你提供的资料，除了模型尺寸、位移约束和个别数据外，没有给出其它的原始数据，如材料属性、网格尺寸、接触对的属性设置、求解设置等，都只是说明有相应的步骤，但没有或很少提供具体操作参数。
参考该资料，我自己添加了所有缺少的数据，做了计算，结果和该资料是类似的。因此，应该是你的操作给出与该资料有某些不一样的地方，需要你自己找出来。
而且，由于该资料中，上面的小面只是水平移动有限的距离，下面的大面i实际上是固定的，因此即使计算有问题，模型也不会飞掉。
下面是我的操作命令流，你可以试试，再和自己的操作对照一下：
fini
/clear
/filn, re_moca, 1
!*
WPSTYLE,,,,,,,,0
!* 设置分析科目为热+结构
/PMETH,OFF,0
KEYW,PR_SET,1
KEYW,PR_STRUC,1
KEYW,PR_THERM,1
KEYW,PR_MULTI,1
!*
!*
/PREP7
!* 定义单元类型
ET,1,PLANE13
!*
KEYOPT,1,1,4
KEYOPT,1,2,0
KEYOPT,1,3,0
KEYOPT,1,4,0
KEYOPT,1,5,0
!* 定义材料属性
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,201000
MPDATA,PRXY,1,,0.3
MPDATA,DENS,1,,7.8e-9
UIMP,1,REFT,,,
MPDATA,ALPX,1,,1.5e-5
MPDATA,MU,1,,0.2
MPDATA,KXX,1,,150
MPDATA,C,1,,80e6
!* 创建两个矩形
RECTNG,0,20,0,5,
RECTNG,0,5,5,10,
!*
TYPE, 1
MAT, 1
REAL,
ESYS, 0
SECNUM,
!* 网格尺寸
ESIZE,0.5,0,
!* 划分网格
MSHKEY,1
AMESH,all
MSHKEY,0
!*
!* 以下使用接触向导定义接触
! /COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_KPCM,KP
CM,_LINECM,LINE
CM,_AREACM,AREA
CM,_VOLUCM,VOLU
! /GSAV,cwz,gsav,,temp
MP,MU,1,0.2
MAT,1
MP,EMIS,1,1
R,3
REAL,3
ET,3,169
ET,4,172
R,3,,,1.0,0.1,0,
RMORE,,,1.0E20,0.0,1.0,
RMORE,0.0,150,1.0,5.67e-8,1.0,0.5
RMORE,0,1.0,1.0,0.0,,1.0
KEYOPT,4,3,0
KEYOPT,4,4,0
KEYOPT,4,5,3
KEYOPT,4,7,0
KEYOPT,4,8,0
KEYOPT,4,9,0
KEYOPT,4,10,2
KEYOPT,4,11,0
KEYOPT,4,12,2
KEYOPT,4,2,0
KEYOPT,4,1,1
! Generate the target surface
LSEL,S,,,3
CM,_TARGET,LINE
TYPE,3
NSLL,S,1
ESLN,S,0
ESURF
CMSEL,S,_ELEMCM
! Generate the contact surface
LSEL,S,,,5
CM,_CONTACT,LINE
TYPE,4
NSLL,S,1
ESLN,S,0
ESURF
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,3
ESEL,A,TYPE,,4
ESEL,R,REAL,,3
! /PSYMB,ESYS,1
! /PNUM,TYPE,1
! /NUM,1
! EPLOT
ESEL,ALL
ESEL,S,TYPE,,3
ESEL,A,TYPE,,4
ESEL,R,REAL,,3
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_KPCM
CMDEL,_KPCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
CMSEL,S,_VOLUCM
CMDEL,_VOLUCM
! /GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
! /COM, CONTACT PAIR CREATION - END
!*
ALLSEL,ALL
!*
EPLOT
SAVE
!*
FINISH
!*
/SOL
!* 瞬态分析
ANTYPE,4
!*
TRNOPT,FULL
LUMPM,0
!*
NLGEOM,1
SSTIF,0
NROPT,FULL, ,
TRNOPT,FULL
EQSLV, , ,0, ,DELE
!*
TOFFST,273,
!*
TUNIF,20,
!*
OUTPR,BASIC,ALL,
/GST,1
!*
SOLCONTROL,ON,0,NOPL
!*
TIMINT,0,STRUCT
TIMINT,1,THERM
TIMINT,1,MAG
TINTP,0.005, , , , , ,
!*
OUTRES,ERASE
OUTRES,NSOL,-10
OUTRES,RSOL,-10
OUTRES,ESOL,-10
OUTRES,FGRA,-10
AUTOTS,1
!* 计算终止时间 0.015
TIME,0.015
!*
!* 定义表数组 press，用于施加压力
*DIM,press,TABLE,2,1,1, , ,
PRESS(1,0) = 0
PRESS(2,0) = 10
PRESS(1,1) = 40
PRESS(2,1) = 40
!*
!* 上面小面沿 x 方向移动 15，相当于速度 100 /s
DA, 2,UX,15
!* 约束大面的四条边界线，相当于约束整个大面
FLST,2,4,4,ORDE,2
FITEM,2,1
FITEM,2,-4
DL,P51X, ,UX,
!*
FLST,2,4,4,ORDE,2
FITEM,2,1
FITEM,2,-4
DL,P51X, ,UY,
!* 在小面的上边界施加压力
SFL, 7,PRES, %PRESS%
!* 设置求解时的子步数
NSUBST,30,1000,30
!*
SAVE
! /STATUS,SOLU
SOLVE
!*
save
FINISH
!*
/POST1
!*
SET,LAST
!* 绘制节点温度云图
/EFACET,1
PLNSOL, TEMP,, 0,1.0
/wait, 3
!* 绘制 mises 应力温度云图
/EFACET,1
PLNSOL, S,EQV, 0,1.0
/wait, 3
!*
fini
!* |
回复此楼
