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Create 3D Sketch Plane Example (VBA)

This example shows how to create a 3D sketch plane.

'------------------------------------------------------------------
' Preconditions: Verify that the specified part template exists.
'
' Postconditions:
' 1. Inserts a 3D sketch of two lines.
' 2. Inserts a 2D sketch of a circle.
' 3. Selects a line in the 3D sketch and the center of the circle
'    in the 2D sketch.
' 4. Inserts a 3D sketch plane.
' 5. Examine the graphics area and the FeatureManager design tree.
'-------------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchManager As SldWorks.SketchManager
Dim swSketchSegment As SldWorks.SketchSegment
Dim swSketch As SldWorks.Sketch
Dim status As Boolean
Sub main()
    Set swApp = Application.SldWorks    
    'Open new part document
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2015\templates\Part.prtdot", 0, 0, 0)    
    'Insert 3D sketch of two lines
    Set swSketchManager = swModel.SketchManager
    swSketchManager.Insert3DSketch True
    Set swSketchSegment = swSketchManager.CreateCenterLine(-0.082642, 0.005659, 0#, -0.049926, 0.045073, 0#)
    Set swSketch = swSketchManager.ActiveSketch
    status = swSketch.SetWorkingPlaneOrientation(0, 0, 0, 0, 1, 0, 0, 0, 1, 1, 0, 0)
    Set swSketchSegment = swSketchManager.CreateCenterLine(-0.049926, 0.045073, 0#, -0.049926, -0.022634, -0.065874)
    Set swSketch = swSketchManager.ActiveSketch
    status = swSketch.SetWorkingPlaneOrientation(0, 0, 0, 0, 0, 1, 1, 0, 0, 0, 1, 0)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True    
    'Insert 2D sketch of a circle
    swModel.ActivateSelectedFeature
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True
    Set swModelDocExt = swModel.Extension
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    swModel.ClearSelection2 True
    Set swSketchSegment = swSketchManager.CreateCircle(-0.056401, 0.005985, 0#, -0.054697, -0.005141, 0#)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True
    swModel.ClearSelection2 True    
    'Insert a 3D sketch plane
    swSketchManager.Insert3DSketch True
    status = swModelDocExt.SelectByID2("Line1@3DSketch1", "EXTSKETCHSEGMENT", -5.65609614209999E-02, 3.70796232466087E-02, 0, True, 0, Nothing, 0)
    status = swModelDocExt.SelectByID2("Point2@Sketch1", "EXTSKETCHPOINT", -5.64010297276809E-02, 5.98490302365917E-03, 0, True, 0, Nothing, 0)
    status = swSketchManager.CreateSketchPlane(9, 9, 0)
    status = swModelDocExt.SelectByID2("Plane1", "SKETCHSURFACES", 0, 0, 0, False, 0, Nothing, 0)
    swModel.ActivateSelectedFeature
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True
End Sub


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