[转帖]ANSYS在荷载步之间改变材料属性例子

AaronSpark

<P>! ANSYS在荷载步之间改变材料属性例子<BR>! 材料泊松比随荷载增加而逐步增大<BR>FINISH<BR>/CLEAR<BR>/PREP7 <BR>FORCE=1. !初始荷载<BR>FC=30. !极限荷载<BR>NSTEP=30 !加载步数<BR>EMU0=0.2 !初始泊松比为0.2<BR>EMUU=0.499 !最终泊松比为0.499<BR>SVM=0. !VON MISES应力<BR>!* <BR>ET,1,SOLID45<BR>!* <BR>!* <BR>MP,EX,1,30E3 <BR>MP,NUXY,1,EMU0<BR>!建立模型<BR>BLC4,0,0,100,100,100<BR>ESIZE,100,0,<BR>VMESH,ALL <BR>/SOLU<BR>!输出RESTART文件<BR>RESCONTRL,DEFINE,ALL,-1,1 <BR>NLGEOM,1<BR>D,2,ALL <BR>D,4,UY <BR>D,5,UY <BR>D,6,UY <BR>D,5,UX<BR>FINISH<BR>SAVE<BR>!分步加载<BR>*DO,I,1,NSTEP<BR>FINISH <BR>/SOLU <BR>!使用重启动功能<BR>*IF,I,GT,1,THEN<BR>ANTYPE,,REST,<BR>PARRES, CHANGE , PARAM, TXT,<BR>*ENDIF<BR>! 如果荷载超过强度的50%，则线性提高泊松比<BR>*IF,SVM,GE,FC*0.5,THEN<BR>MP,EX,1,30E3 <BR>MP,NUXY,1,EMU0+(EMUU-EMU0)*(SVM/FC-0.5)/0.5<BR>*ENDIF<BR>!得到下一步荷载<BR>FORCE=FORCE+1<BR>!加载<BR>SFE,ALL,4,PRES, , FORCE, , , <BR>SOLVE <BR>FINISH <BR>/POST1 <BR>!得到VON MISES应力<BR>*GET,SVM,ELEM,1,NMISC, 4 <BR>PARSAV, ALL, PARAM, TXT,<BR>FINISH <BR>*ENDDO</P>