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Create Replace Face Feature Example (VB.NET)

This example shows how to create a Replace Face feature.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified model document exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Opens the specified part.
' 2. Creates Plane1Surface-Extrude1, and Replace Face1.
' 3. Inspect the FeatureManager design tree, the graphics area, and the
'    Immediate window.
'
' NOTE: Because the model is used elsewhere, do not save changes.
' ---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
 
    Dim selMgr As SelectionMgr
    Dim Part As ModelDoc2
    Dim feat As Feature
    Dim featData As ReplaceFaceFeatureData
    Dim boolstatus As Boolean
    Dim longstatus As Integer, longwarnings As Integer
 
 
    Sub main()
 
 
        Part = swApp.OpenDoc6("C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\samples\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
        swApp.ActivateDoc2("block20"False, longstatus)
        Part = swApp.ActiveDoc
 
        boolstatus = Part.Extension.SelectByID2("""FACE", 0.00687152192142548, 0.0256655537640995, 0.049345602378537, True, 0, Nothing, 0)
        Dim myRefPlane As RefPlane
        myRefPlane = Part.FeatureManager.InsertRefPlane(264, 0.05842, 0, 0, 0, 0)
        Part.ClearSelection2(True)
 
        Dim pointArray As Object
        Dim points(0 To 14) As Double
        points(0) = -0.0700496017443584
        points(1) = 0.0582762055241233
        points(2) = 0
        points(3) = -0.0357558994484748
        points(4) = 0.0853945497913173
        points(5) = 0
        points(6) = -0.00588719099721402
        points(7) = 0.0671372129016845
        points(8) = 0
        points(9) = 0.0273002628375139
        points(10) = 0.0878577815467452
        points(11) = 0
        points(12) = 0.0737626982062238
        points(13) = 0.0582762055241233
        points(14) = 0
        pointArray = points
        Dim skSegment As SketchSegment
        skSegment = Part.SketchManager.CreateSpline((pointArray))
        Part.SketchManager.InsertSketch(True)
        boolstatus = Part.Extension.SelectByID2("Spline1@Sketch2""EXTSKETCHSEGMENT", -0.0549544681183813, 0.0875052976097064, 0, False, 0, Nothing, 0)
        Part.ClearSelection2(True)
        boolstatus = Part.Extension.SelectByID2("Sketch2""SKETCH", 0, 0, 0, False, 4, Nothing, 0)
        Part.SelectionManager.EnableContourSelection = True
        boolstatus = Part.Extension.SelectByID2("Sketch2""SKETCHCONTOUR", 0, 0, 0, True, 4, Nothing, 0)
        Part.FeatureExtruRefSurface2(TrueFalseFalse, 0, 0, 0.14478, 0.14478, FalseFalseFalseFalse, 0.0174532925199433, 0.0174532925199433, FalseFalseFalseFalse)
        Part.SelectionManager.EnableContourSelection = False
        boolstatus = Part.Extension.SelectByID2("""FACE", 0.0585444908073214, 0.0396239999998329, -0.0518899759430838, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Surface-Extrude1""SURFACEBODY", -0.0189730427370591, 0.0726880897401543, 0.115671174990496, True, 0, Nothing, 0)
        Part.ClearSelection2(True)
        boolstatus = Part.Extension.SelectByID2("Surface-Extrude1""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("""FACE", 0.0585444908073214, 0.0396239999998329, -0.0518899759430838, True, 1, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Surface-Extrude1""SURFACEBODY", -0.0189730427370591, 0.0726880897401543, 0.115671174990496, True, 2, Nothing, 0)
        Part.InsertFeatureReplaceFace()
        boolstatus = Part.Extension.SelectByID2("""FACE", -0.0362064915135534, 0.0856902732399476, 0.127037337239983, False, 0, Nothing, 0)
        Part.FeatureManager.HideBodies()
        boolstatus = Part.Extension.SelectByID2("Plane1""PLANE", -0.0693294107213475, 0.0872697709380442, -0.0300713252946179, False, 0, Nothing, 0)
        Part.BlankRefGeom()
 
        boolstatus = Part.Extension.SelectByID2("Replace Face1""BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        selMgr = Part.SelectionManager
        feat = selMgr.GetSelectedObject6(1, -1)
        featData = feat.GetDefinition
 
        featData.AccessSelections(Part, Nothing)
 
        Dim vFacesToReplace As Object
        vFacesToReplace = featData.FacesForReplacement
        Debug.Print(featData.GetFacesForReplacementCount & " face replaced in " & vFacesToReplace(0).GetFeature.Name)
        Debug.Print(featData.GetReplacementSurfacesCount & " replacement surface ")
 
        featData.ReleaseSelectionAccess()
 
    End Sub
 
 
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
 
End Class
 

 



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