Hello
As part of a historical plan rework created in Windows folders, and transferred to the pdm for a few years, I would like to know if any of you would have a trick or a macro in order to "explode" to divide multi-sheet drawings
historically the BE edit a drawing in which we had the assembly and then at each sheet the detailed plans of the parts included in this assembly.
The methodology having evolved following the passage via PDM and automated tasks, then the change of supplier then the change of subcontractor etc .... Today, when we "copy" an old assembly, we have these famous multi-sheet plans that do not correspond to the current process.
Have any of you already been confronted with the problem and have found a solution other than to recreate each room plan by removing the sheets in the so-called general plan as you go?
Currently we use smartdrawing to generate the basemaps of each room, then we copy the sheets of the multi sheet into each file generate, archive and then process the basemaps via integrations.
inappropriate = > human operations that sometimes mix up the drawings
Hello
See attached example to separate a multi-sheet MEP into multiple sheets.
https://www.javelin-tech.com/blog/2014/03/save-multi-sheet-as-its-own-drawing-or-combine-multiple-drawings/
It is undoubtedly possible to automate this via macro if you have some knowledge of VBA.
For the macro you also need to know how you name each MEP from each leaf. (name of the sheet?)
And with a bit of luck it will be enough to get a macro and modify it slightly to rename your MEPs as you wish.
Edit: here is another link forgotten in the previous one for macro example (but not found the macro that goes with it)
https://www.youtube.com/watch?v=lkU1acf2PNg
1 Like
Thank you for the feedback,
The YouTube video is what I'm looking for
How do I download the "Save Drawing Sheet File.swp" macro!!
I look for it if I find it I post it
After some research not found, but if anyone has time to devote to it the solution would be to copy one of the sheets of the multi-sheet, then paste it into a new sheet and save it with the name of this sheet.
Otherwise I had this macro modify from a macro for pdf export but it exports all the sheets (not just the one you want) and you would have to add the deletion of all the unwanted sheets.
'Description: Macro to export Drawing Sheets As PDF with sheet name as file name.
'Precondition: Any active drawing file
'Postconditions: PDF file in the same location as drawing file.
' Please back up your data before use and USE AT OWN RISK
' This macro is provided as is. No claims, support, refund, safety net, or
' warranties are expressed or implied. By using this macro and/or its code in
' any way whatsoever, the user and any entities which the user represents,
' agree to hold the authors free of any and all liability. Free distribution
' and use of this code in other free works is welcome. If any portion of
' this code is used in other works, credit to the authors must be placed in
' that work within a user viewable location (e.g., macro header). All other
' forms of distribution (i.e., not free, fee for delivery, etc) are prohibited
' without the expressed written consent by the authors. Use at your own risk!
' ------------------------------------------------------------------------------
' Written by: Deepak Gupta (http://gupta9665.wordpress.com/)
' -----------------------------------------------------------------------------
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim vSheetNameArr As Variant
Dim vSheetName As Variant
Dim bRet As Boolean
Dim swExportPDFData As SldWorks.ExportPdfData
Dim lErrors As Long
Dim lWarnings As Long
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
' Is document active?
If swModel Is Nothing Then
swApp.SendMsgToUser2 "A Drawing document must be active.", swMbWarning, swMbOk
Exit Sub
End If
' Is it a Drawing document?
If swModel.GetType <> swDocDRAWING Then
swApp.SendMsgToUser2 "A Drawing document must be active.", swMbWarning, swMbOk
Exit Sub
End If
Set swDraw = swModel
Set swSheet = swDraw.GetCurrentSheet
vSheetNameArr = swDraw.GetSheetNames
For Each vSheetName In vSheetNameArr
bRet = swDraw.ActivateSheet(vSheetName): Debug.Assert bRet
swDraw.ViewZoomtofit2
Set swExportPDFData = swApp.GetExportFileData(1)
swExportPDFData.SetSheets swExportData_ExportSpecifiedSheets, Nothing
'swModel.Extension.SaveAs vSheetName + ".pdf", 0, 0, swExportPDFData, lErrors, lWarnings
swModel.Extension.SaveAs Path & "\" & vSheetName & ".slddrw", 0, 0, Nothing, lErrors, lWarnings
Next vSheetName
End Sub
1 Like
lol I had the same idea I opened a multi-sheet export macro in separate pdf
I'll see if I can get the code clamps for this slddrw thing replacing the .pdf
1 Like
Hello
Since you have the myCADtools suite, you can use the "Integration" tool that should meet your expectations.
https://help.visiativ.com/mycadtools/2021/fr/Integration129.html
Attached is an example of an action
- Condition if the document is a MEP, if the number of sheets is not 1
- Then we do the operation of saving each sheet in a new MEP
Kind regards
example.mcact
3 Likes
I just quickly coded something that seems to work.
Just put in the 2nd line the path to your drwdot file.
Then it will have to be improved with some security so as not to launch it in any way.
For the moment you must imperatively open the MEP and then launch the macro (do not open a file in the meantime otherwise you will find your extracted files in the same place as your open file)
'Mettre ci-dessous le chemin vers le modèle de Fond de plan
Const sDrTemplateLaser As String = "U:\Modèle de documents\Mise en plan - Fonds de plan\A4-DECOUPE-b.DRWDOT"
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModel2 As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swDraw2 As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim vSheetNameArr As Variant
Dim vSheetName As Variant
Dim bRet As Boolean
Dim swExportPDFData As SldWorks.ExportPdfData
Dim lErrors As Long
Dim lWarnings As Long
Dim vSheetName2 As Variant
Dim i As Integer
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
' Is document active?
If swModel Is Nothing Then
swApp.SendMsgToUser2 "A Drawing document must be active.", swMbWarning, swMbOk
Exit Sub
End If
' Is it a Drawing document?
If swModel.GetType <> swDocDRAWING Then
swApp.SendMsgToUser2 "A Drawing document must be active.", swMbWarning, swMbOk
Exit Sub
End If
Set swDraw = swModel
Set swSheet = swDraw.GetCurrentSheet
vSheetNameArr = swDraw.GetSheetNames
For Each vSheetName In vSheetNameArr
bRet = swDraw.ActivateSheet(vSheetName): Debug.Assert bRet
swDraw.ViewZoomtofit2
swDraw.ActivateSheet vSheetName
'Debug.Print "Feuille active:" & sheetName
bRet = swDraw.Extension.SelectByID2(vSheetName, "SHEET", 0, 0, 0, False, 0, Nothing, 0)
swModel.EditCopy
Set swDraw2 = swApp.NewDocument(sDrTemplateLaser, 0, 0, 0)
'On supprime la 1ère feuille existantes
vSheetName2 = swDraw.GetSheetNames
Set swModel2 = swApp.ActiveDoc
Set swExt = swModel2.Extension
bRet = swDraw2.PasteSheet(swInsertOption_MoveToEnd, swRenameOption_No)
swDraw2.GetCurrentSheet.SetName vSheetName
Set swModel2 = swApp.ActiveDoc
'*********************************
'On supprime la 1ère feuille existantes
For i = 0 To UBound(vSheetName2) 'Boucle sur toutes les feuilles
Debug.Print vSheetName2(i)
If i = 0 Then
bRet = swExt.SelectByID2(vSheetName2(i), "SHEET", 0, 0, 0, False, 0, Nothing, 0)
'Supprimer la sélection
bRet = swExt.DeleteSelection2(0)
End If
Next
'********************************
swModel2.Extension.SaveAs Path & "\" & vSheetName & ".slddrw", 0, 0, Nothing, lErrors, lWarnings
Next vSheetName
End Sub
So now I'm fulfilled
between macro and integration!
Sorry Jm Savoyat I put sbadenis as the best answer "for those who don't have the mycad suite"
But I love working with integration, plus I can incorporate it into an automated PDM task after checking of course.
2 Likes
@JMSAVOYAT
example file of a higher version .... I thought I had the last update in 2021 SP2! (I want the beta)
@g.casters
A little patience, the myCADtools 2022 SP0 version should be available next week. We are fine-tuning the last details! 
Here's a screenshot of the example.
1 Like
the only tool where I install the SP0 since the beginning to say my level of patience.....
actually!
But this feature in the example I tried to post to you has already been available for a long time!
1 Like
