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Good point about the DVR name.
There is also another area in the early portion of the code that seemed a little risky also.
In Lines 18 through Line 30...
You create a variable for the DocumentDescriptor before the loop of all views, and set its value once per view within that loop. If every view is not referencing the main assembly directly, then that could cause problems later in your code (starting at Lines 29 & 30, onwards). Maybe just set its value once, using the first view on the sheet, instead of for every view, but not sure about how you do your drawings. That variable will retain the last value assigned to it within that loop.
Then at Line 29, you should declare your Document variable first, then set that with DocumentDescriptor.ReferencedDocument. Then on Line 30, declare its ComponentDefinition, then set that with Document.ComponentDefinition. The ReferencedDocument property returns an Object, so it is always good to have an already declared Document type variable to capture its value, then go from there. Just good practice, and order of operations.
Wesley Crihfield
(Not an Autodesk Employee)
I have updated that section of code to this...
Dim oDocDesc As DocumentDescriptor = oDwgViews.Item(1).ReferencedDocumentDescriptor
'Cycle through all the drawing views to check if each is of an assembly.
For Each oDwgView In oDwgViews
'Verify that the selected drawing view is of an assembly.
If oDwgView.ReferencedDocumentDescriptor.ReferencedDocumentType <> kAssemblyDocumentObject Then
MessageBox.Show("All views must be of an assembly.")
Exit Sub
End If
'Verify that the selected drawing view is of an assembly.
If oDwgView.ReferencedDocumentDescriptor IsNot oDocDesc Then
MessageBox.Show("All views must be of the same assembly")
Exit Sub
End If
Next
'Get the component definition for the assembly.
Dim oAsmCompDef As AssemblyComponentDefinition = oDocDesc.ReferencedDocument.ComponentDefinition
Dim oAsm As AssemblyDocument = oAsmCompDef.Parent
Since the rest of the script acts on only one single Component Definition, I made sure that it is the definition of the first view, and that only that assembly is referenced in any view. I did also change the name assignment.
If oDesRep = "" Then
oDesRep = "[Primary]"
End If
I also noticed that the original code is looking for oDwgView.ActiveDesignViewRepresentation which does not appear to be a property of DrawingView (anymore?) so I changed that line to
oDesRep = oDwgView.DesignViewRepresentation
But I have the same issue.
In my code (extra comments everywhere) Line 130 is
oRep.Activate
I thought originally that this might be due to there being 2 DVRs (1 "hidden?" kTransientDesignViewType) that has the same name "[Primary]" and it having trouble assigning oRep with
oRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item(oDesRep)
But I am no longer sure about that. There are no other DVRs present and even if I create am additional one, I have the same issue.
Hi @tfrohe_LSI. Try capturing the DVR's collection to a variable. Then use that variable like...
oDVRs.Item("DVRName").Activate
...instead of...
oRep.Activate
...That way you are working with its name, instead of the object itself. Avoids the 'transient' thing that way.
Edit: You may also want to capture the RepresentationsManager object itself to a variable also, ahead of time, that way you can just use something like:
oRepsMgr.ActiveDesignViewRepresentation
(shorter line of code to get to / check that property later). Just suggestions.
Wesley Crihfield
(Not an Autodesk Employee)
I've updated the code to
'oRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item(oDesRep)
Dim oReps As DesignViewRepresentations = oAsmCompDef.RepresentationsManager.DesignViewRepresentations
if not (oAsmCompDef.RepresentationsManager.ActiveDesignViewRepresentation.Name = oDesRep) Then oReps.Item(oDesRep).Activateand get the same error
It does work if the view is DVR [Primary]. if the first view is anything else, it fails to activate the DVR. If a second view is of another DVR, it fails when it gets to that view.
Hi @tfrohe_LSI. One possibly out there thought that comes to mind is that maybe your assembly, if it is a regular one (not an iAssembly), may have more than its one original/default ModelState in it (named "[Primary]"). If so, then it may be possible that at times you are encountering a ModelState member version of the assembly. If that is the case, then it would act like a ReadOnly document. You would be able to browse through it just fine, but when you try to change something in it, such as activating a different DVR, it will throw an error. If so, there are ways around this, but the code starts getting more complicated. When any model file (part or assembly) has 2 or more ModelStates in it, then there will be one 'factory' document, and at least one 'member' document. The factory is simply the document that is associated with whichever ModelState happens to be 'active' at that time. Then the member documents will be the ones associated with any other ModelStates that are not currently 'active'. The factory version will be fully Read/Write, while the member versions will act like ReadOnly. The exception to this behavior is when you have the 'member edit scope' set to factory scope or all members scope, instead of active member only scope. Or, when editing the ModelStateTable, which contains all of them in one table.
In situations where we are working on a document directly (it is the one actively visible on our screen), and we want our code to be acting upon that document (not some other document referenced within it), it can often be easy to automatically be working with the 'factory' version, but it is not guaranteed. We do have an iLogic snippet for making sure we start out working with the factory document (ThisDoc.FactoryDocument), which is OK for at the start of a rule, but is not always ideal to use down in the middle of a rule. In the middle of a rule that may be iterating through multiple ModelStates, or referenced documents, there are other ways to either get a reference to the factory version document, or force the member version you have a reference for to become the factory version, by activating the ModelState that it is associated with. Also sometimes when moving from one referenced document to another where multiple ModelStates may be involved, we sometimes need to update the referenced document before we can work with it, if we previously made changes to another ModelState version of that same file. I know, it can be a lot to learn and account for.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @tfrohe_LSI. What @Frederick_Law just mentioned is very true. If starting from a drawing, and you only need to change the drawing view(s) to show a different DVR version of the same assembly it is already referencing, then you can just change the view itself to a different DVR directly. Same goes for ModelStates...if the drawing view is set to one ModelState, but you want it to be set to a different ModelState, then there is a built-in method for that also.
DrawingView.ActiveModelState (ReadOnly String)
DrawingView.SetActiveModelState (Sub routine)
And if you need to change both the ModelState of the view, and the DVR of the view, then you should always change its ModelState first, then its DVR second.
However, when starting from the assembly itself (it is showing on your screen when you start the code), and that assembly has 2 or more ModelStates in it, and you want to make sure you are working with the factory version, then there are a few options. If in an iLogic rule, I would recommend using the 'ThisDoc.FactoryDocument' property to obtain your original reference to that assembly's factory document. If elsewhere (in VBA macro or an add-in), then the 'ThisDoc' term will not be recognized. So go ahead and use the 'ThisApplication.ActiveDocument' phrase, but then we will use additional lines of code to make sure we have the factory document. Within the AssemblyComponentDefinition we have a couple properties we can use for this.
AssemblyComponentDefinition.IsModelStateMember (ReadOnly Boolean)
AssemblyComponentDefinition.IsModelStateFactory (ReadOnly Boolean)
AssemblyComponentDefinition.FactoryDocument (ReadOnly, returns Document object, but might not return anything if there are not 2 or more ModelStates present.
We can use these like this:
If oADoc.ComponentDefinition.IsModelStateMember = True Then
oADoc = oADoc.ComponentDefinition.FactoryDocument
End If...to reset the value of our initial AssemblyDocument variable to the new value, so that it will now represent the factory document. Or, you could declare a different variable before this block of code, like oFactoryDoc, then set its value within that block of code. If super curious, you can even compare the initial variable with the new variable afterwards, using 'Is' comparison (not =).
Another think to be aware of when ModelStates are involved is the Document.FullDocumentName property. Sometimes, when multiple ModelStates are involved, this property's value will start with the FullFileName value, but then immediately after the file extension will be something like "<ModelStateMemberName>", which tells us which version we are working with. The "ModelStateMemberName" portion will be the real name of the ModelState, not just that text shown here. There are also ways to separate the FullFileName portion from the ModelState member name portion, using FileManager.GetFullFileName method and FileManager.GetModelStateName method. Then there is this one: FileManager.GetLastActiveModelState. And when iterating through referenced documents, you can use the ThisApplication.Documents.Open() method, where you specify the FullDocumentName, and capture the Document object it returns to your variable, to use later, and it will ensure you are working with the factory document (if there is one). Just some additional tips for the road ahead.
Wesley Crihfield
(Not an Autodesk Employee)
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