焊接模拟ansys实例

焊接模拟ansys实例

!下面的命令流进行的是一个简单的二维焊接分析, 利用ANSYS单元生死和热-结构耦合分析功能进

!行焊接过程仿真, 计算焊接过程中的温度分布和应力分布以及冷却后的焊缝残余应力。

finish

/clear

/filnam,1-2D element birth and death

/title,Weld Analysis by "Element Birth and Death"

/prep7

/unit,si !采用国际单位制

!******************************************************

et,1,13,4 !13号二维耦合单元, 同时具有温度和位移自由度

et,2,13,4

!1号材料是钢

!2号材料是铝

!3号材料是铜

!铝是本次分析中的焊料, 它将钢结构部分和铜结构部分焊接起来

!下面是在几个温度点下, 各材料的弹性模量

mptemp,1,20,500,1000,1500,2000

mpdata,ex,1,1,1.93e11,1.50e11,0.70e11,0.10e11,0.01e11

mpdata,ex,2,1,1.02e11,0.50e11,0.08e11,0.001e11,0.0001e11

mpdata,ex,3,1,1.17e11,0.90e11,0.30e11,0.05e11,0.005e11

!假设各材料都是双线性随动硬化弹塑性本构关系

!下面是各材料在各温度点下的屈服应力和屈服后的弹性模量

tb,bkin,1,5

tbtemp,20,1

tbdata,1,1200e6,0.193e11

tbtemp,500,2

tbdata,1, 933e6,0.150e11

tbtemp,1000,3

tbdata,1, 435e6,0.070e11

tbtemp,1500,4

tbdata,1, 70e6,0.010e11

tbtemp,2000,5

tbdata,1, 7e6,0.001e11

!

tb,bkin,2,5

tbtemp,20,1

tbdata,1,800e6,0.102e11

tbtemp,500,2

tbdata,1,400e6,0.050e11

tbtemp,1000,3

tbdata,1, 70e6,0.008e11

tbdata,1, 1e6,0.0001e11

tbtemp,2000,5

tbdata,1,0.1e6,0.00001e11

!

tb,bkin,3,5

tbtemp,20,1

tbdata,1,900e6,0.117e11

tbtemp,500,2

tbdata,1,700e6,0.090e11

tbtemp,1000,3

tbdata,1,230e6,0.030e11

tbtemp,1500,4

tbdata,1, 40e6,0.005e11

tbtemp,2000,5

tbdata,1, 4e6,0.0005e11

!

!材料密度(假设为常值)

mp,dens,1,8030

mp,dens,2,4850

mp,dens,3,8900

! 热膨胀系数(假设为常值)

mp,alpx,1,1.78e-5

mp,alpx,2,9.36e-6

mp,alpx,3,1.66e-5

!泊松比(假设为常值)

mp,nuxy,1,0.29

mp,nuxy,2,0.30

mp,nuxy,3,0.30

!热传导系数(假设为常值)

mp,kxx,1,16.3

mp,kxx,2,7.44

mp,kxx,3,393

!比热(假设为常值)

mp,c,1,502

mp,c,2,544

mp,c,3,385

!热膨胀系数(假设为常值)

!由于该13号单元还有磁自由度, 此处假设一磁特性, 但并不影响我们所关心的结果

mp,murx,1,1

mp,murx,2,1

mp,murx,3,1

!假设焊料(铝)焊上去后的初始温度是1500℃

mp,reft,2,1500

mp,reft,3,20

!******************************************************

!下面建立几何模型

csys,0

k,1,0,0,0

k,2,0.5,0,0

k,3,1,0,0 !长1米

k,4,0,0.3,0 !厚度0.3米（二维中叫做宽度）

k,5,0.35,0.3,0

k,6,0.65,0.3,0

k,7,1,0.3,0

a,1,2,5,4

a,2,6,5

a,2,3,7,6

划分网格

esize,0.025

type,2

mat,2

amesh,2

!

esize,0.05 !网格划分出现问题

type,1

mat,1

amesh,1

!

mat,3

amesh,3

eplot

!

/solu

antype,4 ! 瞬态分析

trnopt,full

在模型的左边界加位移约束

nsel,all

*get,minx,node,,mnloc,x

nsel,s,loc,x,minx

d,all,ux,0

*get,miny,node,,mnloc,y

nsel,r,loc,y,miny

d,all,uy,0

!*****假设模型的左右边界处温度始终保持在20摄氏度左右*****

!其他边界条件如对流和辐射等均可施加，此处因为只是示意而已，故只施加恒温边