Create Drawing View for Each Model's View Design Representation

[ngdnam88]

Dears,

I'm trying create/add more views in drawing for all Model's View Design Representation create in this post: https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/create-view-design-representation-fo...

Could you please help me how to control Representation View when add base view to drawing?

Thanks!

[JelteDeJong · Accepted solution]

maybe this is some help to you:

' Lots of variable that can be set:
Dim startPositionX = 0
Dim positionY = 0
Dim viewOrientationType As ViewOrientationTypeEnum = ViewOrientationTypeEnum.kFrontViewOrientation
Dim drawingViewStyle As DrawingViewStyleEnum = DrawingViewStyleEnum.kShadedDrawingViewStyle
Dim scale = 1.0

If (ThisDoc.Document.DocumentType <> DocumentTypeEnum.kDrawingDocumentObject) Then
    MsgBox("This only works if you opend a drawing document")
    Return
End If
Dim oTr = ThisApplication.TransientGeometry

Dim dialog As Inventor.FileDialog
ThisApplication.CreateFileDialog(dialog)
dialog.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
dialog.FilterIndex = 1
dialog.ShowOpen()

Dim modelDoc = ThisApplication.Documents.Open(dialog.FileName)
Dim modelDef = modelDoc.ComponentDefinition

Dim doc As DrawingDocument = ThisDoc.Document
Dim sheet As Sheet = doc.ActiveSheet

Dim x = startPositionX
For Each item As DesignViewRepresentation In modelDef.RepresentationsManager.DesignViewRepresentations
    Dim nameValueMap = ThisApplication.TransientObjects.CreateNameValueMap()
    nameValueMap.Add("DesignViewRepresentation", item.Name)

    Dim p As Point2d = oTr.CreatePoint2d(x, positionY)
    Dim view As DrawingView = sheet.DrawingViews.AddBaseView(modelDoc, p, scale,
                    viewOrientationType, drawingViewStyle,,, nameValueMap)

    x = x + view.Width
Next