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，故只施加恒温边界条件
nsel,all
*get,minx,node,,mnloc,x
nsel,s,loc,x,minx
d,all,temp,20
nsel,all
*get,maxx,node,,mxloc,x
nsel,s,loc,x,maxx
d,all,temp,20
由于第2个面是焊接所在区域，因此首先将该区域的单元“杀死”
nna=2
esel,all
*get,emax,elem,,num,max
asel,s,area,,nna
esla
*get,nse,elem,,count
*dim,ne,,nse
*dim,nex,,nse
*dim,ney,,nse
*dim,neorder,,nse
mine=0
!**********************************************
!下面的do循环用于将焊料区的单元按其形心y坐标排序
!以便后面模拟焊料由下向上逐步“生长”过程
*do,i1,1,nse
esel,u,elem,,mine
*get,nse1,elem,,count
ii=0
*do,i,1,emax
*if,esel(i),eq,1,then
ii=ii+1
ne(ii)=i
*endif
*enddo
*do,i,1,nse1
*get,ney(i),elem,ne(i),cent,y
*get,nex(i),elem,ne(i),cent,x
*enddo
miny=1e20
minx=1e20
*do,i,1,nse1
*if,ney(i),lt,miny,then
miny=ney(i)
minx=nex(i)
mine=ne(i)
*else
*if,ney(i),eq,miny,then
*if,nex(i),lt,minx,then
miny=ney(i)
minx=nex(i)
mine=ne(i)
*endif
*endif
*endif
*enddo
neorder(i1)=mine
*enddo
!************************************************************** max_tem=1500 !按照前面假设，焊料的初始温度为1500℃
dt1=1e-3 !用于建立初始条件的一个很小的时间段
dt=5 !焊接一个单元所需的时间
t=0 !起始时间
esel,all
eplot
/auto,1
/replot
*do,i,1,nse
ekill,neorder(i)
esel,s,live
eplot
*enddo
allsel,all
outres,all,all
ic,all,temp,20
kbc,1
timint,0,struct
timint,1,therm
timint,0,mag
tintp,0.005,,,1,0.5,0.2
!
nsub1=2
nsub2=40
!*************************************************
*do,i,1,nse
ealive,neorder(i)
esel,s,live
eplot
esel,all
!******下面的求解用于建立温度的初始条件******
t=t+dt1
time,t
nsubst,1
*do,j,1,4
d,nelem(neorder(i),j),temp,max_tem
*enddo
solve
!****下面的求解用于保证初始的升温速度为零****
t=t+dt1
time,t
solve
!*********下面的步骤用于求解温度分布**********
*do,j,1,4
ddele,nelem(neorder(i),j),temp
*enddo
t=t+dt-2*dt1
time,t
nsubst,nsub1
solve
*enddo
t=t+50000 !*********下面的步骤用于冷却过程求解***** time,t
nsubst,nsub2
solve
save
finish
后处理过
程
/post1
!**************下面的一系列命令用于生成应力的动画文件******* /seg,dele
/cont,1,15,0,1200e6/16,1200e6
/dscale,1,1.0
avprin,0,0
avres,1
/seg,multi,stress1,0.1
esel,all
*do,i,1,nse
esel,u,elem,,neorder(i)
*enddo
*do,i,1,nse
esel,a,elem,,neorder(i)
set,(i-1)*3+1,1
plnsol,s,eqv
*do,j,1,nsub1
set,(i-1)*3+3,j
plnsol,s,eqv
*enddo
*enddo
*do,i,1,nsub2
set,(nse-1)*3+4,i
plnsol,s,eqv
*enddo
/seg,off,stress1,0.1
/anfile,save,stress1,avi
!**********下面的一系列命令用于生成温度的动画文件************ /seg,dele
/cont,1,15,0,1500/16,1500
/dscale,1,1.0
avprin,0,0
avres,1
/seg,multi,temp1,0.1
esel,all
*do,i,1,nse
esel,u,elem,,neorder(i)
*enddo
*do,i,1,nse
esel,a,elem,,neorder(i)
set,(i-1)*3+1,1
plnsol,temp
*do,j,1,nsub1
set,(i-1)*3+3,j
plnsol,temp
*enddo
*enddo
*do,i,1,nsub2
set,(nse-1)*3+4,i
plnsol,temp
*enddo
/seg,off,temp1,0.1
/anfile,save,temp1,avi
finish。