Create Surface-sweep Feature Example (VBA)

This example shows how to create a surface-sweep feature.

'---------------------------------------------------
' Preconditions: Verify that the part template exists.
'
' Postconditions:
' 1. Opens a new part.
' 2. Creates two sketches.
' 3. Inserts a surface-sweep feature.
' 4. Examine the FeatureManager design tree and
'    graphics area.
'---------------------------------------------------
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 swFeature As SldWorks.Feature
Dim swFeatureManager As SldWorks.FeatureManager
Dim status As Boolean

Sub main()

    Set swApp = Application.SldWorks    

    'Open new part document
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2017\templates\part.prtdot", 0, 0, 0)
    Set swModelDocExt = swModel.Extension    

    'Create a sketch
    Set swSketchManager = swModel.SketchManager
    swSketchManager.InsertSketch True
    status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Set swSketchSegment = swSketchManager.CreateLine(0#, 0#, 0#, 0.068491, 0.049604, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.068491, 0.049604, 0#, 0.10923, 0.112837, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.10923, 0.112837, 0#, 0.194652, 0.154023, 0#)
    swSketchManager.InsertSketch True    

    swModel.ViewZoomtofit2
    swModel.ShowNamedView2 "*Isometric", 7
    swModel.ClearSelection2 True

    'Create another sketch
    status = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    swSketchManager.InsertSketch True
    Set swSketchSegment = swSketchManager.CreateLine(-0#, 0#, 0#, 0.021042, 0.091756, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.021042, 0.091756, 0#, 0.098366, 0.085093, 0#)
    Set swSketchSegment = swSketchManager.CreateLine(0.098366, 0.085093, 0#, 0.143062, 0.122696, 0#)
    swModel.ClearSelection2 True
    swSketchManager.InsertSketch True    

    'Insert surface sweep
    status = swModelDocExt.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, False, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, True, 4, Nothing, 0)
    Set swFeatureManager = swModel.FeatureManager
    Set swFeature = swFeatureManager.InsertSweepSurface3(False, 0, False, False, 0, 0, 0, True, True, 0, True, False, 0, 0)    

End Sub