清华大学ANSYS培训实例

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 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

6 －－

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。

圆筒内壁温度:500℃，外壁温度:100℃。两端自由且绝热 R1=0.3 R2=0.5

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

7 －－

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

8 －－

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。

1m 1m 1m 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 Constants… →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

9 －－