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Pack and Go an Assembly (VBA)

This example shows how to get the names of the path and files of an assembly document, add a prefix and suffix to the names, and save the files to a different path using the Pack and Go interface.

' Preconditions:
' 1. Specified assembly exists.
' 2. The folder, c:\temp, exists.
' 3. Open the Immediate window.
' 4. Run the macro.
' Postconditions:
' 1. Prints names of the current path and filenames
'    of the assembly documents to the Immediate window.
' 2. Prints names of the default path and filenames to which to
'    save assembly documents to Immediate window.
' 3. Specifies the Pack and Go destination folder.
' 4. Specifies that all files get saved to the root directory of the
'    Pack and Go destination folder.
' 5. Adds prefix and suffix to user-named filenames.
' 6. Prints names of user-specified path and user-named filenames to
'    Immediate window.
' 7. Creates user-named files in user-specified path using Pack and Go.
' 8. Examine c:\temp to verify.

Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModelDoc As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swPackAndGo As SldWorks.PackAndGo
Dim openFile As String
Dim pgFileNames As Variant
Dim pgFileStatus As Variant
Dim pgGetFileNames As Variant
Dim pgDocumentStatus As Variant
Dim status As Boolean
Dim warnings As Long
Dim errors As Long
Dim i As Long
Dim namesCount As Long
Dim myPath As String
Dim statuses As Variant

Sub main()

Set swApp = Application.SldWorks

' Open assembly
openFile = "C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\samples\tutorial\advdrawings\handle.sldasm"
Set swModelDoc = swApp.OpenDoc6(openFile, swDocASSEMBLY, swOpenDocOptions_Silent, "", errors, warnings)
Set swModelDocExt = swModelDoc.Extension

' Get Pack and Go object
Debug.Print "Pack and Go"
Set swPackAndGo = swModelDocExt.GetPackAndGo

' Get number of documents in assembly
namesCount = swPackAndGo.GetDocumentNamesCount
Debug.Print "  Number of model documents: " & namesCount

' Include any drawings, SOLIDWORKS Simulation results, and SOLIDWORKS Toolbox components
swPackAndGo.IncludeDrawings = True
Debug.Print "  Include drawings: " & swPackAndGo.IncludeDrawings
swPackAndGo.IncludeSimulationResults = True
Debug.Print "  Include SOLIDWORKS Simulation results: " & swPackAndGo.IncludeSimulationResults
swPackAndGo.IncludeToolboxComponents = True
Debug.Print "  Include SOLIDWORKS Toolbox components: " & swPackAndGo.IncludeToolboxComponents

' Get current paths and filenames of the assembly's documents
status = swPackAndGo.GetDocumentNames(pgFileNames)
Debug.Print ""
Debug.Print "  Current path and filenames: "
If (Not (IsEmpty(pgFileNames))) Then
    For i = 0 To UBound(pgFileNames)
        Debug.Print "    The path and filename is: " & pgFileNames(i)
    Next i
End If

' Get current save-to paths and filenames of the assembly's documents
status = swPackAndGo.GetDocumentSaveToNames(pgFileNames, pgFileStatus)
Debug.Print ""
Debug.Print "  Current default save-to filenames: "
If (Not (IsEmpty(pgFileNames))) Then
    For i = 0 To UBound(pgFileNames)
        Debug.Print "   The path and filename is: " & pgFileNames(i)
    Next i
End If

' Set folder where to save the files
myPath = "C:\temp\"
status = swPackAndGo.SetSaveToName(True, myPath)

' Flatten the Pack and Go folder structure; save all files to the root directory
swPackAndGo.FlattenToSingleFolder = True

' Add a prefix and suffix to the new Pack and Go filenames
swPackAndGo.AddPrefix = "SW_"
swPackAndGo.AddSuffix = "_PackAndGo"

 ' Verify document paths and filenames after adding prefix and suffix
ReDim pgGetFileNames(namesCount - 1)
ReDim pgDocumentStatus(namesCount - 1)
status = swPackAndGo.GetDocumentSaveToNames(pgGetFileNames, pgDocumentStatus)
Debug.Print ""
Debug.Print "  My Pack and Go path and filenames after adding prefix and suffix: "
For i = 0 To (namesCount - 1)
     Debug.Print "    My path and filename is: " & pgGetFileNames(i)
Next i

' Pack and Go
statuses = swModelDocExt.SavePackAndGo(swPackAndGo)

End Sub


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