Your first SolidWorks macro (VBA), explained line by line

Every design office has a task like this: forty drawings need to go out as PDFs, and somebody — a degreed engineer, usually — spends an afternoon doing File → Save As → PDF → OK forty times. SolidWorks has had a full automation API since the 90s. It's sitting under Tools → Macro, it speaks VBA, and the license you already own includes all of it. Let's write the classic first macro: save the active drawing as a PDF, correctly.

Record one first (then throw it away)

Tools → Macro → Record, do the Save-As by hand, stop recording, and open what it wrote. Recorded macros are ugly — hardcoded paths, magic numbers, dead lines — but they answer the hardest beginner question: what is the API call for the thing I just did? Record to discover, then rewrite clean. Here's the clean version:

Option Explicit

Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swExport As SldWorks.ExportPdfData
    Dim pdfPath As String
    Dim errs As Long, warns As Long

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc

    If swModel Is Nothing Then
        swApp.SendMsgToUser "Open a drawing first."
        Exit Sub
    End If

    If swModel.GetType <> swDocDRAWING Then
        swApp.SendMsgToUser "This macro only works on drawings."
        Exit Sub
    End If

    ' same folder, same name, .pdf extension
    pdfPath = Left$(swModel.GetPathName, _
                    Len(swModel.GetPathName) - 6) & "pdf"

    Set swExport = swApp.GetExportFileData(swExportPdfData)
    swExport.ViewPdfAfterSaving = False

    swModel.Extension.SaveAs pdfPath, 0, 0, swExport, errs, warns

    If errs <> 0 Then
        swApp.SendMsgToUser "Export failed, error code " & errs
    End If
End Sub

What each part is doing

• `Application.SldWorks` — the running SolidWorks instance. Every macro starts by grabbing this; it's the root of the whole object model.
• `ActiveDoc` → `ModelDoc2` — whatever document is open in front of the user. ModelDoc2 is the workhorse interface: parts, assemblies, and drawings all present it.
• The two guard clauses — the difference between a tool and a booby trap. ActiveDoc is Nothing when no file is open, and GetType stops someone running a drawing macro on a part. Recorded macros have neither; production macros always should.
• `GetPathName` surgery — the saved file's full path; chop SLDDRW (6 chars) off the end and append pdf. Note this is empty for never-saved documents — guard for that too as homework.
• `GetExportFileData(swExportPdfData)` — the options object for PDF export; this is where you'd set "all sheets" (SetSheets) or turn off the annoying auto-open of the finished PDF.
• `Extension.SaveAs` — the modern save call. The errs/warns out-parameters are how it tells you what went wrong; ignoring them is how "the macro worked" and "there's no PDF" happen at the same time.

Run it, wire it to a button

Tools → Macro → Run and pick the .swp. If it earns its keep, give it a toolbar button (Tools → Customize → Commands → Macro) — adoption in an office is directly proportional to how little the macro looks like programming.

Where this goes next

The jump from the active document to every file in a folder — loop the directory, OpenDoc6, export, CloseDoc — is maybe fifteen more lines, and it's the one that turns the forty-PDF afternoon into a coffee break — the finished batch version is in my free code library, ready to download. The same pattern batch-exports STEP files, fixes title blocks, and pulls BOMs into Excel — where it hands off to the Python side of shop automation. And if you'd rather skip to the working tool, I build these.

Nobody in the office will care that it's forty lines of VBA. They'll care that drawings now leave the building in one click.