Get Labels of Datum Origin Example (VBA)

This example shows how to insert a hole table annotation and get some of its properties.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified files exist:
'    * part document
'    * drawing document template
'    * hole table template
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified part document.
' 2. Creates a drawing of the part document.
' 3. Inserts a hole table annotation at the specified vertex.
' 4. Prints to the Immediate window:
'    * the hole table's datum origin x and y labels
'    * whether to display hole sizes using ANSI inch letters
'      and drill numbers
' 5. Examine the Immediate window and drawing.
'
' NOTE: Because the model is used elsewhere, do not save changes.
'----------------------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDrawingDoc As SldWorks.DrawingDoc
Dim swView As SldWorks.View
Dim swModelView As SldWorks.ModelView
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSelectionMgr As SldWorks.SelectionMgr
Dim swHoleTableAnnotation As SldWorks.HoleTableAnnotation
Dim swHoleTable As SldWorks.HoleTable
Dim swDatumOrigin As SldWorks.DatumOrigin
Dim fileName As String
Dim drawingDocTemplate As String
Dim holeTableTemplate As String
Dim status As Boolean
Dim errors As Long
Dim warnings As Long
Sub main()
    Set swApp = Application.SldWorks
    'Open part document and create drawing document
    fileName = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\tolanalyst\minimum_clearance\top_plate.sldprt"
    Set swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
    drawingDocTemplate = "C:\ProgramData\SolidWorks\SolidWorks 2016\templates\Drawing.drwdot"
    Set swDrawingDoc = swApp.NewDocument(drawingDocTemplate, swDwgPaperSizes_e.swDwgPaperBsize, 0.2794, 0.4318)
    Set swView = swDrawingDoc.CreateDrawViewFromModelView3(fileName, "*Front", 0.193046827497194, 0.155595183164983, 0)
    'Insert hole table annotation
    Set swModel = swApp.ActiveDoc
    Set swDrawingDoc = swModel
    Set swModelView = swModel.ActiveView
    Set swModelDocExt = swModel.Extension
    status = swDrawingDoc.ActivateView("Drawing View1")
    status = swModelDocExt.SelectByID2("", "VERTEX", 0.216278249046016, 0.198389907070707, 8.0000000000382E-03, False, 0, Nothing, 0)
    status = swModelDocExt.SelectByID2("", "FACE", 0.228097744219978, 0.151927063973064, 4.0000000000191E-03, False, 0, Nothing, 0)
    swModel.ClearSelection2 True
    status = swModelDocExt.SelectByID2("", "VERTEX", 0.216278249046016, 0.198389907070707, 8.0000000000382E-03, True, 1, Nothing, 0)
    status = swModelDocExt.SelectByID2("", "FACE", 0.228097744219978, 0.151927063973064, 4.0000000000191E-03, True, 2, Nothing, 0)
    Set swSelectionMgr = swModel.SelectionManager
    Set swView = swSelectionMgr.GetSelectedObjectsDrawingView2(1, -1)
    holeTableTemplate = "C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\standard hole table--letters.sldholtbt"
    Set swHoleTableAnnotation = swView.InsertHoleTable2(False, 5.40658670033671E-02, 0.253819263748597, 1, "A", holeTableTemplate)
    swModel.ClearSelection2 True
    'Get hole table and its datum origin
    Set swHoleTable = swHoleTableAnnotation.HoleTable
    Set swDatumOrigin = swHoleTable.DatumOrigin
    'Get datum origin's x and y labels
    Debug.Print "Datum origin:"
    Debug.Print ("  X label: " & swDatumOrigin.XLabel)
    Debug.Print ("  Y label: " & swDatumOrigin.YLabel)
    'Get whether to display hole sizes using ANSI inch letters and drill numbers
    Debug.Print "Display ANSI inch letter and drill number sizes in hole table? " & swHoleTable.ShowANSIInchLetterNumberDrillSizes

End Sub