ExtractFaceBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# ExtractFaceBuilder Class

class `NXOpen.Features.``ExtractFaceBuilder`

  Bases: `NXOpen.Features.FeatureBuilder`

  Represents a `NXOpen.Features.ExtractFace` builder.

  Inputs to this class can be convergent objects.

  To create a new instance of this class, use `NXOpen.Features.FeatureCollection.CreateExtractFaceBuilder()`

  Default values.

  Property | Value
  --- | ---
  AngleTolerance | 45.0
  Associative | True
  CopyThreads | True
  DeleteHoles | False
  FixAtCurrentTimestamp | False
  InheritDisplayProperties | False
  IsPsmOutputBody | false
  MakePositionIndependent | False
  ReplacementAssistant.OneToOne | True

  New in version NX5.0.0.

# Properties

Property | Description
--- | ---
AngleTolerance | Returns or sets the angle Tolerance
Associative | Returns or sets the option that specifies whether the extract face operation is associative
BodyReverseDirection | Returns or sets the option to specify if the extracted faces should have the face normals reversed from the selected input bodies.
BodyToExtract | Returns the bodies
BoundaryFaces | Returns the boundary faces
CopyThreads | Returns or sets the copy threads option
DeleteHoles | Returns or sets the option to specify if holes should be deleted from the extracted faces
ExtractBodyCollector | Returns a collection of bodies to extract
FaceChain | Returns the face chain containing the faces to extract
FaceOption | Returns or sets the face option type
FaceReverseDirection | Returns or sets the option specifying whether to reverse the face normals for the extracted faces.
FacesToExtract | Returns the faces
FeatureOption | Returns or sets the feature option type
FixAtCurrentTimestamp | Returns or sets the option specifying whether to fix the extract face operation at the current timestamp
FrecAtTimeStamp | Returns or sets the option specifying if the results from this builder should be associated
HideOriginal | Returns or sets the option to specify if the original faces should be hidden
InheritDisplayProperties | Returns or sets the inherit display properties from source option
IsPsmOutputBody | Returns or sets the PSM Body Output option
MakePositionIndependent | Returns or sets the option to specify that the extracted faces should be position independent
ObjectToExtract | Returns a list of the extracted objects.
ParentFeatureInternal | Returns or sets whether or not the latest timestamped parent feature of this feature should be made internal
ParentPart | Returns or sets the source part type
PatchSolutionFlag | Returns or sets the patch solution flag
PatchSurfaceFilename | Returns or sets the patch surface filename
ReplacementAssistant | Returns the Replacement Assistant builder.
SeedFace | Returns the seed face for the face chain
SeedReverseDirection | Returns or sets the option that specifies whether to reverse the face normals of the extracted faces relative to the seed face chain
SourcePartOccurrence | Returns or sets the source part occurrence
SurfaceType | Returns or sets the surface type
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename
Tag | Returns the Tag for this object.
TraverseInteriorEdges | Returns or sets the traverse interior edges
Type | Returns or sets the type
UseTangentEdgeAngles | Returns or sets the use tangent angles

# Methods

Method | Description
--- | ---
Commit | Commits any edits that have been applied to the builder.
CommitCreateOnTheFly | Commits the feature and set create on the fly flag
CommitFeature | Commits the feature parameters and creates the feature
Destroy | Deletes the builder, and cleans up any objects created by the builder.
FlipFaceChainDirectionSense | Flip the face chain direction sense
GetCommittedObjects | For builders that create more than one object, this method returns the objects that are created by commit.
GetFaceChainDirectionSense | Returns the face chain direction sense for a given face in the face chain
GetFeature | Returns the feature currently being edited by this builder.
GetObject | Returns the object currently being edited by this builder.
GetProductInterfaceObjects | Gets selected product interface objects
GetSourcePartOccurrences | Gets source part occurrences
GetWaveLinkInformation | Prints wave browser type information about link
HideInternalParentFeatureAfterEdit | Re-suppress an internal parent feature (a slave feature) after it has been edited.
RecreateVectorOfHelpDirVector | Causes the recreation of vector for help dir
SetParentFeatureInternal | Set the parent features which would be internal or slaves to the feature being created or commited
SetProductInterfaceObjects | Sets selected product interface objects
SetSourcePartOccurrences | Sets source part occurrences
ShowInternalParentFeatureForEdit | Unsuppress an internal parent feature (a slave feature) so it can be edited.
ShowResults | Updates the model to reflect the result of an edit to the model for all builders that support showing results.
UnsetParentFeatureInternal | Set the internal parent feature of the feature being edited to external
Validate | Validate whether the inputs to the component are sufficient for commit to be called.

# Enumerations

ExtractFaceBuilderExtractType Enumeration | enum for feature type being extracted
ExtractFaceBuilderFaceOptionType Enumeration | enum for face option type
ExtractFaceBuilderFaceSurfaceType Enumeration | type of resulting surface
ExtractFaceBuilderFeatureOptionType Enumeration | enum for feature option type
ExtractFaceBuilderParentPartType Enumeration | enum for scope of part

# Property Detail

## AngleTolerance

`ExtractFaceBuilder.``AngleTolerance`

  Returns or sets the angle Tolerance

  `-------------------------------------`

  Getter Method

  Signature `AngleTolerance`

  Returns: |
  Return type: | float

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `AngleTolerance`

  Parameters: | angleTolerance (float) –

  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”)

## Associative

`ExtractFaceBuilder.``Associative`

  Returns or sets the option that specifies whether the extract face operation is associative

  `-------------------------------------`

  Getter Method

  Signature `Associative`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `Associative`

  Parameters: | associative (bool) –

  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”)

## BodyReverseDirection

`ExtractFaceBuilder.``BodyReverseDirection`

  Returns or sets the option to specify if the extracted faces should have the face normals reversed from the selected input bodies.

  `-------------------------------------`

  Getter Method

  Signature `BodyReverseDirection`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `BodyReverseDirection`

  Parameters: | bodyNormal (bool) –

  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”)

## BodyToExtract

`ExtractFaceBuilder.``BodyToExtract`

  Returns the bodies

  `-------------------------------------`

  Getter Method

  Signature `BodyToExtract`

  Returns: |
  Return type: | `NXOpen.SelectObjectList`

  New in version NX5.0.0.

  Deprecated since version NX9.0.0: Use `NXOpen.Features.ExtractFaceBuilder.ExtractBodyCollector()` instead.

  License requirements: None.

## BoundaryFaces

`ExtractFaceBuilder.``BoundaryFaces`

  Returns the boundary faces

  `-------------------------------------`

  Getter Method

  Signature `BoundaryFaces`

  Returns: |
  Return type: | `NXOpen.SelectFaceList`

  New in version NX5.0.0.

  License requirements: None.

## CopyThreads

`ExtractFaceBuilder.``CopyThreads`

  Returns or sets the copy threads option

  `-------------------------------------`

  Getter Method

  Signature `CopyThreads`

  Returns: |
  Return type: | bool

  New in version NX8.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `CopyThreads`

  Parameters: | copyThreads (bool) –

  New in version NX8.0.0.

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

## DeleteHoles

`ExtractFaceBuilder.``DeleteHoles`

  Returns or sets the option to specify if holes should be deleted from the extracted faces

  `-------------------------------------`

  Getter Method

  Signature `DeleteHoles`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `DeleteHoles`

  Parameters: | deleteHoles (bool) –

  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”)

## ExtractBodyCollector

`ExtractFaceBuilder.``ExtractBodyCollector`

  Returns a collection of bodies to extract

  `-------------------------------------`

  Getter Method

  Signature `ExtractBodyCollector`

  Returns: |
  Return type: | `NXOpen.ScCollector`

  New in version NX9.0.0.

  License requirements: None.

## FaceChain

`ExtractFaceBuilder.``FaceChain`

  Returns the face chain containing the faces to extract

  `-------------------------------------`

  Getter Method

  Signature `FaceChain`

  Returns: |
  Return type: | `NXOpen.ScCollector`

  New in version NX6.0.0.

  License requirements: None.

## FaceOption

`ExtractFaceBuilder.``FaceOption`

  Returns or sets the face option type

  `-------------------------------------`

  Getter Method

  Signature `FaceOption`

  Returns: |
  Return type: | `NXOpen.Features.ExtractFaceBuilderFaceOptionType`

  New in version NX6.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `FaceOption`

  Parameters: | faceOptionType (`NXOpen.Features.ExtractFaceBuilderFaceOptionType`) –

  New in version NX6.0.0.

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

## FaceReverseDirection

`ExtractFaceBuilder.``FaceReverseDirection`

  Returns or sets the option specifying whether to reverse the face normals for the extracted faces.

  `-------------------------------------`

  Getter Method

  Signature `FaceReverseDirection`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `FaceReverseDirection`

  Parameters: | faceNormal (bool) –

  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”)

## FacesToExtract

`ExtractFaceBuilder.``FacesToExtract`

  Returns the faces

  `-------------------------------------`

  Getter Method

  Signature `FacesToExtract`

  Returns: |
  Return type: | `NXOpen.SelectFaceList`

  New in version NX5.0.0.

  Deprecated since version NX7.5.0: Use `NXOpen.Features.ExtractFaceBuilder.ObjectToExtract()` instead.

  License requirements: None.

## FeatureOption

`ExtractFaceBuilder.``FeatureOption`

  Returns or sets the feature option type

  `-------------------------------------`

  Getter Method

  Signature `FeatureOption`

  Returns: |
  Return type: | `NXOpen.Features.ExtractFaceBuilderFeatureOptionType`

  New in version NX9.0.3.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `FeatureOption`

  Parameters: | featureOptionType (`NXOpen.Features.ExtractFaceBuilderFeatureOptionType`) –

  New in version NX9.0.3.

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

## FixAtCurrentTimestamp

`ExtractFaceBuilder.``FixAtCurrentTimestamp`

  Returns or sets the option specifying whether to fix the extract face operation at the current timestamp

  `-------------------------------------`

  Getter Method

  Signature `FixAtCurrentTimestamp`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `FixAtCurrentTimestamp`

  Parameters: | fixAtTimestamp (bool) –

  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”)

## FrecAtTimeStamp

`ExtractFaceBuilder.``FrecAtTimeStamp`

  Returns or sets the option specifying if the results from this builder should be associated

  `-------------------------------------`

  Getter Method

  Signature `FrecAtTimeStamp`

  Returns: |
  Return type: | `NXOpen.Features.Feature`

  New in version NX6.0.1.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `FrecAtTimeStamp`

  Parameters: | terminalFrec (`NXOpen.Features.Feature`) –

  New in version NX6.0.1.

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

## HideOriginal

`ExtractFaceBuilder.``HideOriginal`

  Returns or sets the option to specify if the original faces should be hidden

  `-------------------------------------`

  Getter Method

  Signature `HideOriginal`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `HideOriginal`

  Parameters: | hideOriginal (bool) –

  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”)

## InheritDisplayProperties

`ExtractFaceBuilder.``InheritDisplayProperties`

  Returns or sets the inherit display properties from source option

  `-------------------------------------`

  Getter Method

  Signature `InheritDisplayProperties`

  Returns: |
  Return type: | bool

  New in version NX6.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `InheritDisplayProperties`

  Parameters: | inheritDisplayProperties (bool) –

  New in version NX6.0.0.

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

## IsPsmOutputBody

`ExtractFaceBuilder.``IsPsmOutputBody`

  Returns or sets the PSM Body Output option

  `-------------------------------------`

  Getter Method

  Signature `IsPsmOutputBody`

  Returns: |
  Return type: | bool

  New in version NX11.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `IsPsmOutputBody`

  Parameters: | psmBodyOutput (bool) –

  New in version NX11.0.0.

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

## MakePositionIndependent

`ExtractFaceBuilder.``MakePositionIndependent`

  Returns or sets the option to specify that the extracted faces should be position independent

  `-------------------------------------`

  Getter Method

  Signature `MakePositionIndependent`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `MakePositionIndependent`

  Parameters: | makePositionIndependent (bool) –

  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”)

## ObjectToExtract

`ExtractFaceBuilder.``ObjectToExtract`

  Returns a list of the extracted objects.

  The objects in the list are `NXOpen.Face` objects.

  `-------------------------------------`

  Getter Method

  Signature `ObjectToExtract`

  Returns: |
  Return type: | `NXOpen.SelectDisplayableObjectList`

  New in version NX7.5.0.

  License requirements: None.

## ParentPart

`ExtractFaceBuilder.``ParentPart`

  Returns or sets the source part type

  `-------------------------------------`

  Getter Method

  Signature `ParentPart`

  Returns: |
  Return type: | `NXOpen.Features.ExtractFaceBuilderParentPartType`

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `ParentPart`

  Parameters: | parentPart (`NXOpen.Features.ExtractFaceBuilderParentPartType`) –

  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”)

## ReplacementAssistant

`ExtractFaceBuilder.``ReplacementAssistant`

  Returns the Replacement Assistant builder.

  Call Enter() to enter or re-enter into the mapping environment. Enter() needs to be executed before invoking any map creation or automatic mapping APIs. The maps inferred internally (internal identifier reuse, inherited from parent and siblings) will be populated when Enter() is executed for the first time after selecting a replacement entity. Call Exit() to exit the mapping environment.

  `-------------------------------------`

  Getter Method

  Signature `ReplacementAssistant`

  Returns: |
  Return type: | `NXOpen.GeometricUtilities.ReplAsstBuilder`

  New in version NX6.0.0.

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

## SeedFace

`ExtractFaceBuilder.``SeedFace`

  Returns the seed face for the face chain

  `-------------------------------------`

  Getter Method

  Signature `SeedFace`

  Returns: |
  Return type: | `NXOpen.SelectFace`

  New in version NX5.0.0.

  License requirements: None.

## SeedReverseDirection

`ExtractFaceBuilder.``SeedReverseDirection`

  Returns or sets the option that specifies whether to reverse the face normals of the extracted faces relative to the seed face chain

  `-------------------------------------`

  Getter Method

  Signature `SeedReverseDirection`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `SeedReverseDirection`

  Parameters: | seedNormal (bool) –

  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”)

## SourcePartOccurrence

`ExtractFaceBuilder.``SourcePartOccurrence`

  Returns or sets the source part occurrence

  `-------------------------------------`

  Getter Method

  Signature `SourcePartOccurrence`

  Returns: |
  Return type: | `NXOpen.TaggedObject`

  New in version NX9.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `SourcePartOccurrence`

  Parameters: | sourcePartOcc (`NXOpen.TaggedObject`) –

  New in version NX9.0.0.

  License requirements: None.

## SurfaceType

`ExtractFaceBuilder.``SurfaceType`

  Returns or sets the surface type

  `-------------------------------------`

  Getter Method

  Signature `SurfaceType`

  Returns: |
  Return type: | `NXOpen.Features.ExtractFaceBuilderFaceSurfaceType`

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `SurfaceType`

  Parameters: | surfaceType (`NXOpen.Features.ExtractFaceBuilderFaceSurfaceType`) –

  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”)

## TraverseInteriorEdges

`ExtractFaceBuilder.``TraverseInteriorEdges`

  Returns or sets the traverse interior edges

  `-------------------------------------`

  Getter Method

  Signature `TraverseInteriorEdges`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `TraverseInteriorEdges`

  Parameters: | traverseInteriorEdges (bool) –

  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”)

## Type

`ExtractFaceBuilder.``Type`

  Returns or sets the type

  `-------------------------------------`

  Getter Method

  Signature `Type`

  Returns: |
  Return type: | `NXOpen.Features.ExtractFaceBuilderExtractType`

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `Type`

  Parameters: | type (`NXOpen.Features.ExtractFaceBuilderExtractType`) –

  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”)

## UseTangentEdgeAngles

`ExtractFaceBuilder.``UseTangentEdgeAngles`

  Returns or sets the use tangent angles

  `-------------------------------------`

  Getter Method

  Signature `UseTangentEdgeAngles`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

  `-------------------------------------`

  Setter Method

  Signature `UseTangentEdgeAngles`

  Parameters: | useTangentAngles (bool) –

  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”)

# Method Detail

## CommitCreateOnTheFly

`ExtractFaceBuilder.``CommitCreateOnTheFly`

  Commits the feature and set create on the fly flag

  Signature `CommitCreateOnTheFly()`

  Returns: |
  Return type: | `NXOpen.Features.Feature`

  New in version NX6.0.0.

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

## FlipFaceChainDirectionSense

`ExtractFaceBuilder.``FlipFaceChainDirectionSense`

  Flip the face chain direction sense

  Signature `FlipFaceChainDirectionSense(face)`

  Parameters: | face (`NXOpen.Face`) –

  New in version NX6.0.0.

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

## GetFaceChainDirectionSense

`ExtractFaceBuilder.``GetFaceChainDirectionSense`

  Returns the face chain direction sense for a given face in the face chain

  Signature `GetFaceChainDirectionSense(face)`

  Parameters: | face (`NXOpen.Face`) –
  Returns: |
  Return type: | bool

  New in version NX6.0.0.

  License requirements: None.

## GetProductInterfaceObjects

`ExtractFaceBuilder.``GetProductInterfaceObjects`

  Gets selected product interface objects

  Signature `GetProductInterfaceObjects()`

  Returns: | items in list
  Return type: | list of `NXOpen.Assemblies.ProductInterface.InterfaceObject`

  New in version NX9.0.0.

  License requirements: None.

## GetSourcePartOccurrences

`ExtractFaceBuilder.``GetSourcePartOccurrences`

  Gets source part occurrences

  Signature `GetSourcePartOccurrences()`

  Returns: |
  Return type: | list of `NXOpen.TaggedObject`

  New in version NX10.0.0.

  License requirements: None.

## GetWaveLinkInformation

`ExtractFaceBuilder.``GetWaveLinkInformation`

  Prints wave browser type information about link

  Signature `GetWaveLinkInformation()`

  Returns: | a tuple
  Return type: | A tuple consisting of (info, xformExists, xformOrigin, xformOrientation, xformScale). info is a str. queried wave information xformExists is a bool. true if there is a transform xformOrigin is a `NXOpen.Point3d`. transformation origin xformOrientation is a `NXOpen.Matrix3x3`. transformation matrix xformScale is a float. transformation scale

  New in version NX6.0.0.

  License requirements: wave (“WAVE FUNCTIONALITY”)

## RecreateVectorOfHelpDirVector

`ExtractFaceBuilder.``RecreateVectorOfHelpDirVector`

  Causes the recreation of vector for help dir

  Signature `RecreateVectorOfHelpDirVector()`

  New in version NX7.5.4.

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

## SetProductInterfaceObjects

`ExtractFaceBuilder.``SetProductInterfaceObjects`

  Sets selected product interface objects

  Signature `SetProductInterfaceObjects(selectedObjects)`

  Parameters: | selectedObjects (list of `NXOpen.Assemblies.ProductInterface.InterfaceObject`) – items in list

  New in version NX9.0.0.

  License requirements: None.

## SetSourcePartOccurrences

`ExtractFaceBuilder.``SetSourcePartOccurrences`

  Sets source part occurrences

  Signature `SetSourcePartOccurrences(sourcePartOccurrences)`

  Parameters: | sourcePartOccurrences (list of `NXOpen.TaggedObject`) –

  New in version NX10.0.0.

  License requirements: None.

## Validate

`ExtractFaceBuilder.``Validate`

  Validate whether the inputs to the component are sufficient for commit to be called.

  If the component is not in a state to commit then an exception is thrown. For example, if the component requires you to set some property, this method will throw an exception if you haven’t set it. This method throws a not-yet-implemented NXException for some components.

  Signature `Validate()`

  Returns: | Was self validation successful
  Return type: | bool

  New in version NX3.0.1.

  License requirements: None.