标签：二次开发

有一段时间没有发博文了，最近有人问到钣金件的相关操作，今天我们来看看钣金零件信息的读取。

Solidworks中钣金件是有一个单独的模块，里面有一些固定的文件夹结构。

最后这个文件夹中包含了展开状态时零件的信息。如长度与折弯线相关的信息都在这里面。

一般我们要找到长 宽 厚 折弯角 与距离  折弯方向 这些信息。

输出结果如下，有些小数的处理就忽略了。大家看看就行。 

粗略的写了下，输入信息在这里。很多就是API帮助里面的例子，大家可以在中文翻译中查找到。

        private void btnSheetmetal_Click(object sender, EventArgs e)
        {
            //连接到Solidworks
            ISldWorks swApp = Utility.ConnectToSolidWorks();
            swApp.CommandInProgress = true;
            ModelDoc2 swModel = (ModelDoc2)swApp.ActiveDoc;

            //钣金 变成平板模式的特征
            List<Feature> flatPatternFeatures = new List<Feature>();

            //Bounding Box草图
            List<string> boundingSketchesName = new List<string>();

            //获取当前钣金状态--这个已经过时

            //swSMBendStateFlattened  2 = 弯曲变平；该模型回滚到FlattenBends功能之后，但恰好在相应的ProcessBends功能之前
            //swSMBendStateFolded 3 = 折弯处已折叠；模型回滚到FlattenBends ProcessBends功能对之后
            //swSMBendStateNone   0 = 不是钣金零件；没有SheetMetal功能
            //swSMBendStateSharps 1 = 弯曲处处于锐利状态；零件回滚到第一个FlattenBends功能之前

            var bendState = swModel.GetBendState();

            if (bendState == 0)
            {
                swApp.SendMsgToUser("不是钣金零件！");
                return;
            }
            //  swApp.SendMsgToUser("当前状态" + bendState);
            if (bendState != 2)
            {
                //swApp.Command((int)swCommands_e.swCommands_Flatten, "");
                //设定当前钣金状态 平板 ，下面这行代码不适用现在的零件 ，只适用于很早之前的零件
                //var setStatus = swModel.SetBendState((int)swSMBendState_e.swSMBendStateFlattened);

                //新钣金均是通过获取零件
                var swFeatureManager = swModel.FeatureManager;
                var flatPatternFolder = (FlatPatternFolder)swFeatureManager.GetFlatPatternFolder();

                var featArray = (object[])flatPatternFolder.GetFlatPatterns();

                for (int i = featArray.GetLowerBound(0); i <= featArray.GetUpperBound(0); i++)
                {
                    var feat = (Feature)featArray[i];
                    Debug.Print("    " + feat.Name);

                    flatPatternFeatures.Add(feat);
                    feat.SetSuppression2((int)swFeatureSuppressionAction_e.swUnSuppressFeature, (int)swInConfigurationOpts_e.swThisConfiguration, null);

                    //解压子特征
                    var swSubFeat = (Feature)feat.GetFirstSubFeature();

                    while ((swSubFeat != null))
                    {
                        Debug.Print(swSubFeat.Name.ToString());
                        switch (swSubFeat.GetTypeName())
                        {
                            //如果是草图
                            case "ProfileFeature":

                                var sketchSpc = (Sketch)swSubFeat.GetSpecificFeature2();
                                object[] vSketchSeg = sketchSpc.GetSketchSegments();

                                for (int j = 0; j < vSketchSeg.Length; j++)
                                {
                                    SketchSegment swSketchSeg = (SketchSegment)vSketchSeg[j];

                                    //如果直线不是折弯线，说明是边界框
                                    if (swSketchSeg.IsBendLine() == false)
                                    {
                                        boundingSketchesName.Add(swSubFeat.Name);
                                    }
                                    else if (swSketchSeg.IsBendLine() == true)
                                    {
                                        Debug.Print("钣金宽度为:" + swSketchSeg.GetLength() * 1000);
                                    }
                                }

                                break;

                            default:
                                break;
                        }

                        swSubFeat = (Feature)swSubFeat.GetNextSubFeature();
                    }
                }

                swModel.EditRebuild3();
            }

            //遍历所有特征

            var swSelMgr = (SelectionMgr)swModel.SelectionManager;
            var swFeat = (Feature)swModel.FirstFeature();

            while ((swFeat != null))
            {
                //Debug.Print(swFeat.Name.ToString());
                // Process top-level sheet metal features
                switch (swFeat.GetTypeName())
                {
                    case "SMBaseFlange":
                        //var swBaseFlange = (BaseFlangeFeatureData)swFeat.GetDefinition();

                        //Debug.Print("钣金宽度为:" + swBaseFlange.D1OffsetDistance * 1000);

                        break;

                    case "SheetMetal":
                        //这里可以获取默认的厚度                        Debug.Print(swFeat.Name.ToString());
                        SheetMetalFeatureData sheetMetalFeatureData = (SheetMetalFeatureData)swFeat.GetDefinition();
                        Debug.Print("钣金默认厚度为:" + sheetMetalFeatureData.Thickness * 1000);

                        break;

                    case "SM3dBend":

                        break;

                    case "SMMiteredFlange":

                        break;
                }
                // process sheet metal sub-features
                var swSubFeat = (Feature)swFeat.GetFirstSubFeature();

                while ((swSubFeat != null))
                {
                    // Debug.Print(swSubFeat.Name.ToString());
                    switch (swSubFeat.GetTypeName())
                    {
                        case "SketchBend":

                            GetHisBendInformation(swApp, swModel, swSubFeat);
                            break;

                        case "OneBend":

                            GetHisBendInformation(swApp, swModel, swSubFeat);

                            break;

                        default:
                            break;
                            // Probably not a sheet metal feature
                    }

                    swSubFeat = (Feature)swSubFeat.GetNextSubFeature();
                }

                swFeat = (Feature)swFeat.GetNextFeature();
            }

            return;
        }

        private void GetHisBendInformation(ISldWorks swApp, ModelDoc2 swModel, Feature swFeat)
        {
            MathUtility swMathUtil = default(MathUtility);
            SelectionMgr swSelMgr = default(SelectionMgr);
            OneBendFeatureData swOneBend = default(OneBendFeatureData);
            Object[] vSketchSegs = null;
            SketchSegment swSketchSeg = default(SketchSegment);
            Sketch swSketch = default(Sketch);
            Feature swSketchFeat = default(Feature);
            SketchLine swSketchLine = default(SketchLine);
            SketchPoint swSkStartPt = default(SketchPoint);
            SketchPoint swSkEndPt = default(SketchPoint);
            SelectData swSelData = default(SelectData);
            double[] nPt = new double[3];
            MathPoint swStartPt = default(MathPoint);
            MathPoint swEndPt = default(MathPoint);
            MathTransform swSkXform = default(MathTransform);
            int[] vID = null;
            int i = 0;

            swMathUtil = (MathUtility)swApp.GetMathUtility();

            swSelMgr = (SelectionMgr)swModel.SelectionManager;
            //swFeat = (Feature)swSelMgr.GetSelectedObject6(1, -1);
            //swSelData = swSelMgr.CreateSelectData();
            swOneBend = (OneBendFeatureData)swFeat.GetDefinition();

            /*swBaseBend 4
            swEdgeFlangeBend 8
            swFlat3dBend 6
            swFlatBend 2
            swFreeFormBend 10 = Obsolete
            swHemBend 9
            swLoftedBend 12
            swMirrorBend 7
            swMiterBend 5
            swNoneBend 3
            swRoundBend 1
            swRuledBend 11 = Obsolete
            swSharpBend 0
            */

            Debug.Print("Type of bend (swBendType_e): " + swOneBend.GetType());
            Debug.Print("折弯次数: " + swOneBend.GetFlatPatternSketchSegmentCount2());
            Debug.Print("折弯序号: " + swOneBend.BendOrder);
            Debug.Print("折弯角度: " + swOneBend.BendAngle * 57.3 + " deg");
            Debug.Print("折弯圆角: " + swOneBend.BendRadius);

            if (swOneBend.BendDown == true)
            {
                Debug.Print("向下折弯: " + "Yes");
            }
            else
            {
                Debug.Print("向下折弯: " + " No");
            }

            vSketchSegs = (Object[])swOneBend.FlatPatternSketchSegments2;

            for (i = 0; i <= vSketchSegs.GetUpperBound(0); i++)
            {
                swSketchSeg = (SketchSegment)vSketchSegs[i];
                swSketch = swSketchSeg.GetSketch();
                swSketchLine = (SketchLine)swSketchSeg;
                swSkStartPt = (SketchPoint)swSketchLine.GetStartPoint2();
                swSkEndPt = (SketchPoint)swSketchLine.GetEndPoint2();
                vID = (int[])swSketchSeg.GetID();

                // Get sketch feature
                swSketchFeat = (Feature)swSketch;
                swSkXform = swSketch.ModelToSketchTransform;
                swSkXform = (MathTransform)swSkXform.Inverse();

                nPt[0] = swSkStartPt.X;
                nPt[1] = swSkStartPt.Y;
                nPt[2] = swSkStartPt.Z;
                swStartPt = (MathPoint)swMathUtil.CreatePoint(nPt);
                swStartPt = (MathPoint)swStartPt.MultiplyTransform(swSkXform);
                double[] swStartPtArrayData;
                swStartPtArrayData = (double[])swStartPt.ArrayData;

                nPt[0] = swSkEndPt.X;
                nPt[1] = swSkEndPt.Y;
                nPt[2] = swSkEndPt.Z;
                swEndPt = (MathPoint)swMathUtil.CreatePoint(nPt);
                swEndPt = (MathPoint)swEndPt.MultiplyTransform(swSkXform);
                double[] swEndPtArrayData;
                swEndPtArrayData = (double[])swEndPt.ArrayData;

                // Debug.Print("File = " + swModel.GetPathName());
                Debug.Print("  Feature = " + swFeat.Name + " [" + swFeat.GetTypeName2() + "]");
                Debug.Print("    Sketch             = " + swSketchFeat.Name);
                Debug.Print("    SegID              = [" + vID[0] + ", " + vID[1] + "]");
                Debug.Print("    Start with respect to sketch   = (" + swSkStartPt.X * 1000.0 + ", " + swSkStartPt.Y * 1000.0 + ", " + swSkStartPt.Z * 1000.0 + ") mm");
                Debug.Print("    End with respect to sketch   = (" + swSkEndPt.X * 1000.0 + ", " + swSkEndPt.Y * 1000.0 + ", " + swSkEndPt.Z * 1000.0 + ") mm");
                Debug.Print("    Start with respect to model    = (" + swStartPtArrayData[0] * 1000.0 + ", " + swStartPtArrayData[1] * 1000.0 + ", " + swStartPtArrayData[2] * 1000.0 + ") mm");
                Debug.Print("    End with respect to model    = (" + swEndPtArrayData[0] * 1000.0 + ", " + swEndPtArrayData[1] * 1000.0 + ", " + swEndPtArrayData[2] * 1000.0 + ") mm");
            }
        }
  

        今天有网友问我关于如何用Exe操作多个Solidworks的问题，其实之前我看到过解决方案，是通过进程和id获取，而不是我们平时常用的 (SldWorks)Marshal.GetActiveObject(“SldWorks.Application.27”);

        所以晚上回来查了些资料，发现了有了解决方案，我精简了一下，做了个dll.大家可以试试。    

 ''' <summary>
    ''' 创建一个新的Solidworks并返回实例
    ''' </summary>
    ''' <param name="version">指定版本号，-1表示默认.</param>
    ''' <param name="suppressDialogs">True 则禁用solidworks弹出消息.</param>
    ''' <param name="requireMainWindow">True 表示运行完显示到主窗口</param>
    ''' <param name="startProcessTimeout">返回Null 如果SolidWorks在指定时间内没有打开。</param>
    ''' <param name="createWindowTimeout">返回Null 如果SolidWorks主窗口在指定时间内没有显示.</param>
    ''' <returns></returns>
    Public Shared Function RunSolidWorks(version As Integer,
                                         visible As Boolean,
                                         Optional suppressDialogs As Boolean = False,
                                         Optional requireMainWindow As Boolean = True,
                                         Optional startProcessTimeout As Integer = 30,
                                         Optional createWindowTimeout As Integer = 15) As SldWorks

        Dim executablePath As String = CTFileSystem.GetSolidWorksExecutablePath(version)

        If File.Exists(executablePath) = False Then Return Nothing

        Dim info As ProcessStartInfo = New ProcessStartInfo(executablePath)

        If suppressDialogs Then info.Arguments = "/r"

        Dim process As Process = Process.Start(info)
        Dim app As SldWorks = Nothing
        Dim t As DateTime = DateTime.Now

        While app Is Nothing
            Threading.Thread.Sleep(1000)
            If Math.Abs(DateTime.Now.Subtract(t).Seconds) > startProcessTimeout Then Return Nothing

            'If it were possible to get a GUID from a process ID then we could use GetActiveObject instead of this
            app = GetComObjectFromProcessId(process.Id)
        End While

        t = DateTime.Now
        While IsRunning(isMainWindowCreated:=True) = False
            Threading.Thread.Sleep(1000)
            If Math.Abs(DateTime.Now.Subtract(t).Seconds) > createWindowTimeout Then Return Nothing
        End While

        If visible = False Then
            Dim frame As Frame = app.Frame()
            If frame Is Nothing Then Return app
            Dim handle As IntPtr = frame.GetHWndx64()
            If ShowWindow(handle, 0) Then Return app
        End If

        Return app
    End Function

我刚刚进行了测试，用起来比较简单。我用代码新建了两个solidworks 2018窗口：

        private SldWorks sldWorks2018_1 = null;
        private SldWorks sldWorks2018_2 = null;

        private void button1_Click(object sender, EventArgs e)
        {
            sldWorks2018_1 = PStandAlone.RunSolidWorks(26, true, false, false, 30, 15);
        }

        private void button2_Click(object sender, EventArgs e)
        {
            sldWorks2018_2 = PStandAlone.RunSolidWorks(26, true, false, false, 30, 15);
        }

        private void button3_Click(object sender, EventArgs e)
        {
            sldWorks2018_1.SendMsgToUser("From 2018 -1");
            sldWorks2018_2.SendMsgToUser("From 2018 -2");
        }

      

源码https://gitee.com/painezeng/PSWStandalone(vb.net)