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Set Material Example (VB.NET)

This example shows how to get the names of the material schema, material databases, and bodies in a part document. This example also shows how to apply a SOLIDWORKS Material to all of the bodies in a part document.

'----------------------------------------------------
' Preconditions:
' 1. Verify that the specified document exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens the specified part document.
' 2. Applies the material ABS PC (polycarbonate plastic)
'    from the SOLIDWORKS Material database to all
'    bodies in the part.
' 3. To verify, examine:
'    * DisplayManager tab
'    * graphics area
'    * Immediate window
'
' NOTE: Because the part document is used 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 swPart As PartDoc
        Dim swBody As Body2
        Dim errors As Integer
        Dim warnings As Integer
        Dim vMatDBarr As Object
        Dim vMatDB As Object
        Dim Bodies As Object
        Dim BodyMaterialError As Integer
        Dim sMatName As String = ""
        Dim sMatDB As String = ""
        Dim itr As Integer
        Dim boolstat as Boolean


        ' Open the document
        swModel = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\multibody\multi_inter.sldprt", swDocumentTypes_e.swDocPART,
swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
        swPart = swModel


        ' Get the material schema and names
        ' of available materials databases
        vMatDBarr = swApp.GetMaterialDatabases
        Debug.Print("Material schema pathname = " & swApp.GetMaterialSchemaPathName)
        For Each vMatDB In vMatDBarr
            Debug.Print("  Material database: " & vMatDB)
        Next


        Debug.Print("")


        Bodies = swPart.GetBodies2(swBodyType_e.swAllBodies, False)
        For itr = 0 To UBound(Bodies)
            swBody = Bodies(itr)
            ' Get the name of the body
            Debug.Print(swBody.Name)


            boolstat = swBody.Select2(False, Nothing)


            ' Set the SOLIDWORKS material for that body
            BodyMaterialError = swBody.SetMaterialProperty("Default", "solidworks materials.sldmat",
"ABS PC")
            ' Comment out previous statement and uncomment following statement to use custom material
            'BodyMaterialError = swBody.SetMaterialProperty("Default", "custom materials.sldmat",
"Custom Plastic")


            ' Get the names of the body's material and the
            ' database to which it belongs
            sMatName = swBody.GetMaterialPropertyName("", sMatDB)
            If sMatName = "" Then
                Debug.Print("Body " & itr & "'s material name: No material applied")
            Else
                Debug.Print("Body " & itr & "'s material name: " & sMatName)
                Debug.Print("Body " & itr & "'s material database: " & sMatDB)
                Debug.Print(" ")
            End If
        Next itr

    End Sub


    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you.
    ''' </summary>
    Public swApp As SldWorks


End Class



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