"Where used" info on drawings
Hello,
The main reason for this is that we used linked drawings using PDF readers that scan for drawings numbers. So for assembly drawings with the BOM we are able to click on the drawing number and the part PDF will open. And I would like for us to be able to use it also the other way around.
If you open a partdrawing (PDF) you will get information on what assembly this part belongs to, and click on the drawing number and the assembly will open. The links between the files are solved, so information on the part drawings with dwg number of assemblies is the thing I am missing.
To answer you question: Perferably i would like the information of the usage of Part1 will be updated. (in the best of worlds)
I hope i make myself understandable.
But i mean, the info is there both in the Design Manager and the Vault.
Isnt there a way to extract this information and use it to put on drawings?
Or like scan the assemblies in the same folder as the part for occurenceses and get the paramaeter "Part number" or something like that using Ilogic?
I tried to do a simple sketch of 2 Assembles both containing the same part.
Best Regards
Alexander
Hi @alexander.duell. I don't currently know how to extract that information from Design Assistant or Vault by code (I am not currently using Vault either), but I could definitely envision an iLogic rule that could scan a directory for assemblies, then check if each assembly has a reference to a specific part, then return those assembly part numbers. Of course this type of thing may not be ideal, and may take a while to process (bogging down Inventor while it runs), depending on how many files it will be scanning through, but sounds doable. I have created solutions before using an iLogic rule that would process all files of a certain type (and other possible filters) within a directory to work with things like iProperties, etc. Does that sound like something you would want to try then? Should we assume that the drawing document for the part will be open and the 'active' document when the rule starts? The bulk of the code for this task could be put into a Function of its own too, so it could then be referenced or called by another larger code, if needed.
Wesley Crihfield
(Not an Autodesk Employee)
OK. I just created this iLogic rule for you to try. I tested this myself first, on a folder with about 115 items in it (some folders, and some other types of files), and I have it set to only search within the same folder where the drawing's model document is saved. My test returned 4 part numbers of assemblies that were referencing the model in the active drawing, then it put a drawing note at the origin point of the active drawing sheet, as expected. Give this a try, and see how it works for you. If other changes may need to be made, we may be able to deal with that later.
Sub Main
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("A Drawing Document must be active for this rule to work. Exiting.", vbCritical, "iLogic")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisApplication.ActiveDocument
Dim oMDoc As Document = GetDrawingModel(oDDoc)
If IsNothing(oMDoc) Then
MsgBox("No 'Model' document found in Drawing. Exiting rule.", vbCritical, "iLogic")
Exit Sub
End If
Dim oPNsRefdBy As List(Of String) = GetWhereUsed(oMDoc)
If oPNsRefdBy.Count = 0 Then
MsgBox("No assemblies found with reference to the 'Model' document.", vbInformation, "iLogic")
Exit Sub
End If
Dim oReport As String = "USED IN: "
For Each oPNRefdBy In oPNsRefdBy
oReport = oReport & vbCrLf & oPNRefdBy
Next
oPos = ThisApplication.TransientGeometry.CreatePoint2d(0,0)
Dim oNote As GeneralNote = oDDoc.ActiveSheet.DrawingNotes.GeneralNotes.AddFitted(oPos, oReport)
End Sub
Function GetDrawingModel(oDrawing As DrawingDocument) As Document
If oDrawing.AllReferencedDocuments.Count = 0 Then Return Nothing
For Each oRefDoc As Document In oDrawing.AllReferencedDocuments
If oRefDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Or _
oRefDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Return oRefDoc
Exit For
End If
Next
'just in case there were referenced documents,
'but none were a Part or Assembly (very rare)
Return Nothing
End Function
Function GetWhereUsed(oDoc As Document) As List(Of String)
Dim oPNs As New List(Of String)
'get the folder where the input document is currently saved
oPath = System.IO.Path.GetDirectoryName(oDoc.FullFileName)
'search within that folder for assemblies that reference the input document
Dim oFileNames() As String = System.IO.Directory.GetFiles(oPath, "*.iam", System.IO.SearchOption.TopDirectoryOnly)
'if no assemblies were found, were done here
If oFileNames.Length = 0 Then
'MsgBox("No assemblies found.",,"")
Return oFileNames.ToList 'returns an empty List
End If
For Each oFileName In oFileNames
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
oOptions.Add("ExpressModeBehavior", "OpenExpress")
oOptions.Add("SkipAllUnresolvedFiles", True)
Dim oADoc As AssemblyDocument = ThisApplication.Documents.OpenWithOptions(oFileName, oOptions, False)
If oADoc.AllReferencedDocuments.Count > 0 Then
For Each oRefDoc As Document In oADoc.AllReferencedDocuments
If oRefDoc.FullFileName = oDoc.FullFileName Then
Dim oPN As String = String.Empty 'just a cautionary reset
oPN = oADoc.PropertySets.Item(3).Item("Part Number").Value
If String.IsNullOrEmpty(oPN) Then oPN = ""
oPNs.Add(oPN)
Exit For 'exit the loop of oRefDoc's
End If
Next
End If
oADoc.ReleaseReference
Next
ThisApplication.Documents.CloseAll(True) 'close all 'unreferenced' documents only
Return oPNs
End FunctionIf this solved your problem, or answered your question, please click ACCEPT SOLUTION.
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Wesley Crihfield
(Not an Autodesk Employee)
OK. I can tell from the second part of the error message that it is not liking the Documents.OpenWithOptions code I'm using to open the assembly documents within the 'GetWhereUsed' function. That method has been around since 'version 11', according to its online help page, but I do know for a fact that the listed available 'Options' shown on that page have changed over the years. You can review that online help page for yourself if you want. The one option I'm using (ExpressModeBehavior) is specifically for when attempting to open an Assembly only. The other option I'm using (SkipAllUnresolvedFiles) says it can be used for when opening any document type. So I'm not sure why they would be causing any problems. The oFileName variable I'm using as the first input variable should contain the 'FullFileName' of the assembly file (as found in the file system). You could try replacing those 4 lines of code with a simple Documents.Open() method instead, and see if that works better for you.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @alexander.duell. I'm not sure if this will fix the error you were having with my first code, but I modified the code to use a regular Documents.Open() line to open the assembly files, instead of the Documents.OpenWithOptions() line, because that is what the error seemed to be pointing to at the time. This code still works for me, but see if this works any better for you.
Sub Main
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("A Drawing Document must be active for this rule to work. Exiting.", vbCritical, "iLogic")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisApplication.ActiveDocument
Dim oMDoc As Document = GetDrawingModel(oDDoc)
If IsNothing(oMDoc) Then
MsgBox("No 'Model' document found in Drawing. Exiting rule.", vbCritical, "iLogic")
Exit Sub
End If
Dim oPNsRefdBy As List(Of String) = GetWhereUsed(oMDoc)
If oPNsRefdBy.Count = 0 Then
MsgBox("No assemblies found with reference to the 'Model' document.", vbInformation, "iLogic")
Exit Sub
End If
Dim oReport As String = "USED IN: "
For Each oPNRefdBy In oPNsRefdBy
oReport = oReport & vbCrLf & oPNRefdBy
Next
oPos = ThisApplication.TransientGeometry.CreatePoint2d(0,0)
Dim oNote As GeneralNote = oDDoc.ActiveSheet.DrawingNotes.GeneralNotes.AddFitted(oPos, oReport)
End Sub
Function GetDrawingModel(oDrawing As DrawingDocument) As Document
If oDrawing.AllReferencedDocuments.Count = 0 Then Return Nothing
For Each oRefDoc As Document In oDrawing.AllReferencedDocuments
If oRefDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Or _
oRefDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Return oRefDoc
Exit For
End If
Next
'just in case there were referenced documents,
'but none were a Part or Assembly (very rare)
Return Nothing
End Function
Function GetWhereUsed(oDoc As Document) As List(Of String)
Dim oPNs As New List(Of String)
'get the folder where the input document is currently saved
oPath = System.IO.Path.GetDirectoryName(oDoc.FullFileName)
'search within that folder for assemblies that reference the input document
Dim oFileNames() As String = System.IO.Directory.GetFiles(oPath, "*.iam", System.IO.SearchOption.TopDirectoryOnly)
'if no assemblies were found, were done here
If oFileNames.Length = 0 Then
'MsgBox("No assemblies found.",,"")
Return oFileNames.ToList 'returns an empty List
End If
For Each oFileName In oFileNames
Dim oADoc As AssemblyDocument = ThisApplication.Documents.Open(oFileName, False)
If oADoc.AllReferencedDocuments.Count > 0 Then
For Each oRefDoc As Document In oADoc.AllReferencedDocuments
If oRefDoc.FullFileName = oDoc.FullFileName Then
Dim oPN As String = String.Empty 'just a cautionary reset
oPN = oADoc.PropertySets.Item(3).Item("Part Number").Value
If String.IsNullOrEmpty(oPN) Then oPN = ""
oPNs.Add(oPN)
Exit For 'exit the loop of oRefDoc's
End If
Next
End If
oADoc.ReleaseReference
Next
ThisApplication.Documents.CloseAll(True) 'close all 'unreferenced' documents only
Return oPNs
End FunctionI also sympathize with @pball here, because I may be in that same position soon. Because we too may be starting to use Vault in the near future, and I'm very apprehensive about it. I don't know hardly anything about coding for Vault right now, and I'm worried about the many hundreds (if not thousands) of iLogic rules (and VBA macros, and fully automated configuration templates) I already have, and if they may become practically useless after the change. And the 'where used' functionality was the first/main attraction for us, because many of our parts are used in many places, and those other places may often need to be updated (of fixed) after certain changes to parts.
Wesley Crihfield
(Not an Autodesk Employee)
