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Insert Lofted Bend Feature Example (VBA)

This example shows how to insert a lofted bend feature in a sheet metal part and get the lofted bend feature data.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified part template exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens a new part.
' 2. Creates a sketch on Front Plane, a reference plane parallel to 
'    Front Plane, and a sketch on that reference plane.
' 3. Selects the sketches and inserts a lofted bend.
' 4. Inspect the Immediate window, FeatureManager design, and graphics area.
'---------------------------------------------------------------------------
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim refPlane As SldWorks.refPlane
Dim skSegment As SldWorks.SketchSegment
Dim feat As SldWorks.Feature
Dim lbfd As SldWorks.LoftedBendsFeatureData
Dim boolstatus As Boolean
Option Explicit

Sub main()
    Set swApp = Application.SldWorks    
    ' Open new part and create a sketch, a reference plane, and another sketch
    ' on that reference plane
    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2016\templates\Part.prtdot", 0, 0, 0)
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    Set skSegment = Part.SketchManager.CreateLine(0#, 0#, 0#, 0.024074, 0.024074, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.024074, 0.024074, 0#, 0.076952, 0.024074, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.076952, 0.024074, 0#, 0.101026, 0#, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    Set refPlane = Part.FeatureManager.InsertRefPlane(8, 0.05, 0, 0, 0, 0)
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
    Set skSegment = Part.SketchManager.CreateLine(-0.031383, 0#, 0#, 0.047146, 0.060616, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.047146, 0.060616, 0#, 0.058036, 0.060616, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.058036, 0.060616, 0#, 0.129686, 0.002436, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    ' Select the sketches for the lofted bend feature
    boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 1, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, True, 1, Nothing, 0)
    ' Insert a lofted bend feature with two bends
    Set feat = Part.FeatureManager.InsertSheetMetalLoftedBend2(0, 0.0007366, False, 0.0007366, True, swBendsPerTransitionSegment, 0, 2, 0, 0)
    ' Get lofted bend feature data
    Set lbfd = feat.GetDefinition
    Debug.Print "Number of sketch profiles in this feature: " & lbfd.GetProfileCount
    Debug.Print "Thickness: " & lbfd.Thickness
    Debug.Print "Reverse thickness direction? " & lbfd.Direction
    Debug.Print "Faceting option as defined in swLoftedBendFacetOptions_e: " & lbfd.FacetingOption
    Debug.Print "Faceting option value: " & lbfd.FacetValue
    Debug.Print "Formed? " & lbfd.FormedMethod
    Debug.Print "Calculate facet transitions using vertexes? " & lbfd.ReferToEndPoint
End Sub


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