Automate SOLIDWORKS Pack and Go with API Macros — Run, Rename, and Open the New Drawing

Pack and Go through the UI is fine for a one-off operation. When you’re doing it repeatedly — versioning a drawing before a revision cycle, archiving a job package, moving a drawing to a different project folder with all its references intact — you want a macro that runs Pack and Go, tells you where the new file landed, closes the original, and opens the copy. The SOLIDWORKS API supports all of this via the IPackAndGo interface, but the documentation examples stop at SavePackAndGo and leave the “then open the copy” part as an exercise for the reader.

This post shows a complete working VBA macro. It covers the IPackAndGo interface in enough depth to adapt it to your specific use case, and flags the three edge cases that break most implementations people try.

The IPackAndGo Interface

You get a PackAndGo object from IModelDocExtension.GetPackAndGo — the extension of whatever document is currently active. This works on assemblies, parts, and drawings. For drawings, the returned object includes the drawing file itself plus all referenced models; you have to set IncludeDrawings = True explicitly or the .slddrw is excluded from the packaged file list.

Key properties and methods:

The critical relationship: GetDocumentNames and GetDocumentSaveToNames return arrays in the same order. Index 0 in the source array corresponds to index 0 in the destination array. This is the mechanism you use to find the new .slddrw path — match by source extension, then read the corresponding destination path.

Why GetDocumentSaveToNames Is the Right Way to Get the New Filename

The naive approach is to construct the destination path yourself: take the original filename, append your prefix, point it at the destination folder. This breaks as soon as the folder structure gets involved.

When FlattenToSingleFolder = False (the default), Pack and Go mirrors the source directory tree under the destination root. A file at C:\Projects\Rev2\Parts\bracket.sldprt ends up at C:\Destination\Parts\bracket.sldprt. If you also added a prefix, it becomes C:\Destination\Parts\COPY_bracket.sldprt. Constructing that path manually requires replicating SOLIDWORKS’s own path-transformation logic.

GetDocumentSaveToNames does that calculation for you. Call it after setting your prefix, suffix, and destination folder but before calling SavePackAndGo. The returned array reflects exactly where each file will land. Read the .slddrw entry from that array and you have the authoritative new path.

Common Failure: IncludeDrawings Is False When Running From a Drawing

When the active document is an assembly, GetDocumentNames returns the assembly’s parts and sub-assemblies. If you called IncludeDrawings = True, it also returns any .slddrw that references the assembly.

When the active document is a drawing, the drawing file is still excluded from GetDocumentNames unless you set IncludeDrawings = True. This trips up most first implementations: Pack and Go runs, the drawing is copied, but GetDocumentSaveToNames returns no .slddrw entry because the interface was configured as if you were packing the referenced models only.

Always set IncludeDrawings = True when automating Pack and Go from a drawing.

Complete VBA Macro

The macro below:

1. Validates that the active document is a drawing
2. Configures Pack and Go options
3. Calls GetDocumentSaveToNames to identify the new .slddrw path before executing
4. Runs SavePackAndGo
5. Closes the original drawing
6. Opens the new drawing

Option Explicit

Sub Main()
    Dim swApp       As SldWorks.SldWorks
    Dim swDoc       As SldWorks.ModelDoc2
    Dim swExt       As SldWorks.ModelDocExtension
    Dim swPnG       As SldWorks.PackAndGo

    Dim origPath    As String
    Dim destFolder  As String
    Dim status      As Boolean
    Dim statuses    As Variant
    Dim errors      As Long
    Dim warnings    As Long

    Dim srcNames    As Variant
    Dim dstNames    As Variant
    Dim docStatus   As Variant
    Dim newDrwPath  As String
    Dim nCount      As Long
    Dim i           As Long

    Set swApp = Application.SldWorks
    Set swDoc = swApp.ActiveDoc

    If swDoc Is Nothing Then
        MsgBox "No document is open."
        Exit Sub
    End If
    If swDoc.GetType <> swDocDRAWING Then
        MsgBox "Active document must be a drawing."
        Exit Sub
    End If

    ' Save before packing — Pack and Go on an unsaved file produces
    ' unpredictable results with relative reference paths
    swDoc.Save3 swSaveAsOptions_Silent, errors, warnings

    origPath   = swDoc.GetPathName
    destFolder = "C:\PackedDrawings\"   ' << change to your target folder

    ' Get Pack and Go object from the active document's extension
    Set swExt = swDoc.Extension
    Set swPnG = swExt.GetPackAndGo

    ' Include the .slddrw itself in the package
    swPnG.IncludeDrawings        = True
    swPnG.IncludeSuppressed      = False
    swPnG.IncludeToolboxComponents = False
    swPnG.FlattenToSingleFolder  = True

    ' Set destination folder (True = folder path, not zip path)
    status = swPnG.SetSaveToName(True, destFolder)

    ' Optionally add a prefix so the copy doesn't overwrite the source
    ' if source and dest happen to share the same folder
    ' swPnG.AddPrefix = "COPY_"

    ' Get count and pre-dimension arrays to match
    nCount = swPnG.GetDocumentNamesCount
    ReDim dstNames(nCount - 1)
    ReDim docStatus(nCount - 1)

    ' GetDocumentSaveToNames returns paths AFTER applying prefix/suffix
    ' and folder transformation — this is the authoritative list
    status = swPnG.GetDocumentSaveToNames(dstNames, docStatus)

    ' Find the new drawing path in the destination list
    newDrwPath = ""
    For i = 0 To nCount - 1
        If LCase(Right(CStr(dstNames(i)), 7)) = ".slddrw" Then
            newDrwPath = CStr(dstNames(i))
            Exit For
        End If
    Next i

    If newDrwPath = "" Then
        MsgBox "Drawing not found in Pack and Go file list." & vbCrLf & _
               "Check that IncludeDrawings = True."
        Exit Sub
    End If

    ' Execute Pack and Go
    statuses = swExt.SavePackAndGo(swPnG)

    ' Verify the new file exists before closing original
    If Dir(newDrwPath) = "" Then
        MsgBox "Pack and Go finished but new drawing not found at:" & vbCrLf & newDrwPath
        Exit Sub
    End If

    ' Close the original
    swApp.CloseDoc origPath

    ' Open the new drawing
    Dim newDoc As SldWorks.ModelDoc2
    Set newDoc = swApp.OpenDoc6(newDrwPath, swDocDRAWING, _
                                swOpenDocOptions_Silent, "", errors, warnings)

    If newDoc Is Nothing Then
        MsgBox "Pack and Go complete, but could not open:" & vbCrLf & newDrwPath & _
               vbCrLf & "Errors: " & errors
    Else
        swApp.ActivateDoc3 newDrwPath, True, swRebuildOnActivation_Always, errors
        MsgBox "Done. Opened: " & newDrwPath
    End If
End Sub

Edge Cases to Know

The file count after adding a drawing. If you start from an assembly and set IncludeDrawings = True, the drawing count increases. Always call GetDocumentNamesCount after setting IncludeDrawings, not before. The count changes when you toggle that property.

FlattenToSingleFolder and filename collisions. If the assembly references two parts named bracket.sldprt in different subdirectories, flattening produces two files with the same target name. SOLIDWORKS will overwrite one silently. If your drawing references a complex assembly with many vendors contributing identically named parts, keep FlattenToSingleFolder = False and construct the new drawing path by matching against the source origPath in GetDocumentNames.

SavePackAndGo return value. SavePackAndGo returns a Variant array, not a Boolean. A non-empty array means something went wrong. Check it before closing the original document:

statuses = swExt.SavePackAndGo(swPnG)

Dim failCount As Long
failCount = 0
If Not IsEmpty(statuses) Then
    Dim j As Long
    For j = 0 To UBound(statuses)
        If statuses(j) <> swFileSaveError_None Then failCount = failCount + 1
    Next j
End If

If failCount > 0 Then
    MsgBox failCount & " file(s) failed to pack. Original not closed."
    Exit Sub
End If

The drawing must be saved before packing. Pack and Go reads file paths from disk. An unsaved drawing with a temp internal name will produce broken references in the packed copy. The macro above calls Save3 before running — don’t remove that call.

Adapting for Renaming Instead of Prefixing

If you need the packed copy to have a completely different name (not just a prefix), use SetDocumentSaveToNames instead of AddPrefix. This takes an array of destination paths in the same order as GetDocumentNames:

Dim srcNames As Variant
status = swPnG.GetDocumentNames(srcNames)

' Build a parallel array of destination paths
Dim newNames() As String
ReDim newNames(nCount - 1)

Dim srcPath As String
Dim baseFolder As String
baseFolder = "C:\PackedDrawings\"

For i = 0 To nCount - 1
    srcPath = CStr(srcNames(i))
    Dim fname As String
    fname = Mid(srcPath, InStrRev(srcPath, "\") + 1)
    ' Apply your custom naming logic here
    newNames(i) = baseFolder & fname
Next i

' Pass array to SetDocumentSaveToNames
status = swPnG.SetDocumentSaveToNames(newNames)

When SetDocumentSaveToNames is used, AddPrefix and AddSuffix are ignored.

Where This Fits in a Drawing Release Workflow

Pack and Go is the right tool when you need a self-contained copy of a drawing with all its references — not just the .slddrw in isolation. If your drawing references an assembly with 40 parts and 3 sub-assemblies, the packed folder has everything needed to open the drawing on a machine that has never seen those files.

For release workflows where PDM handles the archiving, automate the vault export with PDM Task Scheduler or the Task API instead. Pack and Go is for the non-PDM case: job shops, freelancers, or engineering teams handing off a deliverable to a supplier who doesn’t have access to your vault.

If your use case involves batch exports across multiple drawings — not a single Pack and Go but a sweep across a project folder — the pattern from the batch STEP and DXF export post applies: build a file list, loop, and call the operation in silent mode. The same OpenDoc6 with swOpenDocOptions_Silent works for drawings.

For a broader map of what’s automatable via API versus what needs the Task Scheduler or a full add-in, the SolidWorks workflow automation guide has the decision tree.