Link Drawing Views to BOM in SolidWorks with a VBA Macro

Link drawing views to BOM in SolidWorks using a custom VBA macro built on the SolidWorks API—a must‑have SolidWorks automation for any design engineer. This lightweight API macro scans your drawing’s FeatureManager tree to identify the active BOM feature and, with a single command, sets Keep linked to BOM on every model view. No more manual property tweaking or risk of orphaned views slipping through revisions. This my Popular article about SolidWorks API VBA Macro- SolidWorks Automation

Usage of SolidWorks VBA Macro-Link views to BOM

1. Open your drawing sheet that already contains a BOM table.

2. Run the VBA macro from Tools → Macro → Run.

3. Watch the automation link all views to your BOM instantly. Refer this Article to know Reasons to use SolidWorks VBA Macro

Benefits of Link Drawing Views to BOM in SolidWorks using VBA API macro

• Time Savings: Eliminate repetitive clicks—automate view‑to‑BOM linking across single or multi‑sheet drawings.

• Consistency & Accuracy: SolidWorks automations ensure every view stays synchronized with your BOM, reducing errors during updates or revisions.

• Scalability: Whether you’re working on simple two‑view drawings or complex assemblies with dozens of views, this API macro handles it all in one pass.

Prerequisites for Link Drawing Views to BOM in SolidWorks using VBA API macro

Before you begin, make sure you have:

• SolidWorks (2018 or later) installed with the VBA editor enabled.

• A drawing document open that already contains a Bill of Materials (BOM) table.

• Basic familiarity with the SolidWorks VBA API and how to run macros.

Prerequisites & VBA References Setup

Before you paste and run the macro, you need to configure SolidWorks and the VBA editor so the API calls resolve correctly.

1. Enable VBA & Trust Settings

   • In SolidWorks, go to Options → System Options → General and check “Enable VBA macros”.

   • In the Windows Trust Center (if prompted), allow “Trust access to the VBA project object model.”

2. Open the VBA Editor

   • In SolidWorks, navigate to Tools → Macro → New.

   • Save the macro file (e.g. LinkViewsToBOM.swp).

   • The VBA IDE opens automatically.

3. Add SolidWorks API References
   In the VBA IDE, select Tools → References… and check the following libraries (version numbers may vary):

   • SolidWorks 20XX Type Library

   • SolidWorks 20XX Constant Type Library. Refer here about SolidWorks API library

   • (Optional, but helpful) SolidWorks 20XX CommandManager Type Library

   These references expose the SldWorks.* objects, swDocDRAWING constants, and methods like GetFirstView.

4. Paste the Macro Code

   • In Module1, delete any default text.

   • Copy the complete macro (both Sub main() and Function getBomName(...) with Option Explicit) and paste it into the module.

5. Save & Compile

   • Click Debug → Compile VBAProject.

   • Ensure there are no compile errors (missing references will show “User-defined type not defined”).

6. Run the Macro

   • Back in SolidWorks, go to Tools → Macro → Run.

   • Select your saved macro file and click Run.

Once set up, the macro will:

1. Detect your active drawing.

2. Locate the BOM feature via the SolidWorks API.

3. Loop through every view and set Keep linked to BOM.

4. Prompt you to rebuild (Ctrl + B) so changes take effect.

By following these setup steps, you’ll be ready to link drawing views to BOM in SolidWorks with a single click—boosting your SolidWorks automations and streamlining your drawing workflows.

What This Link Drawing Views to BOM in SolidWorks VBA Macro Will Do?

• Validate: Ensure a drawing document is active.

• Discover: Traverse the FeatureManager to locate the BOM (or weldment table) feature.

• Extract: Grab the feature’s internal name (e.g., “BomFeat1”).

• Link: Iterate through all drawing views and link them to the BOM automatically.

• Notify: Prompt you to rebuild the drawing to finalize the links.

Step‑by‑Step Guide to Link Drawing Views to BOM in SolidWorks using VBA Macro?

1. Setting Up the VBA Environment

1. In SolidWorks, go to Tools → Macro → New.

2. Save your macro file (e.g., LinkViewsToBOM.swp).

3. The VBA editor opens. Paste code into the Module1 code window.

2. Checking for an Open Drawing

You only want this macro to run when a drawing document is active. Use:

Line‑by‑Line Explanation

Enable strict variable declaration

Option Explicit

• Forces you to declare every variable with Dim.

• Helps catch typos and ensures you know exactly what variables exist.

Start of the main routine

Sub Main()

• Defines the entry point for the macro.

• Everything the macro does will be nested inside this Sub.

Declare SolidWorks application and document objects

Dim swApp   As SldWorks.SldWorks       ' SolidWorks application interface
Dim swModel As SldWorks.ModelDoc2      ' Any open document (part, assembly, or drawing)
Dim swDraw  As SldWorks.DrawingDoc     ' Specifically a drawing document
Dim swView  As SldWorks.View           ' Individual views on the drawing sheet
Dim BomName As String                  ' Internal name of the BOM feature

• swApp gives us methods to talk to SolidWorks.

• swModel is a generic doc—later we’ll confirm it’s a drawing.

• swDraw is our drawing-specific object once we’ve checked the type.

• swView lets us loop through each view on the sheet.

• BomName will hold the exact feature name of the BOM table.

Connect to the running SolidWorks instance

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc

• Application.SldWorks is the COM entry point.

• ActiveDoc returns whichever document (if any) is currently open and active.

Ensure the user has a drawing open

If swModel Is Nothing Or swModel.GetType <> swDocDRAWING Then
    swApp.SendMsgToUser2 "Please open a drawing document!", _
        swMbWarning, swMbOk
    Exit Sub
End If

• Checks two things:

  1. swModel Is Nothing: No document open at all.

  2. GetType <> swDocDRAWING: The open doc isn’t a drawing.

• If either is true, pop up a warning and stop the macro with Exit Sub.

Cast the generic model to a drawing document

Set swDraw = swModel

Now swDraw exposes drawing‑specific methods like GetFirstView.

Retrieve the BOM feature name

BomName = getBomName(swModel)
If BomName = "" Then Exit Sub
Debug.Print "BOM feature found: " & BomName

• Calls our helper function getBomName (detailed below).
• If it returns an empty string, we assume no BOM was found and abort.
• Debug.Print writes the BOM name to the Immediate Window (useful for debugging).

Loop through all drawing views

Set swView = swDraw.GetFirstView          ' First view is the sheet border
Set swView = swView.GetNextView           ' Skip the sheet format itself

Do While Not swView Is Nothing
    swView.SetKeepLinkedToBOM True, BomName
    Set swView = swView.GetNextView
Loop

• GetFirstView actually returns the sheet frame, so we immediately move to the next.

• In the loop, SetKeepLinkedToBOM True, BomName turns on “Keep linked to BOM” for that view.

• We iterate until there are no more views on the sheet.

Notify the user and end the macro

MsgBox "All views are now linked to BOM '" & BomName & "'." & _
" Please rebuild the drawing (Ctrl+B).", vbInformation
End Sub


Helper function to find and return the BOM’s internal name

Function getBomName(swModel As ModelDoc2) As String
    Dim swFeat    As Feature
    Dim swBomFeat As BomFeature
    
    Set swFeat = swModel.FirstFeature
    Do While Not swFeat Is Nothing
        Select Case swFeat.GetTypeName
            Case "BomFeat", "WeldmentTableFeat"
                ' Grab the BOM-specific feature
                Set swBomFeat = swFeat.GetSpecificFeature2
                getBomName = swBomFeat.Name
                Exit Function
        End Select
        Set swFeat = swFeat.GetNextFeature
    Loop
    
    ' If we exit the loop, no BOM was found
    MsgBox "No BOM or weldment table found in this drawing.", vbCritical
    getBomName = ""
End Function

• FirstFeature gives the top node in the FeatureManager tree.
• We loop through all features using GetNextFeature.
• When we hit either a "BomFeat" or "WeldmentTableFeat", we call GetSpecificFeature2 to access the BOM interface and extract its .Name.
• If the loop finishes with no match, we alert the user and return an empty string.

Compete Code of Link Drawing Views to BOM in SolidWorks using VBA Macro

Option Explicit

'===========================================================
' Macro: Link All Drawing Views to BOM
' Description: Automates setting “Keep linked to BOM” on
'              every view in the active drawing.
'===========================================================
Sub main()
    Dim swApp   As SldWorks.SldWorks      ' SolidWorks application object
    Dim swModel As SldWorks.ModelDoc2     ' Active document (could be part, assembly, or drawing)
    Dim swDraw  As SldWorks.DrawingDoc    ' Drawing document object
    Dim swView  As SldWorks.View          ' Individual drawing view
    Dim BomName As String                 ' Internal name of the BOM feature
    
    ' Connect to the running SolidWorks instance
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc

    ' 1) Validate that a drawing document is active
    If swModel Is Nothing Or swModel.GetType <> swDocDRAWING Then
        swApp.SendMsgToUser2 "Please open a drawing document!", _
            swMbWarning, swMbOk
        Exit Sub    ' Stop if not a drawing
    End If

    ' Cast the generic ModelDoc2 to a DrawingDoc
    Set swDraw = swModel

    ' 2) Find the BOM feature’s internal name
    BomName = getBomName(swModel)
    If BomName = "" Then Exit Sub   ' Abort if none found

    Debug.Print "BOM feature found: " & BomName   ' Output for debugging

    ' 3) Loop through all views on the sheet
    Set swView = swDraw.GetFirstView
    Set swView = swView.GetNextView    ' Skip the sheet format/frame

    Do While Not swView Is Nothing
        ' Link this view to the BOM by name
        swView.SetKeepLinkedToBOM True, BomName
        Set swView = swView.GetNextView  ' Move to the next view
    Loop

    ' 4) Inform the user to rebuild so links update
    MsgBox "All views are now linked to BOM '" & BomName & "'. " & _
           "Please rebuild the drawing (Ctrl+B).", vbInformation
End Sub

'===========================================================
' Function: getBomName
' Purpose : Traverse the FeatureManager tree to locate the
'           BOM or weldment table feature and return its
'           internal name.
' Returns : String (e.g., "BomFeat1"), or "" if not found
'===========================================================
Function getBomName(swModel As ModelDoc2) As String
    Dim swFeat    As SldWorks.Feature        ' Iterator for features
    Dim swBomFeat As SldWorks.BomFeature    ' BOM-specific interface

    ' Start at the top of the FeatureManager tree
    Set swFeat = swModel.FirstFeature

    ' Loop through each feature until we find the BOM or weldment table
    Do While Not swFeat Is Nothing
        Debug.Print "Checking feature type: " & swFeat.GetTypeName

        Select Case swFeat.GetTypeName
            Case "BomFeat", "WeldmentTableFeat"
                ' Found the BOM feature
                Set swBomFeat = swFeat.GetSpecificFeature2
                getBomName = swBomFeat.Name   ' Capture its internal name
                Exit Function
        End Select

        ' Move to the next feature in the tree
        Set swFeat = swFeat.GetNextFeature
    Loop

    ' If we reach here, no BOM feature was found
    MsgBox "No BOM or weldment table found in this drawing.", vbCritical
    getBomName = ""   ' Return empty to indicate failure
End Function

How to use Link Drawing Views to BOM in SolidWorks VBA Macro

Follow these simple steps to link drawing views to BOM in SolidWorks using our VBA macro. This Rank Math–friendly guide ensures you get optimal SEO value while streamlining your SolidWorks automations.

1. Prepare Your Drawing Document

• Open the SolidWorks drawing that already contains your BOM table.

• Ensure the BOM is placed on the active sheet and displays correctly.

2. Enable the VBA Macro Environment

1. In SolidWorks, go to Tools → Macro → New.

2. Save the new macro (e.g., LinkViewsToBOM.swp).

3. In the VBA editor, open Tools → References and check:

   • SolidWorks XX Type Library

   • SolidWorks Constant Type Library

3. Install the Macro Code

• Copy the complete VBA code (shown above) into your module.

• Verify the code starts with Option Explicit and includes both the Sub main() and Function getBomName(...).

4. Run the Macro

• In SolidWorks, navigate to Tools → Macro → Run.

• Select your saved macro (LinkViewsToBOM.swp).

• Click Run—the macro will:

  1. Detect your active drawing.

  2. Find the BOM feature via the SolidWorks API.

  3. Loop through each view and set Keep linked to BOM.

5. Verify the Links

• After completion, a message box appears:

  “All views are now linked to BOM ‘BomFeat1’. Please rebuild the drawing (Ctrl+B).”

• Inspect any view’s properties: the Keep linked to BOM checkbox should be checked and reference your BOM.

6. Rebuild Your Drawing

• Press Ctrl + B or click Rebuild to update all view links.

• Confirm your views update automatically whenever the BOM changes.

Read Also

• SolidWorks VBA Macro Object Library
• SolidWorks VBA Macro
• VBA in SolidWorks