Macro for drawing properties

2D plans
,
1

Hello

New to 3DExperience, I need to create the drawing templates that will be used with the platform. As the latter does not make links between physical products and drawings, I cannot import the properties of my parts and assemblies to the drawings by cross-referencing the attributes in the platform. 
To do this, I am currently using the MyCADTools Integration tool which allows me to write to SLDDRW files the properties retrieved on the part or assembly used in the document. Not all users in my company have the MyCADTools suite, so I'm calling on you for a macro that would allow me to replace the Integration tool and retrieve the SLDPRT/SLDASM properties to SLDDRW. 

Thank you in advance. 


proprietes_slddrw.jpg
2 
Sub Propriétées()

    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2

    Set swApp = CreateObject("SldWorks.Application")
    Set swModel = swApp.ActiveDoc

    Debug.Print "File = " + swModel.GetPathName

    Debug.Print "  Titre             = " + swModel.SummaryInfo(swSumInfoTitle)
    Text = swModel.SummaryInfo(swSumInfoTitle)
    Debug.Print "  Sujet            = " + swModel.SummaryInfo(swSumInfoSubject)
    Debug.Print "  Auteur            = " + swModel.SummaryInfo(swSumInfoAuthor)
    Debug.Print "  Mots clés         = " + swModel.SummaryInfo(swSumInfoKeywords)
    Debug.Print "  Commentaires      = " + swModel.SummaryInfo(swSumInfoComment)
    Debug.Print "  Enregistré par    = " + swModel.SummaryInfo(swSumInfoSavedBy)
    Debug.Print "  Créé le (01)      = " + swModel.SummaryInfo(swSumInfoCreateDate)
    Debug.Print "  Enregistré le (01)= " + swModel.SummaryInfo(swSumInfoSaveDate)
    Debug.Print "  Créé le (02) = " + swModel.SummaryInfo(swSumInfoCreateDate2)
    Debug.Print "  Enregistré le (02)= " + swModel.SummaryInfo(swSumInfoSaveDate2)
    
End Sub

Here is an example I have to display the info

 

3 
Sub Propriétées()

Dim boolstatus As Boolean
Dim lErrors As Long, lWarnings As Long
    
Set swApp = Application.SldWorks
Set CurrentDOC = swApp.ActiveDoc            'Document actif
Set swModel = swApp.ActiveDoc
Set swConfigMgr = swModel.ConfigurationManager
Set swCustPropMgr = swModel.Extension.CustomPropertyManager("")

Set swDraw = swModel
vSheets = swDraw.GetSheetNames
swDraw.ActivateSheet vSheets(0)             'Affiche la 1ère feuille : en cas d'assemblage avec des vues de pièces séparées (soudure)
                                            'la 1ère vue de la 1ère feuille à plus de chance d'être l'assemblage plutôt qu'une pièce
                                            
Set swView = swDraw.GetFirstView            'active/récupère le fond de plan pour les propriétées perso
Set swView = swView.GetNextView             'active/récupère la première vue pour les propriétées perso
Set swRefDoc = swView.ReferencedDocument    '3D de la mise en plan

NP = swRefDoc.GetCustomInfoValue("", "TA PROPRIETE PERSO") 'Récupère le TITRE du 3D
Existe_NP = swModel.GetCustomInfoValue("", "TA PROPRIETE PERSO") 'Teste l'existence de la propriétée dans la MEP

If Existe_NP <> NP Then
    swRefDoc.SummaryInfo(swSumInfoTitle) = NP 'TITRE 'Récapitulatif' du 3D
    swCustPropMgr.Delete "TA PROPRIETE PERSO"
    retVal = swCustPropMgr.Add2("TA PROPRIETE PERSO", swCustomInfoText, NP) 'TITRE 'Personnaliser'
    swModel.SummaryInfo(swSumInfoTitle) = NP 'TITRE 'Récapitulatif'
    swModel.SummaryInfo(swSumInfoAuthor) = "TA PROPRIETE PERSO 02" 'AUTEUR 'Récapitulatif'
    
    'Zoom sur la feuille avant enregistrement
    Dim swModelDocExt As SldWorks.ModelDocExtension
    Set swModelDocExt = swModel.Extension
    swModelDocExt.ViewZoomToSheet

    boolstatus = swRefDoc.Save3(swSaveAsOptions_Silent, lErrors, lWarnings) 'Sauvegarde le 3D
    boolstatus = swModel.Save3(swSaveAsOptions_Silent, lErrors, lWarnings) 'Sauvegarde la MEP
End If

End Sub

to adapt to your case

1 Like
4

Another lead, look at this one:

https://help.solidworks.com/2017/English/api/sldworksapi/Get_Custom_Properties_of_Referenced_Part_Example_VB.htm

or cell there:

https://www.codestack.net/solidworks-api/document/drawing/copy-view-properties/