ANSYS动力学分析的几个入门例子.doc

问题一：悬臂梁受重力作用发生大变形，求其固有频率。 基本过程： 1、建模 2、静力分析 NLGEOM,ON STRES,ON 3、求静力解 4、开始新的求解：modal STRES,ON UPCOORD,1,ON修正坐标 SOLVE. 5、扩展模态解 6、察看结果 /PREP7 ET,1,BEAM189 !使用beam189梁单元 MPTEMP, MPTEMP,1,0 MPDATA,EX,1,210e9 MPDATA,PRXY,1,0.3 MPDATA,DENS,1,7850SECTYPE, 1, BEAM, RECT, secA, 0 !定义梁截面secA SECOFFSET, CENTSECDATA,0.005,0.01,0,0,0,0,0,0,0,0 K, , !建模与分网 K, ,2, K, ,2,1, LSTR, 1, 2 LATT,1, ,1, , 3, ,1 LESIZE,1, , ,20, , , , ,1LMESH, 1 FINISH /SOL !静力大变形求解 ANTYPE,0 NLGEOM,1 PSTRES,ON !计及预应力效果 DK,1, , , ,0,ALL, , , , , , ACEL,0,9.8,0, !只考虑重力作用 TIME,1 AUTOTS,1 NSUBST,20, , ,1KBC,0 SOLVE FINISH /SOLUTION ANTYPE,2 !进行模态求解 MSAVE,0MODOPT,LANB,10 MXPAND,10, , ,0 !取前十阶模态 PSTRES,1 !打开预应力效应 MODOPT,LANB,10,0,0, ,OFF UPCOORD,1,ON !修正坐标以得到正确的应力 PSOLVE,TRIANG !三角化矩阵 PSOLVE,EIGLANB !提取特征值和特征向量 FINISH /SOLU EXPASS,1 !扩展模态解 PSOLVE,EIGEXP FINISH /POST1 SET,LIST !观察结果 FINISH 问题二：循环对称结构模态分析 这是ANSYS HELP里的例子，但那个命令流似乎有些问题，下面是整理过的命令流。 基本过程： 1、建模 2、define cyclic 3、定义约束 4、求模态解 5、展开并察看结果 r1=5 !建模 r2=10 d1=2 nsect=24 alpha_deg=360/nsect alpha_rad=2*acos(-1)/nsect /prep7 csys,1 k,1,0,0,0 k,2,0,0,d1 k,3,r1,0,0 k,4,r1,0,d1 l,3,4 arotat,1,1,2,alpha_deg/2 k,7,r2,0,0 k,8,r2,0,d1 l,7,8 arotat,5,1,2,alpha_deg/2 arotat,2,1,2,alpha_deg/2 arotat,6,1,2,alpha_deg/2 a,5,6,10,9 mshkey,1 et,1,181 r,1,0.20 r,2,0.1 mp,ex,1,10e6 mp,prxy,1,0.3 mp,dens,1,1e-4 esize,0.5 asel,1,4 aatt,1 asel,5 aatt,2 allsel CYCLIC, , , ,CYCLIC !定义基本扇区 AMESH,all !分网 FINISH /SOL !求模态解 ANTYPE,2 MODOPT,LANB,10 MXPAND,10, , ,0PSTRES,0 MODOPT,LANB,10,0,0, ,OFF DK,5, , , ,0,UZ, , , , , , SOLVE FINISH/POST1 SET,LIST SET, , ,1, , , ,4, /CYCEXPAND, ,ONPLNS,U,SUM !观察扩展模态 FINISH 问题三：三角平台受谐波载荷作用,求结构响应 谐波载荷为作用在平台上面一点的集中力，幅值为10N，频率范围5Hz70Hz 基本过程： 1、建模 2. 求模态解 3、用模态叠加法作谐分析 4. 观察结果 /PREP7 !建模 ET,1,BEAM189 ET,2,SHELL93 R,1,0.01, , , , , ,MP,EX,1,210e9 MP,PRXY,1,0.3 MP,DENS,1,7850 SECTYPE, 1, BEAM, RECT, secA, 0 SECOFFSET, CENTSECDATA,0.005,0.008,0,0,0,0,0,0,0,0K, ,-0.5,K, ,0.5, K, ,1, K, ,1,1, K, ,-0.5,1, K, ,0.5,1,K, ,0.5, A,4,5,6LSTR, 1, 5 LSTR, 3, 4 LSTR, 2, 6 LSEL,S,LINE,4,6 LATT,1,1,1, , 7, ,1 LSEL, , , ,ALL LESIZE,ALL, , ,10, , , , ,1LMESH,4,6 TYPE, 2 MSHAPE,0,2DMSHKEY,1 AMESH,1FINISH /SOL !为了使用模态叠加法谐分析 ANTYPE,2 MODOPT,LANB,20 !先取结构前20阶模态MXPAND,20, , ,0MODOPT,LANB,20,0,0, ,OFF KSEL,S,KP,1,3DK,ALL, , , ,0,ALL, , , , , , SOLVE FINISH!/POST1 !最好事先看一下模态结果 !SET,LIST !以了解模态频率范围 !FINISH /SOL !模态叠加法谐响应分析 ANTYPE,3 HROPT,MSUP HROUT,ON HROPT,MSUP,20, , HROUT,ON,OFF,0 F,177,FY,-10, !施加10N的力在节点177的负Y方向 HARFRQ,5,70, !载荷的强制频率范围 NSUBST,200,KBC,1 ALPHAD,5, SOLVE FINISH /POST26 !察看位移响应 FILE,rfrq NUMVAR,20NSOL,2,139,U,Y,PLVAR,2 FINISH 问题四：三角平台受一地震谱激励,求应力分布和支反力 基本过程： 1、建模 2、求模态解 3、求谱解 4、扩展模态 5、模态合并 6、观察结果 /PREP7 !建模 ET,1,BEAM189 ET,2,SHELL93 R,1,0.01, , , , , ,MP,EX,1,210e9 MP,PRXY,1,0.3 MP,DENS,1,7850SECTYPE, 1, BEAM, RECT, secA, 0 SECOFFSET, CENTSECDATA,0.005,0.008,0,0,0,0,0,0,0,0 K, ,-0.5,K, ,0.5, K, ,1, K, ,1,1, K, ,-0.5,1, K, ,0.5,1,K, ,0.5, A,4,5,6LSTR, 1, 5 LSTR, 3, 4 LSTR, 2, 6 LSEL,S,LINE,4,6LATT,1,1,1, , 7, ,1 LSEL, , , ,ALL LESIZE,ALL, , ,10, , , , ,1LMESH,4,6 TYPE, 2 MSHAPE,0,2DMSHKEY,1 AMESH,1FINISH /SOL !取前十阶模态 ANTYPE,2 MODOPT,LANB,10 KSEL,S,KP,1,3DK,ALL, , , ,0,ALL, , , , , , SOLVE FINISH /SOL !谱分析 ANTYPE,8 SPOPT,SPRS,10,1 SVTYP,3 SED,0,1,0, !给出激励方向 FREQ,0.25,1.34,6.73,14.6,28.9,0,0,0,0 !激励谱 SV,0,0.00073,0.00016,0.00034,0.00034,0.00052, SOLVE FINISH /SOL !扩展模态 ANTYPE,2 EXPASS,1 MXPAND,10,0,0,1,0.001, SOLVE FINISH /SOL !模态合并 ANTYPE,8 SRSS,0.001,DISPSOLVE /POST1 !观察结果 SET,LIST/INPUT,mcom PRRSOL,F FINISH 问题五：三角平台受时程载荷作用,求应力分布和变形过程 基本过程： 1、建模 2. 施加随时间变化载荷，定义载荷步 3、求解 4. 在POST1和POST26中观察结果 /PREP7 !建模 ET,1,BEAM189 ET,2,SHELL93R,1,0.01, , , , , ,MP,EX,1,210e9 MP,PRXY,1,0.3 MP,DENS,1,7850 SECTYPE, 1, BEAM, RECT, secA, 0 SECOFFSET, CENTSECDATA,0.005,0.008,0,0,0,0,0,0,0,0K, ,-0.5,K, ,0.5, K, ,1, K, ,1,1, K, ,-0.5,1, K, ,0.5,1,K, ,0.5, A,4,5,6LSTR, 1, 5 LSTR, 3, 4 LSTR, 2, 6 LSEL,S,LINE,4,6 LATT,1,1,1, , 7, ,1 LSEL, , , ,ALL LESIZE,ALL, , ,10, , , , ,1LMESH,4,6 TYPE, 2 MSHAPE,0,2DMSHKEY,1 AMESH,1FINISH /SOL ANTYPE,4 TRNOPT,FULL !完全法瞬态分析 KSEL,S,KP,1,3 DK,ALL, , , ,0,ALL, , , , , , OUTRES,ALL,1 ALPHAD,5, !阻尼 TIME,2 !定义载荷曲线 AUTOTS,1 NSUBST,5