Merge Miter Trimmed Bodies Example (VB.NET)

This example shows how to specify to merge miter trimmed bodies in a structural-member group.

'---------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified weldment profile exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Creates a new document containing a weldment and a structural member.
' 2. Sets to merge miter trimmed bodies in the structural-member group.
' 3. Examine the Immediate window.
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
    Public Sub main()
 
        Dim swModel As ModelDoc2
        Dim swFeatMgr As FeatureManager
        Dim swSelMgr As SelectionMgr
        Dim swWeldFeat As Feature
        Dim swWeldFeatData As StructuralMemberFeatureData
        Dim swFeature As Feature
        Dim swSketchSegment As SketchSegment
        Dim status As Boolean
        Dim template As String
        Dim skLines As Object
        Dim group1 As StructuralMemberGroup
        Dim segments1(1) As SketchSegment
        Dim groups1(0) As DispatchWrapper
        Dim groupArray1(0) As Object
        Dim group As StructuralMemberGroup
        Dim groups As Object
        Dim segments As Object
        Dim i As Integer
        Dim j As Integer
 
        template = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)
        swModel = swApp.NewDocument(template, 0, 0, 0)
        swFeatMgr = swModel.FeatureManager
        swSelMgr = swModel.SelectionManager
        swModel.ClearSelection2(True)
 
        ' Create weldment and structural member 
        skLines = swModel.SketchManager.CreateCornerRectangle(-0.1872393706766, 0.1133237194389, 0, -0.07003610048208, 0.009188409684237, 0)
        swModel.ClearSelection2(True)
        swModel.SketchManager.InsertSketch(True)
        swModel.ViewZoomtofit2()
        swFeature = swFeatMgr.InsertWeldmentFeature()
        group1 = swFeatMgr.CreateStructuralMemberGroup
        status = swModel.Extension.SelectByID2("Line1@Sketch1", "EXTSKETCHSEGMENT", -0.1495427140733, 0.1133237194389, 0, False, 0, Nothing, 0)
        status = swModel.Extension.SelectByID2("Line2@Sketch1", "EXTSKETCHSEGMENT", -0.1872393706766, 0.08238014634844, 0, True, 0, Nothing, 0)
        segments1(0) = swSelMgr.GetSelectedObject6(1, 0)
        segments1(1) = swSelMgr.GetSelectedObject6(2, 0)
        group1.Segments = segments1
        group1.Angle = 0
        group1.ApplyCornerTreatment = True
        group1.CornerTreatmentType = swSolidworksWeldmentEndCondOptions_e.swEndConditionMiter
        group1.MirrorProfile = True
        group1.MirrorProfileAxis = swMirrorProfileOrAlignmentAxis_e.swMirrorProfileOrAlignmentAxis_Vertical
        group1.GapWithinGroup = 0
        groupArray1(0) = group1
        groups1(0) = New DispatchWrapper(groupArray1(0))
        swFeature = swFeatMgr.InsertStructuralWeldment5("C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\weldment profiles\ansi inch\c channel\3 x 5.sldlfp", swConnectedSegmentsOption_e.swConnectedSegments_SimpleCut, False, groups1, "")
        swModel.ClearSelection2(True)
 
        ' Get and set structural-member group information
        status = swModel.Extension.SelectByID2("c channel 3 x 5(1)", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        swWeldFeat = swSelMgr.GetSelectedObject6(1, 0)
        swWeldFeatData = swWeldFeat.GetDefinition
        swWeldFeatData.AccessSelections(swModel, Nothing)
        Debug.Print("")
        Debug.Print("Number of groups: " & swWeldFeatData.GetGroupsCount)
        Debug.Print(" Feature name: " & swWeldFeat.Name)
        groups = swWeldFeatData.Groups
        For i = LBound(groups) To UBound(groups)
            group = groups(i)
            Debug.Print(" Number of segments in group " & i + 1 & ": " & group.GetSegmentsCount)
            Debug.Print(" Apply corner treatment? " & group.ApplyCornerTreatment)
            Debug.Print(" Corner treatment type (1 = swSolidworksWeldmentEndCondOptions_e.swEndconditionMiter): " & group.CornerTreatmentType)
            Debug.Print(" Original merge miter trimmed bodies setting: " & group.MiterMergeCondition)
            If group.CornerTreatmentType = swSolidworksWeldmentEndCondOptions_e.swEndConditionMiter Then
                group.MiterMergeCondition = True
            End If
            Debug.Print(" Modified merge miter trimmed bodies setting: " & group.MiterMergeCondition)
            segments = group.Segments
            For j = LBound(segments) To UBound(segments)
                swSketchSegment = segments(j)
                swSketchSegment.Select4(False, Nothing)
            Next j
        Next i
        swFeature.ModifyDefinition(swWeldFeatData, swModel, Nothing)
 
        swModel.ClearSelection2(True)
 
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class