Insert Thin Cut Extrude Example (VB.NET)

This example shows how to insert a thin cut extrude feature.

'------------------------------------------------------
' Preconditions: Verify that the specified part exists.
'
' Postconditions:
' 1. Opens the part.
' 2. Inserts a thin cut extrude feature in the part.
' 3. Examine the FeatureManager design tree and
'    graphics area.
'
' NOTE: Because this part document is used elsewhere,
' do not save changes.
'-----------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System

Partial Class SolidWorksMacro

    Public 
 Sub main()

        Dim swModel As ModelDoc2
        Dim swModelDocExt As ModelDocExtension
        Dim swSketchManager As SketchManager
        Dim swSketchSegment As SketchSegment
        Dim swFeatureManager As FeatureManager
        Dim swFeature As Feature
        Dim boolstatus As Boolean
        Dim longstatus As Integer, longwarnings As Integer

        ' Open part
        swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\water.sldprt", 1, 0, "", longstatus,
longwarnings)
        swModel = swApp.ActiveDoc

        ' Select face on which to sketch a circle
        swModelDocExt = swModel.Extension
        boolstatus = swModelDocExt.SelectByID2("", "FACE", 0.0001655362220845, -0.0477671348753, 0.072, False, 0, Nothing, 0)
        swModel.ShowNamedView2("*Normal To", swStandardViews_e.swBackView)
        swModel.ClearSelection2(True)

        ' Sketch a circle
        swSketchManager = swModel.SketchManager
        swSketchSegment = swSketchManager.CreateCircle(0.0#, 0.0#, 0.0#, 0.030255, -0.042492, 0.0#)
        swModel.ClearSelection2(True)

        ' Create the thin cut extrude
        boolstatus = swModelDocExt.SelectByID2("Arc1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
        swFeatureManager = swModel.FeatureManager
        swFeature = swFeatureManager.FeatureCutThin2(True, False, False, swEndConditions_e.swEndCondBlind,
swEndConditions_e.swEndCondBlind, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False,
False, False, 0.01, 0.01, 0.01, 0, 0, False, 0.005, True, True, swStartConditions_e.swStartSketchPlane, 0, False)
        swModel.ShowNamedView2("*Isometric", swStandardViews_e.swIsometricView)

    End Sub

    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks

End Class