SOLIDWORKS Macro to Add Bounding Boxes to an Assembly and Its Parts

Description

• Adds a best-fit Bounding Box feature to the active assembly.
• Adds the same feature to every unique part in the assembly, including parts in sub-assemblies.
• Useful for packaging, stock size and shipping dimensions in the BOM.

System Requirements

• SOLIDWORKS Version: SOLIDWORKS 2018 or newer (Bounding Box feature)
• Operating System: Windows 10 or later

Pre-Requisites

• The active document must be an assembly.
• Parts must not be read-only if you want to save the new feature.

Results

• Each part and the assembly get a Bounding Box feature and the related size properties.
• Use File > Save All to keep the changes. Running the macro twice adds a second bounding box.

Steps to Set Up the Macro

1. Open SOLIDWORKS and the document described in the pre-requisites.

2. Create the macro

• Go to Tools > Macro > New, give the .swp file a name and save it. The VBA editor opens.
• Replace everything in the module with the code below.

3. Run the macro

• Press F5 in the VBA editor, or use Tools > Macro > Run.
• For daily use, assign it to a toolbar button or keyboard shortcut via Tools > Customize.

VBA Macro Code

' Disclaimer:
' The code provided should be used at your own risk.
' Blue Byte Systems Inc. assumes no responsibility for any issues or damages that may arise from using or modifying this code.
' For more information, visit https://bluebyte.biz
' Reviewed and updated by Blue Byte Systems Inc.

Option Explicit

' Adds a best-fit Bounding Box feature to the active assembly and to every
' unique part in it. Requires SOLIDWORKS 2018 or newer.
' Run it once: running it again adds a second bounding box.

Dim swApp As SldWorks.SldWorks

Sub main()
    Dim swModel As SldWorks.ModelDoc2
    Dim swAssy As SldWorks.AssemblyDoc
    Dim swComp As SldWorks.Component2
    Dim swCompModel As SldWorks.ModelDoc2
    Dim vComps As Variant
    Dim vItem As Variant
    Dim done As Object
    Dim key As String
    Dim added As Long

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

    If swModel Is Nothing Then
        MsgBox "Open an assembly before running this macro.", vbExclamation
        Exit Sub
    End If
    If swModel.GetType <> swDocASSEMBLY Then
        MsgBox "The active document must be an assembly.", vbExclamation
        Exit Sub
    End If

    Set swAssy = swModel
    swAssy.ResolveAllLightWeightComponents False

    ' Top-level assembly bounding box
    If CreateBoundingBox(swModel) Then added = added + 1

    ' One bounding box per unique part file
    Set done = CreateObject("Scripting.Dictionary")
    vComps = swAssy.GetComponents(False)
    If Not IsEmpty(vComps) Then
        For Each vItem In vComps
            Set swComp = vItem
            Set swCompModel = swComp.GetModelDoc2
            If Not swCompModel Is Nothing Then
                If swCompModel.GetType = swDocPART Then
                    key = LCase(swCompModel.GetPathName)
                    If Not done.Exists(key) Then
                        done.Add key, True
                        If CreateBoundingBox(swCompModel) Then added = added + 1
                    End If
                End If
            End If
        Next
    End If

    swModel.ForceRebuild3 False
    MsgBox added & " bounding box(es) added. Use File > Save All to keep them.", vbInformation
End Sub

Private Function CreateBoundingBox(ByVal swDoc As SldWorks.ModelDoc2) As Boolean
    Dim swFeatMgr As SldWorks.FeatureManager
    Dim swData As SldWorks.BoundingBoxFeatureData
    Dim swFeat As SldWorks.Feature
    Dim wasVisible As Boolean

    wasVisible = swDoc.Visible
    If Not wasVisible Then swDoc.Visible = True

    Set swFeatMgr = swDoc.FeatureManager
    Set swData = swFeatMgr.CreateDefinition(swFmBoundingBox)
    If Not swData Is Nothing Then
        swData.ReferenceFaceOrPlane = swBoundingBoxType_BestFit
        swData.IncludeHiddenBodies = False
        swData.IncludeSurfaces = False
        Set swFeat = swFeatMgr.CreateFeature(swData)
    End If

    If Not wasVisible Then swDoc.Visible = False
    CreateBoundingBox = Not swFeat Is Nothing
End Function

Code Review Notes

We reviewed this macro before publishing it here. Changes from the original version:

• Added a check that the active document is an assembly.
• Parts are tracked by full path instead of title, so parts with the same name in different folders are both handled.
• Sub-assemblies are skipped, and window visibility is restored to its original state.

Need to customize the macro?

Contact us and we will adapt this macro to your workflow, or build a complete SOLIDWORKS or PDM automation for your team.