机翼模型的振动模态分析

机设1305 彭鹏程1310140521

一个简化的飞机机翼模型如图所示，该机翼沿延翼方向为等厚度。有关的几何尺寸见下图，机翼材料的常数为：弹性模量E=0.26GPa，泊松比m=0.3，密度r =886 kg/m。对该结构进行振动模态的分析。

(a) 飞机机翼模型 (b) 翼形的几何坐标点

振动模态分析计算模型示意图

解答这里体单元SOLID45 进行建模，并计算机翼模型的振动模态。

建模的要点：

⑴首先根据机翼横截面的关键点，采用连接直线以及样条函数< BSPLIN >进行连接以形成一个由封闭线围成的面；

⑵在生成的面上采用自由网格划分生成面单元(PLANE42)；

⑶设置体单元SOLID45，采用< VEXT>进行Z 方向的多段扩展；

⑷设置模态分析< ANTYPE,2>，采用Lanczos 方法进行求解<

MODOPT,LANB >；

⑸在后处理中，通过调出相关阶次的模态；

⑹显示变形后的结构图并进行动态演示。

给出的基于图形界面的交互式操作(step by step)过程如下。

(1) 进入ANSYS(设定工作目录和工作文件)

程序→ANSYS →→ANSYS Interactive →Working directory ( 设置工作目录) →Initial jobname(设置工作文件名)：Modal→Run

(2) 设置计算类型

ANSYS Main Menu：Preferences…→Structural →OK

(3) 选择单元类型

ANSYS Main Menu：Preprocessor →Element Type →Add/Edit/Delete →Add…→Structural solid：Quad 4node 42 →Apply →solid →Brick 8node 45→OK →Close

(4) 定义材料参数

ANSYS Main Menu：Preprocessor →Material Props →Material Models →Structural →Linear →Elastic →Isotropic:EX:0.26E9(弹性模量),PRXY:0.3(泊

松比) →OK →Density:886 →OK →Material →Exit

(5) 生成几何模型

ANSYS Main Menu：Preprocessor →Modeling →Create →Keypoints →In Active CS →X,Y,Z location:0,0,0→Apply →X,Y,Z location:0.05,0,0→Apply →X,Y,Z location:0.0575,0.005,0 →

Apply →X,Y,Z location:0.0475,0.0125,0 →Apply →X,Y,Z

location:0.025,0.00625,0 →OK

ANSYS Main Menu：Preprocessor →Modeling →Create →Lines →Lines →Straight Line →依次选择关键点1, 2, 5, 1 →OK

ANSYS Main Menu：Preprocessor →Modeling →Create →Lines →Splines →With Options →Spline thru KPs →依次选择关键点2, 3, 4, 5 →OK →输入以下数据:XV1:-0.025,YV1:0,ZV1:0 →输入以下数据:XV6:-0.025,

YV6:-0.00625, ZV6:0 →OK

ANSYS Main Menu：Preprocessor →Modeling →Create →Areas →Arbitrary →By Lines →选择所有3 条线→OK

(6) 网格划分

ANSYS Main Menu：Preprocessor →Meshing →Mesh Tool →global →Set →Element edge length:0.00625 →OK →Mesh →Pick All →Close →Close(点击关闭Mesh Tool 工具栏)

ANSYS Main Menu：Preprocessor →Modeling →Operate →Extrude →Elem Ext Opts →Element type number:2 SOLID45 →The No. of element

divisions:10 →OK

ANSYS Main Menu：Preprocessor →Modeling →Operate →Extrude →Areas →By XYZ Offset →Pick All →Offsets for extrusion in the Z direction:0,0,0.25 →OK →Close

(7) 模型施加载荷

ANSYS Utility Menu：Select →Entities →Elements →By Attributes →Elem type num →The element type number:1→Unselect →Apply

(8) 模型施加约束

ANSYS Utility Menu：Select →Entities →Nodes →By Location →Z coordinates →T he Z coordinate location:0→From Full →Apply

ANSYS Main Menu →Preprocessor →Loads →Define Loads →Apply →Structural →Displacement →On Nodes →Pick All →All DOF →OK →By Num/Pick →Select All →点击Cancel(关闭窗口)