abaqus带孔平板的有限元分析

有限元软件ABAQUS学习资料

实例1：带孔平板的有限元分析

=100N/mm2 2 =0.3

图1 平面问题的计算分析模型

1.

2. 进入ABAQUS/CAE 开始 程序 ABAQUS 6.xx ABAQUS CAE 新建Model Database

Start Session窗口: Create Model Database

3. 创建几何模型 (Context Bar: Module Part)

Toolbox Area: click New Part Create Part Window: input Name: Plate; select Modeling Space: 2D Planar, Type: Deformable, Base Feature: Shell; input Approximate size: 200; click Continue…

Toolbox Area: click Create Lines: Rectangle (4 Lines) Prompt Area: input -50, 50 enter Prompt Area: input 50,-50 enter Toolbar: click Auto-Fit View

Toolbox Area: click Create Circle: Center and Perimeter Prompt Area: input 0,0 enter Prompt Area: input 5,0 enter center click center click

4. 设置材料属性 (Context Bar: Module Property)

Toolbox Area: click Create Material Edit Material Window: input Name: steel; select Mechanical > Elasticity > Elastic; input Young’s Modulus: 210000, Poisson’s Ratio: 0.3; click OK

Toolbox Area: click Create Section Create Section Window: input Name: SectionPlate; select Category: Solid, Type: Homogeneous; click Continue… Edit Section: click OK Toolbox Area: click Assign Section Viewport: click anywhere of the part Prompt Area: click Done Assign Section Window: click OK

5. 组装零件 (Context Bar: Module Assemble)

Toolbox Area: click Instance Part Create Instance Window: select Parts: plate; click OK

6. 定义加载步 (Context Bar: Module Step)

有限元软件ABAQUS学习资料

Toolbox Area: click Create Step Create Step window: input Name: Tension; select Procedure type: General > Static, General; click Continue… Edit Step Window: click OK

7. 定义载荷与边界条件 (Context Bar: Module Load)

Toolbox Area: click Create Load Create Load Window: input Name: pressure; select Step: Tension, Category: Mechanical, Types for Selected Step: Pressure; click Continue… Viewport: click the right edge of the plate Prompt Area: click Done Edit Load Window: input Magnitude: -100; click OK

Toolbox Area: click Create Boundary Condition Create Boundary Condition Window: input Name: Fix Left Bottom Corner; select Step: Initial, Category: Mechanical, Types for Selected Step: Symmetry/Antisymmetry/Encastre; click Continue... Viewport: click the left bottom corner of the plate Prompt Area: click Done Edit Boundary Condition Window: select ENCASTRE(U1=U2=U3=UR1=UR2=UR3=0); click OK

Toolbox Area: click Create Boundary Condition Create Boundary Condition Window: input Name: Fix Left Edge Horizontally; select Step: Initial, Category: Mechanical, Types for Selected Step: Displacement/Rotation; click Continue… Viewport: click the left edge of the plate Prompt Area: click Done Edit Boundary Condition Window: set U1: ON, U2: OFF, UR3: OFF; click OK

8. 划分网格 (Context Bar: Module Mesh)

Menu Bar: select Seed > Edge by Number Viewport: select the inner circle Prompt Area: click Done Prompt Area: input 16 enter Viewport: shift select the outer four edges Prompt Area: click Done Prompt Area: input 8 enter Prompt Area: click Done Toolbox Bar: click Assign Element Type Element Type Window: (Quad Tab) set Reduced integration: OFF; click OK

Toolbox Bar: click Mesh Part Instance Prompt Area: click Yes

9. 计算分析 (Context Bar: Module Job)

Toolbox Bar: click Create Job Create Job Window: input Name: Plate; click Continue… Edit Job Window: click OK

Toolbox Bar: click Job Manager Job Manager Window: click Submit; click Monitor plate Monitor Window: click Dismiss when job is completed Job Manger Window: click Results

10. 后处理 (Context Bar: Module Visualization)

显示Von Mises应力云图：Toolbox Bar: click Plot Contour

显示应力的最大最小值：Menu Bar: select Viewport > Viewport Annotation Options… Viewport Annotation Options Window: (Legend Tab) select show min/max values: ON; click OK

显示x方向主应力云图：Menu Bar: select Result > Field Output… Field Output Window: select Primary Variable: S Stress components at integration points, Component:

有限元软件ABAQUS学习资料

S11; click OK

11. 计算结果的验证：

对于以上计算方案，由图4得到最大Von Mises等效应力为：288.342 MPa；由图5得到最大的x方向主应力为：300.013 MPa。