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Insert Structural Weldment Example (VB.NET)

This example shows how to create structural weldment features using structural member groups.

' ---------------------------------------------------------------------------
' Preconditions:
' 1. Verify existence of the weldment profile pathname
'    as specified in both InsertStructuralWeldment4 method calls in this macro.
' 2. Open an Immediate Window.
'
' Postconditions:
' 1. Weldment, Structural Member1, and Structural Member2

'    are in the FeatureManager design tree.
' 2. Structural Member1 group is rotated 45 degrees.
' 3. Inspect the Immediate Window for more information.
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Imports System.Diagnostics

Partial Class SolidWorksMacro

    
Dim Part As ModelDoc2
    
Dim boolstatus As Boolean
    Dim FeatMgr As FeatureManager
    
Dim SelMgr As SelectionMgr
    
Dim swWeldFeat As Feature
    
Dim swWeldFeatData As StructuralMemberFeatureData

    
Public Sub Main()

        
Dim MacroFolder As String
        MacroFolder = swApp.GetCurrentMacroPathFolder()
        swApp.SetCurrentWorkingDirectory(MacroFolder)

        
Dim Template As String
        Template = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)
        Part = swApp.NewDocument(Template, 0, 0, 0)

        FeatMgr = Part.FeatureManager
        SelMgr = Part.SelectionManager

        Part.ClearSelection2(
True)

        
Dim vSkLines As Object
        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.1872393706766, 0.1133237194389, 0, -0.07003610048208, 0.009188409684237, 0)

        Part.ClearSelection2(
True)

        vSkLines = Part.SketchManager.CreateCornerRectangle(0.06513561531715, 0.03369083550887, 0, 0.1807053904567, -0.08106219210316, 0)
        Part.SketchManager.InsertSketch(
True)

        Part.ViewZoomtofit2()

        
Dim myFeature As Object
        myFeature = Part.FeatureManager.InsertWeldmentFeature()

        
Dim Group1 As StructuralMemberGroup
        Group1 = FeatMgr.CreateStructuralMemberGroup
        
Dim segments1(1) As SketchSegment
        
Dim GroupArray1(0) As StructuralMemberGroup

        boolstatus = Part.Extension.SelectByID2(
"Line1@Sketch1", "EXTSKETCHSEGMENT", -0.1495427140733, 0.1133237194389, 0, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2(
"Line2@Sketch1", "EXTSKETCHSEGMENT", -0.1872393706766, 0.08238014634844, 0, True, 0, Nothing, 0)

        segments1(0) = SelMgr.GetSelectedObject6(1, 0)
        segments1(1) = SelMgr.GetSelectedObject6(2, 0)

        Group1.Segments = segments1
        Group1.Angle = 0.785714285714286
'radians
        Group1.ApplyCornerTreatment = True
        Group1.CornerTreatmentType = swSolidworksWeldmentEndCondOptions_e.swEndConditionMiter
        Group1.MirrorProfile =
True
        Group1.MirrorProfileAxis = swMirrorProfileOrAlignmentAxis_e.swMirrorProfileOrAlignmentAxis_Vertical
        Group1.GapWithinGroup = 0.0127
'meters

        GroupArray1(0) = Group1

        myFeature = Part.FeatureManager.InsertStructuralWeldment4(
"C:\Program Files\SolidWorks Corp\SolidWorks\data\weldment profiles\ansi inch\c channel\3 x 5.sldlfp", 1, False, GroupArray1)

        Part.ClearSelection2(
True)

        
Dim Group2 As StructuralMemberGroup
        Group2 = FeatMgr.CreateStructuralMemberGroup
        
Dim segments2(1) As SketchSegment
        
Dim GroupArray2(0) As StructuralMemberGroup

        boolstatus = Part.Extension.SelectByID2(
"Line5@Sketch1", "EXTSKETCHSEGMENT", 0.1185825251083, 0.03369083550887, 0, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2(
"Line6@Sketch1", "EXTSKETCHSEGMENT", 0.06513561531715, -0.02774616865332, 0, True, 0, Nothing, 0)

        segments2(0) = SelMgr.GetSelectedObject6(1, 0)
        segments2(1) = SelMgr.GetSelectedObject6(2, 0)

        Group2.Segments = segments2
        Group2.AlignAxis = swMirrorProfileOrAlignmentAxis_e.swMirrorProfileOrAlignmentAxis_Vertical

        GroupArray2(0) = Group2

        myFeature = Part.FeatureManager.InsertStructuralWeldment4(
"C:\Program Files\SolidWorks Corp\SolidWorks\data\weldment profiles\ansi inch\c channel\3 x 5.sldlfp", 1, False, GroupArray2)

        Part.ClearSelection2(
True)

        
' Get Group Information

        Dim Group As StructuralMemberGroup
        
Dim vGroups As Object
        Dim vSegments As Object

        boolstatus = Part.Extension.SelectByID2("Structural Member1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swWeldFeat = SelMgr.GetSelectedObject6(1, 0)

        swWeldFeatData = swWeldFeat.GetDefinition
        swWeldFeatData.AccessSelections(Part,
Nothing)

        Debug.Print(
"")
        Debug.Print(
"Groups Count : " & swWeldFeatData.GetGroupsCount)
        Debug.Print(
" Feature Name : " & swWeldFeat.Name)

        vGroups = swWeldFeatData.Groups

        
Dim i As Long, j As Long
        For i = LBound(vGroups) To UBound(vGroups)
            Group = vGroups(i)
            Debug.Print(
" Segment Count in Group " & i + 1 & "  : " & Group.GetSegmentsCount)
            Debug.Print(
" Rotational angle of group: " & Group.Angle)
            Debug.Print(
" ApplyCornerTreatment: " & Group.ApplyCornerTreatment)
            Debug.Print(
" CornerTreatmentType: " & Group.CornerTreatmentType)
            Debug.Print(
" MirrorProfile: " & Group.MirrorProfile)
            Debug.Print(
" MirrorProfileAxis: " & Group.MirrorProfileAxis)
            Debug.Print(
" GapWithinGroup: " & Group.GapWithinGroup)
            vSegments = Group.Segments
            
For j = LBound(vSegments) To UBound(vSegments)
                vSegments(j).Select(
False)
            
Next j
        
Next i

        swWeldFeatData.ReleaseSelectionAccess()

        boolstatus = Part.Extension.SelectByID2(
"Structural Member2", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swWeldFeat = SelMgr.GetSelectedObject6(1, 0)
        swWeldFeatData = swWeldFeat.GetDefinition
        swWeldFeatData.AccessSelections(Part,
Nothing)

        Debug.Print(
"")
        Debug.Print(
"Groups Count : " & swWeldFeatData.GetGroupsCount)
        Debug.Print(
" Feature Name : " & swWeldFeat.Name)

        vGroups = swWeldFeatData.Groups
        
For i = LBound(vGroups) To UBound(vGroups)
            Group = vGroups(i)
            Debug.Print(
" Segment Count in Group " & i + 1 & "  : " & Group.GetSegmentsCount)
            Debug.Print(
" Rotational angle of group: " & Group.Angle)
            Debug.Print(
" ApplyCornerTreatment: " & Group.ApplyCornerTreatment)
            Debug.Print(
" CornerTreatmentType: " & Group.CornerTreatmentType)
            Debug.Print(
" MirrorProfile: " & Group.MirrorProfile)
            Debug.Print(
" MirrorProfileAxis: " & Group.MirrorProfileAxis)
            Debug.Print(
" GapWithinGroup: " & Group.GapWithinGroup)
            vSegments = Group.Segments
            
For j = LBound(vSegments) To UBound(vSegments)
                vSegments(j).Select(
False)
            
Next j
        
Next i

        swWeldFeatData.ReleaseSelectionAccess()
        Part.ClearSelection2(
True)

    
End Sub

  
    
Public swApp As SldWorks


End Class

 



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