MECH 3130: Mechanics of Materials. Fall Laboratory Manual. Volume II

Transcription

1 MECH 3130: Mechanics of Materials Fall 2015 Laboratory Manual Volume II Instructor Dr. Peter Schwartz Dr. Nels Madsen Lab Teaching Assistants Quang Nguyen: Abhiram Pasumarthy Jing Wu Abdullah Fahim 1

2 CONTENTS 1. FINITE ELEMENT ANALYSIS OVERVIEW 3 2. ANALYSIS OF TRUSS TUTORIAL ANALYSIS OF TRUSS EXERCISE ANALYSIS OF BEAM TUTORIAL ANALYSIS OF BEAM EXERCISE D STRESS ANALYSIS AND SCF TUTORIAL D STRESS ANALYSIS AND SCF EXERCISE ANSYS-CAD INTERFACE & ANALYSIS TUTORIAL ANSYS-CAD INTERFACE & ANALYSIS EXERCISE 73 2

3 LAB # 8 Finite Element Analysis Overview Source: ANSYS documentation What is Finite Element Analysis (FEA)? Finite element method is a numerical analysis technique for obtaining approximate solutions to a wide variety of engineering problems. Usually the problem addressed is too complicated to be solved satisfactorily by classical analytical methods. The finite element method produces many simultaneous algebraic equations, which are generated and solved on a digital computer. The finite element method originated as a method of stress analysis. Today finite element methods are used to analyze problems of heat transfer, fluid flow, lubrication, electric and magnetic fields, and many others. Finite element procedures are used in the design of buildings, electric motors, heat engines, ships, airframes and spacecraft. The word finite element method was first coined by Clough in 1960 in a paper on plane elasticity problems. In the years since 1960 the finite element method received widespread acceptance in engineering. With the advent of the digital computer, it opened a new avenue for solving complex plane elasticity problems. The first commercial finite element software made its appearance in The finite element method works by discretizing (breaking a real object into a large number of small elements). The behavior of each element is readily predicted by set mathematical equations. Then the computer adds up all the individual behaviors to predict the overall behavior of the actual object. The word "finite" in finite element analysis comes from the idea that there are finite numbers of elements in a model. This is in contrast to the classical approach (differential equation method) where an infinitesimal element is considered for derivation of the governing equations. To summarize, the finite element method satisfies the governing equations in an approximate or average sense whereas classical methods insist on validity of the solution at each and every point in the domain. The finite element method is employed to solve almost all physical systems. Structural mechanics (stress analysis) Mechanical vibration Heat transfer - conduction, convection, radiation Fluid Flow - both liquid and gaseous fluids 3

4 Various electrical and magnetic phenomena Acoustics What is a Node? A node is a coordinate location in space where the degrees of freedom (DOF) are defined. In the context of stress analysis of structural members, the DOF represent the possible motion of a point due to loading of the structure. The forces and moments are transferred between two adjacent elements through a node. What is an Element? An element is the basic building block of a finite element model. There are several basic types of elements. Typically, an element is bounded by the nodal points. Examples are solid brick and tetrahedron elements for 3 dimensional problems, Quadrilateral and triangular elements for 2 dimensional problems, beam and truss elements are typical line elements. Also the elements may be straight in shape or curved. Some General Type of Elements in ANSYS: 1. LINK 1 (or 2-D Spar or Truss): LINK 1 is the ANSYS name of the element. 2-D Spar or Truss is the type of the element. LINK1 can be used in a variety of engineering applications. Depending upon the application, you can think of the element as a truss, a link, a spring, etc. The 2-D spar element is a uniaxial tension-compression element with two degrees of freedom at each node: translations in the nodal x and y directions. As in a pin-jointed structure, no bending of the element is considered. 4

5 LINK1 Input Summary: Nodes Degrees of Freedom Real Constants Material Properties : I, J : UX, UY : AREA - Cross-sectional area ISTRN - Initial strain : EX (Young/s Modulus), PRXY (Poisson s Ratio) 2. BEAM3 ( or 2-D Elastic Beam ): BEAM3 is a uniaxial element with tension, compression, and bending capabilities. The element has three degrees of freedom at each node: translations in the nodal x and y directions and rotation about the nodal z-axis. BEAM3 Input Summary: Nodes : I, J Degrees of Freedom : UX, UY, ROTZ Real Constants : AREA - Cross-sectional area, ZZ- Area moment of inertia HEIGHT - Total beam height Material Properties : EX, PRXY Typical Steps in Finite Element Analysis: 1. Discretization of the domain: Divide the structure or continuum into finite elements. Mesh generation programs, called preprocessors help the user in doing this work. 2. Formulation of element properties: In stress analysis, this means determining nodal loads associated with all element deformation states that are allowed. In heat transfer, it means 5

6 determining nodal heat fluxes associated with all element temperature fields that are allowed. 3. Assembly procedure: Assemble elements to obtain the global finite element model of the structure. 4. Apply loads: These are nodal forces and/or moments in stress analysis, nodal heat fluxes in heat transfer analysis. 5. Impose boundary conditions: In stress analysis, specify how the structure is supported. This step involves setting several nodal displacements to known values (which are often zeros). In heat transfer, where typically certain temperature are known, impose all known values of temperatures. 6. Solution: Solve simultaneous linear algebraic equations to determine nodal degrees of freedom (Nodal displacements in stress analysis, nodal temperatures in heat transfer analysis). 7. Post Processing: In stress analysis, calculate element strains from the nodal degrees of freedom and the element displacement field interpolation, and calculate stresses from strains. Finally calculate additional quantities like strain energy, von-mises stress, etc. In heat transfer, calculate element heat fluxes from the nodal temperatures and the element temperature filed interpolation. Output interpretation programs, called Postprocessors, help the user sort the output and display it in graphical form. Introduction to ANSYS: ANSYS finite element analysis software enables engineers to perform the following tasks: Build computer models or transfer CAD models of structures, products, components, or systems. Apply operating loads or other design performance conditions. Study physical responses, such as stress levels, temperature distributions, or electromagnetic fields. Optimize a design early in the development process to reduce production costs. Do prototype testing in environments where it otherwise would be undesirable or impossible (for example, biomedical applications). The ANSYS program has a comprehensive graphical user interface (GUI) that gives users easy, interactive access to program functions, commands, documentation, and reference material. An intuitive menu system helps users navigate through the ANSYS program. Users can input data using a mouse, a keyboard, or a combination of both. 6

7 Overview of Model Generation: What Is Model Generation? In ANSYS terminology, the term model generation usually takes on the narrower meaning of generating the nodes and elements that represent the spatial volume and connectivity of the actual system. Thus, model generation in this discussion will mean the process of defining the geometric configuration of the model's nodes and elements. The ANSYS program offers you the following approaches to model generation: Creating a solid model within ANSYS. Using direct generation. Importing a model created in a computer-aided design (CAD) system. Typical Steps Involved in Model Generation within ANSYS: Begin by planning your approach. Determine your objectives, decide what basic form your model will take, choose appropriate element types, and consider how you will establish an appropriate mesh density. You will typically do this general planning before you initiate your ANSYS session. Enter the preprocessor (PREP7) to initiate your model-building session. Most often, you will build your model using solid modeling procedures. Establish a working plane. Generate basic geometric features using geometric primitives and Boolean operators. Activate the appropriate coordinate system. Generate other solid model features from the bottom up. That is, create key points, and then define lines, areas, and volumes as needed. Use more Boolean operators or number controls to join separate solid model regions together as appropriate. Create tables of element attributes (element types, real constants, material properties, and element coordinate systems). Set element attributes pointers. Create nodes and elements by meshing your solid model. Save your model data to Jobname.DB, and exit the preprocessor. 7

8 Importing Solid Models Created in CAD systems: As an alternative to creating your solid models within ANSYS, you can create them in your favorite CAD system and then import them into ANSYS for analysis, by saving them in the IGES file format or in a file format supported by an ANSYS Connection product. Creating a model using a CAD package has the following advantages: Planning Your Approach: As you begin your model generation, you will (consciously or unconsciously) make a number of decisions that determine how you will mathematically simulate the physical system: What are the objectives of your analysis? Will you model all, or just a portion, of the physical system? How much detail will you include in your model? What kinds of elements will you use? How dense should your finite element mesh be? In general, you will attempt to balance computational expense (CPU time, etc.) against precision of results as you answer these questions. The decisions you make in the planning stage of your analysis will largely govern the success or failure of your analysis efforts. Determine Your Objectives: This first step of your analysis relies not on the capabilities in the ANSYS program, but relies instead on your own education, experience, and professional judgment. Only you can determine what the objectives of your analysis must be. The objectives you establish at the start will influence the remainder of your choices as you generate the model. Your finite element model may be categorized as being 1-Dimensional, 2-dimensional or 3- dimensional, and as being composed of point elements, line elements, area elements, or solid elements. Of course, you can combine different kinds of elements as required (taking care to maintain the appropriate compatibility among degrees of freedom). For example, you might model a stiffened shell structure using 3-D shell elements to represent the skin and 3-D beam elements to represent the ribs. Your choice of model dimensionality and element type will often determine which method of model generation will be most practical for your problem. LINE models can represent 2-D or 3-D beam or pipe structures, as well as 2-D models of 3-D axisymmetric shell structures. Solid modeling usually does not offer much benefit for generating line models; they are more often created by direct generation methods. 8

9 2-D SOLID analysis models are used for thin planar structures (plane stress), "infinitely long" structures having a constant cross section (plane strain), or axisymmetric solid structures. Although many 2-D analysis models are relatively easy to create by direct generation methods, they are usually easier to create with solid modeling. 3-D SHELL models are used for thin structures in 3-D space. Although some 3-D shell analysis models are relatively easy to create by direct generation methods, they are usually easier to create with solid modeling. 3-D SOLID analysis models are used for thick structures in 3-D space that have neither a constant cross section nor an axis of symmetry. Creating a 3-D solid analysis model by direct generation methods usually requires considerable effort. Solid modeling will nearly always make the job easier. Coordinate Systems: The ANSYS program has several types of coordinate systems, each used for a different reason: Global and local coordinate systems are used to locate geometry items (nodes, key points, etc.) in space. The display coordinate system determines the system in which geometry items are listed or displayed. The nodal coordinate system defines the degree of freedom directions at each node and the orientation of nodal results data. The element coordinate system determines the orientation of material properties and element results data. The result coordinate system is the coordinate system in which results are computed and displayed. What Are Loads? The word loads in ANSYS terminology includes boundary conditions and externally or internally applied forcing functions. Structural: displacements, forces, pressures, temperatures (for thermal strain), gravity. Thermal: temperatures, heat flow rates, convections, internal heat generation, infinite surface. Magnetic: magnetic potentials, magnetic flux, magnetic current segments, source current density, infinite surface. 9

10 Electric: electric potentials (voltage), electric current, electric charges, charge densities, infinite surface. Fluid: velocities, pressures. Solution: What Is Solution? In the solution phase of the analysis, the computer takes over and solves the simultaneous set of equations that the finite element method generates. The results of the solution are: Nodal degree-of-freedom values, which form the primary solution and Derived values, which form the element solution. An Overview of Post processing: What Is Post processing? After building the model and obtaining the solution, you will want answers to some critical questions: Will the design really work when put to use? How high are the stresses in this region? How does the temperature of this part vary with time? What is the heat loss across this face of my model? How does the magnetic flux flow through this device? How does the placement of this object affect fluid flow? The postprocessors in the ANSYS program can help you answer these questions and others. Post processing means reviewing the results of an analysis. It is probably the most important step in the analysis, because you are trying to understand how the applied loads affect your design, how good your finite element mesh is, etc. Two postprocessors are available to review your results: POST1, the general postprocessor, and POST26, the time-history postprocessor. POST1 allows you to review the results over the entire model at specific load steps and sub steps (or at specific time-points or frequencies). In a static structural analysis, for example, you can display the stress distribution for load step 3. Or, in a transient thermal analysis, you can display the temperature distribution at time = 100 seconds. POST26 helps user to go over all the load steps at a time and observe the variation of quantities with respect to time or frequency. 10

11 ANSYS Menu Overview: The above figure shows the typical ANSYS menu. ANSYS main is divided into preprocessor, solution, post processor etc. Some of the frequently used options are available in ANSYS pull down menu as well. Any action that is executed through these menus can also be performed by typing an equivalent command in the command window. The Pan-Zoom-Rotate menu facilitates easy visualization of the model in the graphics window. Note: Save all your work until you get your final grade in your H: drive space. You may be asked anytime to show your work before the final grading time. 11

12 LAB # 8 Analysis of Truss - Tutorial The goal of this tutorial is to guide you through the development of a finite element model for a practical two-dimensional bridge truss structure. The geometry of the bridge is shown above. The bridge is constructed from steel members with three unique cross sectional areas (denoted 1, 2, 3, see Fig. 3). The areas are A1 = 13 cm 2, A2 = 42 cm 2, A3 = 20 cm 2. The bridge is considered to be loaded by a 3000 kg automobile as it traverses the span from one side to the other. The truss members will be assumed to be weightless. 12

13 Cross sectional area: 1 : 13 cm 2 2 : 42 cm 2 3 : 20 cm 2 Boundary Conditions: Node N1 and N5 : Ux = Uy = 0. 13

14 Problem statement: Solve the above 2-dimensional truss problem using ANSYS to compute the following: 1. Displacements (Ux and Uy) at all joints (nodes) of the truss in the horizontal and vertical directions. 2. Support reactions at the joints wherever the structure is supported. 3. Forces in each member (element). 4. Strain in each element. 5. Stress in each element. 6. Whether the structure is capable of withstanding the load?. 7. Where does the maximum displacement occur?. 8. Which element is stressed most? Data: 1. Dimensions of the truss and cross sectional area are given above. 2. Boundary conditions are as shown in the Fig Material properties: Young s modulus (E) = 211 GPa Poisson s ratio (υ) = 0.3 Yield strength = 390 MPa 14

15 How to save image files for use in a lab report: To save any picture which is visible at that instance on ANSYS graphics window follow these guidelines: In Ansys pull down menu click PlotCtrls. Then click on Hard Copy It will open a little window titled PS Hard Copy. Check following options: Graphics window, Color, JPEG, Landscape and then in Save to option type the file name as filename.jpg. You can give any file name you want. This will save the picture currently being displayed on graphics window in.jpg format in your current working directory. How to save text files for use in a lab report: To save any text file which is on current displays (text files show words and numbers). Click on file. Then click on save as. Then in file name type filename.txt. You can give any name instead of filename to save the text file. Later you can even pull the file out on windows. To open file on window open file with WordPad ( right click on file icon then open with.. and then select word pad. That will show you formatted output). General guidelines for solving the problem in ANSYS: 1. Open ANSYS window 2. Geometric Modeling Create Key points Create Lines Create areas Create volumes 3. Finite element modeling Declare analysis type Define element type Define the key options (e.g., Plane stress, plane strain, axisymmetric) Define element properties (real constants, e.g., thickness, area of cross section) Define material properties (e.g., E, υ, ρ etc.) Create nodes and elements (Meshing) Merge items (if there is any overlapping among the entities) 15

16 4. Solution Specify analysis type Apply boundary conditions (i.e., fixing the structure) Apply loads Specify the solution parameters Solve the problem 5. Post processing Get the displacements, reaction forces, strains and stresses. Plot the output variables if needed. Caution: ANSYS does not make any distinction between units. It is the user s responsibility to use correct and consistent units while solving the problem. If inconsistent units are used, the solution will be WRONG. For example, if the model is in meter, Young s modulus must be in N/m2 and forces will be in Newton, Pressure (if applied) will be in Pascal, mass density in kg/m3 etc. Similarly if model is in inches, then E in psi, loads are in lb(f) etc. Step by step procedure to solve the truss problem using ANSYS: a) Open ANSYS window: 1. Log on to system, and open up Ansys. 2. Change the Simulation environment to Ansys. 3. Set the working directory as your username/fea/truss/tutorial. 4. Type tutorial in the menu Job Name as shown in Fig Click on run. 16

17 b) Geometric modeling: Figure 6 Creating Key Points: 1. File Change title 2. Type Two dimensional truss problem 3. OK 4. Preprocessor 5. Modeling 6. Create 7. Keypoints 8. On working plane 9. Type the following numbers in ANSYS input window (Press enter key after typing each coordinate. Note the values are in meter.) 0, 0 2.5, 0 5.0, 0 17

18 7.5, , , , , , , OK 11. File Save as Jobname.db Creating Lines: 12. Modeling Create Lines Lines 13. Straight Line 14. Go on clicking on start point and end point until you get the desired geometry. (You can unselect any point by clicking right button of the mouse and reselect by clicking left button.) 15. OK c) Finite Element Modeling: Declare analysis type: 1. Main menu 2. Preferences 3. Structural (as shown in Fig. 8) 4. OK 18

19 Define element type: 5. Preprocessor 6. Element type 7. Add/Edit/Delete 8. Add 9. Link 3D finit stn 180 (as shown in Fig. 9). 10. OK 11. Close Define Element properties (real constants for truss element): 12. Real constants 13. Add/Edit/Delete 14. Add 15. OK 16. Type in the Field AREA as shown in Fig OK 18. Add 19. OK 19

20 20. Type OK 22. Add 23. OK 24. Type OK 26. Close Figure 9 Figure 10 20

21 Define Material properties: 27. Preprocessor 28. Material Props 29. Material Models Structural Linear Elastic Isotropic EX 211e9 (this is Young s modulus) PRXY 0.3 (this is Poisson s Ratio) OK Close the window Create nodes and Elements (Meshing of Rod elements): 30. Preprocessor Meshing Mesh Tool 31. Size Controls: Lines - Set (See Fig. 11) 32. Pick all 33. Ndiv No of Element divisions (enter 1) (see Fig. 11) 34. OK 35. Mesh Attributes 36. Picked Lines 37. Pick all the lines with cross sectional area 13 cm 2 (refer page 12). 38. OK 21

22 Figure Check the following attributes for the elements: (Fig. 12) MAT, Material number =1, REAL, Real constant set number = 1, TYPE, Element type number = OK 41. Mesh 42. Click on the lines with cross sectional area 13 cm OK 44. Plot 22

23 45. Multi-Plots 46. PlotCtrls 47. Numbering 48. Check the Node numbers on (see Fig. 13) 49. Check the Element numbers on in Elements/Attrib numbering (see Fig. 13) 50. OK 51. Repeat the steps from 35 to 45.This time select the lines having cross sectional area of 42 cm2. Assign the REAL, Real constant set number = 2. Figure 12 23

24 Figure Repeat steps from 35 to 45. This time select the lines having cross sectional area of 20 cm 2. Assign the REAL, Real constant set number = Type the command elist in the Command window and pay attention to Fig. 14 and note that following are present in your model. 1 thru 17 3D truss elements (link elements) All elements are of material type 1 Elements 1 thru 8 are having cross sectional area of 13 cm 2 Elements 9 thru 14 are having cross sectional area of 42 cm 2 Elements 15 thru 17 are having cross sectional area of 20 cm Type the commands rlist to verify the cross sectional areas you have specified are indeed present. 55. Type the command mplist to verify the material properties you have specified are indeed present. 24

25 d) Solution: Figure 14 Specify analysis type: 56. Solution 57. Analysis Type 58. New Analysis 59. Static 60. OK Specify solution parameters: 61. Sol n Controls 62. Check the following items in the Basic sub menu of solution controls dialog box as shown in Fig

26 Analysis options - Small displacement static Time at end of load step 1 Write items to result file All solution items 63. OK Figure 15 Apply Boundary conditions: 64. Solution 65. Define Loads 66. Apply 67. Structural 68. Displacement 69. On Nodes 70. Click on node number 1 and 5 (Bottom left and bottom right nodes) 71. OK 72. Check on All DOF (As shown in Fig. 16). 73. OK (A horizontal and a vertical triangle appears indicating that the node is fixed both in x and y directions.) 26

27 Figure 16 Apply Loads: 74. Solution 75. Define Loads 76. Apply 77. Structural 78. Force/Moment 79. On Nodes 80. Click on Node no OK 82. Check FY for Direction of Force/Moment and type a value of (as shown in Fig. 17 This is the total weight of the vehicle W (N) = m (kg)*g (m/sec 2 ) = 3000*10 = N, -ve sign indicates the load is acting downwards). 83. OK 84. Load Step Opts 85. Write LS File 86. Type the number 1 in the field LSNUM 87. OK 88. Define Loads 89. Delete 27

28 90. Structural 91. Force/Moment 92. On Nodes 93. Click on Node Number 2 (Note: see node figure in problem statement and then click on your model on that corresponding node, in your model the number might be different) 94. OK 95. Check ALL in the Lab field 96. OK 97. Repeat the steps 75 to 87 with the following changes: Vertical load of N to be applied on Node no 3 Type the number 2 instead of 1 in step Now delete all the previous loads and ( follow steps 88-96) 99. Repeat the steps 75 to 87 with the following changes: Vertical load of N to be applied on Node no 4 Type the number 3 instead of 1 in step File Save as Jobname.db Note: Here you have created 3 load steps for 3 different positions of car on the bridge, i.e. on left side of bridge, in the middle and on right side of bridge and then you ll solve for all 3 positions one by one. Figure 17 Solving the problem: 101. Solution 102. Solve 103. From LS Files ( Note:LS stands for Load Step ) 104. Type 1, 3 and 1 for LSMIN, LSMAX and LSINC respectively as shown in Fig

29 105. OK 106. You are OK if you get a dialog box Solution is Done. Otherwise contact instructor. Figure 18 e) Post Processing the Results: Read the result file and plot the deformed shape: 107. General Postproc 108. Data & File Opts 109. Check on All items, Click on and select the file, tutorial.rst as shown in Fig OK 111. Read Results 112. First Set 113. Plot Results 114. Deformed Shape 115. Check on Def + undeformed 116. OK 117. This gives the deformed shape overlapped on undeformed shape for load case 1 (Save it as a picture: Plotctrls - Hard Copy - To File Save to - <file.bmp> ) 118. Read Results - Next Set and repeat steps Read Results - Last set and repeat steps

30 Figure 19 Check the reactions: 120. List Results 121. Reaction Solu 122. Check on All items 123. OK 124. Verify whether the reactions are summing up to give the applied load in vertical direction and zero in horizontal direction (This is an important check). Plot displacements: 125. Read Results First Set 126. Plot Results Contour Plot 127. Nodal Solu 128. Check on DOF Solution and y component of displacement 129. OK (Compare your plot Fig. 21) 130. Save this picture Plotctrls - hard copy - to file select the format you wish - save to - <file.bmp> 132. OK (The pictures will be stored in the current working directory). 30

31 Figure 20: Deformed Vs Undeformed plot Figure 21: Vertical displacement (Uy) of the Truss List Nodal displacements, Element forces, stresses and strains: 133. List Results 134. Nodal Solution 135. Check on DOF Solution and and Displacement vector sum 136. OK (Compare your results with those in Fig. 22) 137. Save this file for future reference (File Save as <filename.txt>) List Results 139. Nodal Loads 140. Check on All struc forc F 141. OK (Compare your results with those in Table 1) List Results 143. Element Solution 144. Check on Line Elem Results and Element Results 145. OK. Stresses and Strains in Element coordinate system will be listed in this file (FORCE: axial force in each truss; STRESS: axial stress in each truss. Positive sign of STRESS means tension and negative compression). See Fig. 23 (Save this file for future reference: File Save as - <filename.txt>) Animation: 146. PlotCtrls 147. Animate 148. Deformed Results 31

32 149. Check on DOF Solution and UY 150. OK Exit: 151. SAVE_DB 152. File Exit (Quit No Save! OK) Figure 22: Nodal displacements. 32

33 PRINT F REACTION SOLUTIONS PER NODE ***** POST1 TOTAL REACTION SOLUTION LISTING ***** LOAD STEP= 0 SUBSTEP= 1 TIME= LOAD CASE= 0 THE FOLLOWING X,Y,Z SOLUTIONS ARE IN THE GLOBAL COORDINATE SYSTEM NODE FX FY FZ TOTAL VALUES VALUE E TABLE 1 PRINT ELEM ELEMENT SOLUTION PER ELEMENT ***** POST1 ELEMENT SOLUTION LISTING ***** LOAD STEP 0 SUBSTEP= 1 TIME= LOAD CASE= 0 EL= 1 NODES= 1 2 MAT= 1 XC,YC,ZC= AREA= E-02 LINK180 FORCE= E-10 STRESS= E-07 EPEL= E-19 TEMP= EPTH= Understanding the line element results: EL= 1 element number is 1 NODES= 1 2 nodes 1 and 2 make up element 1 STRESS = E-07 axial stress in element 1 made of nodes 1 and 2 33

34 LAB # 9 1. ANALYSIS OF TRUSSES - Exercises The truss, shown in Fig. 1, is made of AL6061-T6. Use E=10e6 psi and Poisson s ratio = Assume a cross-sectional area of 1 for the outer elements (shown by thicker lines) and ½ for the diagonal elements. (All dimensions in Fig. 1 are in inches). Find the values of axial stresses in each member of the truss using ANSYS package. Repeat your stress calculations for the truss by hand and provide an element-by element comparison with Part- (a). a) Show a picture showing the loads and boundary conditions on which the element numbers are shown. b) Show a picture showing the deformed and undeformed shapes c) Show a picture of the undeformed shape on which the corresponding stress values of each link are hand written beside the links. d) Present the complete hand calculation that you did to find the stress values. e) Present a table comparing the Ansys and hand calculated results. Use the same element numbers in the first picture as reference. 34

35 2. Find the values of axial stresses in each member of the truss shown in Figure 2. Also find displacements at each node. List the values of the maximum displacement and axial stress in the truss. Consider the following material and sectional properties to analyze the truss: Young s modulus of all elements: 13.6e6 psi. Poisson s ratio is Each member along AB,CB,AC,BE,BF,FE,HL( Shown by thick line) has hollow circular cross section With 4.5 inch outer diameter and 2.4 inch inner diameter. Each linking element (shown by thin lines) has solid circular cross-section with diameter 2 inch. Note: Use same type of element as tutorial problem for both these exercise problems a) Show a picture showing the loads and boundary conditions on which the element numbers are also shown. b) Show a picture showing the deformed and undeformed shapes c) Show a picture of the undeformed shape on which the maximum axial stress value and the maximum y displacement value are hand written beside the respective link and node. Note: Do not submit any numerical printed results that are directly output from Ansys. 35

36 LAB # 10 Analysis of Beam - Tutorial Analysis of a Bicycle Handlebar Analyze the bicycle handle bar shown in the Figure 1 (i) without and (ii) with the reinforcement bar. For both cases find maximum stresses in each of the members and deflections at the end of the handle. Find the value of maximum stress and its location. Consider the followings while analyzing the model: a) Each member of the handle has hollow circular section with 3/4 outer diameter and thickness 1/8. b) The reinforcing bar has a hollow circular cross section with outer diameter ½ and thickness 1/8. c) Consider the material as steel with Young s modulus 30E6 psi and Poisson s ratio 0.3. d) Assume a distributed load of 100 lb(f) over the shaded regions of the handle. Note: In this tutorial, the problem is solved with the reinforcement bar. You need to solve without the reinforcement bar and compare the results in the lab. 36

37 Step by step procedure to solve the beam problem using ANSYS: 1. Open Ansys in the working directory named Tutorial under Beam. a) Geometric modeling: Creating key points: 2. File Change title 3. Type Analysis of Bicycle handlebar using 2D beam element 4. OK 5. Preprocessor 6. Modeling 7. Create 8. Key points 9. On Working Plane 10. Type the following numbers in ANSYS input window(press enter key after typing each number) 0,0 4,0 6,0 9, , , ,0 20,0 24,0 12, , , OK 12. Save the file 37

38 Creating Lines: 13. Lines Lines 14. Straight line 15. Go on clicking on start point and end point until you get the desired geometry (You can unselect any point by clicking right button of the mouse) 16. OK (Make sure that you got the geometry shown in Fig File Save as Jobname.db b) Finite element modeling: Declare analysis type: 18. Main Menu 19. Preferences 20. Structural 21. OK Define element type : 22. Preprocessor 23. Element Type 24. Add/Edit/Delete 25. Add 38

39 26. Beam 2 node 188 (as Shown in Fig. 3.) (OR type command: et, 1, BEAM188 in command window) The selection must be displayed in selection display bar. 27. OK 28. Close Define Element properties (real constants for beam element): 29. Preprocessor 30. Sections 31. Beam 32. Common Sections (a beam tool appears as shown in Fig. 4). 33. Type Handle in the Name section, Chose Hollow Circular cross sections and type 0.25 in for inner radius and in for outer radius. Leave N blank. 34. Preview (Beam cross sectional properties appear as shown in Fig. 5). 35. OK 39

40 36. Sections Beam Common Sections 37. Type ID = 2, Name = Reinforcing Bar 38. Choose Hollow Circular cross sections and type Ri=0.125 in, Ro = 0.25 in. 39. Preview 40. OK 41. Save the file Define Material properties: 42. Material Props 43. Material Models 44. Structural (DOUBLE CLICK) Linear Elastic Isotropic Ex=30e6 Prxy = OK 40

41 46. Material Exit 47. Save the file 48. Plot Multi-Plot Create nodes and Elements (Meshing): 49. Select 50. Entities 51. Check the following items Lines By Num/Pick From Full OK (Expand window if you don t see OK button). 52. Mouse pick all the lines except reinforcement bar (long one) 53. OK 54. Select Everything Below Selected Lines 55. Plot - Lines 56. Preprocessor Meshing Mesh Tool 57. Click on Lines Set 58. Pick all 59. Type 5 in NDIV field 60. OK (This is called mesh seeding) 61. Preprocessor Meshing Mesh Attributes Picked lines Pick all 62. Check the following items and click OK. Material number 1 Element type number 1 BEAM188 Element section 1 Handle 63. Mesh (on Mesh Tool window. Sometimes Mesh Tool window is hidden behind the main window and can be found by restoring down the main window) 64. Pick all (This is called meshing) 65. Select - Everything 66. Plot Multi-Plots 41

42 67. Repeat the steps from 49 to 55 by selecting only reinforcement bar 68. Repeat the steps from 57 to 60 by typing 10 in NDIV field for reinforcement bar 69. Repeat 61 to 66 by assigning Element section = Reinforcement bar 70. Select Everything 71. Plot Elements 72. File Save as Jobname.db d) Solution: Specify analysis type 73. Solution Analysis Type New Analysis Static 74. OK 75. Sol n Controls (all defaults) 76. OK Apply Boundary conditions: 77. Solution Define Loads Apply Structural Displacement On Nodes 78. Pick the bottom most node of the supporting rod 79. OK 80. Check on All DOF 81. OK Apply Loads: 82. Solution Define Loads Apply Force/Moment On Nodes 83. Select (6+6 =12) nodes on the handle (6 on each end. Show nodes by clicking Plot-Nodes and select 6 nodes starting from very left (right) on each handle). 84. OK 85. Select FY in the field Lab and type a value of in the field VALUE (Note: 100 lb load is uniformly distributed on 12 nodes (8.33 x 12 = 100).). 86. OK (Compare your model with the one in Fig. 6). 87. File Save as Jobname.db 42

43 Figure 6: Solve the problem: 88. Solution 89. Solve 90. Current LS 91. OK e) Post Processing the results: Read the results file and Plot the deformed shape: 92. General Postproc 93. Data & File Opts 94. Highlight on All Items 95. Click bottom Select Jobname.rst Open OK 96. Read Results First Set 97. Plot Results Deformed Shape (Check on Def + undeformed) 98. OK 99. To save this as a file to be included in report, do the following: 100. Plot Ctrls Hard Copy To File 101. Check on Color, Tiff, Tiff compression, Reverse Video, Portrait 102. OK (Compare your plot with the one in Fig. 7) 43

44 Figure 7: Check reactions 103. List Results Reaction Solu (Check on All Items) 104. OK (Verify whether the summation of vertical reactions equal to the applied load. Plot displacements 105. General PostProc Plot Results Contour Plot Nodal Solu 106. Check on DOF Solution and y-component of displacement Animation 118. PlotCtrls Animate Deformed Results 119. Check on DOF Solution and UY 120. OK 44

45 ANALYSIS OF BEAM - Exercise Solve the statically indeterminate beam using ANSYS. Choose the number of element divisions such that each element would be 1 in length. Assume following material properties for the beam: E = 10.6e6 psi, υ = 0.33 a) Derive the expression for deflection of the beam using the methods discussed in class (Integration, Superposition, Discontinuity Methods). Present the three separate expressions for 0<=x<=30, 30<=x<=60 and 60<=x<=96. b) Present a table comparing the Ansys and hand calculated deflections with a column for percentage error. c) Plot the deflection of the beam from Ansys(as data points) and the hand calculated results(as a curve) on the same graph in Excel. d) Present a picture showing all the boundary conditions and loads. e) Show the locations and values of the maximum deflection and stress on a picture of the deformed shape. 45

46 Lab # 11 2D Stress Analysis Tutorial (A note on stress concentration factor) In engineering practice, the interest is always to know what is the value of maximum stress occurring for given loading and given structural member geometry. Complex stress distribution occurs near the point of load application, at locations where member s cross sectional area changes and more severely where, there is a defect like a crack. Figure (b) and (c) shows the actual and average stress distribution across the cross section passing through the hole (consider the hole as a defect here in a uniaxial test specimen). It is clear that stress at the boundary of hole (top and bottom) is more than the average stress. The results of this kind of investigation are usually reported in terms of Stress Concentration Factor (SCF) K. We define K as a ratio of the maximum stress to the average stress action at the smallest cross section. 46

47 2D Stress Analysis Tutorial Analysis of a Plate with a Hole under uniaxial tension: Dimensions: Length of the plate (L) = 20 in Height of the plate (H) = 10 in Thickness of the plate (t) = 1 in Diameter of the hole (D) = 1 in Loading: Uniform applied stress applied (p) = 100 psi Material Properties: Young s modulus (E) = 28.6 x 106 psi Poisson s ratio (υ) = 0.3 This problem can be solved in ANSYS using 2D plane stress assumption. The symmetry about both X and Y axis will be exploited and only one quarter of the model will be constructed in ANSYS. The Closed form solution is available for this classical problem. The nodal stresses along certain paths will be extracted from the finite element solution and plotted along with the analytical results for comparison. As you become more familiar with ANSYS, it is better 47

48 to work in command mode rather than menu driven mode. This approach is much faster, well suited for routine and repetitive tasks and less prone to errors. The command based approach uses APDL(ANSYS Parametric Design Language). This powerful feature of ANSYS offers great help in automating routine tasks while constructing a huge model. Step by step procedure to solve the problem using ANSYS: a) Open ANSYS window: 1. File Change title 2. Type Stress concentration in rectangular plate with a central hole 3. OK b) Geometric modeling: 4. Preprocessor Modeling Create Keypoints On Working Plane 5. Type the following numbers in same order in ANSYS input window ( Press enter key after typing each coordinates) 0,0 0.5,0 0,0.5 0,-0.5 0,5 0,-5 10,5 10,-5 6. Preprocessor- Modeling Create Lines Arcs -By End KPs & Rad 7. Select key point # 2 ( point (0.5,0)) and 3 ((point (0,0.5) ) 8. OK 9. Select key point # 1 ( origin point) 10. OK 11. Type 0.5 for RAD as shown in Fig OK 13. Make the arc between keypoint # 2 (point (0.5,0)) and 4 (0,-0.5)) with center as kepoint #1 (origin) in same manner as in steps 16 to

49 14. Preprocessor Modeling Create Lines Straight lines 15. Make lines in following manner to get geometry as in Fig. 3. Join from KP(keypoint) 3 to KP 5 ( from and to must be the same as shown here) from KP 4 to KP 6 from KP 5 to KP 7 from KP 6 to KP 8 from KP 7 to KP OK 17. Plot Controls - Numbering 18. Check on Key point numbers and Line numbers 19. OK 20. Plot Multi-Plots 21. File Save Jobname.db 22. Modeling Create Areas Arbitary By line and then Click on all lines. 23. OK 49

50 50

51 c) Finite Element Modeling: Declare analysis type: 24. Main Menu Preferences Structural 25. OK Define element type and real constants: 26. Preprocessor Element type Add/Edit/Delete - Add 27. Choose Structural mass->solid-> Quad 8node OK 29. Options 30. Check on Plane strs w/thk 31. OK 32. Close 33. Real Constants Add/Edit/Delete Add OK 34. Type a value of 1.0 in for Thickness 35. OK Close 36. Plot. ( from pull down menu at top) 37. Lines. Define Material Properties: 38. Preprocessor Material Properties Material Model (Double click) Structural Linear Elastic Isotropic - EX 28.6e6 - PRXY OK - Material - Exit Meshing: 39. Preprocessor Meshing Mesh Tool 40. Size controls: Lines - Set 51

52 41. Mouse click on Lines 1, 2, ( OR If your line number is different from Fig. 3,click on lines making hole boundry). 42. Type 16 for NDIV and 1 for SPACE as shown in Fig OK 44. Size controls: Lines - Set 45. Select lines 3 and 4(leftmost edges). 46. OK 47. Type 16 for No of element divisions and 2 for spacing ratio 48. OK 49. Repeat the steps 40 to 48 for lines 5 and Repeat the steps 40 to 48 for lines 7 (rightmost edge) with NDIV=10, SPACE=1 51. Highlight the following items in the mesh tool as shown in Fig Mesh (in Mesh Tool window) 53. Pick all 54. Verify whether you got the mesh shown in Fig. 6. Note: There are several approaches for generating the mesh. This is one of those, and not necessarily the best one. You are encouraged to try different methods. 52

53 53

54 Figure 5. 54

55 d) Solution: Specify analysis type 55. Solution ( From Main Menu) Analysis Type New Analysis Static OK Apply Boundary conditions: 56. Define Loads Apply Structural Displacement On Lines 57. Click on 3 and 4 (See Fig. 3, leftmost edges) 58. OK 59. Check UX ( and if it doesn t appear in selection box then type UX in that box) and type 0 in the field of VALUE 60. OK Apply Loads: 61. Define Loads Apply Structural Pressure On Lines 62. Click on Line number 7 (rightmost edge see Fig. 3). 63. Type a value of -100 as shown in Fig Save the file Solving the problem: 65. Solution Solve Current LS 66. OK 55

56 e) Post Processing: 67. General PostProc (Main Menu) Data & Result file Opts 68. Read Results First Set 69. Plot Results Contour Plots Nodal Solu Stress X-Direction SX 70. OK (Compare your plot with Fig. 8. You can zoom in hole portion and observe where maximum stress is occurring and by what factor it is greater than applied stress by looking at color chart at bottom). 71. Plot Results Deformed Shape Def + Undeformed OK 72. Plot Results Contour Plot Nodal Solution. 73. Select DOF Solution and UX OK 74. Plot Ctrls Animate Deformed Results 75. Highlight Stress and SX 76. OK 56

57 Plotting Graphs, Extracting table of numbers from ANSYS: 77. General PostProc ( Main menu) Path Operations Define Path By Nodes 78. Select all the nodes along lines 3 in order (starting from the edge of the circular cut-out all the way up to top edge of the plate, See Fig. 3). You can zoom in and out during selection using PlotCtrls Pan Zoom Rotate. 79. OK 80. Give a name for the path (say p1) and type nsets = 6, ndiv=1 as shown in Fig OK 82. Path Operations->Map on to path 83. Check Stress X-Direction SX and type a name S_X for Lab as shown in Fig

58 84. Plot Path item On Graph 85. Highlight on S_X 86. OK (Compare your plot with the one in Fig. 12). 87. You can export the plot into.jpg file by clicking on 58

59 88. PlotCtrls Hard Copy (check -.graphics window, color, JPEG, landscape, save to) (you can specify full path name for saving hard copy i.e., /home/me_h2/yourid/mech3130/ansys/2dstress/tutorial/graph.jpg ) 89. List Path item 90. Highlight on S_X 91. OK 92. Save this ASCII file ( as.txt format) for plotting with other external plotting routines. 59

60 2D STRESS ANALYSIS & SCF - Exercise A photo elastic sheet of 1.5 inch width 6 inch length and in thickness has a symmetrically located 0.5 inch diameter circular cut-out. Plot the variation of σx along the line connecting the top of the hole boundary and the top edge of the plate both from FEA. E=3.2 GPa, υ = Sheet is subjected to a load of 100 psi on the two side boundaries. A thin sheet of aluminum (AL 6061-T6) is subjected to uniform tension as shown. The sheet has circular cut-outs as shown in the Figure. Assume that the sheet is 4 inches wide, 18 inches long, ¼ inch thick, the central cut-out has a diameter of 2 inch, smaller cut-outs have a diameter of ½ inch and the sheet is subjected to a load of 400 lbs. Your report should include plots of SCF vs. R/L at (a) the primary hole, (b) the secondary hole. Also, discuss the influence of eccentricity parameter R/L on the SCF at each location. The various values of L to be used in the simulations are 3 and 6 inches. 60

61 Lab # 12 ANSYS - CAD IGES INTERFACE AND ANALYSIS - Tutorial A chair as shown in the figure is subjected to a load of a person sitting on it. Assume that 2/3 of the person s load is acting on the seat and the remaining is acting on the back rest of the chair. Model the given chair in solid edge software and analyze the same in Ansys to find the deformed shape due to the simultaneous loads. Assumptions: 1. The weight of the person sitting is 150 pounds. 2. The chair is made up of a material with the following properties Young s modulus = 1.34e6 and, Poisson s ratio = The rear two legs of the chair have all degrees of freedom constrained and the other two legs have the z axis displacement constrained. 61

62 Procedure to solve the problem Solid edge modeling 1. Open Solid edge software. 2. Click on new model. 3. Click on the sketch icon and select the plane to sketch Fig 1 4. Click on the line icon(fig 1) 5. Click at points on the sketching plane to draw lines. 6. Change the dimensions and orientation of the lines to suit. 7. Sketch the cross section of the body of the chair(except the legs)(fig 3) 8. Click on Return. 62

63 Fig 2 Fig 3 63

64 9. Select the Sketch 1 from the tree outline and click on the protrude icon. 10. Choose to select from sketch from the drop down menu 11. Now click on the icon. 12. Specify the depth of the protrusion. 13. Click on Return Fig 4 64

65 Fig 5&6 65

66 14. Using the sketch and extrude command in the same way complete the modeling of the legs of the chair (Fig 5&6, arrive at Fig 7). 15. Select the sides of the chair where you had previously chosen planes. 16. Finish the model and save it in.igs format using the Save as command. Fig 7 Analysis using ANSYS: Import model to ANSYS: 1. Open the ANSYS window. 2. Click on file import IGES 3. Check yes for all options and click OK 4. Click browse on the next window and select the igs file you had saved using Solid Edge 66

67 Fig 8&9 67

68 5. Select tolerance to be taken from the IGS file (Fig 9). 6. Click OK Fig The model opens in the ANSYS as shown in Fig 10. Declare Analysis type: 18. Main menu 19. Preferences 20. Structural 21. OK Define element type: 22. Preprocessor 23. Element type 24. Add/Edit/Delete 25. Add 26. Solid brick 8 node 45 68

69 27. OK 28. Close Define Material properties: 29. Preprocessor 30. Material Props 31. Material model (double click) Structural Linear Elastic Isotropic EX 1.34e6 (this is Young s modulus) PRXY 0.4 (this is Poisson s Ratio) OK Close the window Create nodes and Elements (Meshing of Rod elements): 32. The volume is not in a topology to be divided into perfect 4-6 sided elements. 33. It has to be divided into Volumes suitable for meshing 34. Type the following commands in the ANSYS command prompt. 35. wpstyl,defa 36. vsbw,all 37. wpoffs,0,0, vsbw,all 39. Now the chair is divided into 6 volumes viz, four legs, one base and one back part (Fig 11). 40. Click on pre-processor Meshing Mesh Volume Mapped 4-6 sided 41. Select the four legs and the back of the chair. 42. The base of the chair is still not in the topology for meshing. 69

70 43. Click on pre-processor Meshing Mesh 44. Select the base of the chair. Volume sweep Sweep Fig 11 70

71 Fig 12 Apply Loads: 45. Pre-processor 46. Loads 47. Define Loads 48. Apply 49. Structural 50. Displacement 51. Areas 52. Select the rear two legs of the chair and click OK 53. Arrest all DOF and click OK 54. Repeat the same for the other two legs of the chair but arrest only the UZ for these two legs. 55. Pre-processor 56. Loads 57. Define Loads 71

72 58. Apply 59. Structural 60. Pressure 61. Areas 62. Select the area of the seat of the chair 63. Enter the value of pressure load.(calculate the pressure load from the data given) 64. Repeat the same for the back rest part of the chair Solve the problem: 65. Solution 66. Solve 67. Current LS 68. OK Post processing the results: 69. General post processor 70. Plot results 71. Deformed shape(fig 13) 72. Def + undeformed 73. OK Fig 13 72

73 ANSYS - CAD IGES INTERFACE AND ANALYSIS - Exercise 1. Model the chair with the following changes to the Dimensions The thickness of the legs is reduced to1.2 from 1.5 inches. The thickness of the other portions of the chair is reduced to 0.8 instead of 1. The legs and the seat are now perpendicular to each other.(90 o instead of the 110 o and 114 o ) 2. Assume the material to be Aluminum (E=10e6 psi and Poisson s ratio = 0.3).The weight of the person sitting on the chair is now 200 pounds. The other conditions remain the same as in the tutorial. 3. Report the deformed shapes for both the cases.(tutorial and exercise). 4. From your analysis which do you think is the safer chair of the two cases and why? 73