Hide Table of Contents

Get Centerlines in Drawing Example (C#)

This example shows how to get all of the centerlines in all of the drawing views in a drawing.

//------------------------------------
// Preconditions:
// 1. Verify that the drawing document to open exists.
// 2. Open the Immediate window.
//
// Postconditions:
// 1. Opens the specified drawing.
// 2. Inserts a centerline annotation.
// 3. Prints the path and file name of the drawing document
//    to the Immediate window.
// 4. Iterates the sheet and drawing view, prints their names, and
//    prints the name of the centerline annotation to
//    the Immediate window.
// 5. Examine the Immediate window.
//
// NOTE: Because this drawing document is used elsewhere,
// do not save any changes.
//------------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using System.Diagnostics;
 
namespace CenterLinesCSharp.csproj
{
    public partial class SolidWorksMacro
    {
 
        public void Main()
        {
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            DrawingDoc swDrawing = default(DrawingDoc);
            View swView = default(View);
            Centerline swCenterLine = default(Centerline);
            Annotation swAnnotation = default(Annotation);
            bool status = false;
            int errors = 0;
            int warnings = 0;
            string fileName = null;
 
            fileName = "C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\samples\\tutorial\\api\\cylinder20.SLDDRW";
            swModel = (ModelDoc2)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocDRAWING, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, ""ref errors, ref warnings);
            swDrawing = (DrawingDoc)swModel;
            swModelDocExt = (ModelDocExtension)swModel.Extension;
 
            status = swDrawing.ActivateView("Drawing View1");
            status = swModelDocExt.SelectByID2("cylinder20-9@Drawing View1""COMPONENT", 0, 0, 0, false, 0, null, 0);
            status = swModelDocExt.SelectByID2("""FACE", 0.513454307125032, 0.454946591641617, 250.013794595267, false, 0, null, 0);
 
            swCenterLine = (Centerline)swDrawing.InsertCenterLine2();
            swModel.ClearSelection2(true);
 
            swView = (View)swDrawing.GetFirstView();
            Debug.Print("File = " + swModel.GetPathName());
 
            while ((swView != null))
            {
                Debug.Print("  View = " + swView.GetName2());
                swCenterLine = (Centerline)swView.GetFirstCenterLine();
                while ((swCenterLine != null))
                {
                    swAnnotation = (Annotation)swCenterLine.GetAnnotation();
                    Debug.Print("    Name       = " + swAnnotation.GetName());
                    swCenterLine = swCenterLine.GetNext();
                }
                swView = (View)swView.GetNextView();
            }
 
        }
 
        /// <summary>
        ///  The SldWorks swApp variable is pre-assigned for you.
        /// </summary>
        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:   Get Centerlines in Drawing 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) 2018 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.