有限元分析案例图1 钢铸件及其砂模的横截面尺寸砂模的热物理性能如下表所示:铸钢的热物理性能如下表所示:一、初始条件:铸钢的温度为2875o F，砂模的温度为80o F；砂模外边界的对流边界条件：对流系数0.014Btu/hr.in2.o F，空气温度80o F；求3个小时后铸钢及砂模的温度分布。

二、菜单操作:1.Utility Menu>File>Change Title, 输入Casting Solidification;2.定义单元类型:Main Menu>Preprocessor>Element Type>Add/Edit/Delete, Add, Quad 4node 55；3.定义砂模热性能:Main Menu>Preprocessor>Material Props>Isotropic,默认材料编号1, 在Density(DENS)框中输入0.054,在Thermal conductivity (KXX)框中输入0.025,在S pecific heat(C)框中输入0.28;4.定义铸钢热性能温度表:Main Menu>Preprocessor>Material Props>-Temp Dependent->Temp Table,输入T1=0,T2=2643, T3=2750, T4=2875;5.定义铸钢热性能:Main Menu>Preprocessor>Material Props>-Temp Dependent ->Prop Table, 选择Th Conductivity,选择KXX, 输入材料编号2,输入C1=1.44, C2=1.54, C3=1.22, C4=1.22,选择Apply,选择Enthalpy,输入C1=0, C2=128.1, C3=163.8, C4=174.2;6.创建关键点:Main Menu>Preprocessor>-Modeling->Create>Keypoints>In ActiveCS,输入关键点编号1,输入坐标0,0,0, 输入关键点编号2,输入坐标22,0,0, 输入关键点编号3,输入坐标10,12,0,输入关键点编号4, 输入坐标0,12,0;7.创建几何模型:Main Menu>Preprocessor>-Modeling->Create>-Areas-> Arbitrary>Through KPs,顺序选取关键点1,2,3,4;8.Main Menu>Preprocessor>-Modeling->Create>-Areas->Rectangle>By Dimension,输入X1=4,X2=22,Y1=4,Y2=8;9.进行布尔操作:Main Menu>Preprocessor>-Modeling->Operate>-Booleans-> Overlap>Area,Pick all；10.删除多余面:Main Menu>Preprocessor>-Modeling->Delete>Area and Below,311.保存数据库:在Ansys Toolbar中选取SA VE_DB;12.定义单元大小:Main Menu>Preprocessor>-Meshing->Size Cntrls>-Global->Size,在Element edge length框中输入1;13.对砂模划分网格:Main Menu>Preprocessor>-Meshing->Mesh>-Areas->Free,选择砂模;14.对铸钢划分网格:Main Menu>Preprocessor>-Attributes->Define>Default Attribs, 在Material number菜单中选择2;15.Main Menu>Preprocessor>-Meshing->Mesh>-Areas->Free,选择铸钢;16.定义分析类型:Main Menu>Solution>-Analysis Type->New Analysis,选择Transient;17.选择铸钢上的节点:Utility Menu>Select>Entities,选择element,mat,输入2,选择Apply,选择node, attached to element,选择OK;18.定义铸钢的初始温度:Main Menu>Solution>-Loads->Apply>Initial Condit’n>Define,选择Pick all,选择temp,输入2875, OK;19.选择砂模上的节点:Utility Menu>Select>Entities,Nodes, inverse20.定义砂模的初始温度:Main Menu>Solution>-Loads->Apply>Initial Condit’n>Define,选择Pick all,选择temp, 输入80, OK;21.Utility Menu>Select>Everything；22.U tility Menu>Plot>Lines；23.定义对流边界条件:Main Menu>Solution>-Loads->Apply>-Thermal ->Converction>On Lines,选择砂模的三个边界1,3,4, 在file coefficent框中输入80, 在Bulk temperature框中输入, 80;24.设定瞬态分析时间选项:Main Menu>Solution>Load Step Opts>Time/Frequenc>Time-Time Step,Time at end of load step 3 Time Step size0.01 Stepped or ramped b.c. Stepped Automatic time stepping onMinimun time Step size 0.001 Maximum time step size 0.2525.设置输出:Main Menu>Solution>Load Step Opts>Output Ctrls>DB/Results File, 在File write frequency框中选择Every substep;26.求解:Main Menu>Solution>-Solve->Current LS；27.进入后处理: Main Menu>Timehist Postproc；28.定义铸钢中心节点的温度变量:Main Menu>Timehist Postproc>Define Variables, Add, Nodal DOF result,2,204；29.绘制节点温度随时间变化曲线：Main Menu>Timehist Postproc>Graph Variable,2。

三、热应力分析有齿的轴对称管的热应力分析问题描述:管受内压，顶上的线（在Y=1.）代表对称面，我们将对线上的所以节点耦合UY自由度1. 进入ANSYS工作目录，取工作文件名为“pipe-th-str”2. Resume前面定义的轴对称模型:Utility Menu > Resume from …3. 设置菜单过滤为Structural:–Main Menu > Preferences …选则“Structural” 并且不选择“Thermal”, 单击 [OK]4.改变title:–Utility Menu > File > Change Title ... /TITLE = “2D AXI-SYMM THERMAL-STRESS ANALYSIS W/ INT. PRESS - ESIZE=0.125”[OK]5. 删除实体模型上的对流载荷:Main Menu > Preprocessor > Loads > -Loads- Delete > All Load Data > All SolidMod Lds [OK]6.将热单元改变为相应的结构单元:–Main Menu > Preprocessor > Element Type > Switch Elem Type 选择“Thermal to Struc”, 单击[OK]•查看警告信息并单击[Close]7. 设置单元形态为轴对称axisymmetric:–Main Menu > Preprocessor > Element Type>Add/Edit/Delete [Options ...]设置K3 = Axisymmetric, 单击[OK][Close] 8. 从热分析中施加温度载荷:Main Menu > Preprocessor > Loads > -Loads- Apply > Temperature > From Therm Analy ..•选择结果文件单击[OK]•查看警告信息单击[Close]9. 给Y＝0的线施加对称边界条件–Main Menu > Preprocessor > Loads > -Loads- Apply > Displacement > SymmetryB.C.- On Lines +选择线1 和9,单击[OK]10.耦合Y=1节点的UY 自由度:10a.选择Y=1处的节点:Utility Menu > Select > Entities ...•选择“Nodes” 及“By Location”选择“Y coordinates”设置Min,Max to 1, 单击[OK]10.对选择的节点集定义UY自由度耦合:Main Menu > Preprocessor > Coupling / Ceqn > Couple DOFs +•[Pick All]•NSET = 1•设置Lab = UY, 单击[OK]–Utility Menu > Select > Everything11. 给线施加内部常压力:–Main Menu > Loads > -Loads- Apply > Pressure > On Lines +•选择线 4, 单击[OK]•V ALUE = 1000, 单击[OK]12.通过显示体载荷检验温度载荷:–Utility Menu > PlotCtrls > Symbols•设置Body Load Symbols = “Structural temps”,单击[OK]–Utility Menu > Plot > Elements13.存储数据库并获得结果:–拾取“SA VE_DB” (或选择: Utility Menu > File > Save as Jobname.db)Main Menu > Solution > -Solve- Current LS•查看“/STATUS 命令” 窗口并关闭•[OK]•[Close] -求解结束之后关闭黄色的提示窗口14. 进入后处理查看结果:Main Menu > General Postproc >15. 画位移：Main Menu > General Postproc > Plot Results > -Contour Plot- Nodal Solu ...•拾取“DOF solution” 及“Translation USUM”, 选择“Def + undef edge”, 单击[OK]16. 沿Y轴旋转90度并沿x-z 平面映射轴对称应力结果:–Utility Menu > PlotCtrls > Style > Symmetry Expansion > 2D Axi-Symmetric ...拾取“1/4 expansion” and set reflection to “yes”, 单击[OK]–Utility Menu > PlotCtrls > Pan, Zoom, Rotate …[ISO]16. 存盘并离开ANSYS:。