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Fill Holes in Part Example (VBA)

In CAM drilling operations, it might be useful to deduce the appearance of an item before machining begins. This is slightly different than calculating the minimum amount of raw material required, i.e., the stock size. This example shows how to use some of the geometry- and topology-related methods and properties to fill all holes in a part.

' Preconditions: Part containing holes and only one
' solid body is open.
' Postconditions:
' 1. New part is created.
' 2. New part is similar to original part, but new
'    part's holes are filled.
' 3. To see the names of the Surface-Imported, Surface-Knit,
'    and Thicken features created by filling the holes, 
'    examine the FeatureManager design tree.
' * Only holes that completely reside on a face are filled.
' * Fillets and chamfers are not taken into account.
Option Explicit
Sub main()
    Dim swApp                       As SldWorks.SldWorks
    Dim swModel                     As SldWorks.ModelDoc2
    Dim swPart                      As SldWorks.PartDoc
    Dim swBody                      As SldWorks.Body2
    Dim swFace                      As SldWorks.Face2
    Dim swLoop                      As SldWorks.Loop2
    Dim vEdgeArr                    As Variant
    Dim swCurve()                   As SldWorks.Curve
    Dim vCurveArr                   As Variant
    Dim swEdge                      As SldWorks.Edge
    Dim swTempBody                  As SldWorks.Body2
    Dim swSurf                      As SldWorks.Surface
    Dim swSurfCopy                  As SldWorks.Surface
    Dim sPartTemplateName           As String
    Dim swNewModel                  As SldWorks.ModelDoc2
    Dim swNewPart                   As SldWorks.PartDoc
    Dim swFeat()                    As SldWorks.Feature
    Dim swKnitFeat                  As SldWorks.Feature
    Dim swThickFeat                 As SldWorks.Feature
    Dim swNewFeatMgr                As SldWorks.FeatureManager
    Dim i                           As Long
    Dim bRet                        As Boolean
    Dim vBodies                     As Variant
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swPart = swModel
    vBodies = swPart.GetBodies2(swSolidBody, False)
    Set swBody = vBodies(0)
    ' Create new part
    sPartTemplateName = swApp.GetUserPreferenceStringValue(swDefaultTemplatePart)
    Set swNewModel = swApp.NewDocument(sPartTemplateName, swDwgPaperAsize, 0#, 0#)
    Set swNewFeatMgr = swNewModel.FeatureManager
    Set swNewPart = swNewModel
    ReDim swFeat(0)
    Set swFace = swBody.GetFirstFace
    Do While Not swFace Is Nothing
        Set swLoop = swFace.GetFirstLoop
        Do While Not swLoop Is Nothing
            If swLoop.IsOuter Then
                vEdgeArr = swLoop.GetEdges
                If UBound(vEdgeArr) >= 0 Then
                    ReDim swCurve(UBound(vEdgeArr))
                    For i = 0 To UBound(vEdgeArr)
                        Set swEdge = vEdgeArr(i)
                        Set swCurve(i) = swEdge.GetCurve
                    Next i
                    vCurveArr = swCurve
                    Set swSurf = swFace.GetSurface
                    Set swSurfCopy = swSurf.Copy
                    Set swTempBody = swSurfCopy.CreateTrimmedSheet4(vCurveArr, False)
                    ' Typically nothing is returned if the loop is
                    ' perpendicular to the surface, as in the
                    ' end loops of a cylinder
                    If Not swTempBody Is Nothing Then
                        ' Sheet body only has one face
                        Debug.Assert 1 = swTempBody.GetFaceCount
                        Debug.Assert swSheetBody = swTempBody.GetType
                        Set swFeat(UBound(swFeat)) = swNewPart.CreateFeatureFromBody3(swTempBody, False, swCreateFeatureBodyCheck)
                        Debug.Assert Not swFeat(UBound(swFeat)) Is Nothing
                        ReDim Preserve swFeat(UBound(swFeat) + 1)
                    End If
                End If
            End If
            Set swLoop = swLoop.GetNext
        Set swFace = swFace.GetNextFace
    ' Remove last empty feature
    ReDim Preserve swFeat(UBound(swFeat) - 1)
    swNewModel.ClearSelection2 True
    For i = 0 To UBound(swFeat)
        bRet = swFeat(i).Select2(True, 1): Debug.Assert bRet
    Next i
    swNewFeatMgr.InsertSewRefSurface True, False, False, 3.001639406912E-05, 0.0001
    ' Make sure surfaces are successfully sewn together
    Set swKnitFeat = swNewModel.FeatureByPositionReverse(0)
    Debug.Assert Not swKnitFeat Is Nothing
    Debug.Assert "SewRefSurface" = swKnitFeat.GetTypeName
    bRet = swKnitFeat.Select2(False, 1): Debug.Assert bRet
    Set swThickFeat = swNewFeatMgr.FeatureBossThicken(0.01, 0, 0, True, True, True, True)
    Debug.Assert Not swThickFeat Is Nothing
End Sub

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