命令流换成K文件后计算出错

碧海蓝天

我得命令流如下:
可是换成k文件后，在dyna下出现如图错误，望斑竹和各位高手帮小弟看看，不胜感激：
  
!炮弹冲击钢板材料
finish
/cle
/filename,bullet impacts steel plate
/title,Impact of a Bullet into a Concrete Plate
  
/prep7
/view,,1,2,3
/plopts,info,1
/pbc,all,,2
!/pnum,mat,1  
!/num,1  
!*
! --- Enter steel Material Properties For Bullet(刚体)
et,1,mesh200
keyopt,1,1,6
mp,ex,1,210e9
mp,nuxy,1,.28
mp,dens,1,7800
edmp,rigid,1,4,7
!*
et,2,solid164   !定义单元类型(3D)
mp,ex,2,210e9
mp,nuxy,2,.28
mp,dens,2,7800
edmp,rigid,2,4,7
!*  
! --- Create and Mesh Bullet  
k,50000,0,0,9e-2
k,50001,0,10,9e-2
circle,50000,8e-2,50001,,90      ! 以第 1 个keypoin为圆心画弧线 ，半径为8e-2,画出1/4个圆
kdele,50000,50001
/replot
k,3,8e-2,0,81e-2
k,4,0,,81e-2
k,5,0,0,9e-2
l,1,3
l,3,4
l,4,5
l,5,2
l,1,5
al,1,5,6
al,2,3,4,6
esize,0.015
mshape,0,2d
mshkey,1
mat,1
amesh,all
vrotat,1,2,,,,,2,4,360,4
/pnum,volu,1  
/number,0
vplot,all
mat,2
vmesh,all
!*
cm,nbullet,node
cm,ebullet,elem
!*
! --- 对炮弹定义初始速度
edvel,vgen,nbullet,,,-1000.0
!edivelo,nbullet,,,-1000.0
!*
! --- 钢板的材料参数
et,3,solid164   !定义单元类型
mp,ex,3,210e9
mp,nuxy,3,.28
mp,dens,3,7800
! tb材料定义
!*
!mpmod,1,19
tb,plaw,3,,,1
tbdata,1,360e6
tbdata,2,763e6
tbdata,3,0
tbdata,4,40.0
tbdata,5,5.0
tbdata,6,0.75
! --- 钢板建立模型
block,2,-2,2,-2,-0.1,-1.1
esize,.1
mat,3
type,3
vmesh,9
esel,s,mat,,3
nsle
cm,nplate,node
cm,eplate,elem
nsel,all
esel,all
!*
! --- 对钢板的底边施加约束
nsel,s,loc,z,-1.1
nsel,u,loc,x,-1.99,1.99
d,all,ux,0,,,,uy,uz
nsel,s,loc,z,-1.1
nsel,u,loc,y,-1.99,1.99
d,all,ux,0,,,,uy,uz
nsel,all
/replot
eplot
!*
finish  
/prep7
!*  
! --- 定义接触 Eroding Surface-To-Surface Contact Between Bullet and Plate
edcgen,ests,nbullet,nplate,,,,,,1,1,1 ! Set V1=V2=V3=1  
edcontact,1.0,,2,,,,2,,0 ! SFSI, ORIE, and PENCHK explicitly set
!*
! --- 对后处理POST26定义集合
nsel,s,loc,x,-2,2
nsel,r,loc,z,-1.1,0.81
nsel,r,loc,y,-2,2
esln
nsle
cm,elems,elem
cm,nodes,node
nsel,all
esel,all
eplot
finish
!*
/solu
time,.002 ! Endtime
edrst,10 ! Time Increment For Results Output
edopt,,,lsdyna
edhtime,100
edhist,nodes
edhist,elems
eplot
save
!*
finish
!求解
/solu  
/status,solu  
solve

belldingding

把K文件发过来给你看看

yuyuyu

SECTION ID 1 没有设置
  
设置了就好了

femman

In your model you have only 2 parts, Part 2 for bullet, Part 3 for wall, so delete part 1 and relevant section. everything is OK! look like that:

碧海蓝天

femman ,
I have solved it, however,I should still thank you for your suggestion.
  
my method is following: delete the mesh200, and then it's ok!
  
can you tell me how you crack it?you said I should delete part 1, that's to say, delete mesh200?
  
I think different person has different method. it's most important to learn from each other!

femman

I use the Keywords file,which is a direct input for LS-DYNA.
That is also what ANSYS/LS-DYNA must have done in the background.
The point of your problem is "et, mesh200" (i.e.Part1). It is unnecessary.