Create and Edit Linear Sketch Pattern Example (C#)

This example shows how to create and edit a linear sketch pattern.

// -----------------------------------------------------------------------

// Preconditions:

//       (1) SolidWorks is running.

//       (2) The part template exists in the specified folder.

//

// Postconditions:

//         (1) An extrude feature is created.

//         (2) A sketch is opened on the front face of the extrude feature.

//         (3) A linear sketch pattern is created in the open sketch.

//         (4) The sketch is closed.

//         (5) The linear sketch pattern is opened for editing.

//         (6) Linear sketch pattern is edited -- an entity

//             (i.e., Line3) is deleted in each instance of the

//             linear sketch pattern.

// -----------------------------------------------------------------------

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

namespace CreateEditLinearPattern_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        public void Main()

        {

            ModelDoc2 swModel = default(ModelDoc2);

            ModelDocExtension swModelDocExt = default(ModelDocExtension);

            SketchManager swSketchMgr = default(SketchManager);

            Feature swFeature = default(Feature);

            FeatureManager swFeatureMgr = default(FeatureManager);

            object vSkLines = null;

            bool boolstatus = false;

            int longstatus = 0;

            // Reset the counts for untitled documents for this macro

            swApp.ResetUntitledCount(0, 0, 0);

            // Create part document

            swModel = (ModelDoc2)swApp.NewDocument("C:\\Documents and Settings\\All Users\\Application Data\\SolidWorks\\SolidWorks 2010\\templates\\Part.prtdot", 0, 0, 0);

            swApp.ActivateDoc2("Part1", false, ref longstatus);

            swModel = (ModelDoc2)swApp.ActiveDoc;

            // Select the Front plane

            swModelDocExt = swModel.Extension;

            boolstatus = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, false, 0, null, 0);

            // Open a sketch and sketch a rectangle

            swSketchMgr = swModel.SketchManager;

            swSketchMgr.InsertSketch(true);

            swModel.ClearSelection2(true);

            vSkLines = swSketchMgr.CreateCornerRectangle(-0.07606134448097, 0.04933121484909, 0, 0.07649598073515, -0.0510697598658, 0);

            // Change view orientation and clear all selections

            swModel.ShowNamedView2("*Trimetric", 8);

            swModel.ClearSelection2(true);

            // Select the sketch entities to extrude

            swModelDocExt = swModel.Extension;

            boolstatus = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);

            boolstatus = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);

            boolstatus = swModelDocExt.SelectByID2("Line4", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);

            boolstatus = swModelDocExt.SelectByID2("Line3", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);

            // Create the extrude feature

            swFeatureMgr = swModel.FeatureManager;

            swFeature = swFeatureMgr.FeatureExtrusion2(true, false, false, 0, 0, 0.0508, 0.381, false, false, false,

            false, 0.01745329251994, 0.01745329251994, false, false, false, false, true, true, true,

            0, 0, false);

            // Fit the model in the graphics area

            swModel.ViewZoomtofit2();

            // Select the face on the extrude feature and sketch the entities to pattern

            swModel.ShowNamedView2("*Front", 1);

            boolstatus = swModelDocExt.SelectByID2("", "FACE", -0.05428715407583, 0.03314479661076, 0.05079999999998, false, 0, null, 0);

            vSkLines = swSketchMgr.CreateCornerRectangle(-0.00838865116811, 0.00609746454014, 0, 0.00738895920642, -0.007221297464333, 0);

            // Create a linear sketch pattern using the newly

            // sketched rectangle as the linear pattern seed feature

            boolstatus = swSketchMgr.CreateLinearSketchStepAndRepeat(2, 2, 0.0254, 0.0254, 0.296705972839, 1.134464013796, "", true, true, false,

            true, true);

            swModel.ClearSelection2(true);

            // Close the sketch

            swModel.SketchManager.InsertSketch(true);

            // Select an entity in the linear sketch seed

            // pattern and open the linear sketch pattern to edit

            boolstatus = swModelDocExt.SelectByID2("Line3@Sketch2", "EXTSKETCHSEGMENT", -0.002651338304644, -0.007221297464333, 0, false, 0, null, 0);

            swModel.EditSketch();

            // Delete the Line3 sketch entity from each instance

            // of the linear sketch pattern

            boolstatus = swSketchMgr.EditLinearSketchStepAndRepeat(3, 2, 0.0254, 0.0254, 0.296705972839, 1.134464013796, "", false, false, false,

            true, true, "Line2_Line1_Line4_");

        }

        public SldWorks swApp;

    }

}