Statically Indeterminate Beam

Transcription

1 Problem: A rectangular aluminum bar.5 inches thick and 2 inches wide is welded to fixed supports at the ends, and the bar supports a load W=800 lb, acting through the pin as shown. Find the reactions at the supports. Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed. New York: McGraw Hill, May 2002.

2 Overview Anticipated time to complete this tutorial: 20 minutes Tutorial Overview This tutorial is divided into six parts: 1) Tutorial Basics 2) Problem Planning 3) Preprocessing 4) 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 2) Completion of three or more Basic Machine Design Tutorials Objectives 1) Quickly create model using beam elements and sections 2) Properly constrain the model 3) List the reaction forces Outcomes 1) Learn how to set up the problem before starting Ansys 2) Increase familiarity with the graphical user interface (GUI) 3) Learn how to create and mesh more complex geometries 4) Increase familiarity with post processing tools 2

3 In this tutorial: Instructions appear on the left. 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 MB2 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 MB2 and move the mouse up and down. To translate the models use Ctrl and MB1. 3

4 Problem Planning This problem can be solved using an appropriate beam element and cross section. The beam can be defined by three keypoints and two lines. The cross section will have the dimensions of the width and depth of the beam. The two outside keypoints will be constrained in all degrees of freedom to simulate the weld between the beam and the wall. The force will be applied to the center keypoint. 4

5 1) Set the working directory, jobname, and title. Preprocessing 2) Enter Young s modulus and Poisson's ratio for aluminum into a new material model. E:10e6 & PRXY:.33 3) Add a Beam189 element to the model. 4) Create a rectangular beam cross section. > Preprocessor > Sections > Beam > Common Sections 5) Create keypoints. 6) Create lines between keypoints 1 and 2, and keypoints 2 and 3. 7) Set line attributes for both lines. > Preprocessor > Meshing > Mesh Attributes > All lines Make sure that the cross section for the lines is set to the rectangular cross section that you just defined. 8) Set the line element size to 1. > Preprocessor > Meshing > Size Controls > Manual Size > Lines > All lines 9) Mesh the lines. 10) Apply All DOF constraints to the outermost keypoints. 11) Apply an 800 lb force in the -Y direction at the interior keypoint. 12) View the model in 3D by typing the following commands into the command line: /Eshape,1,0 /Replot 5

6 13) Solve the model. Solution/Post Processing 14) Enter the post processor and view results. > General Postprocessor > List Results > Reaction Solution > FY 6

7 Hand Calculations 7