English view

2D plans Layout
1

Hello

When I make the 2d plan of an assembly I notice that the views are English (top view above) 

On solid 2018 I can't find the option for the views to be in iso

Thank you

2

Hello

US views you mean?

Right-click on the plan sheet > Properties > Projection type (check Europe or USA)


vues.png
6 Likes
3

re

ok it works, but how to set to have it by default

1 Like
4

Re

In the SolidWorks banner > Save/Restore Settings > Tools


bandeau.png
2 Likes
5

It's better to have a file in US view than a file that runs in English.

 

NOoooon not banging the head.............. Too late is already far away

7 Likes
6

To have it by default, you have to modify the document template (DRWDOT) and the basemaps (SLDDRT)

For existing shots, a clickable macro can be useful but it will return the views

Personally I use this to reload the basemaps:

Sub main()

Dim swApp           As SldWorks.SldWorks
Dim swModel         As SldWorks.ModelDoc2
Dim swDraw          As SldWorks.DrawingDoc
Dim swSheet         As SldWorks.Sheet
Dim vSheetProps     As Variant
Dim nErrors         As Long
Dim nWarnings       As Long
Dim sFileName       As String
Dim Path            As String
Dim vSheetName      As Variant
Dim i               As Long
Dim Part            As Variant


'***************************************
' Location des fonds de plans
Const sTemplatePath As String = "****A REMPLACER PAR LE DOSSIER CONTENANT LES FOND DE PLANS"

' Noms des templates
'Première page
Const sTemplateName As String = "***A REMPLACER PAR NOM DE FOND DE PLAN PREMIERE PAGE .SLDDRT"
Autres pages
Const sTemplateName2 As String = "***A REMPLACER PAR NOM DE FOND DE PLAN AUTRES PAGES .SLDDRT"
'***************************************
'vérification si plan ouvertt
On Error Resume Next
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
' Check to see if a drawing is loaded.
If swModel Is Nothing Then
        MsgBox "Il faut ouvrir un plan avant de lancer la macro !"
        Exit Sub
End If
If swModel.GetType <> swDocDRAWING Then
        MsgBox "Il faut ouvrir un plan avant de lancer la macro !"
        Exit Sub
End If
'***************************************
'*************************************** Hop, on se charge de la page 1
Set swDraw = swModel
    vSheetName = swDraw.GetSheetNames
        swDraw.ActivateSheet (vSheetName(i))
        Set swSheet = swDraw.GetCurrentSheet
        vSheetProps = swSheet.GetProperties
        
    'Supression de la table "feuille x/x"
    Set Part = swApp.ActiveDoc
    boolstatus = Part.Extension.SelectByID2("", "ANNOTATIONTABLES", 0.361350915138288, 7.25042891639636E-02, 0, False, 0, Nothing, 0)
    Part.EditDelete
    
    'Chargement du nouveau fond de plan
    swModel.SetupSheet5 swSheet.GetName, swDwgPapersUserDefined, swDwgTemplateCustom, vSheetProps(2), vSheetProps(3), True, sTemplatePath & sTemplateName, 0.4318, 0.2794, "Default", True
    swDraw.ViewZoomtofit2
    
    'Selection du calque "selon la norme"
    Set Part = swApp.ActiveDoc
    Set LayerMgr = Part.GetLayerManager
    LayerMgr.SetCurrentLayer ("-Selon la norme-")


'*************************************** Puis toutes les autres pages
For i = 1 To UBound(vSheetName)

        swDraw.ActivateSheet (vSheetName(i))
        Set swSheet = swDraw.GetCurrentSheet
        vSheetProps = swSheet.GetProperties
        
        'Supression de la table "feuille x/x"
        Set Part = swApp.ActiveDoc
        boolstatus = Part.Extension.SelectByID2("", "ANNOTATIONTABLES", 0.361350915138288, 7.25042891639636E-02, 0, False, 0, Nothing, 0)
        Part.EditDelete
        
        'Chargement du nouveau fond de plan
        swModel.SetupSheet5 swSheet.GetName, swDwgPapersUserDefined, swDwgTemplateCustom, vSheetProps(2), vSheetProps(3), True, sTemplatePath & sTemplateName2, 0.4318, 0.2794, "Default", True
        swDraw.ViewZoomtofit2
        
        'Selection du calque "selon la norme"
        Set Part = swApp.ActiveDoc
        Set LayerMgr = Part.GetLayerManager
        LayerMgr.SetCurrentLayer ("-Selon la norme-")

'*************************************** Sauvegarde et fin
Next i
    swDraw.ActivateSheet vSheetName(0)
    swDraw.ForceRebuild3 False
    swDraw.Save3 1, nErrors, nWarnings
        
Set swDraw = Nothing
   

End Sub


 

1 Like
7

Indeed, the correct answer is the cumulation between  @Vincent G and @ DELACOTE.

You have to open the drawing "template" by pressing "Open" and put the "Templates" extension and open the "Layout.drwdot" file to open the default template.

Then, you have to change the "Sheet Property" to "Europe" Projection Type and press Ok.

Save the template and close.

At the next shot, the Projection Type will be European by default.

There you go

3 Likes
8

This is how you set the model correctly because a lot of parameters have to be modified (Document Options/Properties): Views (including sections), dimensions, annotations, ...

3 Likes
9

You can create your own tab when opening new documents by creating your own templates (Part, Assembly and Drawing) in a personal folder (Put your name to the folder; this is the name of the tab).

Then point to this folder (Option / File Locations / Document Templates and press "Add" and go to the folder with your templates.

3 Likes
10

Hello

Ok I created a drawing 1 that I saved and then I set it to default.

Thank you for your help