Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
One of our guys on staff tweaked a pretty slick piece of iLogic code to duplicate sheets. We are a curtainwall manufacturer. So we tend to duplicate a lot of sheets where our 3D frames will be identical, but differ just by notes on the drawings for glass types and such. Code starts with your selected sheet, then a window opens for you to select the same model from the sheet you want to duplicate. After selecting, the sheet dupes and keeps all existing annotations. At it's core, I think it is just doing a Replace Model Reference to create the dupe. Good luck!
Sub Main()
'Set Number of Addresses for Unit in Overall Assembly
Dim NumberOfUnits = 1
'Check that we are in a drawing document.
If ThisDoc.Document.DocumentType = DocumentTypeEnum.kDrawingDocumentObject Then
'Get a reference to the current drawing.
Dim dwgDoc As DrawingDocument = ThisDoc.Document
'Check that we have atleast one view on the sheet.
If dwgDoc.ActiveSheet.DrawingViews.Count > 0 Then
'Get a reference to the original model in the view.
Dim compDoc As Document = dwgDoc.ActiveSheet.DrawingViews(1).ReferencedDocumentDescriptor.ReferencedDocument
'Get the filename of the replacement model
Dim newFileName As String = GetNewReference() 'Sub to show dialog and get file name.
'Open the replacement model.
Dim newFile As Document
If Not String.IsNullOrEmpty(newFileName) Then
'If Not String.IsNullOrEmpty(compDoc) Then
Try
newFile = ThisApplication.Documents.Open(newFileName, False)
'newFile = ThisApplication.Documents.Open(compDoc, False)
Catch
MessageBox.Show("Could not open target file.")
End Try
'Check to see if we have valid documents to work with.
If Not newFile Is Nothing Then
Dim okContinue As Boolean = True
If Not newFile.InternalName = compDoc.InternalName Then
'Display warning if inner names of models do not match.
msgResult = MessageBox.Show("Warning, files do not match." & vbCrLf & " Results can be unpredictable." & vbCrLf & _
"Do you want To Continue", "Copy/Replace Sheet", MessageBoxButtons.YesNo)
If Not msgResult = DialogResult.Yes Then
okContinue = False
End If
End If
If okContinue Then
Dim newDwg As DrawingDocument
Try
'Create the new drawing document.
newDwg = ThisApplication.Documents.Add(kDrawingDocumentObject, Nothing, False)
'Copy the active sheet to the new document.
Dim newSheet As Sheet = dwgDoc.ActiveSheet.CopyTo(newDwg)
'Replace the model reference on the new sheet with the replacement reference
newSheet.DrawingViews(1).ReferencedDocumentDescriptor. _
ReferencedFileDescriptor.ReplaceReference(newFileName)
' 'rename Active Sheet to Unit Address
' dwgDoc.ActiveSheet.Name = InputBox("Enter Unit Address", "Unit Address")
' UpdateUnitAddress()
Dim i As Long = 0
For i = 1 To NumberOfUnits
'Copy the sheet back to the original drawing.
Dim copiedSheet As Sheet = newSheet.CopyTo(dwgDoc)
' copiedSheet.Name = InputBox("Enter Unit Address", "Unit Address")
copiedSheet.Activate()
' UpdateUnitAddress()
Next
newDwg.Close(True)
'Activate the new sheet.
'copiedSheet.Activate()
InventorVb.DocumentUpdate()
Catch
MessageBox.Show("Error occurred copying sheet.")
End Try
End If
End If
End If
End If
End If
' iLogicVb.RunRule("ResetSectionViewCallout_Rule")
End Sub
'Function UpdateUnitAddress() As String
' Dim dwgDoc As DrawingDocument = ThisDoc.Document
' Dim oPromptEntry
' Dim actSheet As Sheet = ThisApplication.ActiveDocument.ActiveSheet
' ActiveSheet = ThisDrawing.Sheet(actSheet.Name)
' oTitleBlock=actSheet.TitleBlock
' oTextBoxes=oTitleBlock.Definition.Sketch.TextBoxes
' For Each oTextBox In oTitleBlock.Definition.Sketch.TextBoxes
' Select oTextBox.Text
' Case "<Unit Address>":
' oPromptEntry = dwgDoc.ActiveSheet.Name
' Dim sSplit As String() = oPromptEntry.Split(New Char() {":"c})
' 'get the first member of array
' oPromptEntry = sSplit(0)
' Call oTitleBlock.SetPromptResultText(oTextBox, oPromptEntry)
' 'MessageBox.Show("Phase2.")
' End Select
' Next
' InventorVb.DocumentUpdate()
'End Function
Function GetNewReference() As String
' Create a new FileDialog object.
Dim oFileDlg As Inventor.FileDialog
Call ThisApplication.CreateFileDialog(oFileDlg)
' Define the filter to select part and assembly files or any file.
oFileDlg.Filter = "Inventor Files (*.iam;*.ipt)|*.iam;*.ipt|All Files (*.*)|*.*"
' Define the part and assembly files filter to be the default filter.
oFileDlg.FilterIndex = 1
' Set the title for the dialog.
oFileDlg.DialogTitle = "Copy/Replace Sheet - Select Replacement Model"
' Set the initial directory that will be displayed in the dialog.
oFileDlg.InitialDirectory = ThisDoc.Path
' Set the flag so an error will be raised if the user clicks the Cancel button.
oFileDlg.CancelError = True
' Show the open dialog. The same procedure is also used for the Save dialog.
' The commented code can be used for the Save dialog.
Try
oFileDlg.ShowOpen
Catch
'MessageBox.Show("User cancelled out of dialog", "Replace Reference")
Finally
If Not oFileDlg.FileName = "" Then
'MessageBox.Show("File " & oFileDlg.FileName & " was selected.", "Replace Reference")
GetNewReference = oFileDlg.FileName
End If
End Try
End Function
Sorry can't mention names for the Kudos. He said he found the code posted somewhere, and just modified it for our assemblies. So if any of this code looks like your handiwork...post your name and I'll give the KUDOS!!! Great time-saver for us.
There are situations where you need a complete sheet with all views again, e.g. to create a different dimensioning or labeling for another manufacturing process. Unfortunately this is not possible in the current version. You have to create the views again on a new sheet.
Software like, oh - Coreldraw does this (and had since, um - it's inception.) But our high-end mechanical design software can't. Hmmm. One of those "two steps forward, one step back" Inventor things I guess.
Oh, and "copy, open another sheet, paste, copy, paste" is a workaround. A laughable, time-consuming workaround.@jason_bush , thanks for posting the iLogic here - will definitely give it a try. Our industry has the same challenges with similar (or identical) notes on multiple sheets.
I would like to be able to copy and paste a sheet within the same drawing, rather than needing to open a separate drawing to copy to, then to copy from that new drawing back to the original. When i first realized this i assumed it was a bug but then the problem persisted for years
Sub IDW_DuplicateSheet()
Dim oDoc As DrawingDocument
Set oDoc = ThisApplication.ActiveDocument
Dim tmpDoc As DrawingDocument
Set tmpDoc = ThisApplication.Documents.Add(kDrawingDocumentObject, , True)
Dim newSheet As Sheet
Set newSheet = oDoc.ActiveSheet.CopyTo(tmpDoc)
Call newSheet.CopyTo(oDoc)
tmpDoc.Close (True)
End Sub
This idea has been implemented within Autodesk Inventor 2021.2. You can now copy a drawing sheet into the same drawing. A right click contextual copy & paste operation, as well as Ctrl+C & Ctrl+V shortcut operations, are both supported. Special thanks to everyone who cast a vote for it.
