Retrieve sketch dimension of part document inside derived assembly

<?xml encoding=”UTF-8″>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: