Can someone help me out with the macro

Below is a simple macro to export the current drawing as a DXF file to
N:\DXF. As you can see, it names the DXF "Draw1.dxf". How can I edit
the macro to so the dxf filename is the same filename as the
SolidWorks drawing, which is our part numbering system. Thanks in
advance.


Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long
Dim Annotation As Object
Dim Gtol As Object
Dim DatumTag As Object
Dim FeatureData As Object
Dim Feature As Object
Dim Component As Object
Sub main()

Set swApp = Application.SldWorks

Set Part = swApp.ActiveDoc
Part.SaveAs2 "N:\DXF\Draw1.DXF", 0, True, False
End Sub

 

This should work.............

Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long
Dim Annotation As Object
Dim Gtol As Object
Dim DatumTag As Object
Dim FeatureData As Object
Dim Feature As Object
Dim Component As Object
Dim PartTitle As String

Sub main()

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc

PartTitle = Part.GetTitle

Part.SaveAs2 "N:\DXF\" & PartTitle & ".DXF", 0, True, False
End Sub

 

Dim swApp As Object
Dim Part As Object
dim partitle as string
dim partitlelen as integer
dim partName as string

Sub main()

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc

partitle = part.gettitle
partitlelen = len(partitle)
partname = left(partitle,partitlelen - (partitlelen -7))

Part.SaveAs2 "N:\DXF\" & partname & ".DXF", 0, True, False

End Sub

 

Thanks! Works great. One last question, is there a command to add to
this that would scale the drawing view 1:1 automatically before
exporting as a DXF?

 

Can we add a suffix to each part number while running this macro? In our
case "-01" to identify the first configuration.

Thanks in advance.

 

Dim swApp As Object
Dim Part As Object
dim partitle as string
dim partitlelen as integer
dim partName as string

Sub main()

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc

partitle = part.gettitle
partitlelen = len(partitle)
partname = left(partitle,partitlelen - (partitlelen -7))

'YOU CAN ADD A LINE LIKE THIS
SUFFIX = "-1"
Part.SaveAs2 "N:\DXF\" & partname & SUFFIX & ".DXF", 0, True, False

End Sub

If you need to get your config names

Dim Config As SldWorks.configuration

Set Config = Part.GetActiveConfiguration
ConfigName = Config.Name
Part.SaveAs2 "N:\DXF\" & partname & ConfigName & ".DXF", 0, True, False

 

Thanks Corey!

 

I couldnt get the 1:1 scale code to work. Maybe I placed it in the
wrong part of the macro. Can you explain. Thanks.

I also wanted to know if its possible to close the drawing without
saving after the DXF file has been created.

Thanks.

 

You have to rebuild after the 1:1

You have to do a rebuild you have finished scaling. Use the sub
below. This way if you want .25 scale or 1 or 2 or 50 you can call it
from another sub and specify the scale

Sub viewScale(MyScale As Double)
Dim swView As SldWorks.View
Dim swApp As SldWorks.SldWorks
Dim Part As DrawingDoc

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Set swView = Part.GetFirstView

'this while statement will traverse every view on the sheet

While Not swView Is Nothing
swView.ScaleDecimal = MyScale
Set swView = swView.GetNextView
Wend
Part.EditRebuild

End Sub

This should do it. I think that if you want to save you have to do a
Part.Save before CloseDoc

Dim ModelDocument as SldWorks.ModelDoc2
Set ModelDocument = Part
swApp.CloseDoc ModelDocument.GetTitle