Property D1FaceNormal As System.Object

Dim instance As ICurveDrivenPatternFeatureData
Dim value As System.Object
 
instance.D1FaceNormal = value
 
value = instance.D1FaceNormal

System.object D1FaceNormal {get; set;}

property System.Object^ D1FaceNormal {
   System.Object^ get();
   void set ( &   System.Object^ value);
}

Property Value

' VBA
'
' This example shows how to pre-select the face normal entity for creating a curve-driven pattern
' that uses a helical curve for Direction 1.
'
' Preconditions: Ensure that the specified part template exists.
'
' Postconditions: Inspect the graphics area and the FeatureManager design tree
'==========================================================

Dim swApp As SldWorks.SldWorks
Dim swFeat As SldWorks.Feature
Dim swFeatMgr As SldWorks.FeatureManager
Dim swFeatData As SldWorks.CurveDrivenPatternFeatureData
Dim swPart As SldWorks.PartDoc
Dim Part As SldWorks.ModelDoc2
Dim skSegment As SldWorks.SketchSegment
Dim myFeature As SldWorks.Feature
Dim vSkLines As Variant
Dim swSheetWidth As Double
Dim swSheetHeight As Double
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Option Explicit

Sub main()

    Set swApp = Application.SldWorks
   
    'Create new part that includes 3 features: Boss-Extrude1, Boss-Extrude2, and Helix/Spiral1
    swSheetWidth = 0
    swSheetHeight = 0
    Set Part = swApp.NewDocument("C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2021\templates\Part.PRTDOT", 0, swSheetWidth, swSheetHeight)
    Set swPart = Part
    swApp.ActivateDoc2 "Part1", False, longstatus
    Set Part = swApp.ActiveDoc
  
    Part.SketchManager.InsertSketch True
    Set skSegment = Part.SketchManager.CreateCircle(0#, 0#, 0#, 0.31751, 0#, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
   
    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 1.029208, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
    Part.SelectionManager.EnableContourSelection = False
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByRay(-8.19439014833279E-03, -2.48002522846491E-03, 8.63600000000702E-02, -0.400036026779312, -0.515038074910024, -0.758094294050284, 8.9519512195122E-04, 2, False, 0, 0)
    Part.ClearSelection2 True
   
    vSkLines = Part.SketchManager.CreatePolygon(-0.19, -0.01, 0, -0.19, 0.05, 0, 6, True)
    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, True, 0, 0, 0.24638, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
    Part.ClearSelection2 True
   
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Set skSegment = Part.SketchManager.CreateCircle(0#, 0#, 0#, 0.3175, 0, 0)
    Part.InsertHelix False, True, False, False, swHelixDefinedBy_e.swHelixDefinedByPitchAndRevolution, 1.016, 1.0167, 1, 0, 3.926
   
    'Pre-select Helix/Spiral1 for Direction 1 entity
    boolstatus = Part.Extension.SelectByID2("Helix/Spiral1", "REFERENCECURVES", 0, 0, 0, False, 1, Nothing, 0)
    'Pre-select Boss-Extrude2 as feature to pattern
    boolstatus = Part.Extension.SelectByID2("Boss-Extrude2", "BODYFEATURE", 0, 0, 0, True, 4, Nothing, 0)
    'Pre-select face on Boss-Extrude1 as face normal entity
    boolstatus = Part.Extension.SelectByRay(0.298048689727977, -0.109451261534383, 0.233585198055067, -0.903801459854838, 2.28031013589574E-02, 0.427344053114907, 7.98164962810585E-03, 2, True, 1024, 0)
  
    Set swFeatMgr = Part.FeatureManager
   
    'Create curve driven pattern feature data object
    Set swFeatData = swFeatMgr.CreateDefinition(swFeatureNameID_e.swFmCurvePattern)
   
    swFeatData.D1AlignmentMethod = 0
    swFeatData.D1CurveMethod = 0
    swFeatData.D1InstanceCount = 8
    swFeatData.D1IsEqualSpaced = True
    swFeatData.D1ReverseDirection = False
    swFeatData.D1Spacing = 0.00254
    swFeatData.D2InstanceCount = 1
    swFeatData.D2IsEqualSpaced = False
    swFeatData.D2PatternSeedOnly = False
    swFeatData.D2ReverseDirection = False
    swFeatData.D2Spacing = 0.00254
    swFeatData.Dir2Specified = False
   
    'Create CrvPattern1 feature
    Set swFeat = swFeatMgr.CreateFeature(swFeatData)
   
    Part.ViewZoomtofit2
   
End Sub

This property is valid only when:

• editing the curve-driven pattern feature
• ICurveDrivePatternFeatureData::D1AlignmentMethod is set to swCurveDrivenPatternAlignment_e.swCurvePatternTangentToCurve
• specifying Direction 1 using a 3D curve

To create a curve-driven pattern feature that uses a 3D curve for Direction 1, you must pre-select the face normal with selection Mark = 1024 before creating the curve-driven pattern feature data object.

If you try to edit this property to null or Nothing, IFeature::ModifyDefinition returns true but the property does not change.

For more information, see the Curve Driven Patterns and the Curve Driven Pattern PropertyManager topic in the SOLIDWORKS user-interface help.