Property StructureSystemToPatternArray As System.Object

Dim instance As ILinearPatternFeatureData
Dim value As System.Object
 
instance.StructureSystemToPatternArray = value
 
value = instance.StructureSystemToPatternArray

System.object StructureSystemToPatternArray {get; set;}

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

Property Value

'VBA
'This example demonstrates how to create a linear pattern using a structure system.
'==========================================================================================
'Preconditions:
'1. Ensure the specified part template exists.
'2. Open an Immediate window.
'3. Press F5.
'
'Postconditions:
' 1. Creates Sketch1 containing two sketch segments.
' 2. Configures the start/end extensions and the member profile.
' 3. Selects the two sketch segments.
' 4. Creates primary Structure System1 with two primary path segment members (Member1 and Member2).
' 5. Creates a Boss-Extrude1 to pattern.
' 6. Inspect the graphics area.
' 7. Press F5 to create LPattern1.
' 8. Press F5 to finish.
' 9. Inspect the Immediate window.
'========================================================================
Dim swApp As SldWorks.SldWorks
Dim modDoc As SldWorks.ModelDoc2
Dim swFeatMgr As SldWorks.FeatureManager
Dim swSelMgr As SldWorks.SelectionMgr
Dim modDocExt As SldWorks.ModelDocExtension
Dim structMemDef As SldWorks.StructureSystemMemberFeatureData
Dim profDef As SldWorks.StructureSystemMemberProfile
Dim PrimDef As SldWorks.PrimaryStructuralMemberFeatureData
Dim memPathSegDef As PrimaryMemberPathSegmentFeatureData
Dim memBetweenPointsSecDef As SldWorks.SecondaryMemberBetweenPointsFeatureData
Dim secMemDatTochange As SldWorks.SecondaryMemberBetweenPointsFeatureData
Dim memSupportPlaneSecDef As SldWorks.SecondaryMemberSupportPlaneFeatureData
Dim segments(2) As Object
Dim stat As Boolean
Dim memData(0) As SldWorks.StructureSystemMemberFeatureData
Dim memDataArray As Variant
Dim structSys As SldWorks.Feature
Dim baseSecondarySystem As SldWorks.StructureSystemFolder
Dim structSysDef As SldWorks.StructureSystemFolder
Dim structSysSecDef As SldWorks.StructureSystemFolder
Dim feat As SldWorks.Feature
Dim structSysModDef As SldWorks.StructureSystemFolder
Dim outProfiles As Variant
Dim MemberData As SldWorks.StructureSystemMemberFeatureData
Dim memberArray As Variant
Dim profileGrpFeat As SldWorks.Feature
Dim profileGrp As SldWorks.ProfileGroupFolder
Dim memTochange As SldWorks.StructureSystemMemberFeatureData
Dim I As Long
Dim j As Long
Dim secDef As SldWorks.SecondaryStructuralMemberFeatureData
Dim UpToMemDef As SldWorks.SecondaryMemberUpToMembersFeatureData
Dim point As Object
Dim Members(0) As Object

Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchMgr As SldWorks.SketchManager
Dim swFeatureMgr As SldWorks.FeatureManager
Dim swSelectionMgr As SldWorks.SelectionMgr
Dim swSketchSegment As SldWorks.SketchSegment
Dim swFeature As SldWorks.Feature
Dim swLinearPatternFeatureData As SldWorks.LinearPatternFeatureData
Dim sketchSegments As Variant
Dim status As Boolean
Dim obj As Object
Dim patternFeatures(1) As Object

Option Explicit

Sub main()
    Set swApp = Application.SldWorks
  
    Dim swSheetWidth As Double
    swSheetWidth = 0
    Dim swSheetHeight As Double
    swSheetHeight = 0
    Set modDoc = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2023\templates\Part.PRTDOT", 0, swSheetWidth, swSheetHeight)
  
    Set modDocExt = modDoc.Extension
  
    modDoc.SketchManager.InsertSketch True
    stat = modDocExt.SelectByID2("Front Plane", "PLANE", -0.077188654347454, 0.054268560279924, 3.86214196026222E-03, False, 0, Nothing, 0)
    modDoc.ClearSelection2 True
  
    Dim skSegment As Object
    Set skSegment = modDoc.SketchManager.CreateLine(-0.168061, 0.084736, 0#, -0.168061, -0.077684, 0#)
    Set skSegment = modDoc.SketchManager.CreateLine(0.075216, 0.107771, 0#, 0.075216, -0.006699, 0#)
    modDoc.ClearSelection2 True
  
    stat = modDocExt.SelectByID2("Top Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    Dim myRefPlane As SldWorks.RefPlane
    Set myRefPlane = modDoc.FeatureManager.InsertRefPlane(8, 0.03, 0, 0, 0, 0)
    modDoc.ClearSelection2 True
    stat = modDocExt.SelectByID2("Top Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    modDoc.ClearSelection2 True
    modDoc.SketchManager.InsertSketch True
  
    stat = modDocExt.SelectByID2("Line1@Sketch1", "EXTSKETCHSEGMENT", -0.168061313304597, 5.44142573846353E-02, 0, False, 0, Nothing, 0)
    stat = modDocExt.SelectByID2("Line2@Sketch1", "EXTSKETCHSEGMENT", 7.52162521083513E-02, 5.32390034454423E-02, 0, True, 0, Nothing, 0)
  
    'Create primary structure system path segment members
    Set structMemDef = modDocExt.CreateStructureSystemMemberData(0)
    Debug.Print "Type of structure system member as defined by swStructureSystemMemberType_e: " & structMemDef.StructureSystemMemberType
                  
    structMemDef.StartEndExtendD1 = 1#
    structMemDef.StartEndExtendD2 = 2#
  
    Set profDef = structMemDef.MemberProfile
  
    profDef.ProfileStandard = "ansi inch"
    profDef.ProfileType = "c channel"
    profDef.ProfileSize = "3 x 5"
  
    Set PrimDef = structMemDef
    Debug.Print "Structure system primary member creation type as defined by swStructureSystemMemberCreationType_e: " & PrimDef.PrimaryMemberType
  
    Set memPathSegDef = PrimDef
    memPathSegDef.MergeTangentMembers = True
  
    Set swSelMgr = modDoc.SelectionManager
  
    Dim segments(1) As Object
    Set segments(0) = swSelMgr.GetSelectedObject6(1, 0)
    Set segments(1) = swSelMgr.GetSelectedObject6(2, 0)
    stat = memPathSegDef.SetPathSegments(segments)
    Debug.Print "Path segments successfully set: " & stat
    
    Dim PrimMemData(0) As SldWorks.StructureSystemMemberFeatureData
    Set PrimMemData(0) = structMemDef
    
    Dim PrimMemDatArray As Variant
    PrimMemDatArray = PrimMemData
  
    Dim structSysFeat As SldWorks.Feature
    Set structSysFeat = modDocExt.CreateStructureSystem(PrimMemDatArray, Nothing)
   
    'Create the axis for the circular pattern
    'status = modDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    'modDoc.SketchManager.InsertSketch True
    'modDoc.ClearSelection2 True
    'Dim skSegmentAxis As Object
    'Set skSegmentAxis = modDoc.SketchManager.CreateLine(0.695357, 0.586267, 0#, 0.695357, -0.704287, 0#)
    'modDoc.ClearSelection2 True
    'modDoc.SketchManager.InsertSketch True
   
    'Create a solid body to also pattern
    status = modDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    modDoc.SketchManager.InsertSketch True
    modDoc.ClearSelection2 True
    status = modDocExt.SketchBoxSelect("0.509957", "-0.990370", "0.000000", "1.024907", "-1.314598", "0.000000")
    status = modDocExt.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
    status = modDocExt.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
    Dim vSkLines As Variant
    vSkLines = modDoc.SketchManager.CreateCornerRectangle(0.713394086918119, -0.907724114572968, 0, 1.44449597678115, -1.33367043301491, 0)
    modDoc.ClearSelection2 True
    modDoc.SketchManager.InsertSketch True
    modDoc.SketchManager.InsertSketch True
    Dim myFeature As SldWorks.Feature
    Set myFeature = modDoc.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.07, 0.01, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, False, True, True, 0, 0, False)
    modDoc.SelectionManager.EnableContourSelection = False

    modDoc.ViewZoomtofit
   
    Stop
   
    Set swModel = swApp.ActiveDoc
    Set swModelDocExt = swModel.Extension
    Set swSketchMgr = swModel.SketchManager
    Set swFeatureMgr = swModel.FeatureManager
    Set swSelectionMgr = swModel.SelectionManager
   
    'Create linear pattern
    Set swLinearPatternFeatureData = swFeatureMgr.CreateDefinition(swFmLPattern)
    swLinearPatternFeatureData.D1EndCondition = 0
    swLinearPatternFeatureData.D1ReverseDirection = True
    swLinearPatternFeatureData.D1Spacing = 0.5
    swLinearPatternFeatureData.D1TotalInstances = 3
    swLinearPatternFeatureData.BodyPattern = True
    swLinearPatternFeatureData.GeometryPattern = False
    swLinearPatternFeatureData.VarySketch = False
   
    'Preselect direction, bodies, structure system folders
    swModel.ClearSelection2 True
    status = swModelDocExt.SelectByRay(1.15634621903263, -1.3336704330149, 6.99999999999932E-02, 0, 0, -1, 2.16151863089938E-02, 1, False, 1, 0)
    status = swModelDocExt.SelectByID2("Boss-Extrude1", "SOLIDBODY", 0, 0, 0, True, 256, Nothing, 0)
    status = swModelDocExt.SelectByID2("Structure System1", "BODYFEATURE", 0, 0, 0, True, 134217728, Nothing, 0)
   
    Set swFeature = swFeatureMgr.CreateFeature(swLinearPatternFeatureData)
       
    Stop  'Examine the graphics area
   
    swModel.ClearSelection2 True
    status = swModelDocExt.SelectByID2("LPattern1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
    Set swFeature = swSelectionMgr.GetSelectedObject6(1, -1)
    Set swLinearPatternFeatureData = swFeature.GetDefinition
    swLinearPatternFeatureData.AccessSelections swModel, Nothing
    Debug.Print "Is LPattern1 a features/faces pattern or a bodies pattern (true if a bodies pattern)? " & swLinearPatternFeatureData.BodyPattern
   
    Dim var As Variant
    var = swLinearPatternFeatureData.StructureSystemToPatternArray
   
    Dim strctSysFolder As StructureSystemFolder
    Dim index As Integer
    For index = LBound(var) To UBound(var)
        Set strctSysFolder = var(index)
        Set patternFeatures(0) = strctSysFolder
        Debug.Print "Number of structure system folders: " & strctSysFolder.GetProfileGroupFoldersCount
    Next
   
    'Uncomment the following lines of code to modify the linear pattern
    'to use another structure system (e.g., Structure System2)
    'Stop
   
    'Dim feat As Feature
    'swModel.ClearSelection2 True
    'status = swModelDocExt.SelectByID2("Structure System2", "BODYFEATURE", 0, 0, 0, True, 0, Nothing, 0)
    'Set feat = swSelectionMgr.GetSelectedObject6(1, 0)
    'Set patternFeatures(1) = feat.GetSpecificFeature2()
   
    ''During linear pattern modification, use StructureSystemPatternArray property to change structure system to pattern
    'swLinearPatternFeatureData.StructureSystemToPatternArray = patternFeatures
   
    Debug.Print swFeature.ModifyDefinition(swLinearPatternFeatureData, swModel, Nothing)
   
    End Sub

This property is valid only if ILinearPatternFeatureData::BodyPattern is true.

Use the setter of this property to change structure systems only after the linear pattern feature has been created.

Before using this property in .NET code, read IDispatch Object Arrays as Input in .NET. To remove a structure system from the pattern, set this property to a DispatchWrapper array containing one null element.

For more information, see the SOLIDWORKS user-interface help > Weldments and Structure System > Pattern and Mirror Support topic.