Export Part to DWG Example (C#)

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

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

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

using System.Diagnostics;

namespace ExportToDWG_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        ModelDoc2 swModel;

        PartDoc swPart;

        string sModelName;

        string sPathName;

        object varAlignment;

        double[] dataAlignment = new double[12];

        object varViews;

        string[] dataViews = new string[2];

        long options;

        public void Main()

        {

            swModel = (ModelDoc2)swApp.ActiveDoc;

            sModelName = swModel.GetPathName();

            sPathName = swModel.GetPathName();

            sPathName = sPathName.Substring(0, (sPathName.Length - 6));

            sPathName = sPathName + "dwg";

            swPart = (PartDoc)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, (int)options, null);

            Debug.Print("Inspect DWG files in " + sPathName.Substring(0, (sPathName.Length - 16)));

        }

        public SldWorks swApp;

    }

}