Insert Cut Extrude Example (VB.NET)

This example shows how to insert a cut extrude feature.

'-------------------------------------------------------------
' Preconditions: Verify that the specified file to open exists.
'
' Postconditions:
' 1. Inserts a cut extrude feature in the model.
' 2. Examine the graphics area.
'
' NOTE: Because the 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 fileerror As Long, filewarning As Long

        ' Open part document
        swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\plate.sldprt", swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", fileerror, filewarning)
        swModel = swApp.ActiveDoc
        swModelDocExt = swModel.Extension

        ' Select the face where to sketch a circle
        boolstatus = swModelDocExt.SelectByID2("", "FACE", -0.02031412853728, 0.006977746007294, -0.008053400767039, False, 0, Nothing, 0)
        swSketchManager = swModel.SketchManager
        swSketchManager.InsertSketch(True)
        swModel.ClearSelection2(True)

        ' Sketch a circle
        swSketchSegment = swSketchManager.CreateCircle(0.0#, 0.0#, 0.0#, 0.01708, -0.030458, 0.0#)
        boolstatus = swModelDocExt.SelectByID2("Arc1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
        swModel.ClearSelection2(True)

        ' Create a cut-extrude feature using the circle
        swFeatureManager = swModel.FeatureManager
        swFeature = swFeatureManager.FeatureCut3(True, False, False, swEndConditions_e.swEndCondThroughAll, swEndConditions_e.swEndCondBlind, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, False, True, True, False, False, False, swStartConditions_e.swStartSketchPlane, 0, False)

    End Sub

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

    ''' </summary>
    Public swApp As SldWorks

End Class