Looping through Sub Assemblies and turning off visibility.
Hi @ahmed.hagi. First thing I see that does not look right is you use of the keyword "Nothing". When comparing against Nothing you should use 'Is' or 'IsNot', not '=' or '<>'. If the variable were declared as a String, instead of no Type declaration, you could try String.IsNullOrEmpty(SAPVal) or just If SAPVal = "", but if it is a Double, Integer, or other numeric data type, there is no comparison with Nothing, it will just have the value of zero, and Boolean's will always be False by default after creation. Also, you could try checking refDoc.DocumentType property to see if it is an assembly first, before trying to assign it to an AssemblyDocument type variable, then use a smaller Try block of code, for more accurate/useful error handling feedback. I don't know what your oData, oDataM, or estr variables represent, but I assume the first two are Dictionary types, and the third something like a List(Of String), but it's difficult to debug without seeing more. Are you wanting this routine to process down into sub assemblies, or just top level components in your main assembly?
Wesley Crihfield
(Not an Autodesk Employee)
Hi @ahmed.hagi ,
There was a lot in that try/catch, which makes it difficult to troubleshoot because once it hits one error, it quits.
Here is an example that breaks it up a bit.
The exception that I was seeing in my data set was the one that happened when the first part component was encountered and the code attempted to set it as a Assembly Document, so changing that to Document helped.
Note that as it was written it only looked at components ( parts and subassemblies) that occurred in the top level assembly. That is to say it was not looking at subcomponents found in the subassemblies.
This example traverses the entire assembly, looking down into each sub assembly.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Sub main Dim oDoc As AssemblyDocument oDoc = ThisApplication.ActiveDocument Dim assemblyDef As AssemblyComponentDefinition assemblyDef = oDoc.ComponentDefinition Dim oOccs As ComponentOccurrences = oDoc.ComponentDefinition.Occurrences Call TraverseAssembly(oOccs) End Sub Function TraverseAssembly(oOccs As ComponentOccurrences) oData = "Test2" 'dummy data since original example was incomplete oDataM = "Test2" 'dummy data since original example was incomplete Dim estr As New ArrayList 'dummy data since original example was incomplete Dim oOcc As ComponentOccurrence For Each oOcc In oOccs Dim refDoc As Document refDoc = oOcc.Definition.Document Dim customPropSet = refDoc.PropertySets.Item("Design Tracking Properties") Dim SAPProp = customPropSet.Item("Stock Number") Dim SAPVal = SAPProp.Value 'msgbox(SAPVal) Try If SAPVal <> Nothing And IsNumeric(SAPVal) Then If (oData.ContainsKey(SAPVal) And oDataM.ContainsKey(SAPVal)) Then If (oData(SAPVal) = oDataM(SAPVal)) Then oOcc.Visible = False Else oOcc.Visible = True estr.Add(CStr(SAPVal) & ": " & oData(SAPVal) & " <> " & oDataM(SAPVal)) End If End If End If Catch Ex As Exception 'MsgBox(Ex.Message) End Try sName = Split(oOcc.Name, ":") sName = sName(0) If oOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then Call TraverseAssembly(refDoc.ComponentDefinition.Occurrences) End If Next End Function
This line uses an iLogic dependent object 'InventorVb', so it should be changed to get/reference the Inventor.Application object another way.
InventorVb.Application.CreateFileDialog(oFileDlg)
Maybe something like this:
Dim InvApp As Inventor.Application = GetObject(,"Inventor.Application")
InvApp.CreateFileDialog(oFileDlg)
Where that variable to represent the Inventor.Application object is at the top of your code.
Also keep in mind that the iLogic rule editor environment already has references to several resources included for us, so that we do not need to have really long 'header' codes in each of our iLogic rules (such as AddReference & Imports lines). And it also creates the 'ThisRule' Class for us, and creates several variables for us that represent Interface type objects within that class that are ready for us to use, without needing to instantiate them. This is all to make life easier for less experienced coders to get into design automation.
And since 'ThisDoc' is also unique to iLogic, the following line would also not work outside of the influence of an iLogic rule, unless you recreated it:
Dim assemblyDef As AssemblyComponentDefinition = ThisDoc.Document.ComponentDefinition
...it seems to me like you could use this instead:
Dim assemblyDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition
The term 'ThisDoc' is another one of those super useful/helpful/dynamic variables created for us in iLogic rules that represents an Interface, and since we do not have access to its source code, the closest API object might be the ThisApplication.ActiveEditDocument.
Same for these two lines:
oWrite = System.IO.File.CreateText(ThisDoc.PathAndFileName(False) & ".txt")ThisDoc.Launch(ThisDoc.PathAndFileName(False) & ".txt")
...in both cases, you could create a variable to use for the needed full file name, with the ".txt" file extension, like the following:
Dim oAsmTxtFile As String = System.IO.Path.ChangeExtension(oAsmDoc.FullFileName, ".txt")
...then use that variable instead of the 'ThisDoc.PathAndFileName()'. Below is an example:
oWrite = System.IO.File.CreateText(oAsmTxtFile)
Since all that 'ThisDoc.Launch() line does is visibly open the file, there are other ways of doing that with vb.net. Perhaps the simplest would be something like this:
Process.Start(oAsmTxtFile)
Wesley Crihfield
(Not an Autodesk Employee)
These two lines will not work:
Dim oWrite = System.IO.File.CreateText(oAsmDoc.PathAndFileName(False) & ".txt")oAsmDoc.Launch(oAsmDoc.PathAndFileName(False) & ".txt")
Because 'PathAndFileName() is a method of the 'ThisDoc' object, not a method of a regular Inventor.Document. If you want to get the full path and file name of an Inventor document, with a different file extension, you can use the line of code I posted in my previous response, as follows:
Dim oAsmTxtFile As String = System.IO.Path.ChangeExtension(oAsmDoc.FullFileName, ".txt")
This would be on its own line just before you get to those other two lines mentioned. Then just use that 'oAsmTextFile' variable as the 'input' into that 'CreateText()' method, or to specify which file to open after it has been created.
oAsmDoc.Launch will not work either, because 'Launch()' is a method of the 'ThisDoc' object, not a method of the regular Inventor.Document type object, and the ThisDoc type object can not be used outside of iLogic. As I mentioned in my previous response, you can use the Process.Start() method in vb.net to open & show that text file after it has been created, instead of the 'ThisDoc.Launch() method, then supply the oAsmTxtFile variable as its 'input'.
Wesley Crihfield
(Not an Autodesk Employee)
You may need to change the following line of code:
Call TraverseAssembly(refDoc.ComponentDefinition.Occurrences)...to the following:
TraverseAssembly(oOcc.SubOccurrences)The 'Call' keywork is used in VBA, but not needed in vb.net or iLogic rules. And there are multiple ways to recursively iterate through component occurrences in an assembly, and how you do so can change how it works. When going down through the 'definitions' of the documents that the components are referencing to get to their child occurrences, you are pretty much guaranteed to be effecting those referenced documents directly, so the changes you make will be made within those referenced documents. But if you go through the ComponentOccurrence.SubOccurrences property, you maintain the 'lineage' with the main/top assembly, so changes will essentially be made to proxies within the main/top assembly. This does not necessarily guarantee that all possible types of changes will not effect any referenced documents, but is the better route if that is what you are trying to achieve.
Changing this one thing may not fix your current problem, but it may help some, if it suits your design intent.
Wesley Crihfield
(Not an Autodesk Employee)
