Insert Cut Extrude Example (VBA)

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.

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

Option Explicit

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swModelDocExt As SldWorks.ModelDocExtension

Dim swSketchManager As SldWorks.SketchManager

Dim swSketchSegment As SldWorks.SketchSegment

Dim swFeatureManager As SldWorks.FeatureManager

Dim swFeature As SldWorks.Feature

Dim boolstatus As Boolean

Dim fileerror As Long, filewarning As Long

Sub main()

Set swApp = Application.SldWorks

' Open document

swApp.OpenDoc6 "C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\plate.sldprt", swDocPART, swOpenDocOptions_Silent, "", fileerror, filewarning

Set swModel = swApp.ActiveDoc

Set 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)

Set swSketchManager = swModel.SketchManager

swSketchManager.InsertSketch True

swModel.ClearSelection2 True

' Sketch a circle

Set swSketchSegment = swSketchManager.CreateCircle(0#, 0#, 0#, 0.01708, -0.030458, 0#)

boolstatus = swModelDocExt.SelectByID2("Arc1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)

swModel.ClearSelection2 True

' Create a cut-extrude feature using the circle

Set swFeatureManager = swModel.FeatureManager

Set swFeature = swFeatureManager.FeatureCut3(True, False, False, swEndCondThroughAll, swEndCondBlind, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, False, True, True, False, False, False, swStartSketchPlane, 0, False)

End Sub