Hide Table of Contents

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 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.Runtime.InteropServices;
using System;
using System.Diagnostics;
namespace ExportToDWG2_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];

        
int 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.ExportToDWG2(sPathName, sModelName, (int)swExportToDWG_e.swExportToDWG_ExportAnnotationViews, false, varAlignment, false, false, 0, varViews);

            
//Export sheet metal to a single drawing file
            options = 13;
            
//0001101 - include flat-pattern geometry, bend lines and sketches
            swPart.ExportToDWG2(sPathName, sModelName, (int)swExportToDWG_e.swExportToDWG_ExportSheetMetal, true, varAlignment, false, false, options, null);

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

        }


        
public SldWorks swApp;

    }

}



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Export Part to DWG Example (C#)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2014 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.