abaqus带孔平板的有限元分析

ABAQUS step-by-step 建模分析实例 1 - 1 - 实例实例 1：带孔平板的有限元分析：带孔平板的有限元分析 y x p 100 50 50 100 R5 p=100N/mm2 t=1 mm E=210000N/mm2 =0.3 单位: mm 图 1 平面问题的计算分析模型 1. 进入 ABAQUS/CAE 开始开始 程序程序 ABAQUS 6.xx ABAQUS CAE 2. 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 Youngs Modulus: 210000, Poissons 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) ABAQUS step-by-step 建模分析实例 1 - 2 - 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 Varia