对于此模型网格划分各位有什么好建议

markzhang_33

模型：
建模思路：分别建立中间的旋转体和周边的叶片，用Vadd命令将两体作布尔加运算，得到单元体：

再用Vgen命令，将单元体拷贝绕轴旋转，生成模型

目前网格划分遇到问题：element type为solid45，esize,8,0。用mshpe,1,3d  vmesh对模型进行四面体网格划分,弹出如下对话框：
这个2.5度从何而来，为什么是定义的2.5度？是不是角度太小对之后计算分析有影响（比如模态分析，因角度太小，无法计算出各阶频率，程序无响应）？个人认为是在叶片和旋转体的结合处出现角度过小的问题，但不知道如何修改，各位有什么好建议。另外，改用smrt命令也出现类似问题，只不过角度数量不同。会不会和elementtype的选择也有一定关系，请各位赐教。
附上建模到网格划分APDL命令流:
finish
/clear
/filenam,a
/title,b

r1=150.955
r2=16.021
r3=32
r4=129.455
r5=169.549
h1=45
h2=29.5
h3=1
h4=11
h5=5
h6=9
h7=19
h8=3.126
h9=3
h10=32.28
h11=4

s1=10.6
s2=3.1
s3=2.9
s4=18
s5=79.834
s6=5
s7=159.924
s8=20.266
s9=19.983
s10=16.569
s11=4.349
s12=20.037

pi=4*atan(1)
d2r=pi/180
ang=16.276
ang1=8.879
ang2=21.457
ang3=13
n_impeller=55

/view,1,0.8,-0.5,-0.5
/ang,1,60
/pnum,line,1
/pnum,area,0
/pnum,volu,0
/number,1
/prep7
k,25,h10,s7,0
k,26,-kx(25),ky(25),0
k,1,h2,0,0
k,2,kx(1),r2,0
k,3,kx(2),ky(2)+s2,0
k,4,kx(3)-h3,ky(3),0
k,5,kx(4),ky(4)+s3,0
k,6,kx(5)-h4,ky(5),0
k,7,kx(6),ky(6)+s1-s2-s3,0
k,8,kx(7)-h5,ky(7),0
k,9,kx(8),ky(8)+s4,0
k,10,kx(9)-h6,ky(9),0
k,11,kx(10),ky(10)+s5,0
k,12,kx(11)+h7,ky(11),0
k,13,kx(12),ky(12)+s6,0
k,14,kx(25)-r3*cos(ang*d2r),ky(25)-r3*sin(ang*d2r),0
k,15,-kx(14),ky(14),0
k,16,-kx(13),ky(13),0
k,17,-kx(12),ky(12),0
k,18,-kx(11),ky(11),0
k,19,-kx(10),ky(10),0
k,20,-kx(9),ky(9),0
k,21,-kx(8),ky(8),0
k,22,kx(21)-h9,ky(21),0
k,23,kx(22),ky(22)-s1,0
k,24,kx(1)-h1,ky(1),0
k,27,-h1/2,r4,0
k,28,-h1/2,ky(27),kz(27)-h11
k,29,-h1/2,ky(28)+s8,kz(28)
k,30,-h1/2,ky(29)+s9*cos(ang3*d2r),kz(29)-s9*sin(ang3*d2r)
k,33,-h1/2,ky(27)+s12,kz(27)
k,32,-h1/2,ky(33)+s11*cos(ang1*d2r),kz(33)-s11*sin(ang1*d2r)
k,31,-h1/2,ky(32)+s10*cos(ang2*d2r),kz(32)-s10*sin(ang2*d2r)

lstr,2,3
lstr,3,4
lstr,4,5
lstr,5,6
lstr,6,7
lstr,7,8
lstr,8,9
lstr,9,10
lstr,10,11
lstr,11,12
lstr,12,13
larc,13,14,25,r3
lstr,14,15
larc,15,16,26,r3
lstr,16,17
lstr,17,18
lstr,18,19
lstr,19,20
lstr,20,21
lstr,21,22
lstr,22,23
lstr,23,2
al,all
cm,a-section1,area
asel,none
a,27,28,29,30,31,32,33
cm,a_impeller,area
allsel,all
vrotat,a-section1,,,,,,1,24,360/n_impeller,1
cm,v-section1,volu
vext,a_impeller,,,h1,,,,,
cm,v_impeller,volu
vadd,v_impeller,v-section1
cm,v-unit,volu

wpro,,,-90
cswpla,11,1,1,1
csys,11
vgen,n_impeller,v-unit,,,,360/n_impeller,,,0
cm,v-whole,volu

et,1,solid45
mp,ex,1,2e11
mp,nuxy,1,0.3
mp,dens,1,7800
vsel,all
vatt,1,,1,0
esize,8,0
mshape,1,3d
vmesh,v-whole
finish
save

ferriswanglei

1.可用周期循环模型来做，见帮助文档 // Modeling and Meshing Guide // 7. Generating the Mesh // 7.8. Using CPCYC and MSHCOPY Commands
2.该警告是指体1中某些单元的角度小于2.5，网格质量比较差。
http://forum.simwe.com/forum.php ... 7491&highlight=

markzhang_33

ferriswanglei 发表于 2011-11-13 09:26
1.可用周期循环模型来做，见帮助文档 // Modeling and Meshing Guide // 7. Generating the Mesh // 7.8. U ...

感谢前辈给的指点，其实周期循环这个想法我之前也想到过。我现在的问题还是在两实体相交处的网格划分。感觉不好画。

ferriswanglei

通过复制面网格来实现，还有如果用循环对称，楼主选择的扇区要改变一下，使扇区两边面的形状完全一样，然后复制网格。

ferriswanglei

/filenam,a  
/title,b
*SET,r1,150.955
*SET,r2,16.021  
*SET,r3,32  
*SET,r4,129.455
*SET,r5,169.549
*SET,h1,45  
*SET,h2,29.5
*SET,h3,1   
*SET,h4,11  
*SET,h5,5   
*SET,h6,9   
*SET,h7,19  
*SET,h8,3.126   
*SET,h9,3   
*SET,h10,32.28  
*SET,h11,4  
*SET,s1,10.6
*SET,s2,3.1
*SET,s3,2.9
*SET,s4,18  
*SET,s5,79.834  
*SET,s6,5   
*SET,s7,159.924
*SET,s8,20.266  
*SET,s9,19.983  
*SET,s10,16.569
*SET,s11,4.349  
*SET,s12,20.037
*SET,pi,4*atan(1)   
*SET,d2r,pi/180
*SET,ang,16.276
*SET,ang1,8.879
*SET,ang2,21.457
*SET,ang3,13
*SET,n_impeller,55  
/prep7  
k,25,h10,s7,0   
k,26,-kx(25),ky(25),0   
k,1,h2,0,0  
k,2,kx(1),r2,0  
k,3,kx(2),ky(2)+s2,0
k,4,kx(3)-h3,ky(3),0
k,5,kx(4),ky(4)+s3,0
k,6,kx(5)-h4,ky(5),0
k,7,kx(6),ky(6)+s1-s2-s3,0  
k,8,kx(7)-h5,ky(7),0
k,9,kx(8),ky(8)+s4,0
k,10,kx(9)-h6,ky(9),0   
k,11,kx(10),ky(10)+s5,0
k,12,kx(11)+h7,ky(11),0
k,13,kx(12),ky(12)+s6,0
k,14,kx(25)-r3*cos(ang*d2r),ky(25)-r3*sin(ang*d2r),0
k,15,-kx(14),ky(14),0   
k,16,-kx(13),ky(13),0   
k,17,-kx(12),ky(12),0   
k,18,-kx(11),ky(11),0   
k,19,-kx(10),ky(10),0   
k,20,-kx(9),ky(9),0
k,21,-kx(8),ky(8),0
k,22,kx(21)-h9,ky(21),0
k,23,kx(22),ky(22)-s1,0
k,24,kx(1)-h1,ky(1),0   
k,27,-h1/2,r4,0
k,28,-h1/2,ky(27),kz(27)-h11
k,29,-h1/2,ky(28)+s8,kz(28)
k,30,-h1/2,ky(29)+s9*cos(ang3*d2r),kz(29)-s9*sin(ang3*d2r)  
k,33,-h1/2,ky(27)+s12,kz(27)
k,32,-h1/2,ky(33)+s11*cos(ang1*d2r),kz(33)-s11*sin(ang1*d2r)
k,31,-h1/2,ky(32)+s10*cos(ang2*d2r),kz(32)-s10*sin(ang2*d2r)
lstr,2,3
lstr,3,4
lstr,4,5
lstr,5,6
lstr,6,7
lstr,7,8
lstr,8,9
lstr,9,10   
lstr,10,11  
lstr,11,12  
lstr,12,13  
larc,13,14,25,r3
lstr,14,15  
larc,15,16,26,r3
lstr,16,17  
lstr,17,18  
lstr,18,19  
lstr,19,20  
lstr,20,21  
lstr,21,22  
lstr,22,23  
lstr,23,2   
al,all  
cm,a-section1,area  
asel,none   
a,27,28,29,30,31,32,33  
cm,a_impeller,area  
allsel,all  
vrotat,a-section1,,,,,,1,24,360/n_impeller,1
cm,v-section1,volu  
vext,a_impeller,,,h1,,,,,   
cm,v_impeller,volu  
wprot,,,90  
CSWPLA,11,1,1,1,
CSYS,11
FLST,3,1,6,ORDE,1   
FITEM,3,1   
VGEN, ,P51X, , , ,180/n_impeller, , , ,1
VADD,ALL
ET,1,MESH200
ET,2,SOLID186   
KEYOPT,1,1,5
KEYOPT,1,2,0
ESIZE,2,0,  
MSHKEY,0
AMESH,1
MSHCOPY,AREA,1,25,11,0,-360/n_impeller,0,0.0001,A1,A2  
MSHKEY,0
MSHAPE,1,3d
VMESH,3
CPCYC,ALL,0.0001,11,0,360/n_impeller,0,0

markzhang_33

ferriswanglei 发表于 2011-11-15 15:47
/filenam,a  
/title,b
*SET,r1,150.955

前辈，请受小弟一拜。

markzhang_33

ferriswanglei 发表于 2011-11-15 15:47
/filenam,a  
/title,b
*SET,r1,150.955

但是依然存在网格质量问题。

markzhang_33

ferriswanglei 发表于 2011-11-15 15:47
/filenam,a  
/title,b
*SET,r1,150.955

前辈，这个模型做了下自由模态分析，发现有问题，不加任何约束，前六阶的频率为什么会有不是0的结果，问题出在哪？
apdl命令（接在网格划分之后）：
/solu
mp,ex,1,7e10
mp,nuxy,1,0.30
mp,dens,1,2700
antype,modal

modopt,lanb,15,0,5000,,off
solve
finish

/solu
expass,1
mxpand,15,0,5000,1,0.001
outres,all,all
outpr,all,all
solve
finish
save

/post1
set,list

maoxy

有没有workbench的循环对称模型实例？  

jacobi

楼主的模型有些小问题，
这些东西会影响网格划分。