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Insert Weldment Features Example (C#)

This example shows how to insert the following weldment features into the FeatureManager design tree:

    *  End cap feature

    *  Fillet bead feature

    *  Gusset feature

    *  Structural weldment

    *  Sub weld folder

    *  Weldment trim feature

//---------------------------------------------------------------------------
// Preconditions:
// 1. Open public_documents\tutorial\weldments\weldment_box2.sldprt
// 2. Expand the Cut list folder in the FeatureManager design tree
//    and observe its contents.
// 3. Delete End cap1 from the FeatureManager design tree.
// 4. Change the path specified for profilePathName, if necessary.
//
// Postconditions: Observe the following in the FeatureManager design tree:
//    * Gusset1 moves to the sub weld folder, Sub Folder1, in the Cut list
//      folder
//    * Trim/Extend8 feature appears at the bottom of the design tree and at
//      the end of the Cut list folder
//    * Structural Member6 feature appears at the bottom of the design tree
//      and at the end of the Cut list folder
//    * End cap5 feature appears at the bottom of the design tree and in the
//      Cut list folder
//    * Gusset5 feature appears at the bottom of the design tree and in the
//      Cut list folder
//    * Fillet Bead5 feature appears at the bottom of the design tree and
//      in the Cut list folder
//
// NOTE: Because this part is used elsewhere,
// do not save any changes when you close it.
//---------------------------------------------------------------------------

 

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

using System;

namespace InsertWeldmentFeatures_CSharp.csproj

{

    partial class SolidWorksMacro

    {

        FeatureManager fm;

        SelectionMgr selMgr;

        ModelDoc2 Part;

        bool boolstatus;

        public void Main()

        {

            object myFeature = null;

            Body2[] obj = new Body2[1];

            Array v = default(Array);

            Part = (ModelDoc2)swApp.ActiveDoc;

            object myModelView = null;

            myModelView = Part.ActiveView;

            selMgr = (SelectionMgr)Part.SelectionManager;

            //InsertSubWeldFolder2

            boolstatus = Part.Extension.SelectByID2("Gusset1", "SOLIDBODY", 0, 0, 0, false, 0, null, 0);

            obj[0] = (Body2)selMgr.GetSelectedObject6(1, -1);

            v = obj;

            fm = Part.FeatureManager;

            myFeature = fm.InsertSubWeldFolder2(v);

            Part.ClearSelection2(true);

            //InsertWeldmentTrimFeature2

            Body2[] obj1 = new Body2[1];

            Body2[] obj2 = new Body2[1];

            long Options = 0;

            Array v1 = default(Array);

            Array v2 = default(Array);

            boolstatus = Part.Extension.SelectByID2("Structural Member1[2]", "SOLIDBODY", 0, 0, 0, true, 2, null, 0);

            boolstatus = Part.Extension.SelectByID2("Structural Member1[1]", "SOLIDBODY", 0, 0, 0, true, 1, null, 0);

            long Count = 0;

            Count = selMgr.GetSelectedObjectCount();

            if (Count == 2)

            {

                obj1[0] = (Body2)selMgr.GetSelectedObject2(1);

                v1 = obj1;

                obj2[0] = (Body2)selMgr.GetSelectedObject2(2);

                v2 = obj2;

                Part.ClearSelection2(true);

                Options = (long)swWeldmentTrimExtendOptionType_e.swWeldmentTrimExtendOption_AllowTrimmedExtensionTrim + (long)swWeldmentTrimExtendOptionType_e.swWeldmentTrimExtendOption_AllowTrimmingExtensionTrim + (long)swWeldmentTrimExtendOptionType_e.swWeldmentTrimExtendOption_CopedCut + (long)swWeldmentTrimExtendOptionType_e.swWeldmentTrimExtendOption_WeldGap;

                myFeature = fm.InsertWeldmentTrimFeature2(1, (int)Options, 0.01, v1, v2);

            }

            //InsertEndCapFeature

            Feature endCapFeature = default(Feature);

            Face2[] face1 = new Face2[1];

            Array x = default(Array);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.6023443450227, 0.6150000000001, -1.013201139555, true, 1, null, 0);

            face1[0] = (Face2)selMgr.GetSelectedObject6(1, -1);

            x = face1;

            endCapFeature = fm.InsertEndCapFeature2(0.005, false, true, 0.003, 0.5, 0.003, x);

            Part.ClearSelection2(true);

            //InsertStructuralWeldment3

            Array segmentObjects = default(Array);

            SketchSegment[] sketchSegments = new SketchSegment[4];

            string profilePathName = null;

            Feature structuralMember = default(Feature);

            StructuralMemberGroup @group = default(StructuralMemberGroup);

            StructuralMemberGroup[] GroupArray1 = new StructuralMemberGroup[1];

            long i = 0;

            @group = fm.CreateStructuralMemberGroup();

            Part.ClearSelection2(true);

            Part.InsertSketch2(true);

            segmentObjects = (System.Array)Part.SketchManager.CreateCornerRectangle(0, 0, 0, 1.0, 2.0, 0);

            for (i = 0; i <= segmentObjects.GetUpperBound(0); i++)

            {

                sketchSegments[i] = (SketchSegment)segmentObjects.GetValue(i);

            }

            @group.Segments = sketchSegments;

            GroupArray1[0] = @group;

            Part.ViewZoomtofit2();

            Part.InsertSketch2(true);

            profilePathName = "C:\\Program Files\\SOLIDWORKS Corp\\SOLIDWORKS\\lang\english\\weldment profiles\\ansi inch\\square tube\\2 x 2 x 0.25.SLDLFP";

            structuralMember = fm.InsertStructuralWeldment3(profilePathName, 1, 0.0, false, GroupArray1);

            Part.ClearSelection2(true);

            //InsertGussetFeature2

            Face2[] faceGFObj = new Face2[2];

            object z = null;

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.02539999999988, 1.94542628561, 0.00429028534694, true, 1, null, 0);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.07780718114736, 1.9746, -0.001856983219, true, 2, null, 0);

            Count = selMgr.GetSelectedObjectCount();

            if (Count == 2)

            {

                faceGFObj[0] = (Face2)selMgr.GetSelectedObject6(1, 1);

                faceGFObj[1] = (Face2)selMgr.GetSelectedObject6(1, 2);

                z = faceGFObj;

                Part.ClearSelection2(true);

                myFeature = fm.InsertGussetFeature2(0.005, 0, 0, false, 0.025, 0.025, 0.015, 0.7853981633975, 0.015, true,

                0.005, 0, false, false, false, z);

            }

            //InsertFilletBeadFeature3

            Face2[] fbFaceObj1 = new Face2[1];

            Face2[] fbFaceObj2 = new Face2[2];

            Part.ClearSelection2(true);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.0412896304482, 0.02548020566445, 0, true, 1, null, 0);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.09804264728081, 0.01499999999999, 0.0008069730266129, true, 2, null, 0);

            boolstatus = Part.Extension.SelectByID2("", "FACE", 0.01364526875011, 0.08738481720087, 0.01330055827532, true, 4, null, 0);

            Count = selMgr.GetSelectedObjectCount();

            // Face Set 1

            fbFaceObj1[0] = (Face2)selMgr.GetSelectedObject6(1, 1);

            // Face Set 2

            fbFaceObj2[0] = (Face2)selMgr.GetSelectedObject6(1, 2);

            //fbFaceObj2(0) = selMgr.GetSelectedObject6(1, 4)

            v1 = fbFaceObj1;

            v2 = fbFaceObj2;

            Part.ClearSelection2(true);

            int[] edges = new int[1];

            Array edgeArray = default(Array);

            edges[0] = 0;

            //edges(1) = 0

            edgeArray = edges;

            myFeature = fm.InsertFilletBeadFeature3(0, 0.003, 0.003, 2, 0.003, 0.006, 0, 0.003, 0.003, 2, 0.003, 0, 1, edgeArray, 0, null, v1, v2);

            Part.ClearSelection2(true);

        }

        public SldWorks swApp;

    }

}



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