- 积分
- 0
- 注册时间
- 2007-10-5
- 仿真币
-
- 最后登录
- 1970-1-1
|
发表于 2009-10-15 16:01:06
|
显示全部楼层
来自 辽宁沈阳
利用MPC184单元模拟扭矩载荷
其主要思路是,在零件一端新建一个“主”节点,然后利用MPC184单元连接这个节点和零件一端的所有节点。可以定义MPC184单元的关键选项,设置其为刚性梁。最后在“主”节点上施加弯矩即可。
/TITLE,TORSION TEST CASE USING MPC184 ELEMENTS
/PREP7
CYL4, , ,.5, , , ,4
/VIEW, 1 ,1,1,1
/REP
!*
ET,1,SOLID92
MP,EX,1,30E6
MP,PRXY,1,.3
MSHAPE,1,3D
MSHKEY,0
VMESH,ALL
N,10000,0,0,5 !CREATE 'MASTER' NODE FOR MPC184'S
ASEL,S,,,2
LSLA,S,1
NSLL,S,1
NSEL,A,,,10000
NPLO
ET,2,184
KEYOP,2,1,1 !SET OPTION FOR BEAM BEHAVIOR, MPC184
TYPE,2
E,10000,58
*REPEAT,24,,1
ALLS
EPLO
DA,1,ALL !CONSTRAIN ONE END OF CYLINDER
F,10000,MZ,500 !APPLY A MOMENT TO THE 'MASTER' NODE
ALLS
/SOLU
NLGEOM,ON
NSUB,3,3,3
SOLV
/POST1
RSYS,1
PLNS,U,Y !PLOT TANGENTIAL DISPLACEMENT |
|