Insert Thin Cut Extrude Example (VB.NET)

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

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

' Preconditions: Specified part exists.

'

' Postconditions: A thin cut extrude feature in inserted in

'                the part.

'

' NOTE: Because this 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 longstatus As Long, longwarnings As Long

 

        ' Open part

        swApp.OpenDoc6("C:\Program Files\SolidWorks Corp\SolidWorks\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