Is it possible to edit iProperties in suppressed parts?
Hi @Lars_Greft. No, you can not do much at all with a suppressed assembly component, other than check the component's name. If you need to read or write to the iProperties of the document which that component represents, you may have to access that document directly through the main assembly's ReferencedDocuments (top level document references only), or its AllReferencedDocuments (all document references from all levels of the assembly), instead of through the component. To do so, you could loop through each oRefDoc As Document In ThisAssembly.AllReferencedDocuments, for example, then use the oRefDoc variable's properties to access its iProperties.
You can either get to its iProperties using API route:
oRefDoc.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value
or extract the document's file name (without path, but with file extension) to use as the first input variable in the iProperties.Value(docName, setName, propname) method.
Wesley Crihfield
(Not an Autodesk Employee)
Sure. I see two things that may be causing problems. The first thing is using that exact term 'ThisAssembly', which is already being used by iLogic in the background. That is a term used to represent an iManagedAssembly object (Interface), so I would advise you to use a different term there for your variable name. Next, I don't think the referenced document that you area writing the iProperty data to is getting updated or saved after the edit, so the edit may not be staying. I modified your code a bit to help remedy these things. Give this version a try.
Dim oADoc As AssemblyDocument = ThisDoc.Document
For Each oRefDoc As Document In oADoc.ReferencedDocuments
If oRefDoc.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value <> "Test" Then
oRefDoc.PropertySets.Item("Inventor Summary Information").Item("Keywords").Value = "Test"
End If
If oRefDoc.RequiresUpdate Then oRefDoc.Update2(True)
If oRefDoc.Dirty Then oRefDoc.Save2(False)
Next
oADoc.UpdateWesley Crihfield
(Not an Autodesk Employee)
In the case of that post, the main method would look like this. (with save and close)
Sub Main()
Dim doc As AssemblyDocument = ThisDoc.Document
Dim refDocNames As List(Of String) = getRefDocList(doc)
For Each refDocName As String In refDocNames
Dim refDoc As Document = getDocument(refDocName)
' Do the work on your document here
MsgBox(refDoc.DisplayName)
refDoc.Save() ' <-- look here
refDoc.Close(True) ' <-- look here
Next
End Sub
Jelte de Jong
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Hi @Lars_Greft. One thing that comes to mind when I see the two terms you are wanting to write to these documents is the BOMStructure property of the AssemblyComponentDefinition, PartComponentDefinition, ComponentDefinition, and the ComponentOccurrence objects, which uses the BOMStructureEnum variations as its value. Many folks use that for setting whether the model is to be used for 'Normal' purposes, 'Reference', 'Purchased', 'Phantom', 'Inseperable', and such. The BOM also uses that value when determining some things, so it can be very useful to take advantage of, if you are not already. Manually, within a model type document, you can open the Document Settings (on the Tools tab > Options panel), and the 'Bill of Materials' tab within that dialog to set its value.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @wfajber. Good point. That's mainly what I have pretty much always done. I knew that the 'level of detail' representations (before ModelStates) were originally created with performance issues in mind, because they primarily record which components in an assembly are suppressed, and suppressing components 'unloads' them from Inventor's session memory, which increases performance. However, many over the years have adopted the use of suppressing components as a means of controlling BOM quantities. After some initial dabbling/testing with that process, and finding out how restrictive their use was to many of my other processes, I have chosen since then to use 'design view representations', component visibility, and the BOMStructure to help control BOM/PartsList related issues, which has worked just fine for me. However, our assembly BOM's are not directly exported/translated into any sort of ERP system (at this time), and we make more use of drawing PartsLists than we do of the assembly's BOM directly. Plus we use a lot of automation tools, where others may not. So I certainly do not fault or discourage any specific way of doing things, because there are a vast array of needs and scenarios out there that require all sorts of different solutions.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @Lars_Greft. I do not have Vault yet, though we have talked about it several times, and may be getting it soon. I wander though what would happen in situations were your assembly may have multiple instances of components that represent the same source document, when 1 or more of them may be suppressed, and 1 or more of them may not be suppressed. If you are writing one of those terms to the document, wouldn't that info be incorrect or misleading? I don't know, just a thought that popped into my mind. One fairly new thing that comes to mind is the 'instance properties', which allows you to set custom iProperty values to each instance of a component in an assembly, even if they represent the same base document. But I don't know if Vault can work with those 'instance' properties, so I don't know if their use would help or not.
Wesley Crihfield
(Not an Autodesk Employee)
