Hello
Is it possible to export a view of an assembly in . DWG? (I arrive with a part, but not with an assembly)
Thank you
Have a nice day
Hello
You would have to temporarily save your assembly in PART to be able to export it in DWG.
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In fact, for the moment I'm going through the layout.
But I wanted to know if there was a faster one.
Unless you missed something, I don't think so.
Wait for another answer.
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through a drawing ;-)
simply save the assembly as a part and select all the components, then treat this new part like any traditional part (export to DXF, DWG)
@+ ;-)
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Basically, that's what I'm already doing^^
So it doesn't get any simpler than that, straight from the assembly.
Thank you for your answers;)
Hello
To avoid all these steps you can also make a small macro that automates the transformation of the asm into prt and then exports it to DWG, it will only take you one click to achieve what you want.
For the backup of the asm in prt it's a simple Part.Saveas3(nomprt, 0, 0) to do and for the export in DWG you should be able to use the macro : http://help.solidworks.com/2016/english/api/sldworksapi/export_part_to_dwg_example_vb.htm
Kind regards
3 Likes
The previous macro uses the "ExportFlatPatternView" function which is deprecated and only transfers the front view, this one uses the "ExportToDWG2" replacement function and allows you to create a DWG of each view, I think it will be more in line with what you want to do.
Kind regards
asmtodwg-v2.swp
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Thank you very much
I never used the Macro, can you explain it to me in two words?
Thank you
Hello
Which version of SW are you on? The libraries loaded in my macro are for SW2017.
In SW, you can do: Tools / Macro / New and copy the code below to replace the one that is automatically written in the new macro then you load a test assembly in SW and finally you do F5 in the Visual Basic window.
Kind regards
Dim swApp As Object
Public swModel As SldWorks.ModelDoc2
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set Part = swApp.ActiveDoc
Dim myModelView As Object
Set myModelView = Part.ActiveView
myModelView.FrameState = swWindowState_e.swWindowMaximized
'on récupére le document actif
Set swModel = swApp.ActiveDoc
If Not swModel Is Nothing Then
'on récupére l'emplacement du fichier
stPath = swModel.GetPathName
'on récupére le nombre de caractére jusqu'au . de l'extension
lgFichier = InStrRev(stPath, ".", -1, vbTextCompare) - 1
'on récupére le chemin sans l'extention
If lgFichier > 0 Then
stPath = Left(stPath, lgFichier)
End If
'si le document est un assemblage
If swModel.GetType = swDocASSEMBLY Then
'on créer le SLDPRT
longstatus = Part.SaveAs3(stPath + ".sldprt", 0, 0)
'On ferme le SDLASM
swApp.CloseDoc swModel.GetTitle
'On ouvre le SLDPRT
Set swModel = swApp.OpenDoc6(stPath + ".sldprt", 1, 0, "", longstatus, longwarnings)
End If
'si le document est une pièce
If swModel.GetType = swDocPART Then
'On l'exporte en DWG
ExportDWG
End If
End If
End Sub
Sub ExportDWG()
Dim swPart As SldWorks.PartDoc
Dim sModelName As String
Dim sPathName As String
Dim varAlignment As Variant
Dim dataAlignment(11) As Double
Dim varViews As Variant
Dim dataViews(5) As String
Dim options As Long
Set swModel = swApp.ActiveDoc
sModelName = swModel.GetPathName
sPathName = swModel.GetPathName
sPathName = Left(sPathName, Len(sPathName) - 6)
sPathName = sPathName + "dwg"
Set swPart = swModel
dataAlignment(0) = 0#
dataAlignment(1) = 0#
dataAlignment(2) = 0#
dataAlignment(3) = 1#
dataAlignment(4) = 0#
dataAlignment(5) = 0#
dataAlignment(6) = 0#
dataAlignment(7) = 1#
dataAlignment(8) = 0#
dataAlignment(9) = 0#
dataAlignment(10) = 0#
dataAlignment(11) = 1#
varAlignment = dataAlignment
dataViews(0) = "*En cours"
dataViews(1) = "*Face"
dataViews(2) = "*Droite"
dataViews(3) = "*Gauche"
dataViews(4) = "*Dessus"
dataViews(5) = "*Arrière"
varViews = dataViews
swPart.ExportToDWG2 sPathName, sModelName, swExportToDWG_ExportAnnotationViews, False, varAlignment, False, False, 0, varViews
End Sub
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Hello, I record the whole thing in room and then I make a dwg.
Kind regards
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I'm in 2016 sp3
Hello
That's where the vba annoys me a little ...
Try replacing the lines:
'If the document is a document
If swModel.GetType = swDocPART Then
'We export it in DWG
ExportDWG
End If
by:
'If the document is a document
If swModel.GetType = swDocPART Then
'We export it in DWG
ExportDWG swModel
End If
Then the line:
Sub ExportDWG
By:
Sub ExportDWG(swModel As SldWorks.ModelDoc2)
And again the line (the one in the Sub ExportDWG(.....):
Set swModel = swApp.ActiveDoc
By:
'Set swModel = swApp.ActiveDoc
Load your assembly and then launch the macro with F5
Kind regards
1 Like
How can I get the same macro for the parts alone?
I have a way to modify the macro alone to learn
Hello
For the parts alone it's the same macro since in this one I transform the asm into prt then I launch the transformation into dwg on the prt so you load a part then you launch the macro and you normally get the 6 DWG created in the Windows folder of the part, At least for me it works too.
Kind regards
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Thank you very much for your help;)