求助：移动高斯热源激光弯曲成形热应力问题
我正在做激光弯曲成形模拟，模仿前面的例子写了个命令流，温度场看起来是正确的，应力场看变形结果一片红色没有任何变化。不知道什么问题，希望大家帮忙看看。/UNITS,SI
/CONFIG,NRES,10000
/PREP7
ET,1,SOLID70
MP,DENS,1,7680
MPTEMP,1,20,100,200,300,400,500
MPTEMP,7,600,700,800,900,1000,1100
MPTEMP,13,1200,1300,1400
MPDATA,KXX,1,1,52,51.5,48,45,44,40
MPDATA,KXX,1,7,36,32,27,27.5,28,29
MPDATA,KXX,1,13,30,32
MPDATA,C,1,1,479,485,494,515,536,558
MPDATA,C,1,7,588,624,691,693,691,691
MPDATA,C,1,13,691.5,692,692.5
/VIEW,1,1,1,1
BLOCK,0,0.04,0,0.04,0,0.002
SAVE
LESIZE,5,,,40
LESIZE,11,,,2
LSEL,S,LINE,,6
LSEL,A,LINE,,8
LSEL,A,LINE,,3
LSEL,A,LINE,,1
lesize,all,,,40,-0.1,,,,1
MSHKEY,1
VATT,1,1,1
VMESH,1
/PNUM,DEFA
EPLOT
FINISH
/SOLU
LSIZE=0.001
V=0.05
TINC=LSIZE/V
rb=0.004
pi=3.1415926
P=3500
A=0.6
Qmax=2*P*A/(pi*rb*rb)
R=0.004
！希望加热完冷却一段时间
MAX_TIME=80
MAX_X=80
MAX_Y=80
*DIM,laser,TABLE,MAX_X,MAX_Y,MAX_TIME,X,Y,TIME
*DO,K,1,MAX_TIME,1
*DO,I,1,MAX_X,1
laser(I,0,K)=(I-1)*LSIZE
*ENDDO
*DO,J,1,MAX_Y,1
laser(0,J,K)=(J-1)*LSIZE
*ENDDO
*DO,I,1,MAX_X,1
*DO,J,1,MAX_Y,1
XCENTER=V*(K-1)*TINC
YCENTER=0.02
*IF,K,LE,41,THEN
DISTANCE=SQRT(((I-1)*LSIZE-XCENTER)**2+((J-1)*LSIZE-YCENTER)**2)
*IF,DISTANCE,LE,R,THEN
laser(I,J,K)=Qmax/EXP(2*DISTANCE**2/(rb**2))
*ELSE
laser(I,J,K)=0
*ENDIF
*ELSE
laser(I,J,K)=0
*ENDIF
*ENDDO
*ENDDO
laser(0,0,K)=(K-1)*TINC
*ENDDO
ANTYPE,TRANS
TUNIF,27
TREF,20
KBC,1
NSEL,S,EXT
NSEL,R,LOC,Y,0-10E-6,0.04+10E-6
ALLSEL,ALL
SF,ALL,CONV,6,25
*SET,DELT,1
TIMINT,ON
AUTOTS,OFF
TT=1.6
*DO,TM,1E-6,TT,TINC
/VIEW,1,1,1,1
/ANG,1
/REP,FAST
FLST,2,1,5,ORDE,1
FITEM,2,2
/GO
!*
TIME,TM
AUTOTS,0
DELTIM, , , ,1
KBC,0
!*
TSRES,ERASE
FLST,2,1,5,ORDE,1
FITEM,2,2
/GO
!*
!*
SFA,P51X,1,HFLUX,%laser%
SOLVE
OUTRES,ALL,ALL,
/PSF,HFLUX,,2
/REPLOT
*ENDDO
OUTRES,ALL,ALL,
FINISH
SAVE
/FILNAME,THERMAL_STRESS_2
/TITLE,STESS_2
/COM,STRUCTURAL
/PREP7
ETCHG,TTS
MPTEMP,1,20,100,200,300,400,500
MPTEMP,7,600,700,800,900,1000,1100
MPTEMP,13,1200,1300,1400
MPDATA,EX,1,1,205E9,202.5E9,200.5E9,200E9,164E9,96E9
MPDATA,EX,1,7,60E9,40E9,30E9,20E9,10E9,10E9
MPDATA,EX,1,13,10E9,10E9,10E9
MPDATA,ALPX,1,1,11.75E-6,11.85E-6,12.35E-6,12.95E-6,13.45E-6,14E-6
MPDATA,ALPX,1,7,14.5E-6,14.85E-6,14.85E-6,14.85E-6,14.85E-6,14.85E-6
MPDATA,ALPX,1,13,14.85E-6,14.85E-6,14.85E-6
MPDATA,PRXY,1,1,0.3,0.319,0.338,0.357,0.376,0.395
MPDATA,PRXY,1,7,0.414,0.433,0.452,0.471,0.49,0.49
MPDATA,PRXY,1,13,0.49,0.49,0.49
TB,BKIN,1,6,2,1
TBTEMP,20
TBDATA,,347E6,,,,,
TBTEMP,300
TBDATA,,279E6,,,,,
TBTEMP,600
TBDATA,,130E6,,,,,
TBTEMP,900
TBDATA,,46E6,,,,,
TBTEMP,1200
TBDATA,,11.4E6,,,,,
TBTEMP,1400
TBDATA,,7.8E6,,,,,
FINISH
/SOLU
LSCLEAR,SOLID
/SOLU
ANTYPE,TRANS
KBC,1
P=0
TUNIF,27
TREF,20
！固定板料一端，不知道这部分有没有错
NSEL,S,LOC,Y,0,0.005
ALLSEL,ALL
D,ALL, ,0, , , ,UX, , , , ,
D,ALL, ,0, , , ,UY, , , , ,
D,ALL, ,0, , , ,UZ, , , , ,
ALLSEL,ALL
TIMINT,ON
AUTOTS,OFF
TT=1.6
TINC=0.02
*DO,TM,1E-6,TT,TINC
！应该先读入温度场结果还是先定义ＴＩＭＥ？还是都无所谓？
LDREAD,TEMP,,,P+TINC,,2CM,RTH
TIME,P+TINC
P=P+TINC
！上面四句能不能替换为：*DO,TM,1E-6,1.6,0.02／LDREAD,TEMP,,,TM,0,'2CM','RTH'／TIME,TM？
SOLVE
*ENDDO
OUTRES,ALL,ALL,
FINISH
另外还有几个问题：
１．想定义多于六个温度下的屈服强度，应该如何定义，使用
ＴＢ只能定义六个温度。
２．如果希望多道扫描，应该怎样设置
谢谢！
３．如何改变数组中某一维的值，例如上例中‘ｌａｓｅｒ’的ｔｉｍｅ栏数据
４．时间分析选项具体什么作用，什么时候应该打开什么分析时间积分选项
如 ＴＩＭＩＮＴ，１，ＳＴＲＵＣＴＵＲＥ／ＴＩＭＩＮＴ，１，ＴＨＥＲＭ
是不是进行热应力分析必须的
问的比较多，希望大家不要烦，多谢
[ 本帖最后由 peipei_ajr 于 2007-6-7 10:02 编辑 ] 唉，怎么都没人回啊 ，可怜
你耦合的时候使用的结构单元是什么？
怎么没有发下你的结构单元,还是solid70?在热-结构耦合的时候，计算完温度场后，需要结构的耦合单元solid45，还是我看你的程序不仔细那？
回复 #3 qltlx 的帖子
模仿书上的例子 不需要再定义阿 用ETCHG命令不是直接转的吗 如果有典型的例子参考就好了 修改表中X的坐标即可进行多道扫描，即如果X>板宽，则。。。，即可 我也是做焊接的也遇到跟你一样的情况就是应力偶合时温度场无法加载在上面，我是用GUI方式加载.rth檔的方式，有谁可以教一下
还有你雷射焊接速度V=0.05这么快啊
请教你一下这是什么样的指令含义
NSEL,S,EXT
NSEL,R,LOC,Y,0-10E-6,0.04+10E-6
ALLSEL,ALL
SF,ALL,CONV,6,25你这段要改依下，因为程序在加载热源处无法再加载对流边介，也就是你A2面，所以不能用ALL会出现错误(虽然程序会自动帮你去出这项边界，不影响结果)所以你可以改成针对单一面做对流边界加载例如
sfa,6,,CONV,42,25 学习了 我正好这两天也做了一个温度场的，你可以拿来对照一下，费了三天劲，才鼓捣出一个成型的命令流，PC机上运行很吃力，你可以试着改变网格大小。
移动的光源
fini
/clear
/config,nres,10000000
/prep7
et,1,solid70
mp,kxx,1,20.4
mp,kyy,1,20.4
mp,kzz,1,20.4
mp,c,1,523
mp,dens,1,4570
mp,alpx,1,7.06e-6
blc4,,,0.01,0.01,0.005
wpoffs,0.0046
wprota,,,90
vsbw,all
wpoffs,,,0.0008
vsbw,all
lsel,s,length,,0.0046
cm,l1,line
lesize,l1,,,10,0.25
lsel,s,length,,0.005
lsel,u,,,9,12,3
cm,l2,line
lesize,l2,,,10,0.25
lsel,s,,,9,12,3
cm,l3,line
lesize,l3,,,10,4
lsel,s,length,,0.01
cm,l4,line
lesize,l4,0.0001
lsel,s,length,,0.0008
cm,l5,line
lesize,l5,0.0001
wpcsys
vmesh,all
physics,write,thermal
physics,clear
etchg,tts
mptemp,1,20,227,727,927
mpdata,ex,1,1,1e11,0.9815e11,0.6878e11,0.5711e11
mp,prxy,1,0.403
mp,dens,1,4570
mp,alpx,1,7.06e-6
tb,bkin,1,4
tbtemp,20,1
tbdata,1, 8e6,1e10
tbtemp,227,2
tbdata,1, 7.97e6,0.9815e10
tbtemp,727,3
tbdata,1, 5.80e6,0.6878e10
tbtemp,927,4
tbdata,1, 5.78e6,0.5711e10
physics,write,struct
physics,clear
fini
/solu
physics,read,thermal
tunif,20
nsel,s,loc,x,0
nsel,a,loc,x,0.01
sf,all,conv,20,20
nsel,s,loc,y,0
nsel,a,loc,y,0.01
sf,all,conv,20,20
nsel,s,loc,z,0
sf,all,conv,20,20
nsel,s,loc,x,0.0046,0.0054
nsel,r,loc,z,0.005
cm,nodecm,node
*do,i,1,108 !加大此数值是延长时间，降到初始温度
antype,trans
trnopt,full
autots,on
kbc,1
*if,i,le,8,then
time,10/6/100*i
timint,on
deltim,0.001,0.0005,0.01
cmsel,s,nodecm
nsel,r,loc,y,0,0.0001*i
sf,all,hflux,1e8
outres,all,4
allsel
solve
sfdele,all,all
nsel,none
*else
*if,i,le,100,then
time,10/6/100*i
timint,on
deltim,0.001,0.0005,0.01
cmsel,s,nodecm
nsel,r,loc,y,0.0001*(i-8),0.0001*(i)
sf,all,hflux,1e8
outres,all,4
allsel
solve
sfdele,all,all
nsel,none
*else
*if,i,le,107,then
time,10/6/100*i
timint,on
deltim,0.001,0.0005,0.01
cmsel,s,nodecm
nsel,r,loc,y,0.0001*(i-8),0.01
sf,all,hflux,1e8
outres,all,4
allsel
solve
sfdele,all,all
*else
time,10/6/100*i*100000
timint,on
deltim,20,10,100
outres,all,5
allsel
solve
*endif
*endif
*endif
*enddo
save,zuoyonghou,db
........................................
/solu
physics,read,struct
*do,i,1,108 !调入温度值（共108步）
ldread,temp,i,,,,,rth
time,10/6/100*i
antype,static
nropt,full
autots,on
nlgeom,on
lnsrch,on
pred,on
allsel,all
outres,all,all
solve
*enddo
save,reyingli,db
............查看节点力的时程图.......
/post26
nsol,2,节点,s,1
plvar,2 楼主把温度结果贴出几个图片来看看
分不同时间点 分享了！学习学习！ 顶一个啊，正需要 存下来了，正想好好学习一下移动加载，感谢奉献 怎么修改呀？ 6# niufangyong
页:
[1]