VBA/iLogic: Auf Zeichnung Abwicklung und skizziertes Symbol einfügen wenn Erstansicht ein Blechteil ist

iLogic-Code

Imports Inventor.ViewOrientationTypeEnum
Imports Inventor.DrawingViewStyleEnum

Sub Main()
    Dim Zeich As DrawingDocument
     Zeich = ThisApplication.ActiveDocument
    
    Dim oSheet As Sheet
     oSheet = Zeich.ActiveSheet
    'Modell er esten Ansicht ermitteln
    Dim Modell As Document
     Modell = oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
    
    'Prüfen ob Modell Blechteil ist
    Dim sDocumentSubType As String
    sDocumentSubType = Modell.SubType
    
    If sDocumentSubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
        'Abwicklungsansicht erstellen
         AddFlatPatternDrawingView (Modell.FullFileName)
         
         'Symbol ergänzen
         Dim SymName As String
         SymName = "CAD-CAM"
        Dim oSketchedSymbolDef As SketchedSymbolDefinition
         oSketchedSymbolDef = Zeich.SketchedSymbolDefinitions.Item(SymName)
        
        Dim oTG As TransientGeometry
         oTG = ThisApplication.TransientGeometry
        
        Dim oSketchedSymbol As SketchedSymbol
         oSketchedSymbol = Zeich.ActiveSheet.SketchedSymbols.Add(oSketchedSymbolDef, oTG.CreatePoint2d(15, 5), 0, 1)
         
    Else
     Exit Sub
    End If
    
End Sub

Public Sub AddFlatPatternDrawingView(Modellpfad As String)
    '  a reference to the drawing document.
    ' This assumes a drawing document is active.
    Dim oDrawDoc As DrawingDocument
     oDrawDoc = ThisApplication.ActiveDocument

    ' a reference to the active sheet.
    Dim oSheet As Sheet
     oSheet = oDrawDoc.ActiveSheet

    ' Create a new NameValueMap object
    Dim oBaseViewOptions As NameValueMap
     oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap

    '  the options to use when creating the base view.
    Call oBaseViewOptions.Add("SheetMetalFoldedModel", False)

    ' Open the sheet metal document invisibly
    Dim oModel As Document
     oModel = ThisApplication.Documents.Open(Modellpfad, False)

    ' Create the placement point object.
    Dim oPoint As Point2d
     oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 20)

    ' Create a base view.
    Dim oBaseView As DrawingView
     oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 0.3, _
    kDefaultViewOrientation, kHiddenLineRemovedDrawingViewStyle, _
    , , oBaseViewOptions)
End Sub

VBA-Code

Private Sub WennBlechDannAbwicklung()
    Dim Zeich As DrawingDocument
    Set Zeich = ThisApplication.ActiveDocument
    
    Dim oSheet As Sheet
    Set oSheet = Zeich.ActiveSheet
    'Modell er esten Ansicht ermitteln
    Dim Modell As Document
    Set Modell = oSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
    
    'Prüfen ob Modell Blechteil ist
    Dim sDocumentSubType As String
    sDocumentSubType = Modell.SubType
    
    If sDocumentSubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
        'Abwicklungsansicht erstellen
         AddFlatPatternDrawingView (Modell.FullFileName)
         
         'Symbol ergänzen
         Dim SymName As String
         SymName = "CAD-CAM"
        Dim oSketchedSymbolDef As SketchedSymbolDefinition
        Set oSketchedSymbolDef = Zeich.SketchedSymbolDefinitions.Item(SymName)
        
        Dim oTG As TransientGeometry
        Set oTG = ThisApplication.TransientGeometry
        
        Dim oSketchedSymbol As SketchedSymbol
        Set oSketchedSymbol = Zeich.ActiveSheet.SketchedSymbols.Add(oSketchedSymbolDef, oTG.CreatePoint2d(0, 0), 0, 1)
         
    Else
     Exit Sub
    End If
    
End Sub

Public Sub AddFlatPatternDrawingView(Modellpfad As String)
    ' Set a reference to the drawing document.
    ' This assumes a drawing document is active.
    Dim oDrawDoc As DrawingDocument
    Set oDrawDoc = ThisApplication.ActiveDocument

    'Set a reference to the active sheet.
    Dim oSheet As Sheet
    Set oSheet = oDrawDoc.ActiveSheet

    ' Create a new NameValueMap object
    Dim oBaseViewOptions As NameValueMap
    Set oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap

    ' Set the options to use when creating the base view.
    Call oBaseViewOptions.Add("SheetMetalFoldedModel", False)

    ' Open the sheet metal document invisibly
    Dim oModel As Document
    Set oModel = ThisApplication.Documents.Open(Modellpfad, False)

    ' Create the placement point object.
    Dim oPoint As Point2d
    Set oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 20)

    ' Create a base view.
    Dim oBaseView As DrawingView
    Set oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 1, _
    kDefaultViewOrientation, kHiddenLineRemovedDrawingViewStyle, _
    , , oBaseViewOptions)
End Sub

Bemerkungen

Das ist natürlich nur ein grobes Codegerüst:

• Hat das Blech noch keine Abwicklung scheitert der Code. Da müsste man ggf. prüfen, ob eine Abwicklung vorhanden ist und wenn nicht dann eine erstellen
• Der Ansichtsmaßstab der Abwicklung und deren Position auf dem Blatt müsste abhängig von der Blechgröße und Blattgröße noch ermittelt werden
• ggf. muss die Position des Symbols angepasst werden

Links zum Thema

VBA Code in iLogic Code "umwandeln"

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