Hide Table of Contents

Traverse Annotations Example (C#)

This example shows how to get display dimension annotations.

// Preconditions:
// 1. Verify that the specified part document exists.
// 2. Open the Immediate window.
// Postconditions:
// 1. Opens the specified part document and selects
//    a sketch containing multiple dimensions.
// 2. Iterates the display dimensions and gets 
//    each display dimension annotation and its position.
// 3. Moves each display dimension annotation 100mm to
//    the right.
// 4. Examine the graphics area and Immediate window.
// NOTE: Because the part document is used elsewhere, do not
// save changes.
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
using System.Diagnostics;
namespace TraverseAnnotationsCSharp.csproj
    public partial class SolidWorksMacro
        public void Main()
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SelectionMgr swSelMgr = default(SelectionMgr);
            Annotation swAnnotation = default(Annotation);
            double[] annotationPosition = null;
            Feature swFeature = default(Feature);
            DisplayDimension swDispDim = default(DisplayDimension);
            string fileName = null;
            int errors = 0;
            int warnings = 0;
            bool status = false;
            //Open part document
            fileName = "C:\\Program Files\\SolidWorks Corp\\SolidWorks\\samples\\tutorial\\tolanalyst\\offset\\top_plate.sldprt";
            swModel = (ModelDoc2)swApp.OpenDoc6(fileName, (int)swDocumentTypes_e.swDocPART, (int)swOpenDocOptions_e.swOpenDocOptions_Silent, ""ref errors, ref warnings);
            //Get and edit sketch with dimensions
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("Sketch1""SKETCH", 0, 0, 0, false, 0, null, 0);
            swSelMgr = (SelectionMgr)swModel.SelectionManager;
            swFeature = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            //Get the first display dimension 
            swDispDim = (DisplayDimension)swFeature.GetFirstDisplayDimension();
            //Iterate through all of the display dimension
            //annotations in the sketch
            while ((swDispDim != null))
                Debug.Print("Display dimension annotation name:");
                //Get the display dimension annotation
                swAnnotation = (Annotation)swDispDim.GetAnnotation();
                Debug.Print("  " + swAnnotation.GetName());
                //Get the position of the display dimension annotation
                annotationPosition = (double[])swAnnotation.GetPosition();
                if ((annotationPosition != null))
                    //Move the display dimension annotation 100mm to the right
                    swAnnotation.SetPosition2(annotationPosition[0] + 0.1, annotationPosition[1], annotationPosition[2]);
                //Get the next display dimension
                swDispDim = (DisplayDimension)swFeature.GetNextDisplayDimension(swDispDim);
        /// <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

Subject:   Feedback on Help Topics
Page:   Traverse Annotations Example (C#)
*   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:


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

Web Help Content Version: API Help (English only) 2016 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.