动载荷作用下的结构动力响应分析

在动载荷作用下的结构动力响应分析一、问题的突出1.求钢结构的动力学响应2.结构及载荷数据立柱间距长180，宽120；顶距地面180E=200GPa,v=0.3,p=7800kg/m3A=100kg,w=20π二、有限单元模型建立1.单元类型选择以及截面性质定义FINISH/CLE/PREP7ET,1,BEAM188mp,ex,1,200e9mp,nuxy,1,0.3mp,dens,1,7800!截面1sectype,1,beam,Isecoffset,centsecdata,0.12,0.12,0.1212,0.00605,0.00605,0.0039!截面2sectype,2,beam,Isecoffset,centsecdata,0.06535,0.06535,0.0805,0.00465,0.00465,0.00285!截面3sectype,3,beam,HRECsecoffset,centsecdata,0.06,0.06,0.0025,0.0025,0.0025,0.00252.模型建立选择Y方向为立柱方向，通过由下向上建模即由关键点到线。k,1,k,2,1.8k,3,1.8,,1.2k,4,,,1.2k,5,,1.5k,6,1.8,1.5k,7,1.8,1.5,1.2k,8,,1.5,1.2l,1,5l,2,6l,3,7l,4,8k,9,1.8/2,1.8,1.2/2l,9,5l,9,6l,9,7l,9,8l,5,8l,8,7l,7,6l,6,53.对于不同的杆赋予不同的截面性质，并进行网格划分lsel,s,,,1,4,1lplotlesize,all,0.04secnum,1lmesh,alllsel,s,,,9,12lplotlesize,all,0.04secnum,2lmesh,alllsel,s,,,5,8,1lplotlesize,all,0.04secnum,3lmesh,all4.约束设置选择Y=0位置的关键点，将四个角全部约束。allsel,all,allksel,s,loc,y,0dk,all,allallsel,all,all5.进入瞬态分析选项，设置时间载荷步和输出相关选项。/soluantype,4outres,all,allTRNOPT,FULLTIME,0.4DELTIM,0.01,0.001,0.056.定义加载函数funtion。（1）在ansys主菜单选Parameters-Funtion-Define/Edit进入函数编辑器，输入加载的函数如图所示。然后保存函数。（2）选择图中的GRAPH可以对加载函数进行绘制。注意选择X的范围和描绘的点数，否则得到的函数图形不合理,X的范围应该在一两个周期范围内，不然画出的图形的周期是周期的N倍。载荷函数周期为:T=2π/W=2π/20π=0.1图中可以看出载荷函数的周期也为0.17.加载（选择函数加载）（1）首先读入载荷的函数文件在ansys主菜单选Parameters-Funtion-Readfromfile中选择定义的载荷函数文件，并取名字为LOAD。（2）选择顶点进行函数加载。fk,9,fy,%load%(3)求解solve三、时间后处理器查看结果顶点Y方向的位移时间图形/POST26ksel,s,,,9nslk,SNSOL,2,304,U,Y,UY_2,XVAR,1PLVAR,2结论：图中可以看出顶点Y方向位移响应的周期T=0.1s,而外载荷的周期也为T=2π/W=0.1.在正弦周期载荷的作用下，结构的响应频率和外载荷的频率是一致的。