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BOM table attached to anchor point{ width=600 }

This VBA macro inserts Bill Of Materials (BOM) table into all or active sheet of the active SOLIDWORKS drawing. First drawing view of the sheet is used as the source

BOM table is attached to the BOM anchor point

Modify the constants in the macro to configure the BOM table options

Const ANCHOR_TYPE As Integer = swBOMConfigurationAnchorType_e.swBOMConfigurationAnchor_TopLeft 'anchor type: swBOMConfigurationAnchor_BottomLeft, swBOMConfigurationAnchor_BottomRight, swBOMConfigurationAnchor_TopLeft, swBOMConfigurationAnchor_TopRight
Const BOM_TYPE As Integer = swBomType_e.swBomType_PartsOnly 'bom type: swBomType_Indented, swBomType_PartsOnly, swBomType_TopLevelOnly
Const TABLE_TEMPLATE As String = "" 'full path to BOM template *.sldbomtbt or empty string for the default template
Const INDENTED_NUMBERING_TYPE As Integer = swNumberingType_e.swNumberingType_Flat 'numbering type (if BOM_TYPE is swBomType_Indented): swIndentedBOMNotSet, swNumberingType_Detailed, swNumberingType_Flat, swNumberingType_None
Const DETAILED_CUT_LIST As Boolean = False 'detailed cut-list (if BOM_TYPE is swBomType_Indented)
Const FOLLOW_ASSEMBLY_ORDER As Boolean = True 'true to check the Follow Assembly Order option

Const ALL_SHEETS As Boolean = True 'True to process all sheets, False to process active sheet only
Const ANCHOR_TYPE As Integer = swBOMConfigurationAnchorType_e.swBOMConfigurationAnchor_TopLeft
Const BOM_TYPE As Integer = swBomType_e.swBomType_PartsOnly
Const TABLE_TEMPLATE As String = ""
Const INDENTED_NUMBERING_TYPE As Integer = swNumberingType_e.swNumberingType_Flat
Const DETAILED_CUT_LIST As Boolean = False
Const FOLLOW_ASSEMBLY_ORDER As Boolean = True

Const ALL_SHEETS As Boolean = True

Dim swApp As SldWorks.SldWorks

Sub main()

Set swApp = Application.SldWorks

Dim swDraw As SldWorks.DrawingDoc

Set swDraw = swApp.ActiveDoc

If ALL_SHEETS Then

Dim vSheetNames As Variant
vSheetNames = swDraw.GetSheetNames

Dim activeSheetName As String
activeSheetName = swDraw.GetCurrentSheet().GetName

Dim i As Integer

For i = 0 To UBound(vSheetNames)
Dim swSheet As SldWorks.sheet
Set swSheet = swDraw.sheet(CStr(vSheetNames(i)))
InsertBomTable swDraw, swSheet
Next

swDraw.ActivateSheet activeSheetName

Else
InsertBomTable swDraw, swDraw.GetCurrentSheet
End If

End Sub

Sub InsertBomTable(draw As SldWorks.DrawingDoc, sheet As SldWorks.sheet)

If False = draw.ActivateSheet(sheet.GetName()) Then
Err.Raise vbError, "", "Failed to activate sheet " & sheet.GetName
End If

Dim vViews As Variant
vViews = sheet.GetViews

Dim swView As SldWorks.View

Set swView = vViews(0)

Dim swBomTableAnn As SldWorks.BomTableAnnotation

Set swBomTableAnn = swView.InsertBomTable4(True, 0, 0, ANCHOR_TYPE, BOM_TYPE, "", TABLE_TEMPLATE, False, INDENTED_NUMBERING_TYPE, DETAILED_CUT_LIST)

If Not swBomTableAnn Is Nothing Then
swBomTableAnn.BomFeature.FollowAssemblyOrder2 = FOLLOW_ASSEMBLY_ORDER
Else
Err.Raise vbError, "", "Failed to insert BOM table into " & swView.Name
End If

End Sub