Retrieve sketch dimension of part document inside derived assembly

By Adam Nagy

If you want to retrieve only specific dimensions from the document that is shown in a drawing view then you can use Sheet.DrawingDimensions.GeneralDimensions.Retrieve()

We start with this this set of documents (can be found in this forum post): 

Here is the d0 dimension in Sketch1 we are trying to get back:

Here is the VBA code to do it:

Private Sub RetrieveTest()
  Dim oDrawDoc As DrawingDocument
  Set oDrawDoc = ThisApplication.ActiveDocument
  Dim oSheet As Sheet
  Set oSheet = oDrawDoc.Sheets.Item(1)
  Dim oView As DrawingView
  Set oView = oSheet.DrawingViews.Item(1)' Create object collection for dimensions to be retrieved
  Dim oTO As TransientObjects
  Set oTO = ThisApplication.TransientObjects
  Dim oObjColl As ObjectCollection
  Set oObjColl = oTO.CreateObjectCollection' Get the derived part document
  Dim oDoc As PartDocument
  Set oDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
  Dim oDef As PartComponentDefinition
  Set oDef = oDoc.ComponentDefinition
  Dim oRefComps As ReferenceComponents
  Set oRefComps = oDef.ReferenceComponents' Get the definition of assembly it's derived from
  Dim oDerAsmDef As DerivedAssemblyDefinition
  Set oDerAsmDef = oRefComps.DerivedAssemblyComponents(1).Definition' Get the part being used
  Dim oPartCompDef As PartComponentDefinition
  Set oPartCompDef = _
    oDerAsmDef.Occurrences(1).ReferencedOccurrence.Definition' Get the dimensions of the first sketch
  Dim oDC As DimensionConstraint
  Set oDC = oPartCompDef.Sketches(1).DimensionConstraints(1)' Show the name of the dimension we are retrieving
  MsgBox (oDC.Parameter.Name)
  Call oObjColl.Add(oDC)' Retrieve subset of dimensions
  Call oSheet.DrawingDimensions.GeneralDimensions.Retrieve( _
    oView, oObjColl)
End Sub

Here is the code in action: