Create Hole Wizard Hole Example (VBA)

This example shows how to create a hole using the hole wizard.

'---------------------------------------------------------------
' Preconditions: Verify that the specified part template exists.
'
' Postconditions:
' 1. Creates a part.
' 2. Creates a hole using the hole wizard.
' 3. Examine the graphics area and FeatureManager
'    design tree.
'---------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swFeatMgr As SldWorks.FeatureManager
Dim swFeat As SldWorks.Feature
Dim swSketchMgr As SldWorks.SketchManager
Dim sketchLines As Variant
Dim longstatus As Long
Dim boolstatus As Boolean
Dim P1(2) As Double
Dim P2(2) As Double
Dim P3(2) As Double

Sub main()

    Set swApp = Application.SldWorks    

    'Create the part for the wizard hole
    swApp.ResetUntitledCount 0, 0, 0
    Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2020\templates\Part.prtdot", 0, 0, 0)
    swApp.ActivateDoc2 "Part1", False, longstatus
    Set swModel = swApp.ActiveDoc
    Set swSketchMgr = swModel.SketchManager
    Set swModelDocExt = swModel.Extension
    Set swFeatMgr = swModel.FeatureManager
    sketchLines = swSketchMgr.CreateCornerRectangle(-0.05096498314664, 0.05060941349678, 0, 0.1021670127265, -0.05037236706354, 0)
    boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
    boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
    boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
    boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
    Set swFeat = swFeatMgr.FeatureExtrusion2(True, False, False, 0, 0, 0.381, 0.381, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, True, True, True, 0, 0, False)

    'Create three points for the reference plane
    P1(0) = -1.41556764402858E-02
    P1(1) = 1.94061273859598E-03
    P1(2) = 0
    P2(0) = -1.41556764402858E-02
    P2(1) = 1.94061273859598E-03
    P2(2) = 1
    P3(0) = -0.149976101832345
    P3(1) = -0.988792859011662
    P3(2) = 0    

    'Create the reference plane
    swModel.CreatePlaneFixed2 P1, P2, P3, False    

    'Select reference plane
    boolstatus = swModelDocExt.SelectByID2("Plane1", "PLANE", -1.56784487003801E-02, -9.16715285390111E-03, 5.58270998665543E-02, False, 0, Nothing, 0)

    'Create the hole wizard countersink hole
    Set swFeat = swFeatMgr.HoleWizard5(swWzdCounterSink, swStandardAnsiMetric, swStandardAnsiMetricFlatHead82, "M2", swEndCondThroughAll, 0.0102, 0.010312189893273, 0, 0.0044, 1.57079632679489, 1.52189893272978E-04, 0, -1, -1, -1, -1, 1, -1, -1, -1, "", False, True, True, True, True, False)       

End Sub