【技術(shù)篇】三梁平面框架結(jié)構(gòu)Ansys有限元分析

如圖3-19所示的框架結(jié)構(gòu),其頂端受均布力作用,用有限元方法分析該結(jié)構(gòu)的位移。結(jié)構(gòu)中各個(gè)截面的參數(shù)都為:

,

,

(1) 進(jìn)入ANSYS(設(shè)定工作目錄和工作文件)

程序 →ANSYS → ANSYS Interactive →Working directory (設(shè)置工作目錄) →Initial jobname(設(shè)置工作文件名): beam3→Run → OK

(2) 設(shè)置計(jì)算類型

ANSYS Main Menu: Preferences… → Structural → OK

(3) 選擇單元類型

ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete… →Add… →beam:2D elastic 3 →OK (返回到Element Types窗口) →Close

(4) 定義材料參數(shù)

ANSYS Main Menu: Preprocessor →Material Props →Material Models→Structural →Linear →Elastic→ Isotropic: EX:3e11 (彈性模量) → OK → 鼠標(biāo)點(diǎn)擊該窗口右上角的“?”來關(guān)閉該窗口

(5) 定義實(shí)常數(shù)以確定平面問題的厚度

ANSYS Main Menu: Preprocessor →Real Constants… →Add/Edit/Delete →Add →Type 1 Beam3→ OK→Real Constant Set No: 1 (第1號(hào)實(shí)常數(shù)), Cross-sectional area:6.8e-4 (梁的橫截面積) →OK →Close

(6) 生成幾何模型

生成節(jié)點(diǎn)

ANSYS Main Menu: Preprocessor →Modeling →Creat→Nodes→ In Active CS→Node number 1 → X:0,Y:0.96,Z:0 →Apply→Node number 2 → X:1.44,Y:0.96,Z:0 →Apply→Node number 3 → X:0,Y:0,Z:0→Apply→Node number 4 → X:1.44,Y:0,Z:0→OK

生成單元

ANSYS Main Menu: Preprocessor → Modeling → Create →Element → Auto Numbered → Thru Nodes → 選擇節(jié)點(diǎn) 1,2(生成單元1)→ apply → 選擇節(jié)點(diǎn) 1, 3(生成單元2)→ apply →選擇節(jié)點(diǎn) 2, 4(生成單元3)→OK

(7) 模型施加約束和外載 左邊加X方向的受力

ANSYS Main Menu: Solution → Define Loads → Apply →Structural → Force/Moment → On Nodes → 選擇節(jié)點(diǎn)1→ apply →Direction of force: FX →VALUE:3000 → OK→

上方施加Y方向的均布載荷

ANSYS Main Menu: Solution → Define Loads → Apply →Structural → Pressure →On Beams →選取單元1(節(jié)點(diǎn)1和節(jié)點(diǎn)2之間)→ apply →VALI:4167→VALJ:4167→OK

左、右下角節(jié)點(diǎn)加約束

ANSYS Main Menu: Solution → Define Loads → Apply →Structural → Displacement → On Nodes → 選取節(jié)點(diǎn)3和節(jié)點(diǎn)4 → Apply → Lab:ALL DOF → OK

(8) 分析計(jì)算

ANSYS Main Menu: Solution → Solve → Current LS →OK → Should the Solve Command be Executed? Y→ Close (Solution is done! ) → 關(guān)閉文字窗口

(9) 結(jié)果顯示

ANSYS Main Menu: General Postproc → Plot Results →Deformed Shape … → Def + Undeformed → OK (返回到Plot Results)

(10) 退出系統(tǒng)

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

(11) 計(jì)算結(jié)果的驗(yàn)證

與MATLAB支反力計(jì)算結(jié)果一致。

/ PREP7 !進(jìn)入前處理

ET,1,beam3 !選擇單元類型

R,1,6.5e-7,6.8e-4 !給出實(shí)常數(shù)(橫截面積、慣性矩)

MP,EX,1,3e11 !給出材料的彈性模量

N,1,0,0.96,0 !生成4個(gè)節(jié)點(diǎn),坐標(biāo)(0,0.96,0),以下類似 N,2,1.44,0.96,0

N,3,0,0,0

N,4,1.44,0,0

E,1,2 !生成單元(連接1號(hào)節(jié)點(diǎn)和2號(hào)節(jié)點(diǎn)) ,以下類似

E,1,3 E,2,4

D,3,ALL !將3號(hào)節(jié)點(diǎn)的位移全部固定

D,4,ALL !將4號(hào)節(jié)點(diǎn)的位移全部固定

F,1,FX,3000 !在1號(hào)節(jié)點(diǎn)處施加X方向的力(3000)

SFBEAM,1,1,PRESS,4167 !施加均布?jí)毫?

FINISH !結(jié)束前處理狀態(tài)

/SOLU !進(jìn)入求解模塊

SOLVE !求解

FINISH !結(jié)束求解狀態(tài)

/POST1 !進(jìn)入后處理

PLDISP,1 !顯示變形狀況

FINISH !結(jié)束后處理