有限元法基本原理与应用技术ANSYS上机.docx

1、有限元法基本原理与应用技术ANSYS上机“有限元法基本原理与使用”课程有限元分析软件ANSYS 上 机 指 南华东理工大学机械与动力工程学院2009年9月Project1 简支梁的变形分析.1Project2 坝体的有限元建模与受力分析.3Project3 平板中心开小孔应力集中系数分析.5Project4 旋转磁盘应力分析. 7Project5 压力容器的有限元求解1.9Project6 压力容器的有限元求解2.11Project7 容器接管有限元建模与变形分析 13Project1 梁的有限元建模与变形分析计算分析模型如图1-1 所示, 习题文件名: beam。NOTE:要求选择不同形状的

2、截面分别进行计算。图1-1梁的计算分析模型梁截面分别采用以下三种截面（单位：m）： 矩形截面： 圆截面： 工字形截面：B=0.1, H=0.15 R=0.1 w1=0.1，w2=0.1，w3=0.2, t1=0.0114,t2=0.0114,t3=0.0071.1 进入ANSYS程序 Ansys Interactive change the working directory into yours input Initial jobname: beamRun1.2设置计算类型 ANSYS Main Menu: Preferences select Structural OK1.3选择单元类型A

3、NSYS Main Menu: Preprocessor Element TypeAdd/Edit/Delete Add select Beam 2 node 188 OK (back to Element Types window) Close (the Element Type window)1.4定义材料参数ANSYS Main Menu: Preprocessor Material Props Material Models Structural Linear Elastic Isotropic input EX:2.1E11, PRXY:0.3 OK1.5定义截面ANSYS Main

4、 Menu: Preprocessor Sections Beam Common Sectns 分别定义矩形截面、圆截面和工字形截面：矩形截面:ID=1,B=0.1，H=0.15 Apply 圆截面：ID=2,R=0.1 Apply 工字形截面：ID=3,w1=0.1，w2=0.1，w3=0.2，t1=0.0114，t2=0.0114，t3=0.007 OK 1.6生成几何模型 生成特征点 ANSYS Main Menu: Preprocessor Modeling Create Keypoints In Active CS 依次输入三个点的坐标：input:1(0,0),2(10,0),3(

5、5,2) OK 生成梁ANSYS Main Menu: Preprocessor Modeling Create Lines lines Straight lines 连接两个特征点，1(0,0),2(10,0) OK1.7 网格划分 ANSYS Main Menu: Preprocessor Meshing Mesh Attributes Picked lines OK 选择: SECT:1（根据所计算的梁的截面选择编号）；Pick Orientation Keypoint(s):YES拾取：3#特征点(5,2) OKMesh Tool Size Controls) lines: Set P

6、ick All(in Picking Menu) input NDIV:200 OK (back to Mesh Tool window) Mesh Pick All (in Picking Menu) Close (the Mesh Tool window)1.8 模型施加约束 最左端节点加约束ANSYS Main Menu: Solution Define Loads Apply Structural Displacement On Nodes pick the node at (0,0) OK select UX, UY,UZ,ROTX, ROTY OK 最右端节点加约束ANSYS Ma

7、in Menu: Solution Define Loads Apply Structural Displacement On Nodes pick the node at (10,0) OK select UY,UZ,ROTX, ROTY OK 施加均布的载荷ANSYS Main Menu: Solution Define Loads Apply Structural Pressure On Beams Pick All VALI:1.0E3 OK1.9 分析计算 ANSYS Main Menu: Solution Solve Current LS OK(to close the solve

8、 Current Load Step window) OK1.10 结果显示 ANSYS Main Menu: General PostprocRead ResultsLast Set ANSYS Main Menu: General Postproc Plot Results Deformed Shape select Def + Undeformed OK (back to Plot Results window) Contour Plot Nodal Solu select: DOF solution, UY, Def + Undeformed , Rotation, ROTZ ,Def

9、 + UndeformedOK1.11 退出系统 ANSYS Utility Menu: File Exit Save EverythingOKProject2 坝体的有限元建模与应力应变分析计算分析模型如图2-1 所示, 习题文件名: dam。图21 坝体的计算分析模型2.1 进入ANSYS程序 AnsysED Interactive change the working directory into yours input Initial jobname: damRun2.2设置计算类型 ANSYS Main Menu: Preferences select Structural OK2.

10、3选择单元类型ANSYS Main Menu: Preprocessor Element TypeAdd/Edit/Delete Add select Solid Quad 4node 42 OK (back to Element Types window) Options select K3: Plane Strain OKClose (the Element Type window)2.4定义材料参数ANSYS Main Menu: Preprocessor Material Props Material Models Structural LinearElastic Isotropic

11、input EX:2.1E11,PRXY:0.3 OK2.5生成几何模型 生成特征点ANSYS Main Menu: Preprocessor Modeling Create Keypoints In Active CS 依次输入四个点的坐标input:1(0,0),2(2,0),3(2,10),4(2-1.2,10) OK 生成坝体截面ANSYS Main Menu: Preprocessor Modeling Create Areas Arbitrary Through KPS 依次连接四个特征点，1(0,0),2(2,0),3(2,10),4(2-1.2,10) OK2.6 网格划分 A

12、NSYS Main Menu: Preprocessor Meshing Mesh Tool(Size Controls) lines: Set 依次拾取两条横边:OKinput NDIV: 40Apply依次拾取两条纵边:OK input NDIV: 200OK (back to the mesh tool window)Mesh: Areas, Shape: Quad, Mapped Mesh Pick All (in Picking Menu) Close( the Mesh Tool window)2.7 模型施加约束 分别给下底边和竖直的纵边施加x和y方向的约束ANSYS Main

13、Menu: Solution Define Loads Apply Structural Displacement On lines pick the lines OK select Lab2:UX, UY OK 给斜边施加水压分布载荷ANSYS 命令菜单栏: Parameters Functions Define/Edit 1) 在下方的下拉列表框内选择Y ,作为设置的变量；2) 在Result窗口中出现Y,写入所施加的载荷函数：1000*9.8*(10-Y)； 3) FileSave(文件扩展名：func) 返回：Parameters Functions Read from file：将需

14、要的.func文件打开，任给一个参数名，它表示随之将施加的载荷OK ANSYS Main Menu: Solution Define Loads Apply Structural Pressure On Lines 拾取斜边；OK 在下拉列表框中，选择：Existing table OK 选择需要的载荷参数名OK2.8 分析计算 ANSYS Main Menu: Solution Solve Current LS OK(to close the solve Current Load Step window) OK2.9 结果显示 ANSYS Main Menu: General Postpro

15、cRead ResultsLast SetANSYS Main Menu: General Postproc Plot Results Deformed Shape select Def + Undeformed OK (back to Plot Results window)Contour Plot Nodal Solu select: DOF solution, UX,UY, Def + Undeformed , Stress ,SX,SY,SZ, Def + UndeformedOK2.10 退出系统 ANSYS Utility Menu: File Exit Save Everythi

16、ngOKProject3 平板中心开小孔应力集中系数分析计算分析模型如图3-1 所示, 习题文件名: plate。10001000的平板，小孔直径40mm，板厚5mm。E =2.1E5 泊松比 =0.3图31 平板开小孔的计算分析模型3.1 进入ANSYS程序 AnsysED Interactive change the working directory into yours input Initial jobname: plateRun3.2设置计算类型 ANSYS Main Menu: Preferences select Structural OK3.3选择单元类型ANSYS Main

17、 Menu: Preprocessor Element TypeAdd/Edit/Delete Add select Solid Quad 4node 42 OK (back to Element Types window) Options select K3: Plane Stress w/thick OKClose (the Element Type window) 输入实参：ANSYS Main Menu: Preprocessor Real Constants Add/Edit/DeleteAddOKThickness THKinput 53.4定义材料参数ANSYS Main Men

18、u: Preprocessor Material Props Material Models Structural LinearElastic Isotropic input EX:2.1E5,PRXY:0.3 OK3.5生成几何模型 生成1/4矩形面和实心圆面ANSYS Main Menu: Preprocessor Modeling Create Areas RetangleBy 2 cornersinput:WP X=0, WP Y=0,Width=500,Height=500 OK ANSYS Main Menu: Preprocessor Modeling Create Areas

19、CircleSolid Circleinput:WP X=0, WP Y=0,Radius=20 OK 布尔操作：矩形面减实心圆面 ANSYS Main Menu: Preprocessor Modeling OperateBooleansSubtractAreas拾取矩形面；OK拾取圆面；OK 打开关键点号码和线的号码 PlotCtrlsNumberingKP Keypoints numbers ON;LINE Line numbers ON PlotLine3.6 网格划分 ANSYS Main Menu: Preprocessor Meshing Mesh Tool(Size Contr

20、ols) lines: Set 依次拾取线9和10:OKinput NDIV: 80，Space:2.5 Apply依次拾取线3和2:OK input NDIV: 40, Space:1 OK ANSYS Main Menu: Preprocessor ModelingMove/ModifyReverse Normalsof Lines依次拾取线9和10:OKOKANSYS Main Menu: Preprocessor Meshing Mesh Tool Mesh: Areas, Shape: Quad, Mapped;Pick cornersMesh Pick 带孔的平板 Pick 依次拾

21、取关键点4,6,5,2OK3.7 模型施加约束 分别施加对称约束及拉伸载荷ANSYS Main Menu: PreprocessorLoadsDefine Loads Apply Structural Displacement Symmetry B.C. On Lines pick依次拾取线9和10 OK ANSYS Main Menu: PreprocessorLoadsDefine Loads Apply Structural PressureOn Lines pick拾取线2 OK 菜单：VALUE Load PRES value:输入-1OK3.8 分析计算 ANSYS Main Me

22、nu: Solution Solve Current LS OK(to close the solve Current Load Step window) OK3.9 结果显示 ANSYS Main Menu: General PostprocRead ResultsLast SetANSYS Main Menu: General Postproc Plot Results Deformed Shape select Def + Undeformed OK (back to Plot Results window)Contour Plot Nodal Solu select: DOF solu

23、tion, UX,UY, Def + Undeformed , Stress ,SX,SY,SZ, Def + UndeformedOK3.10 退出系统 ANSYS Utility Menu: File Exit Save EverythingOKProject4 旋转磁盘应力分析外径：120mm 内孔径：15mm 厚度：1.2mm 弹性模量1.6104MPa =0.3密度：2.2103Kg/m3 转速：10000转/分=1047.19弧度/秒4.1 进入ANSYS程序 AnsysED Interactive change the working directory into yours i

24、nput Initial jobname: plateRun4.2设置计算类型 ANSYS Main Menu: Preferences select Structural OK4.3选择单元类型ANSYS Main Menu: Preprocessor Element TypeAdd/Edit/Delete Add select Solid Quad 4node 42 OK (back to Element Types window) Options select K3: Plane Stress w/thick OKClose (the Element Type window) 输入实参：

25、ANSYS Main Menu: Preprocessor Real Constants Add/Edit/DeleteAddOKThickness THKinput 1.24.4定义材料参数ANSYS Main Menu: Preprocessor Material Props Material Models Structural LinearElastic Isotropic input EX:1.6E4,PRXY:0.3 OKANSYS Main Menu: Preprocessor Material Props Material Models StructuralDensityinpu

26、t DENS:2200E-12OK4.5生成几何模型 生成圆环面ANSYS Main Menu: Preprocessor Modeling Create Areas Annulusinput:WP X=0, WP Y=0,Rad-1 =120/2, Rad-2 =15/2 OK 打开关键点号码和线的号码 PlotCtrlsNumberingKP Keypoints numbers ON;LINE Line numbers ON PlotLine 创建线去分面 ANSYS Main Menu: Preprocessor Modeling Create Line Straight Line分别拾

27、取关键点6和关键点1Apply分别拾取关键点8和关键点2Apply分别拾取关键点7和关键点3Apply分别拾取关键点5和关键点4OK ANSYS Main Menu: Preprocessor Modeling OperateBooleansDivideWith OptionsArea by Line拾取圆环面OK分别拾取线9、10、11、12OKKEEPA Base areas will be: Deleted;KEEPL Subtracted lines will be:Kept4.6 网格划分 ANSYS Main Menu: Preprocessor Meshing Mesh Tool

28、(Size Controls) lines: Set 依次拾取线9、10、11、12:OKinput NDIV: 30，Space:-2 Apply依次拾取线1、2、3、4:OK input NDIV: 30, Space:1 OK ANSYS Main Menu: Preprocessor Meshing Mesh Tool Mesh: Areas, Shape: Quad, Mapped Mesh Pick All (in Picking Menu) Close( the Mesh Tool window)4.7 模型施加约束 转换坐标为柱坐标 WorkplaneChange Active

29、 CS toGlobal Cylindrical SelectEntitiesselect Line; By Num/Pick ;From FullOKpick 依次挑选线5、6、7、8OK PlotLines SelectEntitiesselect Nodes; Attached to ;Lines all; From FullOK PlotNodes耦合：preprocessor-couplingcoupling DOFS第一个选项输入1-OK ANSYS Main Menu: Preprocessor ModelingMove/ModifyRotate Node CSTo Active

30、 CSPick ALLANSYS Main Menu: PreprocessorLoadsDefine Loads Apply StructuralDisplacementOn NodesPick ALLselect: UY OK WorkplaneChange Active CS toGlobal Cartesian SelectEverything ANSYS Main Menu: PreprocessorLoadsDefine Loads Apply StructuralInertiaAngular VelocityGlobalselect OMEGZ Global Cartesian Z-comp:1047.19OK4.8