ansys静力分析实例1.docx

1、ansys静力分析实例1结构分析实验指导书1.问题描述：这是一个关于角支架的单载荷步的结构静力分析。如图所示，左上角的销孔由于焊接而被固定死。右下角的销孔上作用一分布力。本问题的目标是熟悉ANSYS分析的基本过程。使用的是美国的单位体系。材料的氏模量为30E6 psi，泊松比0.27。2.几何建模：第一步：定义矩形1.Main Menu Preprocessor Modeling Create Areas Rectangle By Dimensions2.Enter the following:X1 = 0 ,X2 = 6,Y1 = -1,Y2 = 1 3.Apply to create th

2、e first rectangle. 4.Enter the following:X1 = 4,X2 = 6,Y1 = -1,Y2 = -35.OK to create the second rectangle and close the dialog box.第二步：更改绘图属性和重绘。1.Utility Menu Plot Ctrls Numbering2.Turn on area numbers. 3.OK to change controls, close the dialog box, and replot. 4.Toolbar: SAVE_DB.第三步：更改工作平面为极坐标系并创建

3、第一个圆1.Utility Menu WorkPlane Display Working Plane (toggle on)2.Utility Menu WorkPlane WP Settings3.Click on Polar. 4.Click on Grid and Triad. 5.Enter 0.1 for snap increment. 6.OK to define settings and close the dialog box. 7.Main Menu Preprocessor Modeling Create Areas Circle Solid Circle8.Pick ce

4、nter point at:WP X = 0，WP Y = 09.Move mouse to radius of 1 and click left button to create circle.10.OK to close picking menu. 11.Toolbar: SAVE_DB.第四步：移动工作平面并创建第二个圆1.Utility Menu WorkPlane Offset WP to Keypoints2.Pick keypoint at lower left corner of rectangle.3.Pick keypoint at lower right of recta

5、ngle. 4.OK to close picking menu. 5.Main Menu Preprocessor Modeling Create Areas Circle Solid Circle6.Pick center point at:WP X = 0，WP Y = 07.Move mouse to radius of 1 and click left button to create circle. 8.OK to close picking menu. 9.Toolbar: SAVE_DB.第五步：增加面1.Main Menu Preprocessor Modeling Oper

6、ate Booleans Add Areas2.Pick All for all areas to be added. 3.Toolbar: SAVE_DB.第六步：创建线倒角1.Utility Menu PlotCtrls Numbering2.Turn on line numbering. 3.OK to change controls, close the dialog box, and automatically replot. 4.Utility Menu WorkPlane Display Working Plane (toggle off)5.Main Menu Preproce

7、ssor Modeling Create Lines Line Fillet6.Pick lines 17 and 8.7.OK to finish picking lines (in picking menu).8.Enter 0.4 as the radius. 9.OK to create line fillet and close the dialog box. 10.Utility Menu Plot Lines第七步：创建倒角面1.Utility Menu PlotCtrls Pan, Zoom, Rotate2.Click on Zoom button. 3.Move mouse

8、 to fillet region, click left button, move mouse out and click again.4.Main Menu Preprocessor Modeling Create Areas Arbitrary By Lines5.Pick lines 4, 5, and 1.6.OK to create area and close the picking menu.7.Click on Fit button. 8.Close the Pan, Zoom, Rotate dialog box. 9.Utility Menu Plot Areas10.T

9、oolbar: SAVE_DB.第八步：将面添加到一起1.Main Menu Preprocessor Modeling Operate Booleans Add Areas2.Pick All for all areas to be added. 3.Toolbar: SAVE_DB.第九步：创建第一个销孔1.Utility Menu WorkPlane Display Working Plane (toggle on)2.Main Menu Preprocessor Modeling Create Areas Circle Solid Circle3.Pick center point a

10、t: WP X = 0，WP Y = 0 4.Move mouse to radius of .4 (shown in the picking menu) and click left button to create circle.5.OK to close picking menu.第十步：移动工作平面并创建第二个销孔1.Utility Menu WorkPlane Offset WP to Global Origin2.Main Menu Preprocessor Modeling Create Areas Circle Solid Circle3.Pick center point a

11、t: WP X = 0，WP Y = 04.Move mouse to radius of .4 (shown in the picking menu) and click left mouse button to create circle.5.OK to close picking menu.6.Utility Menu WorkPlane Display Working Plane (toggle off)7.Utility Menu Plot Replot8.Utility Menu Plot Lines9.Toolbar: SAVE_DB.第十一步：从支架上减掉销孔1.Main Me

12、nu Preprocessor Modeling Operate Booleans Subtract Areas2.Pick bracket as base area from which to subtract.3.Apply (in picking menu).4.Pick both pin holes as areas to be subtracted.5.OK to subtract holes and close picking menu.3.定义材料：第十二步：设置分析类型1.Main Menu Preferences2.Turn on structural filtering.

13、3.OK to apply filtering and close the dialog box. 第十三步：定义材料属性1.Main Menu Preprocessor Material Props Material Models2.Double-click on Structural, Linear, Elastic, Isotropic. 3.Enter 30e6 for EX. 4.Enter .27 for PRXY. 5.OK to define material property set and close the dialog box. 6.Material Exit第十四步：

14、定义单元类型和选项1.Main Menu Preprocessor Element Type Add/Edit/Delete 2.Add an element type. 3.Structural solid family of elements. 4.Choose the 8-node quad (PLANE82). 5.OK to apply the element type and close the dialog box. 6.Options for PLANE82 are to be defined. 7.Choose plane stress with thickness opti

15、on for element behavior. 8.OK to specify options and close the options dialog box. 9.Close the element type dialog box. 第十五步：定义实常数(什么是实常数？)1.Main Menu Preprocessor Real Constants Add/Edit/Delete2.Add a real constant set. 3.OK for PLANE82. 4.Enter .5 for THK. 5.OK to define the real constant and clos

16、e the dialog box. 6.Close the real constant dialog box.4.划分网格：第十六步：面网格划分1.Main Menu Preprocessor Meshing Mesh Tool2.Set Global Size control. 3.Type in 0.5. 4.OK. 5.Choose Area Meshing. 6.Click on Mesh. 7.Pick All for the area to be meshed (in picking menu). Close any warning messages that appear.8.C

17、lose the Mesh Tool.5.施加载荷：第十七步：施加位移约束1.Main Menu Solution Define Loads Apply Structural Displacement On Lines2.Pick the four lines around left-hand hole (Line numbers 10, 9, 11, 12).3.OK (in picking menu).4.Click on All DOF. 5.Enter 0 for zero displacement. 6.OK to apply constraints and close dialog

18、 box. 7.Utility Menu Plot Lines8.Toolbar: SAVE_DB.第十八步：施加分布力1.Main Menu Solution Define Loads Apply Structural Pressure On Lines2.Pick line defining bottom left part of the circle (line 6). 3.Apply. 4.Enter 50 for VALUE. 5.Enter 500 for optional value. 6.Apply. 7.Pick line defining bottom right part

19、 of circle (line 7).8.Apply. 9.Enter 500 for VALUE. 10.Enter 50 for optional value. 11.OK. 12.Toolbar: SAVE_DB.6.求解：第十九步：求解1.Main Menu Solution Solve Current LS2.Review the information in the status window, then choose File Close 3.OK to begin the solution. Choose Yes to any Verify messages that app

20、ear.4.Close the information window when solution is done. 7.查看结果：第二十步：读入数据结果1.Main Menu General Postproc Read Results First Set第二十一步：绘制变形图1.Main Menu General Postproc Plot Results Deformed Shape2.Choose Def + undeformed. 3.OK. 4.Utility Menu Plot Ctrls Animate Deformed Shape5.Choose Def + undeformed

21、. 6.OK.第二十二步：绘制应力图1.Main Menu General Postproc Plot Results Contour Plot Nodal Solu2.Choose Stress item to be contoured. 3.Scroll down and choose von Mises (SEQV). 4.OK. 5.Utility Menu Plot Ctrls Animate Deformed Results6.Choose Stress item to be contoured. 7.Scroll down and choose von Mises (SEQV).

22、 8.OK. 9.Make choices in the Animation Controller (not shown), if necessary, then choose Close. 第二十三步：列出约束反力1.Main Menu General Postproc List Results Reaction Solu2.OK to list all items and close the dialog box. 3.Scroll down and find the total vertical force, FY. 4.File Close (Windows).第二十四步：退出ANSYS软件1.Toolbar: Quit.2.Choose Quit - No Save! 3.OK.