Creating DXF and PDF files from SW Drawings

I'm thinking you could using macros and you would need a macro to run when you either close or save the drawing...

Maybe

Deepak Gupta

Amen Allah Jlili

Keith Rice

Can help

As John, mentioned, a macro can be made to do that.

I have this one that I've been using since 2011. The advantages in this macro are that it also saves a copy of the iges file as well AND it also saves those files to your SW file in the Design Binder. We used contract manufacturers all over the world so it was imperative that we had a system that worked. That may not be required in your workflow and disabling those functions is as easy as commenting out the lines as noted.

I have attached the macro file and pasted the text below. This macro would need to be run again to update the files. Though I'm not sure this will actually replace the files as I have never done so.

'This macro saves current drawing to PDF, IGS and DXF. Precondition is that you save an IGS file using the EXACT same name as the drawing file.

'Then this macro also inserts these files into the Design Binder

'Pack and Go will then add these files at the same time

'------------------------------------------------------------------

Option Explicit

    Dim swApp                   As SldWorks.SldWorks

    Dim swModel                 As SldWorks.ModelDoc2

    Dim Linked                  As Boolean

    Dim sPathName               As String

    Dim nErrors                 As Long

    Dim nWarnings               As Long

    Dim nRetval                 As Long

    Dim bShowMap                As Boolean

    Dim swModelDocExt           As SldWorks.ModelDocExtension

    Dim swExportData            As SldWorks.ExportPdfData

    Dim filename                As String

    Dim iPathName               As String

    Dim boolstatus              As Boolean

    Dim boolstatus1             As Boolean

    Dim lErrors                 As Long

    Dim lWarnings               As Long

    Dim bRet                    As Boolean

Sub main()

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

    ' Strip off SolidWorks drawing file extension (.slddrw)

    ' and add DXF file extension (.dxf)

    sPathName = swModel.GetPathName

    sPathName = Left(sPathName, Len(sPathName) - 6)

    sPathName = sPathName + "DXF"

    ' Show current settings

'   If swModel Is Nothing Then MsgBox "A Part or Assembly file must be open", vbExclamation: End

' the above line needs to be modified to check for the precondition of an igs file.

    ' Turn off showing of map

    bShowMap = swApp.GetUserPreferenceToggle(swDXFDontShowMap)

    Set swModelDocExt = swModel.Extension

    Set swExportData = swApp.GetExportFileData(swExportPDFData)

    filename = swModel.GetPathName

    filename = Strings.Left(filename, Len(filename) - 6) & "PDF"

    ' Create IGS filename - comment out if not required

    iPathName = Strings.Left(filename, Len(filename) - 3) & "IGS"

    boolstatus1 = swExportData.SetSheets(swExportData_ExportAllSheets, 1)

    boolstatus1 = swModelDocExt.SaveAs(filename, 0, 0, swExportData, lErrors, lWarnings)

    swApp.SetUserPreferenceToggle swDXFDontShowMap, False

    bRet = swModel.SaveAs4(sPathName, swSaveAsCurrentVersion, swSaveAsOptions_Silent, nErrors, nWarnings)

    If bRet = False Then

        nRetval = swApp.SendMsgToUser2("Problems saving file.", swMbWarning, swMbOk)

    End If

    'Save files to Design Binder

    'comment out the following lines if you don;t wish to save to the design binder in SW

    boolstatus = swModelDocExt.SelectByID2("Design Binder", "DOCSFOLDER", 0, 0, 0, False, 0, Nothing, 0)

       swModelDocExt.InsertAttachment filename, False

       swModelDocExt.InsertAttachment sPathName, False

       swModelDocExt.InsertAttachment iPathName, False

       If boolstatus1 Then

        MsgBox "Save as PDF/DXF and Added .PDF .DXF .IGS to Design Binder successful."

    Else

        MsgBox "Save as PDF failed, Error code:" & lErrors '

    End If

    'End Save files to Design Binder sub

    ' Restore old setting

    swApp.SetUserPreferenceToggle swDXFDontShowMap, bShowMap

End Sub

'----------------------------------------------