Retrieve part name within drawing
There are multiple ways to get access to the 'model' document being represented within a drawing document. If you are using a 'local' (saved within the document) iLogic rule, you can use this route:
ThisDrawing.ModelDocument
The following two references can be used in either a local or external rule (where you've already defined the oDDoc variable as the 'active' drawing document.):
The following line assumes that the first drawing view in your drawing is representing the model document you are targeting.
oDDoc.ActiveSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
This next line simply assumes that the first document being referenced by your drawing is the model document.
oDDoc.ReferencedDocuments.Item(1)
After you have reached that document, you may have to assign the generic document object as the value of a PartDocument type Variable, so that you can access its PartComponentDefinition. The MassProperties are located under that component definition.
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Wesley Crihfield
(Not an Autodesk Employee)
I was attempting to help you achieve your second goal of working with the Mass of the part document. Only assembly documents and part documents have mass, so in order to get to that mass, you have to create a PardDocument type of variable, then set the 'model document' you retried through the lines of code above as the value of this new variable, so that this new variable will be representing that part document. Once you have done this, you will then have access to all the stuff (properties, objects within, functionality) specific to that part document, through this new variable.
'create a variable for a drawing document, then set its value
Dim oDDoc As DrawingDocument = ThisDrawing.Document
'that variable now represents our local drawing document
'check if the model document this drawing is representing is a Part (specificly)
If ThisDrawing.ModelDocument.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
'it is, so create a Part specific document variable, then set its value
Dim oPDoc As PartDocument = ThisDrawing.ModelDocument
'that variable now represents that part document
'create a String (text) type variable, to hold the part's name, then set its value
Dim oName As String = oPDoc.FullFileName
'that variable now represents that text
'create a Double (number with decimal places) type variable, then set its value
'had to climb down through the object structure under that Part to get it
Dim oMass As Double = oPDoc.ComponentDefinition.MassProperties.Mass
'that variable now represents the Mass of the part
'show the user (you) a message containing the data we collected about the part.
MsgBox("Model name = " & oName & vbCrLf & _
"Model Mass = " & oMass, , "")
End If
In iLogic, everything is structured by objects. Documents are one of the objects that are high in the structure. Each object may have a certain set of properties (data, settings, other objects), methods (actions you can do with/to this object), and events (notifications of when stuff happens to this object). There are multiple types of document objects. There is a generic document object which doesn't represent any specific type of Inventor document, and has fewer stuff available to it, then there are the other types of document objects, which represent one specific type of Inventor document only, and will provide access to lots of stuff specific to that type of Inventor document. In your case you are trying to access a Part document, so in order to access part specific stuff and functionality, iLogic needs to understand the document object as that specific type of document.
Wesley Crihfield
(Not an Autodesk Employee)
