Insert Sheet Metal Base Flange Example (VB.NET)

This example shows how to insert a sheet metal base flange.

'----------------------------------------------------------------------------

' Preconditions:

' 1. Open SolidWorks.

' 2. Verify and, if necessary, modify the location of the part template in the code below:

' C:\Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks 2010\templates\Part.prtdot

' 3. Run (F5) this macro.

' Postconditions:

' Observe the following in the model view and the FeatureManager design tree:

'  * Sheet metal base flange, Base-Flange1, connects the two sheet metal parts.

'----------------------------------------------------------------------------

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System

Partial Class SolidWorksMacro

   

    Dim Part As ModelDoc2

    Dim boolstatus As Boolean

    Dim longstatus As Long, longwarnings As Long

    Sub main()

        boolstatus = swApp.ResetUntitledCount(0, 0, 0)

        Part = swApp.NewDocument("C:\Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks 2010\templates\Part.prtdot", 0, 0, 0)

        swApp.ActivateDoc2("Part1", False, longstatus)

        Part = swApp.ActiveDoc

        Part.SketchManager.InsertSketch(True)

        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.07320616684915, 0.04378582530511, 0.008882453015985, False, 0, Nothing, 0)

        Part.ClearSelection2(True)

        Dim vSkLines As Object

        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.09520523544121, 0.05740695090967, 0, -0.03844330645187, -0.0429584598942, 0)

        Part.ShowNamedView2("*Trimetric", 8)

        Part.ClearSelection2(True)

        Dim myFeature As Object

        myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, True, 0, 0, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, True, True, True, 0, 0, False)

        boolstatus = Part.Extension.SelectByID2("", "FACE", -0.0785775433435, 0.01894373057962, 0, True, 0, Nothing, 0)

        boolstatus = Part.FeatureManager.InsertConvertToSheetMetal(0.002, False, False, 0.004, 0.002, 0, 0.5)

        Part.ClearSelection2(True)

        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)

        Part.SketchManager.InsertSketch(True)

        Part.ClearSelection2(True)

        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.02256810687936, 0.06039039042219, 0, 0.02390260459754, -0.04039198125838, 0)

        Part.ClearSelection2(True)

        myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, True, 0, 0, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, True, True, True, 0, 0, False)

        boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0009118315510932, 0.02609254832731, 0, True, 0, Nothing, 0)

        boolstatus = Part.FeatureManager.InsertConvertToSheetMetal(0.002, False, False, 0.004, 0.002, 0, 0.5)

        Part.ClearSelection2(True)

        Part.SketchManager.InsertSketch(True)

        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)

        Part.ClearSelection2(True)

        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.05411927414525, 0.01318437124604, 0, -0.007403979976402, -0.001979918613586, 0)

        Dim customBendAllowanceData As Object

        customBendAllowanceData = Nothing

        myFeature = Part.FeatureManager.InsertSheetMetalBaseFlange2(0.002, False, 0.004, 0.02, 0.01, False, 0, 0, 1, customBendAllowanceData, False, 2, 0.0001, 0.0001, 0.5, True, False, True, True)

        Part.ClearSelection2(True)

    End Sub

    Public swApp As SldWorks

End Class