Buckling of Euler Column

Transcription

1 Problem: An Euler column with one end fixed and one end free is to be made of an aluminum alloy (E = 71 GPa). The cross sectional area of the column is 600 mm and the column is.5 m long. Determine the column buckling load corresponding to the following shapes: a) A solid round bar b) A square bar Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed. New York: McGraw Hill, May 00.

2 Overview Anticipated time to complete this tutorial: 30 minutes Tutorial Overview This tutorial is divided into six parts: 1) Tutorial Basics ) Problem Planning 3) Preprocessing ) Solution 5) Post-Processing 6) Hand Calculations Audience This tutorial assumes an intermediate knowledge of ANSYS 8.0; therefore, it goes into moderate detail to explain each step. A problem planning section has been added to help set up the problem. More advanced ANSYS 8.0 users should be able to complete this tutorial fairly quickly. Prerequisites 1) ANSYS 8.0 in house Structural Tutorial ) Completion of three or more Basic Machine Design Tutorials Objectives 1) Construct a plan for solving the problem ) Build and solve an Ansys model 3) Reuse model with minor alterations to solve a similar problem Outcomes 1) Learn how to set up the problem before starting Ansys ) Increase familiarity with the graphical user interface (GUI) 3) Learn how to create and mesh more complex geometries ) Increase familiarity with post processing tools

3 In this tutorial: Instructions appear on the left. Buckling of Euler Column Visual aids corresponding to the text appear on the right. Tutorial Basics All commands on the toolbars are labeled. However, only operations applicable to the tutorial are explained. The instructions should be used as follows: Bold > Example: Italics MB1 MB MB3 Text in bold are buttons, options, or selections that the user needs to click on > Preprocessor > Element Type > Add/Edit/DeleteFile would mean to follow the options as shown to the right to get you to the Element Types window Text in italics are hints and notes Click on the left mouse button Click on the middle mouse button Click on the right mouse button Some basic ANSYS functions are: To rotate the models use Ctrl and MB3. To zoom use Ctrl and MB and move the mouse up and down. To translate the models use Ctrl and MB1. 3

4 Take a few minutes to plan out your solution to this problem. Your plan should include some of the following items: Problem Planning 1) Obtain all necessary known information. Constant, c, for fixed-free end conditions: E for the aluminum alloy: Length of the column: Poisson's Ratio: Cross sectional area: ) Plan a simple, representative geometry. A solid 3D model of the column is not needed. A D model using just keypoints and lines will suffice if an element is chosen that can represent the cross sectional properties (area, area moment of inertia, etc.) of the column. The column could be built in either the horizontal direction or the vertical direction. 3) Contemplate an appropriate element for the mesh. Since you are creating a D model that represents a 3D model, you need D elements that can represent cross sectional properties. Elements listed under the Beam category (possibly use Beam3) have been used in other tutorials for this purpose. Choose an appropriate mesh size so there is a reasonable number of elements in the mesh. It is not always clear what a reasonable number of elements is. This usually comes with experience, but, for example, you would not want to use 0,000 elements (which could take a long time for the computer to solve) when 10 elements will suffice. ) Determine the best way to apply forces and constraints to the column. Since the column is fixed-free, one end of the column will need to have all of its degrees of freedom constrained and the other end needs to be free to move. The force should be applied to the free end. What force to apply to solve a buckling problem will be given in the tutorial. 5) Determine the best way to solve the first model and then modify it to solve the second. Part (a) of the problem wants you to solve the problem for a solid round bar and Part (b) wants you to solve it for a solid square bar. Note that the only change from solving one to solving the other is that (a) has a different cross sectional area then (b). Hence, a new model does not need to be created from scratch to solve (b), but the model used to solve (a) can be reused with a few minor modifications.

5 1) Change the working directory, jobname, and title of your project. ) Set Preferences to Structural. 3) Add a Beam3 element. ) Set the Real Constants for Beam3. Cross sectional area: Area moment of inertia:.86e-8 Total beam height: ) Create a Material Model. E: 71e9 PRXY:.3 5) Create two Keypoints. KP1: (0,0,0) KP: (0,.5,0) 6) Create a Line between keypoint one and two. 7) Change the Number of element divisions to 10. > Preprocessor > Meshing > Size Cntrls > Manual Size > Lines > All Lines Preprocessing 8) Mesh the line (use > Mesh > Lines command) Your model should look similar to the picture shown to the right: 5

6 Preprocessing 9) Apply Structural Displacement constraint to the bottom keypoint. Constrain all of its degrees of freedom. 10) Apply a Structural Force on the top keypoint. Give it a value of 1 and put it in the negative Y direction. (i.e. a value of -1) Your model should now look like the picture shown to the right. 6

7 Solution The model is ready to solve. To get the critical buckling load the solution must be done in steps. 11) > Solution > Analysis Type > New Analysis Select static and click ok. 1) Open up the unabridged menu and then open the analysis options. Select to include Prestresses. > Solution > Unabridged Menu then > Solution > Analysis Type > Analysis Options then next to stress stiffness or prestress select Prestress ON 13) Solve the model > Solution > Solve > Current LS 1) When it is done solving select Finish > Main menu > Finish 15) Setup the system to find the critical loads. > Solution > Analysis Type > New Analysis Select Eigen Buckling and click ok. Close any warning message that may have appeared when you clicked New Analysis. 16) Set up the buckling options > Solution > Analysis Type > Analysis Options Select Block Lanczos and put a value of 1 for the number of modes to extract 17) Solve the model again > Solution > Solve > Current LS 7

8 18) When it is done solving select Finish > Main menu > Finish 19) Set up an expansion pass to extract the critical load data > Solution > Load Step Opts > Expansion Pass > Single Expand > Expand Modes put a 1 in the number of modes to expand 0) Solve the model for the last time > Solution > Solve > Current LS Solution 8

9 1) Use the post processing tools to get the load value > General Postproc > List Results > Detailed Summary Post Processing The value of the critical load is N. This is the solution for part (a). Part (b) can be easily solved by reusing the model from part (a) with a slight modification. The only thing that needs to be changed in the part (a) model is the Real Constant properties. ) Change the Real Constant values of the model. New Values Cross sectional area: Area moment of inertia: 3e-8 Total beam height: ) Repeat steps 11-1 to get the value of the critical load for part (b). The value of the critical load for part (b) is N. 9

10 Hand Calculations The critical load (Pcr) for Euler buckling is given by: cπ EI Pcr = L Where: C = constant for conditions at the end of the column E = young s modulus I = the area moment of inertia L = is the length of the column For this problem: C =.5 (for a fixed -free column) E = 71 Gpa I is determined by the shape L =.5 m Pcr = π Pcr =.803e (.5)(71GPa) I (.5) 10 * I a) Solid Round bar I is given by: Now solve for I, then Pcr π (.076) I = 6 8 I =.86e Pcr = (.803e Pcr = 803N 10 b) Solid Square bar I is given by: a I = 1 )(.86e 8 To get a, use the known area A = a =.0006m a =.095m Now solve for I, then Pcr (.095) I = 1 8 I = 3e Pcr = (.803e Pcr = 81N 10 )(3e 8 ) ) I πd = 6 To get D, use the known area D A = π =.0006m D =.076m 10