ANSYS上机指南.doc

有限元分析软件
ANSYS
上 机 指 南

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

I

有限元分析软件ANSYS上机指南
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。

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
ü 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

ü 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
ü 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

ü 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

ü 施加y方向的载荷
ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Pressure → On Beams →Pick All →VALI: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

21 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
ü 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

ü 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
ü 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

ü 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 →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

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。

图3-1受均匀内压的球体计算分析模型（截面图）

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
ü 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
ü 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
ü 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，

ü 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

ü 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 VALUE: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。

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
ü 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
ü 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
ü 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。

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 Constants… →Add… →select Type 1→ OK→input AREA:0.25 →OK →Close (the Real Constants Window)

5.6生成几何模型
ü 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

ü 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
ü 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

ü 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

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
ü 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

ü 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
ü 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
ü 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

ü 施加y方向的载荷
ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Pressure → On Beams →Pick All →LKEY:2,VALI: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

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 Constants… →Add… →select Type 1→ OK→input THK:1 →OK →Close (the Real Constants Window)

7.6生成几何模型
ü 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

ü 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
ü 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
ü 施加y方向约束
ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Displacement → On Keypo