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Add and Mate Component Example (VB.NET)

This example shows how to add a component to an assembly and mate it.

'---------------------------------------------------------------------------
' Preconditions:
' 1. Verify that these documents exist in public_documents\tutorial\toolbox:
'   
* lens_mount.sldasm
'   
* camtest.sldprt
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Opens lens_mount.sldasm.
' 2. Adds the specified component, camtest.sldprt, to the assembly.
' 3. Fires the AddItemNotify event.
' 4. Makes the specified component virtual by saving it to the
'    assembly with a new name.
' 5. Fires the RenameItemNotify event.
' 6. Adds a mate between the selected planes to the assembly.
' 7. Inspect the Immediate window and FeatureManager design tree.
'
' NOTE: Because the models are used elsewhere, do not save changes.
'----------------------------------------------------------------------------


Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
Imports System.Collections
 
Partial Class SolidWorksMacro
 
    Public WithEvents swAssemblyDoc As AssemblyDoc
 
    Dim swModel As ModelDoc2
    Dim swDocExt As ModelDocExtension
    Dim openAssem As Hashtable
    Dim tmpPath As String
    Dim tmpObj As ModelDoc2
    Dim boolstat As Boolean, stat As Boolean
    Dim strings As Object
    Dim swComponent As Component2
    Dim matefeature As Feature
    Dim MateName As String
    Dim FirstSelection As String
    Dim SecondSelection As String
    Dim strCompName As String
    Dim AssemblyTitle As String
    Dim AssemblyName As String
    Dim errors As Integer
    Dim warnings As Integer
    Dim mateError As Integer
    Dim
fileName as String
 
    Sub Main() 
 

        ' Open assembly
        fileName =
"C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2017\tutorial\toolbox\lens_mount.sldasm"
        swModel = swApp.OpenDoc6(fileName, swDocumentTypes_e.swDocASSEMBLY, swOpenDocOptions_e.swOpenDocOptions_Silent,
"", errors, warnings)

        ' Set up event
        swAssemblyDoc = swModel
        openAssem = New Hashtable
        AttachEventHandlers()
 
        ' Get title of assembly document
        AssemblyTitle = swModel.GetTitle()
 
        ' Split the title into two strings using the period as the delimiter
        strings = Split(AssemblyTitle, ".")
 
        ' Use AssemblyName when mating the component with the assembly
        AssemblyName = strings(0)
 
        Debug.Print("Name of assembly: " & AssemblyName)
 
        boolstat = True
        Dim strCompModelname As String
        strCompModelname = "camtest.sldprt"
 
        ' Because the component resides in the same folder as the assembly, get
        ' the assembly's path and use it when opening the component
        tmpPath = Left(swModel.GetPathName, InStrRev(swModel.GetPathName"\"))
 
        ' Open the component
        tmpObj = swApp.OpenDoc6(tmpPath + strCompModelname, swDocumentTypes_e.swDocPART, swOpenDocOptions_e.swOpenDocOptions_Silent, "", errors, warnings)
 
        ' Check to see if the file is read-only or cannot be found; display error
        ' messages if either
        If warnings = swFileLoadWarning_e.swFileLoadWarning_ReadOnly Then
            MsgBox("This file is read-only.")
            boolstat = False
        End If
 
        If tmpObj Is Nothing Then
            MsgBox("Cannot locate the file.")
            boolstat = False
        End If
 
        ' Activate the assembly so that you can add the component to it
        swModel = swApp.ActivateDoc3(AssemblyTitle, True, swRebuildOnActivation_e.swUserDecision, errors)
 
        ' Add the camtest part to the assembly document
        swComponent = swAssemblyDoc.AddComponent5(strCompModelname, swAddComponentConfigOptions_e.swAddComponentConfigOptions_CurrentSelectedConfig, ""False"", -1, -1, -1)
 
        ' Make the component virtual
        stat = swComponent.MakeVirtual2(True)
 
        ' Get the name of the component for the mate
        strCompName = swComponent.Name2()
 
        ' Create the name of the mate and the names of the planes to use for the mate
        MateName = "top_coinc_" + strCompName
        FirstSelection = "Top@" + strCompName & "@" + AssemblyName
        SecondSelection = "Front@" + AssemblyName
 
        swModel.ClearSelection2(True)
        swDocExt = swModel.Extension
 
        ' Select the planes for the mate
        boolstat = swDocExt.SelectByID2(FirstSelection, "PLANE", 0, 0, 0, True, 1, Nothing, swSelectOption_e.swSelectOptionDefault)
        boolstat = swDocExt.SelectByID2(SecondSelection, "PLANE", 0, 0, 0, True, 1, Nothing, swSelectOption_e.swSelectOptionDefault)
 
        ' Add the mate
        matefeature = swAssemblyDoc.AddMate5(swMateType_e.swMateCOINCIDENT, swMateAlign_e.swMateAlignALIGNED, False, 0, 0, 0, 0, 0, 0, 0, 0, FalseFalse, 0, mateError)
        matefeature.Name = MateName
        Debug.Print("Mate added: " & matefeature.Name)
 
        swModel.ViewZoomtofit2()
 
    End Sub
 
    Sub AttachEventHandlers()
        AttachSWEvents()
    End Sub
 
 
    Sub AttachSWEvents()
        AddHandler swAssemblyDoc.AddItemNotifyAddressOf Me.swAssemblyDoc_AddItemNotify
        AddHandler swAssemblyDoc.RenameItemNotifyAddressOf Me.swAssemblyDoc_RenameItemNotify
    End Sub
 
    Private Function swAssemblyDoc_AddItemNotify(ByVal EntityType As IntegerByVal itemName As StringAs Integer
        Debug.Print("Component added: " & itemName)
    End Function
 
    Private Function swAssemblyDoc_RenameItemNotify(ByVal EntityType As IntegerByVal oldName As StringByVal NewName As StringAs Integer
        Debug.Print("Virtual component name: " & NewName)
    End Function
 
 
    ''' <summary>
    ''' The SldWorks swApp variable is pre-assigned for you
    ''' </summary>
    Public swApp As SldWorks
 
 
End 
Class



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