用ANSYS可以實現結構的滯回分析，這在地震反應分析等多個方面很有用處，下面是一個簡單的命令流，希望對大家有所啟發。

FINI
/CLEAR
/PREP7
!定義單元類型，實常數，材料特性
ET,1,SHELL143
R,1,12, , , , ,
MP,EX,1,210000
MP,NUXY,1,0.3
!雙線性隨動強化模型
TB,BKIN,1,1,2,1
TBDATA,,310,600,,,,
!定義關鍵點、線、面
K,1,54,0,0
K,2,-54,0,0
K,3,54,0,1000
K,4,-54,0,1000
A,1,2,4,3
!定義邊界荷強迫位移,劃分網格
AESIZE,ALL,27,
MSHAPE,0,2D
MSHKEY,0
CM,_Y,AREA
ASEL, , , , 1
CM,_Y1,AREA
CMSEL,S,_Y
AMESH,_Y1
*DO,I,1,5
D,I,ALL,0
*enddo

!指定求解結果的輸出項目
OUTPR,BASIC,ALL
OUTRES,ALL,ALL

!分為4個荷載步進行求解
!第1荷載步
D,46,ux,60
TIME,1
AUTOTS,0
NSUBST,10, , ,1
KBC,0
LSWRITE,01,
!第2荷載步
D,46,ux,-60
TIME,3
AUTOTS,0
NSUBST,20, , ,1
KBC,0
LSWRITE,02,
!第3荷載步
D,46,ux,60
TIME,5
AUTOTS,0
NSUBST,20, , ,1
KBC,0
LSWRITE,03,
!第4荷載步
D,46,ux,-60
TIME,7
AUTOTS,0
NSUBST,20, , ,1
KBC,0
LSWRITE,04,
!求解
FINISH
/SOLU
LSSOLVE,1,4,1,

!畫出荷載位移曲線
FINISH
/POST26
NSOL,2,46,U,X
RFORCE,3,46,F,X
XVAR,2
PLVAR,3