[求助]在做压电陶瓷的瞬态分析时出现了如下提示！！
各位大虾，我做压电陶瓷的瞬态分析，在向nsel,s,loc,x,10
cp,11,volt,all
*get,front,node,,num,min
ALLSEL
finish
antype,trans,new
trnopt,full
eqslv,sparse
betad,0.1/7650
d,front,volt,800
这时出现一个警告对话框：
Both solid model and finite element model boundary conditions have been
applied to this model. As solid loads are transferred to the nodes or
elements, they can overwrite directly applied loads.
求解完之后，压电陶瓷片一端的位移是0，不知到底哪一步出现了问题，请指教！谢谢！！
[ 本帖最后由 rodge 于 2008-3-14 03:36 编辑 ] 载荷有冲突，你给的代码不全，不知道具体原因，我转几个例子你比较找找毛病吧
（1）对压电陶瓷加z向电压，产生膨胀、收缩
/PREP7
/GRAPHICS,FULL
!############################## parameter #######################
*AFUN,DEG
VOL=0
VOH=20
!########################### Material property #################
!****************** 3---PZT **************************
et,3,solid5 ! UX,UY,UZ,TEMP,VOLT,MAG
!mp,nuxy,3,0.27
mp,dens,3,7.64e3 ! kg/m3
mp,perx,3,8.93e-9 ! F/m
mp,pery,3,8.93e-9 ! F/m
mp,perz,3,6.92e-9 ! F/m
mp,kxx,3,1
mp,murx,3,1
tb,anel,3 ! Anisotropic elastic matrix 72A??? 99.3.4
tbdata,1,11.565e10,6.489e10,6.229e10,0,0,0
tbdata,7,11.565e10,6.229e10,0,0,0
tbdata,12,9.298e10,0,0,0
tbdata,16,1.786e10,0,0
tbdata,19,1.786e10,0
tbdata,21,1.786e10tb,piez,3 ! Piezoelectric matrix 72A??? 99.3.4
tbdata,1,0,0,-12.3082
tbdata,4,0,0,-12.3082
tbdata,7,0,0,20.7574
tbdata,10,0,0,0
tbdata,13,0,17.0357,0
tbdata,16,17.0357,0,0!------------------------ model---------------------------
NUMSTR,KP,1
NUMSTR,LINE,1
NUMSTR,AREA,1block,0,10,0,5,0,1type,3
mat,3
esize,0.5
vmesh,all
!------------boundary condition-----------------------
nsel,s,loc,x,0
d,all,ux
d,all,uy
d,all,uz
! -------------COUPLE THE TWO FACE OF ELECTRODE -------------
nsel,s,loc,z,1
cp,11,volt,all
*get,ntop,node,,num,minnsel,s,loc,z,0
cp,21,volt,all
*get,nbot,node,,num,minALLSfinish
/eof
!-------------------------------------------
/soluantype,staticALLS
d,nTOP,volt,voh
d,nBOT,volt,volESEL,S,TYPE,,3
NSLE
D,ALL,TEMP
!D,ALL,MAG
ALLSnsel,all
esel,allsavesolvefini/eof
（2）对压电陶瓷加x向电压，产生摆动
/PREP7
/GRAPHICS,FULL!############################## parameter #######################
*AFUN,DEGVOL=0
VOH=20!########################### Material property #################!****************** 3---PZT **************************
et,3,solid5 ! UX,UY,UZ,TEMP,VOLT,MAG
!mp,nuxy,3,0.27
mp,dens,3,7.64e3 ! kg/m3
mp,perx,3,8.93e-9 ! F/m
mp,pery,3,8.93e-9 ! F/m
mp,perz,3,6.92e-9 ! F/m
mp,kxx,3,1
mp,murx,3,1tb,anel,3 ! Anisotropic elastic matrix 72A??? 99.3.4
tbdata,1,11.565e10,6.489e10,6.229e10,0,0,0
tbdata,7,11.565e10,6.229e10,0,0,0
tbdata,12,9.298e10,0,0,0
tbdata,16,1.786e10,0,0
tbdata,19,1.786e10,0
tbdata,21,1.786e10tb,piez,3 ! Piezoelectric matrix 72A??? 99.3.4
tbdata,1,0,0,-12.3082
tbdata,4,0,0,-12.3082
tbdata,7,0,0,20.7574
tbdata,10,0,0,0
tbdata,13,0,17.0357,0
tbdata,16,17.0357,0,0
!------------------------ model---------------------------
NUMSTR,KP,1
NUMSTR,LINE,1
NUMSTR,AREA,1block,0,10,0,5,0,1type,3
mat,3esize,0.5vmesh,all!------------boundary condition-----------------------nsel,s,loc,x,0
d,all,ux
d,all,uy
d,all,uz! -------------COUPLE THE TWO FACE OF ELECTRODE -------------nsel,s,loc,x,10
cp,11,volt,all
*get,front,node,,num,minnsel,s,loc,x,0
cp,21,volt,all
*get,back,node,,num,minALLSfinish!-------------------------------------------
/soluantype,staticALLS
d,front,volt,voh
d,back,volt,volESEL,S,TYPE,,3
NSLE
D,ALL,TEMP
D,ALL,MAG
ALLSsavesolvefini/eof
（3）对压电陶瓷加x向位移（压力），产生电压，电压会让结构z变形
/PREP7
/GRAPHICS,FULL
!############################## parameter #######################
*AFUN,DEGVOL=0
VOH=20!########################### Material property #################!****************** 3---PZT **************************
et,3,solid5 ! UX,UY,UZ,TEMP,VOLT,MAG
!mp,nuxy,3,0.27
mp,dens,3,7.64e3 ! kg/m3
mp,perx,3,8.93e-9 ! F/m
mp,pery,3,8.93e-9 ! F/m
mp,perz,3,6.92e-9 ! F/m
mp,kxx,3,1
mp,murx,3,1tb,anel,3 ! Anisotropic elastic matrix 72A??? 99.3.4
tbdata,1,11.565e10,6.489e10,6.229e10,0,0,0
tbdata,7,11.565e10,6.229e10,0,0,0
tbdata,12,9.298e10,0,0,0
tbdata,16,1.786e10,0,0
tbdata,19,1.786e10,0
tbdata,21,1.786e10tb,piez,3 ! Piezoelectric matrix 72A??? 99.3.4
tbdata,1,0,0,-12.3082
tbdata,4,0,0,-12.3082
tbdata,7,0,0,20.7574
tbdata,10,0,0,0
tbdata,13,0,17.0357,0
tbdata,16,17.0357,0,0!------------------------ model---------------------------
NUMSTR,KP,1
NUMSTR,LINE,1
NUMSTR,AREA,1block,0,10,0,5,0,1type,3
mat,3esize,0.5vmesh,all!------------boundary condition-----------------------nsel,s,loc,x,0
d,all,ux
d,all,uy
d,all,uznsel,s,loc,x,10
d,all,ux
d,all,uy
d,all,uz,-0.01!-------------------------------------------
/soluantype,staticALLSESEL,S,TYPE,,3
NSLE
D,ALL,TEMP
D,ALL,MAG
ALLSsavesolvefini/eof
说明:没有贴出结果，请自己运行比较各个例子的结构变形，电压分布,进行研究.转自:simwe 作者:ansyssimulation 请指教 谢谢！对5楼的同志我的回答是肯定的。
知道了
那矩阵是怎么算出来的.请问 建议看一下《ANSYS高级工程有限元分析范例精选》这本书吧 那个警告的问题倒不是很大只是提示你既在有限元模型上加载了，也在几何模型上加载了
程序会自动转换到有限元模型上的 对Z向加电压产生 膨胀 收缩
! -------------COUPLE THE TWO FACE OF ELECTRODE -------------
nsel,s,loc,z,1
cp,11,volt,all
*get,ntop,node,,num,min
nsel,s,loc,z,0
cp,21,volt,all
*get,nbot,node,,num,min
ALLS
finish
/eof
!-------------------------------------------
/solu
antype,static
ALLS
d,nTOP,volt,voh
d,nBOT,volt,vol
ESEL,S,TYPE,,3
NSLE
D,ALL,TEMP
!D,ALL,MAG
ALLS
nsel,all
esel,all
前面的 我都看懂了能不能 麻烦 哪位大大 解释下 后面部分的 APDL命令 干什么用的？ 后面的就是施加电压荷载吧，volt不就是voltage吗，嘿嘿 HAODONGXI 很好的东西哦
页:
[1]