ex4.8.inp

ansys有限元分析程序

! 4.8  用实体单元分析变截面杆的拉伸
! 本程序来源于邢静忠编著的《ANSYS应用实例与分析》，科学出版社，2006年
!
FINISH
/CLEAR, NOSTART
! (1)设置工程选项, 定义分析类型、单元类型和材料参数
/FILNAME, EX4.8
/PREP7
SMRT, OFF
/TITLE, EX4.8, ELONGATION OF A SOLID BAR WITH VARIED SECTION.
ANTYPE, STATIC
ET, 1, SOLID45
MP, EX, 1, 70.71E3
MP, NUXY, 1, 0.3
! (2)定义固定端4个点和自由端4个点，过这8个点定义体，对体剖分单元
/VIEW, 1, 1, 1, 1
K, 1, 25.4, , 25.4
K, 2, -25.4, , 25.4
K, 3, -25.4, , -25.4
K, 4, 25.4, , -25.4
K, 5, 12.7, 254, 12.7
K, 6, -12.7, 254, 12.7
K, 7, -12.7, 254, -12.7
K, 8, 12.7, 254, -12.7
V, 1, 2, 3, 4, 5, 6, 7, 8
LSEL, S, LINE, , 5, 11, 2
LESIZE, ALL, , , 7
LSEL, ALL
ESIZE, , 1
/OUT, SCRATCH
VMESH, 1
/OUT
! (3)施加位移约束和荷载
OUTPR, BASIC, ALL
NSEL, S, LOC, Y, 0
D, ALL, ALL
NSEL, ALL
NSEL, S, LOC, Y, 254
SF, , PRES, -68.949
NSEL, ALL
FINISH
! (4)在求解模块，开始静力分析的求解
/SOLU
SOLVE
FINISH
! (5)在后处理模块中，显示Y方向应力云图
/POST1
ETABLE, SIGY, S, Y
/VIEW, 1, 1
/VUP, 1, -Y
NSLE, S
PLNSOL, S, Y
ESEL, S, ELEM, , 4
PRETAB, SIGY
PRNSOL, S, COMP
ESEL, ALL
NSEL, S, LOC, Y, 254
PRNSOL, DOF
NSEL, ALL
! (6)选择指定位置的节点和单元，并提取它们的位移和应力
/NOPR
MID_NODE = NODE(0, 128, 0)
MID_ELM = ENEARN(MID_NODE)
BOT_NODE = NODE (0, 254, 0)
*GET, DEF, NODE, BOT_NODE, U, Y
*GET, STRSS, ELEM, MID_ELM, ETAB, SIGY
*STATUS, PARM
FINISH