Hello
Is it possible to apply a document template to an older part or assembly?
Basically, I'd like to be able to update the document properties (option => Document properties => Wrapping standard, ...) and add all the custom properties to the template without deleting the old custom properties.
Thank you for your feedback
Hello
Natively this is not possible (you can at best add properties with the task scheduler).
By macro or maybe in the Visiativ tools (MyCadTool) I don't see any other solution.
Via Integration you should be able to do this.
For the standard:
For Properties:
Attached is the help of Integration, it is a paid Visiativ utility, but it is possible to test it for a month of memory.
Otherwise via macro it's feasible since the utility based on the solidworks API does it, but you'll have to look for the ready-made equivalent or write it, if nothing equivalent.
Edit: an example of a macro to change the Hgabillage:
https://help.solidworks.com/2022/english/api/sldworksapi/Change_Drafting_Standard_to_Custom_Example_VB.htm
Hello;
There is no simple solution on this subject...
However, and if it does not concern a large number of files, it is possible to use my solution discussed in the topic:
…
Hello;
For an Assembly, it is always possible to drag it into a document template *. SLDASM (new Assembly document), then decompose it (right-click) to return to its original FeatureTree.
… and save the new assembly.
For the parts it's slightly more complicated (but not that much).
Insert your component into a new document part (document template) as if you were making a derivative part, Check the " Break the link with the original part" option:
Kind regards.
It's ingenious as a technique, on the other hand for the parts seems to me that it's not as simple as you described, I imagine that any link to assembly or function in the context, child derivative part or drawing will be lost
→ @Lynkoa15
Indeed, this implies "breaking" all external references and re-associating the drawings and assemblies.
For the more "MACRO-teux" this macro also does a good part of the JOB: To customize according to your location of the Norms and templates files...
-For advanced users only...
Dim Part As Object
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModExt As SldWorks.ModelDocExtension
Dim NormeActive As String
Dim DefaultSlotMate As String
Sub Norme()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swModExt = swModel.Extension
NormeActive = swModExt.GetUserPreferenceString(SwConst.swDetailingDimensionStandardName, SwConst.swDetailingNoOptionSpecified) 'Ecrit la Norme existante du fichier ouvert dans la variable
Debug.Print NormeActive
ModelDoc = swModel.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplateAssembly)
Debug.Print ModelDoc
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
filetype = swModel.GetType 'Donne le type de document ouvert avec :0=swDocNONE;1=swDocPART;2=swDocASSEMBLY;3=swDocDRAWING
If filetype = 1 Then
boolstatus = Part.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\Emplacement de votre modele PRT.sldstd") '<- Emplacement exacte du fichier sldstd pour vos pièces
End If
If filetype = 2 Then 'Si le fichier ouvert est un Assemblage
boolstatus = Part.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\Emplacement de votre modele ASM.sldstd") '<- Emplacement exacte du fichier sldstd pour vos Assemblages
defaultTemplate = "W:\Modeles_solidworks\Assemblage .asmdot"
End If
If filetype = 3 Then 'Si le fichier ouvert est une Mise en plan
Call Formats
End If
End Sub
-> Dans un nouveau Module
Dim vSheetProps As Variant
Dim nErrors As Long
Dim nTemplatePath As String
Dim swPaperWidth As String
Dim swPaperHeight As String
' Repertoire contenant les modeles des fonds de plans
Const sTemplatePath As String = "W:\Modeles_solidworks\Fonds_de_plans_2023"
' Formats des differents fond de plans disponibles dans le Repertoire ci-dessous
Const A0HTemplateName As String = "A0H.slddrt"
Const A1HTemplateName As String = "A1H.slddrt"
Const A1VTemplateName As String = "A1V.slddrt"
Const A2HTemplateName As String = "A2H.slddrt"
Const A2VTemplateName As String = "A2V .slddrt"
Const A3HTemplateName As String = "A3H.slddrt"
Const A3VTemplateName As String = "A3V.slddrt"
Const A4HTemplateName As String = "A4H.slddrt"
Const A4VTemplateName As String = "A4V.slddrt"
Sub Formats()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim vSheetProps As Variant
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
Set swSheet = swDraw.GetCurrentSheet
'swModel.ActivateSheet vSheetName
Set swSheet = swModel.GetCurrentSheet
vSheetProps = swSheet.GetProperties
swPaperWidth = vSheetProps(5)
swPaperHeight = vSheetProps(6)
Select Case swPaperWidth & swPaperHeight ' Comparaison de la Longueur et de la Largeur du fond de plan present (Unité en Metres)
Case "1,189" & "0,841" ' Format A0H
nTemplatePath = sTemplatePath & "\" & A0HTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A0.sldstd")
Case "0,841" & "0,594" ' Format A1H
nTemplatePath = sTemplatePath & "\" & A1HTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A1.sldstd")
Case "0,594" & "0,841" ' Format A1V
nTemplatePath = sTemplatePath & "\" & A1VTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A1.sldstd")
Case "0,594" & "0,42" ' Format A2H
nTemplatePath = sTemplatePath & "\" & A2HTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A2.sldstd")
Case "0,42" & "0,594" ' Format A2V
nTemplatePath = sTemplatePath & "\" & A2VTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A2.sldstd")
Case "0,42" & "0,297" ' Format A3H
nTemplatePath = sTemplatePath & "\" & A3HTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A3.sldstd")
Case "0,297" & "0,42" ' Format A3V
nTemplatePath = sTemplatePath & "\" & A3VTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A3.sldstd")
Case "0,297" & "0,21" ' Format A4H
nTemplatePath = sTemplatePath & "\" & A4HTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A4.sldstd")
Case "0,21" & "0,297" ' Format A4V
nTemplatePath = sTemplatePath & "\" & A4VTemplateName
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\A4.sldstd")
Case Else
nTemplatePath = sTemplatePath & "\" & A2HTemplateName 'Format par défaut si le fond de plan present n'est pas dans la liste ci-dessus
boolstatus = swModel.Extension.LoadDraftingStandard("W:\Modeles_solidworks\Normes_de_mise_en_plans\ISO-REVTECH_A2.sldstd")
End Select
'On Supprime le fond de plan initial
swModel.SetupSheet5 swSheet.GetName, swDwgPapersUserDefined, swDwgTemplateNone, vSheetProps(2), vSheetProps(3), vSheetProps(4), "", vSheetProps(5), vSheetProps(6), "Default", True
'On Recharge le nouveau fond de plan
swModel.SetupSheet5 swSheet.GetName, swDwgPapersUserDefined, swDwgTemplateCustom, vSheetProps(2), vSheetProps(3), vSheetProps(4), nTemplatePath, vSheetProps(5), vSheetProps(6), "Default", True
swModel.ViewZoomtofit2
End Sub
Be careful to replace all the locations of the name and drawing files...
For the second part of this macro, I use format comparisons to determine
which "basemap" and MEP standard to use.
Kind regards.