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Get Bodies in Components Example (VB.NET)

This example shows how to get the number of normal and user bodies in the components in an assembly.

'-----------------------------------------------------
' Preconditions:
' 1. Verify that the specified assembly document
'    to open exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Gets and prints each component's name, number of
'    solid bodies, body names, and body types
'    to the Immediate window.
' 2. Right-click filterholder<1> in the FeatureManager
'    design tree and click the Open Part button.
'    Notice that there are no screw holes in the part.
' 3. Close the part and examine the filterholder<1>
'    component, which is the orange, flat, circular
'    component located on the front of the assembly
'    in the graphics area. There are screw
'    holes in the component.
' 4. Examine the filterholder<1>'s information in the
'    Immediate window. Because the component was
'    modified in the assembly, its body is identified
'    as a user body.
'
' NOTE: Because this assembly document is used by
' elsewhere, do not save changes.
'-----------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
    Public Sub main()
 
        Dim swModel As ModelDoc2
        Dim swAssembly As AssemblyDoc
        Dim vComponents As Object
        Dim oneComponent As Component2
        Dim vBodies As Object
        Dim vBodyInfo As Object = Nothing
        Dim BodyType As Integer
        Dim errors As Integer, warnings As Integer
        Dim i As Integer, j As Integer
 
        ' Open the assembly
        swModel = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\toolbox\lens_mount.sldasm", swDocumentTypes_e.swDocASSEMBLY, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
        swAssembly = swModel
 
        ' Get the components in the assembly
        vComponents = swAssembly.GetComponents(True)
        For i = 0 To UBound(vComponents)
            oneComponent = vComponents(i)
            Debug.Print(" ")
            Debug.Print("Component name: " & oneComponent.Name2)
            ' Get the solid bodies in the component
            vBodies = oneComponent.GetBodies3(swBodyType_e.swSolidBody, vBodyInfo)
            Debug.Print("  Number of solid bodies: " & (UBound(vBodies) + 1))
            For j = 0 To UBound(vBodies)
                Debug.Print("  Body number: " & (j + 1))
                Debug.Print("  Body name: " & vBodies(j).Name)
                ' Print the type of body
                BodyType = vBodyInfo(j)
                Select Case BodyType
                    Case 0
                        Debug.Print("  Body type: user")
                    Case 1
                        Debug.Print("  Body type: normal")
                End Select
            Next
        Next
    End Sub
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks
 
End Class


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