Insert Thin Cut Extrude Example (VBA)
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.
'----------------------------------------
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 longstatus As Long, longwarnings As Long
Sub main()
Set swApp = Application.SldWorks
' Open part
swApp.OpenDoc6
"C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\water.sldprt",
1, 0, "", longstatus, longwarnings
Set swModel = swApp.ActiveDoc
' Select face on which to sketch a circle
Set swModelDocExt = swModel.Extension
boolstatus = swModelDocExt.SelectByID2("",
"FACE", 1.655362220845E-04, -0.0477671348753, 0.072, False,
0, Nothing, 0)
swModel.ShowNamedView2
"*Normal To", swBackView
swModel.ClearSelection2
True
' Sketch a circle
Set swSketchManager = swModel.SketchManager
Set swSketchSegment = swSketchManager.CreateCircle(0#,
0#, 0#, 0.030255, -0.042492, 0#)
swModel.ClearSelection2
True
' Create the thin cut extrude
boolstatus = swModelDocExt.SelectByID2("Arc1",
"SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
Set swFeatureManager = swModel.FeatureManager
Set swFeature = swFeatureManager.FeatureCutThin2(True,
False, False, swEndCondBlind, 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, swStartSketchPlane,
0, False)
swModel.ShowNamedView2
"*Isometric", swIsometricView
End Sub