压电问题求助啊,版主或者高手们帮帮忙吧(有图和命令流
本帖最后由 mk181 于 2012-7-22 09:57 编辑一下的一个例子,出现问题,求助,请哪位高手帮忙看看,万分感谢
上图为模型,红色画斜线的为压电层,剩余的为水泥层(假设水泥层导电),最外径圆弧加电压100V,内径0V,然后中间压电边缘层都进行了耦合,现在问题是加上电压后,只有最外边一层压电层有产生压电效应,,求高手帮我看看是怎么回事,以下是我的命令流
/prep7
*SET,tpzt,0.005
*SET,tcem,0.02
*SET,r,0.05
ET,1,PLANE223,1001
ET,2,plane183
MP,PERX,1,635
MP,PERY,1,730
MP,PERZ,1,730
TB,PIEZ,1,,,1
TBDATA,18,5.25E-10
TBDATA,11,5.25E-10
TBDATA,7,-1.065e-10
TBDATA,4,-1.065e-10
TBDATA,1,3E-10
TB,ANEL,1,1,,1
TBTEMP,0
TBDATA,1,1.61E-11,-5.52E-12,-5.52E-12
TBDATA,7,1.24E-11,-3.98E-12
TBDATA,12,1.24E-11
TBDATA,16,3.91E-11
TBDATA,19,3.27E-11
TBDATA,21,3.91E-11
MP,PERX,2,1e10
MP,RSVX,2,0 !设电阻率为0
TB,ANEL,2,1,21,1
TBTEMP,0
TBDATA,,7.28E-012,-2.185E-012,-2.185E-012,0,0,0
TBDATA,,1.6E-012,0,0,0,0,2E-012
TBDATA,,0,0,0,1.894E-011,0,0
TBDATA,,0,0,0,,,
CSYS,1
CYL4,0,0,r+tpzt,0,r,90
CYL 4,0,0,r+tpzt+tcem,0, r+tpzt,90
CYL 4,0,0, r+2*tpzt+tcem,0, r+tpzt+tcem,90
CYL 4,0,0, r+2*tpzt+2*tcem,0, r+2*tpzt+tcem,90
CYL 4,0,0, r+3*tpzt+2*tcem,0, r+2*tpzt+2*tcem,90
CYL 4,0,0, r+3*tpzt+3*tcem,0, r+3*tpzt+2*tcem,90
CYL 4,0,0, r+4*tpzt+3*tcem,0, r+3*tpzt+3*tcem,90
AGLUE,1,2,3,4,5,6,7
ASEL,S,AREA,,1
AATT,1,,1
ASEL,S,AREA,,9
AATT,1,,1
ASEL,S,AREA,,11
AATT,1,,1
ASEL,S,AREA,,13
AATT,1,,1
ASEL,S,AREA,,8
AATT,2,,2
ASEL,S,AREA,,10
AATT,2,,2
ASEL,S,AREA,,12
AATT,2,,2
ASEL,ALL
LESIZE,3,,3 !以线3为标准线建立角度间隔为3度的线尺寸
MSHKEY,1 !设置映射网格划分
MSHAPE,0,2D
SHPP,OFF !关闭单元形状检查以允许生成边缘实体网格
AMESH,ALL
NUMMRG,KP !关键点编号压缩合并
/SOLU
CSYS,1
NSEL,S,LOC, Y,0
D,ALL,ALL !施加固定约束
LSEL,S,LINE,,3
NSLL,S,1
CM,BOT,NODE
CP,1,VOLT,ALL
*GET,N1,NODE,0,NUM,MIN
D,N1,VOLT,0
LSEL,S,LINE,,25
NSLL,S,1
CM,TOP,NODE
CP,2,VOLT,ALL
*GET,N2,NODE,0,NUM,MIN
D,N2,VOLT,100
LSEL,S, , , 1
NSLL,S,1
CM,pzt0,NODE
CP,3,VOLT,ALL
LSEL,S, , , 5
NSLL,S,1
CM,pzt1,NODE
CP,4,VOLT,ALL
LSEL,S, , , 9
NSLL,S,1
CM,pzt2,NODE
CP,5,VOLT,ALL
LSEL,S, , , 13
NSLL,S,1
CM,pzt3,NODE
CP,6,VOLT,ALL
LSEL,S, , , 17
NSLL,S,1
CM,pzt4,NODE
CP,7,VOLT,ALL
LSEL,S, , , 21
NSLL,S,1
CM,pzt5,NODE
CP,8,VOLT,ALL !将所有压电层都耦合
ANTYPE,STATIC
NSEL,ALL
ESEL,ALL
SOLVE
自顶~~~~~~~~~~~~~ 怎么没人回答呢。。。。。。 出现的是什么问题啊 alwvke 发表于 2012-7-23 09:34 static/image/common/back.gif
出现的是什么问题啊
现在是施加电压后只有最外层有电压,里面几层都没反应,后来我把单元都改成了plane223,求解后显示“There are elements with negative and positive electric charge reaction solutions for the volt degree of freedom in the model. The analysis is not valid.”计算不出结果,不知道怎么回事啊 mk181 发表于 2012-7-23 10:43 static/image/common/back.gif
现在是施加电压后只有最外层有电压,里面几层都没反应,后来我把单元都改成了plane223,求解后显示“Ther ...
我感觉里面几层没反应应该就是element type没设对,后面的正负电荷不太懂啊,不好意思,论坛上都得不到什么自己问题想要的答案,咱还是自己捉摸吧,总能解决的 alwvke 发表于 2012-7-23 11:13 static/image/common/back.gif
我感觉里面几层没反应应该就是element type没设对,后面的正负电荷不太懂啊,不好意思,论坛上都得不到什 ...
还是自己再想想吧,谢谢了 我的QQ847378687,请楼主加我 1、D,ALL,ALL !施加固定约束
这也包括电压约束为0,显然不正确
2、MP,RSVX,2,0 !设电阻率为0
设置了电阻率为0,对于压电分析并不会自动默认那些都是同电位的,建议把所有同电位的节点(水泥块里和边界的节点)电压耦合。 hy1966 发表于 2012-7-24 18:15 static/image/common/back.gif
1、D,ALL,ALL !施加固定约束
这也包括电压约束为0,显然不正确
2、MP,RSVX,2,0 ...
谢谢您的指点,我又把所有的节点又都耦合了一遍,但是计算时显示“There are elements with negative and positive electric charge reaction solutions for the volt degree of freedom in the model. The analysis is not valid.”,请您帮我看一下是哪里出了问题呢
以下是我的命令流
/prep7
*SET,tpzt,0.005
*SET,tcem,0.02
*SET,r,0.05
ET,1,PLANE223,1001
MP,PERX,1,635
MP,PERY,1,730
MP,PERZ,1,730
TB,PIEZ,1,,,1
TBDATA,18,5.25E-10
TBDATA,11,5.25E-10
TBDATA,7,-1.065e-10
TBDATA,4,-1.065e-10
TBDATA,1,3E-10
TB,ANEL,1,1,,1
TBTEMP,0
TBDATA,1,1.61E-11,-5.52E-12,-5.52E-12
TBDATA,7,1.24E-11,-3.98E-12
TBDATA,12,1.24E-11
TBDATA,16,3.91E-11
TBDATA,19,3.27E-11
TBDATA,21,3.91E-11
MP,PERX,2,1e10
TB,ANEL,2,1,21,1
TBTEMP,0
TBDATA,,7.28E-012,-2.185E-012,-2.185E-012,0,0,0
TBDATA,,1.6E-012,0,0,0,0,2E-012
TBDATA,,0,0,0,1.894E-011,0,0
TBDATA,,0,0,0,,,
CSYS,1
CYL4,0,0,r+tpzt,0,r,30,l
CYL 4,0,0,r+tpzt+tcem,0, r+tpzt,30
CYL 4,0,0, r+2*tpzt+tcem,0, r+tpzt+tcem,30
CYL 4,0,0, r+2*tpzt+2*tcem,0, r+2*tpzt+tcem,30
CYL 4,0,0, r+3*tpzt+2*tcem,0, r+2*tpzt+2*tcem,30
CYL 4,0,0, r+3*tpzt+3*tcem,0, r+3*tpzt+2*tcem,30
CYL 4,0,0, r+4*tpzt+3*tcem,0, r+3*tpzt+3*tcem,30
AGLUE,1,2,3,4,5,6,7
ASEL,S,AREA,,1
AATT,1,,1
ASEL,S,AREA,,9
AATT,1,,1
ASEL,S,AREA,,11
AATT,1,,1
ASEL,S,AREA,,13
AATT,1,,1
ASEL,S,AREA,,8
AATT,2,,1
ASEL,S,AREA,,10
AATT,2,,1
ASEL,S,AREA,,12
AATT,2,,1
ASEL,ALL
LESIZE,3,,3 !以线3为标准线建立角度间隔为3度的线尺寸
MSHKEY,1 !设置映射网格划分
MSHAPE,0,2D
SHPP,OFF !关闭单元形状检查以允许生成边缘实体网格
AMESH,ALL
NUMMRG,KP !关键点编号压缩合并
CSYS,1
NSEL,S,LOC, Y,0
D,all,UX,0
D,all,UY,0 !施加固定约束
LSEL,S,LINE,,3
NSLL,S,1
CM,BOT,NODE
D,BOT,VOLT,0
LSEL,S,LINE,,25
NSLL,S,1
CM,TOP,NODE
CP,2,VOLT,ALL
*GET,N2,NODE,0,NUM,MIN
D,N2,VOLT,100
LSEL,S, , , 1
NSLL,S,1
CM,pzt0,NODE
CP,3,VOLT,ALL
LSEL,S, , , 5
NSLL,S,1
CM,pzt1,NODE
CP,4,VOLT,ALL
LSEL,S, , , 9
NSLL,S,1
CM,pzt2,NODE
CP,5,VOLT,ALL
LSEL,S, , , 13
NSLL,S,1
CM,pzt3,NODE
CP,6,VOLT,ALL
LSEL,S, , , 17
NSLL,S,1
CM,pzt4,NODE
CP,7,VOLT,ALL
LSEL,S, , , 21
NSLL,S,1
CM,pzt5,NODE
CP,8,VOLT,ALL
NSEL,S,LOC,X,0.0525
CP,9,VOLT,ALL
NSEL,S,LOC,X,0.065
CP,10,VOLT,ALL
NSEL,S,LOC,X,0.0775
CP,11,VOLT,ALL
NSEL,S,LOC,X,0.090
CP,12,VOLT,ALL
NSEL,S,LOC,X,0.1025
CP,13,VOLT,ALL
NSEL,S,LOC,X,0.115
CP,14,VOLT,ALL
NSEL,S,LOC,X,0.1275
CP,15,VOLT,ALL
NSEL,S,LOC,X,0.05125
CP,16,VOLT,ALL
NSEL,S,LOC,X,0.05375
CP,17,VOLT,ALL
NSEL,S,LOC,X,0.06
CP,18,VOLT,ALL
NSEL,S,LOC,X,0.070
CP,19,VOLT,ALL
NSEL,S,LOC,X,0.07625
CP,20,VOLT,ALL
NSEL,S,LOC,X,0.07875
CP,21,VOLT,ALL
NSEL,S,LOC,X,0.085
CP,22,VOLT,ALL
NSEL,S,LOC,X,0.095
CP,23,VOLT,ALL
NSEL,S,LOC,X,0.10125
CP,24,VOLT,ALL
NSEL,S,LOC,X,0.10375
CP,25,VOLT,ALL
NSEL,S,LOC,X,0.110
CP,26,VOLT,ALL
NSEL,S,LOC,X,0.120
CP,27,VOLT,ALL
NSEL,S,LOC,X,0.12625
CP,28,VOLT,ALL
NSEL,S,LOC,X,0.12875
CP,29,VOLT,ALL
/SOLU
ANTYPE,STATIC
NSEL,ALL
SOLVE !求解
本帖最后由 hy1966 于 2012-7-25 20:36 编辑
我在ANSYS9.0上运行没有发现你说的问题。
你的帖子中
NSEL,S,LOC, Y,0
D,all,UX,0
D,all,UY,0 !施加固定约束
这表明这个模型的一个边完全刚性。
如果只是为了支撑,D,all,UY,0就可以了,或者选择某个点来约束也可以。如果本身是自由的,也不一定要固定约束。
hy1966 发表于 2012-7-25 19:12 static/image/common/back.gif
我在ANSYS9.0上运行没有发现你说的问题。
你的帖子中
NSEL,S,LOC, Y,0
在ansys9.0里可以得出结果吗,在12.0里面根本无法计算啊,那一边就是固定端,不可以移动的 hy1966 发表于 2012-7-25 19:12 static/image/common/back.gif
我在ANSYS9.0上运行没有发现你说的问题。
你的帖子中
NSEL,S,LOC, Y,0
您看我在最外层施加100V电压时,是不是不应该用“LSEL,S,LINE,,25
NSLL,S,1
CM,TOP,NODE
CP,2,VOLT,ALL
*GET,N2,NODE,0,NUM,MIN
D,N2,VOLT,100”,这好像只是给一个点施加的电压吧,是不是应该用D,top,volt,100呢 你运行一下这个看有没有问题,在ANSYS9.0上没有任何提示、警告和错误
/prep7
*SET,tpzt,0.005
*SET,tcem,0.02
*SET,r,0.05
ET,1,PLANE223,1001
MP,PERX,1,635
MP,PERY,1,730
MP,PERZ,1,730
TB,PIEZ,1,,,1
TBDATA,18,5.25E-10
TBDATA,11,5.25E-10
TBDATA,7,-1.065e-10
TBDATA,4,-1.065e-10
TBDATA,1,3E-10
TB,ANEL,1,1,,1
TBTEMP,0
TBDATA,1,1.61E-11,-5.52E-12,-5.52E-12
TBDATA,7,1.24E-11,-3.98E-12
TBDATA,12,1.24E-11
TBDATA,16,3.91E-11
TBDATA,19,3.27E-11
TBDATA,21,3.91E-11
MP,PERX,2,1e10
TB,ANEL,2,1,21,1
TBTEMP,0
TBDATA,,7.28E-012,-2.185E-012,-2.185E-012,0,0,0
TBDATA,,1.6E-012,0,0,0,0,2E-012
TBDATA,,0,0,0,1.894E-011,0,0
TBDATA,,0,0,0,,,
CSYS,1
CYL4,0,0,r+tpzt,0,r,30,l
CYL 4,0,0,r+tpzt+tcem,0, r+tpzt,30
CYL 4,0,0, r+2*tpzt+tcem,0, r+tpzt+tcem,30
CYL 4,0,0, r+2*tpzt+2*tcem,0, r+2*tpzt+tcem,30
CYL 4,0,0, r+3*tpzt+2*tcem,0, r+2*tpzt+2*tcem,30
CYL 4,0,0, r+3*tpzt+3*tcem,0, r+3*tpzt+2*tcem,30
CYL 4,0,0, r+4*tpzt+3*tcem,0, r+3*tpzt+3*tcem,30
AGLUE,1,2,3,4,5,6,7
ASEL,S,AREA,,1
AATT,1,,1
ASEL,S,AREA,,9
AATT,1,,1
ASEL,S,AREA,,11
AATT,1,,1
ASEL,S,AREA,,13
AATT,1,,1
ASEL,S,AREA,,8
AATT,2,,1
ASEL,S,AREA,,10
AATT,2,,1
ASEL,S,AREA,,12
AATT,2,,1
ASEL,ALL
LESIZE,3,,3 !以线3为标准线建立角度间隔为3度的线尺寸
MSHKEY,1 !设置映射网格划分
MSHAPE,0,2D
!SHPP,OFF !关闭单元形状检查以允许生成边缘实体网格
AMESH,ALL
NUMMRG,KP !关键点编号压缩合并
CSYS,1
NSEL,S,LOC, Y,0
D,all,UX,0
D,all,UY,0 !施加固定约束
LSEL,S,LINE,,3
NSLL,S,1
CM,BOT,NODE
D,BOT,VOLT,0
LSEL,S,LINE,,25
NSLL,S,1
CM,TOP,NODE
CP,2,VOLT,ALL
*GET,N2,NODE,0,NUM,MIN
D,N2,VOLT,100
allsel
ASEL,S, , ,8
NSLA,S,1
CM,pzt0,NODE
CP,3,VOLT,ALL
ASEL,S, , ,10
NSLA,S,1
CM,pzt1,NODE
CP,4,VOLT,ALL
ASEL,S, , ,12
NSLA,S,1
CM,pzt2,NODE
CP,5,VOLT,ALL
finish
/SOLU
ANTYPE,STATIC
ALLSEL
SOLVE !求解
/post1
/CONT,1,25,AUTO
/DSCALE,ALL,1.0
PLNSOL, VOLT,, 0,1.0 hy1966 发表于 2012-7-27 21:40 static/image/common/back.gif
你运行一下这个看有没有问题,在ANSYS9.0上没有任何提示、警告和错误
/prep7
*SET,tpzt,0.005
hy1966老师,请问一下,如何显示计算结果中的径向应力环向应力等,貌似输入RSYS,1后的结果和RSYS,0后的结果是一样的啊
页:
[1]