Insert Sheet Metal Base Flange Example (C#)

This example shows how to insert a sheet metal base flange.

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

// Preconditions:

// 1. Open SolidWorks.

// 2. Verify and, if necessary, modify the location of the part template in the code below:

//  C:\Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks 2010\templates\Part.prtdot

// 3. Run (F5) this macro.

// Postconditions:

// Observe the following in the model view and the FeatureManager design tree:

//  * Sheet metal base flange, Base-Flange1, connects the two sheet metal parts.

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

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

namespace InsertSheetMetalBaseFlange2_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        ModelDoc2 Part;

        bool boolstatus;

        long longstatus;

        int status;

        public void Main()

        {

            longstatus = (long)swApp.ResetUntitledCount(0, 0, 0);

            Part = (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 status);

            Part = (ModelDoc2)swApp.ActiveDoc;

            Part.SketchManager.InsertSketch(true);

            boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.07320616684915, 0.04378582530511, 0.008882453015985, false, 0, null, 0);

            Part.ClearSelection2(true);

            object vSkLines = null;

            vSkLines = Part.SketchManager.CreateCornerRectangle(-0.09520523544121, 0.05740695090967, 0, -0.03844330645187, -0.0429584598942, 0);

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

            Part.ClearSelection2(true);

            object myFeature = null;

            myFeature = Part.FeatureManager.FeatureExtrusion2(true, false, true, 0, 0, 0.01, 0.01, false, false, false,

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

            0, 0, false);

            boolstatus = Part.Extension.SelectByID2("", "FACE", -0.0785775433435, 0.01894373057962, 0, true, 0, null, 0);

            boolstatus = Part.FeatureManager.InsertConvertToSheetMetal(0.002, false, false, 0.004, 0.002, 0, 0.5);

            Part.ClearSelection2(true);

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

            Part.SketchManager.InsertSketch(true);

            Part.ClearSelection2(true);

            vSkLines = Part.SketchManager.CreateCornerRectangle(-0.02256810687936, 0.06039039042219, 0, 0.02390260459754, -0.04039198125838, 0);

            Part.ClearSelection2(true);

            myFeature = Part.FeatureManager.FeatureExtrusion2(true, false, true, 0, 0, 0.01, 0.01, false, false, false,

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

            0, 0, false);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0009118315510932, 0.02609254832731, 0, true, 0, null, 0);

            boolstatus = Part.FeatureManager.InsertConvertToSheetMetal(0.002, false, false, 0.004, 0.002, 0, 0.5);

            Part.ClearSelection2(true);

            Part.SketchManager.InsertSketch(true);

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

            Part.ClearSelection2(true);

            vSkLines = Part.SketchManager.CreateCornerRectangle(-0.05411927414525, 0.01318437124604, 0, -0.007403979976402, -0.001979918613586, 0);

            CustomBendAllowance customBendAllowanceData = null;

            customBendAllowanceData = null;

            myFeature = Part.FeatureManager.InsertSheetMetalBaseFlange2(0.002, false, 0.004, 0.02, 0.01, false, 0, 0, 1, customBendAllowanceData,

            false, 2, 0.0001, 0.0001, 0.5, true, false, true, true);

            Part.ClearSelection2(true);

        }

        public SldWorks swApp;

    }

}