Create Projection Split Line Feature Example (VBA)

This example shows how to create a projection split line feature.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified document template exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Creates a new model document with a feature extrusion, reference plane,
'    and sketch of an ellipse.
' 2. Creates Split Line1 in the FeatureManager design tree.
' 3. Inspect the Immediate window.
'----------------------------------------------------------------------------
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim skSegment As SldWorks.SketchSegment
Dim myRefPlane As SldWorks.RefPlane
Dim swSelMgr As SldWorks.SelectionMgr
Dim swSplitLine As SldWorks.SplitLineFeatureData
Dim vSkLines As Variant
Dim myFeature As SldWorks.Feature
Dim boolstatus As Boolean
Dim longstatus As Long

Sub main()

    Set swApp = Application.SldWorks

    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2015\templates\Part.prtdot", 0, 0, 0)
    Set Part = swApp.ActiveDoc
  
    Set skSegment = Part.SketchManager.CreateEllipse(-2.12512457655407E-02, 1.22505076014363E-02, 0, 2.77468345541365E-03, 7.05202391259263E-03, 0, -1.96159170237913E-02, 1.98085370103935E-02, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
   

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

    Set myRefPlane = Part.FeatureManager.InsertRefPlane(8, 0.01778, 0, 0, 0, 0)
    Part.ClearSelection2 True
   

    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -4.07148636658249E-02, 2.47341229458697E-02, 1.94913387248102E-02, False, 0, Nothing, 0)
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
    boolstatus = Part.Extension.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
   

    vSkLines = Part.SketchManager.CreateCornerRectangle(-6.25406077424486E-02, 2.97244912047745E-02, 0, 5.84903577919818E-02, -0.018090206988802, 0)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 4, Nothing, 0)
   

    Set myFeature = Part.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.00254, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
    Part.SelectionManager.EnableContourSelection = False
 

    boolstatus = Part.Extension.SelectByID2("Boss-Extrude1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", -1.43044793836914E-02, 3.34438727079956E-03, 0, True, 4, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("", "FACE", -1.81817275523031E-02, 1.32444059746035E-02, 1.77800000000161E-02, True, 1, Nothing, 0)
   

    Part.InsertSplitLineProject True, True
   

    Set swSelMgr = Part.SelectionManager
    Set swSelData = swSelMgr.CreateSelectData
   

    boolstatus = Part.Extension.SelectByID2("Split Line1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
   

    Set myFeature = swSelMgr.GetSelectedObject6(1, -1)
    Set swSplitLine = myFeature.GetDefinition
   

    ' Get split line feature data
     boolstatus = swSplitLine.AccessSelections(Part, Nothing)
    
    Debug.Print myFeature.Name
    Debug.Print "    Split type as defined in swSplitLineFeatureType_e: " & swSplitLine.GetType
    Debug.Print "    Single Direction? " & swSplitLine.SingleDirection
    Debug.Print "    Reversed? " & swSplitLine.ReverseDirection
  

    swSplitLine.ReleaseSelectionAccess

End Sub