ansys命令流

（1）创建物理环境
/COM, Structural ! 指定结构分析
/TITLE,Tunnel Support Structural Analysis ! 定义工作标题
/FILNAM,support,1 ! 定义工作文件名

！进入前处理器
/PREP7
！定义单元
ET,1,BEAM3
ET,2,COMBIN14
! 定义材料属性
MP,EX,1,3E10
MP,PRXY,1,0.2
MP,DENS,1,2500
! 定义实常数
R,1,0.65,0.65*0.65*0.65/12,0.65,
R,2,0.85,0.85*0.85*0.85/12,0.85,0,0,0,
R,3,300000000, , ,
（2）建立几何模型
! 创建隧道衬砌支护关键点
K,1,,,,
K,2,,3.85,,
K,3,.88,5.5,,
K,4,2.45,6.15,,
K,5,4.02,5.5,,
K,6,4.9,3.85,,
K,7,4.9,0,,
! 创建隧道衬砌支护线
LARC,1,2,6,8.13,
LARC,2,3,6,3.21,
LARC,3,4,6,2.22,
LARC,4,5,2,2.22,
LARC,5,6,2,3.21,
LARC,6,7,2,8.13,
LARC,7,1,4,6,
！保存几何模型
SAVE,'Support-geom','db','D:\ansys\example301\'
（3）划分网格，生成隧道衬砌支护单元
lsel,s,line,,1,6,1
LATT,1,1,1, , , ,
LSEL,s, , ,7
LATT,1,2,1, , , ,
lsel,s,line,,1,6,5
LESIZE,all,,,4,
lsel,s,line,,2,5,1
LESIZE,all,,,2,
lsel,s,line,,7
LESIZE,all,,,8,
lsel,all
Lmesh,all ！线网格划分，生成支护单元
（4）添加弹簧单元
/PNUM,NODE,1 ！打开节点号开关
！生成24根弹簧单元
PSPRNG,1,TRAN,300000000,-0.97029572,-0.241921895,
PSPRNG,2,TRAN,300000000,-0.97437006,0.22495105,
PSPRNG,3,TRAN,300000000,-0.98628560,-0.1604761,
PSPRNG,4,TRAN,300000000,-0.99919612,-0.00872654,
PSPRNG,5,TRAN,300000000,-0.98901586,0.14780941,
PSPRNG,6,TRAN,300000000,-0.70710678,0.70710678,
PSPRNG,7,TRAN,300000000,-0.88294757,0.469471561,
PSPRNG,10,TRAN,300000000,0.70710678,0.70710678,
PSPRNG,13,TRAN,300000000,0.88294757,0.469471561,
PSPRNG,12,TRAN,300000000,0.97437006,0.22495105,
PSPRNG,15,TRAN,300000000,0.98901586,0.14780941,
PSPRNG,16,TRAN,300000000,0.99996192,-0.00872654,
PSPRNG,17,TRAN,300000000,0.98628560,-0.1604768,
PSPRNG,14,TRAN,300000000,0.97029572,-0.241921895,
PSPRNG,18,TRAN,300000000,0.30901699,-0.95105651,
PSPRNG,19,TRAN,300000000,0.20791169,-0.9781476,
PSPRNG,20,TRAN,300000000,0.10452846,-0.99452189,
PSPRNG,21,TRAN,300000000,0,-1,
PSPRNG,22,TRAN,300000000,-0.10452846,-0.99452189,
PSPRNG,23,TRAN,300000000,-0.20791169,-0.9781476,
PSPRNG,24,TRAN,300000000,-0.30901699,-0.95105651,
（5）保存模型
alls
SAVE
FINISH
（6）施加约束和荷载
/SOL
NSEL,S,NODE,,25,45,1
d,all,uy,0
d,all,ux,0
！施加重力加速度
allsel
ACEL,acely,

0,9.8,0,
！施加围岩压力
allsel
NSEL,S,NODE,,1,17,1
F,all,FY,-80225 ！施加节点1到节点17上的垂直匀布力
NSEL,S,NODE,,18,24,1
F,all,FY,80225 ！施加节点18到节点24上的水平匀布力
NSEL,S,NODE,,1,9,1
NSEL,a,NODE,,22,24,1
F,all,FX,16045
NSEL,S,NODE,,10,21,1
F,all,FX,-16045
！给隧道仰拱施加水压
NSEL,S,NODE,,18
F,all,FX,-161803 ！施加节点18的水平方向的水压分力
NSEL,S,NODE,,18
F,all,FY,70381 ！施加节点18的垂直方向的水压分力
NSEL,S,NODE,,19
F,all,FX,-182309
NSEL,S,NODE,,19
F,all,FY,50101
NSEL,S,NODE,,20
F,all,FX,-198904
NSEL,S,NODE,,20
F,all,FY,13093
NSEL,S,NODE,,21
F,all,FX,0
NSEL,S,NODE,,21
F,all,FY,125960
NSEL,S,NODE,,22
F,all,FX,198904
NSEL,S,NODE,,22
F,all,FY,13093
NSEL,S,NODE,,23
F,all,FX,182309
NSEL,S,NODE,,19
F,all,FY,50101
NSEL,S,NODE,,24
F,all,FX,161803
NSEL,S,NODE,,18
F,all,FY,70381
（7）求解分析修改模型
！进入求解器
allsel
solve ！进行求解
！进入后处理器
/POST1
PLDISP,1 ！绘制结构变形图
FINISH
！进入前处理器删除受拉弹簧单元
/PREP7
！删除受拉弹簧单元
EDELE,26 ！删除弹簧单元26
NDEL,26 ！删除节点26
EDELE,30
NDEL,30
EDELE,31
NDEL,31
EDELE,32
NDEL,32
EDELE,33
NDEL,33
EDELE,34
NDEL,34
！进行再次求解
allsel ！选择模型
solve ！进行求解
！保存求解结果
SAVE,'support result.db',
（8）绘制最终结构变形图
/POST1 ！进入后处理器
PLDISP,1 ！绘制最终结构变形图
（9）制节点弯矩、剪力、轴力表
ETABLE,IMOMENT,SMISC, 6 ！制结构弯矩表
ETABLE,JMOMENT,SMISC,12

ETABLE,ISHEAR,SMISC, 2 ！制结构剪力表
ETABLE,JSHEAR,SMISC, 8

ETABLE,ZHOULI-I,SMISC, 1 ！制结构轴力表
ETABLE,ZHOULI-J,SMISC, 7
（10）设置弯矩、剪力、轴力标题并绘制出分布图
/TITLE,BENDING MOMENT distribution ！定义弯矩分布标题
PLLS,IMOMENT,JMOMENT,-0.8,1 ！绘制结构弯矩分布图

/TITLE,SHEAR force distribution ！定义剪力分布标题
PLLS,ISHEAR,JSHEAR,1,1 ！绘制剪力分布图

/TITLE,ZHOULI force distribution ！定义轴力分布标题
PLLS,ZHOULI-I,ZHOULI-J,-0.6,1 ！绘制轴力分布图
（11）列出节点位移
PRNSOL,U,COMP

！显示所有节点总位移矢量
PRNSOL,ROT,COMP ！显示所有节点总旋转位移矢量
（12）列表显示结构的弯矩、剪力、轴力
PRETAB,IMOMENT,JMOMENT,ISHEAR,JSHEAR,ZHOULI-I,ZHOULI-J
（13）完成分析退出ANSYS
FINISH
/EXIT