Insert Cut Extrude Example (VB.NET)

This example shows how to insert a cut extrude feature.

'---------------------------------------------

' Preconditions: Specified file exists.

'

' Postconditions: A cut extrude feature is inserted in

'                the model.

'

' NOTE: Because the part document is used by an online

' SolidWorks tutorial, do not save any changes when

' closing the document.

'----------------------------------------------

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:\Program Files\SolidWorks Corp\SolidWorks\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