Hi everyone,
We use the revision tables in the MEPs to increment the revision index and note the changes made.
Thus, the revision property is located in the MEP file.
Is it possible to link this property of the MEP revision index to a property in the part or assembly in order to add it to bills of materials, for example?
Thank you in advance.
Have a nice day
Hello @remrem, it's been a while... 
If you have access to the MyCadTools suite, the Smartproperties tool allows you to do this:
But I don't recommend it at all, this function doesn't have a notion of " Automatic Update".
=> If the drawing is updated with a new index, you will have to restart the Smartproperties on this drawing and then open the associated 3D and restart the Smartproperties again... This is a huge potential for error.
Hello remrem,
I think it would not be advisable to index 3D. As only the 3D said times.
What we do to send a 3D to customers through a WWTP by re-naming it with the index and the date of creation of the WWTP.
Otherwise use a PLM to manage all this...
It's up to you.
@+.
AR.
Yes. Indeed. I'm back. 
I don't have the MyCadTools suite...
Indeed, the objective is to limit errors.
I don't really understand your answer.
If 3D is a good time, why not index 3D?
Well, there will be a risk of errors.
so I advise you to do a re-named WWTP with the index and date of completion.
There you go...
@+.
AR.
Hello,
In our country (even if we have Solidworks PDM), it is the 3D that carries the index in its properties.
The information is duplicated in the drawing properties either by macro or via the vault.
Then we also have macros that retrieve the information from the index property to format export names (STEP, IGES, STL...)
Thank you for your answer, you don't use revision tables?
No, never implemented
That's why my revision is in the MEP.
When a new row is created in the table, the " Revision " property is automatically incremented. But it is in the MEP.
Hello
But what if the error comes from the plan, but not from the 3D?
At home has become complicated 
There is a room index and a plan index.
We indicate on the general plans in the nomenclature the index of the piece. And in the detail shots too.
This information is independent of each other.
If the 3D part changes, the 3D evolves and the plan inevitably goes up as well.
If the plan evolves (e.g. a nota or other) the plan goes up by index but not the piece?
You can link the subscript of the plan and the room, you have to recreate a custom property chain with a term different from the subscript of the plan. That said, the plan index will continue to exist. You have to recreate text linked to a property in the title block and in the revision bar.
Hello,
With us it's just the same as @Cyril_f : it's the 3D that carries the clue (which is easy to retrieve in the 2D as a result).
NB: in practice the 2 have an index that is mounted in parallel, but the main one remains that of 3D.
To answer @FRED78's question, we mount a hint on the 3D even if the modification is only done in practice on the 2D (like adding a nota) because a small note can have a big impact on the part (even if its 3D geometry does not change).
What is the string to bind this property?
Used perhaps for the wrong purpose, I was thinking of a chain from 3D to MEP, part - assembly, assembly - plan. And to forward a link (the clue) from 3D to 2D.
But I probably expressed myself badly
Here's a macro that replaces the " Revision" property of the part or assembly with the "Revision " property of the MEP.
Option Explicit
Dim PrtPath As String
Dim AsmPath As String
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swDrawModel As SldWorks.ModelDoc2
Dim swDrawModelDocExt As ModelDocExtension
Dim swDrawCustProp As CustomPropertyManager
Dim swDrawDoc As SldWorks.DrawingDoc
Dim swDrawView As SldWorks.View
Dim DrawVal As String
Dim DrawRevision As String
Dim DrawBool As Boolean
Dim swRefModel As SldWorks.ModelDoc2
Dim swRefPath As String
Dim swRefModelDocExt As ModelDocExtension
Dim swRefCustProp As CustomPropertyManager
Dim RefReturn As Integer
Dim RefBool As Boolean
Dim RefVal As String
Dim RefRevision As String
Dim RefDocType As swDocumentTypes_e
Dim FileError As Long
Dim FileWarning As Long
Set swApp = Application.SldWorks
Set swDrawModel = swApp.ActiveDoc
If swDrawModel Is Nothing Then
swApp.SendMsgToUser2 "Ouvrir un fichier mise en plan", swMbWarning, swMbOk
Exit Sub
End If
If swDrawModel.GetType <> swDocDRAWING Then 'swDocASSEMBLY, swDocPART
swApp.SendMsgToUser2 "Ouvrir un fichier mise en plan", swMbWarning, swMbOk
Exit Sub
Else
RefDocType = RefDocTypeSearch(swDrawModel.GetPathName)
Select Case RefDocType
Case swDocPART
Set swRefModel = swApp.OpenDoc6(PrtPath, swDocPART, swOpenDocOptions_Silent, "", FileError, FileWarning)
Debug.Print "PrtPath = " & PrtPath
Debug.Print "FileError = " & FileError
Debug.Print "FileWarning = " & FileWarning
Case swDocASSEMBLY
Set swRefModel = swApp.OpenDoc6(AsmPath, swDocASSEMBLY, swOpenDocOptions_Silent, "", FileError, FileWarning)
Debug.Print "AsmPath = " & AsmPath
Debug.Print "FileError = " & FileError
Debug.Print "FileWarning = " & FileWarning
End Select
If Not swRefModel Is Nothing Then
swRefPath = swRefModel.GetPathName
If IsFileExist(swRefModel.GetPathName) Then
Set swDrawModelDocExt = swDrawModel.Extension
Set swDrawCustProp = swDrawModelDocExt.CustomPropertyManager("")
DrawBool = swDrawCustProp.Get4("Révision", False, DrawVal, DrawRevision)
Debug.Print "DrawBool = " & DrawBool
Debug.Print "DrawRevision = " & DrawRevision
Set swRefModelDocExt = swRefModel.Extension
Set swRefCustProp = swRefModelDocExt.CustomPropertyManager("")
RefReturn = swRefCustProp.Set("Révision", DrawRevision)
Debug.Print "RefReturn = " & RefReturn
RefBool = swRefCustProp.Get4("Révision", False, RefVal, RefRevision)
Debug.Print "RefModelPath = " & swRefModel.GetPathName
Debug.Print "RefBool = " & RefBool
Debug.Print "RefRevision = " & RefRevision
End If
End If
End If
End Sub
Function RefDocTypeSearch(DrawPath As String) As swDocumentTypes_e
Dim DrawPathLow As String
DrawPathLow = LCase(DrawPath)
Debug.Print "DrawPath = " & DrawPath
Debug.Print "DrawPathLow = " & DrawPathLow
PrtPath = Replace(DrawPathLow, "slddrw", "sldprt")
AsmPath = Replace(DrawPathLow, "slddrw", "sldasm")
If IsFileExist(PrtPath) Then
RefDocTypeSearch = swDocPART
Exit Function
End If
If IsFileExist(AsmPath) Then
RefDocTypeSearch = swDocASSEMBLY
End If
End Function
Function IsFileExist(FullName As String) As Boolean
' Vérifie l'existence d'un fichier
IsFileExist = Dir(FullName) <> ""
End Function
Assembly, part, and MEp files must be in the same folder
Happy Birthday from Forum @remrem 
!
Thanks for macro sharing. (The key will be to remember to launch it regularly ).
Be careful for those who use " Revision " (without accent), it will be necessary to modify the code slightly...
Thank you. 
I signed up in 2013 and already had white hair 
Happy birthday forum one of the very rare, much older than me!
And for me still very little white hair! 
@remrem , I took the liberty of starting from your macro to make it a little more " universal " (don't blame me).
The changes are mainly focused on double reading
" Revision " versus " Revision ".
I also used the " Perplexity " AI to add text comments (AIs are still only good at this but it's still very practical).
In theory, compatibility with the Solidworks > 2022 version is also increased. (but I can't test!).
Tip:
For those who own the " Mycad " Suite, this version is supposed to be compatible with its use in Smartproperties (and therefore automatable when closing the Smartproperties Window (in the event that your revisions are generated with this utility).
This should greatly reduce the risk of bad revision between 3D and Drawings...
Example:
Option Explicit
' =====================================================
' DÉCLARATIONS GLOBALES
' =====================================================
' Ces variables globales stockent les chemins des fichiers pièce (.sldprt) et assemblage (.sldasm)
' détectés automatiquement à partir du chemin de la mise en plan (.slddrw).
' Pourquoi globales ? Pour qu'elles soient accessibles par toutes les fonctions de la macro.
Dim PrtPath As String ' Chemin complet vers la pièce référencée
Dim AsmPath As String ' Chemin complet vers l'assemblage référencé
' =====================================================
' PROCÉDURE PRINCIPALE : main()
' =====================================================
' BUT : Synchroniser la propriété "Révision/Revision" de la mise en plan vers son modèle référencé
' (pièce ou assemblage). Fonctionne avec SolidWorks 2022 et ses spécificités API.
Sub main()
On Error GoTo GestionErreur ' Gestion centralisée des erreurs
' =====================================================
' DÉCLARATION DES OBJETS SOLIDWORKS
' =====================================================
' swApp : Instance principale de SolidWorks (toujours accessible via Application.SldWorks)
Dim swApp As SldWorks.SldWorks
' swDrawModel : Document actif (la mise en plan)
Dim swDrawModel As SldWorks.ModelDoc2
' Extensions et gestionnaires de propriétés personnalisées
Dim swDrawModelDocExt As ModelDocExtension
Dim swDrawCustProp As CustomPropertyManager
' Modèle référencé (pièce ou assemblage à synchroniser)
Dim swRefModel As SldWorks.ModelDoc2
Dim swRefModelDocExt As ModelDocExtension
Dim swRefCustProp As CustomPropertyManager
Dim RefDocType As swDocumentTypes_e ' Type du document référencé
' =====================================================
' VARIABLES UTILITAIRES
' =====================================================
Dim DrawRevision As String ' Valeur de révision dans la mise en plan
Dim RefRevision As String ' Valeur de révision dans le modèle
Dim PropName As String ' Nom exact de la propriété (ex: "Revision" ou "Révision")
Dim FileError As Long ' Code d'erreur ouverture fichier
Dim FileWarning As Long ' Code d'avertissement ouverture fichier
Dim Msg As String ' Message informatif
Dim addRes As Long ' Résultat de l'ajout de propriété
' =====================================================
' ÉTAPE 1 : CONNEXION À SOLIDWORKS ET VÉRIFICATIONS
' =====================================================
Set swApp = Application.SldWorks ' Récupère l'instance SolidWorks courante
Set swDrawModel = swApp.ActiveDoc ' Document actif = mise en plan
' Vérification : un document doit être actif
If swDrawModel Is Nothing Then
swApp.SendMsgToUser2 "Aucun document actif. Ouvrez une mise en plan.", swMbWarning, swMbOk
Exit Sub
End If
' Vérification : le document actif DOIT être une mise en plan (.slddrw)
If swDrawModel.GetType <> swDocDRAWING Then
swApp.SendMsgToUser2 "Le document actif n'est pas une mise en plan.", swMbWarning, swMbOk
Exit Sub
End If
' =====================================================
' ÉTAPE 2 : DÉTECTION DU MODÈLE RÉFÉRENCÉ
' =====================================================
' Recherche automatique du fichier .sldprt ou .sldasm correspondant au .slddrw
RefDocType = RefDocTypeSearch(swDrawModel.GetPathName)
If RefDocType = 0 Then
swApp.SendMsgToUser2 "Aucun modèle référencé trouvé (.sldprt ou .sldasm).", swMbWarning, swMbOk
Exit Sub
End If
' =====================================================
' ÉTAPE 3 : OUVERTURE SILENCIEUSE DU MODÈLE
' =====================================================
' Ouverture sans interface utilisateur (swOpenDocOptions_Silent)
Select Case RefDocType
Case swDocPART ' Pièce
Set swRefModel = swApp.OpenDoc6(PrtPath, swDocPART, swOpenDocOptions_Silent, "", FileError, FileWarning)
Case swDocASSEMBLY ' Assemblage
Set swRefModel = swApp.OpenDoc6(AsmPath, swDocASSEMBLY, swOpenDocOptions_Silent, "", FileError, FileWarning)
End Select
' Vérification ouverture réussie
If swRefModel Is Nothing Or FileError <> 0 Then
swApp.SendMsgToUser2 "Échec ouverture modèle.", swMbStop, swMbOk
Exit Sub
End If
' =====================================================
' ÉTAPE 4 : LECTURE PROPRIÉTÉS M ISE EN PLAN
' =====================================================
Set swDrawModelDocExt = swDrawModel.Extension
Set swDrawCustProp = swDrawModelDocExt.CustomPropertyManager("") ' Propriétés document ("" = niveau document)
' DÉTECTION INTELLIGENTE du nom exact de la propriété révision
PropName = DetectRevisionPropertyFixed(swDrawCustProp)
Debug.Print "=== PROPNAME FINAL : '" & PropName & "' ===" ' Debug pour développeur
If PropName = "" Then
swApp.SendMsgToUser2 "Aucune propriété Révision/Revision trouvée.", swMbStop, swMbOk
GoTo NettoyageSimple
End If
' Lecture de la valeur (avec fallback si vide)
If Not GetCustomPropValue(swDrawCustProp, PropName, DrawRevision) Then
DrawRevision = "NON_RENSEIGNÉ" ' Valeur par défaut
Debug.Print "Valeur mise en plan vide ? fallback"
End If
Debug.Print "Valeur À SYNCHRONISER : '" & DrawRevision & "'"
' =====================================================
' ÉTAPE 5 : ACCÈS PROPRIÉTÉS MODÈLE RÉFÉRENCÉ
' =====================================================
Set swRefModelDocExt = swRefModel.Extension
Set swRefCustProp = swRefModelDocExt.CustomPropertyManager("") ' Propriétés du modèle
' =====================================================
' ÉTAPE 6 : SYNCHRONISATION (CRU DE LA MACRO)
' =====================================================
Debug.Print "--- DÉBUT SYNCHRO ---"
' ? IMPORTANT SolidWorks 2022 : Force la reconstruction pour rafraîchir les propriétés
swRefModel.ForceRebuild3 False ' False = ne pas afficher les messages
' Test 1 : La propriété existe-t-elle déjà dans le modèle ?
If GetCustomPropValue(swRefCustProp, PropName, RefRevision) Then
Debug.Print " ? Propriété existe : '" & RefRevision & "'"
If RefRevision <> DrawRevision Then
Debug.Print " ? MISE À JOUR nécessaire"
' Mise à jour de la valeur existante
Dim setRes As Long
setRes = swRefCustProp.Set2(PropName, DrawRevision) ' Set2 = mise à jour
Debug.Print " ? Set2 retour : " & setRes
If setRes = 0 Then
Msg = "? " & PropName & " mise à jour : " & DrawRevision
Else
Msg = "? Échec mise à jour " & PropName
End If
Else
Msg = "? Déjà OK : " & PropName & " = " & DrawRevision
End If
Else
Debug.Print " ? CRÉATION propriété manquante"
' Création avec Add2 (stable sur SolidWorks 2022)
addRes = swRefCustProp.Add2(PropName, swCustomInfoText, DrawRevision)
Debug.Print " ? Add2 retour : " & addRes
If addRes = 0 Or addRes = 2 Then ' 0=OK, 2=existe déjà
Msg = "? " & PropName & " créée : " & DrawRevision
Else
' Fallback Add3 si Add2 échoue
addRes = swRefCustProp.Add3(PropName, swCustomInfoText, DrawRevision, 0)
Debug.Print " ? Add3 fallback retour : " & addRes
If addRes = 0 Or addRes = 2 Then
Msg = "? " & PropName & " créée (Add3) : " & DrawRevision
Else
Msg = "? ÉCHEC création " & PropName & " (Add2=" & addRes & ", Add3=" & addRes & ")"
End If
End If
End If
' Debug.Print "--- SYNCHRO TERMINÉE : " & Msg & " ---"
' swApp.SendMsgToUser2 Msg, swMbInformation, swMbOk ' Décommentez pour voir le résultat
' =====================================================
' NETTOYAGE : FERMETURE MODÈLE
' =====================================================
NettoyageSimple:
If Not swRefModel Is Nothing Then
On Error Resume Next ' Ignore erreurs de fermeture
swApp.CloseDoc swRefModel.GetPathName ' Ferme sans sauvegarde
On Error GoTo 0 ' Restaure gestion erreurs normale
End If
Exit Sub
' =====================================================
' GESTION D'ERREUR CENTRALE
' =====================================================
GestionErreur:
swApp.SendMsgToUser2 "Erreur : " & Err.Description, swMbStop, swMbOk
Debug.Print "ERREUR # " & Err.Number & " : " & Err.Description
Resume NettoyageSimple ' Nettoyage avant sortie
End Sub
' =====================================================
' FONCTION : DetectRevisionPropertyFixed()
' =====================================================
' BUT : Détecte intelligemment le nom exact de la propriété révision
' Teste d'abord "Revision" ? "Révision" ? scan complet des propriétés
Function DetectRevisionPropertyFixed(CustMgr As CustomPropertyManager) As String
Dim propNames As Variant
Dim i As Long
Dim PropName As String
Dim propVal As String
Debug.Print "=== SCAN COMPLET ==="
' 1?? PRIORITÉ 1 : Test direct "Revision" (standard anglais)
If CustMgr.Get4("Revision", False, "", propVal) Then
DetectRevisionPropertyFixed = "Revision"
Debug.Print "? DIRECT : Revision"
Exit Function
End If
' 2?? PRIORITÉ 2 : Test "Révision" (standard français)
If CustMgr.Get4("Révision", False, "", propVal) Then
DetectRevisionPropertyFixed = "Révision"
Debug.Print "? DIRECT : Révision"
Exit Function
End If
' 3?? PRIORITÉ 3 : Scan complet de TOUTES les propriétés
propNames = CustMgr.GetNames ' Tableau des noms de propriétés
Debug.Print "Nb props: " & IIf(IsEmpty(propNames), 0, UBound(propNames) + 1)
If Not IsEmpty(propNames) Then
For i = 0 To UBound(propNames)
PropName = CStr(propNames(i))
Debug.Print "Prop " & i & ": '" & PropName & "'"
' Recherche insensible à la casse contenant "revision"
If InStr(LCase(PropName), "revision") > 0 Then
DetectRevisionPropertyFixed = PropName
Debug.Print "? TROUVÉ : '" & PropName & "'"
Exit Function
End If
Next i
End If
Debug.Print "? RIEN TROUVÉ"
DetectRevisionPropertyFixed = "" ' Aucune propriété trouvée
End Function
' =====================================================
' FONCTION : GetCustomPropValue()
' =====================================================
' BUT : Lit une propriété personnalisée avec gestion des valeurs vides
' RETOUR : True si propriété existe, False sinon
Function GetCustomPropValue(CustMgr As CustomPropertyManager, PropName As String, ByRef PropValue As String) As Boolean
Dim res As Boolean
Dim valOut As String, valEval As String ' valEval = valeur évaluée (résolue)
On Error Resume Next ' Ignore erreurs Get4
res = CustMgr.Get4(PropName, False, valOut, valEval) ' Lecture propriété
On Error GoTo 0 ' Restaure gestion erreurs
Debug.Print " Get4('" & PropName & "') ? res=" & res & " | val='" & valEval & "'"
If res Then
PropValue = IIf(valEval = "", "VIDE", valEval) ' Gère les valeurs vides
GetCustomPropValue = True
Else
PropValue = ""
GetCustomPropValue = False
End If
End Function
' =====================================================
' FONCTION : RefDocTypeSearch()
' =====================================================
' BUT : Détecte si le chemin .slddrw pointe vers .sldprt OU .sldasm
' Remplit les variables globales PrtPath/AsmPath
Function RefDocTypeSearch(DrawPath As String) As swDocumentTypes_e
Dim DrawPathLow As String
DrawPathLow = LCase(DrawPath) ' Minuscules pour comparaison
' Conversion automatique des noms de fichiers
PrtPath = Replace(DrawPathLow, "slddrw", "sldprt") ' Mise en plan ? Pièce
AsmPath = Replace(DrawPathLow, "slddrw", "sldasm") ' Mise en plan ? Assemblage
Debug.Print "Test pièce : " & PrtPath & " ? " & IIf(IsFileExist(PrtPath), "OK", "KO")
Debug.Print "Test assem : " & AsmPath & " ? " & IIf(IsFileExist(AsmPath), "OK", "KO")
If IsFileExist(PrtPath) Then
RefDocTypeSearch = swDocPART
Exit Function
End If
If IsFileExist(AsmPath) Then
RefDocTypeSearch = swDocASSEMBLY
End If ' Retourne 0 si aucun fichier trouvé
End Function
' =====================================================
' FONCTION UTILITAIRE : IsFileExist()
' =====================================================
' BUT : Teste l'existence d'un fichier sur disque
Function IsFileExist(FullName As String) As Boolean
IsFileExist = (Dir(FullName) <> "") ' VBA standard : Dir retourne "" si fichier inexistant
End Function
I don't blame you.
AI is good but do you understand what it does?
The comments sometimes contain questions because she doesn't understand everything and some elements sting my eyes such as the " On error " which is to be avoided because it does not allow to locate the defects.
My code is certainly not exhaustive but the error management by managing it will allow me (it is expected) to alert the user according to the errors.