有限元分析上机指导书之 ANSYS连杆建模实践.doc
有限元分析实验指导书之二维单元的使用（连杆分析）1. 进入ANSYS工作目录,将 “c-rod” 作为jobname。2.创建两个圆面： Main Menu > Preprocessor > -Modeling- Create > -Areas- Circle > By Dimensions . RAD1 = 1.4 RAD2 = 1 THETA1 = 0 THETA2 = 180, 单击Apply 然后设置THETA1 = 45,再单击OK3.打开面:编号 Utility Menu > PlotCtrls > Numbering . 设置面号on, 然后单击OK4.创建两个矩形面: Main Menu > Preprocessor > -Modeling- Create > -Areas- Rectangle > By Dimensions . X1 = -0.3, X2 = 0.3, Y1 = 1.2, Y2 = 1.8, 单击Apply X1 = -1.8, X2 = -1.2, Y1 = 0, Y2 = 0.3, 单击 OK5.偏移工作平面到给定位置 (X=6.5): Utility Menu > WorkPlane > Offset WP to > XYZ Locations + 在ANSYS输入窗口输入6.5 OK6.将激活的坐标系设置为工作平面坐标系: Utility Menu > WorkPlane > Change Active CS to > Working Plane6.52.50.51.80.31.0R1.4R0.4R0.7R45oSpline through six control pointsCLCLCrank pin endWrist pin endAll dimensions in inches45o0.280.40.334.754.03.257.创建另两个圆面: Main Menu > Preprocessor > -Modeling- Create > -Areas- Circle > By Dimensions . RAD1 = 0.7 RAD2 = 0.4 THETA1 = 0 THETA2 = 180, 然后单击Apply 第二个圆THETA2 = 135, 然后单击OK8.对面组分别执行布尔运算: Main Menu > Preprocessor > -Modeling- Operate > -Booleans- Overlap > Areas + 首先选择左侧面组, 单击 Apply 然后选择右侧面组, 单击OK 9.将激活的坐标系设置为总体笛卡尔坐标系: Utility Menu > WorkPlane > Change Active CS to > Global Cartesian10.定义四个新的关键点: Main Menu > Preprocessor > -Modeling- Create > Keypoints > In Active CS 第一个关键点, X=2.5, Y=0.5, 单击Apply 第二个关键点, X=3.25, Y=0.4, 单击Apply 第三个关键点, X=4, Y=0.33, 单击Apply 第四个关键点, X=4.75, Y=0.28, 单击OK11.将激活的坐标系设置为总体柱坐标系: Utility Menu > WorkPlane > Change Active CS to > Global Cylindrical12.通过一系列关键点创建多义线: Main Menu > Preprocessor > -Modeling- Create > -Lines- Splines > With Options > Spline thru KPs + 如图按顺序拾取六个关键点, 然后单击 OK XV1 = 1 YV1 = 135 XV6 = 1 YV6 = 45 OK13.在关键点1和18之间创建直线: Main Menu > Preprocessor > -Modeling- Create > -Lines- Lines > Straight Line + 拾取如图的两个关键点, 然后单击 OK14.打开线的编号并画线: Utility Menu > PlotCtrls > Numbering . 打开线的编号, 单击 OK Utility Menu > Plot > Lines15.由前面定义的线6, 1, 7, 25创建一个新的面: Main Menu > Preprocessor > -Modeling- Create > -Areas- Arbitrary > By Lines + 拾取四条线 (6, 1, 7, and 25),然后单击 OK16.放大连杆的左面部分: Utility Menu > PlotCtrls > Pan, Zoom, Rotate Box Zoom17.创建三个线倒角: Main Menu > Preprocessor > -Modeling- Create > -Lines- Line Fillet + 拾取线36 和 40,然后单击 Apply RAD = .25,然后单击 Apply 拾取线40 和 31, 然后单击 Apply Apply 拾取线 30和39, 然后单击OK OK Utility Menu > Plot > Lines18.由前面定义的三个线倒角创建新的面: Main Menu > Preprocessor > -Modeling- Create > -Areas- Arbitrary > By Lines + 拾取线12, 10, 及13, 单击 Apply 拾取线17, 15, 及19, 单击Apply 拾取线23, 21, 及24, 单击OK Utility Menu > Plot > Areas 19.将面加起来形成一个面: Main Menu > Preprocessor > -Modeling- Operate > Add > Areas + Pick All20.使模型充满整个图形窗口: Utility Menu > PlotCtrls > Pan, Zoom, Rotate Fit21.关闭线及面的编号: Utility Menu > PlotCtrls > Numbering . 关闭线及面的编号, 单击 OK Utility Menu > Plot > Areas22.将激活的坐标系设置为总体笛卡尔坐标系: Utility Menu > WorkPlane > Change Active CS to > Global Cartesian Or issue:CSYS,023.将面沿XZ面进行映射 (在 Y 方向): Main Menu > Preprocessor > -Modeling- Reflect > Areas + Pick All 选择X-Z面, 单击OK24.将面加起来形成一个面: Main Menu > Preprocessor > -Modeling- Operate > Add > Areas + Pick All 25.关闭工作平面: Utility Menu > WorkPlane > Display Working Plane26.存储数据库并离开ANSYS: 拾取 “SAVE_DB” 拾取“QUIT” 选择 “Quit - No Save!”OK27. 选取93号壳单元Main Menu>Preprocessor>Element Type>Add/Edit/Delete>Add>28. 设置壳单元厚度为0.3Main Menu>Preprocessor>Real Constants>Add/Edit/Delete>Add>ok29. 设置材料参数Main Menu>Preprocessor>Material Props>Material Models30. 分网Main Menu>Preprocessor>Meshing>MeshTool31. 施加约束Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Lines选取小孔边缘，约束小孔的所有自由度32. 加载Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Lines选取大孔的半个边缘，33. 显示壳单元的厚度旋转模型，使模型显示成薄片状勾选Display of element后，能显示0.3的壁厚。34. 求解Main Menu>Solution>Solve>Current LS35. 后处理Main Menu>General Postproc>Plot Results>Contour Plot>Nodal SoluMain Menu>General Postproc>Plot Results>Contour Plot>Element Solu输出窗口图片为 .emf 文件（可调入word文件中）
