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Insert and Position DXF/DWG File in Drawing Example (C#)

This example shows how to insert and position a DXF/DWG file in a drawing.

//---------------------------------------------------------------------------
// Preconditions:
// 1. Open a drawing.
// 2.
Replace DXF_file_path with the pathname of an existing DXF/DWG file.
// 3. Open the Immediate window.
//
// Postconditions:
// 1. Inserts the DXF/DWG file as per the specified import data.
// 2. Inspect the Immediate window.
//---------------------------------------------------------------------------
using Microsoft.VisualBasic;
using System;
using System.Collections;
using System.Collections.Generic;
using System.Data;
using System.Diagnostics;
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
namespace InsertDXFDrawing_CSharp.csproj
{
    
partial class SolidWorksMacro
    {

        
public void Main()
        {
            
const string sDwgFileName = "DXF_file_path";

            
ModelDoc2 swModel = default(ModelDoc2);
            
ModelView swModelView = default(ModelView);
            
DrawingDoc swDraw = default(DrawingDoc);
            
FeatureManager swFeatMgr = default(FeatureManager);
            
Feature swFeat = default(Feature);
            
Sketch swSketch = default(Sketch);
            
View swView = default(View);
            
double[] vPos = null;
            
bool bRet = false;
            
ImportDxfDwgData importData = default(ImportDxfDwgData);

            swModel = (
ModelDoc2)swApp.ActiveDoc;
            swModelView = (
ModelView)swModel.ActiveView;

            bRet = swModel.Extension.SelectByID2(
"Sheet1", "SHEET", 0.0, 0.0, 0, false, 0, null, 0);

            swDraw = (
DrawingDoc)swModel;
            swFeatMgr = swModel.FeatureManager;
            importData = (
ImportDxfDwgData)swApp.GetImportFileData(sDwgFileName);

            
// Unit
            importData.set_LengthUnit("", (int)swLengthUnit_e.swINCHES);

            
// Position
            bRet = importData.SetPosition("", (int)swDwgImportEntitiesPositioning_e.swDwgEntitiesCentered, 0, 0);

            
// Sheet scale
            bRet = importData.SetSheetScale("", 1.0, 2.0);

            
// Paper size
            bRet = importData.SetPaperSize("", (int)swDwgPaperSizes_e.swDwgPaperAsize, 0.0, 0.0);

            
//Import method
            importData.set_ImportMethod("", (int)swImportDxfDwg_ImportMethod_e.swImportDxfDwg_ImportToExistingDrawing);

            
// Import file with importData
            swFeat = swFeatMgr.InsertDwgOrDxfFile2(sDwgFileName, importData);
            swSketch = (
Sketch)swFeat.GetSpecificFeature2();

            swView = (
View)swDraw.GetFirstView();

            
while ((swView != null))
            {
                
if (object.ReferenceEquals(swSketch, swView.GetSketch()))
                {
                    
break;
                }
                swView = (
View)swView.GetNextView();
            }

            vPos = (
double[])swView.Position;

            
Debug.Print("File = " + swModel.GetPathName());
            
Debug.Print("  Sketch       = " + swFeat.Name);
            
Debug.Print("  View         = " + swView.Name);
            
Debug.Print("    Old Pos    = (" + vPos[0] * 1000.0 + ", " + vPos[1] * 1000.0 + ") mm");

            
// Move to right
            vPos[0] = vPos[0] + 0.01;
            swView.Position = vPos;

            vPos = (
double[])swView.Position;
            
Debug.Print("    New Pos    = (" + vPos[0] * 1000.0 + ", " + vPos[1] * 1000.0 + ") mm");

            
// Redraw
            double[] rect = null;
            rect =
null;
            swModelView.GraphicsRedraw(rect);

        }

        
public SldWorks swApp;

    }
}



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