Chapter 22 - Finite Element Analysis Using ANSYS PDF

CHAPTER 22 Finite Element Analysis...

CHAPTER 22 Finite Element Analysis Using ANSYS† CHAPTER OUTLINE 22.1 Introduction 663 22.4 Finite Element Discretization 665 22.2 GUI Layout in ANSYS 664 22.4.1 Element Type 665 22.3 Terminology 664 22.4.2 To Define an Element 665 22.3.1 Database and Files 664 22.4.3 Meshing Methods 666 22.3.2 Defining the Jobname 664 22.4.4 Mesh Density Control 666 22.3.3 File Management Tips 664 22.4.5 Material Properties 666 22.3.4 Defining an Analysis Title 665 22.5 System of Units 667 22.3.5 Save and Resume 665 22.6 Stages in Solution 667 22.3.6 Tips on SAVE and RESUME 665 663 22.1 INTRODUCTION ANSYS is a general-purpose finite element software that includes preprocessing (to create the geometry and generating mesh), solver, and postprocessing modules in a unified Graphical User Interface (GUI) environment. ANSYS commonly refers to ANSYS Mechanical or ANSYS Multiphysics. In ANSYS, a problem can be solved in either a batch mode or an interactive mode. In batch mode, an input file is to be created and executed from the command line. In the interactive mode, GUI is used and the operations to be performed are either chosen from a menu or typed in a graphics window. Examples are presented to illustrate both the modes in this chapter. † ANSYS FEM software is marketed by ANSYS, Inc, Southpointe, 275 Technology Drive, Canonsburg, PA 15317. The Finite Element Method in Engineering. DOI: 10.1016/B978-1-85617-661-3.00022-2 © 2011 Elsevier Inc. All rights reserved.  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis 22.2 GUI LAYOUT IN ANSYS FIGURE 22.1 664 ANSYS Graphical User Interface. 22.3 TERMINOLOGY 22.3.1 Database and Files The database refers to the data ANSYS maintains in memory as users build, solve, and postprocess models. The database stores both input data and ANSYS results data: Input data—information that users must enter, such as dimensions, material properties, and loads Results data—quantities that ANSYS calculates, such as displacements, stresses and temperatures 22.3.2 Defining the Jobname Utility Menu > File > Change Jobname The jobname is a name up to 32 characters that identifies the ANSYS job. When we define a jobname for analysis, the jobname becomes the first part of the name of all files the analysis creates. (The extension or suffix for these file names is a file identifier such as.DB.) By using a jobname for each analysis, we ensure that no files are overwritten. 22.3.3 File Management Tips Run each analysis in a separate working directory. Use different jobnames to differentiate analysis runs. We should keep the following files after any ANSYS analysis: log file (log); database file (.db); results files (.rst,.rth, …); load step files, if any (.s01,.s02, …)  CHAPTER 22 Finite Element Analysis Using ANSYS 22.3.4 Defining an Analysis Title Utility Menu > File > Change Title This will define a title for the analysis. ANSYS includes the title on all graphics displays and on the solution output. 22.3.5 Save and Resume Since the database is stored in the computer’s memory (RAM), it is a good practice to save it to a disk frequently so that we can restore the information in the event of a computer crash or power failure. The FIGURE 22.2 SAVE operation copies the database from memory to a file called the Solving Database (DB) File. database file (or db file for short). The easiest way to save is to click on: Toolbar > SAVE_DB Or use: Utility Menu > File > Save as Jobname.db Utility Menu > File > Save as… To restore the database from the db file back into memory, use the RESUME operation. Toolbar > RESUME_ DB (see Figure 22.2), or use: Utility Menu > File > Resume Jobname.db Utility Menu > File > Resume from… 22.3.6 Tips on SAVE and RESUME Periodically we need to save the database as we progress through an analysis. ANSYS 665 does not do automatic saves. We should definitely SAVE the database before attempting an unfamiliar operation (such as a Boolean or meshing) or an operation that may cause major changes (such as a delete). RESUME can then be used as an “undo” if we don’t like the results of that operation. SAVE is also recommended before doing a solver. 22.4 FINITE ELEMENT DISCRETIZATION Finite Element Discretization or Meshing is the process used to “fill” the solid model with nodes and elements, that is, to create the FEA model. Remember, we need nodes and elements for the finite element solution, not just the solid model. The Solid Model in CAD does not participate in the finite element solution. 22.4.1 Element Type The element type is an important choice that determines the following element characteristics: Degree of Freedom (dof ) set. A thermal element type, for example, has 1 dof: TEMP, whereas a structural element type may have up to 6 dof: UX, UY, UZ, ROTX, ROTY, ROTZ. Element shape—brick, tetrahedron, quadrilateral, triangle, and so on Dimensionality—2D solid (X-Y plane only), or 3D solid Assumed displacement shape—linear versus quadratic 22.4.2 To Define an Element Main Menu > Preprocessor > Element Type > Add/Edit/Delete > Add  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis 22.4.3 Meshing Methods FIGURE 22.3 Specification of Element Type. FREE AND MAPPED MESHING METHODS Free Mesh Has no element shape restrictions. The mesh does not follow any pattern. Suitable for complex shaped areas and volumes. Volume meshes consist of high-order tetrahedral (10 nodes), and a large number of degrees of freedom. Mapped Mesh Restricts element shapes to quadrilaterals (areas) and hexahedra (volume). 666 Typically has a regular pattern with obvious rows of elements. Suitable only for “regular” shapes such as rectangles and bricks. 22.4.4 Mesh Density Control ANSYS provides many tools to control mesh density, on a global and local level: Global controls: SmartSizing; Global element sizing; Default sizing 6 Local controls: Keypoint sizing; Line sizing; Area sizing To Access the MeshTool: Main Menu > Preprocessor > Meshing > MeshTool. SmartSizing: Turn on SmartSizing, and set the desired size level. Size level ranges from 1 (fine) to 10 (coarse), defaults to 6. Then mesh all volumes (or all areas) at once, rather than one by one. Advanced SmartSize controls, such as mesh expansion and transition factors, are available via Main Menu > Preprocessor > Meshing > Size Cntrls > SmartSize > Adv Opts. Global Element Sizing: Allows you to specify a maximum element edge length for the entire model (or number of divisions per line): Go to Size Controls, Global, and click [Set] or Main Menu > Preprocessor > Meshing > Size Cntrls > ManualSize > Global > Size. 22.4.5 Material Properties Every analysis requires material property input: Young’s modulus (EX), Poisson’s ratio (PRXY) for structural elements, thermal conductivity (KXX) for thermal elements, and so on. To define the material properties: Main Menu > Preprocessor > Material Props > Material Models. More than one set of material properties can be defined when needed.  CHAPTER 22 Finite Element Analysis Using ANSYS FIGURE 22.4 Specification of Material Properties. 22.5 SYSTEM OF UNITS The ANSYS program does not assume a system of units for the analysis (except in magnetic field analyses). We can use any system of units so long as we make sure that we use that system for all the data we enter (units must be consistent for all input data). It is suggested to use SI system whenever possible to avoid confusion. 1. ANSYS had no built-in unit system. 2. The units must be consistent as indicated below. Quantity SI SI (mm) US Unit (ft) US Unit (inch) 667 Length m mm ft in Force N N lbf lbf Mass kg tonne (103 kg) slug lbf S2/in Time s s s s Stress Pa (N/m2) MPa (N/mm2) lbf/ft2 psi (lbf/in2) Energy J MJ (10−3 J) ft lbf in lbf Density kg/m3 tonne/mm3 slug/ft3 lbf s2/in4 22.6 STAGES IN SOLUTION ANSYS is a general-purpose finite element modeling package for numerically solving a wide variety of mechanical problems. These problems include static/dynamic structural analysis (both linear and nonlinear), heat transfer and fluid problems, as well as acoustic and electromagnetic problems. In general, a finite element solution may be broken into the following three stages. This is a general guideline that can be used for setting up any finite element analysis. PREPROCESSING Preprocessing consists of defining the problem; major steps follow: Define keypoints/lines/areas/volumes. Define element type and material/geometric properties. Define Mesh lines/areas/volumes as required. The amount of detail required will depend on the dimensionality of the analysis (i.e., 1D, 2D, axisymmetric, 3D).  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis SOLUTION The solution stage comprises assigning loads, constraints, and solving. Specify the loads (point or pressure). Specify the constraints (translational and rotational). Solve the resulting set of equations. POSTPROCESSING This stage includes additional processing and viewing of the results, such as the following: Lists of nodal displacements Element forces and moments Deflection plots Stress contour diagrams EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS ANSYS 7.0 is used to solve the following 2D Truss problem. Problem Description Determine the nodal deflections, reaction forces, and stresses for the truss shown in Figure 22.5. (E = 200 GPa, A = 3250 mm2) 2 4 4 8 6 3 11 668 280 kN 210 kN 280 kN 360 kN 3.118 m 1 5 7 9 60° 2 60° 6 10 R 1 3 5 7 3.6 m 3.6 m 3.6 m FIGURE 22.5 Two Dimensional Truss. Preprocessing: Defining the Problem 1. Input a Title (such as Bridge Truss Tutorial). In the Utility menu bar select File > Change Title: The following window will appear: FIGURE 22.6 Giving a Title to the Problem. Enter the title and click OK. This title will appear in the bottom left corner of the Graphics window once we begin. Note: to get the title to appear immediately, select Utility Menu > Plot > Replot. 2. Enter Keypoints. The overall geometry is defined in ANSYS using keypoints, which specify various principal coordinates to define the body. For this example, these keypoints are the ends of each truss.  CHAPTER 22 Finite Element Analysis Using ANSYS ❍ We define seven keypoints for the simplified structure as given in the following table: Coordinate Keypoint x y 1 0 0 2 1800 3118 3 3600 0 4 5400 3118 5 7200 0 6 9000 3118 7 10,800 0 ❍ These keypoints are depicted as node numbers in Figure 22.5. ❍ From the ANSYS Main Menu select: Preprocessor > Modeling > Create > Keypoints > In Active CS The following window will then appear: 669 FIGURE 22.7 Specifying Coordinates of Keypoint (Node) 1. ❍ To define the first keypoint, which has the coordinates x = 0 and y = 0, enter keypoint number 1 in the appropriate box, and enter the x,y coordinates 0, 0 in their appropriate boxes (as shown in Figure 22.7). Click Apply to accept what we have typed. ❍ Enter the remaining keypoints using the same method. Note When entering the final data point, click on OK to indicate that we are finished entering keypoints. If we first press Apply and then OK for the final keypoint, we will have defined it twice! If we did press Apply for the final point, simply press Cancel to close this dialog box. Units Note the units of measure (i.e., mm) were not specified. It is the responsibility of the user to ensure that a consistent set of units is used for the problem; make conversions where necessary. Correcting Mistakes When defining keypoints, lines, areas, volumes, elements, constraints, and loads we are bound to make mistakes. Fortunately these are easily corrected so that we don’t need to begin from scratch every time an error is made! Every Create menu for generating these various entities also has a corresponding Delete menu for fixing things. 3. Form Lines The keypoints must now be connected. We will use the mouse to select the keypoints to form the lines. ❍ In the main menu select: Preprocessor > Modeling > Create > Lines > Lines > In Active Coord. ❍ Use the mouse to pick keypoint #1 (i.e., click on it). It will now be marked by a small yellow box. (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS (Continued ) ❍ Now move the mouse toward keypoint #2. A line will now show up on the screen joining these two points. Left click and a permanent line will appear. ❍ Connect the remaining keypoints using the same method. ❍ When you are done, click on OK in the Lines in Active Coord window, minimize the Lines menu and the Create menu. Your ANSYS Graphics window should look similar to Figure 22.8. 670 FIGURE 22.8 Connecting Lines between Keypoints (Nodes). Disappearing Lines Please note that any lines we have created may disappear throughout our analysis. However, they have most likely not been deleted. If this occurs at any time, from the Utility Menu select: Plot > Lines 4. Define the Type of Element It is now necessary to create elements. This is called meshing. ANSYS first needs to know what kind of elements to use: ❍ From the Preprocessor Menu, select: Element Type > Add/Edit/Delete. ❍ Click on the Add… button. The following window (Figure 22.9) will appear: FIGURE 22.9 Window for Library of Element Types.  CHAPTER 22 Finite Element Analysis Using ANSYS ❍ For this example, we will use the 2D spar element as selected in the above figure. Select the element shown and click OK. We should see Type 1 LINK1 in the Element Types window. ❍ Click on Close in the Element Types dialog box. 5. Define Geometric Properties We now need to specify geometric properties for our elements: ❍ In the Preprocessor menu, select Real Constants > Add/Edit/Delete. ❍ Click Add… and select Type 1 LINK1 (actually it is already selected). Click on OK. The following window (Figure 22.17) will appear: FIGURE 22.10 Specification of Area of Cross-section of Members. ❍ As shown in the window, enter the cross-sectional area (3250 mm). ❍ Click on OK. ❍ Set 1 now appears in the dialog box. Click on Close in the Real Constants window. 6. Element Material Properties 671 We then need to specify material properties, in the Preprocessor menu select Material Props > Material Models. Double-click on Structural > Linear > Elastic > Isotropic. FIGURE 22.11 Specification of Value of Young’s Modulus. We are going to give the properties of Steel. Enter the following field: EX 200000 ❍ Set these properties and click on OK. (Note: We may obtain the note PRXY will be set to 0.0. This is Poisson’s ratio and is not required for this element type. Click OK on the window to continue. Close Define Material Model Behavior by clicking on the X box in the upper right corner. (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS (Continued ) 7. Mesh Size The last step before meshing is to tell ANSYS what size the elements should be. There are a variety of ways to do this but we will deal with just one method for now. ❍ In the Preprocessor menu, select Meshing > Size Cntrls > ManualSize > Lines > All Lines. ❍ In the size NDIV field, enter the desired number of divisions per line. For this example we want only 1 division per line, therefore, enter 1 and then click OK. Note that we have not yet meshed the geometry; we have simply defined the element sizes. 8. Mesh Now the frame can be meshed. ❍ In the Preprocessor menu, select Meshing > Mesh > Lines and click Pick All in the Mesh Lines Window. Your model should now appear similar to the one shown in Figure 22.8. Plot Numbering To show the line numbers, keypoint numbers, node numbers: From the Utility Menu (top of screen) select PlotCtrls > Numbering… Fill in the window as shown in Figure 22.12 and click OK. 672 FIGURE 22.12 Showing Line and Keypoint (Node) Numbers. Now we can turn numbering on or off at our discretion Saving Our Work Save the model at this time, so that if we make some mistakes later on, we will at least be able to come back to this point. To do this, on the Utility Menu select File > Save as…. Select the name and location where we want to save your file. It is a good idea to save your job at different times throughout the building and analysis of the model to backup your work in case of a system crash. Solution Phase: Assigning Loads and Solving We have now defined our model. It is time to apply the load(s) and constraint(s) and solve the resulting system of equations.  CHAPTER 22 Finite Element Analysis Using ANSYS Open up the Solution menu (from the same ANSYS Main Menu). 1. Define Analysis Type First we must tell ANSYS how we want it to solve this problem: ❍ From the Solution Menu, select Analysis Type > New Analysis. ❍ Ensure that Static is selected; that is, we are going to do a static analysis on the truss as opposed to a dynamic analysis, for example. ❍ Click OK. 2. Apply Constraints It is necessary to apply constraints to the model; otherwise the model is not tied down or grounded and a singular solution will result. In mechanical structures, these constraints will typically be fixed, pinned and roller-type connections. As shown above, the left end of the truss bridge is pinned while the right end has a roller connection. ❍ In the Solution menu, select Define Loads > Apply > Structural > Displacement > On Keypoints. ❍ Select the left end of the bridge (Keypoint 1) by clicking on it in the Graphics Window and click on OK in the Apply U,ROT on KPs window. 673 FIGURE 22.13 Specifying UX and UY as Displacement dof at Key Points (Nodes). ❍ This location is fixed, which means that all translational and rotational degrees of freedom (dofs) are constrained. Therefore, select All DOF by clicking on it and enter 0 in the Value field and click OK. We will see some blue triangles in the graphics window indicating the displacement constraints. ❍ Using the same method, apply the roller connection to the right end (UY constrained). Note that more than one dof constraint can be selected at a time in the Apply U,ROT on KPs window. Therefore, we may need to deselect the All DOF option to select just the UY option. 3. Apply Loads As shown in the diagram, there are four downward loads of 280 kN, 210 kN, 280 kN, and 360 kN at keypoints 1, 3, 5, and 7, respectively. ❍ Select Define Loads > Apply > Structural > Force/Moment > on Keypoints. ❍ Select the first Keypoint (left end of the truss) and click OK in the Apply F/M on KPs window. ❍ Select FY in the Direction of force/mom. This indicates that we will be applying the load in the y direction ❍ Enter a value of –280,000 in the Force/moment value box and click OK. Note that we are using units of N here, which is consistent with the previous values input. ❍ The force will appear in the graphics window as a red arrow. ❍ Apply the remaining loads in the same manner. (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS (Continued ) FIGURE 22.14 Specifying the Values of Loads at Nodes. The applied loads and constraints should now appear as shown in Figure 22.15. 674 FIGURE 22.15 Display of Loads and Constraints. 4. Solving the System We now tell ANSYS to find the solution: ❍ In the Solution menu select Solve > Current LS. This indicates that we desire the solution under the current Load Step (LS). ❍ The windows in Figure 22.16 will appear. Ensure that our solution options are the same as shown above and click OK. ❍ Once the solution is done, a window will pop up displaying “Solution is done”.  CHAPTER 22 Finite Element Analysis Using ANSYS FIGURE 22.16 Display of Solution Options. Postprocessing: Viewing the Results 1. Hand Calculations We will first calculate the forces and stress in element 1 (as labeled in the problem description). ∑M1 = 0 = :210 kNð3:6 mÞ − 280 kNð7:2 mÞ − 360 kNð10:8 mÞ + F7 ð10:8 mÞ 210 kNð3:6 mÞ + 280 kNð7:2 mÞ + 360 kNð10:8 mÞ F7 = = 617 kN 10:8 m "∑Fy = 0 = − 280 kN − 210 kN − 280 kN − 360 kN + 617 kN + F1 F1 = 280 kN + 210 kN + 280 kN + 360 kN − 617 kN = 513 kN 675 Element 1 Forces/Stress 513 kN − 280 kN FE1 = = 269 kN cosð30Þ FE1 σ E1 = = 269 kN 2 = 82:8 MPa A 3250 mm 2. Results Using ANSYS Reaction Forces A list of the resulting reaction forces can be obtained for this element From the Main Menu, select General Postproc > List Results > Reaction Solu. Select All struc forc F and click OK. FIGURE 22.17 Display of Reaction Forces. These values agree with the reaction forces calculated by hand above. (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS (Continued ) Deformation In the General Postproc menu, select Plot Results > Deformed Shape. Select Def + undef edge and click OK to view both the undeformed and the deformed object. FIGURE 22.18 Display of Undeformed System. 676 Observe the value of the maximum deflection in the upper left corner (DMX = 7.409). One should also observe that the constrained degrees of freedom appear to have a deflection of 0 (as expected!). Deflection For a more detailed version of the deflection of the beam: From the General Postproc menu select Plot results > Contour Plot > Nodal Solution. Select DOF solution and USUM in the display window. Leave the other selections as the default values. Click OK. FIGURE 22.19 Display of Deformed System.  CHAPTER 22 Finite Element Analysis Using ANSYS The deflection can also be obtained as a list as shown below. General Postproc > List Results > Nodal Solution select DOF Solution and ALL DOFs from the lists in the List Nodal Solution window and click OK. This means that we want to see a listing of all degrees of freedom from the solution. FIGURE 22.20 Window with Nodal Displacements. Are these results what we expected? Note that all the degrees of freedom were constrained to zero at node 1, while UY was constrained to zero at node 7. If we want to save these results to a file, select File within the results window (at the upper left corner of this list window) and select Save as. Axial Stress For line elements (i.e., links, beams, spars, and pipes), you will often need to use the Element Table to gain access to derived data (i.e., stresses, strains). For this example, we should obtain axial stress to compare with the hand calculations. From the General Postprocessor menu select Element Table > Define Table. Click on Add… 677 Enter SAXL in the Lab box. This specifies the name of the item that we are defining. Next, in the Item, Comp boxes, select By sequence number and LS. Then enter 1 after LS in the selection box. Click on OK and close the Element Table Data window. Plot the Stresses by selecting Element Table > Plot Elem Table. A window will appear. Ensure that SAXL is selected and click OK. Because we changed the contour intervals for the Displacement plot to User Specified, we need to switch this back to Auto Calculated to obtain new values for VMIN/VMAX. Utility Menu > PlotCtrls > Style > Contours > Uniform Contours … FIGURE 22.21 Display of Stresses (Contours). (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.1: ANALYSIS OF A TWO-DIMENSIONAL TRUSS (Continued ) Again, we may wish to select more appropriate intervals for the contour plot. List the Stresses From the Element Table menu, select List Elem Table. From the List Element Table Data window which appears, ensure that SAXL is highlighted. Click OK. FIGURE 22.22 678 Table of Element Stresses. EXAMPLE 22.2: HEAT TRANSFER IN A STEEL ROD (LINK) 75 °C FIGURE 22.23 Heat Transfer in a Steel Rod (Link). A steel link, with no internal stresses, is pinned between two solid structures at a reference temperature of 0°C (273 K). One of the solid structures is heated to a temperature of 75°C (348 K). As heat is transferred from the solid structure into the link, the link will attempt to expand. However, since it is pinned, this cannot occur, and as such, stress is created in the link. A steady-state solution of the resulting stress will be found to simplify the analysis. Loads will not be applied to the link, only a temperature change of 75°C. The link is steel with a modulus of elasticity of 200 GPa, a thermal conductivity of 60.5 W/m*K, and a thermal expansion coefficient of 12e-6/K. As in the case of Example 22.1, the following steps are used in the solution process: Preprocessing: Construct geometry by defining key points and lines, Specify element type and element constants, Specify the material, Generate the mesh, Apply the boundary conditions. Solution: Solve with current LS (load step), Display solution. Postprocessing: Plot the solution, List the nodal/element solution.  CHAPTER 22 Finite Element Analysis Using ANSYS FIGURE 22.24 Begin to Solve with Current Load Step. 679 FIGURE 22.25 Completion of Solution. (Continued )  PART 7 ABAQUS and ANSYS Software and MATLAB®Programs for Finite Element Analysis EXAMPLE 22.2: HEAT TRANSFER IN A STEEL ROD (LINK) (Continued ) 680 FIGURE 22.26 Listing of Thermal Stresses in Elements. FIGURE 22.27 Display of Defomation Shape.  CHAPTER 22 Finite Element Analysis Using ANSYS Comparison Expansion due to thermal stress in a link can be calculated using: δ = αΔTL Expansion due to structural forces can be determined using: δ = PL EA Solving for the structural forces due to the thermal expansion, P = αΔTEA or F σ= = αΔTE A Therefore, in this example, σ = ð0:000012/kÞð348 K − 273 KÞ ð200e3 MPaÞ = 180 MPa PROBLEMS Find the deflections and stresses in the beams described in the following problems using the finite element method with the following data: P = 1000 N, L = 1 m, E = 70 × 109 Pa, M0 = 50,000 N-cm, cross-section of the beam: rectangular with depth 2 cm and width (perpendicular to the page) 1 cm. Use ANSYS for solving the problems. 22.1 A uniform cantilever beam of length L subject to a concentrated transverse load P at the free end as shown in 681 Figure 1.20. 22.2 A uniform cantilever beam of length L subject to a concentrated bending moment M0 at the free end as shown in Figure 1.21. 22.3 A uniform fixed-simply supported beam of length L subject to a concentrated transverse load P at the middle as shown in Figure 1.22. 22.4 A uniform fixed-simply supported beam of length L subject to a concentrated bending moment M0 at the middle as shown in Figure 1.23. 22.5 A uniform fixed-fixed beam of length L subject to a concentrated transverse load P at a distance of (3 L/4) from the left end as shown in Figure 1.24.