I figured this out with much help from yall's posts on this forum.  Sharing macro as thanks!  There have been a few posts in the past that didn't arrive at a solution; will point them here.

Let me know if you see a way to improve!

Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swDraw As SldWorks.DrawingDoc
    Dim swSheet As SldWorks.Sheet
    Dim swView As SldWorks.View
           
    Dim swModel As SldWorks.ModelDoc2
    Dim swFeature As SldWorks.Feature
    Dim swBodyFolder As SldWorks.BodyFolder
    Dim swCustPropMgr As SldWorks.CustomPropertyManager
                
    Dim bool As Boolean
    Dim sViewName, sViewBodyName, sBodyName, sPropVal As String
                
    Set swApp = Application.SldWorks
    Set swDraw = swApp.ActiveDoc
    bool = swDraw.ActivateSheet(swDraw.GetSheetNames(0))
    Set swSheet = swDraw.GetCurrentSheet
    Set swView = swDraw.GetFirstView
    
    'Find the main referenced view of the document on sheet1.  If default, find the first view.
    If swSheet.CustomPropertyView = "Default" Then
        Do While Not swView Is Nothing
            If (swView.ReferencedDocument Is Nothing) Then
                Set swView = swView.GetNextView 'skip empty sheet "views" etc
            Else
                sViewName = swView.Name
                Exit Do
            End If
        Loop
    Else
        sViewName = swSheet.CustomPropertyView
        Do While swView.Name <> sViewName And Not swView Is Nothing
            Set swView = swView.GetNextView
        Loop
    End If
    
    'If no referenced document was found, swView will be empty.  So no use trying to copy variables from a part.
    If swView Is Nothing Then Exit Sub
    
    Set swModel = swView.ReferencedDocument
           
    'If it is a view of a single body Weldment Member, get cutlist properties & populate title block
    If swModel.GetType = swDocPART Then
        If swModel.IsWeldment And swView.GetBodiesCount = 1 Then
        sViewBodyName = swView.Bodies(0).GetSelectionId
        sBodyName = Left(sViewBodyName, InStr(sViewBodyName, "@") - 1)
        
        'Loop thru all features looking for cutlist items
        Set swFeature = swModel.FirstFeature
        Do While Not swFeature Is Nothing
            If swFeature.GetTypeName = "CutListFolder" Then
                Set swBodyFolder = swFeature.GetSpecificFeature2
                
                'Loop through cutlist looking for body.  Should only be one body, but loop just to be sure.
                For i = 0 To UBound(swBodyFolder.GetBodies)
                    If swBodyFolder.GetBodies(i).Name = sBodyName Then
                    
                        'Body found! This is where the properties are
                        Set swCustPropMgr = swFeature.CustomPropertyManager
                        Exit Do
                    End If
                Next i
                
            End If
            Set swFeature = swFeature.GetNextFeature
        Loop
        End If
    End If
    
    'get custom properties from normal model if weldment info not found
    If swCustPropMgr Is Nothing Then
        Set swCustPropMgr = swModel.Extension.CustomPropertyManager(swView.ReferencedConfiguration)
    End If
    
    sPropVal = swCustPropMgr.Get("PartNumber")
    bool = swDraw.Extension.CustomPropertyManager("").Add2("PartNumber", swCustomInfoText, sPropVal)
    bool = swDraw.Extension.CustomPropertyManager("").Set("PartNumber", sPropVal)
    
    sPropVal = swCustPropMgr.Get("Description")
    bool = swDraw.Extension.CustomPropertyManager("").Add2("Description", swCustomInfoText, sPropVal)
    bool = swDraw.Extension.CustomPropertyManager("").Set("Description", sPropVal)
    swDraw.EditRebuild3
End Sub