有限元分析及应用例子FEM14

第9章受内外压筒体的有限元建模与应力变形分析(Project 2)

计算分析模型如图9-1 所示, 习题文件名: cylinder。

X

(a)

σO=100N/mm2

σI =200N/mm2

γ =7.85g/cm3

µ =0.3

E =210000N/mm2

(b)

图9-1 计算分析模型

9.1进入ANSYS

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

9.2 设置计算类型

ANSYS Main Menu: Preferences…→select Structural →OK

9.3 选择单元类型

ANSYS Main Menu: Preprocessor → Element Type →Add/Edit/Delete… → Add… →select Solid Quad 4node 42 →Apply →select Solid Brick 8node 45 → OK → Close (the Element

Types window)

9.4定义材料参数

ANSYS Main Menu: Preprocessor →Material Props →Materials Models →Structural→Lineal →Elastic→Isotropic…→input EX:2.1e5, PRXY:0.3→ OK 关闭材料定义窗口

9.5构造筒体模型

➊生成模型截平面

ANSYS Main Menu: Preprocessor →Modeling→Create →Keypoints →In Active CS… →按次序输入横截平面的十个特征点和旋转对称轴上两点坐标（十个特征点：(300,0,0), (480,0,0), (480,100,0), (400,100,0), (400,700,0), (480,700,0), (480,800,0), (300,800,0), (300,650,0), (300,150,0)，对称轴上两点：(0,0,0), (0,800,0)）（每次输入完毕，用Apply结束，0可以不输入）

→Cancel (back to Create window) →-Areas- Arbitrary → Through KPs →依次连接截面边线上的十个特征点(注意在选完第10点后结束，不要再选第1点)→ OK

➋对平面进行网格划分

ANSYS Main Menu: Preprocessor →Meshing→Mesh Tool →(Size Controls) Globl: Set →input SIZE (element edge length): 50 →OK (back to MeshTool window)→Mesh → Pick All (in Picking Menu) → Close( the MeshTool window)

➌用旋转法生成筒体模型

ANSYS Main Menu: Preprocessor →Modeling→Operate →Extrude→Elem Ext Opts→select TYPE:SOLID 45→Element sizing options for extrusion No. Elem divs: 1→OK (back to Extrude window)→Areas →About Axis →Pick All(in Picking Menu)→OK→Pick the two keypoints (11,12) of the Symmetrical Axis → OK→input ARC: 90; NSEG: 3→ OK

9.6 模型加位移约束

ANSYS Main Menu: Solution→Define Loads →Apply→Structural→Displacement

➊两截面分别加Z, X方向的约束

ANSYS Utility Menu: Select → Entities…→Nodes → By Location →select X coordinates →input 0→ OK (back to Displacement window)→On Nodes → Pick All(in Picking Menu) → select Lab2:UX →OK →ANSYS Utility Menu: Select → Everything

ANSYS Utility Menu: Select → Entities…→ Nodes → By Location →select Z coordinates →input 0→ OK (back to Displacement window)→On Nodes →Pick All(in Picking Menu) → select Lab2:UZ →OK →ANSYS Utility Menu: Select →Everything

➋底面加Y方向的约束

ANSYS Utility Menu: Select → Entities… → Nodes → By Location →select Y coordinates →input 0→ OK (back to Displacement window)→On Nodes →Pick All(in Picking Menu) →

select Lab2:UY → OK →ANSYS Utility Menu: Select →Everything

9.7 模型加载荷

ANSYS Main Menu: Solution→ Define Loads→Apply→Structural→Pressure →On Areas →pick the Internal Load Surface of model (Total 6 areas) → OK→input V ALUE:200 → Apply →(忽略警告信息)pick the External Load Surface of model → OK→input V ALUE:100→ OK

9.8 分析计算

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

9.9 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: Stress, Von Mises, Def + Undeformed→OK

9.10 退出系统

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

9.11完全的直接命令输入方式操作

finish !finish the last case

/clear,start !restart

/prep7 !preprocessor

et,1,plane42 !define the elements

et,2,solid45

mp,ex,1,210000 !define materials parameters

mp,prxy,1,0.3

k,1,300,,, !define key points of section frame

k,2,480,,,

k,3,480,100,,

k,4,400,100,,

k,5,400,700,,

k,6,480,700,,

k,7,480,800,,

k,8,300,800,,

k,9,300,650,,

k,10,300,150,,

k,11,,,, !define key points of revolving axis

k,12,,800,0

a,1,2,3,4,5,6,7,8,9,10 !link the key points to an area

esize,50,, !define element edge length