Hide Table of Contents

Select Bodies Example (VBA)

This example shows how to select both solid and surface bodies in either a part or an assembly.

' Preconditions:
' 1. Open a part or assembly.
' 2. Open the Immediate window.
' Postconditions:
' 1. Selects all solid and surface bodies.
' 2. Examine the Immediate window.
Option Explicit
Sub SelectBodies(swApp As SldWorks.SldWorks, swModel As SldWorks.ModelDoc2, vBody As Variant, sPadStr As String)
    Dim swModExt As SldWorks.ModelDocExtension
    Dim swBody As SldWorks.Body2
    Dim sBodySelStr As String
    Dim sBodyTypeSelStr As String
    Dim i As Long
    Dim bRet As Boolean
    If IsEmpty(vBody) Then Exit Sub
    Set swModExt = swModel.Extension
    For i = 0 To UBound(vBody)
        Set swBody = vBody(i)
        sBodySelStr = swBody.GetSelectionId
        Debug.Print "  " & sPadStr & sBodySelStr
        Select Case swBody.GetType
            Case swSolidBody
                sBodyTypeSelStr = "SOLIDBODY"
            Case swSheetBody
                sBodyTypeSelStr = "SURFACEBODY"
            Case Else
                Debug.Assert False
        End Select
        bRet = swModExt.SelectByID2(sBodySelStr, sBodyTypeSelStr, 0#, 0#, 0#, True, 0, Nothing, swSelectOptionDefault): Debug.Assert bRet
    Next i
End Sub
Sub ProcessComponent(swApp As SldWorks.SldWorks, swModel As SldWorks.ModelDoc2, swComp As SldWorks.Component2, nLevel As Long)
    Dim vChildComp As Variant
    Dim swChildComp As SldWorks.Component2
    Dim sPadStr As String
    Dim vBody As Variant
    Dim i As Long
    For i = 0 To nLevel - 1
        sPadStr = sPadStr + "  "
    Next i
    Debug.Print sPadStr & swComp.Name2 & " <" & swComp.ReferencedConfiguration & ">"
    ' Solid bodies
    vBody = swComp.GetBodies2(swSolidBody)
    SelectBodies swApp, swModel, vBody, sPadStr
    ' Surface bodies
    vBody = swComp.GetBodies2(swSheetBody)
    SelectBodies swApp, swModel, vBody, sPadStr
    vChildComp = swComp.GetChildren
    For i = 0 To UBound(vChildComp)
        Set swChildComp = vChildComp(i)
        ProcessComponent swApp, swModel, swChildComp, nLevel + 1
    Next i
End Sub
Sub ProcessAssembly(swApp As SldWorks.SldWorks, swModel As SldWorks.ModelDoc2)
    Dim swConfigMgr As SldWorks.ConfigurationManager
    Dim swConf As SldWorks.Configuration
    Dim swRootComp As SldWorks.Component2
    Set swConfigMgr = swModel.ConfigurationManager
    Set swConf = swConfigMgr.ActiveConfiguration
    Set swRootComp = swConf.GetRootComponent3(True)
    ProcessComponent swApp, swModel, swRootComp, 1
End Sub
Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swPart As SldWorks.PartDoc
    Dim vBody As Variant
    Dim i As Long
    Dim bRet As Boolean
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    swModel.ClearSelection2 True
    Debug.Print "File = " & swModel.GetPathName
    Select Case swModel.GetType
        Case swDocPART
            Set swPart = swModel
            ' Solid bodies
            vBody = swPart.GetBodies2(swSolidBody, True)
            SelectBodies swApp, swModel, vBody, ""
            ' Surface bodies
            vBody = swPart.GetBodies2(swSheetBody, True)
            SelectBodies swApp, swModel, vBody, ""
        Case swDocASSEMBLY
            ProcessAssembly swApp, swModel
        Case Else
            Exit Sub
    End Select
End Sub

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Select Bodies Example (VBA)
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: API Help (English only) 2015 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.