ilogic - create drawing from part
For the issue of the open dialog hanging up, please check this setting, in your project file... if it is not set to no, then setting to no might resolve this issue... I can't recall, but I remember having this issue in the past with that Open Drawing option.
See this link for more explination:
https://forums.autodesk.com/t5/inventor-forum/using-unique-file-names-option/m-p/6008909#M590217
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
As for creating a new drawing if the one isn't found, I'm not sure that we can access the create new view interfaces via automation, but something like this should get you started in creating the drawing.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
Try
ThisApplication.Documents.Open _
(ThisDoc.PathAndFileName(True).Replace("ipt", "idw"))
Return 'exit rule
Catch
End Try
oNewDrawing = ThisDoc.ChangeExtension(".idw")
oTemplateFolder = ThisApplication.FileOptions.TemplatesPath
oTemplate = oTemplateFolder & "Standard.idw"
Dim oDrawingDoc As DrawingDocument
oDrawingDoc = ThisApplication.Documents.Add _
(DocumentTypeEnum.kDrawingDocumentObject, oTemplate, True)
oDrawingDoc.Activate()
Dim oSheet As Sheet
oSheet = oDrawingDoc.Sheets.Item(1)
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(10, 10)
Dim oView As DrawingView
oView = oSheet.DrawingViews.AddBaseView(oDoc, oPoint, 1, _
ViewOrientationTypeEnum.kFrontViewOrientation, _
DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)
oDrawingDoc.SaveAs(oNewDrawing, False)
MessageBox.Show("This new file saved as: "& oNewDrawing, "iLogic")
Or maybe something like this since you mentioned you need to choose the template
Imports System.IO
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
Try 'to open the drawing
ThisApplication.Documents.Open _
(ThisDoc.PathAndFileName(True).Replace("ipt", "idw"))
Return 'exit rule
Catch
End Try
'since nothing found create it...
oNewDrawing = ThisDoc.ChangeExtension(".idw")
oTemplateFolder = ThisApplication.FileOptions.TemplatesPath
Dim oList As New ArrayList
Dim Folder As New IO.DirectoryInfo(oTemplateFolder)
For Each File As IO.FileInfo In Folder.GetFiles("*.idw", IO.SearchOption.AllDirectories)
Dim sName As New FileInfo(File.Name)
oList.Add(sName.Name)
Next
oTemplate = InputListBox("Select a template", oList, oList(0),"iLogic", "List")
oTemplate = oTemplateFolder & oTemplate
Dim oDrawingDoc As DrawingDocument
oDrawingDoc = ThisApplication.Documents.Add _
(DocumentTypeEnum.kDrawingDocumentObject, oTemplate, True)
oDrawingDoc.Activate()
Dim oSheet As Sheet
oSheet = oDrawingDoc.Sheets.Item(1)
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(10, 10)
Dim oView As DrawingView
oView = oSheet.DrawingViews.AddBaseView(oDoc, oPoint, 1, _
ViewOrientationTypeEnum.kFrontViewOrientation, _
DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)
oDrawingDoc.SaveAs(oNewDrawing, False)
MessageBox.Show("This new file saved as: "& oNewDrawing, "iLogic")
Hey Curtis -
Do you know how to get this running on an assembly? Currently throwing an error
I can change the PartDocument to an AssemblyDocument and it runs however I'm just not sure how to leave it looking for a part, but catch the error and run as an Assembly Doc instead?
This feels like a simple thing - but it doesn't quite compute yet/
Imports System.IO
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
'change this to
Imports System.IO
Dim oDoc As AssemblyDocument
oDoc = ThisApplication.ActiveDocument
'But if I try to run two variables I get stuck in the Try loop
Dim oAsm As AssemblyDocument
Dim oDpc As PartDocument
oDoc = ThisApplication.ActiveDocument
oAsm = ThisApplication.ActiveDocument
Try 'to open the drawing
ThisApplication.Documents.Open _
(ThisDoc.PathAndFileName(True).Replace("ipt", "idw"))
Return 'exit rule
Catch
ThisApplication.Documents.Open _
(ThisAsm.PathAndFileName(True).Replace("ipt", "idw"))
Return 'exit rule
End Try
'I'm just not sure how to catch the failure and turn it into opening an assembly doc.
But..... I managed to get this & my other macros into buttons
#myfirstbutton
It's the small things in life that are really satisfying...
Maybe just something like this.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Imports System.IO
Dim oDoc As Document
oDoc = ThisApplication.ActiveDocument
oExt = Right(oDoc.FullDocumentName,3) 'get file extension
Try 'to open the drawing
ThisApplication.Documents.Open _
(ThisDoc.PathAndFileName(True).Replace(oExt, "idw"))
Return 'exit rule
Catch
End Try
'since nothing found create it...
oNewDrawing = ThisDoc.ChangeExtension(".idw")
oTemplateFolder = ThisApplication.FileOptions.TemplatesPath
Dim oList As New ArrayList
Dim Folder As New IO.DirectoryInfo(oTemplateFolder)
For Each File As IO.FileInfo In Folder.GetFiles("*.idw", IO.SearchOption.AllDirectories)
Dim sName As New FileInfo(File.Name)
oList.Add(sName.Name)
Next
oTemplate = InputListBox("Select a template", oList, oList(0), "iLogic", "List")
oTemplate = oTemplateFolder & oTemplate
Logger.Info(oTemplate)
Dim oDrawingDoc As DrawingDocument
oDrawingDoc = ThisApplication.Documents.Add _
(DocumentTypeEnum.kDrawingDocumentObject, oTemplate, True)
oDrawingDoc.Activate()
Dim oSheet As Sheet
oSheet = oDrawingDoc.Sheets.Item(1)
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(10, 10)
Dim oView As DrawingView
oView = oSheet.DrawingViews.AddBaseView(oDoc, oPoint, 1, _
ViewOrientationTypeEnum.kFrontViewOrientation, _
DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle)
