有限元分析课上机例题

有限元分析课上机例 习题1、由等直杆构成的平面桁架如图1所示，等直杆的截面积为25cm2，弹性模量为E=2.1e5 Mpa，泊松比为0.3，所受的集中力载荷为1.0e8N。分析该桁架受载后结构的构型，给出桁架各部分的纵向位移分布图。 图1 超静定桁架 1.1 进入ANSYS， 1.2定义工作文件名 文件名为truss 1.3选择单元类型 ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →选择Link 2D spar 1  →OK (back to Element Types window) 1.4定义材料参数 ANSYS Main Menu: Preprocessor →Material Props →Material Models →Structural →Linear →Elastic →Isotropic →input EX:2.1e11, PRXY:0.3 → OK 1.5定义实常数  ANSYS Main Menu: Preprocessor →Real Constants… →Add… →select Type 1→ OK→input AREA:0.0025 →OK →Close (the Real Constants Window) 1.6生成几何模型 ? 生成特征点 ANSYS Main Menu: Preprocessor →Modeling →Create →Keypoints →In Active CS →依次输入四个点的坐标：input:1(0,1),2(1,1),3(2,1),4(1,0) →OK ? 生成桁架 ANSYS Main Menu: Preprocessor →Modeling →Create →Lines →Lines →Straight Line →参照图1连接四个特征点，1(0,1),2(1,1),3(2,1),4(1,0) →OK 1.7 网格划分 ANSYS Main Menu: Preprocessor →Meshing →Size Controls→ManualSize→Global→Size， input NDIV: 1 →OK →(back to the mesh tool window)Mesh: lines → Pick All (in Picking Menu) →Close( the Mesh Tool window) 1.8 模型施加约束 ? 分别给1,2,3三个特征点施加x和y方向的约束 ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Displacement → On Keypoints →拾取1(0,1),2(1,1),3(2,1)三个特征点 →OK →select  Lab2:UX, UY（同时选） → OK ? 给4#特征点施加y方向载荷 ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Force/Moment →On Keypoints →拾取特征点4(1,0) →OK →Lab中选: FY, Value中输入: -100e6 →OK 1.9 分析计算 ANSYS Main Menu: Solution →Solve →Current LS →OK(to close the solve Current Load Step window) →OK 1.10 结果显示 ANSYS Main Menu: General Postproc →Plot Results →Deformed Shape… → select Def + Undeformed →OK (back to Plot Results window) →Contour Plot →Nodal Solu… →select: DOF solution, Y-component of displacement, →OK 1.11 退出系统  ANSYS Utility Menu: File → Exit → Save Everything→OK 习题2、一侧固定的方板如图2所示，长宽均为1m，厚度为5cm，方板的右侧受 到均布拉力 的作用。材料的弹性模量为 ，泊松比为0.3。求板的受力变形及X向和Y向位移分布图。 图2 矩形板示意图 2.1 进入ANSYS 2.2设置名称 2.3选择单元类型 ANSYS Main Menu: Preprocessor →Element Type→Add/Edit/Delete →Add →select Solid Quad 8node 82  →OK (back to Element Types window) 2.4定义材料参数 ANSYS Main Menu: Preprocessor →Material Props →Material Models →Structural →Linear →Elastic →Isotropic →input EX:2.1e11, PRXY:0.3 → OK 2.6生成几何模型 ? 生成特征点 ANSYS Main Menu: Preprocessor →Modeling →Create →Keypoints →In Active CS →依次输入五个点的坐标：input:1(0,0),2(1,0), 3(1,1),4(0,1) →OK ? 生成平板 ANSYS Main Menu: Preprocessor →Modeling →Create →Areas →Arbitrary →Through KPS →连接特征点1－4 →OK    2.7 网格划分 ANSYS Main Menu: Preprocessor →Meshing →Size Controls→ManualSize→Global→Size， input     SIZE: 0.1 →OK →(back to the mesh tool window)Mesh: Areas → Free → Pick All (in Picking Menu) →Close( the Mesh Tool window) 2.8 模型施加约束 ? 给模型施加x方向约束 ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Displacement → On Lines →拾取模型左部的竖直边：Lab2: UX UY →OK ? 施加x方向载荷 ? ANSYS Main Menu: Solution →Define Loads →Apply →Structural →Pressure →On Lines →拾取模型右部的竖直边→Load PRES value:-200e6施加 2.9 分析计算 ANSYS Main Menu: Solution →Solve →Current LS →OK(to close the solve Current Load Step window) →OK 2.10 结果显示 ANSYS Main Menu: General Postproc →Plot Results →Deformed Shape… → select Def + Undeformed →OK (back to Plot Results window) →Contour Plot →Nodal Solu →select: DOF solution, UX,UY, Def + Undeformed →OK 2.11 退出系统  ANSYS Utility Menu: File→ Exit →Save Everything→OK