CreateOffsetRegionBuilder(offsetRegion)

Parameters:	offsetRegion (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.OffsetRegionBuilder object
Return type:	`NXOpen.Features.OffsetRegionBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateOffsetSurfaceBuilder¶

FeatureCollection.CreateOffsetSurfaceBuilder¶

Creates an Offset Surface builder

Signature CreateOffsetSurfaceBuilder(offsetSurface)

Parameters:	offsetSurface (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	OffsetSurfaceBuilder object
Return type:	`NXOpen.Features.OffsetSurfaceBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateOptimizeCurveBuilder¶

FeatureCollection.CreateOptimizeCurveBuilder¶

Creates a NXOpen.Features.OptimizeCurveBuilder

Signature CreateOptimizeCurveBuilder()

Returns:	OptimizeCurveBuilder object
Return type:	`NXOpen.Features.OptimizeCurveBuilder`

New in version NX10.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateOptimizeFaceBuilder¶

FeatureCollection.CreateOptimizeFaceBuilder¶

Creates a NXOpen.Features.OptimizeFaceBuilder

Signature CreateOptimizeFaceBuilder()

Returns:
Return type:	`NXOpen.Features.OptimizeFaceBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateOvercrownFeatureBuilder¶

FeatureCollection.CreateOvercrownFeatureBuilder¶

Creates a Overcrown feature builder

Signature CreateOvercrownFeatureBuilder(overcrown)

Parameters:	overcrown (`NXOpen.Features.Feature`) – `NXOpen.Features.OvercrownBuilder` to be edited, if None then create a new one.
Returns:	OvercrownBuilder object
Return type:	`NXOpen.Features.OvercrownBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePaintParametersBuilder¶

FeatureCollection.CreatePaintParametersBuilder¶

Creates a NXOpen.Features.PaintParametersBuilder

Signature CreatePaintParametersBuilder()

Returns:
Return type:	`NXOpen.Features.PaintParametersBuilder`

New in version NX9.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateParallelBuilder¶

FeatureCollection.CreateParallelBuilder¶

Creates a NXOpen.Features.ParallelBuilder

Signature CreateParallelBuilder(parallel)

Parameters:	parallel (`NXOpen.Features.Parallel`) – `NXOpen.Features.Parallel` to be edited
Returns:
Return type:	`NXOpen.Features.ParallelBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePartModuleBuilder¶

FeatureCollection.CreatePartModuleBuilder¶

Creates a NXOpen.Features.PartModuleBuilder

Signature CreatePartModuleBuilder(partModule)

Parameters:	partModule (`NXOpen.Features.PartModule`) – `NXOpen.Features.PartModule` to be edited
Returns:
Return type:	`NXOpen.Features.PartModuleBuilder`

New in version NX8.0.0.

License requirements: usr_defined_features (“USER DEFINED FEATURES”)

CreatePartModuleRelationshipBuilder¶

FeatureCollection.CreatePartModuleRelationshipBuilder¶

Creates a NXOpen.GeometricUtilities.PartModuleRelationshipBuilder

Signature CreatePartModuleRelationshipBuilder(partModule)

Parameters:	partModule (`NXOpen.Features.PartModule`) – `NXOpen.Features.PartModule` to be edited
Returns:
Return type:	`NXOpen.GeometricUtilities.PartModuleRelationshipBuilder`

New in version NX8.0.0.

License requirements: wave (“WAVE FUNCTIONALITY”)

CreatePasteFaceBuilder¶

FeatureCollection.CreatePasteFaceBuilder¶

Creates a paste face builder

Signature CreatePasteFaceBuilder(pasteFace)

Parameters:	pasteFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.PasteFaceBuilder object
Return type:	`NXOpen.Features.PasteFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePatchBuilder¶

FeatureCollection.CreatePatchBuilder¶

Creates a NXOpen.Features.PatchBuilder

Signature CreatePatchBuilder(patch)

Parameters:	patch (`NXOpen.Features.Feature`) – Patch Features to be edited
Returns:	PatchBuilder object
Return type:	`NXOpen.Features.PatchBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePatchOpeningsBuilder¶

FeatureCollection.CreatePatchOpeningsBuilder¶

Creates a NXOpen.Features.PatchOpeningsBuilder

Signature CreatePatchOpeningsBuilder(patchOpenings)

Parameters:	patchOpenings (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:
Return type:	`NXOpen.Features.PatchOpeningsBuilder`

New in version NX5.0.0.

License requirements: None.

CreatePatternFaceBuilder¶

FeatureCollection.CreatePatternFaceBuilder¶

Creates a pattern face builder, don’t use it until nx502

Signature CreatePatternFaceBuilder(patternFace)

Parameters:	patternFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.PatternFaceBuilder object
Return type:	`NXOpen.Features.PatternFaceBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePatternFaceFeatureBuilder¶

FeatureCollection.CreatePatternFaceFeatureBuilder¶

Creates a NXOpen.Features.PatternFaceFeatureBuilder

Signature CreatePatternFaceFeatureBuilder(patternFaceFeature)

Parameters:	patternFaceFeature (`NXOpen.Features.PatternFaceFeature`) – `NXOpen.Features.PatternFaceFeature` to be edited
Returns:
Return type:	`NXOpen.Features.PatternFaceFeatureBuilder`

New in version NX9.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePatternFeatureBuilder¶

FeatureCollection.CreatePatternFeatureBuilder¶

Creates NXOpen.Features.PatternFeatureBuilder

Signature CreatePatternFeatureBuilder(patternFeature)

Parameters:	patternFeature (`NXOpen.Features.Feature`) – `NXOpen.Features.PatternFeatureBuilder` to be edited
Returns:	PatternFeatureBuilder object
Return type:	`NXOpen.Features.PatternFeatureBuilder`

New in version NX7.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePatternGeometryBuilder¶

FeatureCollection.CreatePatternGeometryBuilder¶

Creates a NXOpen.Features.PatternGeometryBuilder

Signature CreatePatternGeometryBuilder(patternGeometry)

Parameters:	patternGeometry (`NXOpen.Features.PatternGeometry`) – The feature class `NXOpen.Features.PatternGeometry`
Returns:	The builder for the feature class
Return type:	`NXOpen.Features.PatternGeometryBuilder`

New in version NX9.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePedestrianProtectionBuilder¶

FeatureCollection.CreatePedestrianProtectionBuilder¶

Creates a NXOpen.Features.VehicleDesign.PedestrianProtectionBuilder

Signature CreatePedestrianProtectionBuilder(pedestrianProtection)

Parameters:	pedestrianProtection (`NXOpen.Features.Feature`) – feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.VehicleDesignCollection.CreatePedestrianProtectionBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreatePerpendicularBuilder¶

FeatureCollection.CreatePerpendicularBuilder¶

Creates a NXOpen.Features.PerpendicularBuilder

Signature CreatePerpendicularBuilder(perpendicular)

Parameters:	perpendicular (`NXOpen.Features.Perpendicular`) – `NXOpen.Features.Perpendicular` to be edited
Returns:	Features.

PerpendicularBuilder object :rtype: NXOpen.Features.PerpendicularBuilder

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePointSetBuilder¶

FeatureCollection.CreatePointSetBuilder¶

Creates a NXOpen.Features.PointSetBuilder

Signature CreatePointSetBuilder(pointSet)

Parameters:	pointSet (`NXOpen.Features.PointSet`) – `NXOpen.Features.PointSet` to be edited
Returns:
Return type:	`NXOpen.Features.PointSetBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePoleSmoothingBuilder¶

FeatureCollection.CreatePoleSmoothingBuilder¶

Creates a NXOpen.Features.PoleSmoothingBuilder

Signature CreatePoleSmoothingBuilder(poleSmoothing)

Parameters:	poleSmoothing (`NXOpen.Features.PoleSmoothing`) – `NXOpen.Features.PoleSmoothing` to be edited
Returns:
Return type:	`NXOpen.Features.PoleSmoothingBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateProjectCurveBuilder¶

FeatureCollection.CreateProjectCurveBuilder¶

Creates a NXOpen.Features.ProjectCurveBuilder

Signature CreateProjectCurveBuilder(projectCurve)

Parameters:	projectCurve (`NXOpen.Features.Feature`) – `NXOpen.Features.ProjectCurve` to be edited
Returns:	ProjectCurveBuilder object
Return type:	`NXOpen.Features.ProjectCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreatePromotionBuilder¶

FeatureCollection.CreatePromotionBuilder¶

Creates a NXOpen.Features.PromotionBuilder

Signature CreatePromotionBuilder(promotion)

Parameters:	promotion (`NXOpen.Features.Promotion`) – `NXOpen.Features.Promotion` to be edited
Returns:
Return type:	`NXOpen.Features.PromotionBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreatePullFaceBuilder¶

FeatureCollection.CreatePullFaceBuilder¶

Creates a NXOpen.Features.PullFaceBuilder

Signature CreatePullFaceBuilder(pullFace)

Parameters:	pullFace (`NXOpen.Features.PullFace`) – `NXOpen.Features.PullFace` to be edited
Returns:
Return type:	`NXOpen.Features.PullFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateRadialDimensionBuilder¶

FeatureCollection.CreateRadialDimensionBuilder¶

Creates a NXOpen.Features.RadialDimensionBuilder

Signature CreateRadialDimensionBuilder(radialDimension)

Parameters:	radialDimension (`NXOpen.Features.RadialDimension`) – `NXOpen.Features.RadialDimension` to be edited
Returns:
Return type:	`NXOpen.Features.RadialDimensionBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateRapidSurfaceBuilder¶

FeatureCollection.CreateRapidSurfaceBuilder¶

Creates a Rapid Surfacing feature builder

Signature CreateRapidSurfaceBuilder(rapidSurface)

Parameters:	rapidSurface (`NXOpen.Features.RapidSurface`) – `NXOpen.Features.RapidSurface` to be edited
Returns:	RapidSurfaceBuilder object
Return type:	`NXOpen.Features.RapidSurfaceBuilder`

New in version NX5.0.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateRasterImage¶

FeatureCollection.CreateRasterImage¶

Creates a raster image

Signature CreateRasterImage(origin, matrix, length, height, imageFileName, translucency, maximumTextureSize)

Parameters:	origin (`NXOpen.Point3d`) – The origin for the raster image matrix (`NXOpen.Matrix3x3`) – The rotation matrix for the raster image length (float) – Length of the image, given in the units parameter height (float) – Height of the image, give in the units parameter imageFileName (str) – Name of the image file to use. For now, it must be a .tif file translucency (float) – 0.0 for no translucency, 1.0 for fully transparent maximumTextureSize (`NXOpen.Features.RasterImageMaxTextureSize`) –
Returns:	RasterImage object
Return type:	`NXOpen.Features.RasterImage`

New in version NX4.0.0.

License requirements: studio_visualize (“STUDIO VISUALIZE”)

CreateReferenceMapperBuilder¶

FeatureCollection.CreateReferenceMapperBuilder¶

Creates a NXOpen.Features.ReferenceMapperBuilder

Signature CreateReferenceMapperBuilder(booleanBuilderTag)

Parameters:	booleanBuilderTag (`NXOpen.Features.FeatureBuilder`) – `NXOpen.Features.FeatureBuilder`
Returns:	ReferenceMapperBuilder
Return type:	`NXOpen.Features.ReferenceMapperBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateRefitFaceBuilder¶

FeatureCollection.CreateRefitFaceBuilder¶

Creates a RefitFaceBuilder

Signature CreateRefitFaceBuilder(refitFace)

Parameters:	refitFace (`NXOpen.Features.RefitFace`) – `NXOpen.Features.RefitFace` to be edited
Returns:
Return type:	`NXOpen.Features.RefitFaceBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateReflectionDataBuilder¶

FeatureCollection.CreateReflectionDataBuilder¶

Creates a NXOpen.Features.VehicleDesign.ReflectionDataBuilder

Signature CreateReflectionDataBuilder(reflectionData)

Parameters:	reflectionData (`NXOpen.Features.Feature`) – Feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.VehicleDesignCollection.CreateReflectionDataBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreateRemoveParametersBuilder¶

FeatureCollection.CreateRemoveParametersBuilder¶

Creates a NXOpen.Features.RemoveParametersBuilder

Signature CreateRemoveParametersBuilder()

Returns:	Features.

RemoveParametersBuilder object :rtype: NXOpen.Features.RemoveParametersBuilder

New in version NX6.0.0.

License requirements: None.

CreateRenameLinkedPartModulePartBuilder¶

FeatureCollection.CreateRenameLinkedPartModulePartBuilder¶

Creates a NXOpen.GeometricUtilities.RenameLinkedPartModulePartBuilder

Signature CreateRenameLinkedPartModulePartBuilder()

Returns:
Return type:	`NXOpen.GeometricUtilities.RenameLinkedPartModulePartBuilder`

New in version NX9.0.0.

License requirements: None.

CreateRenewFeatureBuilder¶

FeatureCollection.CreateRenewFeatureBuilder¶

Creates a NXOpen.GeometricUtilities.RenewFeatureBuilder

Signature CreateRenewFeatureBuilder()

Returns:
Return type:	`NXOpen.GeometricUtilities.RenewFeatureBuilder`

New in version NX11.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateReorderBlendsBuilder¶

FeatureCollection.CreateReorderBlendsBuilder¶

Creates a NXOpen.Features.ReorderBlendsBuilder

Signature CreateReorderBlendsBuilder(reorderBlends)

Parameters:	reorderBlends (`NXOpen.Features.ReorderBlends`) – `NXOpen.Features.ReorderBlends` to be edited
Returns:
Return type:	`NXOpen.Features.ReorderBlendsBuilder`

New in version NX7.5.1.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateReplaceBlendBuilder¶

FeatureCollection.CreateReplaceBlendBuilder¶

Creates a NXOpen.Features.ReplaceBlendBuilder

Signature CreateReplaceBlendBuilder(replaceBlend)

Parameters:	replaceBlend (`NXOpen.Features.ReplaceBlend`) – `NXOpen.Features.ReplaceBlend` to be edited
Returns:	`NXOpen.Features.ReplaceBlendBuilder` object
Return type:	`NXOpen.Features.ReplaceBlendBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateReplaceFaceBuilder¶

FeatureCollection.CreateReplaceFaceBuilder¶

Creates a replace face builder, don’t use it until nx502

Signature CreateReplaceFaceBuilder(replaceFace)

Parameters:	replaceFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.ReplaceFaceBuilder object
Return type:	`NXOpen.Features.ReplaceFaceBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateReplaceFeatureBuilder¶

FeatureCollection.CreateReplaceFeatureBuilder¶

Creates a NXOpen.Features.ReplaceFeatureBuilder

Signature CreateReplaceFeatureBuilder()

Returns:
Return type:	`NXOpen.Features.ReplaceFeatureBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateResizeBlendBuilder¶

FeatureCollection.CreateResizeBlendBuilder¶

Creates a resize blend builder, don’t use it until nx502

Signature CreateResizeBlendBuilder(resizeBlend)

Parameters:	resizeBlend (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.ResizeBlendBuilder object
Return type:	`NXOpen.Features.ResizeBlendBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateResizeChamferBuilder¶

FeatureCollection.CreateResizeChamferBuilder¶

Creates a NXOpen.Features.ResizeChamferBuilder

Signature CreateResizeChamferBuilder(resizeChamfer)

Parameters:	resizeChamfer (`NXOpen.Features.ResizeChamfer`) – `NXOpen.Features.ResizeChamfer` to be edited
Returns:
Return type:	`NXOpen.Features.ResizeChamferBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateResizeFaceBuilder¶

FeatureCollection.CreateResizeFaceBuilder¶

Creates a resize face builder, don’t use it until nx502

Signature CreateResizeFaceBuilder(resizeFace)

Parameters:	resizeFace (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.ResizeFaceBuilder object
Return type:	`NXOpen.Features.ResizeFaceBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateResizePlaneBuilder¶

FeatureCollection.CreateResizePlaneBuilder¶

Creates a Resize Datum Plane feature builder

Signature CreateResizePlaneBuilder(resizePlane)

Parameters:	resizePlane (`NXOpen.Features.Feature`) – `NXOpen.Features.DatumPlaneFeature` to be edited
Returns:	ResizePlaneBuilder object
Return type:	`NXOpen.Features.ResizePlaneBuilder`

New in version NX6.0.3.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateRevolveBuilder¶

FeatureCollection.CreateRevolveBuilder¶

Creates a Revolve builder

Signature CreateRevolveBuilder(revolve)

Parameters:	revolve (`NXOpen.Features.Feature`) – `NXOpen.Features.RevolveBuilder` to be edited, if None then create a new one
Returns:	RevolveBuilder object
Return type:	`NXOpen.Features.RevolveBuilder`

New in version NX3.0.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateRibbonBuilder¶

FeatureCollection.CreateRibbonBuilder¶

Creates a ribbon builder

Signature CreateRibbonBuilder(ribbon)

Parameters:	ribbon (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:	Features.RibbonBuilder object
Return type:	`NXOpen.Features.RibbonBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateRpoBuilder¶

FeatureCollection.CreateRpoBuilder¶

Creates a Relative Positioning Object builder

Signature CreateRpoBuilder(rpo)

Parameters:	rpo (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be repositioned
Returns:	RPOBuilder object
Return type:	`NXOpen.Features.RPOBuilder`

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateRuledBuilder¶

FeatureCollection.CreateRuledBuilder¶

Creates a Ruled Surface builder

Signature CreateRuledBuilder(ruled)

Parameters:	ruled (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited
Returns:
Return type:	`NXOpen.Features.RuledBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateScaleBuilder¶

FeatureCollection.CreateScaleBuilder¶

Creates a NXOpen.Features.ScaleBuilder

Signature CreateScaleBuilder(scale)

Parameters:	scale (`NXOpen.Features.Feature`) – `NXOpen.Features.Scale` to be edited
Returns:	ScaleBuilder object
Return type:	`NXOpen.Features.ScaleBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateSeatBeltAnchorageBuilder¶

FeatureCollection.CreateSeatBeltAnchorageBuilder¶

Creates a NXOpen.Features.VehicleDesign.SeatBeltAnchorageBuilder

Signature CreateSeatBeltAnchorageBuilder(seatBeltAnchorage)

Parameters:	seatBeltAnchorage (`NXOpen.Features.Feature`) – Feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use Features.VehicleDesignCollection.CreateSeatBeltAnchorageBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreateSectionCurveBuilder¶

FeatureCollection.CreateSectionCurveBuilder¶

Creates a NXOpen.Features.SectionCurveBuilder

Signature CreateSectionCurveBuilder(sectionCurves)

Parameters:	sectionCurves (`NXOpen.Features.Feature`) – `NXOpen.Features.SectionCurve` to be edited
Returns:
Return type:	`NXOpen.Features.SectionCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSectionEditBuilder¶

FeatureCollection.CreateSectionEditBuilder¶

Creates a NXOpen.Features.SectionEditBuilder

Signature CreateSectionEditBuilder(sectionEdit)

Parameters:	sectionEdit (`NXOpen.Features.SectionEdit`) – `NXOpen.Features.SectionEdit` to be edited
Returns:
Return type:	`NXOpen.Features.SectionEditBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSectionInertiaAnalysisBuilder¶

FeatureCollection.CreateSectionInertiaAnalysisBuilder¶

Creates a NXOpen.Features.SectionInertiaAnalysisBuilder

Signature CreateSectionInertiaAnalysisBuilder(sectionInertiaAnalysis)

Parameters:	sectionInertiaAnalysis (`NXOpen.Features.SectionInertiaAnalysis`) – `NXOpen.Features.SectionInertiaAnalysis` to be edited
Returns:
Return type:	`NXOpen.Features.SectionInertiaAnalysisBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSectionSurfaceBuilder¶

FeatureCollection.CreateSectionSurfaceBuilder¶

Create a section surface

Signature CreateSectionSurfaceBuilder(sectionSurface)

Parameters:	sectionSurface (`NXOpen.Features.SectionSurface`) – `NXOpen.Features.SectionSurface` to be edited
Returns:
Return type:	`NXOpen.Features.SectionSurfaceBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.FeatureCollection.CreateSectionSurfaceBuilderEx() instead.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSectionSurfaceBuilderEx¶

FeatureCollection.CreateSectionSurfaceBuilderEx¶

Creates a NXOpen.Features.SectionSurfaceBuilderEx

Signature CreateSectionSurfaceBuilderEx(sectionSurfaceEx)

Parameters:	sectionSurfaceEx (`NXOpen.Features.SectionSurface`) – `NXOpen.Features.SectionSurface` to be edited
Returns:
Return type:	`NXOpen.Features.SectionSurfaceBuilderEx`

New in version NX9.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSewBuilder¶

FeatureCollection.CreateSewBuilder¶

Creates a Sew feature builder

Signature CreateSewBuilder(sew)

Parameters:	sew (`NXOpen.Features.Feature`) – `NXOpen.Features.SewBuilder` to be edited
Returns:	SewBuilder object
Return type:	`NXOpen.Features.SewBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateShellBuilder¶

FeatureCollection.CreateShellBuilder¶

Creates an Shell builder

Signature CreateShellBuilder(shell)

Parameters:	shell (`NXOpen.Features.Feature`) – `NXOpen.Features.ShellBuilder` to be edited
Returns:	ShellBuilder object
Return type:	`NXOpen.Features.ShellBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateShellFaceBuilder¶

FeatureCollection.CreateShellFaceBuilder¶

Creates a NXOpen.Features.ShellFaceBuilder

Signature CreateShellFaceBuilder(shellFace)

Parameters:	shellFace (`NXOpen.Features.ShellFace`) – `NXOpen.Features.ShellFace` to be edited
Returns:	`NXOpen.Features.ShellFaceBuilder` object
Return type:	`NXOpen.Features.ShellFaceBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateShowRelatedFacesBuilder¶

FeatureCollection.CreateShowRelatedFacesBuilder¶

Creates a NXOpen.Features.ShowRelatedFacesBuilder

Signature CreateShowRelatedFacesBuilder()

Returns:
Return type:	`NXOpen.Features.ShowRelatedFacesBuilder`

New in version NX7.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateSilhouetteFlangeBuilder¶

FeatureCollection.CreateSilhouetteFlangeBuilder¶

Creates a NXOpen.Features.SilhouetteFlangeBuilder

Signature CreateSilhouetteFlangeBuilder(silhouetteFlange)

Parameters:	silhouetteFlange (`NXOpen.Features.SilhouetteFlange`) – `NXOpen.Features.SilhouetteFlange` to be edited
Returns:
Return type:	`NXOpen.Features.SilhouetteFlangeBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateSketchFitCurveBuilder¶

FeatureCollection.CreateSketchFitCurveBuilder¶

Creates a NXOpen.Features.SketchFitCurveBuilder

Signature CreateSketchFitCurveBuilder(fitCurve)

Parameters:	fitCurve (`NXOpen.Curve`) – `NXOpen.Curve` to be edited
Returns:	SketchFitCurveBuilder object
Return type:	`NXOpen.Features.SketchFitCurveBuilder`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSketchSplineBuilder¶

FeatureCollection.CreateSketchSplineBuilder¶

Creates a Studio Spline builder for sketcher

Signature CreateSketchSplineBuilder(spline)

Parameters:	spline (`NXOpen.Spline`) – `NXOpen.Spline` to be edited
Returns:	SketchSplineBuilder object
Return type:	`NXOpen.Features.SketchSplineBuilder`

New in version NX8.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR geometric_tol (“GDT”), solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

CreateSmoothSplineBuilder¶

FeatureCollection.CreateSmoothSplineBuilder¶

Creates a NXOpen.Features.SmoothSplineBuilder

Signature CreateSmoothSplineBuilder(smoothSpline)

Parameters:	smoothSpline (`NXOpen.Features.SmoothSpline`) – `NXOpen.Features.SmoothSpline` to be edited
Returns:
Return type:	`NXOpen.Features.SmoothSplineBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

CreateSnipSurfaceBuilder¶

FeatureCollection.CreateSnipSurfaceBuilder¶

Creates a NXOpen.Features.SnipSurfaceBuilder

Signature CreateSnipSurfaceBuilder(snipSurface)

Parameters:	snipSurface (`NXOpen.Features.SnipSurface`) – `NXOpen.Features.SnipSurface` to be edited
Returns:
Return type:	`NXOpen.Features.SnipSurfaceBuilder`

New in version NX6.0.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateSphereBuilder¶

FeatureCollection.CreateSphereBuilder¶

Creates a NXOpen.Features.SphereBuilder

Signature CreateSphereBuilder(sphere)

Parameters:	sphere (`NXOpen.Features.Sphere`) – `NXOpen.Features.Sphere` to be edited
Returns:
Return type:	`NXOpen.Features.SphereBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSphericalCornerBuilder¶

FeatureCollection.CreateSphericalCornerBuilder¶

Creates a NXOpen.Features.SphericalCornerBuilder

Signature CreateSphericalCornerBuilder(sphericalCorner)

Parameters:	sphericalCorner (`NXOpen.Features.SphericalCorner`) – `NXOpen.Features.SphericalCorner` to be edited
Returns:
Return type:	`NXOpen.Features.SphericalCornerBuilder`

New in version NX8.5.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateSplitBodyBuilder¶

FeatureCollection.CreateSplitBodyBuilder¶

Creates a NXOpen.Features.SplitBodyBuilder

Signature CreateSplitBodyBuilder(splitBody)

Parameters:	splitBody (`NXOpen.Features.SplitBody`) – `NXOpen.Features.SplitBody` to be edited
Returns:
Return type:	`NXOpen.Features.SplitBodyBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSplitBodyBuilderUsingCollector¶

FeatureCollection.CreateSplitBodyBuilderUsingCollector¶

Creates a NXOpen.Features.SplitBodyBuilder.

Leverage body collectors if possible

Signature CreateSplitBodyBuilderUsingCollector(splitBody)

Parameters:	splitBody (`NXOpen.Features.SplitBody`) – `NXOpen.Features.SplitBody` to be edited
Returns:
Return type:	`NXOpen.Features.SplitBodyBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateStudioSplineBuilder¶

FeatureCollection.CreateStudioSplineBuilder¶

Creates a Studio Spline builder

Signature CreateStudioSplineBuilder(splineFeature)

Parameters:	splineFeature (`NXOpen.Features.StudioSpline`) – `NXOpen.Features.StudioSpline` to be edited
Returns:	StudioSplineBuilder object
Return type:	`NXOpen.Features.StudioSplineBuilder`

New in version NX5.0.0.

Deprecated since version NX8.0.0: Use NXOpen.Features.FeatureCollection.CreateStudioSplineBuilderEx() instead.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateStudioSplineBuilderEx¶

FeatureCollection.CreateStudioSplineBuilderEx¶

Creates a Studio Spline builder

Signature CreateStudioSplineBuilderEx(spline)

Parameters:	spline (`NXOpen.NXObject`) – `NXOpen.Features.StudioSpline` or `NXOpen.Spline` to be edited
Returns:	StudioSplineBuilderEx object
Return type:	`NXOpen.Features.StudioSplineBuilderEx`

New in version NX8.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateStudioSurfaceBuilder¶

FeatureCollection.CreateStudioSurfaceBuilder¶

Creates a Studio Surface Builder

Signature CreateStudioSurfaceBuilder(studioSurface)

Parameters:	studioSurface (`NXOpen.Features.Feature`) – `NXOpen.Features.StudioSurface` to be edited
Returns:	StudioSurfaceBuilder

object :rtype: NXOpen.Features.StudioSurfaceBuilder

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateStudioXformBuilder¶

FeatureCollection.CreateStudioXformBuilder¶

Creates a Features.

StudioXformBuilder

Signature CreateStudioXformBuilder(studioXform)

Parameters:	studioXform (`NXOpen.Features.StudioXform`) – `NXOpen.Features.StudioXform` to be edited
Returns:
Return type:	`NXOpen.Features.StudioXformBuilder`

New in version NX6.0.0.

Deprecated since version NX8.5.0: Use NXOpen.Features.FeatureCollection.CreateStudioXformBuilderEx() instead.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateStudioXformBuilderEx¶

FeatureCollection.CreateStudioXformBuilderEx¶

Creates a Features.

StudioXformBuilderEx

Signature CreateStudioXformBuilderEx(studioXform1)

Parameters:	studioXform1 (`NXOpen.Features.StudioXform`) – `NXOpen.Features.StudioXform` to be edited
Returns:
Return type:	`NXOpen.Features.StudioXformBuilderEx`

New in version NX7.0.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateStyledBlendBuilder¶

FeatureCollection.CreateStyledBlendBuilder¶

Creates a NXOpen.Features.StyledBlendBuilder

Signature CreateStyledBlendBuilder(styledBlend)

Parameters:	styledBlend (`NXOpen.Features.StyledBlend`) – `NXOpen.Features.StyledBlend` to be edited
Returns:
Return type:	`NXOpen.Features.StyledBlendBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateStyledCornerBuilder¶

FeatureCollection.CreateStyledCornerBuilder¶

Creates a NXOpen.Features.StyledCornerBuilder

Signature CreateStyledCornerBuilder(styledCorner)

Parameters:	styledCorner (`NXOpen.Features.StyledCorner`) – `NXOpen.Features.StyledCorner` to be edited
Returns:
Return type:	`NXOpen.Features.StyledCornerBuilder`

New in version NX6.0.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateStyledSweepBuilder¶

FeatureCollection.CreateStyledSweepBuilder¶

Creates a NXOpen.Features.StyledSweepBuilder

Signature CreateStyledSweepBuilder(styledSweep)

Parameters:	styledSweep (`NXOpen.Features.Feature`) – `NXOpen.Features.StyledSweep` to be edited
Returns:	Features.

StyledSweepBuilder object :rtype: NXOpen.Features.StyledSweepBuilder

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR studio_free_form (“STUDIO FREE FORM”)

CreateSubtractFeature¶

FeatureCollection.CreateSubtractFeature¶

Creates a subtract feature.

Signature CreateSubtractFeature(targetBody, retainTargetBody, toolBodies, retainToolBodies, allowNonAssociativeBoolean)

Parameters:	targetBody (`NXOpen.Body`) – Target body retainTargetBody (bool) – Retain option for target body toolBodies (list of `NXOpen.Body`) – Tool bodies retainToolBodies (bool) – Retain option for tool bodies allowNonAssociativeBoolean (bool) – Allow boolean operation even if it results into non-associative boolean
Returns:	a tuple
Return type:	A tuple consisting of (features, nonAssociativeBoolean, unparameterizedSolids). features is a list of `NXOpen.Features.BooleanFeature`. Array of boolean features nonAssociativeBoolean is a bool. True if operation resulted in a non-associative boolean. False otherwise unparameterizedSolids is a bool. True if operation resulted in unparameterized solids. False otherwise

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSweepAlongGuideBuilder¶

FeatureCollection.CreateSweepAlongGuideBuilder¶

Creates a NXOpen.Features.SweepAlongGuideBuilder

Signature CreateSweepAlongGuideBuilder(sweepAlongGuide)

Parameters:	sweepAlongGuide (`NXOpen.Features.SweepAlongGuide`) – `NXOpen.Features.SweepAlongGuide` to be edited
Returns:
Return type:	`NXOpen.Features.SweepAlongGuideBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSweptBuilder¶

FeatureCollection.CreateSweptBuilder¶

Creates a NXOpen.Features.SweptBuilder

Signature CreateSweptBuilder(swept)

Parameters:	swept (`NXOpen.Features.Swept`) – `NXOpen.Features.Swept` to be edited
Returns:
Return type:	`NXOpen.Features.SweptBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateSymmetricBuilder¶

FeatureCollection.CreateSymmetricBuilder¶

Creates a NXOpen.Features.SymmetricBuilder

Signature CreateSymmetricBuilder(symmetric)

Parameters:	symmetric (`NXOpen.Features.Symmetric`) – `NXOpen.Features.Symmetric` to be edited
Returns:
Return type:	`NXOpen.Features.SymmetricBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateTangentBuilder¶

FeatureCollection.CreateTangentBuilder¶

Creates a NXOpen.Features.TangentBuilder

Signature CreateTangentBuilder(tangent)

Parameters:	tangent (`NXOpen.Features.Tangent`) – `NXOpen.Features.Tangent` to be edited
Returns:	Features.

TangentBuilder object :rtype: NXOpen.Features.TangentBuilder

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”), solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateTextBuilder¶

FeatureCollection.CreateTextBuilder¶

Creates a NXOpen.Features.TextBuilder

Signature CreateTextBuilder(text)

Parameters:	text (`NXOpen.Features.Text`) – `NXOpen.Features.Text` to be edited
Returns:
Return type:	`NXOpen.Features.TextBuilder`

New in version NX7.5.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateThickenBuilder¶

FeatureCollection.CreateThickenBuilder¶

Creates a Thicken feature builder

Signature CreateThickenBuilder(thicken)

Parameters:	thicken (`NXOpen.Features.Feature`) – `NXOpen.Features.Thicken` to be edited
Returns:	ThickenBuilder object
Return type:	`NXOpen.Features.ThickenBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateThroughCurveMeshBuilder¶

FeatureCollection.CreateThroughCurveMeshBuilder¶

Creates a NXOpen.Features.ThroughCurveMeshBuilder

Signature CreateThroughCurveMeshBuilder(throughCurveMesh)

Parameters:	throughCurveMesh (`NXOpen.Features.Feature`) – `NXOpen.Features.ThroughCurveMesh` to be edited, if None then create a new one
Returns:	ThroughCurveMeshBuilder object
Return type:	`NXOpen.Features.ThroughCurveMeshBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateThroughCurvesBuilder¶

FeatureCollection.CreateThroughCurvesBuilder¶

Creates a NXOpen.Features.ThroughCurvesBuilder

Signature CreateThroughCurvesBuilder(throughCurves)

Parameters:	throughCurves (`NXOpen.Features.Feature`) – `NXOpen.Features.ThroughCurves` to be edited, if None then create a new one
Returns:	ThroughCurvesBuilder object
Return type:	`NXOpen.Features.ThroughCurvesBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateTrimBody2Builder¶

FeatureCollection.CreateTrimBody2Builder¶

Creates a NXOpen.Features.TrimBody2Builder for Trim Body feature

Signature CreateTrimBody2Builder(trimBody2)

Parameters:	trimBody2 (`NXOpen.Features.TrimBody2`) – `NXOpen.Features.TrimBody2` to be edited
Returns:
Return type:	`NXOpen.Features.TrimBody2Builder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateTrimBodyBuilder¶

FeatureCollection.CreateTrimBodyBuilder¶

Creates a trim body builder object.

Use this method only for editing pre-NX7.5.0 trim body features.. Use CreateTrimBody2Builder() and NXOpen.Features.TrimBody2 to create and edit trim body features.

Signature CreateTrimBodyBuilder(trimbodyFeat)

Parameters:	trimbodyFeat (`NXOpen.Features.Feature`) – `NXOpen.Features.TrimBody` to be edited
Returns:	Features.TrimBodyBuilder object
Return type:	`NXOpen.Features.TrimBodyBuilder`

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateTrimCurve2FeatureBuilder¶

FeatureCollection.CreateTrimCurve2FeatureBuilder¶

Creates a NXOpen.Features.TrimCurve2Builder

Signature CreateTrimCurve2FeatureBuilder(trimCurve2Feature)

Parameters:	trimCurve2Feature (`NXOpen.Features.TrimCurve2`) – `NXOpen.Features.TrimCurve2` to be edited
Returns:
Return type:	`NXOpen.Features.TrimCurve2Builder`

New in version NX11.0.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateTrimCurveBuilder¶

FeatureCollection.CreateTrimCurveBuilder¶

Overloaded method CreateTrimCurveBuilder

CreateTrimCurveBuilder(trimCurve)
CreateTrimCurveBuilder(trimCurve)

-------------------------------------

Creates a NXOpen.Features.TrimCurveBuilder

Signature CreateTrimCurveBuilder(trimCurve)

Parameters:	trimCurve (`NXOpen.Features.TrimCurve`) – `NXOpen.Features.TrimCurve` to be edited
Returns:	Trim Curve Builder object
Return type:	`NXOpen.Features.TrimCurveBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

-------------------------------------

Creates a NXOpen.Features.TrimCurveBuilder

Signature CreateTrimCurveBuilder(trimCurve)

Parameters:	trimCurve (`NXOpen.Spline`) – The trimmed curve to be edited
Returns:	Trim Curve Builder object
Return type:	`NXOpen.Features.TrimCurveBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

-------------------------------------

CreateTrimExtendBuilder¶

FeatureCollection.CreateTrimExtendBuilder¶

Creates a NXOpen.Features.TrimExtendBuilder

Signature CreateTrimExtendBuilder(trimExtend)

Parameters:	trimExtend (`NXOpen.Features.Feature`) – `NXOpen.Features.TrimExtend` to be edited
Returns:
Return type:	`NXOpen.Features.TrimExtendBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateTrimsheetBuilder¶

FeatureCollection.CreateTrimsheetBuilder¶

Creates a NXOpen.Features.TrimSheetBuilder

Signature CreateTrimsheetBuilder(trimSheet)

Parameters:	trimSheet (`NXOpen.Features.Feature`) – `NXOpen.Features.TrimSheet` to be edited, if None then create a new one
Returns:	Trim Sheet Builder object
Return type:	`NXOpen.Features.TrimSheetBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateTubeBuilder¶

FeatureCollection.CreateTubeBuilder¶

Creates a NXOpen.Features.TubeBuilder

Signature CreateTubeBuilder(tube)

Parameters:	tube (`NXOpen.Features.Feature`) – `NXOpen.Features.TubeBuilder` to be edited
Returns:	TubeBuilder object
Return type:	`NXOpen.Features.TubeBuilder`

New in version NX5.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CreateUniteFeature¶

FeatureCollection.CreateUniteFeature¶

Creates a unite feature.

Signature CreateUniteFeature(targetBody, retainTargetBody, toolBodies, retainToolBodies, allowNonAssociativeBoolean)

Parameters:	targetBody (`NXOpen.Body`) – Target body retainTargetBody (bool) – Retain option for target body toolBodies (list of `NXOpen.Body`) – Tool bodies retainToolBodies (bool) – Retain option for tool bodies allowNonAssociativeBoolean (bool) – Allow boolean operation even if it results into non-associative boolean
Returns:	a tuple
Return type:	A tuple consisting of (features, nonAssociativeBoolean, unparameterizedSolids). features is a list of `NXOpen.Features.BooleanFeature`. Array of boolean features nonAssociativeBoolean is a bool. True if operation resulted in a non-associative boolean. False otherwise unparameterizedSolids is a bool. True if operation resulted in unparameterized solids. False otherwise

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateUnnestModuleBuilder¶

FeatureCollection.CreateUnnestModuleBuilder¶

Creates a NXOpen.GeometricUtilities.UnnestModuleBuilder

This API is now deprecated. Please use NXOpen.Features.FeatureCollection instead.

Signature CreateUnnestModuleBuilder()

Returns:	Returns a `NXOpen.GeometricUtilities.UnnestModuleBuilder` builder
Return type:	`NXOpen.GeometricUtilities.UnnestModuleBuilder`

New in version NX9.0.0.

Deprecated since version NX10.0.0: Please use NXOpen.Features.FeatureCollection instead.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateUnsewBuilder¶

FeatureCollection.CreateUnsewBuilder¶

Creates a NXOpen.Features.UnsewBuilder

Signature CreateUnsewBuilder(unsew)

Parameters:	unsew (`NXOpen.Features.Unsew`) – `NXOpen.Features.Unsew` to be edited
Returns:
Return type:	`NXOpen.Features.UnsewBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateUntrimBuilder¶

FeatureCollection.CreateUntrimBuilder¶

Creates a NXOpen.Features.UntrimBuilder

Signature CreateUntrimBuilder(untrim)

Parameters:	untrim (`NXOpen.Features.Feature`) – `NXOpen.Features.Untrim` to be edited
Returns:	Features.

UntrimBuilder object :rtype: NXOpen.Features.UntrimBuilder

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateUserDefinedObjectFeatureBuilder¶

FeatureCollection.CreateUserDefinedObjectFeatureBuilder¶

Creates a UserDefinedObjectFeature builder

Signature CreateUserDefinedObjectFeatureBuilder(udoFeature)

Parameters:	udoFeature (`NXOpen.Features.Feature`) – `NXOpen.Features.UserDefinedObjectFeature` to be edited - may be None if creating a new feature.
Returns:	UserDefinedObjectFeatureBuilder object
Return type:	`NXOpen.Features.UserDefinedObjectFeatureBuilder`

New in version NX5.0.0.

License requirements: None.

CreateVarOffsetFaceBuilder¶

FeatureCollection.CreateVarOffsetFaceBuilder¶

Creates a NXOpen.Features.VarOffsetFaceBuilder

Signature CreateVarOffsetFaceBuilder(varOffsetFace)

Parameters:	varOffsetFace (`NXOpen.Features.VarOffsetFace`) – `Features.VarOffsetFace` to be edited
Returns:
Return type:	`NXOpen.Features.VarOffsetFaceBuilder`

New in version NX11.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateVariableOffsetBuilder¶

FeatureCollection.CreateVariableOffsetBuilder¶

Creates a NXOpen.Features.VariableOffsetBuilder

Signature CreateVariableOffsetBuilder(variableOffset)

Parameters:	variableOffset (`NXOpen.Features.VariableOffset`) – `NXOpen.Features.VariableOffset` to be edited
Returns:
Return type:	`NXOpen.Features.VariableOffsetBuilder`

New in version NX8.0.0.

License requirements: studio_free_form (“STUDIO FREE FORM”)

CreateVarsweepBuilder¶

FeatureCollection.CreateVarsweepBuilder¶

Creates a Varsweep feature builder

Signature CreateVarsweepBuilder(varsweep)

Parameters:	varsweep (`NXOpen.Features.Feature`) – Varsweep to be edited
Returns:	VarsweepBuilder object
Return type:	`NXOpen.Features.VarsweepBuilder`

New in version NX4.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateVehicleCoordinateSystemBuilder¶

FeatureCollection.CreateVehicleCoordinateSystemBuilder¶

Creates a NXOpen.Features.VehicleDesign.VehicleCoordinateSystemBuilder

Signature CreateVehicleCoordinateSystemBuilder(vehicleCoordinateSystem)

Parameters:	vehicleCoordinateSystem (`NXOpen.Features.Feature`) – feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX7.5.0.

Deprecated since version NX9.0.0: Use Features.VehicleDesignCollection.CreateHoodVisibilityBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”) OR ug_body_design (“Body Design”) OR nx_posture (“NX Jack Posture Prediction”)

CreateVirtualBlendEdgeBuilder¶

FeatureCollection.CreateVirtualBlendEdgeBuilder¶

Creates a NXOpen.Features.VirtualBlendEdgeBuilder

Signature CreateVirtualBlendEdgeBuilder()

Returns:
Return type:	`NXOpen.Features.VirtualBlendEdgeBuilder`

New in version NX7.0.1.

License requirements: None.

CreateVirtualCurveBuilder¶

FeatureCollection.CreateVirtualCurveBuilder¶

Creates a NXOpen.Features.VirtualCurveBuilder

Signature CreateVirtualCurveBuilder(virtualCurve)

Parameters:	virtualCurve (`NXOpen.Features.VirtualCurve`) – `NXOpen.Features.VirtualCurve` to be edited
Returns:
Return type:	`NXOpen.Features.VirtualCurveBuilder`

New in version NX7.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateVisionPlaneBuilder¶

FeatureCollection.CreateVisionPlaneBuilder¶

Creates a NXOpen.Features.VehicleDesign.VisionPlaneBuilder

Signature CreateVisionPlaneBuilder(visionPlane)

Parameters:	visionPlane (`NXOpen.Features.Feature`) – feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.VehicleDesignCollection.CreateVisionPlaneBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreateWaveDatumBuilder¶

FeatureCollection.CreateWaveDatumBuilder¶

Creates a Wavedatum Builder

Signature CreateWaveDatumBuilder(wavedatum)

Parameters:	wavedatum (`NXOpen.Features.Feature`) – Wavedatum Features to be edited
Returns:
Return type:	`NXOpen.Features.WaveDatumBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateWavePointBuilder¶

FeatureCollection.CreateWavePointBuilder¶

Creates a NXOpen.Features.WavePointBuilder

Signature CreateWavePointBuilder(wavepoint)

Parameters:	wavepoint (`NXOpen.Features.Feature`) – Wavepoint Features to be edited
Returns:
Return type:	`NXOpen.Features.WavePointBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

CreateWaveRoutingBuilder¶

FeatureCollection.CreateWaveRoutingBuilder¶

Creates a NXOpen.Features.WaveRoutingBuilder

Signature CreateWaveRoutingBuilder(waverouting)

Parameters:	waverouting (`NXOpen.Features.Feature`) – Waverouting Features to be edited
Returns:
Return type:	`NXOpen.Features.WaveRoutingBuilder`

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateWaveSketchBuilder¶

FeatureCollection.CreateWaveSketchBuilder¶

Creates a Wavesketch Builder

Signature CreateWaveSketchBuilder(wavesketch)

Parameters:	wavesketch (`NXOpen.Features.Feature`) – Wavesketch Features to be edited
Returns:
Return type:	`NXOpen.Features.WaveSketchBuilder`

New in version NX5.0.1.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateWindshieldDatumBuilder¶

FeatureCollection.CreateWindshieldDatumBuilder¶

Creates a NXOpen.Features.VehicleDesign.WindshieldDatumBuilder

Signature CreateWindshieldDatumBuilder(windshieldDatum)

Parameters:	windshieldDatum (`NXOpen.Features.Feature`) – feature to be edited
Returns:
Return type:	`NXOpen.Features.FeatureBuilder`

New in version NX6.0.0.

Deprecated since version NX9.0.0: Use NXOpen.Features.VehicleDesignCollection.CreateWindshieldDatumBuilder() instead.

License requirements: nx_general_packaging (“NX General Packaging”)

CreateWrapBuilder¶

FeatureCollection.CreateWrapBuilder¶

Creates a NXOpen.Features.WrapBuilder

Signature CreateWrapBuilder(wrap)

Parameters:	wrap (`NXOpen.Features.WrapUnwrap`) – `NXOpen.Features.WrapUnwrap` to be edited
Returns:	WrapBuilder object
Return type:	`NXOpen.Features.WrapBuilder`

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

CreateWrapGeometryBuilder¶

FeatureCollection.CreateWrapGeometryBuilder¶

Creates a NXOpen.Features.WrapGeometryBuilder

Signature CreateWrapGeometryBuilder(wrapGeometry)

Parameters:	wrapGeometry (`NXOpen.Features.WrapGeometry`) – `NXOpen.Features.WrapGeometry` to be edited
Returns:
Return type:	`NXOpen.Features.WrapGeometryBuilder`

New in version NX6.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

DeleteAllPartInformationalFeatureAlerts¶

FeatureCollection.DeleteAllPartInformationalFeatureAlerts¶

Delete all informational alerts from all the features in a given part

Signature DeleteAllPartInformationalFeatureAlerts()

New in version NX5.0.0.

License requirements: None.

DeleteInformationalAlerts¶

FeatureCollection.DeleteInformationalAlerts¶

Delete all informational alerts from the features and if numFrecs is 0 then delete informational alerts from all features in the part

Signature DeleteInformationalAlerts(feature)

Parameters:	feature (list of `NXOpen.NXObject`) – Array of feature on which information alerts are to be deleted

New in version NX10.0.0.

License requirements: None.

DeleteWarningAlerts¶

FeatureCollection.DeleteWarningAlerts¶

Delete all warning alerts from the features and if numFrecs is 0 then delete warning alerts from all features in the part

Signature DeleteWarningAlerts(feature)

Parameters:	feature (list of `NXOpen.NXObject`) – Array of feature on which warning alerts are to be deleted

New in version NX10.0.0.

License requirements: None.

FindObject¶

FeatureCollection.FindObject¶

Finds the NXOpen.Features 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) – Identifier of the body you want
Returns:	Feature with this identifier
Return type:	`NXOpen.Features.Feature`

New in version NX3.0.0.

License requirements: None.

GetAllPartFeaturesWithAlerts¶

FeatureCollection.GetAllPartFeaturesWithAlerts¶

Returns a list of all features from a given part that have update alerts

Signature GetAllPartFeaturesWithAlerts()

Returns:
Return type:	list of `NXOpen.Features.Feature`

New in version NX5.0.0.

License requirements: None.

GetAssociatedFeature¶

FeatureCollection.GetAssociatedFeature¶

Get the feature associated with an object

Signature GetAssociatedFeature(object)

Parameters:	object (`NXOpen.NXObject`) – Object to find associated feature.
Returns:	Feature associated with object. Set to Null if no feature is associated to the object.
Return type:	`NXOpen.Features.Feature`

New in version NX3.0.0.

License requirements: None.

GetAssociatedFeaturesOfBody¶

FeatureCollection.GetAssociatedFeaturesOfBody¶

Returns all features that are associated with this body

Signature GetAssociatedFeaturesOfBody(body)

Parameters:	body (`NXOpen.Body`) – `NXOpen.Body` whose associated features you want
Returns:	The associated NXOpen.Features.Feature`s of the input :py:class:`NXOpen.Body
Return type:	list of `NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetAssociatedFeaturesOfEdge¶

FeatureCollection.GetAssociatedFeaturesOfEdge¶

Returns all features that are associated with the faces of this edge

Signature GetAssociatedFeaturesOfEdge(edge)

Parameters:	edge (`NXOpen.Edge`) – `NXOpen.Edge` whose associated features you want
Returns:	The associated NXOpen.Features.Feature`s of the input :py:class:`NXOpen.Edge
Return type:	list of `NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetAssociatedFeaturesOfFace¶

FeatureCollection.GetAssociatedFeaturesOfFace¶

Returns all features associated with this face

Signature GetAssociatedFeaturesOfFace(face)

Parameters:	face (`NXOpen.Face`) – `NXOpen.Face` whose associated features you want
Returns:	The associated NXOpen.Features.Feature`s of the input :py:class:`NXOpen.Face
Return type:	list of `NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetFeatures¶

FeatureCollection.GetFeatures¶

Returns all the features in the part.

Note that this is a low level routine that can return additional features that are not browseable in the user interface. The order in which features are returned is not significant and may change

Signature GetFeatures()

Returns:	Features in the part
Return type:	list of `NXOpen.Features.Feature`

New in version NX3.0.0.

License requirements: None.

GetIsMasterCutVisibleInView¶

FeatureCollection.GetIsMasterCutVisibleInView¶

Returns if a NXOpen.Features.MasterCutBuilder is visible in specified NXOpen.CutView .

Signature GetIsMasterCutVisibleInView(masterCut, view)

Parameters:	masterCut (`NXOpen.Features.Feature`) – `NXOpen.Features.MasterCutBuilder` to be tested view (`NXOpen.CutView`) – Cut view
Returns:	True if master cut is visible in view

False otherwise :rtype: bool

New in version NX5.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetParentFeatureOfBody¶

FeatureCollection.GetParentFeatureOfBody¶

Returns the feature that created this body.

Signature GetParentFeatureOfBody(body)

Parameters:	body (`NXOpen.Body`) – `NXOpen.Body` whose parent features you want
Returns:	The parent `NXOpen.Features.Feature` of the input `NXOpen.Body`
Return type:	`NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetParentFeatureOfFace¶

FeatureCollection.GetParentFeatureOfFace¶

Returns the feature that created this face

Signature GetParentFeatureOfFace(face)

Parameters:	face (`NXOpen.Face`) – `NXOpen.Face` whose parent feature you want
Returns:	The parent `NXOpen.Features.Feature` of the input `NXOpen.Face`
Return type:	`NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetParentFeaturesOfEdge¶

FeatureCollection.GetParentFeaturesOfEdge¶

Returns the features that created the faces of this edge.

Typically the parent features of the 2 faces of the edge will be returned

Signature GetParentFeaturesOfEdge(edge)

Parameters:	edge (`NXOpen.Edge`) – `NXOpen.Edge` whose parent features you want
Returns:	The parent NXOpen.Features.Feature`s of the input :py:class:`NXOpen.Edge
Return type:	list of `NXOpen.Features.Feature`

New in version NX8.5.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

GetPartFeaturesWithNewAlerts¶

FeatureCollection.GetPartFeaturesWithNewAlerts¶

Returns a list of features that generated update alerts during recent update

Signature GetPartFeaturesWithNewAlerts()

Returns:
Return type:	list of `NXOpen.Features.Feature`

New in version NX5.0.0.

License requirements: None.

InsertNewDesignGroup¶

FeatureCollection.InsertNewDesignGroup¶

Creates a new empty design group after a specified referece design group

Signature InsertNewDesignGroup(referenceDesignGroup)

Parameters:	referenceDesignGroup (`NXOpen.Features.Feature`) – Reference design group to create new feature after
Returns:	The new created design group
Return type:	`NXOpen.Features.Feature`

New in version NX12.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

ReorderFeature¶

FeatureCollection.ReorderFeature¶

Reorders the Feature with respect to the given feature

Signature ReorderFeature(features, target, beforeOrAfter)

Parameters:	features (list of `NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be reordered target (`NXOpen.Features.Feature`) – Target feature beforeOrAfter (`NXOpen.Features.FeatureCollectionReorderType`) – Reorder Before/After

New in version NX6.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

ReorganizeFeature¶

FeatureCollection.ReorganizeFeature¶

Reorganizes the Feature with respect to the given feature across the part module

Signature ReorganizeFeature(features, target, beforeOrAfter)

Parameters:	features (list of `NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be reorganized target (`NXOpen.Features.Feature`) – Target feature beforeOrAfter (`NXOpen.Features.FeatureCollectionReorderType`) – Reorder Before/After

New in version NX10.0.0.

License requirements: usr_defined_features (“USER DEFINED FEATURES”)

ReplaceWithIndependentSketch¶

FeatureCollection.ReplaceWithIndependentSketch¶

Replace the given features with Independent Sketch

Signature ReplaceWithIndependentSketch(features)

Parameters:	features (list of `NXOpen.Features.Feature`) – Features to be replaced
Returns:
Return type:	`NXOpen.Features.SketchConversionReport`

New in version NX7.5.0.

License requirements: None.

SetCanResetMcf¶

FeatureCollection.SetCanResetMcf¶

Sets whether mcf is allowed

Signature SetCanResetMcf(canResetMcf)

Parameters:	canResetMcf (bool) –

New in version NX8.5.0.

License requirements: None.

SetEditWithRollbackFeature¶

FeatureCollection.SetEditWithRollbackFeature¶

Sets the feature being edited with rollback

Signature SetEditWithRollbackFeature(feature)

Parameters:	feature (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited

New in version NX8.0.0.

License requirements: None.

StartEditWithRollbackManager¶

FeatureCollection.StartEditWithRollbackManager¶

Creates a NXOpen.Features.EditWithRollbackManager

Signature StartEditWithRollbackManager(featureToEdit, featureEditMark)

Parameters:	featureToEdit (`NXOpen.Features.Feature`) – `NXOpen.Features.Feature` to be edited featureEditMark (int) – If any error occurs during edit, the system will undo to this mark
Returns:	EditWithRollbackManager object
Return type:	`NXOpen.Features.EditWithRollbackManager`

New in version NX11.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

SuppressFeatures¶

FeatureCollection.SuppressFeatures¶

Suppress the given features

Signature SuppressFeatures(features)

Parameters:	features (list of `NXOpen.Features.Feature`) – Features to be suppressed

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)

UnsuppressFeatures¶

FeatureCollection.UnsuppressFeatures¶

Unsuppress the given features

Signature UnsuppressFeatures(features)

Parameters:	features (list of `NXOpen.Features.Feature`) – Features to be unsuppressed
Returns:	Features which were not unsuppressed due to errors
Return type:	list of `NXOpen.Features.Feature`

New in version NX3.0.0.

License requirements: solid_modeling (“SOLIDS MODELING”)