SOLIDWORKS Macro to create Drawings for All Configurations with Updated BOM

Article by Samony Riyaz updated November 21, 2019


Have you ever had a part with tens or hundreds or thousands of configurations? And you’re responsible for creating a drawing for EACH of those configurations with a correct BOM?

Well fear no more! We’ve got a SOLIDWORKS Macro for you in which all you have to do is…Change two lines, Click a button, Sit back and Relax while SOLIDWORKS generates the files automatically.

Let’s begin.

  1. Create a New Macro
    • Use the New Macro button in the Macro Toolbar (or select Tools > Macro > New)
  2. Ensure that the references in SOLIDWORKS Visual Basic Editor (VBA) are correct with your SOLIDWORKS Version
  3. Copy the code below and change the Highlighted Orange text to match your environment:
  4. Save the code
  5. Run

Preconditions: Ensure you are running the code below on a DRAWING containing a MODEL, which contains multiple configurations.

Results: In the OUTPUT_FOLDER of your choice, you should see the Drawing files for EACH configuration with an updated BOM

Const OUTPUT_FOLDER = "C:\Out\"
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swRefModel As SldWorks.ModelDoc2
Sub main()
Dim i As Integer
Dim vConfs As Variant
Dim swView As SldWorks.View
Dim confName As String
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
Set swView = swDraw.GetFirstView().GetNextView
Set swRefModel = swView.ReferencedDocument
vConfs = swRefModel.GetConfigurationNames
For i = 0 To UBound(vConfs)
confName = vConfs(i)
ProcessViews confName
swModel.ForceRebuild3 False
boolstatus = swModel.Extension.SaveAs(OUTPUT_FOLDER + confName + ".slddrw", swSaveAsVersion_e.swSaveAsCurrentVersion, swSaveAsOptions_e.swSaveAsOptions_Copy, Nothing, 0, 0)
Next i
MsgBox "Completed"
Set swApp = Nothing
Set swModel = Nothing
Set swDraw  = Nothing
Set swRefModel = Nothing
End Sub
Sub ProcessViews(confName As String)
Dim i As Integer
Dim vSheets As Variant
Dim j As Integer
Dim vViews As Variant
Dim swFeat As SldWorks.Feature
Dim swView As SldWorks.View
vSheets = swDraw.GetViews
For i = 0 To UBound(vSheets)
vViews = vSheets(i)
For j = 0 To UBound(vViews)
Set swView = vViews(j)
swView.ReferencedConfiguration = confName
Next j
'delete BOM
Set swFeat = swDraw.FirstFeature
Debug.Print swFeat.Name + " - " + swFeat.GetTypeName
While Not swFeat Is Nothing
Debug.Print swFeat.Name + " - " + swFeat.GetTypeName
If "BomFeat" = swFeat.GetTypeName Then
swFeat.Select2 False, -1
swDraw.Extension.DeleteSelection2 swDeleteSelectionOptions_e.swDelete_Absorbed
End If
Set swFeat = swFeat.GetNextFeature
boolstatus = swModel.Extension.SelectByID2(swView.Name, "DRAWINGVIEW", 0, 0, 0, False, 0, Nothing, 0)
AnchorType = swBOMConfigurationAnchorType_e.swBOMConfigurationAnchor_TopLeft
BomType = swBomType_e.swBomType_PartsOnly
Configuration = confName
TableTemplate = ""
' Insert BOM table
Set swBomAnn = swView.InsertBomTable2(True, 0.4, 0.3, AnchorType, BomType, Configuration, TableTemplate)
swModel.ClearSelection2 True
' Update FeatureManager design tree
Next i
Set swFeat = Nothing
Set swView = Nothing
End Sub

NOTE: The API examples are provided as is and should be used as reference only. You may use it in your environment, change it, or distribute it, but Javelin is not responsible for any types of damages whatsoever (including without limitation, damages from the loss of use, data, profits, or business) arising out of the uses of this information, applications or services.

Learn more about SOLIDWORKS Macros/API

Javelin provides SOLIDWORKS VB for Applications and SOLIDWORKS API training courses, which you can take live online, or in one of our Canadian classrooms. Check our schedule to learn more.

Related Links

Certified SOLIDWORKS Services available from Javelin

Javelin can help you to:

Samony Riyaz