清华大学的ansys资料!基础篇.doc

“有限元分析及应用”本科生课程有限元分析软件

ANSYS6.1ed 上机指南

清华大学机械工程系

2002年9月

说明

本《有限元分析软件ANSYS6.1ed:上机指南》由清华大学机械工程系石伟老师组织编写，由助教博士生孔劲执笔, 于2002年9月完成，基本操作指南中的所有算例都在相应的软件系统中进行了实际调试和通过。

本上机指南的版权归清华大学机械工程系所有，未经同意，任何单位和个人不得翻印。

联系人：石伟

北京市清华大学机械工程系（邮编100084）

Tel: (010) 62788117 Fax: (010) 62770190

目录

Project1 简支梁的变形分析 (1)

Project2 坝体的有限元建模与受力分析 (3)

Project3 受内压作用的球体的应力与变形分析 (5)

Project4 受热载荷作用的厚壁圆筒的有限元建模与温度场求解 (7)

Project5 超静定桁架的有限元求解 (9)

Project6 超静定梁的有限元求解 (11)

Project7 平板的有限元建模与变形分析 (13)

Project1 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截面分别进行计算。

梁承受均布载荷：1.0e5 Pa

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=0.007

1.1进入ANSYS

程序→ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: beam→Run

1.2设置计算类型

ANSYS Main Menu: Preferences →select Structural →OK

1.3选择单元类型

ANSYS Main Menu: Preprocessor →Element Type→Add/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→OK

1.5定义截面

ANSYS Main 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(5,1)→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) →OK

1.7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(5,1) →OK→Mesh Tool →Size Controls) lines: Set →Pick All(in Picking Menu) →input NDIV:5→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 →OK

?最右端节点加约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Nodes→pick the node at (10,0) →OK→select UY,UZ,ROTX →OK

?施加y方向的载荷

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Pressure→On Beams→Pick All→V ALI:100000 →OK

1.9 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

1.10 结果显示

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 + Undeformed→OK

1.11 退出系统

ANSYS Utility Menu: File→Exit →Save Everything→OK

Project2 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2－1 坝体的计算分析模型

2.1 进入ANSYS

程序 →ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: dam →Run 2.2设置计算类型

ANSYS Main Menu : Preferences →select Structural → OK 2.3选择单元类型

ANSYS Main Menu : Preprocessor →Element Type →Add/Edit/Delete →Add →select Solid Quad 4node 42 →OK (back to Element Types window) → Options… →select K3: Plane Strain →OK →Close (the Element Type window)

2.4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 → OK 2.5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(10,0),3(1,5),4(0.45,5) →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(10,0),3(1,5),4(0.45,5) →OK

2.6网格划分

ANSYS Main Menu: Preprocessor →Meshing →Mesh Tool→(Size Controls) lines:Set →依次拾取两条横边:OK→input NDIV: 15 →Apply→依次拾取两条纵边:OK →input NDIV: 20 →OK →(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 Menu: Solution→Define Loads →Apply→Structural →Displacement →On lines→pick the lines →OK→select Lab2:UX, UY →OK

?给斜边施加x方向的分布载荷

ANSYS 命令菜单栏: Parameters→Functions →Define/Edit→1) 在下方的下拉列表框内选择x ,作为设置的变量；2) 在Result窗口中出现{X},写入所施加的载荷函数：1000*{X}；3) File>Save(文件扩展名：func) →返回：Parameters→Functions →Read from file：将需要的.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→OK

2.8 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

2.9 结果显示

ANSYS Main Menu: General Postproc →Plot Results→Deforme d 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 + Undeformed→OK

2.10 退出系统

ANSYS Utility Menu: File→Exit…→Save Everything→OK

Project3受内压作用的球体的有限元建模与分析

计算分析模型如图3-1 所示, 习题文件名: sphere。

承受内压：1.0e8 Pa

3.1进入ANSYS

程序→ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: sphere→Run

3.2设置计算类型

ANSYS Main Menu: Preferences… →select Structural →OK

3.3选择单元类型

ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →select Solid Quad 4node 42 →OK (back to Element Types window)→Options… →select K3: Axisymmetric →OK→Close (the Element Type window)

3.4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→OK

3.5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(0.3,0),2(0.5,0),3(0,0.5),4(0,0.3)→OK

?生成球体截面

ANSYS 命令菜单栏: Work Plane>Change Active CS to>Global Spherical →ANSYS Main Menu: Preprocessor →Modeling →Create →Lines →In Active Coord→依次连接1,2,3,4点→OK →Preprocessor →Modeling →Create →Areas →Arbitrary →By Lines →依次拾取四条边→OK →ANSYS 命令菜单栏: Work Plane>Change Active CS to>Global

Cartesian

3.6网格划分

ANSYS Main Menu: Preprocessor →Meshing →Mesh Tool→(Size Controls) lines:Set →拾取两条直边:OK→input NDIV: 10 →Apply→拾取两条曲边:OK →input NDIV: 20 →OK →(back to the mesh tool window)Mesh: Areas, Shape: Quad, Mapped →Mesh →Pick All (in Picking Menu) →Close( the Mesh Tool window)

3.7模型施加约束

?给水平直边施加约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Lines →拾取水平边：Lab2: UY →OK，

?给竖直边施加约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement Symmetry B.C.→On Lines→拾取竖直边→OK

?给内弧施加径向的分布载荷

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Pressure →On Lines →拾取小圆弧；OK →input V ALUE:100e6→OK

3.8 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

3.9 结果显示

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, UX,UY, Def + Undeformed , Stress ,SX,SY,SZ,Def + Undeformed→OK

3.10 退出系统

ANSYS Utility Menu: File→Exit…→Save Everything→OK

Project4受热载荷作用的厚壁圆筒的有限元建模与温度场求解计算分析模型如图4-1 所示, 习题文件名: cylinder。

R2=0.5 圆筒内壁温度:500℃，外壁温度:100℃。两端自由且绝热

图4-1受热载荷作用的厚壁圆筒的计算分析模型（截面图）

4.1进入ANSYS

程序→ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: cylinder →Run

4.2设置计算类型

ANSYS Main Menu: Preferences… →select Thermal →OK

4.3选择单元类型

ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →select Thermal Solid Quad 4node 55 →OK (back to Element Types window)→Options… →select K3: Axisymmetric →OK→Close (the Element Type window)

4.4定义材料参数

ANSYS Main Menu: Preprocessor →Material Props →Material Models →Thermal→Conductivity→Isotropic→input KXX:7.5→OK

4.5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(0.3,0),2(0.5,0),3(0.5,1),4(0.3,1)→OK

?生成圆柱体截面

ANSYS Main Menu: Preprocessor →Modeling →Create →Areas →Arbitrary →Through KPS→依次连接四个特征点，1(0.3,0),2(0.5,0),3(0.5,1),4(0.3,1) →OK

4.6网格划分

ANSYS Main Menu: Preprocessor →Meshing →Mesh Tool→(Size Controls) lines:Set →拾取两条水平边:OK→input NDIV: 5 →Apply→拾取两条竖直边:OK →input NDIV: 15 →OK →(back to the mesh tool window)Mesh: Areas, Shape: Quad, Mapped →Mesh →Pick All (in Picking Menu) →Close( the Mesh Tool window)

4.7模型施加约束

?分别给两条直边施加约束

ANSYS Main Menu: Solution→Define Loads →Apply→Thermal →Temperature →On Lines →拾取左边, Value: 500 →Apply(back to the window of apply temp on lines)→拾取右边，Value：100 →OK

4.8 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

4.9 结果显示

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, Temperature TEMP →OK

4.10 退出系统

ANSYS Utility Menu: File→Exit…→Save Everything→OK

Project5超静定桁架的有限元建模与分析

计算分析模型如图5-1 所示, 习题文件名: truss。

载荷：1.0e8 N

图5－1 超静定桁架的计算分析模型

5.1进入ANSYS

程序→ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: truss→Run

5.2设置计算类型

ANSYS Main Menu: Preferences →select Structural →OK

5.3选择单元类型

ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →select Link 2D spar 1 →OK (back to Element Types window)→Options… →select K3: Plane Strain →OK→Close (the Element Type window)

5.4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→OK

5.5定义实常数

ANSYS Main Menu: Preprocessor →Real Constant s… →Add… →select Type 1→OK →input AREA:0.25 →OK →Close (the Real Constants Window)

5.6生成几何模型

?生成特征点

ANSYS Main Menu: Preprocessor →Modeling →Create →Keypoints →In Active CS →依次输入四个点的坐标：input:1(1,1),2(2,1),3(3,1),4(2,0)→OK

?生成桁架

ANSYS Main Menu: Preprocessor →Modeling →Create →Lines →Lines →Straight Line →依次连接四个特征点，1(1,1),2(2,1),3(3,1),4(2,0) →OK

5.7网格划分

ANSYS Main Menu: Preprocessor →Meshing →Mesh Tool→(Size Controls) lines:Set →依次拾取三根杆:OK→input NDIV: 1 →OK →(back to the mesh tool window)Mesh: lines →Mesh→Pick All (in Picking Menu) →Close( the Mesh Tool window)

5.8模型施加约束

?分别给1,2,3三个特征点施加x和y方向的约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Keypoints→拾取1(1,1),2(2,1),3(3,1)三个特征点→OK→select Lab2:UX, UY →OK

?给4#特征点施加y方向载荷

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Force/Moment →On Keypoints →拾取特征点4(2,0)→OK →Lab: FY, Value: -100e6 →OK

5.9 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

5.10 结果显示

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 →OK

5.11 退出系统

ANSYS Utility Menu: File →Exit →Save Everything→OK

Project6超静定梁的有限元建模计算

计算分析模型如图6-1 所示, 习题文件名: statically indeterminate beam

梁承受均布载荷：1.0e5 Pa

图6－1 超静定梁的计算分析模型

6.1进入ANSYS

程序→ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: statically indeterminate beam→Run

6.2设置计算类型

ANSYS Main Menu: Preferences →select Structural →OK

6.3选择单元类型

ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →select Beam tapered 44 →OK(back to Element Types window)→Close (the Element Type window)

6.4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→OK

6.5定义截面

ANSYS Main Menu: Preprocessor →Sections →Beam →Common Sectns→定义矩形截面:ID=1,B=0.01,H=0.1 →OK

6.6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(1,0),3(2,0),4(0,0,1) →OK

?生成梁

ANSYS Main Menu: Preprocessor →Modeling →Create →Lines →lines →Straight lines →依次连接三个特征点，1(0,0), 2(1,0),3(2,0) →OK

?显示梁体

ANSYS命令菜单栏：PlotCtrls >Style >Size and Style→/ESHAPE →On →OK

6.7网格划分

ANSYS Main Menu: Preprocessor →Meshing→Mesh Attributes→Picked lines →OK →拾取: SECT:1；Pick Orientation Keypoint(s):YES→拾取：4#特征点(0,0,1) →OK→Mesh Tool →(Size Controls) lines:Set →Pick All(in Picking Menu) →input NDIV:8→OK (back to Mesh Tool window) →Mesh →Pick All(in Picking Menu) →Close (the Mesh Tool window)

6.8模型施加约束

?分别给1,2,3三个特征点加约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Keypoints→拾取1,2,3 keypoints →OK→select All DOF →OK

?施加y方向的载荷

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Pressure→On Beams→Pick All→LKEY:2,V ALI:100000 →OK

6.9 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

6.10 结果显示

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 + Undeformed→OK

6.11 退出系统

ANSYS Utility Menu: File→Exit →Save Everything→OK

Project7 平板的有限元建模与变形分析

计算分析模型如图7-1 所示, 习题文件名: plane

0.5 m

0.5 m

板承受均布载荷：1.0e5 Pa

图7－1 受均布载荷作用的平板计算分析模型

7.1 进入ANSYS

程序 →ANSYSED 6.1 →Interactive →change the working directory into yours →input Initial jobname: plane →Run 7.2设置计算类型

ANSYS Main Menu : Preferences →select Structural → OK 7.3选择单元类型

ANSYS Main Menu : Preprocessor →Element Type →Add/Edit/Delete →Add →select Solid Quad 4node 42 →OK (back to Element Types window) → Options… →select K3: Plane stress w/thk →OK →Close (the Element Type window)

7.4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 → OK

7.5定义实常数

ANSYS Main Menu: Preprocessor →Real Constant s… →Add … →select Type 1→ OK →input THK:1 →OK →Close (the Real Constants Window)

7.6生成几何模型 ? 生成特征点

ANSYS Main Menu: Preprocessor →Modeling →Create →Keypoints →In Active CS →依次输入五个点的坐标：input:1(0,0),2(1,0), 3(1,1),4(0,1),5(0.5,0.5) →OK

?生成平板

ANSYS Main Menu: Preprocessor →Modeling →Create →Areas →Arbitrary →Through KPS→连接特征点1,2,5 →Apply →连接特征点2,3,5 →Apply →连接特征点3,4,5 →Apply →连接特征点4,1,5 →OK

7.7网格划分

ANSYS Main Menu: Preprocessor →Meshing→Mesh Tool →(Size Controls) lines: Set →Pick All(in Picking Menu) →input NDIV:1→OK→(back to the mesh tool window)Mesh: Areas, Shape: Tri, Free →Mesh →Pick All(in Picking Menu) →Close( the Mesh Tool window)

7.8模型施加约束

?给模型施加x方向约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Lines→拾取模型左部的竖直边：Lab2: UX →OK

?施加y方向约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural →Displacement →On Keypoints→拾取4# 特征点：Lab2: UY →OK

7.9 分析计算

ANSYS Main Menu: Solution →Solve →Current LS→OK(to close the solve Current Load Step window) →OK

7.10 结果显示

ANSYS Main Menu: General Postproc →Plot Results→Defo rmed Shape…→select Def + Undeformed→OK (back to Plot Results window) →Contour Plot→Nodal Solu →select: DOF solution, UX,UY, Def + Undeformed →OK

7.11 退出系统

ANSYS Utility Menu: File→Exit →Save Everything→OK