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Create Replace Face Feature Example (VBA)

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 Plane1, Surface-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.
' ---------------------------------------------------------------------------

Dim swApp As SldWorks.SldWorks
Dim selMgr As SldWorks.SelectionMgr
Dim Part As SldWorks.ModelDoc2
Dim feat As SldWorks.Feature
Dim featData As SldWorks.ReplaceFaceFeatureData
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Option Explicit

Sub main()

    Set swApp = Application.SldWorks
   

    Set Part = swApp.OpenDoc6("C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\samples\tutorial\api\block20.sldprt", 1, 0, "", longstatus, longwarnings)
    swApp.ActivateDoc2 "block20", False, longstatus
    Set Part = swApp.ActiveDoc
   

    boolstatus = Part.Extension.SelectByID2("", "FACE", 6.87152192142548E-03, 2.56655537640995E-02, 0.049345602378537, True, 0, Nothing, 0)
    Dim myRefPlane As SldWorks.RefPlane
    Set myRefPlane = Part.FeatureManager.InsertRefPlane(264, 0.05842, 0, 0, 0, 0)
    Part.ClearSelection2 True
   

    Dim pointArray As Variant
    Dim points() As Double
    ReDim points(0 To 14) As Double
    points(0) = -7.00496017443584E-02
    points(1) = 5.82762055241233E-02
    points(2) = 0
    points(3) = -3.57558994484748E-02
    points(4) = 8.53945497913173E-02
    points(5) = 0
    points(6) = -5.88719099721402E-03
    points(7) = 6.71372129016845E-02
    points(8) = 0
    points(9) = 2.73002628375139E-02
    points(10) = 8.78577815467452E-02
    points(11) = 0
    points(12) = 7.37626982062238E-02
    points(13) = 5.82762055241233E-02
    points(14) = 0
    pointArray = points
    Dim skSegment As SldWorks.SketchSegment
    Set skSegment = Part.SketchManager.CreateSpline((pointArray))
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("Spline1@Sketch2", "EXTSKETCHSEGMENT", -5.49544681183813E-02, 8.75052976097064E-02, 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 True, False, False, 0, 0, 0.14478, 0.14478, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False
    Part.SelectionManager.EnableContourSelection = False
    boolstatus = Part.Extension.SelectByID2("", "FACE", 5.85444908073214E-02, 3.96239999998329E-02, -5.18899759430838E-02, True, 0, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "SURFACEBODY", -1.89730427370591E-02, 7.26880897401543E-02, 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", 5.85444908073214E-02, 3.96239999998329E-02, -5.18899759430838E-02, True, 1, Nothing, 0)
    boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "SURFACEBODY", -1.89730427370591E-02, 7.26880897401543E-02, 0.115671174990496, True, 2, Nothing, 0)
    Part.InsertFeatureReplaceFace
    boolstatus = Part.Extension.SelectByID2("", "FACE", -3.62064915135534E-02, 8.56902732399476E-02, 0.127037337239983, False, 0, Nothing, 0)
    Part.FeatureManager.HideBodies
    boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", -6.93294107213475E-02, 8.72697709380442E-02, -3.00713252946179E-02, False, 0, Nothing, 0)
    Part.BlankRefGeom
   

    boolstatus = Part.Extension.SelectByID2("Replace Face1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
    Set selMgr = Part.SelectionManager
    Set feat = selMgr.GetSelectedObject6(1, -1)
    Set featData = feat.GetDefinition
   

    featData.AccessSelections Part, Nothing
   

    Dim vFacesToReplace As Variant
    vFacesToReplace = featData.FacesForReplacement
    Debug.Print featData.GetFacesForReplacementCount & " face replaced in " & vFacesToReplace(0).GetFeature.Name
    Debug.Print featData.GetReplacementSurfacesCount & " replacement surface "

    featData.ReleaseSelectionAccess

End Sub

 



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