ANSYS在荷载步之间改变材料属性例子

ANSYS在荷载步之间改变材料属性例子

! Example of modify material between load steps in ANSYS

! 材料泊松比随荷载增加而逐步增大

! 作者：陆新征清华大学土木系

! Author: Lu Xinzheng Dept. Civil Engrg. of Tsinghua University

FINISH

/CLEAR

/PREP7

FORCE=1. !初始荷载

FC=30. !极限荷载

NSTEP=30 !加载步数

EMU0=0.2 !初始泊松比为0.2

EMUU=0.499 !最终泊松比为0.499

SVM=0. !VON MISES应力

!*

ET,1,SOLID45

!*

!*

MP,EX,1,30E3

MP,NUXY,1,EMU0

!建立模型

BLC4,0,0,100,100,100

ESIZE,100,0,

VMESH,ALL

/SOLU

!输出RESTART文件

RESCONTRL,DEFINE,ALL,-1,1

NLGEOM,1

D,2,ALL

D,4,UY

D,5,UY

D,6,UY

D,5,UX

FINISH

SAVE

!分步加载

*DO,I,1,NSTEP

FINISH

/SOLU

!使用重启动功能

*IF,I,GT,1,THEN

ANTYPE,,REST,

PARRES, CHANGE , PARAM, TXT,

*ENDIF

! 如果荷载超过强度的50%，则线性提高泊松比

*IF,SVM,GE,FC*0.5,THEN

MP,EX,1,30E3

MP,NUXY,1,EMU0+(EMUU-EMU0)*(SVM/FC-0.5)/0.5 *ENDIF

!得到下一步荷载

FORCE=FORCE+1

!加载

SFE,ALL,4,PRES, , FORCE, , ,

SOLVE

FINISH

/POST1

!得到VON MISES应力

*GET,SVM,ELEM,1,NMISC, 4

PARSAV, ALL, PARAM, TXT,

FINISH

*ENDDO