Hide Table of Contents

Pack and Go an Assembly (VBA)

This example shows how to get the names of the path and files of an assembly document, assign them new names, add a prefix and suffix to the new names, and save the newly named 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. Names of the current path and filenames
'    of the assembly documents are printed to Immediate window.
' 2. Names of the default path and filenames to which to
'    save assembly documents are printed to Immediate window.
' 3. User-specified path and user-named files for assembly documents
'    created.
' 4. Prefix and suffix added to user-named filenames.
' 5. Names of user-specified path and user-named filenames printed to
'    Immediate window.
' 6. User-named files created in user-specified path using Pack and Go.
' 7. 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 myFileName As String
Dim pgFileNames As Variant
Dim pgFileStatus As Variant
Dim pgSetFileNames() As String
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 j 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 and simulation results
wPackAndGo.IncludeDrawings = True
Debug.Print "  Include drawings: " & swPackAndGo.IncludeDrawings
swPackAndGo.IncludeSimulationResults = True
Debug.Print "  Include simulation results: " & swPackAndGo.IncludeSimulationResults
' 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
' Folder where to save the files
myPath = "C:\temp\"
' Create your own filenames for the model's documents
ReDim pgSetFileNames(namesCount - 1)
Debug.Print ""
Debug.Print "  My Pack and Go path and filenames before adding prefix and suffix: "
j = 0
For i = 0 To (namesCount - 1)
         myFileName = pgFileNames(i)
         ' Determine type of SolidWorks file based on file extension
             If InStr(LCase(myFileName), "sldprt") > 0 Then
                 myFileName = j & ".sldprt"
             ElseIf InStr(LCase(myFileName), "sldasm") > 0 Then
                 myFileName = j & ".sldasm"
            ElseIf InStr(LCase(myFileName), "slddrw") > 0 Then
                 myFileName = j & ".slddrw"
             Else
                 ' Only packing up SolidWorks files
                 Exit Sub
             End If
        pgSetFileNames(i) = myPath & myFileName
        Debug.Print "    My path and filename is: " & pgSetFileNames(i)
         j = j + 1
Next i
' Ensure that any copied drawing references the correct copied part
status = sw
PackAndGo.SetSaveToName(True, myPath)
' Set document paths and names for Pack and Go
status = swPackAndGo.SetDocumentSaveToNames(pgSetFileNames)
' 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

 



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

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Pack and Go an Assembly (VBA)
*Comment:  
*   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:



x

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
x

Web Help Content Version: API Help (English only) 2014 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.