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Add Attribute to Feature and Include In Library Feature Example (VBA)

This example shows how to add an attribute to a feature and include that attribute with the feature if the feature is saved as a library feature. This example also includes instructions on how to verify that the attribute is included on each instance of the library feature.

' Preconditions:
' 1. Open a new part document.
' 2. Sketch a rectangle and extrude it.
' 3. Sketch a straight slot that fits on a face of
'    of the just-created extrude and cut-extrude the slot.
'    The cut-extrude should be named Cut-Extrude1.
' 4. Open the Immediate window.
' 5. Run the macro.
' Postconditions:
' 1. The Cut-Extrude1 feature is added to the part document with
'    an attribute of TestAttribute, which is visible in the
'    FeatureManager design tree.
' 2. Examine the Immediate window.
' To verify that the attribute is included in a library feature:
' 1. Drag the Cut-Extrude1 feature to the Design Library and
'    save the library feature.
' 2. Close the part document.
' 3. Open an existing model document and drag-and-drop the 
'    just-created library feature on the model.
' 4. Expand the just-dropped library feature in the FeatureManager 
'    design tree. Cut-Extrude1 and TestAttribute should appear beneath 
'    the just-dropped library feature in the FeatureManager design tree.
' 5. Close the model document.
Option Explicit
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swModelDocExt As SldWorks.ModelDocExtension
    Dim swSelectionMgr As SldWorks.SelectionMgr
    Dim swFeature As SldWorks.Feature
    Dim swAttribute As SldWorks.Attribute
    Dim swAttributeDef As SldWorks.AttributeDef
    Dim swFace As SldWorks.Face2
    Dim swParameter as SldWorks.Parameter
    Dim Faces As Variant
    Dim bool As Boolean    
    Sub main()    
        Set swApp = Application.SldWorks
        Set swModel = swApp.ActiveDoc
        Set swModelDocExt = swModel.Extension
        Set swSelectionMgr = swModel.SelectionManager        
        ' Create attribute
        Set swAttributeDef = swApp.DefineAttribute("TestPropagationOfAttribute")
        bool = swAttributeDef.AddParameter("TestAttribute", swParamTypeDouble, 2#, 0)
        bool = swAttributeDef.Register        
        ' Select the feature to which to add the attribute
        bool = swModelDocExt.SelectByID2("Cut-Extrude1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
        Set swFeature = swSelectionMgr.GetSelectedObject6(1, -1)
        Debug.Print ("Name of feature to which to add attribute: " & swFeature.Name)        
        ' Add the attribute to one of the feature's faces
        Faces = swFeature.GetFaces
        Set swFace = Faces(0)
        Set swAttribute = swAttributeDef.CreateInstance5(swModel, swFace, "TestAttribute", 0, swAllConfiguration)
        swAttribute.IncludeInLibraryFeature = True
        Debug.Print ("Include attribute in library feature? " & swAttribute.IncludeInLibraryFeature)
        Debug.Print ("Name of attribute: " & swAttribute.GetName)
        ' Add the attribute to one of the feature's faces
        Set swParameter = swAttribute.GetParameter("TestAttribute")
        Debug.Print ("Name of parameter: " & swParameter.GetName)         
        swModel.ForceRebuild3 (False)
End Sub

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