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

//---------------------------------------------------------------------------
// Preconditions:
// 1. Open a drawing.
// 2. Replace DXF_file_path with the pathname of an existing DXF/DWG file.
// 3. Ensure the namespace matches the name of your C# project.
//
// Postconditions:
// 1. Inspect the Immediate window.
// 2. The DXF/DWG file is inserted as per the specified import data.
// 3. The drawing is moved to the right.
//---------------------------------------------------------------------------
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;

    }
}