Problem: Using Castigliano's Theorem, determine the deflection at point A. Neglect the weight of the beam. W 1 N/m B 5 cm H 1 cm 1.35 m
Overview Anticipated time to complete this tutorial: 45 minutes Tutorial Overview This tutorial is divided into six parts: 1) Tutorial Basics ) Starting Ansys 3) Preprocessing 4) Solution 5) Post-Processing 6) Hand Calculations Audience This tutorial assumes minimal knowledge of ANSYS 8.; therefore, it goes into moderate detail to explain each step. More advanced ANSYS 8. users should be able to complete this tutorial fairly quickly. Prerequisites 1) ANSYS 8. in house Structural Tutorial Objectives 1) earn how to define keypoints, lines, and elements ) earn how to apply structural constraints and loads 3) Use parameters in the modeling process 4) earn how to find and interpret nodal solutions Outcomes 1) earn how to start Ansys 8. ) Gain familiarity with the graphical user interface (GUI) 3) earn how to create and mesh a simple geometry 4) earn how to apply boundary constraints and solve problems
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 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
Starting Ansys For this tutorial the windows version of ANSYS 8. will be demonstrated. The path below is one example of how to access ANSYS; however, this path will not be the same on all computers. For Windows XP start ANSYS by either using: > Start > All Programs > ANSYS 8. > ANSYS or the desktop icon (right) if present. Note: The path to start ANSYS 8. may be different for each computer. Check with your local network manager to find out how to start ANSYS 8.. 4
Starting Ansys Once ANSYS 8. is loaded, two separate windows appear: the main ANSYS Advanced Utility Window and the ANSYS Output Window. The ANSYS Advanced Utility Window, also known as the Graphical User Interface (GUI), is the location where all the user interface takes place. Graphical User Interface Output Window The Output Window documents all actions taken, displays errors, and solver status. 5
Starting Ansys The main utility window can be broken up into three areas. A short explanation of each will be given. First is the Utility Toolbar: From this toolbar you can use the command line approach to ANSYS and access multiple menus that you can t get to from the main menu. Note: It would be beneficial to take some time and explore these pull down menus and familiarize yourself with them. Second is the ANSYS Main Menu as shown to the right. This menu is designed to use a top down approach and contains all the steps and options necessary to properly preprocess, solve, and postprocess a model. Third is the Graphical Interface window where all geometry, boundary conditions, and results are displayed. The tool bar located on the right hand side has all the visual orientation tools that are needed to manipulate your model. 6
Starting Ansys With ANSYS 8. open select > File > Change Jobname and enter a new job name in the blank field of the change jobname window. Enter the problem title for this tutorial. > OK In order to know where all the output files from ANSYS will be placed, the working directory must be set in order to avoid using the default folder: C:\Documents and Settings. File > Change Directory > then select the location that you want all of the ANSYS files to be saved. Be sure to change the working directory at the beginning of every problem. With the jobname and directory set, the ANSYS database (.db) file can be given a title. Following the same steps as you did to change the jobname and the directory, give the model a title. 7
Preprocessing To begin the analysis, a preference needs to be set. Preferences allow you to apply filtering to the menu choices; Ansys will remove or gray out functions that are not needed. A structural analysis, for example, will not need all the options available for a thermal, electromagnetic, or fluid dynamic analysis. > Main Menu > Preferences Place a check mark next to the Structural box. >Ok ook at the ANSYS Main Menu. Click once on the + sign next to Preprocessor. > Main Menu > Preprocessor The Preprocessor options currently available are displayed in the expansion of the Main Menu tree as shown to the right. The most important preprocessing functions are defining the element type, defining real constants, material properties, and modeling and meshing the geometry. 8
Preprocessing For this problem, you will use parameters to assign numerical values to the constants w, b, h, l, and E. You will then use these constants to set up the problem. Note: Although ANSYS refers to these constants as parameters, they do not automatically update themselves. For example: Suppose you define h and then define the x- component of a keypoint as.5*h. The x-component of the keypoint value is set to 1 (i.e..5* 1). If you then change the value of h to equal 4, the previously defined x component of the keypoint DOES NOT change to. Parameters are most useful if you have to use a repeated value while creating your model. To define a parameter, go to the Utility Menu and select > Parameters > Scalar Parameters In the selection box, enter the parameter, followed by, followed by the value of the parameter. To transfer the entry to the Items box, click Accept. Enter the following parameters: W 1 B.5 H.1 1.35 E 7e9 > Close Note: Make sure that all of your entries are dimensionally consistent (i.e. don t enter values with both cm and m, or m and lbs, etc). Select one unit system before you begin the problem and be consistent throughout. 9
Preprocessing The ANSYS Main Menu is designed in such a way that you should start at the beginning and work towards the bottom of the menu in preparing, solving, and analyzing your model. Note: This procedure will be shown throughout the tutorial. Select the + next to Element Type or click on Element Type. The extension of the menu is shown to the right. > Element Type Select Add/Edit/Delete and the Element type window appears. Select add and the ibrary of Element Types window appears. > Add/Edit/Delete > Add In this window, select the types of elements to be defined and used for the problem. For a pictorial description of what each element can be used for, click on the Help button. For this model D Elastic Beam elements will be used. The degrees of freedom for this type of element are UX, UY, and ROTZ, which will suit the needs of this problem. > Beam > D Elastic 3 > OK In the Element Types window Type 1 Beam3 should be visible signaling that the element type has been chosen. Close the Element Types window. > Close 1
Preprocessing The properties for the Beam3 element need to be chosen. This is done by adding a Real Constant. > Preprocessor > Real Constants > Add/Edit/Delete The Real Constants window should appear. Select add to create a new set. > Add The Element Type for Real Constants window should appear. From this window, select Beam 3 as the element type. > Type 1 Beam3 > OK The Real Constant Set for Beam3 window will appear. From this window you can interactively customize the element type. Use the parameters to fill in blanks for the cross-sectional area, area moment of inertia, and total beam height. Enter the values into the table as shown at the right. > OK Close the Real Constants window. > Close 11
Preprocessing The material properties for the Beam3 element need to be defined. > Preprocessor > Material Props > Material Models The Define Material Models Behavior window should now be open. This window has many different possibilities for defining the materials for your model. We will use isotropic linearly elastic structural properties. Select the following from the Material Models Available window: > Structural > inear > Elastic > Isotropic The window titled inear Isotropic Properties for Material Number 1 now appears. This window is the entry point for the material properties to be used for the model. Enter the parameter E for EX (Young's Modulus) and.3 for PRXY (Poisson's Ratio). > OK Close the Define Material Model Behavior window. > Material > Exit 1
Preprocessing The next step is to define the keypoints (KP s) that will help you build the rest of your model: > Preprocessing > Modeling > Create > Keypoints > In Active CS The Create Keypoints in Active CS window will now appear. Here the KP s will be given numbers and their respective (XYZ) coordinates. Enter the KP numbers and coordinates that define the beam. Select Apply after each KP has been defined. Note: Be sure to change the keypoint number every time you click apply to finish adding a keypoint. If you don t it will replace the last keypoint you entered with the new coordinates you just entered. KP # 1: X, Y, Z KP # : X.5*, Y, Z KP # 3: X.7*, Y, Z KP # 4: X, Y, Z Select OK when complete. If a mistake was made in creating the keypoints, select: > Preprocessing > Modeling > Delete > Keypoints Select the incorrect KP s and select OK. Your screen should look similar to the example below. 13
Preprocessing At times it will be helpful to turn on the keypoint numbers. > PlotCtrls > Numbering Put a checkmark next to keypoint numbers > OK Other numbers (for lines, areas, etc..) can be turned on in a similar manner. At times it will also be helpful to have a list of keypoints (or nodes, lines, elements, loads, etc.). To generate a list of keypoints: > ist > Keypoint > Coordinates Only A list similar to the one to the right should appear. Note that the x-coordinates for the keypoints are now listed as values (,.3375,.945, 1.35), not (,.5*,.7*, and ). 14
The next step is to create lines between the KP s. > Preprocessing > Modeling > Create > ines > ines > Straight ines Preprocessing The Create Straight ines window should appear. You will create 3 lines. Create line 1 between the first two keypoints. For line 1: MB1 KP1 then MB1 KP. The other lines will be created in a similar manner. For line : MB1 KP then MB1 KP 3. For line 3: MB1 KP3 then MB1 KP 4. Verify that each line only goes between the specified keypoints. When you are done creating the lines click ok in the Create Straight ines window. > OK If you make a mistake, do the following to delete the lines: > Preprocessing > Modeling > Delete > ines Only You should now have something similar to the image shown below. 15
Preprocessing Now that the model has been created, it needs to be meshed. Only meshed models can be used to find a solution. Models are meshed with elements. First, the element size will be specified. > Preprocessing > Meshing > Size Cntrls > Manual Size > ines > All ines The Element Sizes on All Selected ines window should appear. From this window the number of elements per lines segment can be defined along with the Element edge length. Enter 1 into the Number of element divisions field. > OK Note: you could change the element edge length after completing the tutorial to a different value and rerun the solution to see how it affects the results. With the mesh parameters complete, the lines representing the beam can now be meshed. Select: > Preprocessing > Meshing > Mesh > ines From the Mesh ines window select Pick All. > Pick all This will select all the line segments and simultaneously mesh them. The meshed line should appear similar as shown below. This completes the preprocessing phase. 16
You will now move into the solution phase. Solution Before applying the loads and constraints to the beam, we will select to start a new analysis: > Solution > Analysis Type > New Analysis For the type of analysis select Static and select OK. The constraints will now be added. For this problem, the left end of the beam is constrained from moving in the X and Y directions and from rotating about the Z axis. There is an additional constraint restricting motion in the Y direction at keypoint 3. To apply constraints select: > Solution > Define oads > Apply > Structural > Displacement > On Keypoints The Apply U, ROT on KP s window now appears. It will be easier to select the keypoints if the keypoint numbers are turned on as previously explained. However, the current view probably shows just the elements and not the keypoints. You can see both the elements and the keypoints on the screen by selecting: > Plot > Multiplots To see just the keypoints; Plot > Keypoints > Keypoints Use the plot menu to view your model in a way most helpful to completing each step in this tutorial. 17
With the Apply U, ROT on KP s window open select KP 1 from the ANSYS graphics window. > Apply The Apply U, ROT on KP s large window should appear. From this window the degrees of freedom can be specified. To the right of DOFs to be constrained select All DOF. > Apply. The constraints now appear at the location of keypoint 1. Now select KP 3. > Apply Solution The Apply U, ROT on KP s large window should reappear. Unselect All DOF by using MB1 and then select UY. > OK The beam is now correctly constrained. The constrained model should appear similar to the image below. 18
Solution The loads will now be applied to the beam. > Solutions > Define oads > Apply > Structural > Pressure > On Beams The Apply Pres on KP s window should appear. Select all the elements between keypoints and 4 (there should be in all). > Apply The expanded Apply Pressure on Beams window should appear. From this window the direction of the pressure and its magnitude can be specified. Enter w in the Pressure at Node I value field which will apply the pressure over the beam from keypoints to 4. A positive entry in this field is defined as a downward pressure. Verify that all the fields match those of the figure shown to the right. >OK The fully loaded and constrained model should appear similar to the picture shown below. 19
If you wish to view a 3D picture of your model select > Plot Controls > Style > Size and Shape Solution The Size and Shape window opens. Click the check box next to Display of element to turn on the 3D image. Now when you rotate your model using CTR + MB, the model should appear to be 3D. You should see something similar to the image below. You are now ready to solve the model.
Solution The next step is to solve the current load step that has been created. Select: Solution > Solve > Current S The Solve Current oad Step window will appear. To begin the analysis select OK. The analysis should begin. When it is complete a Note window should appear that states that the solution is done. Close both the Note window and /STATUS Command window. 1
Results are viewed by using post processing commands. Post Processing You are interested in knowing the vertical displacement at point A, a distance of.3375 m away from the origin. Ansys has automatically created a node at this location; you need to figure out which node number has been assigned to the location. On the Utility Tool Bar select > ist > Nodes The Sort Node isting window should appear. Select the Output listing to contain coordinates only and sort first by the X Coordinate. Your window should appear similar to the window at the right. > Ok The NIST window should appear with a listing of all the nodes sorted by the X coordinate. Find the node that has the X coordinate of.3375. In this case, it is node.
Post Processing You can now inquire about the nodal displacement in the Y direction at node. On the Ansys Main Menu select > General Postproc > ist Results > Nodal Solution The ist Nodal Solution window should appear. Select DOF solution, Translation UY. > Ok The PRNSO window should appear. This window shows the Y displacements for each node in the model. You are interested in the Y displacement at node : -.1668e- m or 1.67 mm in the negative Y direction. 3
Post Processing You may also be interested in the overall deflection shape of the beam. One way to do this is through the Results Viewer. On the Ansys Main Menu select > General Postproc > Results Viewer This opens up the Results Viewer interface. On the Results Viewer toolbar, select > Nodal Solution > DOF Solution > Y-Component of displacement Click the contour plot button on the Results Viewer toolbar and observe the nodal solution plot. 4
Using Castigliano s Theorem: Solve for the reaction force, Rb. Hand Calculations Cutting the beam at the appropriate locations: x Mpt Wx Wx Mpt Mpt Rb 1 EI Mpt.3 Wx () dx Mpt x Mpt + Rb( x.3) Wx Wx Mpt Rb( x.3) Mpt ( x.3) Rb.75 1 Wx Rb( x.3) EI.3 [ ( x.3 ] dx 5
Hand Calculations Mpt Mpt + Rb( x.3).75w ( x.375) Mpt.75W ( x.375) Rb( x.3) Mpt Rb 1 EI y Rb ( x.3) [.75W ( x.375) Rb( x.3) ][ ( x.3 ].75.75 1 Wx Rb( x.3) EI.3.75 Rb.6444W Ra.356W dx [ ( x.3] dx + [.75W ( x.375) Rb( x.3) ][ ( x.3] dx Solving for the imaginary force at Q: 6
Hand Calculations 7 1.3 dx EI Q Mpt Wx Mpt x Wx Mpt Mpt + dx EI Q Mpt x W Wx Mpt x W Wx Mpt Mpt.75.3 1 ).3 (.644 ).3 (.644
Hand Calculations 8 [ ][ ] EI W e y dx x W x W x EI y x Q Mpt x Q x W x W Mpt x Q x W x W Mpt Mpt i i 4 4.75 *1.85.3 (.644 ).375 (.75.75 1.75) (.7) ( ).375 (.75 ).3 (.644.7) ( ).375 (.75 ).3 (.644 + + +