1）启动 ANSYS Mechanical APDL
设置工作文件名：undeterm；或用其他工作文件名。
2）设置计算类型
Main Menu → Preferences →select Structural → OK
3）选择单元类型
Main Menu → Preprocessor →Element Type→Add/Edit/Delete →Add →select
Beam 2 node 188 →OK(back to Element Types window) →Close (the Element Type window)
4）定义材料参数
Main Menu → Preprocessor →Material Props →Material Models →Structural →
Linear →Elastic →Isotropic →input EX:2.1e11, PRXY:0.3 → OK
5）定义截面
Main Menu → Preprocessor →Sections →Beam →Common Sectns →定义矩形截面:
ID=1,B=0.01,H=0.1 →OK
6）生成几何模型
生成特征点
Main Menu → Preprocessor →Modeling →Create →Keypoints →In Active CS →依
次输入三个支点的坐标，并输入方向控制特征点的坐标：input:1(0,0),2(1,0),3(2,0),4(0,1) →
OK
生成梁
Main Menu → Preprocessor →Modeling →Create →Lines →lines →Straight lines
→依次连接三个特征点，1(0,0), 2(1,0),3(2,0) →OK
显示梁体
Utility Menu → PlotCtrls >Style >Size and Style →/ESHAPE →On →OK
7）网格划分
Main Menu → Preprocessor →Meshing →Mesh Attributes →Picked lines →OK →
拾取: SECT:1；Pick Orientation Keypoint(s):YES→拾取：4#特征点(0,1) →OK→Mesh Tool → (Size Controls) lines: Set →Pick All(in Picking Menu) →input NDIV:8 →OK (back to Mesh
Tool window) → Mesh →Pick All (in Picking Menu) → Close (the Mesh Tool window)
定义截面方向控制点的详细介绍在 5.1 节中。
8）模型施加约束
分别给 1,2,3 三个特征点加约束
Main Menu → Solution →Define Loads →Apply →Structural →Displacement →
On Keypoints →拾取 1,2,3 keypoints →OK→select All DOF →OK
施加 y 方向的载荷
Main Menu → Solution →Define Loads →Apply →Structural →Pressure → On
Beams →Pick All →LKEY:2,VALI:100000 (均布载荷只需在第 1 个编辑框输入参数) →OK
9）分析计算
Main Menu → Solution →Solve →Current LS →OK(to close the solve Current Load
Step window) →OK
10）结果显示
用云图（fringe）方式显示变形：
Main Menu → General Postproc →Plot Results →Deformed Shape… → select Def
+ Undeformed →OK (back to Plot Results window)
用云图方式显示结点位移、结点转角
Main Menu → General Postproc →Plot Results →Contour Plot →Nodal Solu →select:
DOF solution, UY, Def + Undeformed , Rotation, ROTZ ,Def + Undeformed→OK
列出支反力的计算结果：
Utility Menu → List → Results → Reaction solution
列出支反力的下拉菜单项“Reaction Solution”如图 5.9 所示，选择“Reaction Solution”菜
单项后弹出“List Reaction Solution”对话窗口，如图 5.10 所示。在“List Reaction Solution”
对话窗口中的“Item to be listed”下拉框中选择“All items”，列出全部支反力的计算结果。
