Export Part to DWG Example (VB.NET)

This example shows how to export sheet metal and annotation views of a part to DWG files.

' ---------------------------------------------------------------------------

' Preconditions: Open:

' <SolidWorks_install_dir>\samples\HandsOn\weldedcorner\weldedcorner.sldprt

'

' Postconditions: Inspect the Immediate Window for the location of

' three exported drawings containing:

'        - flat pattern sheet metal

'        - *Current annotation view

'        - *Front annotation view

' --------------------------------------------------------------------------

Imports SolidWorks.Interop.sldworks

Imports SolidWorks.Interop.swconst

Imports System

Imports System.Diagnostics

Partial Class SolidWorksMacro

    Dim swModel As ModelDoc2

    Dim swPart As PartDoc

    Dim sModelName As String

    Dim sPathName As String

    Dim varAlignment As Object

    Dim dataAlignment(11) As Double

    Dim varViews As Object

    Dim dataViews(1) As String

    Dim options As Long

    Sub main()

        swModel = swApp.ActiveDoc

        sModelName = swModel.GetPathName

        sPathName = swModel.GetPathName

        sPathName = Left(sPathName, Len(sPathName) - 6)

        sPathName = sPathName + "dwg"

        swPart = swModel

        dataAlignment(0) = 0.0#

        dataAlignment(1) = 0.0#

        dataAlignment(2) = 0.0#

        dataAlignment(3) = 1.0#

        dataAlignment(4) = 0.0#

        dataAlignment(5) = 0.0#

        dataAlignment(6) = 0.0#

        dataAlignment(7) = 1.0#

        dataAlignment(8) = 0.0#

        dataAlignment(9) = 0.0#

        dataAlignment(10) = 0.0#

        dataAlignment(11) = 1.0#

        varAlignment = dataAlignment

        dataViews(0) = "*Current"

        dataViews(1) = "*Front"

        varViews = dataViews

 

        'Export each annotation view to a separate drawing file

        swPart.ExportToDWG(sPathName, sModelName, 3, False, varAlignment, False, False, 0, varViews)

 

        'Export flat pattern of the sheet metal to a single drawing file

        options = 13   '0001101 - include flat pattern geometry, bend lines and sketches

        swPart.ExportToDWG(sPathName, sModelName, 1, True, varAlignment, False, False, options, Nothing)

 

        Debug.Print("Inspect DWG files in " + Left(sPathName, Len(sPathName) - 16))

    End Sub

    

    Public swApp As SldWorks

End Class