ANSYS热分析的经典实例（圆筒罐热分析）

2017-03-03  by:CAE仿真在线  来源:互联网

一圆筒形的罐有一接管,罐外径为3英尺,壁厚为0.2英尺,接管外径为0.5英尺,壁厚为0.1英尺,罐与接管的轴线垂直且接管远离罐的端部。如图所示:

罐内流体温度为华氏450度,与罐壁的对流换热系数年为250BUT/hr-ft2-oF,接管内流体的温度为华氏100度,与管壁的对流换热系数随管壁温度而变。接管与罐为同一种材料,它的热物理性能如下表所示:

温度	70	200	300	400	500	oF
密度	0.285	0.285	0.285	0.285	0.285	lbm/in3
导热系数	8.35	8.90	9.35	9.8	10.23	Btu/hr-ft-oF
比热	0.113	0.117	0.119	0.122	0.125	Btu/lbm-oF
对流系数*	426	405	352	275	221	Btu/hr-ft2-oF

*接管内壁对流系数

求罐与接管的温度分布。

以下分别列出LOG文件及菜单操作

/prep7

/title,Steady-state thermal analysis of pipe junction

/units,bin !使用英制单位

et,1,90 !定义热单元

mp,dens,1,.285 !密度

mptemp,,70,200,300,400,500 !建立温度表

mpdata,kxx,1,,8.35/12,8.90/12,9.35/12,9.80/12,10.23/12 !导热系数

mpdata,c,1,,0.133,0.177,0.119,0.122,0.125 !比热

mpdata,hf,2,,426/144,405/144,352/144,275/144,221/144 !接管对流系数

!定义几何模型参数

ri1=1.3 !罐内半径

ro1=1.5 !罐外半径

z1=2 !罐长

ri2=0.4 !接管内半径

ro2=0.5 !接管外半径

z2=2 !接管长

!建立几何模型

cylind,ri1,ro1,,z1,,90 !1/4罐体

wprota,0,-90 !将工作平面旋转到垂直于接管轴线

cylind,ri2,ro2,,z2,-90 !1/4接管

wpstyl,defa !将工作平面恢复到默认状态

vovlap,1,2 !进行OVERLAP布尔操作

/pnum,volu,1 !打开实体编号

/view,,-3,-1,1 !定义显示角度

/type,,4

/title, Volumes used in building pipe/tank junction

vplot !显示实体

vdele,3,4,,1 !删除多余实体

!划分网格

asel,,loc,z,z1 !选择罐上Z=Z1的面

asel,a,loc,y,0 !添加选择罐上Y=0的面

cm,aremote,area !创建名为AREMOTE的面组

/pnum,area,1

/pnum,line,1

/title,lines showing the portion being modeled

aplot

/noerase

lplot

/erase

accat,all !组合罐远端的面及线,为映射划分网

!格作准备

lccat,12,7

lccat,10,5

lesize,20,,,4 !在接管壁厚方向分4等分

lesize,40,,,6 !在接管长度方向分6等分

lesize,6,,,4 !在罐壁厚方向分4等分

allsel !选择EVERYTHING

esize,0.4 !设定默认的单元大小

mshape,0,3d !选择3D映射网格

mshkey,1

save !保存数据文件

vmesh,all !划分网格,产生节点与单元

/pnum,defa

/title, elements in portion being modeled

eplot !显示单元

finish

!加载求解

/solu

antype,static !定义为稳态分析

nropt,auto !设置求解选项为Program-chosen

!Newton-Raphson

tunif,450 !设定初始所有节点温度

csys,1 !变为柱坐标

nsel,s,loc,x,ri1 !选择罐内表面的节点

sf,all,conv,250/144,450 !定义对流边界条件

cmsel,,aremote !选择AREMOTE面组

nsla,,1 !选择属于AREMOTE面组的节点

d,all,temp,450 !定义节点温度

wprota,0,-90 !将工作平面旋转到垂直于接管轴线

cswpla,11,1 !创建局部柱坐标

nsel,s,loc,x,ri2 !选择接管内壁的节点

sf,all,conv,-2,100 !定义对流边界条件

allsel !选择EVERYTHING

/pbc,temp,,1 !显示所有温度约束

/psf,conv,,2 !显示所有对流边界

/title,Boundary conditions

nplot !显示节点

wpstyle,defa !工作平面恢复默认状态

csys,0 !变为直角坐标

autots,on !打开自动步厂长

nsubst,50 !设定子步数量

kbc,0 !设定为阶越

outpr,nsol,last !设置输出

solve !进行求解

finish

!进入后处理

/post1

/title,Temperature contrours at pipe/tank junction

plnsol,temp !显示温度彩色云图

finish

/exit,all

菜单操作

1、 设定标题:Utility Menu>File>Change Title,输入Steady-State analysis of pipe junction,选择OK;

2、 设定单位制:在命令提示行输入/UNITS,BIN;

3、 定义单元类型:Main Menu>Preprocesor>Element Type>Add/Edit/Delete,选择Thermal Solid, Bricck 20 node 90号单元;

4、 定义材料属性

(1) Main Menu>Preprocessor>Material Props>-Constant->Isotropic,默认材料编号1,在DENSITY框中输入0.285;

(2) Main Menu>Preprocessor>Material Props>-Temp Dependent->Temp Table,输入温度70,200,300,400,500;

(3) Main Menu>Preprocessor>Material Props>-Temp Dependent->Prop Table,选择导热系数KXX,材料编号为1,输入与温度表对应的导热系数8.35/12,8.9/12,9.35/12,9.8/12,10.23/12,选择APPLY;

(4) 选择比热C,材料编号为1,输入0.113,0.117,0.119,0.122,0.125,选择APPLY;

(5) 选择对流系数HF,材料编号为2,输入426/144,405/144,352/144,275/144, 221/144,选择OK。

5、 定义几何模型参数:Utility Menu>Parameters>Scalar Parameters,输入ri1=1.3,ro1=1.5,z1=2,ri2=0.4,ro2=0.5,z2=2;

6、 建立几何模型

(1) Main Menu>Preprocessor>-Modeling->Create>-Volumes->Cylinder>By

Dimensions, Outer radius框中输入ro1,Optional inner radium框中输入ri1,Z coordinates框中输入0和Z1,Ending angle框中输入90;

(2) Utility Menu>WorkPlane>Offset WP by Increments,在XY,YZ,ZX框中输入0,-90;

(3) Main Menu>Preprocessor>-Modeling->Create>-Volumes->Cylinder>By

Dimensions; Outer radius框中输入ro2, Optional inner radium框中输入ri2, Z coordinates框中输入0和Z2,Starting angle框中输入-90,Ending angle框中输入0;

(4) Utility Menu>WorkPlane>Align WP with>Global Cartesian;

7、 进行布尔操作:Main Menu>Preprocessor>-Modeling->Operate>-Booleans->

Overlap >Volumes,选择Pick All;

8、 观察几何模型

(1) Utility Menu>PlotCtrls>Numbering,打开volumes;

(2) Utility Menu>PlotCtrls>View Direction, 在Coords of view point框中输入-3,-1,1;

9、 删除多余实体Main Menu>Preprocessor>-Modeling->Delete>Volume and Below,在命令输入行输入3,4回车;

10、 创建组AREMOTE

(1) Utility Menu>Select>Entities,选择Area, By location, Z Coordinates, 在Min, Max框中输入Z1,选择APPLY,Y Coordinates, 在Min, Max框中输入0,OK;

(2) Utility Menu>Select>Comp/Assembly>Create Component,在Component name框中输入AREMOTE, 在Components is made of菜单中选择AREA;

11、 组合面及线

(1) Main Menu>Preprocessor>-Meshing->Mesh>-Volumes->Mapped>

-Concatenate->Area,选择Pick all;

(2) Main Menu>Preprocessor>-Meshing->Mesh>-Volumes->Mapped>

-Concatenate->Lines,在命令行中输入12,7回车,选择APPLY,在命令行中输入10,5回车,OK;

12、 设定网格密度

(1) Main Menu>Preprocessor>-Meshing->Size Cntrls>Picked Lines,选择线6和20,OK,在No. of element divisions框中输入4,OK;

(2) Main Menu>Preprocessor>-Meshing->Size Cntrls>Picked Lines,选择线40,OK,在No. of element divisions框中输入6,OK;

(3) Utility Menu>Select>Everything;

(4) Main Menu>Preprocessor>-Meshing->Size Cntrls>-Global->Size,在element edge length框中输入0.4,OK;

13、 划分网格:Main Menu>Preprocessor>-Meshing->Mesh>-Volumes->Mapped>4 to 6 sides,选择Pick All;

14、 定义求解类型及选项

(1) Main Menu>Solution>-Analysis Type->New Analysis,选择Steady-State;

(2) Main Menu>Solution>-Analysis Options,选择Program-chosen;

15、 施加对流载荷

(1) Utility Menu>WorkPlane>Change Active CS to>Global Cylindrical;

(2) Utility Menu>Select>Entities,选择Nodes, By location, X,在Min, Max框中输入ri1,OK;

(3) Main Menu>Solution>-Loads->Apply>-Thermal->Convection>On Nodes,选择Pick All, 输入250/144及450,OK;

16、 在AREMOTE组上施加温度约束

(1) Utility Menu>Select>Comp/Assembly>Select Comp/Assembly,选aremote;

(2) Utility Menu>Select>Entities,选择Nodes, Attached to, On the Area all, OK;

(3) Main Menu>Solution>-Loads->Apply>-Thermal->Temperature>On Nodes,选择Pick all,输入45,OK;

17、 施加与温度有关的对流边界条件

(1) Utility Menu>WorkPlane>Offset WP by Increments,在XY,YZ,ZX Angles框中输入0,-90,OK;

(2) Utility Menu>WorkPlane>Local Coordinate Systems>Create Local CS>At WP Origin,在Type of coordinate system菜单中,选择Cylindrical 1,OK;

(3) Utility Menu>Select Entities,选择Nodes, By location, X, 在Min, Max框中输入ri2,OK;

(4) Main Menu>Solution>-Loads->Apply>-Thermal->Convection>On Nodes,选择Pick All,在Film coefficient框中输入-2,在Bulk temperature框中输入100,OK;

(5) Utility Menu>Select>Everything;

(6) Utility Menu>PlotCtrls>Symbols,在Show pres and convect as菜单中选择Arrow, OK;

(7) Utility Menu>Plot>Nodes;

18、 恢复工作平面及坐标系统

(1) Utility Menu>WorkPlane>Change Active CS to>Global Cartesian;

(2) Utility Menu>WorkPlane>Align WP with>Global Cartesian;

19、 设定载荷步选项:

Main Menu>Solution>-Load Step Options->Time/Frequenc>Time and Substeps,在Number of substeps框中输入50,设置Automatic time stepping为On;

20、 求解:Main Menu>Solution>-Solve->Current LS

21、 显示温度分布彩色云图: Main Menu>General Postproc>Plot Results>-Contour Plot->Nodal Solu,选择Temperature TEMP。

相关标签搜索：ANSYS热分析的经典实例（圆筒罐热分析） Ansys有限元培训 Ansys workbench培训 ansys视频教程 ansys workbench教程 ansys APDL经典教程 ansys资料下载 ansys技术咨询 ansys基础知识 ansys代做 Fluent、CFX流体分析 HFSS电磁分析 Abaqus培训