问题：
如下模型如何划分网格？
附上生成模型的命令流如下：
finish
/clear,all
/prep7
et,1,solid45
cyl4,3,10
wpoffs,5
sph4,4,2
vsbv,1,2
nummrg,all
vsbw,all
wpoffs,2
vsbw,all
wpoffs,-4
vsbw,all
wprota,-90
vsbw,all
wpoffs,3/2
vsbw,all
wpoffs,-3
vsbw,all
wprota,-90
vsbw,all
vsel,s,loc,z,0,2
vsel,a,loc,z,7,10
vsel,a,loc,y,-5,3/2
esize,10
vsweep,all
wpoffs,2
vsbw,all
wpoffs,-4
vsbw,all
vsel,inve
vplot
esize,10
所生成的完整模型如下：
但是上面中间凹入部分无法划分网格，请问如何进行修改？
答复：
试了一下，做了一个命令流，全部划分六面体网格，只是靠近下凹的部位有部分单元 (总数的约 6%) 的质量受到警告。
命令流如下：
finish
/clear,all
/filn, simwe_meshing, 1
!*
/prep7
!*
et,1,solid45
!*
MPTEMP,
MPTEMP,1,0
MPDATA,EX,1,210000
MPDATA,PRXY,1,0.3
!*
cyl4,3,10
!*
wpoffs,5
sph4,4,2
vsbv,1,2
nummrg,all
!*
VSBW, 3
!*
VDELE, 1, , ,1
numcmp,all
!*
LPLOT
!*
/VIEW,1,1
/ANG,1
/AUTO,1
lplot
!*
wpro,90.000000
VSBW, 1
!*
VDELE, 3, , ,1
!*
VDRAG, 7, , , , , , 13
!*
FLST,2,2,6,ORDE,2
FITEM,2,1
FITEM,2,-2
VOVLAP,P51X
!*
VDELE, 3, , ,1
numcmp,all
!*
KWPAVE, 5
FLST,2,2,6,ORDE,2
FITEM,2,1
FITEM,2,-2
VSBW,P51X
!*
KWPAVE, 1
wpro,90.000000,
FLST,2,3,6,ORDE,3
FITEM,2,1
FITEM,2,3
FITEM,2,-4
VSBW,P51X
!*
numcmp,all
!*
TYPE, 1
MAT, 1
REAL,
ESYS, 0
SECNUM,
!*
WPSTYLE,0
LESIZE,ALL, , ,10, ,1, , ,1,
!*
FLST,5,4,4,ORDE,4
FITEM,5,16
FITEM,5,-17
FITEM,5,30
FITEM,5,32
LSEL, , , ,P51X
!*
LESIZE,all, , ,16,3, , , ,0
lsel,all
!*
LESIZE, 3, , ,10,3, , , ,1
LESIZE, 12, , ,10,0.3333, , , ,0
!*
FLST,5,2,4,ORDE,2
FITEM,5,8
FITEM,5,13
LSEL, , , ,P51X
!*
LESIZE,all, , ,16,0.3333, , , ,0
lsel,all
!*
LESIZE, 5, , ,16,1/3, , , ,0
!*
FLST,5,9,4,ORDE,8
FITEM,5,1
FITEM,5,-2
FITEM,5,4
FITEM,5,6
FITEM,5,-7
FITEM,5,9
FITEM,5,-11
FITEM,5,20
LSEL, , , ,P51X
!*
LESIZE,all, , ,10, , , , ,1
!*
allsel,all
lplot
!*
VSYMM,X,all, , , ,0,0
NUMMRG,KP, , , ,LOW
!*
KWPAVE, 14
CSYS,4
!*
VSYMM,X,all, , , ,0,0
NUMMRG,KP, , , ,LOW
!*
MSHAPE,0,3d
MSHKEY,1
VMESH,all
MSHKEY,0
!*
WPSTYLE,0
/AUTO,1
eplot
csys,0
!*
save
最终的网格如下：
同时，弹出一个警告信息：总计 28400 个单元，有 1704 个单元的质量超过了警告限 (6%)，不过没有错误单元。这种情况，可以忽略该警告，继续进行后续操作。