Sheet Metal Drawing automation

jaimin.ja.3 — Fri, 02 Jun 2023 10:29:53 GMT

IS THERE ANY POSSIBITY TO AUTOMATE THIS PROCESS?

FROM ASSEMBLY OPEN SHEETMETAL COMPONENTS ONE BY ONE
OPEN DRAFTING FILE ANSI.idw (PATH - "C:\Users\Public\Documents\Autodesk\Inventor 2023\Templates\en-US\Metric\ANSI (mm).idw")
VIEW1 = PLACE BASE VIEW (Flat Pattern (Sheet Metal View)) (Style = Hidden Line Removed)
VIEW2 = PLACE ISOMATRIC VIEW (Style = Hidden Line Removed)

FOR THE SCALE AND POSITION OF THIS TWO VIEW CONSIDE FOLLOWING CODE

If ActiveSheet.View("VIEW1").Height < 250 Then ActiveSheet.View("VIEW1").Scale = 0.6 ActiveSheet.View("VIEW1").SetCenter(175, 222) ActiveSheet.View("VIEW2").SetCenter(450,262.5) ElseIf ActiveSheet.View("VIEW1").Height < 500 Then ActiveSheet.View("VIEW1").Scale = 0.4 ActiveSheet.View("VIEW1").SetCenter(175, 222) ActiveSheet.View("VIEW2").SetCenter(450,262.5) ElseIf ActiveSheet.View("VIEW1").Height < 1000 Then ActiveSheet.View("VIEW1").Scale = 1/4.5 ActiveSheet.View("VIEW1").SetCenter(175, 222) ActiveSheet.View("VIEW2").SetCenter(450,262.5) End If ActiveSheet.View("VIEW2").Scale = ActiveSheet.View("VIEW1").Scale

GIVE BEND ANNOTATION (FOR BEND ANNOTATION USE FOLLOWING CODE)

Dim oDoc As DrawingDocument Dim oSheet As Sheet Dim oView As DrawingView Dim oCurve As DrawingCurve Dim oBendNote As BendNote Dim BendNoteCount As Integer oDoc = ThisApplication.ActiveDocument oSheet = oDoc.ActiveSheet BendNoteCount = oSheet.DrawingNotes.BendNotes.Count If BendNoteCount=0 Then '[add bend notes to views For Each oView In oSheet.DrawingViews For Each oCurve In oView.DrawingCurves If oCurve.EdgeType = Inventor.DrawingEdgeTypeEnum.kBendDownEdge _ Or oCurve.EdgeType = Inventor.DrawingEdgeTypeEnum.kBendUpEdge Then ' Create the bend note oBendNote = oSheet.DrawingNotes.BendNotes.Add(oCurve) End If Next 'oCurve Next ']oView Else 'do nothing End If

SAVE IDW FILE (IF POSSIBLE, FILE NAME SHOULD BE LIKE <PART NO> & <MATERIAL> & <THIKNESS>
EXPORT DWG FILE WITH SAME NAME
EXPORT PDF FILE WITH SAME NAME

SAVE THESE FILES IN TO SAME FOLDER

Re: Sheet Metal Drawing automation

JelteDeJong — Fri, 02 Jun 2023 22:05:23 GMT

This rule is not finished (but I'm tired.) I guess that this does most of what you are looking for. Give it a try:

Sub Main() Dim doc As AssemblyDocument = ThisDoc.Document For Each refDoc As Document In doc.AllReferencedDocuments If (IsSheetmetal(refDoc) = False) Then Return Dim drawing = CreateNewDrawing() Dim flatView = CreateFlatpatternView(drawing.ActiveSheet, refDoc) Dim isoView = CreateIsoView(drawing.ActiveSheet, refDoc) Next End Sub Public Function IsSheetmetal(doc As Document) As Boolean Return doc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End Function Public Function CreateNewDrawing() As DrawingDocument Dim templateFileName = "C:\Users\Public\Documents\Autodesk\Inventor 2023\Templates\en-US\Metric\ANSI (mm).idw" Return ThisApplication.Documents.Add(DocumentTypeEnum.kDrawingDocumentObject, templateFileName) End Function Public Function CreateFlatpatternView(sheet As Sheet, doc As Document) As DrawingView Dim point = CreatePoint(17.5, 22.2) Dim nvm = ThisApplication.TransientObjects.CreateNameValueMap() nvm.Add("SheetMetalFoldedModel", False) Dim view = sheet.DrawingViews.AddBaseView(doc, point, 1, ViewOrientationTypeEnum.kFrontViewOrientation, DrawingViewStyleEnum.kHiddenLineDrawingViewStyle, "VIEW1",, nvm) SetScale(view) view.Center = point AddBendNotes(view) Return view End Function Public Function CreateIsoView(sheet As Sheet, doc As Document) As DrawingView Dim point = CreatePoint(45, 26.25) Dim view = sheet.DrawingViews.AddBaseView(doc, point, 1, ViewOrientationTypeEnum.kFrontViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle, "VIEW2") SetScale(view) view.Center = point Return view End Function Public Sub SetScale(view As DrawingView) view.Scale = 1 If (view.Height < 25) Then view.Scale = 0.6 ElseIf (view.Height < 500) Then view.Scale = 0.4 ElseIf (view.Height < 1000) Then view.Scale = 1 / 4.5 End If End Sub Public Function CreatePoint(x As Double, y As Double) Return ThisApplication.TransientGeometry.CreatePoint2d(x, y) End Function Public Sub AddBendNotes(view As DrawingView) Dim sheet = view.Parent For Each curve In view.DrawingCurves If (curve.EdgeType = DrawingEdgeTypeEnum.kBendDownEdge Or curve.EdgeType = DrawingEdgeTypeEnum.kBendUpEdge) Then sheet.DrawingNotes.BendNotes.Add(curve) End If Next End Sub

topic Re: Sheet Metal Drawing automation in Inventor Programming Forum

Sheet Metal Drawing automation

Re: Sheet Metal Drawing automation