C# SolidWorks 二次开发 API—遍历草图

代码:

这里示意获取草图中线段的总长:

private void Btn_T_sketchsegment_Click(object sender, EventArgs e)
        {
            ISldWorks swApp = Utility.ConnectToSolidWorks();

            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SelectionMgr swSelMgr = default(SelectionMgr);
            Feature swFeature = default(Feature);
            string fileName = null;
            bool status = false;
            int errors = 0;
            int warnings = 0;

            //打开文件
            fileName = "C:\\Users\\Public\\Documents\\SOLIDWORKS\\SOLIDWORKS 2018\\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);

            swModelDocExt = (ModelDocExtension)swModel.Extension;

            //选中草图
            status = swModelDocExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, false, 0, null, 0);

            swSelMgr = (SelectionMgr)swModel.SelectionManager;
            //转换
            swFeature = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            //进入编辑草图
            swModel.EditSketch();
            //获取草图中的所有线
            object[] vSketchSeg = (object[])swFeature.GetSpecificFeature2().GetSketchSegments();

            SketchSegment swSketchSeg;
            double totalLenth = 0;
            foreach (var tempSeg in vSketchSeg)
            {
                swSketchSeg = (SketchSegment)tempSeg;
                //这里判断 不是文本,并且不是中心线 则加入长度
                if (swSketchSeg.GetType() != (int)swSketchSegments_e.swSketchTEXT && swSketchSeg.ConstructionGeometry == false)
                {
                    totalLenth = totalLenth + swSketchSeg.GetLength();
                }
            }

            swModel.EditSketch();
            //显示总长
            swApp.SendMsgToUser("Total Length:" + totalLenth * 1000);
        }

 

posted @
2019-09-30 12:54 
painezeng  阅读(
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C# SolidWorks 二次开发 API—如何通过面属性命名选中对象

今天有人问到如何选中零件中已经命名的面.那我们就先把这个记录一下.

比如,零件中我们命名了一个面的名称

有两种情况:

1,零件中选中该面:

             ISldWorks swApp = Utility.ConnectToSolidWorks();
            ModelDoc2 swModel = swApp.ActiveDoc;
            SelectionMgr swSelMgr = swModel.SelectionManager;          
             PartDoc part1 = (PartDoc)swModel;
            //在零件中选择
            Face2 face1 = part1.GetEntityByName("SFace1", (int)swSelectType_e.swSelFACES);
            Entity entity1 = (Entity)face1;
            entity1.Select(false);

 

 

2.装配中:

 #region 装配中选择

            //这里我们默认该零件已经是选中装配,否则我们需要遍历一次零件,仅做示例

            Component2 component = swSelMgr.GetSelectedObjectsComponent4(1, -1);

            swModel.ClearSelection();

            ModelDoc2 modelDoc = component.GetModelDoc2();

            //转换为PartDoc
            PartDoc part = (PartDoc)modelDoc;

            Face2 face = part.GetEntityByName("SFace1", (int)swSelectType_e.swSelFACES);

            Entity entity = (Entity)face;

            //在装配中再转换成装配中的实体
            Entity entityInComp = (Entity)component.GetCorrespondingEntity(entity);

            entityInComp.Select(false);

            #endregion

 

posted @
2019-09-29 18:23 
painezeng  阅读(
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C# SolidWorks 二次开发 API—删除草图中的约束关系

这一个比较简单,其实就是遍历一下草图中的对象,然后获取关系,删除.

代码:

 private void btn_DeleteConstraints_Click(object sender, EventArgs e)
        {
            //请先打开clamp1这个零件

            ISldWorks swApp = Utility.ConnectToSolidWorks();
            ModelDoc2 swModel = swApp.ActiveDoc;
            SelectionMgr swSelMgr = swModel.SelectionManager;

            //选择草图
            swModel.Extension.SelectByID2("Sketch2", "SKETCH", 0, 0, 0, false, 4, null, 0);

            //进入编辑草图
            swModel.EditSketch();

            //获取当前草图对象
            Sketch swSketch = swModel.GetActiveSketch2();

            //获取该草图中的所有线
            object[] vSketchSeg = swSketch.GetSketchSegments();

            //定义选择
            SelectData swSelData = swSelMgr.CreateSelectData();

            SketchSegment swSketchSeg;
            //遍历线
            for (int i = 0; i < vSketchSeg.Length; i++)
            {
                swSketchSeg = (SketchSegment)vSketchSeg[i];
                swSketchSeg.Select4(false, swSelData);
                //删除关系
                swModel.SketchConstraintsDelAll();
            }


            object[] vSketchPt = (SketchPoint[])swSketch.GetSketchPoints2();
            SketchPoint swSketchPt;
            //遍历点
            for (int i = 0; i < vSketchPt.Length; i++)
            {
                swSketchPt = (SketchPoint)vSketchPt[i];
                swSketchPt.Select4(false, swSelData);
                swModel.SketchConstraintsDelAll();
            }
            //退出编辑草图
            swModel.InsertSketch2(true);

            swModel.ClearSelection2(true);
        }

 

posted @
2019-09-27 22:50 
painezeng  阅读(
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C# SolidWorks 二次开发 API—指定过滤器

当我们需要用户选择时,可以利用代码创建指定的选择器.

其实就像手工点击工具条内的过滤器一样:

 

        private void btnFilter_Click(object sender, EventArgs e)
        {
            ISldWorks swApp = Utility.ConnectToSolidWorks();

            ModelDoc2 modelDoc2 = swApp.ActiveDoc;
            //SelectionMgr selectionMgr = modelDoc2.SelectionManager;

            //设置可选择类型的数组
            swSelectType_e[] filters = new swSelectType_e[1];

            //让用户只能选择实体

            filters[0] = swSelectType_e.swSelSOLIDBODIES;

            swApp.SetSelectionFilters(filters, true);
        }

 

posted @
2019-09-26 21:49 
painezeng  阅读(
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C# SolidWorks 二次开发 API—插入库特征

要想提高设计效率，做库特征是很常见的。例如我们下面这个视频，利用库特征在打了很多小孔。

利用库特征快速插入特征

这一次我们来看如何用代码插入库特征。

我们以API实例中的一个例子来说明一下过程：

        public DispatchWrapper[] ObjectArrayToDispatchWrapperArray(object[] Objects)
        {
            int ArraySize = 0;
            ArraySize = Objects.GetUpperBound(0);
            DispatchWrapper[] d = new DispatchWrapper[ArraySize + 1];
            int ArrayIndex = 0;
            for (ArrayIndex = 0; ArrayIndex <= ArraySize; ArrayIndex++)
            {
                d[ArrayIndex] = new DispatchWrapper(Objects[ArrayIndex]);
            }
            return d;
        }

        public DispatchWrapper[] LibRefs;

        private void btnInsertLibF_Click(object sender, EventArgs e)
        {
            ISldWorks swApp = Utility.ConnectToSolidWorks();

            //可以参考API帮助中的:Create Library Feature Data Object and Library Feature With References Example (C#)

            //Step1:新建一个零件.
            Feature swFeature = default(Feature);
            ModelDoc2 swModel = default(ModelDoc2);
            ModelDocExtension swModelDocExt = default(ModelDocExtension);
            SketchManager swSketchManager = default(SketchManager);
            SelectionMgr swSelectionManager = default(SelectionMgr);
            FeatureManager swFeatureManager = default(FeatureManager);
            LibraryFeatureData swLibFeat = default(LibraryFeatureData);
            bool status = false;
            object[] sketchLines = null;
            object Refs = null;
            object RefTypes = null;
            int RefCount = 0;
            int k = 0;
            int i = 0;
            DispatchWrapper[] LibRefs = null;

            string libPath = "C:\\ProgramData\\SOLIDWORKS\\SOLIDWORKS 2018\\design library\\features\\metric\\slots\\straight slot.sldlfp";

            // Create part
            swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SOLIDWORKS 2018\\templates\\Part.prtdot", 0, 0, 0);
            swModelDocExt = (ModelDocExtension)swModel.Extension;
            status = swModelDocExt.SelectByID2("Top Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swSketchAddConstToRectEntity, (int)swUserPreferenceOption_e.swDetailingNoOptionSpecified, false);
            status = swModelDocExt.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, (int)swUserPreferenceOption_e.swDetailingNoOptionSpecified, true);
            swSketchManager = (SketchManager)swModel.SketchManager;
            sketchLines = (object[])swSketchManager.CreateCornerRectangle(0, 0, 0, 1, 0.5, 0);
            swModel.ShowNamedView2("*Trimetric", 8);
            swModel.ClearSelection2(true);
            status = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line4", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("Line3", "SKETCHSEGMENT", 0, 0, 0, true, 0, null, 0);
            swFeatureManager = (FeatureManager)swModel.FeatureManager;
            swFeature = (Feature)swFeatureManager.FeatureExtrusion2(true, false, false, 0, 0, 0.01, 0.01, false, false, false,
            false, 0.0174532925199433, 0.0174532925199433, false, false, false, false, true, true, true,
            0, 0, false);
            swSelectionManager = (SelectionMgr)swModel.SelectionManager;
            swSelectionManager.EnableContourSelection = false;

            swModel = (ModelDoc2)swApp.ActiveDoc;

            string actName = swModel.GetPathName();

            #region 第一种方法

            //Step2:初始化库特征
            swLibFeat = (LibraryFeatureData)swFeatureManager.CreateDefinition((int)swFeatureNameID_e.swFmLibraryFeature);
            status = swLibFeat.Initialize(libPath);

            //step3:获取库特征需要的参考对象
            RefCount = swLibFeat.GetReferencesCount();
            Refs = (object[])swLibFeat.GetReferences2((int)swLibFeatureData_e.swLibFeatureData_FeatureRespect, out RefTypes);

            if ((RefTypes != null))
            {
                Debug.Print("Types of references required (edge = 1): ");
                int[] RefType = (int[])RefTypes;
                for (k = RefType.GetLowerBound(0); k <= RefType.GetUpperBound(0); k++)
                {
                    Debug.Print("    " + RefType[k].ToString());
                }
            }
            //setp4:设定库特征默认的配置名称
            swLibFeat.ConfigurationName = "Default";
            //setp5:选择一个面,并插入库特征
            status = swModelDocExt.SelectByID2("", "FACE", 0.522458766456054, 0.288038964184011, 0.00999999999987722, false, 0, null, 0);
            swFeature = (Feature)swFeatureManager.CreateFeature(swLibFeat);
            //step6:
            swLibFeat = null;
            swLibFeat = (LibraryFeatureData)swFeature.GetDefinition();
            status = swLibFeat.AccessSelections(swModel, null);

            //step7:选择真实的参考
            status = swModelDocExt.SelectByID2("", "EDGE", 0.960865149149924, 0.497807163546383, 0.0131011390528215, true, 0, null, 0);
            status = swModelDocExt.SelectByID2("", "EDGE", 0.99866860703213, 0.481385806014544, 0.0113313929676906, true, 0, null, 0);
            int selCount = 0;
            selCount = swSelectionManager.GetSelectedObjectCount2(-1);

            object[] selectedObjects = new object[selCount];

            for (i = 0; i < selCount; i++)
            {
                object selectedObject = null;
                selectedObject = (object)swSelectionManager.GetSelectedObject6(i + 1, -1);
                selectedObjects[i] = selectedObject;
            }

            // 转换对象
            LibRefs = (DispatchWrapper[])ObjectArrayToDispatchWrapperArray((selectedObjects));

            // 设定引用关系到刚生成的库特征
            swLibFeat.SetReferences(LibRefs);

            // 更新库功能
            status = swFeature.ModifyDefinition(swLibFeat, swModel, null);

            // 取消抑制库功能
            status = swModelDocExt.SelectByID2("straight slot<1>", "BODYFEATURE", 0, 0, 0, false, 0, null, 0);
            swModel.EditUnsuppress2();

            swModel.ClearSelection2(true);

            #endregion 第一种方法

            #region 第二种方法(已过时)

            ////先选中线,再插入库特征.

            ////要先打开库特征,然后切换到当前零件,选中参考特征,最后插入特征库

            //int errors = 0;
            //int warnings = 0;

            //swApp.OpenDoc6(libPath, 1, 0, "", errors, warnings);

            //swModel = swApp.ActivateDoc2(actName, true, errors);

            //status = swModelDocExt.SelectByID2("", "FACE", 0.522458766456054, 0.288038964184011, 9.99999999987722E-03, false, 0, null, 0);
            //status = swModelDocExt.SelectByID2("", "EDGE", 0.960865149149924, 0.497807163546383, 0.0131011390528215, true, 1, null, 0);
            //status = swModelDocExt.SelectByID2("", "EDGE", 0.99866860703213, 0.481385806014544, 0.0113313929676906, true, 2, null, 0);

            //swModel.InsertLibraryFeature(libPath);

            #endregion 第二种方法(已过时)
        }
  

 

posted @
2019-09-25 20:07 
painezeng  阅读(
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C# SolidWorks 二次开发 API — 文件导出(x_t/dxf)

小例子，导出文件。

下面是代码：

        private void btnExport_Click(object sender, EventArgs e)
        {
            ISldWorks swApp = Utility.ConnectToSolidWorks();

            if (swApp != null)
            {
                ModelDoc2 swModel = (ModelDoc2)swApp.ActiveDoc;

                if (swModel.GetType() == (int)swDocumentTypes_e.swDocPART || swModel.GetType() == (int)swDocumentTypes_e.swDocASSEMBLY)
                {
                    ModelDocExtension swModExt = (ModelDocExtension)swModel.Extension;

                    int error = 0;

                    int warnings = 0;

                    //设置导出版本
                    swApp.SetUserPreferenceIntegerValue((int)swUserPreferenceIntegerValue_e.swParasolidOutputVersion, (int)swParasolidOutputVersion_e.swParasolidOutputVersion_161);

                    swModExt.SaveAs(@"C:\export.x_t", (int)swSaveAsVersion_e.swSaveAsCurrentVersion, (int)swSaveAsOptions_e.swSaveAsOptions_Silent, null, ref error, ref warnings);
                }
                else if (swModel.GetType() == (int)swDocumentTypes_e.swDocDRAWING)
                {
                    ModelDocExtension swModExt = (ModelDocExtension)swModel.Extension;

                    int error = 0;

                    int warnings = 0;

                    //设置dxf 导出版本 R14
                    swApp.SetUserPreferenceIntegerValue((int)swUserPreferenceIntegerValue_e.swDxfVersion, 2);

                    //是否显示 草图
                    swModel.SetUserPreferenceToggle(196, false);

                    swModExt.SaveAs(@"C:\export.dxf", (int)swSaveAsVersion_e.swSaveAsCurrentVersion, (int)swSaveAsOptions_e.swSaveAsOptions_Silent, null, ref error, ref warnings);
                }
            }
        }

 

 

 

 

 

posted @
2019-09-24 16:15 
painezeng  阅读(
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