Change the Plane of a Sketch Example (VBA)

This example shows how to modify the plane of a sketch.

'----------------------------------------------------------------------------
' Preconditions: Verify that the specified template exists.
'
' Postconditions:
' 1. Creates a new part document with a sketch of a spline.
' 2. Changes the plane of the sketch Top Plane to the Front Plane.
' 3. Examine the FeatureManager design tree and graphics area.
'----------------------------------------------------------------------------

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim skSegment As SldWorks.SketchSegment
Dim boolstatus As Boolean
 

Option Explicit

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.NewDocument("C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2017\templates\Part.prtdot", 0, 0, 0)
  

    boolstatus = Part.Extension.SelectByID2("Top Plane", "PLANE", -4.94443883882606E-02, 0.010829578664819, 1.87336739521956E-02, True, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
   

    Dim pointArray As Variant
    Dim points() As Double
    ReDim points(0 To 11) As Double
    points(0) = -6.96700449874595E-02
    points(1) = -2.05096087491173E-02
    points(2) = 0
    points(3) = -3.49133034431539E-02
    points(4) = 1.51865041882777E-02
    points(5) = 0
    points(6) = 1.83177421652422E-02
    points(7) = 0
    points(8) = 0
    points(9) = 0.060902578651959
    points(10) = 3.36608082523681E-02
    points(11) = 0
    pointArray = points
   

    Set skSegment = Part.SketchManager.CreateSpline((pointArray))
    Part.SketchManager.InsertSketch True
   

    boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Top Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    boolstatus = Part.DeSelectByID("Top Plane", "PLANE", 0, 0, 0)
   

    ' Select sketch and new plane for the sketch
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
    ' Change the plane of the sketch
    boolstatus = Part.Extension.ChangeSketchPlane(1, Nothing)
    boolstatus = Part.EditRebuild3()
   

    Part.ShowNamedView2 "*Isometric", 7
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
   

End Sub