ANSYS Tutorial Overview for Mechanical Engineering

UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta University of Alberta ANSYS Tutorials ANSYS is a general purpose finite element modeling package for numerically solving a wide variety of mechanical problems These problems include staticdynamic structural analysis both linear and nonlinear heat transfer and fluid problems as well as acoustic and electromagnetic problems Most of these tutorials have been created using ANSYS 70 therefore make note of small changes in the menu structure if you are using an older or newer version This web site has been organized into the following six sections I ANSYS Utilities An introduction to using ANSYS This includes a quick explanation of the stages of analysis how to start ANSYS the use of the windows in ANSYS convergence testing savingrestoring jobs and working with ProE I Basic Tutorials Detailed tutorials outlining basic structural analysis using ANSYS It is recommended that you complete these tutorials in order as each tutorial builds upon skills taught in previous examples I Intermediate Tutorials Complex skills such as dynamic analysis and nonlinearities are explored in this section It is recommended that you have completed the Basic Tutorials prior to attempting these tutorials I Advanced Tutorials Advanced skills such as substructuring and optimization are explored in this section It is recommended that you have completed the Basic Tutorials prior to attempting these tutorials I Postprocessing Tutorials Postprocessing tools available in ANSYS such as Xsectional views of the geometry are shown in this section It is recommended that you have completed the Basic Tutorials prior to attempting these tutorials I Command Line Files Example problems solved using command line coding only in addition to several files to help you to generate your own command line files UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc ANSYS Utilities An introduction to using ANSYS including a quick explanation of the stages of analysis how to start ANSYS and the use of the windows in ANSYS and using ProENGINEER with ANSYS G Introduction to Finite Element Analysis A brief introduction of the 3 stages involved in finite element analysis G Starting up ANSYS How to start ANSYS using windows NT and Unix XWindows G ANSYS Environment An introduction to the windows used in ANSYS G ANSYS Interface An explanation of the Graphic User Interface GUI in comparison to the command file approach G Convergence Testing This file can help you to determine how small your meshing elements need to be before you can trust the solution G SavingRestoring Jobs Description of how to save your work in ANSYS and how to resume a previously saved job G ANSYS Files Definitions of the different files created by ANSYS G Printing Results Saving data and figures generated in ANSYS G Working with Pro Engineer A description of how to export geometry from ProE into ANSYS Copyright 2001 University of Alberta UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Two Dimensional Truss Bicycle Space Frame Plane Stress Bracket Modeling Tools Solid Modeling Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Basic Tutorials The following documents will lead you through several example problems using ANSYS ANSYS 70 was used to create some of these tutorials while ANSYS 571 was used to create others therefore if you are using a different version of ANSYS make note of changes in the menu structure Complete these tutorials in order as each tutorial will build on skills taught in the previous example G Two Dimensional Truss Basic functions will be shown in detail to provide you with a general knowledge of how to use ANSYS This tutorial should take approximately an hour and a half to complete G Bicycle Space Frame Intermediate ANSYS functions will be shown in detail to provide you with a more general understanding of how to use ANSYS This tutorial should take approximately an hour and a half to complete G Plane Stress Bracket Boolean operations plane stress and uniform pressure loading will be introduced in the creation and analysis of this 2Dimensional object G Solid Modeling This tutorial will introduce techniques such as filleting extrusion copying and working plane orienation to create 3Dimensional objects UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering Intermediate Tutorials The majority of these examples are simple verification problems to show you how to use the intermediate techniques in ANSYS You may be using a different version of ANSYS than what was used to create these tutorials therefore make note of small changes in the menu structure These tutorials can be completed in any order however it is expected that you have completed the Basic Tutorials before attempting these G Effect of Self Weight Incorporating the weight of an object into the finite element analysis is shown in this simple cantilever beam example G Distributed Loading The application of distributed loads and the use of element tables to extract data is expalined in this tutorial G NonLinear Analysis A large moment is applied to the end of a cantilever beam to explore Geometric Nonlinear behaviour large deformations There is also an associated tutorial for an explanation of the Graphical Solution Tracking GST plot G Buckling In this tutorial both the Eigenvalue and Nonlinear methods are used to solve a simple buckling problem G NonLinear Materials The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model G Dynamic Analysis These tutorial explore the dynamic analyis capabilities of ANSYS Modal Harmonic and Transient Analyses are shown in detail G Thermal Examples Analysis of a pure conduction a mixed convectionconductioninsulated boundary condition example and a transient heat conduction analysis University of Alberta ANSYS Inc Copyright 2001 University of Alberta G Modelling Using Axisymmetry Utilizing axisymmetry to model a 3D structure in 2D to reduce computational time UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Advanced Tutorials The majority of these examples are simple verification problems to show you how to use the more advanced techniques in ANSYS You may be using a different version of ANSYS than what was used to create these tutorials therefore make note of small changes in the menu structure These tutorials can be completed in any order however it is expected that you have completed the Basic Tutorials G Springs and Joints The creation of models with multiple elements types will be explored in this tutorial Additionally elements COMBIN7 and COMBIN14 will be explained as well as the use of parameters to store data G Design Optimization The use of Design Optimization in ANSYS is used to solve for unknown parameters of a beam G Substructuring The use of Substructuring in ANSYS is used to solve a simple problem G Coupled StructuralThermal Analysis The use of ANSYS physics environments to solve a simple structuralthermal problem G Using PElements The stress distribution of a model is solved using pelements and compared to helements G Melting Using Element Death Using element death to model a volume melting G Contact Elements Model of two beams coming into contact with each other G ANSYS Parametric Design Language Design a truss using parametric variables Copyright 2001 University of Alberta UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES XSectional Results Advanced XSec Res Data Plotting Graphical Properties Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Postprocessing Tutorials These tutorials were created to show some of the tools available in ANSYS for postprocessing You may be using a different version of ANSYS than what was used to create these tutorials therefore make note of small changes in the menu structure These tutorials can be completed in any order however it is expected that you have completed the Basic Tutorials G Viewing Cross Sectional Results The method to view cross sectional results for a volume are shown in this tutorial G Advanced XSectional Results Using Paths to Post Process Results The purpose of this tutorial is to create and use paths to provide extra detail during post processing G Data Plotting Using Tables to Post Process Results The purpose of this tutorial is to outline the steps required to plot results using tables a special type of array G Changing Graphical Properties This tutorial outlines some of the basic graphical changes that can be made to the main screen and model UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Command Line Files The following files should help you to generate your own command line files G Creating Command Files Directions on generating and running command files G ANSYS Command File Programming Features This file shows some of the commonly used programming features in the ANSYS command file language known as ADPL ANSYS Parametric Design Language Prompting the user for parameters performing calculations with paramaters and control structures are illustrated The following files include some example problems that have been created using command line coding Basic Tutorials This set of command line codes are from the Basic Tutorial section Intermediate Tutorials This set of command line codes are from the Intermediate Tutorial section Advanced Tutorials This set of command line codes are from the Advanced Tutorial section PostProc Tutorials This set of command line codes are from the PostProc Tutorial section Radiation Analysis A simple radiation heat transfer between concentric cylinders Copyright 2001 University of Alberta UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Introduction ANSYS is a general purpose finite element modeling package for numerically solving a wide variety of mechanical problems These problems include staticdynamic 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 1 Preprocessing defining the problem the major steps in preprocessing are given below H Define keypointslinesareasvolumes H Define element type and materialgeometric properties H Mesh linesareasvolumes as required The amount of detail required will depend on the dimensionality of the analysis ie 1D 2D axisymmetric 3D 2 Solution assigning loads constraints and solving here we specify the loads point or pressure contraints translational and rotational and finally solve the resulting set of equations 3 Postprocessing further processing and viewing of the results in this stage one may wish to see H Lists of nodal displacements H Element forces and moments H Deflection plots H Stress contour diagrams UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Starting up ANSYS Starting up ANSYS Large File Sizes ANSYS can create rather large files when running and saving be sure that your local drive has space for it Getting the Program Started In the Mec E 33 lab there are two ways that you can start up ANSYS 1 Windows NT application 2 Unix XWindows application Windows NT Start Up Starting up ANSYS in Windows NT is simple G Start Menu G Programs G ANSYS 57 G Run Interactive Now Unix XWindows Start Up Starting the Unix version of ANSYS involves a few more steps G in the task bar at the bottom of the screen you should see something labeled XWin32 If you dont see this minimized program you can may want to reboot the computer as it automatically starts this application when booting G right click on this menu and selection Sessions and then select Mece G you will now be prompted to login to GPU do this 3029 G once the Xwindows emulator has started you will see an icon at the bottom of the screen that looks like a paper and pencil dont select this icon but rather click on the up arrow above it and select Terminal G a terminal command window will now start up G in that window type xansys57 G at the UNIX prompt and a small launcher menu will appear G select the Run Interactive Now menu item UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES ANSYS 571 PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS 70 Environment The ANSYS Environment for ANSYS 70 contains 2 windows the Main Window and an Output Window Note that this is somewhat different from the previous version of ANSYS which made use of 6 different windows 1 Main Window Within the Main Window are 5 divisions a Utility Menu The Utility Menu contains functions that are available throughout the ANSYS session such as file controls selections graphic controls and parameters b Input Lindow The Input Line shows program prompt messages and allows you to type in commands directly c Toolbar The Toolbar contains push buttons that execute commonly used ANSYS commands More push buttons can be added if desired d Main Menu The Main Menu contains the primary ANSYS functions organized by preprocessor solution general postprocessor design optimizer It is from this menu that the vast majority of modelling commands are issued This is where you will note the greatest change between previous versions of ANSYS and version 70 However while the versions appear different the menu structure has not changed e Graphics Window The Graphic Window is where graphics are shown and graphical picking can be made It is here where you will graphically view the model in its various stages of construction and the ensuing results from the analysis 2 Output Window The Output Window shows text output from the program such as listing of data etc It is usually positioned behind the main window and can de put to the front if necessary UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Interface Graphical Interface vs Command File Coding There are two methods to use ANSYS The first is by means of the graphical user interface or GUI This method follows the conventions of popular Windows and XWindows based programs The second is by means of command files The command file approach has a steeper learning curve for many but it has the advantage that an entire analysis can be described in a small text file typically in less than 50 lines of commands This approach enables easy model modifications and minimal file space requirements The tutorials in this website are designed to teach both the GUI and the command file approach however many of you will find the command file simple and more efficient to use once you have invested a small amount of time into learning the code For information and details on the full ANSYS command language consult Help Table of Contents Commands Manual UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta FEM Convergence Testing Introduction A fundamental premise of using the finite element procedure is that the body is subdivided up into small discrete regions known as finite elements These elements defined by nodes and interpolation functions Governing equations are written for each element and these elements are assembled into a global matrix Loads and constraints are applied and the solution is then determined The Problem The question that always arises is How small do I need to make the elements before I can trust the solution What to do about it In general there are no real firm answers on this It will be necessary to conduct convergence tests By this we mean that you begin with a mesh discretization and then observe and record the solution Now repeat the problem with a finer mesh ie more elements and then compare the results with the previous test If the results are nearly similar then the first mesh is probably good enough for that particular geometry loading and constraints If the results differ by a large amount however it will be necessary to try a finer mesh yet The Consequences Finer meshes come with a cost however more calculational time and large memory requirements both disk and RAM It is desired to find the minimum number of elements that give you a converged solution Beam Models For beam models we actually only need to define a single element per line unless we are applying a distributed load on a given frame member When point loads are used specifying more that one element per line will not change the solution it will only slow the calculations down For simple models it is of no concern but for a larger model it is desired to minimize the number of elements and thus calculation time and still obtain the desired accuracy General Models In general however it is necessary to conduct convergence tests on your finite element model to confirm that a fine enough element discretization has been used In a solid mechanics problem this would be done by creating several models with different mesh sizes and comparing the resulting deflections and stresses for example In general the stresses will converge more slowly than the displacement so it is not sufficient to examine the displacement convergence UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Saving and Restoring Jobs Saving Your Job It is good practice to save your model at various points during its creation Very often you will get to a point in the modeling where things have gone well and you like to save it at the point In that way if you make some mistakes later on you will at least be able to come back to this point To save your model select Utility Menu Bar File Save As Jobnamedb Your model will be saved in a file called jobnamedb where jobname is the name that you specified in the Launcher when you first started ANSYS It is a good idea to save your job at different times throughout the building and analysis of the model to backup your work incase of a system crash or other unforseen problems Recalling or Resuming a Previously Saved Job Frequently you want to start up ANSYS and recall and continue a previous job There are two methods to do this 1 Using the Launcher H In the ANSYS Launcher select Interactive and specify the previously defined jobname H Then when you get ANSYS started select Utility Menu File Resume Jobnamedb H This will restore as much of your database geometry loads solution etc that you previously saved 2 Or start ANSYS and select Utitily Menu File Resume from and select your job from the list that appears UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Files Introduction A large number of files are created when you run ANSYS If you started ANSYS without specifying a jobname the name of all the files created will be FILE where the represents various extensions described below If you specified a jobname say Frame then the created files will all have the file prefix Frame again with various extensions framedb Database file binary This file stores the geometry boundary conditions and any solutions framedbb Backup of the database file binary frameerr Error file text Listing of all error and warning messages frameout Output of all ANSYS operations text This is what normally scrolls in the output window during an ANSYS session framelog Logfile or listing of ANSYS commands text Listing of all equivalent ANSYS command line commands used during the current session etc Depending on the operations carried out other files may have been written These files may contain results etc What to save When you want to clean up your directory or move things from the scratch directory what files do you need to save G If you will always be using the GUI then you only require the db file This file stores the geometry boundary conditions and any solutions Once the ANSYS has started and the jobname has been specified you need only activate the resume command to proceed from where you last left off see Saving and Restoring Jobs G If you plan on using ANSYS command files then you need only store your command file andor the log file This file contains a complete listing of the ANSYS commands used to get you model to its current point That file may be rerun as is or edited and rerun as desired Command File Creation and Execution If you plan to use the command mode of operation starting with an existing log file rename it first so that it does not get over written or added to from another ANSYS run UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Printing and Plotting ANSYS Results to a File Printing Text Results to a File ANSYS produces lists and tables of many types of results that are normally displayed on the screen However it is often desired to save the results to a file to be later analyzed or included in a report 1 Stresses instead of using Plot Results to plot the stresses choose List Results Select Elem Table Data and choose what you want to list from the menu You can pick multiple items When the list appears on the screen in its own window Select FileSave As and give a file name to store the results 2 Any other solutions can be done in the same way For example select Nodal Solution from the List Results menu to get displacements 3 Preprocessing and Solution data can be listed and saved from the List menu in the Utility Menu bar Save the resulting list in the same way described above Plotting of Figures There are two major routes to get hardcopies from ANSYS The first is a quick a rasterbased screen dump while the second is a scalable vector plot 10 Quick Image Save When you want to quickly save an image of the entire screen or the current Graphics window select G Utility menu barPlotCtrlsHard Copy G In the window that appears you will normally want to select Graphics window Monochrome Reverse Video Landscape and Save to G Then enter the file name of your choice G Press OK This raster image file may now be printed on a PostScript printer or included in a document 20 Better Quality Plots The second method of saving a plot is much more flexible but takes a lot more work to set up as youll see Redirection Normally all ANSYS plots are directed to the plot window on the screen To save some plots to a file to be later printed or included in a document or what have you you must first redirect the plots to a file by issuing Utility menu barPlotCtrlsRedirect PlotsTo File Type in a filename eg framepic in the Selection Window Now issue whatever plot commands you want within ANSYS remembering that the plots will not be displayed to the screen but rather they will be written to the selected file You can put as many plots as you want into the plot file When you are finished plotting what you want to the file redirect plots back to the screen using Utility menu barPlotCtrlsRedirect PlotsTo Screen Display and Conversion The plot file that has been saved is stored in a proprietary file format that must be converted into a more common graphic file format like PostScript or HPGL for example This is performed by running a separate program called display To do this you have a couple of options 1 select display from the ANSYS launcher menu if you started ANSYS that way 2 shut down ANSYS or open up a new terminal window and then type display at the Unix prompt Either way a large graphics window will appear Decrease the size of this window because it most likely covers the window in which you will enter the display plotting commands Load your plot file with the following command fileframepic if your plot file is plotspic Note that although the file is plotspic with a period Display wants plotspicwith a comma You can display your plots to the graphics window by issuing the command like plotn where n is plot number If you plotted 5 images to this file in ANSYS then n could be any number from 1 to 5 Now that the plots have been read in they may be saved to printer files of various formats 1 Colour PostScript To save the images to a colour postscript file enter the following commands in display pscrcolor2 showpscr plotn where n is the plot number as above You can plot as many images as you want to postscript files in this manner For subsequent plots you only require the plotn command as the other options have now been set Each image is plotted to a postscript file such as pscrxxgrph where xx is a number starting at 00 Note when you import a postscript file into a word processor the postscript image will appear as blank box The printer information is still present but it can only be viewed when its printed out to a postscript printer Printing it out Now that youve got your color postscript file what are you going to do with it Take a look here for instructions on colour postscript printing at a couple of sites on campus where you can have your beautiful stress plot plotted to paper overheads or even posters 2 Black White PostScript The above mentioned colour postscript files can get very large in size and may not even print out on the postscript printer in the lab because it takes so long to transfer the files to the printer and process them A way around this is to print them out in a black and white postscript format instead of colour besides the colour specifications dont do any good for the black and white lab printer anyways To do this you set the postscript color option to 3 ie and then issue the other commands as before pscrcolor3 showpscr plotn Note when you import a postscript file into a word processor the postscript image will appear as blank box The printer information is still present but it can only be viewed when its printed out to a postscript printer 3 HPGL The third commonly used printer format is HPGL which stands for Hewlett Packard Graphics Language This is a compact vector format that has the advantage that when you import a file of this type into a word processor you can actually see the image in the word processor To use the HPGL format issue the following commands showhpgl plotn Final Steps It is wise to rename these plot files as soon as you leave display for display will overwrite the files the next time it is run You may want to rename the postscript files with an eps extension to indicate that they are encapsulated postscript images In a similar way the HPGL printer files could be given an hpgl extension This renaming is done at the Unix commmand line the mv command A list of all available display commands and their options may be obtained by typing help When complete exit display by entering finish UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Introduction Starting up ANSYS ANSYS Environment ANSYS Interface Convergence Testing SavingRestoring Jobs ANSYS Files Printing Results Working with ProE Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Finite Element Method using ProENGINEER and ANSYS Notes by RW Toogood The transfer of a model from ProENGINEER to ANSYS will be demonstrated here for a simple solid model Model idealizations such as shells and beams will not be treated Also many modeling options for constraints loads mesh control analysis types will not be covered These are fairly easy to figure out once you know the general procedures presented here Step 1 Make the part Use ProE to make the part Things to note are H be aware of your model units H note the orientation of the model default coordinate system in ANSYS will be the same as in ProE H IMPORTANT remove all unnecessary andor cosmetic features like rounds chamfers holes etc by suppressing them in ProE Too much small geometry will cause the mesh generator to create a very fine mesh with many elements which will greatly increase your solver time Of course if the feature is critical to your design you will want to leave it You must compromise between accuracy and available CPU resources The figure above shows the original model for this demonstration This is a model of a short cantilevered bracket that bolts to the wall via the thick plate on the left end Model units are inches A load is applied at the hole in the right end Some cosmetic features are located on the top surface and the two sides Several edges are rounded For this model the interest is in the stress distribution around the vertical slot So the plate and the loading hole are removed as are the cosmetic features and rounds resulting in the defeatured geometry shown below The model will be constrained on the left face and a uniform load will be applied to the right face Step 2 Create the FEM model In the pulldown menu at the top of the ProE window select Applications Mechanica An information window opens up to remind you about the units you are using Press Continue In the MECHANICA menu at the right check the box beside FEM Mode and select the command Structure A new toolbar appears on the right of the screen that contains icons for creating all the common modeling entities constraints loads idealizations All these commands are also available using the command windows that will open on the right side of the screen or in dialog windows that will open when appropriate Notice that a small green coordinate system WCS has appeared This is how you will specify the directions of constraints and forces Other coordinate systems eg cylindrical can be created as required and used for the same purpose The MEC STRUCT menu appears on the right Basically to define the model we proceed down this menu in a topdown manner Model is already selected for you which opens the STRC MODEL menu This is where we specify modeling information We proceed in a top down manner The Features command allows you to create additional simulation features like datum points curves surface regions and so on Idealizations lets you create special modeling entities like shells and beams The Current CSYS command lets you create or select an alternate coordinate system for specifying directions of constraints and loads Defining Constraints For our simple model all we need are constraints loads and a specified material Select Constraints New We can specify constraints on four entity types basically points edges and surfaces Constraints are organized into constraint sets Each constraint set has a unique name default of the first one is ConstraintSet1 and can contain any number of individual constraints of different types Each individual constraint also has a unique name default of the first one is Constraint1 In the final computed model only one set can be included but this can contain numerous individual constraints Select Surface We are going to fully constrain the left face of the cantilever A dialog window opens as shown above Here you can give a name to the constraint and identify which constraint set it belongs to Since we elected to create a surface constraint we now select the surface we want constrained push the Surface selection button in the window and then click on the desired surface of the model The constraints to be applied are selected using the buttons at the bottom of the window In general we specify constraints on translation and rotation for any mesh node that will appear on the selected entity For each direction X Y and Z we can select one of the four buttons Free Fixed Prescribed and Function of Coordinates For our solid model the rotation constraints are irrelevant since nodes of solid elements do not have this degree of freedom anyway For beams and shells rotational constraints are active if specified For our model leave all the translation constraints as FIXED and select the OK button You should now see some orange symbols on the left face of the model along with some text labels that summarize the constraint settings Defining Loads In the STRC MODEL menu select Loads New Surface The FORCEMOMENT window opens as shown above Loads are also organized into named load sets A load set can contain any number of individual loads of different types A FEM model can contain any number of different load sets For example in the analysis of a pressurized tank on a support system with a number of nozzle connections to other pipes one load set might contain only the internal pressure another might contain the support forces another a temperature load and more might contain the forces applied at each nozzle location These can be solved at the same time and the principle of superposition used to combine them in numerous ways Create a load called endload in the default load set LoadSet1 Click on the Surfaces button then select the right face of the model and middle click to return to this dialog Leave the defaults for the load distribution Enter the force components at the bottom Note these are relative to the WCS Then select OK The load should be displayed symbolically as shown in the figure below Note that constraint and load sets appear in the model tree You can select and edit these in the usual way using the right mouse button Assigning Materials Our last job to define the model is to specify the part material In the STRC MODEL menu select Materials Whole Part In the library dialog window select a material and move it to the right pane using the triple arrow button in the center of the window In an assembly you could now assign this material to individual parts If you select the Edit button you will see the properties of the chosen material At this point our model has the necessary information for solution constraints loads material Step 3 Define the analysis Select Analyses New Specify a name for the analysis like ansystest Select the type Structural or Modal Enter a short description Now select the Add buttons beside the Constraints and Loads panes to add ConstraintSet1 and LoadSet1 to the analysis Now select OK Step 4 Creating the mesh We are going to use defaults for all operations here The MEC STRUCT window select Mesh Create Solid Start Accept the default for the global minimum The mesh is created and another dialog window opens Element Quality Checks This indicates some aspects of mesh quality that may be specified and then by selecting the Check button at the bottom evaluated for the model The results are indicated in columns on the right If the mesh does not pass these quality checks you may want to go back to specify mesh controls discussed below Select Close Here is an image of the default mesh shown in wire frame Improving the Mesh In the mesh command you can select the Controls option This will allow you to select points edges and surfaces where you want to specify mesh geometry such as hard points maximum mesh size and so on Beware that excessively tight mesh controls can result in meshes with many elements For example setting a maximum mesh size along the curved ends of the slot results in the following mesh Notice the better representation of the curved edges than in the previous figure This is at the expense of more than double the number of elements Note that mesh controls are also added to the model tree Step 5 Creating the Output file All necessary aspects of the model are now created constraints loads materials mesh In the MEC STRUCT menu select Run This opens the Run FEM Analysis dialog window shown here In the Solver pulldown list at the top select ANSYS In the Analysis list select Structural You pick either Linear or Parabolic elements The analysis we defined containing constraints loads mesh and material is listed Select the Output to File radio button at the bottom and specify the output file name default is the analysis name with extension ans Select OK and read the message window We are now finished with ProE Go to the top pulldown menus and select Applications Standard Save the model file and leave the program Copy the ans file from your ProE working directory to the directory you will use for running ANSYS Step 6 Importing into ANSYS Launch ANSYS Interactive and select File Read Input From Select the ans file you created previously This will read in the entire model You can display the model using in the pull down menus Plot Elements Step 7 Running the ANSYS solver In the ANSYS Main Menu on the left select Solution Solve Current LS OK After a few seconds you will be informed that the solution is complete Step 8 Viewing the results There are myriad possibilities for viewing FEM results A common one is the following General Postproc Plot Results Contour Plot Nodal Solu Pick the Von Mises stress values and select Apply You should now have a color fringe plot of the Von Mises stress displayed on the model Updated 8 November 2002 using ProENGINEER 2001 RWT Please report errors or omissions to Roger Toogood UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Two Dimensional Truss Bicycle Space Frame Plane Stress Bracket Modeling Tools Solid Modeling Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Two Dimensional Truss Introduction This tutorial was created using ANSYS 70 to solve a simple 2D Truss problem This is the first of four introductory ANSYS tutorials Problem Description Determine the nodal deflections reaction forces and stress for the truss system shown below E 200GPa A 3250mm2 Modified from Chandrupatla Belegunda Introduction to Finite Elements in Engineering p123 Preprocessing Defining the Problem 1 Give the Simplified Version a Title such as Bridge Truss Tutorial In the Utility menu bar select File Change Title The following window will appear Enter the title and click OK This title will appear in the bottom left corner of the Graphics Window once you 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 H We are going to define 7 keypoints for the simplified structure as given in the following table keypoint coordinate x y 1 0 0 2 1800 3118 3 3600 0 4 5400 3118 5 7200 0 6 9000 3118 7 10800 0 these keypoints are depicted by numbers in the above figure H From the ANSYS Main Menu select Preprocessor Modeling Create Keypoints In Active CS The following window will then appear H 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 xy coordinates 0 0 in their appropriate boxes as shown above Click Apply to accept what you have typed H Enter the remaining keypoints using the same method Note When entering the final data point click on OK to indicate that you are finished entering keypoints If you first press Apply and then OK for the final keypoint you will have defined it twice If you did press Apply for the final point simply press Cancel to close this dialog box Units Note the units of measure ie mm were not specified It is the responsibility of the user to ensure that a consistent set of units are used for the problem thus making any conversions where necessary Correcting Mistakes When defining keypoints lines areas volumes elements constraints and loads you are bound to make mistakes Fortunately these are easily corrected so that you dont 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 up 3 Form Lines The keypoints must now be connected We will use the mouse to select the keypoints to form the lines H In the main menu select Preprocessor Modeling Create Lines Lines In Active Coord The following window will then appear H Use the mouse to pick keypoint 1 ie click on it It will now be marked by a small yellow box H Now move the mouse toward keypoint 2 A line will now show on the screen joining these two points Left click and a permanent line will appear H Connect the remaining keypoints using the same method H When youre 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 the following figure Disappearing Lines Please note that any lines you have created may disappear throughout your 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 for our problem H From the Preprocessor Menu select Element Type AddEditDelete The following window will then appear H Click on the Add button The following window will appear H For this example we will use the 2D spar element as selected in the above figure Select the element shown and click OK You should see Type 1 LINK1 in the Element Types window H Click on Close in the Element Types dialog box 5 Define Geometric Properties We now need to specify geometric properties for our elements H In the Preprocessor menu select Real Constants AddEditDelete H Click Add and select Type 1 LINK1 actually it is already selected Click on OK The following window will appear H As shown in the window above enter the crosssectional area 3250mm H Click on OK H Set 1 now appears in the dialog box Click on Close in the Real Constants window 6 Element Material Properties You then need to specify material properties H In the Preprocessor menu select Material Props Material Models H Double click on Structural Linear Elastic Isotropic We are going to give the properties of Steel Enter the following field EX 200000 H Set these properties and click on OK Note You may obtain the note PRXY will be set to 00 This is poissons ratio and is not required for this element type Click OK on the window to continue Close the Define Material Model Behavior by clicking on the X box in the upper right hand corner 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 just deal with one method for now H In the Preprocessor menu select Meshing Size Cntrls ManualSize Lines All Lines H 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 H In the Preprocessor menu select Meshing Mesh Lines and click Pick All in the Mesh Lines Window Your model should now appear as shown in the following window Plot Numbering To show the line numbers keypoint numbers node numbers G From the Utility Menu top of screen select PlotCtrls Numbering G Fill in the Window as shown below and click OK Now you can turn numbering on or off at your discretion Saving Your Work Save the model at this time so if you make some mistakes later on you 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 you 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 or what have you Solution Phase Assigning Loads and Solving You have now defined your model It is now time to apply the loads and constraints and solve the the resulting system of equations Open up the Solution menu from the same ANSYS Main Menu 1 Define Analysis Type First you must tell ANSYS how you want it to solve this problem H From the Solution Menu select Analysis Type New Analysis H Ensure that Static is selected ie you are going to do a static analysis on the truss as opposed to a dynamic analysis for example H 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 rollertype connections As shown above the left end of the truss bridge is pinned while the right end has a roller connection H In the Solution menu select Define Loads Apply Structural Displacement On Keypoints H 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 H 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 You will see some blue triangles in the graphics window indicating the displacement contraints H 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 UROT on KPs window Therefore you 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 280kN 210kN 280kN and 360kN at keypoints 1 3 5 and 7 respectively H Select Define Loads Apply Structural ForceMoment on Keypoints H Select the first Keypoint left end of the truss and click OK in the Apply FM on KPs window H Select FY in the Direction of forcemom This indicate that we will be applying the load in the y direction H Enter a value of 280000 in the Forcemoment value box and click OK Note that we are using units of N here this is consistent with the previous values input H The force will appear in the graphics window as a red arrow H Apply the remaining loads in the same manner The applied loads and constraints should now appear as shown below 4 Solving the System We now tell ANSYS to find the solution H In the Solution menu select Solve Current LS This indicates that we desire the solution under the current Load Step LS H The above windows will appear Ensure that your solution options are the same as shown above and click OK H Once the solution is done the following window will pop up Click Close and close the STATUS Command Window Postprocessing Viewing the Results 1 Hand Calculations We will first calculate the forces and stress in element 1 as labeled in the problem description 2 Results Using ANSYS Reaction Forces A list of the resulting reaction forces can be obtained for this element H from the Main Menu select General Postproc List Results Reaction Solu H Select All struc forc F as shown above and click OK These values agree with the reaction forces claculated by hand above Deformation H In the General Postproc menu select Plot Results Deformed Shape The following window will appear H Select Def undef edge and click OK to view both the deformed and the undeformed object H Observe the value of the maximum deflection in the upper left hand corner DMX7409 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 H From the General Postproc menu select Plot results Contour Plot Nodal Solution The following window will appear H Select DOF solution and USUM as shown in the above window Leave the other selections as the default values Click OK H Looking at the scale you may want to use more useful intervals From the Utility Menu select Plot Controls Style Contours Uniform Contours H Fill in the following window as shown and click OK You should obtain the following H 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 H Are these results what you expected Note that all the degrees of freedom were constrained to zero at node 1 while UY was constrained to zero at node 7 H If you wanted to save these results to a file select File within the results window at the upper lefthand corner of this list window and select Save as Axial Stress For line elements ie links beams spars and pipes you will often need to use the Element Table to gain access to derived data ie stresses strains For this example we should obtain axial stress to compare with the hand calculations The Element Table is different for each element therefore we need to look at the help file for LINK1 Type help link1 into the Input Line From Table 12 in the Help file we can see that SAXL can be obtained through the ETABLE using the item LS1 H From the General Postprocessor menu select Element Table Define Table H Click on Add H As shown above enter SAXL in the Lab box This specifies the name of the item you are defining Next in the Item Comp boxes select By sequence number and LS Then enter 1 after LS in the selection box H Click on OK and close the Element Table Data window H Plot the Stresses by selecting Element Table Plot Elem Table H The following window will appear Ensure that SAXL is selected and click OK H Because you changed the contour intervals for the Displacement plot to User Specified you need to switch this back to Auto calculated to obtain new values for VMINVMAX Utility Menu PlotCtrls Style Contours Uniform Contours Again you may wish to select more appropriate intervals for the contour plot H List the Stresses I From the Element Table menu select List Elem Table I From the List Element Table Data window which appears ensure SAXL is highlighted I Click OK Note that the axial stress in Element 1 is 829MPa as predicted analytically Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Quitting ANSYS To quit ANSYS select QUIT from the ANSYS Toolbar or select Utility MenuFileExit In the dialog box that appears click on Save Everything assuming that you want to and then click on OK UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Two Dimensional Truss Bicycle Space Frame Plane Stress Bracket Modeling Tools Solid Modeling Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Space Frame Example Verification Example Preprocessing Solution Postprocessing Command Line Bicycle Example Preprocessing Solution Postprocessing Command Line Introduction This tutorial was created using ANSYS 70 to solve a simple 3D space frame problem Problem Description The problem to be solved in this example is the analysis of a bicycle frame The problem to be modeled in this example is a simple bicycle frame shown in the following figure The frame is to be built of hollow aluminum tubing having an outside diameter of 25mm and a wall thickness of 2mm Verification The first step is to simplify the problem Whenever you are trying out a new analysis type you need something ie analytical solution or experimental data to compare the results to This way you can be sure that youve gotten the correct analysis type units scale factors etc The simplified version that will be used for this problem is that of a cantilever beam shown in the following figure Preprocessing Defining the Problem 1 Give the Simplified Version a Title such as Verification Model Utility Menu File Change Title 2 Enter Keypoints For this simple example these keypoints are the ends of the beam H We are going to define 2 keypoints for the simplified structure as given in the following table keypoint coordinate x y z 1 0 0 0 2 500 0 0 H From the ANSYS Main Menu select Preprocessor Modeling Create Keypoints In Active CS 3 Form Lines The two keypoints must now be connected to form a bar using a straight line H Select Preprocessor Modeling Create Lines Lines Straight Line H Pick keypoint 1 ie click on it It will now be marked by a small yellow box H Now pick keypoint 2 A permanent line will appear H When youre done click on OK in the Create Straight Line window 4 Define the Type of Element It is now necessary to create elements on this line H From the Preprocessor Menu select Element Type AddEditDelete H Click on the Add button The following window will appear H For this example we will use the 3D elastic straight pipe element as selected in the above figure Select the element shown and click OK You should see Type 1 PIPE16 in the Element Types window H Click on the Options button in the Element Types dialog box The following window will appear H Click and hold the K6 button second from the bottom and select Include Output and click OK This gives us extra force and moment output H Click on Close in the Element Types dialog box and close the Element Type menu 5 Define Geometric Properties We now need to specify geometric properties for our elements H In the Preprocessor menu select Real Constants AddEditDelete H Click Add and select Type 1 PIPE16 actually it is already selected Click on OK H Enter the following geometric properties Outside diameter OD 25 Wall thickness TKWALL 2 This defines an outside pipe diameter of 25mm and a wall thickness of 2mm H Click on OK H Set 1 now appears in the dialog box Click on Close in the Real Constants window 6 Element Material Properties You then need to specify material properties H In the Preprocessor menu select Material Props Material Models H Double click Structural Linear Elastic and select Isotropic double click on it H Close the Define Material Model Behavior Window We are going to give the properties of Aluminum Enter the following field EX 70000 PRXY 033 H Set these properties and click on OK 7 Mesh Size H In the Preprocessor menu select Meshing Size Cntrls ManualSize Lines All Lines H In the size SIZE field enter the desired element length For this example we want an element length of 2cm therefore enter 20 ie 20mm and then click OK Note that we have not yet meshed the geometry we have simply defined the element sizes Alternatively we could enter the number of divisions we want in the line For an element length of 2cm we would enter 25 ie 25 divisions NOTE It is not necessary to mesh beam elements to obtain the correct solution However meshing is done in this case so that we can obtain results ie stress displacement at intermediate positions on the beam 8 Mesh Now the frame can be meshed H In the Preprocessor menu select Meshing Mesh Lines and click Pick All in the Mesh Lines Window 9 Saving Your Work Utility Menu File Save as Select the name and location where you want to save your file Solution Phase Assigning Loads and Solving 1 Define Analysis Type H From the Solution Menu select Analysis Type New Analysis H Ensure that Static is selected and click OK 2 Apply Constraints H In the Solution menu select Define Loads Apply Structural Displacement On Keypoints H Select the left end of the rod Keypoint 1 by clicking on it in the Graphics Window and click on OK in the Apply UROT on KPs window H 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 3 Apply Loads As shown in the diagram there is a vertically downward load of 100N at the end of the bar H In the Structural menu select ForceMoment on Keypoints H Select the second Keypoint right end of bar and click OK in the Apply FM window H Click on the Direction of forcemom at the top and select FY H Enter a value of 100 in the Forcemoment value box and click OK H The force will appear in the graphics window as a red arrow The applied loads and constraints should now appear as shown below 4 Solving the System We now tell ANSYS to find the solution H Solution Solve Current LS Postprocessing Viewing the Results 1 Hand Calculations Now since the purpose of this exercise was to verify the results we need to calculate what we should find Deflection The maximum deflection occurs at the end of the rod and was found to be 62mm as shown above Stress The maximum stress occurs at the base of the rod and was found to be 649MPa as shown above pure bending stress 2 Results Using ANSYS Deformation H from the Main Menu select General Postproc from the ANSYS Main Menu In this menu you will find a variety of options the two which we will deal with now are Plot Results and List Results H Select Plot Results Deformed Shape H Select Def undef edge and click OK to view both the deformed and the undeformed object H Observe the value of the maximum deflection in the upper left hand corner shown here surrounded by a blue border for emphasis This is identical to that obtained via hand calculations Deflection For a more detailed version of the deflection of the beam H From the General Postproc menu select Plot results Contour Plot Nodal Solution H Select DOF solution and USUM Leave the other selections as the default values Click OK H You may want to have a more useful scale which can be accomplished by going to the Utility Menu and selecting Plot Controls Style Contours Uniform Contours H 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 translational and rotational degrees of freedom from the solution If we had only wanted to see the displacements for example we would have chosen ALL Us instead of ALL DOFs H Are these results what you expected Again the maximum deflection occurs at node 2 the right end of the rod Also note that all the rotational and translational degrees of freedom were constrained to zero at node 1 H If you wanted to save these results to a file use the mouse to go to the File menu at the upper lefthand corner of this list window and select Save as Stresses For line elements ie beams spars and pipes you will need to use the Element Table to gain access to derived data ie stresses strains H From the General Postprocessor menu select Element Table Define Table H Click on Add H As shown above in the ItemComp boxes in the above window select Stress and von Mises SEQV H Click on OK and close the Element Table Data window H Plot the Stresses by selecting Plot Elem Table in the Element Table Menu H The following window will appear Ensure that SEQV is selected and click OK H If you changed the contour intervals for the Displacement plot to User Specified you may need to switch this back to Auto calculated to obtain new values for VMINVMAX Utility Menu PlotCtrls Style Contours Uniform Contours Again select more appropriate intervals for the contour plot H List the Stresses I From the Element Table menu select List Elem Table I From the List Element Table Data window which appears ensure SEQV is highlighted I Click OK Note that a maximum stress of 64914 MPa occurs at the fixed end of the beam as predicted analytically Bending Moment Diagrams To further verify the simplified model a bending moment diagram can be created First lets look at how ANSYS defines each element Pipe 16 has 2 nodes I and J as shown in the following image To obtain the bending moment for this element the Element Table must be used The Element Table contains most of the data for the element including the bending moment data for each element at Node I and Node J First we need to obtain obtain the bending moment data H General Postproc Element Table Define Table Click Add H In the window A Enter IMoment as the User label for item this will give a name to the data B Select By sequence num in the Item box C Select SMISC in the first Comp box D Enter SMISC6 in the second Comp box E Click OK This will save all of the bending moment data at the left hand side I side of each element Now we need to find the bending moment data at the right hand side J side of each element H Again click Add in the Element Table Data window A Enter JMoment as the User label for item again this will give a name to the data B Same as above C Same as above D For step D enter SMISC12 in the second Comp box E Click OK H Click Close in the Element Table Data window and close the Element Table Menu Select Plot Results Contour Plot Line Elem Res H From the Plot LineElement Results window select IMOMENT from the pull down menu for LabI and JMOMENT from the pull down menu for LabJ Click OK Note again that you can modify the intervals for the contour plot Now you can double check these solutions analytically Note that the line between the I and J point is a linear interpolation H Before the explanation of the above steps enter help pipe16 in the command line as shown below and then hit enter H Briefly read the ANSYS documentation which appears pay particular attention to the Tables near the end of the document shown below Table 1 PIPE16 Item Sequence Numbers and Definitions for the ETABLE Commands node I name item e Definition MFORX SMISC 1 Member forces MFORY SMISC 2 at the node MFORZ SMISC 3 MMOMX SMISC 4 Member moments at the node MMOMY SMISC 5 MMOMZ SMISC 6 Note that SMISC 6 which we used to obtain the values at node I correspond to MMOMZ the Member moment for node I The value of e varies with different Element Types therefore you must check the ANSYS Documentation files for each element to determine the appropriate SMISC corresponding to the plot you wish to generate Command File Mode of Solution The above example was solved using the Graphical User Interface or GUI of ANSYS This problem can also been solved using the ANSYS command language interface To see the benefits of the command line clear your current file G From the Utility menu select File Clear and Start New G Ensure that Read File is selected then click OK G select yes in the following window Copy the following code into the command line then hit enter Note that the text following the are comments PREP7 Preprocessor K1000 Keypoint 1 x y z K250000 Keypoint 2 x y z L12 Line from keypoint 1 to 2 ET1PIPE16 Element Type pipe 16 KEYOPT161 This is the changed option to give the extra force and moment output R1252 Real Constant Material 1 Outside Diameter Wall thickness MPEX170000 Material Properties Youngs Modulus Material 1 70000 MPa MPPRXY1033 Material Properties Major Poissons Ratio Material 1 033 LESIZEALL20 Element sizes all of the lines 20 mm LMESH1 Mesh the lines FINISH Exit preprocessor SOLU Solution ANTYPE0 The type of analysis static DK1 0 0ALL Apply a Displacement to Keypoint 1 to all DOF FK2FY100 Apply a Force to Keypoint 2 of 100 N in the y direction STATUSSOLU SOLVE Solve the problem FINISH Note that you have now finished Postprocessing and the Solution Phase with just these few lines of code There are codes to complete the Postprocessing but we will review these later Bicycle Example Now we will return to the analysis of the bike frame The steps which you completed in the verification example will not be explained in great detail therefore use the verification example as a reference as required We will be combining the use of the Graphic User Interface GUI with the use of command lines Recall the geometry and dimensions of the bicycle frame Preprocessing Defining the Problem 1 Clear any old ANSYS files and start a new file Utility Menu File Clear and Start New 2 Give the Example a Title Utility menu File Change Title 3 Defining Some Variables We are going to define the vertices of the frame using variables These variables represent the various lengths of the bicycle members Notice that by using variables like this it is very easy to set up a parametric description of your model This will enable us to quickly redefine the frame should changes be necessary The quickest way to enter these variables is via the ANSYS Input window which was used above to input the command line codes for the verification model Type in each of the following lines followed by Enter x1 500 x2 825 y1 325 y2 400 z1 50 4 Enter Keypoints For this space frame example these keypoints are the frame vertices H We are going to define 6 keypoints for this structure as given in the following table these keypoints are depicted by the circled numbers in the above figure keypoint coordinate x y z 1 0 y1 0 2 0 y2 0 3 x1 y2 0 4 x1 0 0 5 x2 0 z1 6 x2 0 z1 H Now instead of using the GUI window we are going to enter code into the command line First open the Preprocessor Menu from the ANSYS Main Menu The preprocessor menu has to be open in order for the preprocessor commands to be recognized Alternatively you can type PREP7 into the command line The command line format required to enter a keypoint is as follows K NPT X Y Z where each Abbreviation is representative of the following Keypoint Reference number for the keypoint coords xyz For a more detailed explanation type help k into the command line For example to enter the first keypoint type K10y10 into the command line followed by Enter As with any programming language you may need to add comments The exclamation mark indicates that anything following it is commented out ie for the second keypoint you might type K20y20 keypoint x0 yy2 z0 H Enter the 4 remaining keypoints listed in the table above using the command line H Now you may want to check to ensure that you entered all of the keypoints correctly Utility Menu List Keypoints Coordinates only Alternatively type KLIST into the command line H If there are any keypoints which need to be reentered simply reenter the code A previously defined keypoint of the same number will be redefined However if there is one that needs to be deleted simply enter the following code KDELE where corresponds to the number of the keypoint In this example we defined the keypoints by making use of previously defined variables like y1 325 This was simply used for convenience To define keypoint 1 for example we could have alternatively used the coordinates x 0 y 325 z 0 5 Changing Orientation of the Plot H To get a better view of our view of our model well view it in an isometric view H Select Utility menu bar PlotCtrls Pan Zoom Rotate I In the window that appears shown left you have many controls Try experimenting with them By turning on the dynamic mode click on the checkbox beside Dynamic Mode you can use the mouse to drag the image translating and rotating it on all three axes I To get an isometric view click on Iso at the top right You can either leave the Pan Zoom Rotate window open and move it to an empty area on the screen or close it if your screen is already cluttered 6 Create Lines We will be joining the following keypoints together line keypoint 1st 2nd 1 1 2 2 2 3 3 3 4 4 1 4 5 3 5 6 4 5 7 3 6 8 4 6 Again we will use the command line to create the lines The command format to create a straight line looks like L P1 P2 Line Keypoint at the beginning of the line Keypoint at the end of line For example to obtain the first line I would write L12 Note unlike Keypoints Lines will automatically assign themselves the next available reference number H Enter the remaining lines until you get a picture like that shown below H Again check to ensure that you entered all of the lines correctly type LLIST into the command line H If there are any lines which need to be changed delete the line by typing the following code LDELE where corresponds to the reference number of the line This can be obtained from the list of lines And then reenter the line note a new reference number will be assigned You should obtain the following 7 Define the Type of Element Preprocessor Element Type AddEditDelete Add As in the verification model define the type of element pipe16 As in the verification model dont forget to change Option K6 Include Output to obtain extra force and moment output 8 Define Geometric Properties Preprocessor Real Constants AddEditDelete Now specify geometric properties for the elements Outside diameter OD 25 Wall thickness TKWALL 2 9 Element Material Properties To set Youngs Modulus and Poissons ratio we will again use the command line ensure that the preprocessor menu is still open if not open it by clicking Preprocessor in the Main Menu MP LAB MAT C0 Material PropertyValid material property label Material Reference Number value H To enter the Elastic Modulus LAB EX of 70000 MPa type MPEX170000 H To set Poissons ratio PRXY type MPPRXY1033 10 Mesh Size As in the verification model set the element length to 20 mm Preprocessor Meshing Size Cntrls ManualSize Lines All Lines 11 Mesh Now the frame can be meshed H In the Preprocessor menu select Mesh Lines and click Pick All in the Mesh Lines Window Saving Your Job Utility Menu File Save as Solution Phase Assigning Loads and Solving Close the Preprocessor menu and open up the Solution menu from the same ANSYS Main Menu 1 Define Analysis Type Solution Analysis Type New Analysis Static 2 Apply Constraints Once again we will use the command line We are going to pin translational DOFs will be fixed the first keypoint and constrain the keypoints corresponding to the rear wheel attachment locations in both the y and z directions The following is the command line format to apply constraints at keypoints DK KPOI Lab VALUE VALUE2 KEXPND Lab2 Lab3 Lab4 Lab5 Lab6 Displacement on K K DOF label value value2 Expansion key other DOF labels Not all of the fields are required for this example therefore when entering the code certain fields will be empty For example to pin the first keypoint enter DK1UX0UYUZ The DOF labels for translation motion are UX UY UZ Note that the 5th and 6th fields are empty These correspond to value2 and the Expansion key which are not required for this constraint Also note that all three of the translational DOFs were constrained to 0 The DOFs can only be contrained in 1 command line if the value is the same To apply the contraints to Keypoint 5 the command line code is DK5UY0UZ Note that only UY and UZ are contrained to 0 UX is not constrained Again note that the 5th and 6th fields are empty because they are not required H Apply the constraints to the other rear wheel location Keypoint 6 UY and UZ H Now list the constraints DKLIST and verify them against the following If you need to delete any of the constraints use the following command DKDELE K Lab ie DKDELE1UZ would delete the constraint in the z direction for Keypoint 1 3 Apply Loads We will apply vertical downward loads of 600N at the seat post location keypoint 3 and 200N at the pedal crank location keypoint 4 We will use the command line to define these loading conditions FK KPOI Lab value value2 Force loads at keypoints K Force Label directions FX FY FZ value1 value2 if reqd To apply a force of 600N downward at keypoint 3 the code should look like this FK3FY600 Apply both the forces and list the forces to ensure they were inputted correctly FKLIST If you need to delete one of the forces the code looks like this FKDELE K Lab ie FKDELE3FY would delete the force in the y direction for Keypoint 3 The applied loads and constraints should now appear as shown below 4 Solving the System Solution Solve Current LS Postprocessing Viewing the Results To begin Postprocessing open the General Postproc Menu 1 Deformation Plot Results Deformed Shape Def undef edge H You may want to try plotting this from different angles to get a better idea whats going on by using the PanZoomRotate menu that was earlier outlined H Try the Front view button Note that the views of Front Left Back etc depend on how the object was first defined H Your screen should look like the plot below 2 Deflections Now lets take a look at some actual deflections in the frame The deflections have been calculated at the nodes of the model so the first thing well do is plot out the nodes and node numbers so we know what nodes were after H Go to Utility menu PlotCtrls Numbering and turn on Node numbers Turn everything else off H Note the node numbers of interest Of particular interest are those nodes where the constraints were applied to see if their displacementsrotations were indeed fixed to zero Also note the node numbers of the seat and crank locations H List the Nodal Deflections Main Menu General Postproc List Results Nodal Solution Are the displacements and rotations as you expected H Plot the deflection as well General Postproc Plot Results Contour Plot Nodal Solution select DOF solution and USUM in the window H Dont forget to use more useful intervals 3 Element Forces We could also take a look at the forces in the elements in much the same way H Select Element Solution from the List Results menu H Select Nodal force data and All forces from the lists displayed H Click on OK H For each element in the model the forcemoment values at each of the two nodes per element will be displayed H Close this list window when you are finished browsing H Then close the List Results menu 4 Stresses As shown in the cantilever beam example use the Element Table to gain access to derived stresses H General Postproc Element Table Define Table H Select Add H Select Stress and von Mises H Element Table Plot Elem Table H Again select appropriate intervals for the contour plot 5 Bending Moment Diagrams As shown previously the bending moment diagram can be produced Select Element Table Define Table to define the table remember SMISC6 and SMISC12 And Plot Results Line Elem Res to plot the data from the Element Table Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Quitting ANSYS To quit ANSYS select QUIT from the ANSYS Toolbar or select Utility MenuFileExit In the dialog box that appears click on Save Everything assuming that you want to and then click on OK UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Two Dimensional Truss Bicycle Space Frame Plane Stress Bracket Modeling Tools Solid Modeling Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Plane Stress Bracket Verification Example Preprocessing Solution Postprocessing Command Line Bracket Example Preprocessing Solution Postprocessing Command Line Introduction This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS The plane stress bracket tutorial builds upon techniques covered in the first tutorial 3D Bicycle Space Frame it is therefore essential that you have completed that tutorial prior to beginning this one The 2D Plane Stress Bracket will introduce boolean operations plane stress and uniform pressure loading Problem Description The problem to be modeled in this example is a simple bracket shown in the following figure This bracket is to be built from a 20 mm thick steel plate A figure of the plate is shown below This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right Verification Example The first step is to simplify the problem Whenever you are trying out a new analysis type you need something ie analytical solution or experimental data to compare the results to This way you can be sure that youve gotten the correct analysis type units scale factors etc The simplified version that will be used for this problem is that of a flat rectangular plate with a hole shown in the following figure Preprocessing Defining the Problem 1 Give the Simplified Version a Title Utility Menu File Change Title 2 Form Geometry Boolean operations provide a means to create complicated solid models These procedures make it easy to combine simple geometric entities to create more complex bodies Subtraction will used to create this model however many other Boolean operations can be used in ANSYS a Create the main rectangular shape Instead of creating the geometry using keypoints we will create an area using GUI Preprocessor Modeling Create Areas Rectangle By 2 Corners I Fill in the window as shown above This will create a rectangle where the bottom left corner has the coordinates 000 and the top right corner has the coordinates 2001000 Alternatively the command line code for the above command is BLC400200100 b Create the circle Preprocessor Modeling Create Areas Circle Solid Circle I Fill in the window as shown above This will create a circle where the center has the coordinates 100500 the center of the rectangle and the radius of the circle is 20 mm Alternatively the command line code for the above command is CYL41005020 c Subtraction Now we want to subtract the circle from the rectangle Prior to this operation your image should resemble the following I To perform the Boolean operation from the Preprocessor menu select Modeling Operate Booleans Subtract Areas I At this point a Subtract Areas window will pop up and the ANSYS Input window will display the following message ASBA Pick or enter base areas from which to subtract as shown below I Therefore select the base area the rectangle by clicking on it Note The selected area will turn pink once it is selected I The following window may appear because there are 2 areas at the location you clicked I Ensure that the entire rectangular area is selected otherwise click Next and then click OK I Click OK on the Subtract Areas window I Now you will be prompted to select the areas to be subtracted select the circle by clicking on it and then click OK You should now have the following model Alternatively the command line code for the above step is ASBA12 3 Define the Type of Element It is now necessary to define the type of element to use for our problem Preprocessor Menu Element Type AddEditDelete H Add the following type of element Solid under the Structural heading and the Quad 82 element as shown in the above figure PLANE82 is a higher order version of the twodimensional fournode element PLANE42 PLANE82 is an eight noded quadrilateral element which is better suited to model curved boundaries For this example we need a plane stress element with thickness therefore H Click on the Options button Click and hold the K3 button and select Plane strs wthk as shown below Alternatively the command line code for the above step is ET1PLANE82 followed by KEYOPT133 4 Define Geometric Properties H As in previous examples Preprocessor menu Real Constants AddEditDelete H Enter a thickness of 20 as shown in the figure below This defines a plate thickness of 20mm Alternatively the command line code for the above step is R120 5 Element Material Properties H As shown in previous examples select Preprocessor Material Props Material models Structural Linear Elastic Isotropic We are going to give the properties of Steel Enter the following when prompted EX 200000 PRXY 03 Alternatively the command line code for the above step is MPEX1200000 followed by MPPRXY103 6 Mesh Size To tell ANSYS how big the elements should be Preprocessor Meshing Size Cntrls Manual Size Areas All Areas H Select an element edge length of 25 We will return later to determine if this was adequate for the problem Alternatively the command line code for the above step is AESIZEALL25 7 Mesh Now the frame can be meshed H In the Preprocessor menu select Meshing Mesh Areas Free and select the area when prompted Alternatively the command line code for the above step is AMESHALL You should now have the following Saving Your Job Utility Menu File Save as Solution Phase Assigning Loads and Solving You have now defined your model It is now time to apply the loads and constraints and solve the the resulting system of equations 1 Define Analysis Type H Ensure that a Static Analysis will be performed Solution Analysis Type New Analysis Alternatively the command line code for the above step is ANTYPE0 2 Apply Constraints As shown previously the left end of the plate is fixed H In the Solution Define Loads Apply Structural Displacement On Lines H Select the left end of the plate and click on Apply in the Apply UROT on Lines window H Fill in the window as shown below H This location is fixed which means that all DOFs are constrained Therefore select All DOF by clicking on it and enter 0 in the Value field as shown above You will see some blue triangles in the graphics window indicating the displacement contraints Alternatively the command line code for the above step is DL4ALL0 3 Apply Loads H As shown in the diagram there is a load of 20Nmm distributed on the right hand side of the plate To apply this load Solution Define Loads Apply Structural Pressure On Lines H When the window appears select the line along the right hand edge of the plate and click OK H Calculate the pressure on the plate end by dividing the distributed load by the thickness of the plate 1 MPa H Fill in the Apply PRES on lines window as shown below NOTE I The pressure is uniform along the surface of the plate therefore the last field is left blank I The pressure is acting away from the surface of the plate and is therefore defined as a negative pressure The applied loads and constraints should now appear as shown below 4 Solving the System Solution Solve Current LS Postprocessing Viewing the Results 1 Hand Calculations Now since the purpose of this exercise was to verify the results we need to calculate what we should find Deflection The maximum deflection occurs on the right hand side of the plate and was calculated to be 0001 mm neglecting the effects of the hole in the plate ie just a flat plate The actual deflection of the plate is therefore expected to be greater but in the same range of magnitude Stress The maximum stress occurs at the top and bottom of the hole in the plate and was found to be 39 MPa 2 Convergence using ANSYS At this point we need to find whether or not the final result has converged We will do this by looking at the deflection and stress at particular nodes while changing the size of the meshing element Since we have an analytical solution for the maximum stress point we will check the stress at this point First we need to find the node corresponding to the top of the hole in the plate First plot and number the nodes Utility Menu Plot Nodes Utility Menu PlotCtrls Numbering H The plot should look similar to the one shown below Make a note of the node closest to the top of the circle ie 49 H List the stresses General Postproc List Results Nodal Solution Stress Principals SPRIN and check the SEQV Equivalent Stress von Mises Stress for the node in question as shown below in red The equivalent stress was found to be 29141 MPa at this point We will use smaller elements to try to get a more accurate solution H Resize Elements a To change the element size we need to go back to the Preprocessor Menu Preprocessor Meshing Size Cntrls Manual Size Areas All Areas now decrease the element edge length ie 20 b Now remesh the model Preprocessor Meshing Mesh Areas Free Once you have selected the area and clicked OK the following window will appear c Click OK This will remesh the model using the new element edge length d Solve the system again note that the constraints need not be reapplied Solution Menu Current LS H Repeat steps a through d until the model has converged note the number of the node at the top of the hole has most likely changed It is essential that you plot the nodes again to select the appropriate node Plot the stressdeflection at varying mesh sizes as shown below to confirm that convergence has occured Note the shapes of both the deflection and stress curves As the number of elements in the mesh increases ie the element edge length decreases the values converge towards a final solution The von Mises stress at the top of the hole in the plate was found to be approximatly 38 MPa This is a mere 25 difference between the analytical solution and the solution found using ANSYS The approximate maximum displacement was found to be 00012 mm this is 20 greater than the analytical solution However the analytical solution does not account for the large hole in the center of the plate which was expected to significantly increase the deflection at the end of the plate Therefore the results using ANSYS were determined to be appropriate for the verification model 3 Deformation H General Postproc Plot Results Deformed Shape Def undeformd to view both the deformed and the undeformed object H Observe the locations of deflection 4 Deflection H General Postproc Plot Results Nodal Solution Then select DOF solution USUM in the window H Alternatively obtain these results as a list General Postproc List Results Nodal Solution H Are these results what you expected Note that all translational degrees of freedom were constrained to zero at the left end of the plate 5 Stresses H General Postproc Plot Results Nodal Solution Then select Stress von Mises in the window H You can list the von Mises stresses to verify the results at certain nodes General Postproc List Results Select Stress Principals SPRIN Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Bracket Example Now we will return to the analysis of the bracket A combination of GUI and the Command line will be used for this example The problem to be modeled in this example is a simple bracket shown in the following figure This bracket is to be built from a 20 mm thick steel plate A figure of the plate is shown below This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right Preprocessing Defining the Problem 1 Give the Bracket example a Title Utility Menu File Change Title 2 Form Geometry Again Boolean operations will be used to create the basic geometry of the Bracket a Create the main rectangular shape The main rectangular shape has a width of 80 mm a height of 100mm and the bottom left corner is located at coordinates 00 I Ensure that the Preprocessor menu is open Alternatively type PREP7 into the command line window I Now instead of using the GUI window we are going to enter code into the command line Now I will explain the line required to create a rectangle BLC4 XCORNER YCORNER WIDTH HEIGHT BLC4 X coord bottom left Y coord bottom left width height I Therefore the command line for this rectangle is BLC40080100 b Create the circular end on the right hand side The center of the circle is located at 8050 and has a radius of 50 mm The following code is used to create a circular area CYL4 XCENTER YCENTER RAD1 CYL4 X coord for the center Y coord for the center radius I Therefore the command line for this circle is CYL4805050 c Now create a second and third circle for the left hand side using the following dimensions parameter circle 2 circle 3 XCENTER 0 0 YCENTER 20 80 RADIUS 20 20 d Create a rectangle on the left hand end to fill the gap between the two small circles XCORNER 20 YCORNER 20 WIDTH 20 HEIGHT 60 Your screen should now look like the following e Boolean Operations Addition We now want to add these five discrete areas together to form one area I To perform the Boolean operation from the Preprocessor menu select Modeling Operate Booleans Add Areas I In the Add Areas window click on Pick All Alternatively the command line code for the above step is AADDALL You should now have the following model f Create the Bolt Holes We now want to remove the bolt holes from this plate I Create the three circles with the parameters given below parameter circle 1 circle 2 circle 3 WP X 80 0 0 WP Y 50 20 80 radius 30 10 10 I Now select Preprocessor Modeling Operate Booleans Subtract Areas I Select the base areas from which to subract the large plate that was created I Next select the three circles that we just created Click on the three circles that you just created and click OK Alternatively the command line code for the above step is ASBA6ALL Now you should have the following 3 Define the Type of Element As in the verification model PLANE82 will be used for this example H Preprocessor Element Type AddEditDelete H Use the Options button to get a plane stress element with thickness Alternatively the command line code for the above step is ET1PLANE82 followed by KEYOPT133 H Under the Extra Element Output K5 select nodal stress 4 Define Geometric Contants H Preprocessor Real Constants AddEditDelete H Enter a thickness of 20mm Alternatively the command line code for the above step is R120 5 Element Material Properties H Preprocessor Material Props Material Library Structural Linear Elastic Isotropic We are going to give the properties of Steel Enter the following when prompted EX 200000 PRXY 03 The command line code for the above step is MPEX1200000 followed by MPPRXY103 6 Mesh Size H Preprocessor Meshing Size Cntrls Manual Size Areas All Areas H Select an element edge length of 5 Again we will need to make sure the model has converged Alternatively the command line code for the above step is AESIZEALL5 7 Mesh H Preprocessor Meshing Mesh Areas Free and select the area when prompted Alternatively the command line code for the above step is AMESHALL Saving Your Job Utility Menu File Save as Solution Phase Assigning Loads and Solving You have now defined your model It is now time to apply the loads and constraints and solve the the resulting system of equations 1 Define Analysis Type H Solution New Analysis and select Static Alternatively the command line code for the above step is ANTYPE0 2 Apply Constraints As illustrated the plate is fixed at both of the smaller holes on the left hand side H Solution Define Loads Apply Structural Displacement On Nodes H Instead of selecting one node at a time you have the option of creating a box polygon or circle of which all the nodes in that area will be selected For this case select circle as shown in the window below You may want to zoom in to select the points Utilty Menu PlotCtrls Pan Zoom Rotate Click at the center of the bolt hole and drag the circle out so that it touches all of the nodes on the border of the hole H Click on Apply in the Apply UROT on Lines window and constrain all DOFs in the Apply UROT on Nodes window H Repeat for the second bolt hole 3 Apply Loads As shown in the diagram there is a single vertical load of 1000N at the bottom of the large bolt hole Apply this force to the respective keypoint Solution Define Loads Apply Structural ForceMoment On Keypoints Select a force in the y direction of 1000 The applied loads and constraints should now appear as shown below 4 Solving the System Solution Solve Current LS PostProcessing Viewing the Results We are now ready to view the results We will take a look at the deflected shape and the stress contours once we determine convergence has occured 1 Convergence using ANSYS As shown previously it is necessary to prove that the solution has converged Reduce the mesh size until there is no longer a sizeable change in your convergence criteria 2 Deformation H General Postproc Plot Results Def undeformed to view both the deformed and the undeformed object The graphic should be similar to the following H Observe the locations of deflection Ensure that the deflection at the bolt hole is indeed 0 3 Deflection H To plot the nodal deflections use General Postproc Plot Results Contour Plot Nodal Solution then select DOF Solution USUM in the window H Alternatively obtain these results as a list General Postproc List Results Nodal Solution H Are these results what you expected Note that all translational degrees of freedom were constrained to zero at the bolt holes 4 Stresses H General Postproc Plot Results Nodal Solution Then select von Mises Stress in the window H You can list the von Mises stresses to verify the results at certain nodes General Postproc List Results Select Stress Principals SPRIN Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Quitting ANSYS To quit ANSYS click QUIT on the ANSYS Toolbar or select Utility Menu File Exit In the window that appears select Save Everything assuming that you want to and then click OK UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Two Dimensional Truss Bicycle Space Frame Plane Stress Bracket Modeling Tools Solid Modeling Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Solid Model Creation Introduction This tutorial is the last of three basic tutorials devised to illustrate commom features in ANSYS Each tutorial builds upon techniques covered in previous tutorials it is therefore essential that you complete the tutorials in order The Solid Modelling Tutorial will introduce various techniques which can be used in ANSYS to create solid models Filleting extrusion sweeping copying and working plane orientation will be covered in detail Two Solid Models will be created within this tutorial Problem Description A We will be creating a solid model of the pulley shown in the following figure Geometry Generation We will create this model by first tracing out the cross section of the pulley and then sweeping this area about the y axis Creation of Cross Sectional Area 1 Create 3 Rectangles Main Menu Preprocessor Modeling Create Rectangle By 2 Corners BLC4 XCORNER YCORNER WIDTH HEIGHT The geometry of the rectangles Rectangle 1 Rectangle 2 Rectangle 3 WP X XCORNER 2 3 8 WP Y YCORNER 0 2 0 WIDTH 1 5 05 HEIGHT 55 1 5 You should obtain the following 2 Add the Areas Main Menu Preprocessor Modeling Operate Boolean Add Areas AADD ALL ANSYS will label the united area as AREA 4 and the previous three areas will be deleted 3 Create the rounded edges using circles Preprocessor Modeling Create Areas Circle Solid circles CYL4XCENTERYCENTERRAD The geometry of the circles Circle 1 Circle 2 WP X XCENTER 3 85 WP Y YCENTER 55 02 RADIUS 05 02 4 Subtract the large circle from the base Preprocessor Operate Subtract Areas ASBABASESUBTRACT 5 Copy the smaller circle for the rounded edges at the top Preprocessor Modeling Copy Areas H Click on the small circle and then on OK H The following window will appear It asks for the xy and z offset of the copied area Enter the y offset as 46 and then click OK H Copy this new area now with an x offset of 05 You should obtain the following 6 Add the smaller circles to the large area Preprocessor Operate Add Areas AADDALL 7 Fillet the inside edges of the top half of the area Preprocessor Create Lines Line Fillet H Select the two lines shown below and click on OK H The following window will appear prompting for the fillet radius Enter 01 H Follow the same procedure and create a fillet with the same radius between the following lines 8 Create the fillet areas H As shown below zoom into the fillet radius and plot and number the lines Preprocessor Modeling Create Areas Arbitrary By Lines H Select the lines as shown below H Repeat for the other fillet 9 Add all the areas together Preprocessor Operate Add Areas AADDALL 10 Plot the areas Utility Menu Plot Areas Sweep the Cross Sectional Area Now we need to sweep the area around a y axis at x0 and z0 to create the pulley 1 Create two keypoints defining the y axis Create keypoints at 000 and 050 and number them 1001 and 1002 respectively KXYZ 2 By default the graphics will now show all keypoints Plot Areas 3 Sweep the area about the y axis Preprocessor Modeling Operate Extrude Areas About axis H You will first be prompted to select the areas to be swept so click on the area H Then you will be asked to enter or pick two keypoints defining the axis H Plot the Keypoints Utility Menu Plot Keypoints Then select the following two keypoints H The following window will appear prompting for sweeping angles Click on OK You should now see the following in the graphics screen Create Bolt Holes 1 Change the Working Plane By default the working plane in ANSYS is located on the global Cartesian XY plane However for us to define the bolt holes we need to use a different working plane There are several ways to define a working plane one of which is to define it by three keypoints H Create the following Keypoints X Y Z 2001 0 3 0 2002 1 3 0 2003 0 3 1 H Switch the view to top view and plot only keypoints 2 Align the Working Plane with the Keypoints Utility Menu WorkPlane Align WP with Keypoints H Select Keypoints 2001 then 2002 then 2003 IN THAT ORDER The first keypoint 2001 defines the origin of the working plane coordinate system the second keypoint 2002 defines the xaxis orientation while the third 2003 defines the orientation of the working plane The following warning will appear when selecting the keypoint at the origin as there are more than one in this location Just click on Next until the one selected is 2001 H Once you have selected the 3 keypoints and clicked OK the WP symbol green should appear in the Graphics window Another way to make sure the active WP has moves is Utility Menu WorkPlane Show WP Status note the origin of the working plane By default those values would be 000 3 Create a Cylinder solid cylinder with x55 y0 r05 depth1 You should see the following in the graphics screen We will now copy this volume so that we repeat it every 45 degrees Note that you must copy the cylinder before you use boolean operations to subtract it because you cannot copy an empty space 4 We need to change active CS to cylindrical Y Utility Menu WorkPlane Change Active CS to Global Cylindrical Y This will allow us to copy radially about the Y axis 5 Create 8 bolt Holes Preprocessor Copy Volumes H Select the cylinder volume and click on OK The following window will appear fill in the blanks as shown Youi should obtain the following model H Subtract the cylinders from the pulley hub Boolean operations to create the boltholes This will result in the following completed structure Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Problem Description B We will be creating a solid model of the Spindle Base shown in the following figure Geometry Generation We will create this model by creating the base and the back and then the rib Create the Base 1 Create the base rectangle WP X XCORNER WP Y YCORNER WIDTH HEIGHT 0 0 109 102 2 Create the curved edge using keypoints and lines to create an area H Create the following keypoints X Y Z Keypoint 5 20 82 0 Keypoint 6 20 20 0 Keypoint 7 0 82 0 Keypoint 8 0 20 0 You should obtain the following H Create arcs joining the keypoints Main Menu Preprocessor Modeling Create Lines Arcs By End KPs Rad I Select keypoints 4 and 5 either click on them or type 45 into the command line when prompted I Select Keypoint 7 as the centerofcurvature when prompted I Enter the radius of the arc 20 in the Arc by End KPs Radius window I Repeat to create an arc from keypoints 1 and 6 Alternatively type LARC45720 followed by LARC16820 into the command line H Create a line from Keypoint 5 to 6 Main Menu Preprocessor Modeling Create Lines Lines Straight Line L56 H Create an Arbitrary area within the bounds of the lines Main Menu Preprocessor Modeling Create Areas Arbitrary By Lines AL4567 H Combine the 2 areas into 1 to form Area 3 Main Menu Preprocessor Modeling Operate Booleans Add Volumes AADD12 You should obtain the following image 3 Create the 4 holes in the base We will make use of the copy feature in ANSYS to create all 4 holes H Create the bottom left circle XCENTER0 YCENTER20 RADIUS10 H Copy the area to create the bottom right circle DX69 AGEN Copies include originalAreaArea2 if 2 areas to be copiedDXDYDZ H Copy both circles to create the upper circles DY62 H Subtract the three circles from the main base ASBA3ALL You should obtain the following 4 Extrude the base Preprocessor Modeling Operate Extrude Areas Along Normal The following window will appear once you select the area H Fill in the window as shown length of extrusion 26mm Note to extrude the area in the negative z direction you would simply enter 26 Alternatively type VOFFST626 into the command line Create the Back 1 Change the working plane As in the previous example we need to change the working plane You may have observed that geometry can only be created in the XY plane Therefore in order to create the back of the Spindle Base we need to create a new working plane where the XY plane is parallel to the back Again we will define the working plane by aligning it to 3 Keypoints H Create the following keypoints X Y Z 100 109 102 0 101 109 2 0 102 159 102 sqrt3002 H Align the working plane to the 3 keypoints Recall when defining the working plane the first keypoint defines the origin the second keypoint defines the xaxis orientation while the third defines the orientation of the working plane Alternatively type KWPLAN1100101102 into the command line 2 Create the back area H Create the base rectangle XCORNER0 YCORNER0 WIDTH102 HEIGHT180 H Create a circle to obtain the curved top XCENTER51 YCENTER180 RADIUS51 H Add the 2 areas together 3 Extrude the area length of extrusion 26mm Preprocessor Modeling Operate Extrude Areas Along Normal VOFFST2726 4 Add the base and the back together H Add the two volumes together Preprocessor Modeling Operate Booleans Add Volumes VADD12 You should now have the following geometry Note that the planar areas between the two volumes were not added together H Add the planar areas together dont forget the other side Preprocessor Modeling Operate Booleans Add Areas AADD Area 1 Area 2 Area 3 5 Create the Upper Cylinder H Create the outer cylinder XCENTER51 YCENTER180 RADIUS32 DEPTH60 Preprocessor Modeling Create Volumes Cylinder Solid Cylinder CYL45118032 60 H Add the volumes together H Create the inner cylinder XCENTER51 YCENTER180 RADIUS185 DEPTH60 H Subtract the volumes to obtain a hole You should now have the following geometry Create the Rib 1 Change the working plane H First change the active coordinate system back to the global coordinate system this will make it easier to align to the new coordinate system Utility Menu WorkPlane Align WP with Global Cartesian Alternatively type WPCSYS10 into the command line H Create the following keypoints X Y Z 200 20 61 26 201 0 61 26 202 20 61 30 H Align the working plane to the 3 keypoints Recall when defining the working plane the first keypoint defines the origin the second keypoint defines the xaxis orientation while the third defines the orientation of the working plane Alternatively type KWPLAN1200201202 into the command line 2 Change active coordinate system We now need to update the coordiante system to follow the working plane changes ie make the new Work Plane origin the active coordinate Utility Menu WorkPlane Change Active CS to Working Plane CSYS4 3 Create the area H Create the keypoints corresponding to the vertices of the rib X Y Z 203 12905773526 0 0 204 12905773526 38 sqrt3276 0 H Create the rib area through keypoints 200 203 204 Preprocessor Modeling Create Areas Arbitrary Through KPs A200203204 4 Extrude the area length of extrusion 20mm 5 Add the volumes together You should obtain the following Quitting ANSYS To quit ANSYS select QUIT from the ANSYS Toolbar or select Utility MenuFileExit In the dialog box that appears click on Save Everything assuming that you want to and then click on OK UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Effect of Self Weight on a Cantilever Beam Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the required steps to account for the weight of an object in ANSYS Loads will not be applied to the beam shown below in order to observe the deflection caused by the weight of the beam itself The beam is to be made of steel with a modulus of elasticity of 200 GPa Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title Effects of Self Weight for a Cantilever Beam 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 ANSYS Inc Copyright 2001 University of Alberta 3 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxyz We are going to define 2 keypoints for this beam as given in the following table Keypoint Coordinates xyz 1 00 2 10000 4 Create Lines Preprocessor Modeling Create Lines Lines In Active Coord L12 Create a line joining Keypoints 1 and 2 5 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axes and rotation about the Z axis 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 500 ii Area moment of inertia IZZ 416667 iii Total beam height 10 This defines a beam with a height of 10 mm and a width of 50 mm 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 8 Define Element Density Preprocessor Material Props Material Models Structural Linear Density In the window that appears enter the following density for steel i Density DENS 786e6 9 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will use an element edge length of 100mm 10 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix keypoint 1 ie all DOF constrained 3 Define Gravity It is necessary to define the direction and magnitude of gravity for this problem H Select Solution Define Loads Apply Structural Inertia Gravity H The following window will appear Fill it in as shown to define an acceleration of 981ms2 in the y direction Note Acceleration is defined in terms of meters not mm as used throughout the problem This is because the units of acceleration and mass must be consistent to give the product of force units Newtons in this case Also note that a positive acceleration in the y direction stimulates gravity in the negative Y direction There should now be a red arrow pointing in the positive y direction This indicates that an acceleration has been defined in the y direction DK1ALL0 ACEL98 The applied loads and constraints should now appear as shown in the figure below 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Hand Calculations Hand calculations were performed to verify the solution found using ANSYS The maximum deflection was shown to be 5777mm 2 Show the deformation of the beam General Postproc Plot Results Deformed Shape Def undef edge PLDISP2 As observed in the upper left hand corner the maximum displacement was found to be 5777mm This is in agreement with the theortical value Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Application of Distributed Loads Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data Please note that this material was also covered in the Bicycle Space Frame tutorial under Basic Tutorials A distributed load of 1000 Nm 1 Nmm will be applied to a solid steel beam with a rectangular cross section as shown in the figure below The crosssection of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa ANSYS Inc Copyright 2001 University of Alberta Preprocessing Defining the Problem 1 Open preprocessor menu PREP7 2 Give example a Title Utility Menu File Change Title title Distributed Loading 3 Create Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxy We are going to define 2 keypoints the beam vertices for this structure as given in the following table Keypoint Coordinates xy 1 00 2 10000 4 Define Lines Preprocessor Modeling Create Lines Lines Straight Line LKK Create a line between Keypoint 1 and Keypoint 2 5 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 element This element has 3 degrees of freedom translation along the X and Y axiss and rotation about the Z axis With only 3 degrees of freedom the BEAM3 element can only be used in 2D analysis 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 100 ii Area Moment of Inertia IZZ 833333 iii Total beam height HEIGHT 10 This defines an element with a solid rectangular cross section 10mm x 10mm 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 8 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will use an element length of 100mm 9 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All 10 Plot Elements Utility Menu Plot Elements You may also wish to turn on element numbering and turn off keypoint numbering Utility Menu PlotCtrls Numbering Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Pin Keypoint 1 ie UX and UY constrained and fix Keypoint 2 in the y direction UY constrained 3 Apply Loads We will apply a distributed load of 1000 Nm or 1 Nmm over the entire length of the beam H Select Solution Define Loads Apply Structural Pressure On Beams H Click Pick All in the Apply FM window H As shown in the following figure enter a value of 1 in the field VALI Pressure value at node I then click OK The applied loads and constraints should now appear as shown in the figure below Note To have the constraints and loads appear each time you select Replot you must change some settings Select Utility Menu PlotCtrls Symbols In the window that appears select Pressures in the pull down menu of the Surface Load Symbols section 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Plot Deformed Shape General Postproc Plot Results Deformed Shape PLDISP2 2 Plot Principle stress distribution As shown previously we need to use element tables to obtain principle stresses for line elements 1 Select General Postproc Element Table Define Table 2 Click Add 3 In the window that appears a enter SMAXI in the User Label for Item section b In the first window in the Results Data Item section scroll down and select By sequence num c In the second window of the same section select NMISC d In the third window enter 1 anywhere after the comma 4 click Apply 5 Repeat steps 2 to 4 but change SMAXI to SMAXJ in step 3a and change 1 to 3 in step 3d 6 Click OK The Element Table Data window should now have two variables in it 7 Click Close in the Element Table Data window 8 Select General Postproc Plot Results Line Elem Res 9 Select SMAXI from the LabI pull down menu and SMAXJ from the LabJ pull down menu Note H ANSYS can only calculate the stress at a single location on the element For this example we decided to extract the stresses from the I and J nodes of each element These are the nodes that are at the ends of each element H For this problem we wanted the principal stresses for the elements For the BEAM3 element this is categorized as NMISC 1 for the I nodes and NMISC 3 for the J nodes A list of available codes for each element can be found in the ANSYS help files ie type help BEAM3 in the ANSYS Input window As shown in the plot below the maximum stress occurs in the middle of the beam with a value of 750 MPa Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta NonLinear Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam shown below There are several causes for nonlinear behaviour such as Changing Status ex contact elements Material Nonlinearities and Geometric Nonlinearities change in response due to large deformations This tutorial will deal specifically with Geometric Nonlinearities To solve this problem the load will added incrementally After each increment the stiffness matrix will be adjusted before increasing the load The solution will be compared to the equivalent solution using a linear response Preprocessing Defining the Problem ANSYS Inc Copyright 2001 University of Alberta 1 Give example a Title Utility Menu File Change Title 2 Create Keypoints Preprocessor Modeling Create Keypoints In Active CS We are going to define 2 keypoints the beam vertices for this structure to create a beam with a length of 5 inches Keypoint Coordinates xy 1 00 2 50 3 Define Lines Preprocessor Modeling Create Lines Lines Straight Line Create a line between Keypoint 1 and Keypoint 2 4 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axiss and rotation about the Z axis With only 3 degrees of freedom the BEAM3 element can only be used in 2D analysis 5 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 003125 ii Area Moment of Inertia IZZ 4069e5 iii Total beam height HEIGHT 0125 This defines an element with a solid rectangular cross section 025 x 0125 inches 6 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 30e6 ii Poissons Ratio PRXY 03 If you are wondering why a Linear model was chosen when this is a nonlinear example it is because this example is for nonlinear geometry not nonlinear material properties If we were considering a block of wood for example we would have to consider nonlinear material properties 7 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will specify an element edge length of 01 50 element divisions along the line 8 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All LMESHALL Solution Assigning Loads and Solving 1 Define Analysis Type Solution New Analysis Static ANTYPE0 2 Set Solution Controls H Select Solution Analysis Type Soln Control The following image will appear Ensure the following selections are made as shown above A Ensure Large Static Displacements are permitted this will include the effects of large deflection in the results B Ensure Automatic time stepping is on Automatic time stepping allows ANSYS to determine appropriate sizes to break the load steps into Decreasing the step size usually ensures better accuracy however this takes time The Automatic Time Step feature will determine an appropriate balance This feature also activates the ANSYS bisection feature which will allow recovery if convergence fails C Enter 5 as the number of substeps This will set the initial substep to 15 th of the total load The following example explains this Assume that the applied load is 100 lbin If the Automatic Time Stepping was off there would be 5 load steps each increasing by 15 th of the total load I 20 lbin I 40 lbin I 60 lbin I 80 lbin I 100 lbin Now with the Automatic Time Stepping is on the first step size will still be 20 lbin However the remaining substeps will be determined based on the response of the material due to the previous load increment D Enter a maximum number of substeps of 1000 This stops the program if the solution does not converge after 1000 steps E Enter a minimum number of substeps of 1 F Ensure all solution items are writen to a results file NOTE There are several options which have not been changed from their default values For more information about these commands type help followed by the command into the command line Function Command Comments Load Step KBC Loads are either linearly interpolated ramped from the one substep to another ie the load will increase from 10 lbs to 20 lbs in a linear fashion or they are step functions ie the load steps directly from 10 lbs to 20 lbs By default the load is ramped You may wish to use the stepped loading for ratedependent behaviour or transient load steps Output OUTRES This command controls the solution data written to the database By default all of the solution items are written at the end of each load step You may select only a specific iten ie Nodal DOF solution to decrease processing time Stress Stiffness SSTIF This command activates stress stiffness effects in nonlinear analyses When large static deformations are permitted as they are in this case stress stiffening is automatically included For some special nonlinear cases this can cause divergence because some elements do not provide a complete consistent tangent Newton Raphson NROPT By default the program will automatically choose the NewtonRaphson options Options include the full NewtonRaphson the modified NewtonRaphson the previously computed matrix and the full NewtonRaphson with unsymmetric matrices of elements Convergence Values CNVTOL By default the program checks the outofbalance load for any active DOF 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 ie all DOFs constrained 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Place a 100 lbin moment in the MZ direction at the right end of the beam Keypoint 2 5 Solve the System Solution Solve Current LS SOLVE The following will appear on your screan for NonLinear Analyses This shows the convergence of the solution General Postprocessing Viewing the Results 1 View the deformed shape General Postproc Plot Results Deformed Shape Def undeformed PLDISP1 2 View the deflection contour plot General Postproc Plot Results Contour Plot Nodal Solu DOF solution UY PLNSOLUY01 3 List Horizontal Displacement If this example is performed as a linear model there will be no nodal deflection in the horizontal direction due to the small deflections assumptions However this is not realistic for large deflections Modeling the system nonlinearly these horizontal deflections are calculated by ANSYS General Postproc List Results Nodal Solution DOF solution UX Other results can be obtained as shown in previous linear static analyses Time History Postprocessing Viewing the Results As shown you can obtain the results such as deflection stress and bending moment diagrams the same way you did in previous examples using the General Postprocessor However you may wish to view time history results such as the deflection of the object and the step sizes of the load As you recall the load was applied in steps The step size was automatically determined in ANSYS 1 Define Variables H Select TimeHist Postpro Define Variables Add Nodal DOF results H Select Keypoint 2 Node 2 when prompted H Complete the following window as shown to define the translational displacement in the y direction Translational displacement of node 2 is now stored as variable 2 variable 1 being time 2 Graph Results over time H Select TimeHist Postpro Graph Variables H Enter 2 UY as the 1st variable to graph shown below 1st variable to graph 2nd variable 3rd variable 4th variable 5th variable 6th variable 7th variable 8th variable 9th variable 10th variable Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Graphical Solution Tracking Introduction This tutorial was completed using ANSYS 70 This will act as an explanation of what the Graphical Solution Tracking plot is acutally describing An example of such a plot is shown below and will be used throughout the explanation 1 Title and Axis Labels The title of the graph is really just the time value of the last calculated iteration In this example the time at the end of the analysis was set to 1 This can be changed with the Time command before the Solve command is issued For more information regarding setting the time value and many other solution control option see Chapter 85 of the Structural Analysis Guide in the Help file ANSYS Inc Copyright 2001 University of Alberta The xaxis is labelled Cumulative Iteration Number As ANSYS steps through nonlinear analysis it uses a solver NewtonRaphson etc that iterates to find a solution If the problem is relatively linear very few iterations will be required and thus the length of the graph will be small However if the solution is highly nonlinear or is not converging many iterations will be required The length of the graph in these cases can be quite long Again for more information about changing iteration settings you can see Chapter 85 in the help file The yaxis is labelled Absolute Convergence Norm In the case of a structural analysis which this graph is taken from this absolute convergence norm refers to nonnormalized values ie there are units associated with these values Some analyses use normalized values In reality it doesnt really matter because it is only a comparison that is going on This is what will be explained next 2 Curves and Legend As can be guessed from the legend labels this graph relates to forces and moments These values are graphed because they are the corresponding values in the solution vector for the DOFs that are active in the elements being used If this graph were from a thermal analysis the curves may be for temperature For each parameter there are two curves plotted For ease of explanation we will look at the force curves I The F CRIT curve refers to the convergence criteria force value This value is equal to the product of VALUE x TOLER The default value of VALUE is the square root of the sum of the squares SRSS of the applied loads or MINREF which defaults to 0001 which ever is greater This value can be changed using the CNVTOL command which is discussed in the help file The value of TOLER defaults to 05 for loads One may inquire why the F CRIT value increases as the number of iterations increases This is because the analysis is made up of a number of substeps In the case of a structural example such as this these substeps are basically portions of the total load being applied over time For instance a 100N load broken up with 20 substeps means 20 5N loads will be applied consequtively until the entire 100N is applied Thus the F CRIT value at the start will be 120th of the final F CRIT value I The F L2 curve refers to the L2 Vector Norm of the forces The L2 norm is the SRSS of the force imbalances for all DOFs In simpler terms this is the SRSS of the difference between the calculated internal force at a particular DOF and the external force in that direction For each substep ANSYS iterates until the F L2 value is below the F CRIT value Once this occurs it is deemed the solution is within tolerance of the correct solution and it moves on to the next substep Generally when the curves peak this is the start of a new substep As can be seen in the graph above a peak follow everytime the L2 value drops below the CRIT value as expected UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Buckling Introduction This tutorial was created using ANSYS 70 to solve a simple buckling problem It is recommended that you complete the NonLinear Tutorial prior to beginning this tutorial Buckling loads are critical loads where certain types of structures become unstable Each load has an associated buckled mode shape this is the shape that the structure assumes in a buckled condition There are two primary means to perform a buckling analysis 1 Eigenvalue Eigenvalue buckling analysis predicts the theoretical buckling strength of an ideal elastic structure It computes the structural eigenvalues for the given system loading and constraints This is known as classical Euler buckling analysis Buckling loads for several configurations are readily available from tabulated solutions However in reallife structural imperfections and nonlinearities prevent most realworld structures from reaching their eigenvalue predicted buckling strength ie it overpredicts the expected buckling loads This method is not recommended for accurate realworld buckling prediction analysis 2 Nonlinear Nonlinear buckling analysis is more accurate than eigenvalue analysis because it employs nonlinear largedeflection static analysis to predict buckling loads Its mode of operation is very simple it gradually increases the applied load until a load level is found whereby the structure becomes unstable ie suddenly a very small increase in the load will cause very large deflections The true nonlinear nature of this analysis thus permits the modeling of geometric imperfections load perterbations material nonlinearities and gaps For this type of analysis note that small offaxis loads are necessary to initiate the desired buckling mode ANSYS Inc Copyright 2001 University of Alberta This tutorial will use a steel beam with a 10 mm X 10 mm cross section rigidly constrained at the bottom The required load to cause buckling applied at the topcenter of the beam will be calculated Eigenvalue Buckling Analysis Preprocessing Defining the Problem 1 Open preprocessor menu PREP7 2 Give example a Title Utility Menu File Change Title titleEigenValue Buckling Analysis 3 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS KXY We are going to define 2 Keypoints for this beam as given in the following table Keypoints Coordinates xy 1 00 2 0100 4 Create Lines Preprocessor Modeling Create Lines Lines In Active Coord L12 Create a line joining Keypoints 1 and 2 5 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axes and rotation about the Z axis 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 100 ii Area moment of inertia IZZ 833333 iii Total Beam Height HEIGHT 10 This defines a beam with a height of 10 mm and a width of 10 mm 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 8 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will specify an element edge length of 10 mm 10 element divisions along the line 9 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All LMESHALL Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Activate prestress effects To perform an eigenvalue buckling analysis prestress effects must be activated H You must first ensure that you are looking at the unabridged solution menu so that you can select Analysis Options in the Analysis Type submenu The last option in the solution menu will either be Unabridged menu which means you are currently looking at the abridged version or Abriged Menu which means you are looking at the unabridged menu If you are looking at the abridged menu select the unabridged version H Select Solution Analysis Type Analysis Options H In the following window change the SSTIFPSTRES item to Prestress ON which ensures the stress stiffness matrix is calculated This is required in eigenvalue buckling analysis 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 ie all DOF constrained 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints The eignenvalue solver uses a unit force to determine the necessary buckling load Applying a load other than 1 will scale the answer by a factor of the load Apply a vertical FY point load of 1 N to the top of the beam keypoint 2 The applied loads and constraints should now appear as shown in the figure below 5 Solve the System Solution Solve Current LS SOLVE 6 Exit the Solution processor Close the solution menu and click FINISH at the bottom of the Main Menu FINISH Normally at this point you enter the postprocessing phase However with a buckling analysis you must reenter the solution phase and specify the buckling analysis Be sure to close the solution menu and reenter it or the buckling analysis may not function properly 7 Define Analysis Type Solution Analysis Type New Analysis Eigen Buckling ANTYPE1 8 Specify Buckling Analysis Options H Select Solution Analysis Type Analysis Options H Complete the window which appears as shown below Select Block Lanczos as an extraction method and extract 1 mode The Block Lanczos method is used for large symmetric eigenvalue problems and uses the sparse matrix solver The Subspace method could also be used however it tends to converge slower as it is a more robust solver In more complex analyses the Block Lanczos method may not be adequate and the Subspace method would have to be used 9 Solve the System Solution Solve Current LS SOLVE 10 Exit the Solution processor Close the solution menu and click FINISH at the bottom of the Main Menu FINISH Again it is necessary to exit and reenter the solution phase This time however is for an expansion pass An expansion pass is necessary if you want to review the buckled mode shapes 11 Expand the solution H Select Solution Analysis Type Expansion Pass and ensure that it is on You may have to select the Unabridged Menu again to make this option visible H Select Solution Load Step Opts ExpansionPass Single Expand Expand Modes H Complete the following window as shown to expand the first mode 12 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 View the Buckling Load To display the minimum load required to buckle the beam select General Postproc List Results Detailed Summary The value listed under TIMEFREQ is the load 41123 which is in Newtons for this example If more than one mode was selected in the steps above the corresponding loads would be listed here as well POST1 SETLIST 2 Display the Mode Shape H Select General Postproc Read Results Last Set to bring up the data for the last mode calculated H Select General Postproc Plot Results Deformed Shape NonLinear Buckling Analysis Ensure that you have completed the NonLinear Tutorial prior to beginning this portion of the tutorial Preprocessing Defining the Problem 1 Open preprocessor menu PREP7 2 Give example a Title Utility Menu File Change Title TITLE Nonlinear Buckling Analysis 3 Create Keypoints Preprocessor Modeling Create Keypoints In Active CS KXY We are going to define 2 keypoints the beam vertices for this structure to create a beam with a length of 100 millimeters Keypoint Coordinates xy 1 00 2 0100 4 Define Lines Preprocessor Modeling Create Lines Lines Straight Line Create a line between Keypoint 1 and Keypoint 2 L12 5 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axiss and rotation about the Z axis With only 3 degrees of freedom the BEAM3 element can only be used in 2D analysis 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 100 ii Area Moment of Inertia IZZ 833333 iii Total beam height HEIGHT 10 This defines an element with a solid rectangular cross section 10 x 10 millimeters 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200e3 ii Poissons Ratio PRXY 03 8 Define Mesh Size Preprocessor Meshing Size Cntrls Lines All Lines For this example we will specify an element edge length of 1 mm 100 element divisions along the line ESIZE1 9 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All LMESHALL Solution Assigning Loads and Solving 1 Define Analysis Type Solution New Analysis Static ANTYPE0 2 Set Solution Controls H Select Solution Analysis Type Soln Control The following image will appear Ensure the following selections are made under the Basic tab as shown above A Ensure Large Static Displacements are permitted this will include the effects of large deflection in the results B Ensure Automatic time stepping is on Automatic time stepping allows ANSYS to determine appropriate sizes to break the load steps into Decreasing the step size usually ensures better accuracy however this takes time The Automatic Time Step feature will determine an appropriate balance This feature also activates the ANSYS bisection feature which will allow recovery if convergence fails C Enter 20 as the number of substeps This will set the initial substep to 120 th of the total load D Enter a maximum number of substeps of 1000 This stops the program if the solution does not converge after 1000 steps E Enter a minimum number of substeps of 1 F Ensure all solution items are writen to a results file Ensure the following selection is made under the Nonlinear tab as shown below A Ensure Line Search is On This option is used to help the NewtonRaphson solver converge B Ensure Maximum Number of Iterations is set to 1000 NOTE There are several options which have not been changed from their default values For more information about these commands type help followed by the command into the command line 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 ie all DOFs constrained 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Place a 50000 N load in the FY direction on the top of the beam Keypoint 2 Also apply a 250 N load in the FX direction on Keypoint 2 This horizontal load will persuade the beam to buckle at the minimum buckling load The model should now look like the window shown below 5 Solve the System Solution Solve Current LS SOLVE The following will appear on your screen for NonLinear Analyses This shows the convergence of the solution General Postprocessing Viewing the Results 1 View the deformed shape H To view the element in 2D rather than a line Utility Menu PlotCtrls Style Size and Shape and turn Display of element ON as shown below H General Postproc Plot Results Deformed Shape Def undeformed PLDISP1 H View the deflection contour plot General Postproc Plot Results Contour Plot Nodal Solu DOF solution UY PLNSOLUY01 Other results can be obtained as shown in previous linear static analyses Time History Postprocessing Viewing the Results As shown you can obtain the results such as deflection stress and bending moment diagrams the same way you did in previous examples using the General Postprocessor However you may wish to view time history results such as the deflection of the object over time 1 Define Variables H Select Main Menu TimeHist Postpro The following window should open automatically If it does not open automatically select Main Menu TimeHist Postpro Variable Viewer H Click the add button in the upper left corner of the window to add a variable H Doubleclick Nodal Solution DOF Solution YComponent of displacement as shown below and click OK Pick the uppermost node on the beam and click OK in the Node for Data window H To add another variable click the add button again This time select Reaction Forces Structural Forces Y Component of Force Pick the lowermost node on the beam and click OK H On the Time History Variable window click the circle in the XAxis column for FY3 This will make the reaction force the xvariable The Time History Variables window should now look like this 2 Graph Results over Time H Click on UY2 in the Time History Variables window H Click the graphing button in the Time History Variables window H The labels on the plot are not updated by ANSYS so you must change them manually Select Utility Menu Plot Ctrls Style Graphs Modify Axes and relabel the X and Yaxis appropriately The plot shows how the beam became unstable and buckled with a load of approximately 40000 N the point where a large deflection occured due to a small increase in force This is slightly less than the eigenvalue solution of 41123 N which was expected due to nonlinear geometry issues discussed above Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc NonLinear Materials Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model For instance the case when a large force is applied resulting in a stresses greater than yield strength In such a case a multilinear stressstrain relationship can be included which follows the stressstrain curve of the material being used This will allow ANSYS to more accurately model the plastic deformation of the material For this analysis a simple tension speciment 100 mm X 5 mm X 5 mm is constrained at the bottom and has a load pulling on the top This specimen is made out of a experimental substance called WhoKilledKenium The stressstrain curve for the substance is shown above Note the linear section up to approximately 225 MPa where the Youngs Modulus is constant 75 GPa The material then begins to yield and the relationship becomes plastic and nonlinear Preprocessing Defining the Problem Copyright 2001 University of Alberta 1 Give example a Title Utility Menu File Change Title title NonLinear Materials 2 Create Keypoints Preprocessor Modeling Create Keypoints In Active CS PREP7 KXY We are going to define 2 keypoints the beam vertices for this structure to create a beam with a length of 100 millimeters Keypoint Coordinates xy 1 00 2 0100 3 Define Lines Preprocessor Modeling Create Lines Lines Straight Line Create a line between Keypoint 1 and Keypoint 2 L12 4 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the LINK1 2D spar element This element has 2 degrees of freedom translation along the X and Y axiss and can only be used in 2D analysis 5 Define Real Constants Preprocessor Real Constants Add In the Real Constants for LINK1 window enter the following geometric properties i Crosssectional area AREA 25 ii Initial Strain 0 This defines an element with a solid rectangular cross section 5 x 5 millimeters 6 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 75e3 ii Poissons Ratio PRXY 03 Now that the initial properties of the material have been outlined the stressstrain data must be included Preprocessor Material Props Material Models Structural Nonlinear Elastic Multilinear Elastic The following window will pop up Fill in the STRAIN and STRESS boxes with the following data These are points from the stressstrain curve shown above approximating the curve with linear interpolation between the points When the data for the first point is input click Add Point to add another When all the points have been inputed click Graph to see the curve It should look like the one shown above Then click OK Curve Points Strain Stress 1 0 0 2 0001 75 3 0002 150 4 0003 225 5 0004 240 6 0005 250 7 0025 300 8 0060 355 9 0100 390 10 0150 420 11 0200 435 12 0250 449 13 0275 450 To get the problem geometry back select Utility Menu Plot Replot REPLOT 7 Define Mesh Size Preprocessor Meshing Manual Size Size Cntrls Lines All Lines For this example we will specify an element edge length of 5 mm 20 element divisions along the line 8 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All LMESHALL Solution Assigning Loads and Solving 1 Define Analysis Type Solution New Analysis Static ANTYPE0 2 Set Solution Controls H Select Solution Analysis Type Soln Control The following image will appear Ensure the following selections are made under the Basic tab as shown above A Ensure Large Static Displacements are permitted this will include the effects of large deflection in the results B Ensure Automatic time stepping is on Automatic time stepping allows ANSYS to determine appropriate sizes to break the load steps into Decreasing the step size usually ensures better accuracy however this takes time The Automatic Time Step feature will determine an appropriate balance This feature also activates the ANSYS bisection feature which will allow recovery if convergence fails C Enter 20 as the number of substeps This will set the initial substep to 120 th of the total load D Enter a maximum number of substeps of 1000 This stops the program if the solution does not converge after 1000 steps E Enter a minimum number of substeps of 1 F Ensure all solution items are writen to a results file This means rather than just recording the data for the last load step data for every load step is written to the database Therefore you can plot certain parameters over time Ensure the following selection is made under the Nonlinear tab as shown below A Ensure Line Search is On This option is used to help the NewtonRaphson solver converge B Ensure Maximum Number of Iterations is set to 1000 NOTE There are several options which have not been changed from their default values For more information about these commands type help followed by the command into the command line 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 ie all DOFs constrained 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Place a 10000 N load in the FY direction on the top of the beam Keypoint 2 5 Solve the System Solution Solve Current LS SOLVE The following will appear on your screen for NonLinear Analyses This shows the convergence of the solution General Postprocessing Viewing the Results 1 To view the element in 2D rather than a line Utility Menu PlotCtrls Style Size and Shape and turn Display of element ON as shown below 2 View the deflection contour plot General Postproc Plot Results Contour Plot Nodal Solu DOF solution UY PLNSOLUY01 Other results can be obtained as shown in previous linear static analyses Time History Postprocessing Viewing the Results As shown you can obtain the results such as deflection stress and bending moment diagrams the same way you did in previous examples using the General Postprocessor However you may wish to view time history results such as the deflection of the object over time 1 Define Variables H Select Main Menu TimeHist Postpro The following window should open automatically If it does not open automatically select Main Menu TimeHist Postpro Variable Viewer H Click the add button in the upper left corner of the window to add a variable H Select Nodal Solution DOF Solution YComponent of displacement as shown below and click OK Pick the uppermost node on the beam and click OK in the Node for Data window H To add another variable click the add button again This time select Reaction Forces Structural Forces YComponent of Force Pick the lowermost node on the beam and click OK H On the Time History Variable window click the circle in the XAxis column for FY3 This will make the reaction force the xvariable The Time History Variables window should now look like this 2 Graph Results over Time H Click on UY2 in the Time History Variables window H Click the graphing button in the Time History Variables window H The labels on the plot are not updated by ANSYS so you must change them manually Select Utility Menu Plot Ctrls Style Graphs Modify Axes and relabel the X and Yaxis appropriately This plot shows how the beam deflected linearly when the force and subsequently the stress was low in the linear range However as the force increased the deflection proportional to strain began to increase at a greater rate This is because the stress in the beam is in the plastic range and thus no longer relates to strain linearly When you verify this example analytically you will see the solutions are very similar The difference can be attributed to the ANSYS solver including large deflection calculations Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Modal Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple modal analysis of the cantilever beam shown below Preprocessing Defining the Problem The simple cantilever beam is used in all of the Dynamic Analysis Tutorials If you havent created the model in ANSYS please use the links below Both the command line codes and the GUI commands are shown in the respective links ANSYS Inc Copyright 2001 University of Alberta Solution Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Modal ANTYPE2 2 Set options for analysis type H Select Solution Analysis Type Analysis Options The following window will appear H As shown select the Subspace method and enter 5 in the No of modes to extract H Check the box beside Expand mode shapes and enter 5 in the No of modes to expand H Click OK Note that the default mode extraction method chosen is the Reduced Method This is the fastest method as it reduces the system matrices to only consider the Master Degrees of Freedom see below The Subspace Method extracts modes for all DOFs It is therefore more exact but it also takes longer to compute especially when the complex geometries H The following window will then appear For a better understanding of these options see the Commands manual H For this problem we will use the default options so click on OK 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 ie all DOFs constrained 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Verify extracted modes against theoretical predictions H Select General Postproc Results Summary The following window will appear The following table compares the mode frequencies in Hz predicted by theory and ANSYS Mode Theory ANSYS Percent Error 1 8311 8300 01 2 5194 5201 02 3 14568 14564 00 4 28569 28551 00 5 47222 47254 01 Note To obtain accurate higher mode frequencies this mesh would have to be refined even more ie instead of 10 elements we would have to model the cantilever using 15 or more elements depending upon the highest mode frequency of interest 2 View Mode Shapes H Select General Postproc Read Results First Set This selects the results for the first mode shape H Select General Postproc Plot Results Deformed shape Select Def undef edge The first mode shape will now appear in the graphics window H To view the next mode shape select General Postproc Read Results Next Set As above choose General Postproc Plot Results Deformed shape Select Def undef edge H The first four mode shapes should look like the following 3 Animate Mode Shapes H Select Utility Menu Menu at the top Plot Ctrls Animate Mode Shape The following window will appear H Keep the default setting and click OK H The animated mode shapes are shown below I Mode 1 Mode 2 I Mode 4 Using the Reduced Method for Modal Analysis This method employs the use of Master Degrees of Freedom These are degrees of freedom that govern the dynamic characteristics of a structure For example the Master Degrees of Freedom for the bending modes of cantilever beam are For this option a detailed understanding of the dynamic behavior of a structure is required However going this route means a smaller reduced stiffness matrix and thus faster calculations The steps for using this option are quite simple G Instead of specifying the Subspace method select the Reduced method and specify 5 modes for extraction G Complete the window as shown below NoteFor this example both the number of modes and frequency range was specified ANSYS then extracts the minimum number of modes between the two G Select Solution Master DOF User Selected Define G When prompted select all nodes except the left most node fixed The following window will appear G Select UY as the 1st degree of freedom shown above The same constraints are used as above The following table compares the mode frequencies in Hz predicted by theory and ANSYS Reduced Mode Theory ANSYS Percent Error 1 8311 8300 01 2 5194 5201 01 3 14568 14566 00 4 28569 28571 00 5 47222 47366 03 As you can see the error does not change significantly However for more complex structures larger errors would be expected using the reduced method Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Harmonic Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to explain the steps required to perform Harmonic analysis the cantilever beam shown below We will now conduct a harmonic forced response test by applying a cyclic load harmonic at the end of the beam The frequency of the load will be varied from 1 100 Hz The figure below depicts the beam with the application of the load ANSYS Inc Copyright 2001 University of Alberta ANSYS provides 3 methods for conducting a harmonic analysis These 3 methods are the Full Reduced and Modal Superposition methods This example demonstrates the Full method because it is simple and easy to use as compared to the other two methods However this method makes use of the full stiffness and mass matrices and thus is the slower and costlier option Preprocessing Defining the Problem The simple cantilever beam is used in all of the Dynamic Analysis Tutorials If you havent created the model in ANSYS please use the links below Both the command line codes and the GUI commands are shown in the respective links Solution Assigning Loads and Solving 1 Define Analysis Type Harmonic Solution Analysis Type New Analysis Harmonic ANTYPE3 2 Set options for analysis type H Select Solution Analysis Type Analysis Options The following window will appear H As shown select the Full Solution method the Real imaginary DOF printout format and do not use lumped mass approx H Click OK The following window will appear Use the default settings shown below 3 Apply Constraints H Select Solution Define Loads Apply Structural Displacement On Nodes The following window will appear once you select the node at x0 Note small changes in the window compared to the static examples H Constrain all DOF as shown in the above window 4 Apply Loads H Select Solution Define Loads Apply Structural ForceMoment On Nodes H Select the node at x1 far right H The following window will appear Fill it in as shown to apply a load with a real value of 100 and an imaginary value of 0 in the positive y direction Note By specifying a real and imaginary value of the load we are providing information on magnitude and phase of the load In this case the magnitude of the load is 100 N and its phase is 0 Phase information is important when you have two or more cyclic loads being applied to the structure as these loads could be in or out of phase For harmonic analysis all loads applied to a structure must have the SAME FREQUENCY 5 Set the frequency range H Select Solution Load Step Opts TimeFrequency Freq and Substps H As shown in the window below specify a frequency range of 0 100Hz 100 substeps and stepped bc By doing this we will be subjecting the beam to loads at 1 Hz 2 Hz 3 Hz 100 Hz We will specify a stepped boundary condition KBC as this will ensure that the same amplitude 100 N will be applyed for each of the frequencies The ramped option on the other hand would ramp up the amplitude where at 1 Hz the amplitude would be 1 N and at 100 Hz the amplitude would be 100 N You should now have the following in the ANSYS Graphics window 6 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results We want to observe the response at x1 where the load was applyed as a function of frequency We cannot do this with General PostProcessing POST1 rather we must use TimeHist PostProcessing POST26 POST26 is used to observe certain variables as a function of either time or frequency 1 Open the TimeHist Processing POST26 Menu Select TimeHist Postpro from the ANSYS Main Menu 2 Define Variables In here we have to define variables that we want to see plotted By default Variable 1 is assigned either Time or Frequency In our case it is assigned Frequency We want to see the displacement UY at the node at x1 which is node 2 To get a list of nodes and their attributes select Utility Menu List nodes H Select TimeHist Postpro Variable Viewer and the following window should pop up H Select Add the green sign in the upper left corner from this window and the following window should appear H We are interested in the Nodal Solution DOF Solution YComponent of displacement Click OK H Graphically select node 2 when prompted and click OK The Time History Variables window should now look as follows 3 List Stored Variables H In the Time History Variables window click the List button 3 buttons to the left of Add The following window will appear listing the data 4 Plot UY vs frequency H In the Time History Variables window click the Plot button 2 buttons to the left of Add The following graph should be plotted in the main ANSYS window Note that we get peaks at frequencies of approximately 83 and 51 Hz This corresponds with the predicted frequencies of 8311 and 5194Hz To get a better view of the response view the log scale of UY H Select Utility Menu PlotCtrls Style Graphs Modify Axis The following window will appear H As marked by an A in the above window change the Yaxis scale to Logarithmic H Select Utility Menu Plot Replot H You should now see the following This is the response at node 2 for the cyclic load applied at this node from 0 100 Hz H For ANSYS version lower than 70 the Variable Viewer window is not available Use the Define Variables and Store Data functions under TimeHist Postpro See the help file for instructions Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Transient Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to show the steps involved to perform a simple transient analysis Transient dynamic analysis is a technique used to determine the dynamic response of a structure under a timevarying load The time frame for this type of analysis is such that inertia or damping effects of the structure are considered to be important Cases where such effects play a major role are under step or impulse loading conditions for example where there is a sharp load change in a fraction of time If inertia effects are negligible for the loading conditions being considered a static analysis may be used instead For our case we will impact the end of the beam with an impulse force and view the response at the location of impact ANSYS Inc Copyright 2001 University of Alberta Since an ideal impulse force excites all modes of a structure the response of the beam should contain all mode frequencies However we cannot produce an ideal impulse force numerically We have to apply a load over a discrete amount of time dt After the application of the load we track the response of the beam at discrete time points for as long as we like depending on what it is that we are looking for in the response The size of the time step is governed by the maximum mode frequency of the structure we wish to capture The smaller the time step the higher the mode frequency we will capture The rule of thumb in ANSYS is timestep 1 20f where f is the highest mode frequency we wish to capture In other words we must resolve our step size such that we will have 20 discrete points per period of the highest mode frequency It should be noted that a transient analysis is more involved than a static or harmonic analysis It requires a good understanding of the dynamic behavior of a structure Therefore a modal analysis of the structure should be initially performed to provide information about the structures dynamic behavior In ANSYS transient dynamic analysis can be carried out using 3 methods G The Full Method This is the easiest method to use All types of nonlinearities are allowed It is however very CPU intensive to go this route as full system matrices are used G The Reduced Method This method reduces the system matrices to only consider the Master Degrees of Freedom MDOFs Because of the reduced size of the matrices the calculations are much quicker However this method handles only linear problems such as our cantilever case G The Mode Superposition Method This method requires a preliminary modal analysis as factored mode shapes are summed to calculate the structures response It is the quickest of the three methods but it requires a good deal of understanding of the problem at hand We will use the Reduced Method for conducting our transient analysis Usually one need not go further than Reviewing the Reduced Results However if stresses and forces are of interest than we would have to Expand the Reduced Solution Preprocessing Defining the Problem The simple cantilever beam is used in all of the Dynamic Analysis Tutorials If you havent created the model in ANSYS please use the links below Both the command line codes and the GUI commands are shown in the respective links Solution Assigning Loads and Solving 1 Define Analysis Type H Select Solution Analysis Type New Analysis Transient H The following window will appear Select Reduced as shown 2 Define Master DOFs H Select Solution Master DOFs User Selected Define H Select all nodes except the left most node at x0 The following window will open choose UY as the first dof in this window For an explanation on Master DOFs see the section on Using the Reduced Method for modal analysis 3 Constrain the Beam Solution Menu Define Loads Apply Structural Displacement On nodes Fix the left most node constrain all DOFs 4 Apply Loads We will define our impulse load using Load Steps The following time history curve shows our load steps and time steps Note that for the reduced method a constant time step is required throughout the time range We can define each load step load and time at the end of load segment and save them in a file for future solution purposes This is highly recommended especially when we have many load steps and we wish to rerun our solution We can also solve for each load step after we define it We will go ahead and save each load step in a file for later use at the same time solve for each load step after we are done defining it a Load Step 1 Initial Conditions i Define Load Step We need to establish initial conditions the condition at Time 0 Since the equations for a transient dynamic analysis are of second order two sets of initial conditions are required initial displacement and initial velocity However both default to zero Therefore for this example we can skip this step ii Specify Time and Time Step Options I Select Solution Load Step Opts TimeFrequenc Time Time Step I set a time of 0 for the end of the load step as shown below I set DELTIM to 0001 This will specify a time step size of 0001 seconds to be used for this load step iii Write Load Step File I Select Solution Load Step Opts Write LS File The following window will appear I Enter LSNUM 1 as shown above and click OK The load step will be saved in a file jobnames01 b Load Step 2 i Define Load Step I Select Solution Define Loads Apply Structural ForceMoment On Nodes and select the right most node at x1 Enter a force in the FY direction of value 100 N ii Specify Time and Time Step Options I Select Solution Load Step Opts TimeFrequenc Time Time Step and set a time of 0001 for the end of the load step iii Write Load Step File Solution Load Step Opts Write LS File Enter LSNUM 2 c Load Step 3 i Define Load Step I Select Solution Define Loads Delete Structural ForceMoment On Nodes and delete the load at x1 ii Specify Time and Time Step Options I Select Solution Load Step Opts TimeFrequenc Time Time Step and set a time of 1 for the end of the load step iii Write Load Step File Solution Load Step Opts Write LS File Enter LSNUM 3 5 Solve the System H Select Solution Solve From LS Files The following window will appear H Complete the window as shown above to solve using LS files 1 to 3 Postprocessing Viewing the Results To view the response of node 2 UY with time we must use the TimeHist PostProcessor POST26 1 Define Variables In here we have to define variables that we want to see plotted By default Variable 1 is assigned either Time or Frequency In our case it is assigned Frequency We want to see the displacement UY at the node at x1 which is node 2 To get a list of nodes and their attributes select Utility Menu List nodes H Select TimeHist Postpro Variable Viewer and the following window should pop up H Select Add the green sign in the upper left corner from this window and the following window should appear H We are interested in the Nodal Solution DOF Solution YComponent of displacement Click OK H Graphically select node 2 when prompted and click OK The Time History Variables window should now look as follows 2 List Stored Variables H In the Time History Variables window click the List button 3 buttons to the left of Add The following window will appear listing the data 3 Plot UY vs frequency H In the Time History Variables window click the Plot button 2 buttons to the left of Add The following graph should be plotted in the main ANSYS window A few things to note in the response curve I There are approximately 8 cycles in one second This is the first mode of the cantilever beam and we have been able to capture it I We also see another response at a higher frequency We may have captured some response at the second mode at 52 Hz of the beam I Note that the response does not decay as it should not We did not specify damping for our system Expand the Solution For most problems one need not go further than Reviewing the Reduced Results as the response of the structure is of utmost interest in transient dynamic analysis However if stresses and forces are of interest we would have to expand the reduced solution Lets say we are interested in the beams behaviour at peak responses We should then expand a few or all solutions around one peak or dip We will expand 10 solutions within the range of 008 and 011 seconds 1 Expand the solution H Select Finish in the ANSYS Main Menu H Select Solution Analysis Type ExpansionPass and switch it to ON in the window that pops open H Select Solution Load Step Opts ExpansionPass Single Expand Range of Solus H Complete the window as shown below This will expand 10 solutions withing the range of 008 and 011 seconds 2 Solve the System Solution Solve Current LS SOLVE 3 Review the results in POST1 Review the results using either General Postprocessing POST1 or TimeHist Postprocessing POST26 For this case we can view the deformed shape at each of the 10 solutions we expanded Damped Response of the Cantilever Beam We did not specify damping in our transient analysis of the beam We specify damping at the same time we specify our time time steps for each load step We will now rerun our transient analysis but now we will consider damping Here is where the use of load step files comes in handy We can easily change a few values in these files and rerun our whole solution from these load case files G Open up the first load step file Dynamics01 for editing Utility Menu File List Other Dynamics01 The file should look like the following COMANSYS RELEASE 571 UP20010418 144402 08202001 NOPR TITLE Dynamic Analysis LSNUM 1 ANTYPE 4 TRNOPTREDUDAMP BFUNIFTEMPTINY DELTIM 1000000000E03 TIME 000000000 TREF 000000000 ALPHAD 000000000 BETAD 000000000 DMPRAT 000000000 TINTPR50 5000000000E03 TINTPR50 100000000 0500000000 100000000 NCNV 1 000000000 0 000000000 000000000 ERESXDEFA ACEL 000000000 000000000 000000000 OMEGA 000000000 000000000 000000000 0 DOMEGA 000000000 000000000 000000000 CGLOC 000000000 000000000 000000000 CGOMEGA 000000000 000000000 000000000 DCGOMG 000000000 000000000 000000000 D 1UX 000000000 000000000 D 1UY 000000000 000000000 D 1ROTZ 000000000 000000000 GOPR G Change the damping value BETAD from 0 to 001 in all three load step files G We will have to rerun the job for the new load step files Select Utility Menu file Clear and Start New G Repeat the steps shown above up to the point where we select MDOFs After selecting MDOFs simply go to Solution Solve From LS files and in the window that opens up select files from 1 to 3 in steps of 1 G After the results have been calculated plot up the response at node 2 in POST26 The damped response should look like the following Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Simple Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple conduction problem The Simple Conduction Example is constrained as shown in the following figure Thermal conductivity k of the material is 10 WmC and the block is assumed to be infinitely long Preprocessing Defining the Problem ANSYS Inc Copyright 2001 University of Alberta 1 Give example a Title 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create geometry Preprocessor Modeling Create Areas Rectangle By 2 Corners X0 Y0 Width1 Height1 BLC40011 4 Define the Type of Element Preprocessor Element Type AddEditDelete click Add Select Thermal Mass Solid Quad 4Node 55 ET1PLANE55 For this example we will use PLANE55 Thermal Solid Quad 4node 55 This element has 4 nodes and a single DOF temperature at each node PLANE55 can only be used for 2 dimensional steadystate or transient thermal analysis 5 Element Material Properties Preprocessor Material Props Material Models Thermal Conductivity Isotropic KXX 10 Thermal conductivity MPKXX110 6 Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas 005 AESIZEALL005 7 Mesh Preprocessor Meshing Mesh Areas Free Pick All AMESHALL Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis SteadyState ANTYPE0 2 Apply Constraints For thermal problems constraints can be in the form of Temperature Heat Flow Convection Heat Flux Heat Generation or Radiation In this example all 4 sides of the block have fixed temperatures H Solution Define Loads Apply Note that all of the Structural options cannot be selected This is due to the type of element PLANE55 selected H Thermal Temperature On Nodes H Click the Box option shown below and draw a box around the nodes on the top line The following window will appear H Fill the window in as shown to constrain the side to a constant temperature of 500 H Using the same method constrain the remaining 3 sides to a constant value of 100 Orange triangles in the graphics window indicate the temperature contraints 3 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Results Using ANSYS Plot Temperature General Postproc Plot Results Contour Plot Nodal Solu DOF solution Temperature TEMP Note that due to the manner in which the boundary contitions were applied the top corners are held at a temperature of 100 Recall that the nodes on the top of the plate were constrained first followed by the side and bottom constraints The top corner nodes were therefore first constrained at 500C then overwritten when the side constraints were applied Decreasing the mesh size can minimize this effect however one must be aware of the limitations in the results at the corners Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Thermal Mixed Boundary Example ConductionConvection Insulated Introduction This tutorial was created using ANSYS 70 to solve simple thermal examples Analysis of a simple conduction as well a mixed conduction convectioninsulation problem will be demonstrated The Mixed ConvectionConductionInsulated Boundary Conditions Example is constrained as shown in the following figure Note that the section is assumed to be infinitely long Preprocessing Defining the Problem ANSYS Inc Copyright 2001 University of Alberta 1 Give example a Title 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create geometry Preprocessor Modeling Create Areas Rectangle By 2 Corners X0 Y0 Width1 Height1 BLC40011 4 Define the Type of Element Preprocessor Element Type AddEditDelete click Add Select Thermal Mass Solid Quad 4Node 55 ET1PLANE55 As in the conduction example we will use PLANE55 Thermal Solid Quad 4node 55 This element has 4 nodes and a single DOF temperature at each node PLANE55 can only be used for 2 dimensional steadystate or transient thermal analysis 5 Element Material Properties Preprocessor Material Props Material Models Thermal Conductivity Isotropic KXX 10 MPKXX110 This will specify a thermal conductivity of 10 WmC 6 Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas 005 AESIZEALL005 7 Mesh Preprocessor Meshing Mesh Areas Free Pick All AMESHALL Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis SteadyState ANTYPE0 2 Apply Conduction Constraints In this example all 2 sides of the block have fixed temperatures while convection occurs on the other 2 sides H Solution Define Loads Apply Thermal Temperature On Lines H Select the top line of the block and constrain it to a constant value of 500 C H Using the same method constrain the left side of the block to a constant value of 100 C 3 Apply Convection Boundary Conditions H Solution Define Loads Apply Thermal Convection On Lines H Select the right side of the block The following window will appear H Fill in the window as shown This will specify a convection of 10 Wm2C and an ambient temperature of 100 degrees Celcius Note that VALJ and VAL2J have been left blank This is because we have uniform convection across the line 4 Apply Insulated Boundary Conditions H Solution Define Loads Apply Thermal Convection On Lines H Select the bottom of the block H Enter a constant Film coefficient VALI of 0 This will eliminate convection through the side thereby modeling an insulated wall Note you do not need to enter a Bulk or ambient temperature You should obtain the following 5 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Results Using ANSYS Plot Temperature General Postproc Plot Results Contour Plot Nodal Solu DOF solution Temperature TEMP Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Transient Thermal Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple transient conduction problem Special thanks to Jesse Arnold for the analytical solution shown at the end of the tutorial The example is constrained as shown in the following figure Thermal conductivity k of the material is 5 WmK and the block is assumed to be infinitely long Also the density of the material is 920 kgm3 and the specific heat capacity c is 2040 kJkgK It is beneficial if the ThermalConduction tutorial is completed first to compare with this solution ANSYS Inc Copyright 2001 University of Alberta Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title TitleTransient Thermal Conduction 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create geometry Preprocessor Modeling Create Areas Rectangle By 2 Corners X0 Y0 Width1 Height1 BLC40011 4 Define the Type of Element Preprocessor Element Type AddEditDelete click Add Select Thermal Mass Solid Quad 4Node 55 ET1PLANE55 For this example we will use PLANE55 Thermal Solid Quad 4node 55 This element has 4 nodes and a single DOF temperature at each node PLANE55 can only be used for 2 dimensional steadystate or transient thermal analysis 5 Element Material Properties Preprocessor Material Props Material Models Thermal Conductivity Isotropic KXX 5 Thermal conductivity MPKXX110 Preprocessor Material Props Material Models Thermal Specific Heat C 204 MPC1204 Preprocessor Material Props Material Models Thermal Density DENS 920 MPDENS1920 6 Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas 005 AESIZEALL005 7 Mesh Preprocessor Meshing Mesh Areas Free Pick All AMESHALL At this point the model should look like the following Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Transient ANTYPE4 The window shown below will pop up We will use the defaults so click OK 2 Set Solution Controls Solution Analysis Type Soln Controls The following window will pop up A Set Time at end of loadstep to 300 and Automatic time stepping to ON B Set Number of substeps to 20 Max no of substeps to 100 Min no of substeps to 20 C Set the Frequency to Write every substep Click on the NonLinear tab at the top and fill it in as shown D Set Line search to ON E Set the Maximum number of iterations to 100 For a complete description of what these options do refer to the help file Basically the time at the end of the load step is how long the transient analysis will run and the number of substeps defines how the load is broken up By writing the data at every step you can create animations over time and the other options help the problem converge quickly 3 Apply Constraints For thermal problems constraints can be in the form of Temperature Heat Flow Convection Heat Flux Heat Generation or Radiation In this example 2 sides of the block have fixed temperatures and the other two are insulated H Solution Define Loads Apply Note that all of the Structural options cannot be selected This is due to the type of element PLANE55 selected H Thermal Temperature On Nodes H Click the Box option shown below and draw a box around the nodes on the top line and then click OK The following window will appear H Fill the window in as shown to constrain the top to a constant temperature of 500 K H Using the same method constrain the bottom line to a constant value of 100 K Orange triangles in the graphics window indicate the temperature contraints 4 Apply Initial Conditions Solution Define Loads Apply Initial Conditn Define Pick All Fill in the IC window as follows to set the initial temperature of the material to 100 K 5 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Results Using ANSYS Plot Temperature General Postproc Plot Results Contour Plot Nodal Solu DOF solution Temperature TEMP Animate Results Over Time H First specify the contour range Utility Menu PlotCtrls Style Contours Uniform Contours Fill in the window as shown with 8 contours user specified from 100 to 500 H Then animate the data Utility Menu PlotCtrls Animate Over Time Fill in the following window as shown 20 frames 0 300 Time Range Auto contour scaling OFF DOF solution TEMP You can see how the temperature rises over the area over time The heat flows from the higher temperature to the lower temperature constraints as expected Also you can see how it reaches equilibrium when the time reaches approximately 200 seconds Shown below are analytical and ANSYS generated temperature vs time curves for the center of the block As can be seen the curves are practically identical thus the validity of the ANSYS simulation has been proven Center Temperature over Time ANSYS Generated Solution Time History Postprocessing Viewing the Results 1 Creating the Temperature vs Time Graph H Select Main Menu TimeHist Postpro The following window should open automatically If it does not open automatically select Main Menu TimeHist Postpro Variable Viewer H Click the add button in the upper left corner of the window to add a variable H Select Nodal Solution DOF Solution Temperature as shown below and click OK Pick the center node on the mesh node 261 and click OK in the Node for Data window H The Time History Variables window should now look like this 2 Graph Results over Time H Ensure TEMP2 in the Time History Variables window is highlighted H Click the graphing button in the Time History Variables window H The labels on the plot are not updated by ANSYS so you must change them manually Select Utility Menu Plot Ctrls Style Graphs Modify Axes and relabel the X and Yaxis appropriately Note how this plot does not exactly match the plot shown above This is because the solution has not completely converged To cause the solution to converge one of two things can be done decrease the mesh size or increase the number of substeps used in the transient analysis From experience reducing the mesh size will do little in this case as the mesh is adequate to capture the response Instead increasing the number of substeps from say 20 to 300 will cause the solution to converge This will greatly increase the computational time required though which is why only 20 substeps are used in this tutorial Twenty substeps gives an adequate and quick approximation of the solution Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Effect of Self Weight Distributed Loading NonLinear Analysis Solution Tracking Buckling NonLinear Materials Dynamic Modal Dynamic Harmonic Dynamic Transient ThermalConduction ThermalMixed Bndry Transient Heat Axisymmetric Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta Modelling Using Axisymmetry Introduction This tutorial was completed using ANSYS 70 This tutorial is intended to outline the steps required to create an axisymmetric model The model will be that of a closed tube made from steel Point loads will be applied at the center of the top and bottom plate to make an analytical verification simple to calculate A 34 cross section view of the tube is shown below As a warning point loads will create discontinuities in the your model near the point of application If you chose to use these types of loads in your own modelling be very careful and be sure to understand the theory of how the FEA package is appling the load and the assumption it is making In this case we will only be concerned about the stress distribution far from the point of application so the discontinuities will have a negligable effect ANSYS Inc Copyright 2001 University of Alberta Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title Axisymmetric Tube 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create Areas Preprocessor Modeling Create Areas Rectangle By Dimensions RECTNGX1X2Y1Y2 For an axisymmetric problem ANSYS will rotate the area around the yaxis at x0 Therefore to create the geometry mentioned above we must define a Ushape We are going to define 3 overlapping rectangles as defined in the following table Rectangle X1 X2 Y1 Y2 1 0 20 0 5 2 15 20 0 100 3 0 20 95 100 4 Add Areas Together Preprocessor Modeling Operate Booleans Add Areas AADDALL Click the Pick All button to create a single area 5 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the PLANE2 Structural Solid Triangle 6node element This element has 2 degrees of freedom translation along the X and Y axes Many elements support axisymmetry however if the Ansys Elements Reference which can be found in the help file does not discuss axisymmetric applications for a particular element type axisymmetry is not supported 6 Turn on Axisymmetry While the Element Types window is still open click the Options button Under Element behavior K3 select Axisymmetric 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 8 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas For this example we will use an element edge length of 2mm 9 Mesh the frame Preprocessor Meshing Mesh Areas Free click Pick All Your model should know look like this Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints H Solution Define Loads Apply Structural Displacement Symmetry BC On Lines Pick the two edges on the left at x0 as shown below By using the symmetry BC command ANSYS automatically calculates which DOFs should be constrained for the line of symmetry Since the element we are using only has 2 DOFs per node we could have constrained the lines in the xdirection to create the symmetric boundary conditions H Utility Menu Select Entities Select Nodes and By Location from the scroll down menus Click Y coordinates and type 50 into the input box as shown below then click OK Solution Define Loads Apply Structural Displacement On Nodes Pick All Constrain the nodes in the ydirection UY This is required to constrain the model in space otherwise it would be free to float up or down The location to constrain the model in the ydirection y50 was chosen because it is along a symmetry plane Therefore these nodes wont move in the ydirection according to theory 3 Utility Menu Select Entities In the select entities window click Sele All to reselect all nodes It is important to always reselect all entities once youve finished to ensure future commands are applied to the whole model and not just a few entities Once youve clicked Sele All click on Cancel to close the window 4 Apply Loads H Solution Define Loads Apply Structural ForceMoment On Keypoints Pick the top left corner of the area and click OK Apply a load of 100 in the FY direction H Solution Define Loads Apply Structural ForceMoment On Keypoints Pick the bottom left corner of the area and click OK Apply a load of 100 in the FY direction H The applied loads and constraints should now appear as shown in the figure below 5 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Hand Calculations Hand calculations were performed to verify the solution found using ANSYS The stress across the thickness at y 50mm is 0182 MPa 2 Determine the Stress Through the Thickness of the Tube H Utility Menu Select Entities Select Nodes By Location Y coordinates and type 4555 in the MinMax box as shown below and click OK H General Postproc List Results Nodal Solution Stress Components SCOMP The following list should pop up H If you take the average of the stress in the ydirection over the thickness of the tube 018552 0178662 the stress in the tube is 0182 MPa matching the analytical solution The average is used because in the analytical case it is assumed the stress is evenly distributed across the thickness This is only true when the location is far from any stress concentrators such as corners Thus to approximate the analytical solution we must average the stress over the thickness 3 Plotting the Elements as Axisymmetric Utility Menu PlotCtrls Style Symmetry Expansion 2D Axisymmetric The following window will appear By clicking on 34 expansion you can produce the figure shown at the beginning of this tutorial 4 Extra Exercise It is educational to repeat this tutorial but leave out the key option which enables axisymmetric modelling The rest of the commands remain the same If this is done the model is a flat rectangular plate with a rectangular hole in the middle Both the stress distribution and deformed shape change drastically as expected due to the change in geometry Thus when using axisymmetry be sure to verify the solutions you get are reasonable to ensure the model is infact axisymmetric Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Application of Joints and Springs in ANSYS Introduction This tutorial was created using ANSYS 571 This tutorial will introduce G the use of multiple elements in ANSYS G elements COMBIN7 Joints and COMBIN14 Springs G obtainingstoring scalar information and store them as parameters A 1000N vertical load will be applied to a catapult as shown in the figure below The catapult is built from steel tubing with an outer diameter of 40 mm a wall thickness of 10 and a modulus of elasticity of 200GPa The springs have a stiffness of 5 Nmm Preprocessing Defining the Problem 1 Open preprocessor menu PREP7 2 Give example a Title Utility Menu File Change Title titleCatapult 3 Define Element Types For this problem 3 types of elements are used PIPE16 COMBIN7 Revolute Joint COMBIN14 SpringDamper It is therefore required that the types of elements are defined prior to creating the elements This element has 6 degrees of freedom translation along the X Y and Z axis and rotation about the XY and Z axis a Define PIPE16 With 6 degrees of freedom the PIPE16 element can be used to create the 3D structure I Preprocessor Element Type AddEditDelete click Add I Select Pipe Elast straight 16 I Click on Apply You should see Type 1 PIPE16 in the Element Types window b Define COMBIN7 COMBIN7 Revolute Joint will allow the catapult to rotate about nodes 1 and 2 I Select Combination Revolute Joint 7 I Click Apply c Define COMBIN14 Now we will define the spring elements I Select Combination Spring damper 14 I Click on OK In the Element Types window there should now be three types of elements defined 4 Define Real Constants Real Constants must be defined for each of the 3 element types a PIPE16 I Preprocessor Real Constants AddEditDelete click Add I Select Type 1 PIPE16 and click OK I Enter the following properties then click OK OD 40 TKWALL 10 Set 1 will now appear in the dialog box b COMBIN7 Joint Five of the degrees of freedom UX UY UZ ROTX and ROTY can be constrained with different levels of flexibility These can be defined by the 3 real constants K1 UX UY K2 UZ and K3 ROTX ROTY For this example we will use high values for K1 through K3 since we only expect the model to rotate about the Z axis I Click Add I Select Type 2 COMBIN7 Click OK I In the Real Constants for COMBIN7 window enter the following geometric properties then click OK XY transnational stiffness K1 1e9 Z directional stiffness K2 1e9 Rotational stiffness K3 1e9 I Set 2 will now appear in the dialog box Note The constants that we define in this problem refer to the relationship between the coincident nodes By having high values for the stiffness in the XY plane and along the Z axis we are essentially constraining the two coincident nodes to each other c COMBIN14 Spring I Click Add I Select Type 3 COMBIN14 Click OK I Enter the following geometric properties Spring constant K 5 In the Element Types window there should now be three types of elements defined 5 Define Element Material Properties 1 Preprocessor Material Props Material Models 2 In the Define Material Model Behavior Window ensure that Material Model Number 1 is selected 3 Select Structural Linear Elastic Isotropic 4 In the window that appears enter the give the properties of Steel then click OK Youngs modulus EX 200000 Poissons Ratio PRXY 033 6 Define Nodes Preprocessor Modeling Create Nodes In Active CS Nxyz We are going to define 13 Nodes for this structure as given in the following table as depicted by the circled numbers in the figure above Node Coordinates xyz 1 000 2 001000 3 100001000 4 100000 5 010001000 6 010000 7 700700500 8 400400500 9 000 10 001000 11 00500 12 001500 13 00500 7 Create PIPE16 elements a Define element type Preprocessor Modeling Create Elements Elem Attributes The following window will appear Ensure that the Element type number is set to 1 PIPE16 Material number is set to 1 and Real constant set number is set to 1 Then click OK b Create elements Preprocessor Modeling Create Elements Auto Numbered Thru Nodes E node a node b Create the following elements joining Nodes a and Nodes b Note because it is difficult to graphically select the nodes you may wish to use the command line for example the first entry would be E16 Node a Node b 1 6 2 5 1 4 2 3 3 4 10 8 9 8 7 8 12 5 13 6 12 13 5 3 6 4 You should obtain the following geometry Oblique view 8 Create COMBIN7 Joint elements a Define element type Preprocessor Modeling Create Elements Elem Attributes Ensure that the Element type number is set to 2 COMBIN7 and that Real constant set number is set to 2 Then click OK b Create elements When defining a joint three nodes are required Two nodes are coincident at the point of rotation The elements that connect to the joint must reference each of the coincident points The other node for the joint defines the axis of rotation The axis would be the line from the coincident nodes to the other node Preprocessor Modeling Create Elements Auto Numbered Thru Nodes Enode a node b node c Create the following lines joining Node a and Node b Node a Node b Node c 1 9 11 2 10 11 9 Create COMBIN14 Spring elements a Define element type Preprocessor Modeling Create Elements Elem Attributes Ensure that the Element type number is set to 3 COMBIN7 and that Real constant set number is set to 3 Then click OK b Create elements Preprocessor Modeling Create Elements Auto Numbered Thru Nodes Enode a node b Create the following lines joining Node a and Node b Node a Node b 5 8 8 6 NOTE To ensure that the correct nodes were used to make the correct element in the above table you can list all the elements defined in the model To do this select Utilities Menu List Elements Nodes Attributes 10 Meshing Because we have defined our model using nodes and elements we do not need to mesh our model If we initially defined our model using keypoints and lines we would have had to create elements in our model by meshing the lines It is the elements that ANSYS uses to solve the model 11 Plot Elements Utility Menu Plot Elements You may also wish to turn on element numbering and turn off keypoint numbering Utility Menu PlotCtrls Numbering Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution New Analysis Static ANTYPE0 2 Allow Large Deflection Solution Soln Controls basic NLGEOM ON Because the model is expected to deform considerably we need to include the effects of large deformation 3 Apply Constraints Solution Loads Apply Structural Displacement On Nodes H Fix Nodes 3 4 12 and 13 ie all degrees of freedom are constrained 4 Apply Loads Solution Loads Apply Structural ForceMoment On Nodes H Apply a vertical point load of 1000N at node 7 The applied loads and constraints should now appear as shown in the figure below Note To have the constraints and loads appear each time you select Replot in ANSYS you must change some settings under Utility Menu Plot Ctrls Symbols In the window that appears check the box beside All Applied BCs in the Boundary Condition Symbol section 5 Solve the System Solution Solve Current LS SOLVE Note During the solution you will see a yellow warning window which states that the Coefficient ratio exceeds 10e8 This warning indicates that the solution has relatively large displacements This is due to the rotation about the joints Postprocessing Viewing the Results 1 Plot Deformed Shape General Postproc Plot Results Deformed Shape PLDISP2 2 Extracting Information as Parameters In this problem we would like to find the vertical displacement of node 7 We will do this using the GET command a Select Utility Menu Parameters Get Scalar Data b The following window will appear Select Results data and Nodal results as shown then click OK c Fill in the Get Nodal Results Data window as shown below d To view the defined parameter select Utility Menu Parameters Scalar Parameters Therefore the vertical displacement of Node 7 is 32378 mm This can be repeated for any of the other nodes you are interested in Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Design Optimization Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to introduce a method of solving design optimization problems using ANSYS This will involve creating the geometry utilizing parameters for all the variables deciding which variables to use as design state and objective variables and setting the correct tolerances for the problem to obtain an accurately converged solution in a minimal amount of time The use of hardpoints to apply forcesconstraints in the middle of lines will also be covered in this tutorial A beam has a force of 1000N applied as shown below The purpose of this optimization problem is to minimize the weight of the beam without exceeding the allowable stress It is necessary to find the cross sectional dimensions of the beam in order to minimize the weight of the beam However the width and height of the beam cannot be smaller than 10mm The maximum stress anywhere in the beam cannot exceed 200 MPa The beam is to be made of steel with a modulus of elasticity of 200 GPa Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title Design Optimization 2 Enter initial estimates for variables To solve an optimization problem in ANSYS parameters need to be defined for all design variables H Select Utility Menu Parameters Scalar Parameters H In the window that appears shown below type W20 in the Selection section H Click Accept The Scalar Parameters window will stay open H Now type H20 in the Selection section H Click Accept H Click Close in the Scalar Parameters window NOTE None of the variables defined in ANSYS are allowed to have negative values 3 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxy We are going to define 2 Keypoints for this beam as given in the following table Keypoints Coordinates xy 1 00 2 10000 4 Create Lines Preprocessor Modeling Create Lines Lines In Active Coord L12 Create a line joining Keypoints 1 and 2 5 Create Hard Keypoints Hardpoints are often used when you need to apply a constraint or load at a location where a keypoint does not exist For this case we want to apply a force 34 of the way down the beam Since there are not any keypoints here and we cant be certain that one of the nodes will be here we will need to specify a hardpoint H Select Preprocessor Modeling Create Keypoints Hard PT on line Hard PT by ratio This will allow us to create a hardpoint on the line by defining the ratio of the location of the point to the size of the line H Select the line when prompted H Enter a ratio of 075 in the Create HardPT by Ratio window which appears You have now created a keypoint labelled Keypoint 3 34 of the way down the beam 6 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axes and rotation about the Z axis 7 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties Note that is used instead for exponents i Crosssectional area AREA WH ii Area moment of inertia IZZ WH312 iii Thickness along Y axis H NOTE It is important to use independent variables to define dependent variables such as the moment of inertia During the optimization the width and height will change for each iteration As a result the other variables must be defined in relation to the width and height 8 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 9 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will specify an element edge length of 100 mm 10 element divisions along the line 10 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All LMESHALL Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Pin Keypoint 1 ie UX UY constrained and constrain Keypoint 2 in the Y direction 3 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Apply a vertical FY point load of 2000N at Keypoint 3 The applied loads and constraints should now appear as shown in the figure below 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results Extracting Information as Parameters To perform an optimization we must extract the required information In this problem we would like to find the maximum stress in the beam and the volume as a result of the width and height variables 1 Define the volume H Select General Postproc Element Table Define Table Add H The following window will appear Fill it in as shown to obtain the volume of the beam Note that this is the volume of each element If you were to list the element table you would get a volume for each element Therefore you have to sum the element values together to obtain the total volume of the beam Follow the instructions below to do this H Select General Postproc Element Table Sum of Each Item H A little window will appear notifying you that the tabular sum of each element table will be calculated Click OK You will obtain a window notifying you that the EVolume is now 400000 mm2 2 Store the data Volume as a parameter H Select Utility Menu Parameters Get Scalar Data H In the window which appears select Results Data and Elem table sums H the following window will appear Select the items shown to store the Volume as a parameter Now if you view the parameters Utility Menu Parameters Scalar Parameters you will see that Volume has been added 3 Define the maximum stress at the i node of each element in the beam H Select General Postproc Element Table Define Table Add H The following window will appear Fill it in as shown to obtain the maximum stress at the i node of each element and store it as SMAXI Note that nmisc1 is the maximum stress For further information type Help beam3 into the command line Now we will need to sort the stresses in descending order to find the maximum stress H Select General Postproc List Results Sorted Listing Sort Elems H Complete the window as shown below to sort the data from SMAXI in descending order 4 Store the data Max Stress as a parameter H Select Utility Menu Parameters Get Scalar Data H In the window which appears select Results Data and Other operations H In the that appears fill it in as shown to obtain the maximum value 5 Define maximum stress at the j node of each element for the beam H Select General Postproc Element Table Define Table Add H Fill this table as done previously however make the following changes I save the data as SMAXJ instead of SMAXI I The element table data enter NMISC3 instead of NMISC1 This will give you the max stress at the j node H Select General Postproc List Results Sorted Listing Sort Elems to sort the stresses in descending order H However select SMAXJ in the Item Comp selection box 6 Store the data Max Stress as a parameter H Select Utility Menu Parameters Get Scalar Data H In the window which appears select Results Data and Other operations H In the that appears fill it in as shown previously however name the parameter SMaxJ 7 Select the largest of SMAXJ and SMAXI H Type SMAXSMAXISMAXJ into the command line This will set the largest of the 2 values equal to SMAX In this case the maximum values for each are the same However this is not always the case 8 View the parametric data Utility Menu Parameters Scalar Parameters Note that the maximum stress is 28125 which is much larger than the allowable stress of 200MPa Design Optimization Now that we have parametrically set up our problem in ANSYS based on our initial width and height dimensions we can now solve the optimization problem 1 Write the command file It is necessary to write the outline of our problem to an ANSYS command file This is so that ANSYS can iteratively run solutions to our problem based on different values for the variables that we will define H Select Utility Menu File Write DB Log File H In the window that appears type a name for the command file such as optimizetxt H Click OK If you open the command file in a text editor such as Notepad it should similar to this BATCH COMANSYS RELEASE 70 UP20021010 161003 05262003 inputstart70ansCProgram FilesAnsys Incv70ANSYSapdl1 title Design Optimization SETW 20 SETH 20 PREP7 K100 K210000 L 1 2 HPTCREATELINE10RATI075 ET1BEAM3 R1WHWH312H MPTEMP MPTEMP10 MPDATAEX1200000 MPDATAPRXY13 LESIZEALL100 1 1 LMESH 1 FINISH SOL ANTYPE0 FLST213ORDE1 FITEM21 GO DKP51X 0UXUY FLST213ORDE1 FITEM22 GO DKP51X 0UY FLST213ORDE1 FITEM23 GO FKP51XFY2000 STATUSSOLU SOLVE FINISH POST1 AVPRIN00 ETABLEEVolumeVOLU SSUM GETVolumeSSUM ITEMEVOLUME AVPRIN00 ETABLESMaxINMISC 1 ESORTETABSMAXI01 GETSMaxISORTMAX AVPRIN00 ETABLESMaxJNMISC 3 ESORTETABSMAXJ01 GETSMaxJSORTMAX SETSMAXSMAXISMAXJ LGWRITEoptimizationCTempCOMMENT Several small changes need to be made to this file prior to commencing the optimization If you created the geometry etc using command line code most of these changes will already be made However if you used GUI to create this file there are several occasions where you used the graphical picking device Therefore the actual items that were chosen need to be entered The code P51X symbolizes the graphical selection To modify the file simply open it using notepad and make the required changes Save and close the file once you have made all of the required changes The following is a list of the changes which need to be made to this file which was created using the GUI method H Line 32 DKP51X 0 0UXUY Change this to DK1 0 0UXUY This specifies the constraints at keypoint 1 H Line 37 DKP51X 0 0UY Change to DK2 0 0UY This specifies the constraints at keypoint 2 H Line 42 FKP51XFY2000 Change to FK3FY2000 This specifies the force applied on the beam There are also several lines which can be removed from this file If you are comfortable with command line coding you should remove the lines which you are certain are not required 2 Assign the Command File to the Optimization H Select Main Menu Design Opt Analysis File Assign H In the file list that appears select the filename that you created when you wrote the command file H Click OK 3 Define Variables and Tolerances ANSYS needs to know which variables are critical to the optimization To define variables we need to know which variables have an effect on the variable to be minimized In this example our objective is to minimize the volume of a beam which is directly related to the weight of the beam ANSYS categorizes three types of variables for design optimization Design Variables DVs Independent variables that directly effect the design objective In this example the width and height of the beam are the DVs Changing either variable has a direct effect on the solution of the problem State Variables SVs Dependent variables that change as a result of changing the DVs These variables are necessary to constrain the design In this example the SV is the maximum stress in the beam Without this SV our optimization will continue until both the width and height are zero This would minimize the weight to zero which is not a useful result Objective Variable OV The objective variable is the one variable in the optimization that needs to be minimized In our problem we will be minimizing the volume of the beam NOTE As previously stated none of the variables defined in ANSYS are allowed to have negative values Now that we have decided our design variables we need to define ranges and tolerances for each variable For the width and height we will select a range of 10 to 50 mm for each Because a small change in either the width or height has a profound effect on the volume of the beam we will select a tolerance of 001mm Tolerances are necessary in that they tell ANSYS the largest amount of change that a variable can experience before convergence of the problem For the stress variable we will select a range of 195 to 200 MPa with a tolerance of 001MPa Because the volume variable is the objective variable we do not need to define an allowable range We will set the tolerance to 200mm3 This tolerance was chosen because it is significantly smaller than the initial magnitude of the volume of 400000mm3 20mm x 20mm x 1000mm a Define the Design Variables width and height of beam I Select Main Menu Design Opt Design Variables Add I Complete the window as shown below to specify the variable limits and tolerances for the height of the beam I Repeat the above steps to specify the variable limits for the width of the beam identical to specifications for height b Define the State Variables I Select Main Menu Design Opt State Variables Add I In the window fill in the following sections I Select SMAX in the Parameter Name section I Enter Lower Limit MIN 195 I Upper Limit MAX 200 I Feasibility Tolerance TOLER 0001 c Define the Objective Variable I Select Main Menu Design Opt Objective I Select VOLUME in the Parameter Name section I Under Convergence Tolerance enter 200 6 Define the Optimization Method There are several different methods that ANSYS can use to solve an optimization problem To ensure that you are not finding a solution at a local minimum it is advisable to use different solution methods If you have trouble with getting a particular problem to converge it would be a good idea to try a different method of solution to see what might be wrong For this problem we will use a FirstOrder Solution method H Select Main Menu Design Opt Method Tool H In the Specify Optimization Method window select FirstOrder H Click OK H Enter Maximum iterations NITR 30 Percent step size SIZE 100 Percent forward diff DELTA 02 H Click OK Note the significance of the above variables is explained below NITR Max number of iterations Defaults to 10 SIZE that is applied to the size of each line search step Defaults to 100 DELTA forward difference applied to the design variable range that is used to compute the gradient Defaults to 02 7 Run the Optimization H Select Main Menu Design Opt Run H In the Begin Execution of Run window confirm that the analysis file methodtype and maximum iterations are correct H Click OK The solution of an optimization problem can take awhile before convergence This problem will take about 15 minutes and run through 19 iterations View the Results 1 View Final Parameters Utility Menu Parameters Scalar Parameters You will probably see that the width1324 mm height2916 mm and the stress is equal to 19983 MPa with a volume of 386100mm2 2 View graphical results of each variable during the solution H Select Main Menu Design Opt Design Sets Graphs Tables H Complete the window as shown to obtain a graph of the height and width of the beam changing with each iteration A For the Xvariable parameter select Set number B For the Yvariable parameter select H and W C Ensure that Graph is selected as opposed to List Now you may wish to specify titles for the X and Y axes H Select Utility Menu Plot Ctrls Style Graphs Modify Axes H In the window enter Number of Iterations for the Xaxis label section H Enter Width and Height mm for the Yaxis label H Click OK H Select Utility Menu PlotCtrls In the graphics window you will see a graph of width and height throughout the optimization You can print the plot by selecting Utility Menu PlotCtrls Hard Copy You can plot graphs of the other variables in the design by following the above steps Instead of using width and height for the yaxis label and variables use whichever variable is necessary to plot Alternatively you could list the data by selecting Main Menu Design Opt Design Sets List In addition all of the results data ie stress displacement bending moments are available from the General Postproc menu Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing Analytical Solution UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Substructuring Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the how to use substructuring in ANSYS Substructuring is a procedure that condenses a group of finite elements into one superelement This reduces the required computation time and also allows the solution of very large problems A simple example will be demonstrated to explain the steps required however please note that this model is not one which requires the use of substructuring The example involves a block of wood E 10 GPa v 029 connected to a block of silicone E 25 MPa v 041 which is rigidly attached to the ground A force will be applied to the structure as shown in the following figure For this example substructuring will be used for the wood block The use of substructuring in ANSYS is a three stage process 1 Generation Pass Generate the superelement by condensing several elements together Select the degrees of freedom to save master DOFs and to discard slave DOFs Apply loads to the superelement 2 Use Pass Create the full model including the superelement created in the generation pass Apply remaining loads to the model The solution will consist of the reduced solution tor the superelement and the complete solution for the nonsuperelements 3 Expansion Pass Expand the reduced solution to obtain the solution at all DOFs for the superelement Note that a this method is a bottomup substructuring each superelement is created separately and then assembled in the Use Pass Top down substructuring is also possible in ANSYS the entire model is built then superelement are created by selecting the appropriate elements This method is suitable for smaller models and has the advantage that the results for multiple superelements can be assembled in postprocessing Expansion Pass Creating the Superelement Preprocessing Defining the Problem 1 Give Generation Pass a Jobname Utility Menu File Change Jobname Enter GEN for the jobname 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create geometry of the superelement Preprocessor Modeling Create Areas Rectangle By 2 Corners BLC4XCORNERYCORNERWIDTHHEIGHT Create a rectangle with the dimensions all units in mm XCORNER WP X 0 YCORNER WP Y 40 Width 100 Height 100 4 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use PLANE42 2D structural solid This element has 4 nodes each with 2 degrees of freedom translation along the X and Y axes 5 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for wood i Youngs modulus EX 10000 MPa ii Poissons Ratio PRXY 029 6 Define Mesh Size Preprocessor Meshing Size Cntrls Manual Size Areas All Areas For this example we will use an element edge length of 10mm 7 Mesh the block Preprocessor Meshing Mesh Areas Free click Pick All AMESH1 Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Substructuring ANTYPESUBST 2 Select Substructuring Analysis Options It is necessary to define the substructuring analysis options H Select Solution Analysis Type Analysis Options H The following window will appear Ensure that the options are filled in as shown I Sename the name of the superelement matrix file will default to the jobname I In this case the stiffness matrix is to be generated I With the option SEPR the stiffness matrix or load matrix can be printed to the output window if desired 3 Select Master Degrees of Freedom Master DOFs must be defined at the interface between the superelement and other elements in addition to points where loads constraints are applied H Select Solution Master DOFs User Selected Define H Select the Master DOF as shown in the following figure H In the window that appears set the 1st degree of freedom to All DOF 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Nodes Place a load of 5N in the x direction on the top left hand node The model should now appear as shown in the figure below 5 Save the database Utility Menu File Save as Jobnamedb SAVE Save the database to be used again in the expansion pass 6 Solve the System Solution Solve Current LS SOLVE Use Pass Using the Superelement The Use Pass is where we model the entire model including the superelements from the Generation Pass Preprocessing Defining the Problem 1 Clear the existing database Utility Menu File Clear Start New 2 Give Use Pass a Jobname Utility Menu File Change Jobname FILNAME USE Enter USE for the jobname 3 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 Now we need to bring the Superelement into the model 4 Define the Superelement Type Preprocessor Element Type AddEditDelete Select Superelement MATRIX50 5 Create geometry of the nonsuperelement Silicone Preprocessor Modeling Create Areas Rectangle By 2 Corners BLC4XCORNERYCORNERWIDTHHEIGHT Create a rectangle with the dimensions all units in mm XCORNER WP X 0 YCORNER WP Y 0 Width 100 Height 40 6 Define the NonSuperelement Type Preprocessor Element Type AddEditDelete We will again use PLANE42 2D structural solid 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for silicone i Youngs modulus EX 25 MPa ii Poissons Ratio PRXY 041 8 Define Mesh Size Preprocessor Meshing Size Cntrls Manual Size Areas All Areas For this block we will again use an element edge length of 10mm Note that is is imperative that the nodes of the non superelement match up with the superelement MDOFs 9 Mesh the block Preprocessor Meshing Mesh Areas Free click Pick All AMESH1 10 Offset Node Numbering Since both the superelement and the nonsuperelement were created independently they contain similarly numbered nodes ie both objects will have node 1 etc If we bring in the superelement with similar node numbers the nodes will overwrite existing nodes from the nonsuperelements Therefore we need to offset the superelement nodes Determine the number of nodes in the existing model H Select Utility Menu Parameters Get Scalar Data H The following window will appear Select Model Data For Selected set as shown H Fill in the following window as shown to set MaxNode the highest node number Offset the node numbering H Select Preprocessor Modeling Create Elements Superelements BY CS Transfer H Fill in the following window as shown to offset the node numbers and save the file as GEN2 Read in the superelement matrix H Select Preprocessor Modeling Create Elements Superelements From SUB File H Enter GEN2 as the Jobname of the matrix file in the window shown below H Utility Menu Plot Replot 11 Couple Node Pairs at Interface of Superelement and NonSuperelements Select the nodes at the interface H Select Utility Menu Select Entities H The following window will appear Select Nodes By Location Y coordinates 40 as shown Couple the pair nodes at the interface H Select Preprocessor Coupling Ceqn Coincident Nodes Reselect all of the nodes H Select Utility Menu Select Entities H In the window that appears click Nodes By NumPick From Full Sele All Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Lines Fix the bottom line ie all DOF constrained 3 Apply superelement load vectors H Determine the element number of the superelement Select Utility Menu PlotCtrls Numbering You should find that the superelement is element 41 H Select Solution Define Loads Apply Load Vector For Superelement H The following window will appear Fill it in as shown to apply the superelement load vector 4 Save the database Utility Menu File Save as Jobnamedb SAVE Save the database to be used again in the expansion pass 5 Solve the System Solution Solve Current LS SOLVE General Postprocessing Viewing the Results 1 Show the Displacement Contour Plot General Postproc Plot Results Contour Plot Nodal Solution DOF solution Translation USUM PLNSOLUSUM01 Note that only the deformation for the nonsuperelements is plotted This results agree with what was found without using substructuring see figure below Expansion Pass Expanding the Results within the Superelement To obtain the solution for all elements within the superelement you will need to perform an expansion pass Preprocessing Defining the Problem 1 Clear the existing database Utility Menu File Clear Start New 2 Change the Jobname back to Generation pass Jobname Utility Menu File Change Jobname FILNAME GEN Enter GEN for the jobname 3 Resume Generation Pass Database Utility Menu File Resume Jobnamedb RESUME Solution Phase Assigning Loads and Solving 1 Activate Expansion Pass H Enter the Solution mode by selecting Main Menu Solution or by typing SOLU into the command line H Type EXPASSON into the command line to initiate the expansion pass 2 Enter the Superelement name to be Expanded H Select Solution Load STEP OPTS ExpansionPass Single Expand Expand Superelem H The following window will appear Fill it in as shown to select the superelement 3 Enter the Superelement name to be Expanded H Select Solution Load Step Opts ExpansionPass Single Expand By Load Step H The following window will appear Fill it in as shown to expand the solution 4 Solve the System Solution Solve Current LS SOLVE General Postprocessing Viewing the Results 1 Show the Displacement Contour Plot General Postproc Plot Results Contour Plot Nodal Solution DOF solution Translation USUM PLNSOLUSUM01 Note that only the deformation for the superelements is plotted and that the contour intervals have been modified to begin at 0 This results agree with what was found without using substructuring see figure below Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Coupled StructuralThermal Analysis Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to outline a simple coupled thermalstructural analysis 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 attemp to expand However since it is pinned this cannot occur and as such stress is created in the link A steadystate 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 degrees Celsius The link is steel with a modulus of elasticity of 200 GPa a thermal conductivity of 605 WmK and a thermal expansion coefficient of 12e6 K Preprocessing Defining the Problem According to Chapter 2 of the ANSYS CoupledField Guide A sequentially coupled physics analysis is the combination of analyses from different engineering disciplines which interact to solve a global engineering problem For convenience the solutions and procedures associated with a particular engineering discipline will be referred to as a physics analysis When the input of one physics analysis depends on the results from another analysis the analyses are coupled Thus each different physics environment must be constructed seperately so they can be used to determine the coupled physics solution However it is important to note that a single set of nodes will exist for the entire model By creating the geometry in the first physical environment and using it with any following coupled environments the geometry is kept constant For our case we will create the geometry in the Thermal Environment where the thermal effects will be applied Although the geometry must remain constant the element types can change For instance thermal elements are required for a thermal analysis while structural elements are required to deterime the stress in the link It is important to note however that only certain combinations of elements can be used for a coupled physics analysis For a listing see Chapter 2 of the ANSYS CoupledField Guide located in the help file The process requires the user to create all the necessary environments which are basically the preprocessing portions for each environment and write them to memory Then in the solution phase they can be combined to solve the coupled analysis Thermal Environment Create Geometry and Define Thermal Properties 1 Give example a Title Utility Menu File Change Title title Thermal Stress Example 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxyz We are going to define 2 keypoints for this link as given in the following table Keypoint Coordinates xyz 1 00 2 10 4 Create Lines Preprocessor Modeling Create Lines Lines In Active Coord L12 Create a line joining Keypoints 1 and 2 representing a link 1 meter long 5 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the LINK33 Thermal Mass Link 3D conduction element This element is a uniaxial element with the ability to conduct heat between its nodes 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for LINK33 window enter the following geometric properties i Crosssectional area AREA 4e4 This defines a beam with a crosssectional area of 2 cm X 2 cm 7 Define Element Material Properties Preprocessor Material Props Material Models Thermal Conductivity Isotropic In the window that appears enter the following geometric properties for steel i KXX 605 8 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will use an element edge length of 01 meters 9 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All 10 Write Environment The thermal environment the geometry and thermal properties is now fully described and can be written to memory to be used at a later time Preprocessor Physics Environment Write In the window that appears enter the TITLE Thermal and click OK 11 Clear Environment Preprocessor Physics Environment Clear OK Doing this clears all the information prescribed for the geometry such as the element type material properties etc It does not clear the geometry however so it can be used in the next stage which is defining the structural environment Structural Environment Define Physical Properties Since the geometry of the problem has already been defined in the previous steps all that is required is to detail the structural variables 1 Switch Element Type Preprocessor Element Type Switch Elem Type Choose Thermal to Struc from the scoll down list This will switch to the complimentary structural element automatically In this case it is LINK 8 For more information on this element see the help file A warning saying you should modify the new element as necessary will pop up In this case only the material properties need to be modified as the geometry is staying the same 2 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs Modulus EX 200e9 ii Poissons Ratio PRXY 03 Preprocessor Material Props Material Models Structural Thermal Expansion Coef Isotropic i ALPX 12e6 3 Write Environment The structural environment is now fully described Preprocessor Physics Environment Write In the window that appears enter the TITLE Struct Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Read in the Thermal Environment Solution Physics Environment Read Choose thermal and click OK If the Physics option is not available under Solution click Unabridged Menu at the bottom of the Solution menu This should make it visible 3 Apply Constraints Solution Define Loads Apply Thermal Temperature On Keypoints Set the temperature of Keypoint 1 the leftmost point to 348 Kelvin 4 Solve the System Solution Solve Current LS SOLVE 5 Close the Solution Menu Main Menu Finish It is very important to click Finish as it closes that environment and allows a new one to be opened without contamination If this is not done you will get error messages The thermal solution has now been obtained If you plot the steadystate temperature on the link you will see it is a uniform 348 K as expected This information is saved in a file labelled Jobnamerth were rth is the thermal results file Since the jobname wasnt changed at the beginning of the analysis this data can be found as filerth We will use these results in determing the structural effects 6 Read in the Structural Environment Solution Physics Environment Read Choose struct and click OK 7 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix Keypoint 1 for all DOFs and Keypoint 2 in the UX direction 8 Include Thermal Effects Solution Define Loads Apply Structural Temperature From Therm Analy As shown below enter the file name Filerth This couples the results from the solution of the thermal environment to the information prescribed in the structural environment and uses it during the analysis 9 Define Reference Temperature Preprocessor Loads Define Loads Settings Reference Temp For this example set the reference temperature to 273 degrees Kelvin 10 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Hand Calculations Hand calculations were performed to verify the solution found using ANSYS As shown the stress in the link should be a uniform 180 MPa in compression 2 Get Stress Data Since the element is only a line the stress cant be listed in the normal way Instead an element table must be created first General Postproc Element Table Define Table Add Fill in the window as shown below CompStr By Sequence Num LS LS1 ETABLECompStressLS1 3 List the Stress Data General Postproc Element Table List Elem Table COMPSTR OK PRETABCompStr The following list should appear Note the stress in each element 0180e9 Pa or 180 MPa in compression as expected Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Using PElements Introduction This tutorial was completed using ANSYS 70 This tutorial outlines the steps necessary for solving a model meshed with pelements The pmethod manipulates the polynomial level plevel of the finite element shape functions which are used to approximate the real solution Thus rather than increasing mesh density the plevel can be increased to give a similar result By keeping mesh density rather coarse computational time can be kept to a minimum This is the greatest advantage of using pelements over helements A uniform load will be applied to the right hand side of the geometry shown below The specimen was modeled as steel with a modulus of elasticity of 200 GPa Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title PMethod Meshing 2 Activate the pMethod Solution Options ANSYS Main Menu Preferences PMETHON Select pMethod Struct as shown below 3 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 4 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxyz We are going to define 12 keypoints for this geometry as given in the following table Keypoint Coordinates xyz 1 00 2 0100 3 20100 4 4552 5 5552 6 80100 7 100100 8 1000 9 800 10 5548 11 4548 12 200 5 Create Area Preprocessor Modeling Create Areas Arbitrary Through KPs A123456789101112 Click each of the keypoints in numerical order to create the area shown below 6 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the PLANE145 pElements 2D Quad element This element has eight nodes with 2 degrees of freedom each translation along the X and Y axes It can support a polynomial with maximum order of eight After clicking OK to select the element click Options to open the keyoptions window shown below Choose Plane stress TK for Analysis Type Keyopts 1 and 2 can be used to set the starting and maximum plevel for this element type For now we will leave them as default Other types of pelements exist in the ANSYS library These include Solid127 and Solid128 which have electrostatic DOFs and Plane145 Plane146 Solid147 Solid148 and Shell150 which have structural DOFs For more information on these elements go to the Element Library in the help file 7 Define Real Constants Preprocessor Real Constants Add In the Real Constants for PLANE145 window enter the following geometric properties i Thickness THK 10 This defines an element with a thickness of 10 mm 8 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 9 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas For this example we will use an element edge length of 5mm 10 Mesh the frame Preprocessor Meshing Mesh Areas Free click Pick All Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Set Solution Controls Solution Analysis Type Soln Controls The following window will pop up A Set Time at end of loadstep to 1 and Automatic time stepping to ON B Set Number of substeps to 20 Max no of substeps to 100 Min no of substeps to 20 C Set the Frequency to Write every substep 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Lines Fix the left side of the area ie all DOF constrained 4 Apply Loads Solution Define Loads Apply Pressure On Lines Apply a pressure of 100 Nmm2 The applied loads and constraints should now appear as shown in the figure below 5 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Read in the Last Data Set General Postproc Read Results Last Set 2 Plot Equivalent Stress General Postproc Plot Results Contour Plot Element Solu In the window that pops up select Stress von Mises SEQV The following stress distribution should appear 3 Plot pLevels General Postproc Plot Results pMethod pLevels The following distribution should appear Note how the order of the polynomial increased in the area with the greatest range in stress This allowed the elements to more accurately model the stress distribution through that area For more complex geometries these orders may go as high as 8 As a comparison a plot of the stress distribution for a normal helement PLANE2 model using the same mesh and one with a mesh 5 times finer are shown below ELEMENT SOLUTION As one can see from the two plots the mesh density had to be increased by 5 times to get the accuracy that the pelements delivered This is the benefit of using pelements You can use a mesh that is relatively coarse thus computational time will be low and still get reasonable results However care should be taken using pelements as they can sometimes give poor results or take a long time to converge Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Melting Using Element Death Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to outline the steps required to use element death to model melting of a material Element death is the turning off of elements according to some desired criterion The elements are still technically there they just have zero stiffness and thus have no affect on the model This tutorial doesnt take into account heat of fusion or changes in thermal properties over temperature ranges rather it is concerned with the element death procedure More accurate models using element death can then be created as required Element birth is also possible but will not be discussed here For further information see Chapter 10 of the Advanced Guide in the ANSYS help file regarding element birth and death The model will be an infinitely long rectangular block of material 3cm X 3cm as shown below It will be subject to convection heating which will cause the block to melt Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title Element Death 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create Rectangle Preprocessor Modeling Create Areas Rectangle By 2 Corners Fill in the window with the following dimensions WP X 0 WP Y 0 Width 003 Height 003 BLC400003003 4 Define the Type of Element Preprocessor Element Type AddEditDelete For this example we will use PLANE55 Thermal Solid Quad 4node 55 This element has 4 nodes and a single DOF temperature at each node PLANE55 can only be used for 2 dimensional steadystate or transient thermal analysis 5 Define Element Material Properties Preprocessor Material Props Material Models Thermal Conductivity Isotropic In the window that appears enter the following properties i Thermal Conductivity KXX 18 Preprocessor Material Props Material Models Thermal Specific Heat In the window that appears enter the following properties i Specific Heat C 2040 Preprocessor Material Props Material Models Thermal Density In the window that appears enter the following properties i Density DENS 920 6 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Areas For this example we will use an element edge length of 00005m 7 Mesh the frame Preprocessor Meshing Mesh Areas Free click Pick All Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Transient The window shown below will pop up We will use the defaults so click OK ANTYPE4 2 Turn on NewtonRaphson solver Due to a glitch in the ANSYS software there is no apparent way to do this with the graphical user interface Therefore you must type NROPTFULL into the commmand line This step is necessary as element killing can only be done when the N R solver has been used 3 Set Solution Controls Solution Analysis Type Soln Controls The following window will pop up A Set Time at end of loadstep to 60 and Automatic time stepping to OFF B Set Number of substeps to 20 C Set the Frequency to Write every substep Click on the NonLinear tab at the top and fill it in as shown D Set Line search to ON E Set the Maximum number of iterations to 100 For a complete description of what these options do refer to the help file Basically the time at the end of the load step is how long the transient analysis will run and the number of substeps defines how the load is broken up By writing the data at every step you can create animations over time and the other options help the problem converge quickly 4 Apply Initial Conditions Solution Define Loads Apply Initial Conditn Define Pick All Fill in the IC window as follows to set the initial temperature of the material to 268 K 5 Apply Boundary Conditions For thermal problems constraints can be in the form of Temperature Heat Flow Convection Heat Flux Heat Generation or Radiation In this example all external surfaces of the material will be subject to convection with a coefficient of 10 Wm2K and a surrounding temperature of 368 K Solution Define Loads Apply Thermal Convection On Lines Pick All Fill in the popup window as follows with a film coefficient of 10 and a bulk temperature of 368 The model should now look as follows H Solve the System Solution Solve Current LS SOLVE Postprocessing Prepare for Element Death 1 Read Results General Postproc Read Results Last Set SETLAST 2 Create Element Table Element death can be used in various ways For instance the user can manually kill or turn off elements to create the desired effect Here we will use data from the analysis to kill the necessary elements to model melting Assume the material melts at 273 K We must create an element table containing the temperature of all the elements H From the General Postprocessor menu select Element Table Define Table H Click on Add H Fill the window in as shown below with a title Melty and select DOF solution Temperature TEMP and click OK We can now select elements from this table in the temperature range we desire 3 Select Elements to Kill Assume that the melting temperature is 273 K thus any element with a temperature of 273 or greater must be killed to simulate melting Utility Menu Select Entities Use the scroll down menus to select Elements By Results From Full and click OK Ensure the element table Melty is selected and enter a VMIN value of 273 as shown Solution Phase Killing Elements 1 Restart the Analysis Solution Analysis Type Restart OK You will likely have two messages pop up at this point Click OK to restart the analysis and close the warning message The reason for the warning is ANSYS defaults to a multiframe restart which this analysis doesnt call for thus it is just warning the user 2 Kill Elements The easiest way to do this is to type ekillall into the command line Since all elements above melting temperature had been selected this will kill only those elements The other option is to use Solution Load Step Opts Other Birth Death Kill Elements and graphically pick all the melted elements This is much too time consuming in this case Postprocessing Viewing Results 1 Select Live Elements Utility Menu Select Entities Fill in the window as shown with Elements Live Elems Unselect and click Sele All With the window still open select Elements Live Elems From Full and click OK 2 View Results General Postproc Plot Results Contour Plot Nodal Solu DOF solution Temperature TEMP The final melted shape should look as follows This procedure can be programmed in a loop using command line code to more accurately model element death over time Rather than running the analysis for a time of 60 and killing any elements above melting temperature at the end a check can be done after each substep to see if any elements are above the specified temperature and be killed at that point That way the prescribed convection can then act on the elements below those killed more accurately modelling the heating process Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Contact Elements Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to utilize contact elements to simulate how two beams react when they come into contact with each other The beams as shown below are 100mm long 10mm x 10mm in crosssection have a Youngs modulus of 200 GPa and are rigidly constrained at the outer ends A 10KN load is applied to the center of the upper causing it to bend and contact the lower Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title Contact Elements 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Define Areas Preprocessor Modeling Create Area Rectangle By 2 Corners BLC4WP X WP Y Width Height We are going to define 2 rectangles as described in the following table Rectangle Variables WP XWP YWidthHeight 1 0 15 100 10 2 50 0 100 10 4 Define the Type of Element H Preprocessor Element Type AddEditDelete For this problem we will use the PLANE42 Solid Quad 4node 42 element This element has 2 degrees of freedom at each node translation along the X and Y H While the Element Types window is still open click Options Change Element behavior K3 to Plane strs w thk as shown below This allows a thickness to be input for the elements 5 Define Real Constants Preprocessor Real Constants Add In the Real Constants for PLANE42 window enter the following geometric properties i Thickness THK 10 This defines a beam with a thickness of 10 mm 6 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 7 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Areas All Lines For this example we will use an element edge length of 2mm 8 Mesh the frame Preprocessor Meshing Mesh Areas Free click Pick All 9 Define the Type of Contact Element H Preprocessor Element Type AddEditDelete For this problem we will use the CONTAC48 Contact pttosurf 48 element CONTAC48 may be used to represent contact and sliding between two surfaces or between a node and a surface in 2D The element has two degrees of freedom at each node translations in the nodal x and y directions Contact occurs when the contact node penetrates the target line H While the Element Types window is still open click Options Change Contact timeload prediction K7 to Reasonabl TL inc This is an important step It initiates a process during the solution calculations where the time step or load step depending on what the user has specified in the solution controls incremements slowly when contact is immenent This way one surface wont penetrate too far into the other and cause the solution to fail It is important to note CONTAC48 elements are created in the space between two surfaces prescribed by the user This will be covered below As the surfaces approach each other the contact element is slowly crushed until its upper nodes lie along the same line as the lower nodes Thus ANSYS can calculate when the two prescribed surfaces have made contact Other contact elements such as CONTA175 require a target element such as TARGE169 to function When using contact elements in your own analyses be sure to understand how the elements work The ANSYS help file has plenty of useful information regarding contact elements and is worth reading 10 Define Real Constants for the Contact Elements Preprocessor Real Constants Add In the Real Constants for CONTAC48 window enter the following properties i Normal contact stiffness KN 200000 CONTAC48 elements basically use a penalty approach to model contact When one surface comes into contact with the other ANSYS numerically puts a spring of stiffness KN between the two ANSYS recommends a value between 001 and 100 times Youngs modulus for the material Since this spring is so stiff the behaviour of the model is like the two surfaces have made contact This KN value can greatly affect your solution so be sure to read the help file on contact so you can recognize when your solution is not converging and why A good rule of thumb is to start with a low value of KN and see how the solution converges start watching the ANSYS Output Window If there is too much penetration you should increase KN If it takes a lot of iterations to converge for a single substep you should decrease KN ii Target length tolerance TOLS 10 Real constant TOLS is used to add a small tolerance that will internally increase the length of the target This is useful for problems when node to node contact is likely to occur rather than node to element edge In this situation the contact node may repeatedly slip off one of the target nodes resulting in convergence difficulties A small value of TOLS given in is usually enough to prevent such difficulties The other real constants can be used to model sliding friction tolerances etc Information about these other constants can be found in the help file 11 Define Nodes for Creating Contact Elements Unlike the normal meshing sequence used for most elements contact elements must be defined in a slightly different manner Sets of nodes that are likely to come into contact must be defined and used to generate the necessary elements ANSYS has many recommendations about which nodes to select and whether they should act as target nodes or source nodes In this simple case source nodes are those that will move into contact with the other surface where as target nodes are those that are contacted These terms are important when using the automatic contact element mesher to ensure the elements will correctly model contact between the surfaces A strong understanding of how the elements work is important when using contact elements for your own analysis First the source nodes will be selected I Utility Menu Select Entities Select Areas and By NumPick from the pull down menus select From Full from the radio buttons and click OK Select the top beam and click OK This will ensure any nodes that are selected in the next few steps will be from the upper beam In this case it is not too hard to ensure you select the correct nodes However when the geometry is complex you may inadvertantly select a node from the wrong surface and it could cause problems during element generation I Utility Menu Select Entities Select Nodes and By Location from the pull down menus Y coordinates and Reselect from the radio buttons and enter a value of 15 and click OK This will select all nodes along the bottom of the upper beam I Utility Menu Select Entities Select Nodes and By Location from the pull down menus X coordinates and Reselect from the radio buttons and enter values of 50100 This will select the nodes above the lower beam I Now if you list the selected nodes Utility Menu List Nodes you should only have the following nodes remaining It is important to try and limit the number of nodes you use to create contact elements If you have a lot of contact elements it takes a great deal of computational time to reach a solution In this case the only nodes that could make contact with the lower beam are those directly above it thus those are the only nodes we will use to create the contact elements I Utility Menu Select CompAssembly Create Component Enter the component name Source as shown below and click OK Now we can use this component Source as a list of nodes to be used in other functions This can be very useful in other applications as well Now select the target nodes Using the same procedure as above select the nodes on the lower beam directly under the upper beam Be sure to reselect all nodes before starting to select others This is done by opening the entity select menu Utility Menu Select Entities clicking the Also Select radio button and click the Sele All button These values will be the ones youll use I Click the lower area for the area select I The Y coordinate is 10 I The X coordinates vary from 50 to 100 When creating the component this time enter the name Target IMPORTANT Be sure to reselect all the nodes before continuing This is done by opening the entity select menu Utility Menu Select Entities clicking the Also Select radio button and click the Sele All button 12 Generate Contact Elements Main Menu Preprocessor Modeling Create Elements Elem Attributes Fill the window in as shown below This ensures ANSYS knows that you are dealing with the contact elements and the associated real constants Main Menu Preprocessor Modeling Create Elements Surf Contact Node to Surf The following window will pop up Select the node set SOURCE from the first drop down menu Ccomp and TARGET from the second drop down menu Tcomp The rest of the selections remain unchanged At this point your model should look like the following Unfortunately the contact elements dont get plotted on the screen so it is sometimes difficult to tell they are there If you wish you can plot the elements Utility Menu Plot Elements and turn on element numbering Utility Menu PlotCtrls Numbering ElemAttrib numbering Element Type Numbers If you zoom in on the contact areas you can see little purple stars Contact Nodes and thin purple lines Target Elements numbered 2 which correspond to the contact elements shown below The preprocessor stage is now complete Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Set Solution Controls H Select Solution Analysis Type Soln Control The following image will appear Ensure the following selections are made under the Basic tab as shown above A Ensure Automatic time stepping is on Automatic time stepping allows ANSYS to determine appropriate sizes to break the load steps into Decreasing the step size usually ensures better accuracy however this takes time The Automatic Time Step feature will determine an appropriate balance This feature also activates the ANSYS bisection feature which will allow recovery if convergence fails B Enter 100 as the number of substeps This will set the initial substep to 1100 th of the total load C Enter a maximum number of substeps of 1000 This stops the program if the solution does not converge after 1000 steps D Enter a minimum number of substeps of 20 E Ensure all solution items are writen to a results file Ensure the following selection is made under the Nonlinear tab as shown below A Ensure Maximum Number of Iterations is set to 100 NOTE There are several options which have not been changed from their default values For more information about these commands type help followed by the command into the command line These solution control values are extremely important in determining if your analysis will succeed or fail If you have too few substeps the contact nodes may be driven through the target elements before ANSYS realizes it has happened In this case the solution will resemble that of an analysis that didnt have contact elements defined at all Therefore it is important to choose a relatively large number of substeps initially to ensure the model is defined properly Once everything is working you can reduce the number of substeps to optimize the computational time Also if the maximum number of substeps or iterations is left too low ANSYS may stop the analysis before it has a chance to converge to a solution Again leave these relatively high at first 3 Apply Constraints Solution Define Loads Apply Structural Displacement On Lines Fix the left end of the upper beam and the right end of the lower beam ie all DOF constrained 4 Apply Loads Solution Define Loads Apply Structural ForceMoment On Nodes Apply a load of 10000 in the FY direction to the center of the top surface of the upper beam Note this is a point load on a 2D surface This type of loading should be avoided since it will cause a singularity However the displacement or stress near the load is not of interest in this analyis thus we will use a point load for simplicity The applied loads and constraints should now appear as shown in the figure below 5 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results 1 Open postprocessor menu ANSYS Main Menu General Postproc POST1 2 Adjust Graphical Scaling Utility Menu PlotCtrls Style Displacement Scaling Click the 10 true scale radio button then click ok This is of huge importance I lost many hours trying to figure out why the contact elements werent working when in fact it was just due to the displacement scaling to which ANSYS defaulted If you leave the scaling as default many times it will look like your contact nodes have gone through the target elements 3 Show the Stress Distribution in the Beams General Postproc Plot Results Contour Plot Nodal Solu Stress von Mises 4 Adjust Contour Scale Utility Menu PlotCtrls Style Contours NonUniform Contours Fill in the window as follows This should produce the following stress distribution plot As seen in the figure the load on the upper beam caused it to deflect and come in contact with the lower beam producing a stress distribution in both Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Springs and Joints Design Optimization Substructuring Coupled Field pElement Element Death Contact Elements APDL Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Parametric Design Language APDL Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to familiarize the user with the ANSYS Parametric Design Language APDL This will be a very basic introduction to APDL covering things like variable definition and simple looping Users familiar with basic programming languages will probably find the APDL very easy to use To learn more about APDL and see more complex examples please see the APDL Programmers Guide located in the help file This tutorial will cover the preprocessing stage of constructing a truss geometry Variables including length height and number of divisions of the truss will be requested and the APDL code will construct the geometry Preprocessing Use of APDL Shown below is the APDL code used to construct the truss shown above using a length of 200 m a height of 10 m and 20 divisions The following discussion will attempt to explain the commands used in the code It is assumed the user has been exposed to basic coding and can follow the logic finish clear prep7 askLENGTHHow long is the truss100 askHEIGHTHow tall is the truss20 askDIVISIONHow many cross supports even number2 DELTAL LENGTHDIVISION22 NUMK DIVISION 1 COUNT 1 XCOORD 0 doi1NUMK1 COUNT COUNT 1 OSCILATE 1COUNT XCOORD XCOORD DELTAL ifOSCILATEGT0THEN kiXCOORD0 else kiXCOORDHEIGHT endif enddo KEYP 0 doj1DIVISION1 KEYP KEYP 1 LKEYPKEYP1 ifKEYPLEDIVISION1THEN LKEYPKEYP2 endif enddo et1link1 r1100 mpex1200000 mpprxy103 esize1 lmeshall finish 1 ASK Command The ASK command prompts the user to input data for a variable In this case askLENGTHHow long is the truss100 prompts the user for a value describing the length of the truss This value is stored under the variable LENGTH Thus in later parts of the code LENGTH can be used in other commands rather than typing in 200 m The 100 value at the end of the string is the default value if the user were to enter no value and just hit the enter key 2 Variable Definition Using the Command ANSYS allows the user to define a variable in a few ways As seen above the ASK command can be used define a variable but this is usually only used for data that will change from run to run The SET command can also be used to define variables For more information on this command see the help file However the most intutitive method is to use It is used in the following manner the variable you wish to define some arguement This argument can be a single value or a mathematical expression as seen in the line defining DELTAL 3 DO Loops Doloops are useful when you want to repeat a command a known number of times The syntax for the expression is DO Par IVAL FVAL INC where Par is the parameter that will be incremented by the loop IVAL is the initial value the parameter starts as FVAL is the final value the parameter will reach and INC is the increment value that the parameter will be increased by during each iteration of the loop For example doi110K1 is a doloop which increases the parameter i from 1 to 10 in steps of 1 ie 1238910 It is necessary to use a ENDDO command at the end of the loop to locate where ANSYS should look for the next command once the loop has finished In between the DO and ENDDO the user can place code that will utilize the repetative characteristics of the loop 4 IF Statement Ifstatements can be used as decision makers determining if a certain case has occured For example in the code above there is a statement ifOSCILATEGT0THEN This translates to if the variable OSCILATE is greater than zero then Any code directly following the if command will be carried out if the statement is true If it is not true it will skip to the else command This command is only used in conjunction with the if command Any code directly following the else command will be carried out when the original statement is false An endif command is necessary after all code in the if and else sections to define an ending Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION XSectional Results Advanced XSec Res Data Plotting Graphical Properties Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Viewing XSectional Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to view cross sectional results Deformation Stress etc of the following example Preprocessing Defining the Problem 1 Give example a Title Utility Menu File Change Title title CrossSectional Results of a Simple Cantilever Beam 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Create Block Preprocessor Modeling Create Volumes Block By 2 Corners Z BLC400WidthHeightLength Where Width 40mm Height 60mm Length 400mm 4 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the SOLID45 3D Structural Solid element This element has 8 nodes each with 3 degrees of freedom translation along the X Y and Z directions 5 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 6 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Global Size esize20 For this example we will use an element size of 20mm 7 Mesh the volume Preprocessor Meshing Mesh Volumes Free click Pick All vmeshall Solution Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Areas Fix the left hand side should be labeled Area 1 3 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Apply a load of 2500N downward on the back right hand keypoint Keypoint 7 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results Now since the purpose of this tutorial is to observe results within different crosssections of the colume we will first outline the steps required to view a slice G Offset the working plane for a cross section view WPOFFS G Select the TYPE of display for the sectionTYPE For this example we are trying to display a section therefore options 1 5 or 8 are relevant and are summarized in the table below Type Description Visual Representation SECT or 1 Section display Only the selected section is shown without any remaining faces or edges shown CAP or 5 Capped hidden diplay This is as though you have cut off a portion of the model and the remaining model can be seen ZQSL or 8 QSLICE Zbuffered display This is the same as SECT but the outline of the entire model is shown G Align the cutting plane with the working planeCPLANE 1 Deflection Before we begin selecting cross sections lets view deflection of the entire model H Select General Postproc Plot Results Contour Plot Nodal Solu From this one may wish to view several cross sections through the YZ plane To illustrate how to take a cross section lets take one halfway through the beam in the YZ plane H First offset the working plane to the desired position halfway through the beam Select Utility Menu WorkPlane Offset WP by Increments In the window that appears increase Global X to 30 Width2 and rotate Y by 90 degrees H Select the type of plot and align the cutting plane with the working plane Note that in GUI these two steps are combined Select Utility Menu PlotCtrls Style HiddenLine Options Fill in the window that appears as shown below to select TYPEZQSL and CPLANEWorking Plane As desired you should now have the following This can be repeated for any slice however note that the command lines required to do the same are as follows WPOFFSWidth200 Offset the working plane for crosssection view WPROTA0090 Rotate the working plane CPLANE1 Cutting plane defined to use the WP TYPE18 PLNSOLUSUM01 Also note that to realign the working plane with the active coordinate system simply use WPCSYS10 2 Equivalent Stress Again lets view stresses within the entire model First we need to realign the working plane with the active coordinate system Select Utility Menu WorkPlane Align WP with Active Coord Sys NOTE To check the position of the WP select Utility Menu WorkPlane Show WP Status Next we need to change TYPE to the default settingno hidden or section operations Select Utility Menu PlotCtrls Style Hidden Line Options And change the Type of Plot to Nonhidden H Select General Postproc Plot Results Contour Plot Nodal Solu Stress von Mises Lets say that we want to take a closer look at the base of the beam through the XY plane Because it is much easier we are going to use command line WPOFFS00116Length Offset the working plane CPLANE1 Cutting plane defined to use the WP TYPE15 Use the capped hidden display PLNSOLSEQV01 Note that we did not need to rotate the WP because we want to look at the XY plane which is the default Also note that we are using the capped hidden display this time You should now see the following 3 Animation Now for something a little more impressive lets show an animation of the Von Mises stress through the beam Unfortunately the ANSYS commands are not as user friendly as they could be but please bear with me H Select Utility Menu PlotCtrls Animate QSlice Contours H In the window that appears just change the Item to be contoured to Stress von Mises H You will then be asked to select 3 nodes the origin the sweep direction and the Y axis In the graphics window select the node at the origin of the coordinate system as the origin of the sweep the sweep will start there Next the sweep direction is in the Z direction so select any node in the z direction parallel to the first node Finally select the node in the back bottom left hand side corner as the Y axis You should now see an animated version of the contour slices through the beam For more information on how to modify the animation type help ancut into the command line Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION XSectional Results Advanced XSec Res Data Plotting Graphical Properties Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Advanced XSectional Results Using Paths to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to create and use paths to provide extra detail during post processing For example one may want to determine the effects of stress concentrators along a certain path Rather than plotting the entire contour plot a plot of the stress along that path can be made In this tutorial a steel plate measuring 100 mm X 200 mm X 10 mm will be used Three holes are drilled through the vertical centerline of the plate The plate is constrained in the ydirection at the bottom and a uniform distributed load is pulling on the top of the plate Preprocessing Defining the Problem 1 Give the example a Title H Utility Menu File Change Title title Use of Paths for Post Processing 2 Open preprocessor menu H ANSYS Main Menu Preprocessor PREP7 3 Define Rectangular Ares H Preprocessor Modeling Create Areas Rectangle By 2 Corners BLC400200100 H Create a rectangle where the bottom left corner has the coordinates 00 and the width and height are 200 and 100 respectively 4 Create Circles H Preprocessor Modeling Create Areas Circle Solid Circle cyl4WP XWP YRadius H Create three circles with parameters shown below Circle Parameters WP X WP Y Radius 1 50 50 10 2 100 50 10 3 150 50 10 5 Subtract the Circles H Preprocessor Modeling Operate Booleans Subtract Areas H First select the area to remain ie the rectangle and click OK Then select the areas to be subtracted ie the circles and click OK H The remaining area should look as shown below 6 Define the Type of Element H Preprocessor Element Type AddEditDelete H For this problem we will use the PLANE2 Solid Triangle 6node element This element has 2 degrees of freedom translation along the X and Y axes H In the Element Types window click Options and set Element behavior to Plane strs wthk 7 Define Real Constants H Preprocessor Real Constants Add H In the Real Constants for PLANE2 window enter a thickness of 10 8 Define Element Material Properties H Preprocessor Material Props Material Models Structural Linear Elastic Isotropic H In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 9 Define Mesh Size H Preprocessor Meshing Size Cntrls ManualSize Areas All Areas H For this example we will use an element edge length of 5mm 10 Mesh the Area H Preprocessor Meshing Mesh Areas Free click Pick All Solution Phase Assigning Loads and Solving 1 Define Analysis Type H Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints H Solution Define Loads Apply Structural Displacement On Lines H Constrain the bottom of the area in the UY direction 3 Apply Loads H Solution Define Loads Apply Structural Pressure On Lines H Apply a constant uniform pressure of 200 on the top of the area The model should now look like the figure below 4 Solve the System H Solution Solve Current LS SOLVE Postprocessing Viewing the Results To see the stress distribution on the plate you could create a normal contour plot which would have the distribution over the entire plate However if the stress near the holes are of interest you could create a path through the center of the plate and plot the stress on that path Both cases will be plotted below on a split screen 1 Contour Plot H Utility Menu PlotCtrls Window Controls Window Layout H Fill in the Window Layout as seen below H General Postproc Plot Results Contour Plot Nodal Solu Stress von Mises The display should now look like this To ensure the top plot is not erased when the second plot is created you must make a couple of changes H Utility Menu PlotCtrls Window Controls Window On or Off Turn window 1 off H To keep window 1 visible during replots select Utility Menu PlotCtrls Erase Option Erase Between Plots and ensure there is no checkmark meaning this function off H To have the next graph plot in the bottom half of the screen select Utility Menu PlotCtrls Window Controls Window Layout and select Window 2 Bottom Half Do not replot 2 Create Path H General PostProc Path Operations Define Path By Location H In the window shown below name the path Cutline and set the Number of divisions to 1000 H Fill the next two window in with the following parameters Parameters Path Point Number X Loc Y Loc Z Loc 1 0 50 0 2 200 50 0 When the third window pops up click Cancle because we only enabled two points on the path in the previous step 3 Map the Stress onto the Path Now the path is defined you must choose what to map to the path or in other words what results should be available to the path For this example equivalent stress is desired H General Postproc Path Operations Map onto Path H Fill the next window in as shown below Stress von Mises and click OK H The warning shown below will probably pop up This is just saying that some of the 1000 points you defined earlier are not on interpolation points special points on the elements therefore there is no data to map This is of little concern though since there are plenty of points that do lie on interpolation points to produce the necessary plot so disregard the warning 4 Plot the Path Data H General Postproc Path Operations Plot Path Item On Geometry H Fill the window in as shown below The display should look like the following Note there will be dots on the plot showing node locations Due to resolution restrictions these dots are not shown here This plot makes it easy to see how the stress is concentrated around the holes Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION XSectional Results Advanced XSec Res Data Plotting Graphical Properties Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Data Plotting Using Tables to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to plot Vertical Deflection vs Length of the following beam using tables a special type of array By plotting this data on a curve rather than using a contour plot finer resolution can be achieved This tutorial will use a steel beam 400 mm long with a 40 mm X 60 mm cross section as shown above It will be rigidly constrained at one end and a 2500 N load will be applied to the other Preprocessing Defining the Problem 1 Give the example a Title Utility Menu File Change Title title Use of Tables for Data Plots 2 Open preprocessor menu ANSYS Main Menu Preprocessor PREP7 3 Define Keypoints Preprocessor Modeling Create Keypoints In Active CS Kxyz We are going to define 2 keypoints for this beam as given in the following table Keypoint Coordinates xyz 1 00 2 4000 4 Create Lines Preprocessor Modeling Create Lines Lines In Active Coord L12 Create a line joining Keypoints 1 and 2 5 Define the Type of Element Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axes and rotation about the Z axis 6 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 2400 ii Area moment of inertia IZZ 320e3 iii Total beam height 40 This defines a beam with a height of 40 mm and a width of 60 mm 7 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 200000 ii Poissons Ratio PRXY 03 8 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will use an element edge length of 20mm 9 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All Solution Phase Assigning Loads and Solving 1 Define Analysis Type Solution Analysis Type New Analysis Static ANTYPE0 2 Apply Constraints Solution Define Loads Apply Structural Displacement On Keypoints Fix keypoint 1 ie all DOF constrained 3 Apply Loads Solution Define Loads Apply Structural ForceMoment On Keypoints Apply a load of 2500N on keypoint 2 The model should now look like the figure below 4 Solve the System Solution Solve Current LS SOLVE Postprocessing Viewing the Results It is at this point the tables come into play Tables a special type of array are basically matrices that can be used to store and process data from the analysis that was just run This example is a simplified use of tables but they can be used for much more For more information type help in the command line and search for Array Parameters 1 Number of Nodes Since we wish to plot the verticle deflection vs length of the beam the location and verticle deflection of each node must be recorded in the table Therefore it is necessary to determine how many nodes exist in the model Utility Menu List Nodes OK For this example there are 21 nodes Thus the table must have at least 21 rows 2 Create the Table H Utility Menu Parameters Array Parameters DefineEdit Add H The window seen above will pop up Fill it out as shown Graph Table 2221 Note there are 22 rows one more than the number of nodes The reason for this will be explained below Click OK and then close the DefineEdit window 3 Enter Data into Table First the horizontal location of the nodes will be recorded H Utility Menu Parameters Get Array Data H In the window shown below select Model Data Nodes H Fill the next window in as shown below and click OK Graph11 All Location X Naming the array parameter Graph11 fills in the table starting in row 1 column 1 and continues down the column Next the vertical displacement will be recorded H Utility Menu Parameters Get Array Data Results data Nodal results H Fill the next window in as shown below and click OK Graph12 All DOF solution UY Naming the array parameter Graph12 fills in the table starting in row 1 column 2 and continues down the column 4 Arrange the Data for Ploting Users familiar with the way ANSYS numbers nodes will realize that node 1 will be on the far left as it is keypoint 1 node 2 will be on the far right keypoint 2 and the rest of the nodes are numbered sequentially from left to right Thus the second row in the table contains the data for the last node This causes problems during plotting thus the information for the last node must be moved to the final row of the table This is why a table with 22 rows was created to provide room to move this data H Utility Menu Parameters Array Parameters DefineEdit Edit H The data for the end of the beam Xlocation 400 UY 0833 is in row two Cut one of the cells to be moved right click Copy or CtrlX press the down arrow to get to the bottom of the table and paste it into the appropriate column right click Paste or CtrlV When both values have been moved check to ensure the two entries in row 2 are zero Select File ApplyQuit 5 Plot the Data H Utility Menu Plot Array Parameters H The following window will pop up Fill it in as shown with the Xlocation data on the Xaxis and the vertical deflection on the Yaxis H To change the axis labels select Utility Menu Plot Ctrls Style Graphs Modify Axes H To see the changes to the labels select Utility Menu Replot H The plot should look like the one seen below Command File Mode of Solution The above example was solved using a mixture of the Graphical User Interface or GUI and the command language interface of ANSYS This problem has also been solved using the ANSYS command language interface that you may want to browse Open the HTML version copy and paste the code into Notepad or a similar text editor and save it to your computer Now go to File Read input from and select the file A PDF version is also available for printing UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION XSectional Results Advanced XSec Res Data Plotting Graphical Properties Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Changing Graphical Properties Introduction This tutorial was created using ANSYS 70 This tutorial covers some of the methods that can be employed to change how the output to the screen looks For instance changing the background colour numbering the nodes etc Since the purpose of this tutorial is not to build or analysis a model please copy the following code and paste it into the input line below the utility menu finish clear title Changing Graphical Properties prep7 K100 K21000 L12 et1beam3 r110083333310 mpex1200000 mpprxy103 esize5 lmeshall finish solu antype0 dk1allall fk2fy100 solve finish You should obtain the following screen Graphical Options 1 Number the Nodes Utility Menu PlotCtrls Numbering The following window will appear From this window you can select which items you wish to number When you click OK the window will disappear and your model should be numbered appropriately However sometimes the numbers wont show up This could be because you had previously selected a plot of a different item To remedy this problem select the same item you just numbered from the Utility Plot menu and the numbering will show up For instance select the node numbering and plot the nodes You should get the following As shown the nodes have been numbered You can also see some other information that ANSYS is providing The arrows on the left and the right are the force that was applied and the resulting external reactive forces and moments The triangles on the left are the constraints and the coordinate triad is also visible These extra symbols may not be necessary so the next section will show how to turn these symbols off 2 Symbol Toggles Utility Menu PlotCtrls Symbols This window allows the user to toggle many symbols on or off In our case there are no Surface or Body Loads or Initial Conditions so those sections wont be used Under the Boundary conditions section click on None to turn off all the force and reaction symbols The result should be as follows 3 Triad Toggle Utility Menu PlotCtrls Window Controls Window Options This window also allows the user to toggle many things on and off In this case it is things associated with the window background As shown in the window the legend or title can be turned off etc To turn off the triad select Not Shown from the Location of triad drop down menu The following output should be the result Notice how it is much easier to see the node numbers near the origin now 4 Element Shape Utility Menu PlotCtrls Style Size and Shape When using line elements such as BEAM3 it is sometime difficult to visualize what the elements really look like To aid in this process ANSYS can display the elements shapes based on the real constant description Click on the toggle box beside ESHAPE to turn on element shapes and click OK to close the window If there is no change in output dont be alarmed Recall we selected a plot of just the nodes thus elements are not going to show up Select Utility Menu Plot Elements The following should appear As shown the elements are no longer just a line but they have volume according to the real constants To get a better 3D view of the model you can change the view orientation 5 View Orientation Utility Menu PlotCtrls Pan Zoom Rotate This window allows the user to rotate the view translate the view and zoom You can also select predefined views such as isometric or oblique Basic rotating translating and zooming can also be done using the mouse This is very handy when you just want to quickly change the orientation of the model By holding the Control button on the keyboard and holding the Left mouse button the model will translate By holding the Control button on the keyboard and holding the Middle mouse button the model will zoom or rotate on the plane of the screen By holding the Control button on the keyboard and holding the Right mouse button the model will rotate about all axis Using these options its easy to see the elements in 3 D 6 Changing Contours First plot the deformation contour for the beam General Postproc Plot Results Contour Plot Nodal Solution DOF Solution USUM If the contour divisions are not appropriate they can be changed Utility Meny PlotCtrls Style Contours Either Uniform or Nonuniform Contours can be selected Under uniform contours be sure to click on User specified if you are inputing your own contour divisions Under nonuniform contours you can create a logarithmic contour division or some similiar contour where uniform divisions dont capture the information you desire If you dont like the colours of the contour those can also be changed Utility Menu PlotCtrls Style Colours Contour Colours The colours for each division can be selected from the drop down menus 7 Changing Background Colour Perhaps you desire to use a plot for a presentation but dont want a black background Utility Menu PlotCtrls Style Colours Window Colours Select the background colour you desire for the window you desire Here we are only using Window 1 and well set the background colour to white The resulting display is shown below Notice how all the text disappeared This is because the text colour is also white If there is information that needs to be added such as contour values this can be done in other graphic editors To save the display select Utility Menu PlotCtrls Capture Image Under the File heading select Save As There are lots of other option that can be used to change the presentation of data in ANSYS these are just a few If you are looking for a specific option the PlotCtrls menu is a good place to start as is the help file UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Command File Creation and Execution Generating the Command File There are two choices to generate the command file 1 Directly type in the commands into a text file from scratch This assumes a good knowledge of the ANSYS command language and the associated options If you know what some of the commands and are unsure of others execute the desired operation from the GUI and then go to File List Log File This will then open up a new window showing the command line equivialent of all commands entered to this point You may directly cut and paste from here to a text editor or if youd like to save the whole file see the next item in this list 2 Setup and solve the problem as you normally would using the ANSYS graphic user interface GUI Then before you are finished enter the command File Save DB Log File This saves the equivalent ANSYS commands that you entered in the GUI mode to a text file You can now edit this file with a text editor to clean it up delete errors from your GUI use and make changes as desired Running the Command File To run the ANSYS command file G save the ASCII text commands in a text file eg framecmd G start up either the GUI or text mode of ANSYS GUI Command File Loading To run this command file from the GUI you would do the following G From the File menu select Read Input from Change to the appropriate directory where the file framecmd is stored and select it G Now ANSYS will execute the commands from that file The output window shows the progress of this procedure Any errors and warnings will be listed in this window G When it is complete you may not have a full view of your structure in the graphic window You may need to select Plot Elements or Plot Lines or what have you G Assuming that the analysis worked properly you can now use the postprocessor to view element deflections stress etc G If you want to fix some errors or make some changes to the command file make those changes in a separate window in a text editor Save those changes to disk G To rerun the command file you should first of all clear the current model from ANSYS Select File Clear Start New G Then read in the file as before File Read Input from Command Line File Loading Alternatively you can also read in the command file right from the ANSYS command line Assuming that you started ANSYS using the commands ansys52binansysu52 and then entered showx11c This has now started ANSYS in the text mode and has told it what graphic device to use in this case an X Windows X11c mode At this point you could type in menuon but you might not want to turn on the full graphic mode if working on a slow machine or if you are executing the program remotely Lets assume that we dont turn the menu mode on If the command file is in the current directory for ANSYS then from the ANSYS input window type inputframecmd and yes that is a comma between frame and cmd If ANSYS can not find the file in the current directory you may need to point it to the proper directory If the file was in the directory myfilesansysframe for example you would use the following syntax inputframecmdmyfilesansysframe If you want to rerun a new or modified file it is necessary to clear the current model in memory with the command clearstart This full procedure of loading in command files and clearing jobs and starting over again can be completed as many times as desired ANSYS Command Groupings ANSYS contains hundreds of commands for generating geometry applying loads and constraints setting up different analysis types and postprocessing The following is only a brief summary of some of the more common commands used for structural analysis Category Command Description Syntax Basic Geometry k keypoint definition kkpxcoordycoordzcoord l straight line creation lkp1kp2 larc circular arc line from keypoints larckp1kp2kp3rad kp3 defines plane circle circular line creation creates keypoints see online help spline spline line through keypoints splinekp1kp2 kp6 a area definition from keypoints akp1kp2 kp18 al area definition from lines al1l2 l10 v volume definition from keypoints vkp1kp2 kp8 va volume definition from areas vaa1a2 a10 vext create volume from area extrusion see online help vdrag create volume by dragging area along path see online help Solid Modeling Primitives rectng rectangle creation rectngx1x2y1y2 block block volume creation blockx1x2y1y2z1z2 cylind cylindrical volume creation cylindrad1rad2z1z2theta1theta2 sphere spherical volume creation sphererad1rad2theta1theta2 prism cone torus various volume creation commands see online help Boolean Operations aadd adds separate areas to create single area aadda1a2 a9 aglue creates new areas by glueing properties remain separate agluea1a2 a9 asba creat new area by area substraction asbaa1a2 aina create new area by area intersection ainaa1a2 a9 vadd vlgue vsbv vinv volume boolean operations see online help Elements Meshing et defines element type etnumbertype may define as many as required current type is set by type type set current element type pointer typenumber r define real constants for elements rnumberr1r2 r6 may define as many as required current type is set by real real sets current real constant pointer realnumber mp sets material properties for elements mplabelnumberc0c1 c4 may define as many as required current type is set by mat mat sets current material property pointer matnumber esize sets size or number of divisions on lines esizesizendivs use either size or ndivs eshape controls element shape see online help lmesh mesh lines lmeshline1line2inc or lmeshall amesh mesh areas amesharea1area2inc or ameshall vmesh mesh volumes vmeshvol1vol2inc or vmeshall Sets Selection ksel select a subset of keypoints see online help nsel select a subset of nodes see online help lsel select a subjset of lines see online help asel select a subset of areas see online help nsla select nodes within selected areas see online help allsel select everything ie reset selection allsel Constraints dk defines a DOF constraint on a keypoint dkkplabelvalue labels UXUYUZROTXROTYROTZALL d defines a DOF constraint on a node dnodelabelvalue labels UXUYUZROTXROTYROTZALL dl defines antisymmetry DOF constraints on a line dllinearealabel labels SYMM symmetry ASYM antisymmetry Loads fk defines a fkkplabelvalue labels FXFYFZMXMYMZ f defines a force at a node fnodelabelvalue labels FXFYFZMXMYMZ UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta ANSYS Command File Programming Features The following ANSYS command listing shows some of the commonly used programming features in the ANSYS command file language known as ADPL ANSYS Parametric Design Language It illustrates G entering parameters variables G prompting the user for parameters G performing calculations with paramaters note that the syntax and functions are similar to FORTRAN G control structures H if then else endif H looping This example file does not do anything really useful in itself besides generate keypoints along a line but it does illustrate some of the programming features of the ANSYS command language PREP7 preprocessor phase x1 5 define some parameters x2 10 askndivsEnter number of divisions default 55 the above command prompts the user for input to be entered into the variable ndivs if only is entered a default of 5 is used IFndivsGT1THEN if ndivs is greater than 1 dx x2x1ndivs DOi1ndivs11 do i 1 ndivs 1 in steps of one x x1 dxi1 kix00 ENDDO ELSE k1x100 k2x200 ENDIF pnumkp1 turn keypoint numbering on kplot plot keypoints klistallcoord list all keypoints with coordinates UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Command Line Tutorials Basic Tutorials The following documents contain the command line code for the Basic Tutorials ANSYS 70 was used to create all of these tutorials Two Dimensional Truss Basic functions will be shown to provide you with a general knowledge of command line codes Bicycle Space Frame Intermediate ANSYS functions will be shown in detail to provide you with a more general understanding of how to use ANSYS Plane Stress Bracket Boolean operations plane stress and uniform pressure loading will be introduced in the creation and analysis of this 2Dimensional object Solid Modeling This tutorial will introduce techniques such as filleting extrusion copying and working plane orienation to create 3Dimensional objects UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Command Line Tutorials Intermediate Tutorials The following documents contain the command line code for the Intermediate Tutorials ANSYS 70 was used to create all of these tutorials Effect of Self Weight Incorporating the weight of an object into the finite element analysis is shown in this simple cantilever beam example Distributed Loading The application of distributed loads and the use of element tables to extract data is expalined in this tutorial NonLinear Analysis A large moment is applied to the end of a cantilever beam to explore Geometric Nonlinear behaviour large deformations Buckling In this tutorial both the Eigenvalue and Nonlinear methods are used to solve a simple buckling problem NonLinear Materials The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model Dynamic Analysis Modal This tutorial will explore the modal analyis capabilities of ANSYS Dynamic Analysis Harmonic This tutorial will explore the harmonic analyis capabilities of ANSYS Dynamic Analysis Transient This tutorial will explore the transient analyis capabilities of ANSYS Thermal Examples Pure Conduction Analysis of a pure conduction boundary condition example Thermal Examples Mixed ConvectionConduction Insulated Analysis of a Mixed ConvectionConduction Insulated boundary condition example Thermal Examples Transient Heat Conduction Analysis of heat conduction over time Modelling Using Axisymmetry Utilizing axisymmetry to model a 3D structure in 2D to reduce computational time UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Command Line Tutorials Advanced Tutorials The following documents contain the command line code for the Advanced Tutorials ANSYS 70 was used to create all of these tutorials Springs and Joints The creation of models with multiple elements types will be explored in this tutorial Additionally elements COMBIN7 and COMBIN14 will be explained as well as the use of parameters to store data Design Opimization The use of Design Optimization in ANSYS is used to solve for unknown parameters of a beam Substructuring The use of Substructuring in ANSYS is used to solve a simple problem Coupled StructuralThermal Analysis The use of ANSYS physics environments to solve a simple structural thermal problem Using PElements The stress distribution of a model is solved using pelements and compared to helements Melting Using Element Death Using element death to model a volume melting Contact Elements Model of two beams coming into contact with each other ANSYS Parametric Design Language Design a truss using parametric variables UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Command Line Tutorials Postproc Tutorials The following documents contain the command line code for the Postproc Tutorials ANSYS 70 was used to create all of these tutorials Viewing Cross Sectional Results The method to view cross sectional results for a volume are shown in this tutorial Advanced XSectional Results Using Paths to Post Process Results The purpose of this tutorial is to create and use paths to provide extra detail during post processing Data Plotting Using Tables to Post Process Results The purpose of this tutorial is to outline the steps required to plot results using tables a special type of array UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Radiation Example Problem Description Radiation heat transfer between concentric cylinders will be modeled in this example This is a general version of one of the verification examples converted to metric units ANSYS Command Listing PREP7 TITLE RADIATION HEAT TRANSFER BETWEEN CONCENTRIC CYLINDERS ANTYPESTATIC this is a general version of VM125 converted to metric rin200254 inches to metres rout800254 ndiv20 arc360 emis107 emis205 T1700 degrees C T2400 offset273 to convert to degrees K stefbolt5699108 metric version k100 center of tube 1 k500 center of retort k6001 k71 k8001 circle1rin67arcndiv inner cylinder generated clockwise CIRCLE5rout87arcndiv outer cylinder generated counterclockwise ET1LINK321 HEAT CONDUCTING BAR SUPPRESS SOLUTION OUTPUT R11 UNIT CROSSSECTIONAL AREA ARBITRARY MPKXX11 CONDUCTIVITY of inner cylinder arbitrary MAT1 ESIZE1 csys1 cylindrical coord system lselslocxrin LMESHALL lselall MPKXX21 CONDUCTIVITY of outer cylinder arbitrary MAT2 lselslocxrout LMESHall lselall csys0 reset to rect coord system FINISH AUX12 EMIS1emis1 EMIS2emis2 VTYPE0 HIDDEN PROCEDURE FOR VIEW FACTORS GEOM1 GEOMETRY SPECIFICATION 2D STEFstefbolt StefanBoltzmann constant WRITEVM125 WRITE RADIATION MATRIX TO FILE VM125SUB FINISH PREP7 DOFTEMP ET2MATRIX5011 SUPERELEMENT RADIATION MATRIX TYPE2 SEVM125 defines superelement and where its written to TOFFSToffset TEMPERATURE OFFSET FOR ABSOLUTE SCALE csys1 nselslocxrout SELECT OUTER CYLINDER NODES DALLTEMPT1 T1 273 700 DEG K nselall nselslocxrin SELECT INNER CYLINDER NODES DALLTEMPT2 T2 273 400 DEG K nselall csys0 FINISH SOLU SOLVE FINISH POST1 csys1 nselslocxrin SELECT INNER CYLINDER NODES com COM heat flow from inner to outer com PRRSOL PRINT HEAT FLOW FROM INNER TO OUTER CYLINDER nselall nselslocxrout select outer cylinder nodes com COM heat flow from outer to inner com PRRSOL PRINT HEAT FLOW FROM OUTER TO INNER CYLINDER FSUMHEAT only from selected nodes nselall GETQFSUM0ITEMHEAT DIMLABELCHAR12 DIMVALUE13 LABEL11 QWm the 1 below is for unit length numerstefbolt2pirin1offsetT14offsetT24 exactnumer1emis1rinrout1emis21 VFILLVALUE11DATAexact VFILLVALUE12DATAQ VFILLVALUE13DATAABSQexact COM COM VM125 RESULTS COMPARISON COM COM TARGET ANSYS RATIO COM VWRITELABEL11VALUE11VALUE12VALUE13 1XA8 F101 F101 1F53 COM COM FINISH UNIX Applications Editors The are several editors available on the system The first three mentioned below are text based while the remaining have a graphical user interface vi emacs The vi and emacs editors are very powerful but have a steep learning curve You will probably require a tutorialreference book to help you get started with either of these editors The bookstore and CNS carry such manuals These editors have the advantage that most every UNIX system that youll come across will have them so they are always available pico A very simple editor that is sufficient for most work is pico It is the same editor that is used in the Pine mail package that you may have tried out with your Unix GPU account To use pico to edit the file testdat for example one simply types pico testdat at the UNIX prompt In pico the commonly used editing commands are listed at the bottom of its screen The character represents the control Crtl key Some commonly used commands are Ctrl x save and exit Ctrl o save dont exit Ctrl r read an external file into the present file Ctrl 6 mark text press this key then use the cursor keys to mark text Ctrl k cut text to a buffer or just delete it Ctrl u uncut text puts the contents of the buffer at the cursor location Note that the mouse and the delete and insert keys do not have any effect in pico but the backspace key does work normally nedit nedit is a very simple to use yet powerful X Windows editor It features pulldown menus multiple file editing undo and block delimiting with the mouse Very nice check it out Windows Editors Two other editors are available by starting up the Microsoft Windows emulator From a UNIX command window type wabi or win NotePad The first of these editors is called notepad and it is available in the Windows Accessories folder It uses a very small font and is only useful for editing small text files PFE Another option is a powerful text editor called Programmers File Editor It is located in usr localwinappspfe directory and it is called pfeexe look under the r drive Create an icon for this program by using the New menu item in the Program Manager This editor features undo and allows you to edit multiple text files of any size and save them in a DOS or UNIX format Note that UNIX and DOS have different conventions for storing carriage returns in text files Files must be saved in a UNIX format if they are to be used by compilers and Matlab Therefore when saving files in PFE ensure that the UNIX option is selected select Save As from the File menu and look at the option in the dialog box The appendix describes several customizations that you may want to consider for the PFE editor This editor is available as freeware for Windows on the winsite also know as CICA archive see FTP so that you can obtain a copy for your computer at home Problems with File Names Note that Windows editors cannot access files which do not comply to the 83 file format used by DOS For this reason it is not possible to use the Windows editors to directly edit some UNIX files An easy workaround is to rename the file to a DOSlegal name It could then be edited saved and then renamed back to its original name Applications ANSYS ANSYS is a general purpose finite element modeling package for numerically solving a wide variety of mechanical problems These problems include staticdynamic structural analysis both linear and nonlinear heat transfer and fluid problems as well as acoustic and electromagnetic problems ANSYS can be run as a text mode program the default startup mode or as a true XWindows application The text mode is useful for people who wish to simply submit batch command files to perform an analysis or if they wish to work on projects at home over a modem To start ANSYS two methods are avialable 1 Type xansys52 at the UNIX prompt and a small launcher menu will appear Select the Run Interactive Now menu item Some scrolling of text will go by and then stop Press Enter to continue A multiwindowed environment now appears from which to enter your commands If the text used in ANSYS is a little too small for your taste it can be changed in the little start up launcher menu that first appeared From this menu it is necessary to select the Interactive item Then choose GUI configuration From the next dialog box that appears select your desired font size 2 An alternate method to start ANSYS is to type ansys at the UNIX prompt Some scrolling text will go by and then stop Press Enter to continue Once this is done you may enter ANSYS commands To start the XWindows portion of the program issue the following two commands at the ANSYS prompt showx11c menuon A multiwindowed environment now appears from which to enter your commands ANSYS can create rather large files when running and saving therefore it is advisable to start up ANSYS in the scratch directory and then savedelete the appropriate files when you are done You many want to check out some detailed online ANSYS tutorials If youve got some time check out the ANSYS Web page For further information on using ANSYS see Dr Fyfe ProEngineer ProEngineer is a parametric 3D solid modeling and drafting software tool Tutorials for Release 20 are available in the bookstore A companion program ProMechanica performs finite element analysis including static analysis sensitivity studies and design optimization ProMechanica can be run integrated with ProE or in standalone mode If youve got some time check out the Parametric Technology Corporation Web page For more information about this program see Dr Toogood Rampant Rampant is a general purpose inviscid laminar and turbulent flow modeling package To see a detailed enlargement of the ribbon flow on the car click on the car figure If youve got some time and want to see some more beautiful pictures like that shown above check out the Fluent Web page For further information on this program see Dr Yokota FORTRAN The FORTRAN compiler is invoked by typing xlf options filenamef Normally no options are required For learning about the compilers many options type the command xlf by itself If your program code consists of many files and libraries consider using a make file to simplify the programs maintenance Note that the name of the FORTRAN program must have an extension of lower case f ie your file must be named something like testf and not testfor or TESTF If you compile a program using the syntax xlf testf the name of the resulting executable will default to aout logical isnt it This program would be run by entering aout To change the executables output name to test for example we would compile the program in the following way xlf o test testf To run this program you now type test Note that the preceding the name of the executable can be omitted if the current directory is in your path this is changed in your cshrc file see Configuration Files It is possible and usually desirable to have source code in multiple files For example you might have a main program and several subroutine files These can be compiled and linked in onestep by xlf o main mainf sub1f sub2f sub3f Sending compiler error messages to a file If you want to send the compiler output such as error messages to a file you can do it by appending errorfile to the xlf command line For example xlf mainf sub1f errorfile will compile mainf and sub1f and send any compiler output to the file errorfile Capturing program output To send output from a program to a file instead of the screen i e redirecting it execute the program as follows test output where test is the name of the executable and output is the name of the file to which the output will be sent If the program normally prompts the user for input the prompt will not appear on the screen because it too is being sent to the output file The keyboard will still accept the input however So if you know when to enter data and what data to enter you can still run your program this way MATLAB Matlab is a general purpose programming and analysis package with a wealth of builtin numerical symbolic and plotting functions You will normally want to start Matlab from the X Windows screen to take advantage of the graphical environment Matlab is started from a terminal window by entering matlab When started Matlab displays its startup logo and the usual Matlab prompt appears Matlab commands may then be issued from this prompt Normally you will want to be editing and running Matlab m files The most convenient method to do this is to open up a second window see X Windows and run a text editor from this window In this way you will have one window to edit your m files and the second window to run them from Matlab Be sure to save any edited files to disk before trying to run them from Matlab as Matlab only has the copy on disk available to it Note that it is only necessary to save the file and not actually exit the editor In that way it is quick to toggle back and forth between the Matlab and editor windows Note that the text m files created on under DOSWindows and UNIX environments have different formats and will cause errors in Matlab if you try to run them in the other environment unless you make the necessary conversions when copying them tofrom your floppy disk see Floppy Disks It is often necessary to save text output from a Matlab session for documentation purposes This is accomplished by means of the diary command From the Matlab prompt type diary filename where filename is the name of the file where Matlab will echo all keyboard commands and all ensuing text output from the program Note that only the output from those commands that you issue after the diary command will be written to this file After you are finished writing all that you want to this file turn off the diary function with the diary off command The resulting text file may then be edited printed and even imported into a word processor To obtain a PostScript printer file of a currently displayed graph in Matlab you simply type print dps filename where the switch dps specifies device PostScript and filename is the name of the file that the PostScript printing commands will be written to See the section on Printing regarding how one prints PostScript files A great source of Matlab information and useful programs m files can be found by checking out the Mathworks Web page Remote Access You may gain access to this lab from other computers on campus or even at home by starting up a telnet session or via a remote login to connect to one of the labs workstations The workstations are named mec01labs through to mec30labs Depending from where you are trying to access these computers you may need to enter the full address of these workstations which has the form mecxxlabsualbertaca where xx is any workstation number from 01 to 30 For example if you were in another lab on campus with telnet capabilities such as the labs in Cameron and CAB you could access workstation mec08 by entering the command telnet mec08labs You may also need to access another mecxx workstation from within the MecE 33 lab for such purposes as printing and resetting a hung workstation The rlogin command is useful for this purpose For example you may login onto workstation 18 from any other workstation in the lab by issuing the command rlogin mec18 Avoid rlogins and telnets into mec12 unless you are having a PostScript file printed Once the job is completed logout immediately as there are only 2 remote logins open to that workstation Also avoid rlogins to mec24 as it is a major file server for the network Note that if you are going to be remotely running an X Windows application you must have an X server running on your local machine If you have logged in remotely from another X Windows machine you simply need enter the xhost hostname command to set this up However if you have logged in from a PC or MAC from another place on campus or at home you will need to acquire and run an X server program One such program is available from CNS and is called Micro XWin it is available in GSB room 240 for 20 It is a Windows based program and its emulation speed is good when running locally on the fast network backbone on campus but is very slow when running it over a modem The other thing that you must do when running an X Windows application remotely is to tell the remote workstation where the X output is to be sent This is specified with the following command setenv DISPLAY location0 where location is your current workstation name hostname or your local IP address In this command note the upper case DISPLAY and the trailing 0 zero EMail and the Internet Having a GPU account means that you can send and receive EMail If your CNS login id is jblow for example then your Email address is jblowgpusrvualbertaca The mecxxlabs machines do not have an email program on them but GPU does To use Email then it is necessary to rlogin or telnet to GPU You can enter the mail program called pine either through lynx or by typing pine at the prompt Pine is based on the pico editor and is easy to use and fairly self explanatory For more information on using some of the services offered by the internet see FTP newsgroups and WWW Printing Printing is not performed by directly sending printing commands from a particular application You must first create ASCII text files or PostScript files and then use one of the procedures listed below Black White Printing Text Files It is possible to print pure text files ASCII free of charge to the printers located in the small room just outside the main part of the computing lab To do this type lpr filename where filename is the name of the text file to print This file is printed in the small room just outside the main part of the lab with an accompanying banner page with your username on it Do not send PostScript printer files to this printer Uptodate printing instructions are found in the file usrlocaldocprintertxt PostScript files PostScript files are files in a special language that only certain printers can understand Many applications such as ANSYS and Matlab have the capability to save pictures as PostScript files The laser printer in the little room outside Mec 33 is a PostScript printer To use it telnet or rlogin to mec12 and type lprps filename where filename is the name of a PostScript file Within one minute you must insert your copycard a library PhotoCard in the machine beside the printer If you fail to do so your job but not your file will be deleted Prints are 020 per page To print from Windows applications in Wabi you must print to a PostScript file and print it using this procedure see Wabi Printing Large PostScript Files note that very large PostScript files will probably not print on this printer due to the large transfer times required to copy the file to the printer If you have problems with this you will have to print the file elsewhere One option is to consider the possibilities listed in the section below on color printing Color PostScript Printing Many applications can output color PostScript files to display results There are two facilities on campus for printing these files both require encapsulated PostScript files or eps files CNS Versatec Color Plotter this facility permits output plot sizes from 8 12 X 11 to 33 X 44 for a very reasonable price From a GPU account login issue the command plotpostscript filenameeps scale c where filenameeps is the name of the PostScript eps file and scale is a scaling factor from 1 to 4 a factor of 1 is for an 8 12 X 11 page and 4 is for a 33 X 44 poster The c indicates the plot is to be made in color The plots are picked up and paid for in the General Services Building room 240 Education PostScript Color Printer To use this service you must use FTP to copy your eps file to the IP address 12912885145 see FTP It is then necessary to call extension 5433 on campus and tell them what file to print the number of copies and whether or not you want the printout on paper or overhead transparencies The output is picked up and paid for in the basement of the Education Building Instructional Resource Center room B111 For further information see table of contents getting started or appendices Two Dimensional Truss Introduction This tutorial was created using ANSYS 70 to solve a simple 2D Truss problem This is the first of four introductory ANSYS tutorials Problem Description Determine the nodal deflections reaction forces and stress for the truss system shown below Note that Youngs Modulus E is 200GPa while the crass sectional area A is 3250mm2 for all of the elements Modified from Chandrupatla Belegunda Introduction to Finite Elements in Engineering p123 ANSYS Command Listing ANSYS command file to perform 2D Truss Tutorial Chandrupatla p123 title Bridge Truss Tutorial PREP7 preprocessor phase define parameters mm height 3118 width 3600 define keypoints K1 0 0 keypoint x y K2 width2height K3 width 0 K4 3width2 height K5 2width 0 K6 5width2 height K7 3width 0 define lines L12 line connecting kpoint 1 and 2 L13 L23 L24 L34 L35 L45 L46 L56 L57 L67 element definition ET1LINK1 element type 1 spring element R13250 real constant 1 Xsect area 3200 mm2 MPEX1200e3 material property 1 Youngs modulus 200 GPa LESIZEALL 111 specify divisions on unmeshed lines LMESHall mesh all lines FINISH finish preprocessor SOLU enter solution phase apply some constraints DK1ALL0 define a DOF constraint at a keypoint DK7UY0 apply loads FK1FY280e3 define a force load to a keypoint FK3FY210e3 FK5FY280e3 FK7FY360e3 SOLVE solve the resulting system of equations FINISH finish solution POST1 PRRSOLF List Reaction Forces PLDISP2 Plot Deformed shape PLNSOLUSUM01 Contour Plot of deflection ETABLESAXLLS 1 Axial Stress PRETABSAXL List Element Table PLETABSAXLNOAV Plot Axial Stress Two Dimensional Truss Introduction This tutorial was created using ANSYS 70 to solve a simple 2D Truss problem This is the first of four introductory ANSYS tutorials Problem Description Determine the nodal deflections reaction forces and stress for the truss system shown below Note that Youngs Modulus E is 200GPa while the crass sectional area A is 3250mm2 for all of the elements Modified from Chandrupatla Belegunda Introduction to Finite Elements in Engineering p123 ANSYS Command Listing ANSYS command file to perform 2D Truss Tutorial Chandrupatla p123 title Bridge Truss Tutorial PREP7 preprocessor phase define parameters mm height 3118 width 3600 define keypoints K1 0 0 keypoint x y K2 width2height K3 width 0 K4 3width2 height K5 2width 0 K6 5width2 height K7 3width 0 define lines L12 line connecting kpoint 1 and 2 L13 L23 L24 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTTrussTrusshtml Copyright 2001 University of Alberta L34 L35 L45 L46 L56 L57 L67 element definition ET1LINK1 element type 1 spring element R13250 real constant 1 Xsect area 3200 mm2 MPEX1200e3 material property 1 Youngs modulus 200 GPa LESIZEALL 111 specify divisions on unmeshed lines LMESHall mesh all lines FINISH finish preprocessor SOLU enter solution phase apply some constraints DK1ALL0 define a DOF constraint at a keypoint DK7UY0 apply loads FK1FY280e3 define a force load to a keypoint FK3FY210e3 FK5FY280e3 FK7FY360e3 SOLVE solve the resulting system of equations FINISH finish solution POST1 PRRSOLF List Reaction Forces PLDISP2 Plot Deformed shape PLNSOLUSUM01 Contour Plot of deflection ETABLESAXLLS 1 Axial Stress PRETABSAXL List Element Table PLETABSAXLNOAV Plot Axial Stress University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTTrussTrusshtml Copyright 2001 University of Alberta 3D Space Frame Example Problem Description The problem to be modeled in this example is a simple bicycle frame shown in the following figure The frame is to be built of hollow aluminum tubing having an outside diameter of 25mm and a wall thickness of 2mm for the main part of the frame For the rear forks the tubing will be 12mm outside diameter and 1mm wall thickness ANSYS Command Listing Command File mode of 3D Bicycle Space Frame title3D Bicycle Space Frame prep7 Enter the preprocessor Define Some Parameters x1 500 These parameters are not required ie one could x2 825 directly enter in the coordinates into the keypoint y1 325 definition below y2 400 However using parameters makes it very easy to z1 50 quickly make changes to your model Define Keypoints K1 0y1 0 kkeypoint numberxcoordycoordzcoord K2 0y2 0 K3x1y2 0 K4x1 0 0 K5x2 0 z1 K6x2 0z1 Define Lines Linking Keypoints L12 lkeypoint1keypoint2 L23 L34 L41 L46 L45 L35 these last two line are for the rear forks L36 Define Element Type ET1pipe16 KEYOPT161 Define Real Constants Note the inside diameter must be positive R1252 rreal set numberoutside diameterwall thickness R2121 second set of real constants for rear forks Define Material Properties MPEX170000 mpYoungs modulusmaterial numbervalue MPPRXY1033 mpPoissons ratiomaterial numbervalue Define the number of elements each line is to be divided into LESIZEALL20 lesizeline numberall linessize of element Line Meshing REAL1 turn on real property set 1 LMESH161 mesh those lines which have that property set mesh lines 1 through 6 in steps of 1 REAL2 activate real property set 2 LMESH78 mesh the rear forks FINISH Finish preprocessing SOLU Enter the solution processor ANTYPE0 Analysis typestatic Define Displacement Constraints on Keypoints dk command DK1UX0UYUZ dkkeypointdirectiondisplacementdirectiondirection DK5UY0UZ DK6UY0UZ Define Forces on Keypoints fk command FK3FY600 fkkeypointdirectionforce FK4FY200 SOLVE Solve the problem FINISH Finish the solution processor SAVE Save your work to the database post1 Enter the general post processor WINDALLOFF WIND1LTOP WIND2RTOP WIND3LBOT WIND4RBOT GPLOT GCMD1 PLDISP2 Plot the deformed and undeformed edge GCMD2 PLNSOLUSUM01 Set up Element Table information Element tables are tables of information regarding the solution data You must tell Ansys what pieces of information you want by using the etable command etablearbitrary nameitem namedata code number The arbitrary name is a name that you give the data in the table It serves as a reference name to retrieve the data later Use a name that describes the data and is easily remembered The item name and data code number come off of the tables provided Examples For the VonMises or equivalent stresses at angle 0 at both ends of the element node i and node j etablevonmi0nmisc5 etablevonmj0nmisc45 For the Axial stresses at angle 0 etableaxii0ls1 etableaxij0ls33 For the Direct axial stress component due to axial load no bending Note it is independent of angular location etabledirismisc13 etabledirjsmisc15 ADD OTHERS THAT YOU NEED IN HERE To plot the data simply type plls name for node i name for node j for example GCMD3 PLLSvonmi0vonmj0 GCMD4 PLLSaxii0axij0 CONT290027 CONT39018 CONT491818 FOCALL03400001 replot PRNSOLDOF 3D Space Frame Example Problem Description The problem to be modeled in this example is a simple bicycle frame shown in the following figure The frame is to be built of hollow aluminum tubing having an outside diameter of 25mm and a wall thickness of 2mm for the main part of the frame For the rear forks the tubing will be 12mm outside diameter and 1mm wall thickness ANSYS Command Listing Command File mode of 3D Bicycle Space Frame title3D Bicycle Space Frame prep7 Enter the preprocessor Define Some Parameters x1 500 These parameters are not required ie one could x2 825 directly enter in the coordinates into the keypoint y1 325 definition below y2 400 However using parameters makes it very easy to z1 50 quickly make changes to your model Define Keypoints K1 0y1 0 kkeypoint numberxcoordycoordzcoord K2 0y2 0 K3x1y2 0 K4x1 0 0 K5x2 0 z1 K6x2 0z1 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBikePrinthtml Copyright 2001 University of Alberta Define Lines Linking Keypoints L12 lkeypoint1keypoint2 L23 L34 L41 L46 L45 L35 these last two line are for the rear forks L36 Define Element Type ET1pipe16 KEYOPT161 Define Real Constants Note the inside diameter must be positive R1252 rreal set numberoutside diameterwall thickness R2121 second set of real constants for rear forks Define Material Properties MPEX170000 mpYoungs modulusmaterial numbervalue MPPRXY1033 mpPoissons ratiomaterial numbervalue Define the number of elements each line is to be divided into LESIZEALL20 lesizeline numberall linessize of element Line Meshing REAL1 turn on real property set 1 LMESH161 mesh those lines which have that property set mesh lines 1 through 6 in steps of 1 REAL2 activate real property set 2 LMESH78 mesh the rear forks FINISH Finish preprocessing SOLU Enter the solution processor ANTYPE0 Analysis typestatic Define Displacement Constraints on Keypoints dk command DK1UX0UYUZ dkkeypointdirectiondisplacementdirectiondirection DK5UY0UZ DK6UY0UZ Define Forces on Keypoints fk command FK3FY600 fkkeypointdirectionforce FK4FY200 SOLVE Solve the problem FINISH Finish the solution processor SAVE Save your work to the database University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBikePrinthtml Copyright 2001 University of Alberta post1 Enter the general post processor WINDALLOFF WIND1LTOP WIND2RTOP WIND3LBOT WIND4RBOT GPLOT GCMD1 PLDISP2 Plot the deformed and undeformed edge GCMD2 PLNSOLUSUM01 Set up Element Table information Element tables are tables of information regarding the solution data You must tell Ansys what pieces of information you want by using the etable command etablearbitrary nameitem namedata code number The arbitrary name is a name that you give the data in the table It serves as a reference name to retrieve the data later Use a name that describes the data and is easily remembered The item name and data code number come off of the tables provided Examples For the VonMises or equivalent stresses at angle 0 at both ends of the element node i and node j etablevonmi0nmisc5 etablevonmj0nmisc45 For the Axial stresses at angle 0 etableaxii0ls1 etableaxij0ls33 For the Direct axial stress component due to axial load no bending Note it is independent of angular location etabledirismisc13 etabledirjsmisc15 ADD OTHERS THAT YOU NEED IN HERE To plot the data simply type plls name for node i name for node j for example GCMD3 PLLSvonmi0vonmj0 GCMD4 PLLSaxii0axij0 CONT290027 CONT39018 CONT491818 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBikePrinthtml Copyright 2001 University of Alberta FOCALL03400001 replot PRNSOLDOF University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBikePrinthtml Copyright 2001 University of Alberta Plane Stress Bracket Verification Example The first step is to simplify the problem Whenever you are trying out a new analysis type you need something ie analytical solution or experimental data to compare the results to This way you can be sure that youve gotten the correct analysis type units scale factors etc The simplified version that will be used for this problem is that of a flat rectangular plate with a hole shown in the following figure ANSYS Command Listing Command File mode of 2D Plane Stress Verification title 2D Plane Stress Verification PREP7 Preprocessor BLC400200100 rectangle bottom left corner coords width height CYL41005020 circlecenter coords radius ASBA12 substract area 2 from area 1 ET1PLANE42 element Type plane 42 KEYOPT133 This is the changed option to give the plate a thickness R120 Real Constant Material 1 Plate Thickness MPEX1200000 Material Properties Youngs Modulus Material 1 200000 MPa MPPRXY103 Material Properties Major Poissons Ratio Material 1 03 AESIZEALL5 Element sizes all of the lines 5 mm AMESHALL Mesh the lines FINISH Exit preprocessor SOLU Solution ANTYPE0 The type of analysis static DL4 ALL0 Apply a Displacement to Line 4 to all DOF SFL2PRES1 Apply a Distributed load to Line 2 SOLVE Solve the problem FINISH POST1 PLNSOLSEQV Plane Stress Bracket Verification Example The first step is to simplify the problem Whenever you are trying out a new analysis type you need something ie analytical solution or experimental data to compare the results to This way you can be sure that youve gotten the correct analysis type units scale factors etc The simplified version that will be used for this problem is that of a flat rectangular plate with a hole shown in the following figure ANSYS Command Listing Command File mode of 2D Plane Stress Verification title 2D Plane Stress Verification PREP7 Preprocessor BLC400200100 rectangle bottom left corner coords width height CYL41005020 circlecenter coords radius ASBA12 substract area 2 from area 1 ET1PLANE42 element Type plane 42 KEYOPT133 This is the changed option to give the plate a thickness R120 Real Constant Material 1 Plate Thickness MPEX1200000 Material Properties Youngs Modulus Material 1 200000 MPPRXY103 Material Properties Major Poissons Ratio Material 1 AESIZEALL5 Element sizes all of the lines 5 mm AMESHALL Mesh the lines University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBPVerifPrinthtml Copyright 2001 University of Alberta FINISH Exit preprocessor SOLU Solution ANTYPE0 The type of analysis static DL4 ALL0 Apply a Displacement to Line 4 to all DOF SFL2PRES1 Apply a Distributed load to Line 2 SOLVE Solve the problem FINISH POST1 PLNSOLSEQV University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBPVerifPrinthtml Copyright 2001 University of Alberta Plane Stress Bracket Introduction This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS The plane stress bracket tutorial builds upon techniques covered in the first tutorial 3D Bicycle Space Frame it is therefore essential that you have completed that tutorial prior to beginning this one The 2D Plane Stress Bracket will introduce boolean operations plane stress and uniform pressure loading Problem Description The problem to be modeled in this example is a simple bracket shown in the following figure This bracket is to be built from a 20 mm thick steel plate A figure of the plate is shown below This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right ANSYS Command Listing Command File mode of 2D Plane Stress Bracket title 2D Plane Stress Bracket prep7 Enter the preprocessor Create Geometry BLC40080100 CYL4805050 CYL402020 CYL408020 BLC420202060 AADDALL Boolean Addition add all of the areas together CYL4805030 Create Bolt Holes CYL402010 CYL408010 ASBA6ALL Boolean Subtraction subtracts all areas other than 6 from base area 6 Define Element Type ET1PLANE82 KEYOPT133 Plane stress element with thickness Define Real Constants Note the inside diameter must be positive R120 rreal set number plate thickness Define Material Properties MPEX1200000 mpYoungs modulusmaterial numbervalue MPPRXY103 mpPoissons ratiomaterial numbervalue Define the number of elements each line is to be divided into AESIZEALL5 lesizeall areassize of element Area Meshing AMESHALL amesh all areas FINISH Finish preprocessing SOLU Enter the solution processor ANTYPE0 Analysis typestatic Define Displacement Constraints on Lines dl command DL 7 ALL0 There is probably a way to do these all at once DL 8 ALL0 DL 9 ALL0 DL10 ALL0 DL11 ALL0 DL12 ALL0 DL13 ALL0 DL14 ALL0 Define Forces on Keypoints fk command FK9FY1000 fkkeypointdirectionforce SOLVE Solve the problem FINISH Finish the solution processor SAVE Save your work to the database post1 Enter the general post processor WINDALLOFF WIND1LTOP WIND2RTOP WIND3LBOT WIND4RBOT GPLOT GCMD1 PLDISP2 Plot the deformed and undeformed edge GCMD2 PLNSOLUSUM01 Plot the deflection USUM GCMD3 PLNSOLSEQV01 Plot the equivalent stress GCMD4 PLNSOLEPTOEQV01 Plot the equivalent strain CONT210000036 Set contour ranges CONT31008 CONT4100005e3 FOCALL03400001 Focus point replot PRNSOLDOF Prints the nodal solutions Plane Stress Bracket Introduction This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS The plane stress bracket tutorial builds upon techniques covered in the first tutorial 3D Bicycle Space Frame it is therefore essential that you have completed that tutorial prior to beginning this one The 2D Plane Stress Bracket will introduce boolean operations plane stress and uniform pressure loading Problem Description The problem to be modeled in this example is a simple bracket shown in the following figure This bracket is to be built from a 20 mm thick steel plate A figure of the plate is shown below This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right ANSYS Command Listing Command File mode of 2D Plane Stress Bracket title 2D Plane Stress Bracket prep7 Enter the preprocessor Create Geometry BLC40080100 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBracketPrinthtml Copyright 2001 University of Alberta CYL4805050 CYL402020 CYL408020 BLC420202060 AADDALL Boolean Addition add all of the areas together CYL4805030 Create Bolt Holes CYL402010 CYL408010 ASBA6ALL Boolean Subtraction subtracts all areas other than 6 from ba Define Element Type ET1PLANE82 KEYOPT133 Plane stress element with thickness Define Real Constants Note the inside diameter must be positive R120 rreal set number plate thickness Define Material Properties MPEX1200000 mpYoungs modulusmaterial numbervalue MPPRXY103 mpPoissons ratiomaterial numbervalue Define the number of elements each line is to be divided into AESIZEALL5 lesizeall areassize of element Area Meshing AMESHALL amesh all areas FINISH Finish preprocessing SOLU Enter the solution processor ANTYPE0 Analysis typestatic Define Displacement Constraints on Lines dl command DL 7 ALL0 There is probably a way to do these all at once DL 8 ALL0 DL 9 ALL0 DL10 ALL0 DL11 ALL0 DL12 ALL0 DL13 ALL0 DL14 ALL0 Define Forces on Keypoints fk command FK9FY1000 fkkeypointdirectionforce University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBracketPrinthtml Copyright 2001 University of Alberta SOLVE Solve the problem FINISH Finish the solution processor SAVE Save your work to the database post1 Enter the general post processor WINDALLOFF WIND1LTOP WIND2RTOP WIND3LBOT WIND4RBOT GPLOT GCMD1 PLDISP2 Plot the deformed and undeformed edge GCMD2 PLNSOLUSUM01 Plot the deflection USUM GCMD3 PLNSOLSEQV01 Plot the equivalent stress GCMD4 PLNSOLEPTOEQV01 Plot the equivalent strain CONT210000036 Set contour ranges CONT31008 CONT4100005e3 FOCALL03400001 Focus point replot PRNSOLDOF Prints the nodal solutions University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTBracketPrinthtml Copyright 2001 University of Alberta Solid Model Creation Introduction This tutorial is the last of three basic tutorials devised to illustrate commom features in ANSYS Each tutorial builds upon techniques covered in previous tutorials it is therefore essential that you complete the tutorials in order The Solid Modelling Tutorial will introduce various techniques which can be used in ANSYS to create solid models Filleting extrusionsweeping copying and working plane orientation will be covered in detail Two Solid Models will be created within this tutorial We will create a solid model of the pulley shown in the following figure We will also create a solid model of the Spindle Base shown in the following figure ANSYS Command Listing Pulley Model PREP7 BLC420155 Create rectangles BLC43251 BLC480055 AADDALL Add the areas together CYL435505 Create circles CYL4850202 ASBA41 Subtract an area AGEN2246 Mirrors an area AGEN2105 AADDALL Adds all areas LFILLT22701 Create a fillet radius of 01mm between lines 30 and 7 LFILLT26701 AL369 Creates fillet area arbitrary area using lines 91011 AL101114 AADDALL Sweep K1001000 Keypoints K1002050 VROTAT3 10011002360 Sweep area 4 about axis formed by keypoints 1001 and 1002 K2001030 K2002130 K2003031 KWPLAN1200120022003 Align WorkPlane with keypoints CSYS5 Change Active CS to Global Cartesian Y CYL455005 1 Create circle VGEN85 45 0 Pattern the circle every 45 degrees Subtract areas vsbvall5 vsbv136 vsbvall7 vsbv48 vsbvall9 vsbv210 vsbvall11 vsbv212 Spindle Base Model PREP7 BLC400109102 Create rectangle K52082 Keypoints K62020 K7082 K8020 LARC45720 Line arcs LARC16820 L56 AL4567 Creates area from 4 lines AADD12 Now called area 3 CYL402010 Area 1 AGEN21 69 Mirrors area 1 AGEN212 62 Mirrors again ASBA3ALL Subtracts areas VOFFST626 Creates volume from area K1001091020 Keypoints K10110920 K102159102sqrt3002 KWPLAN1100101102 Defines working plane BLC400102180 Create rectangle CYL45118051 Create circle AADD2526 Add them together VOFFST2726 Volume from area VADD12 Add volumes AADD333438 Add areas AADD323637 CYL45118032 60 Create cylinder VADD13 Add volumes CYL451180185 60 Another cylinder VSBV21 Subtract it WPCSYS10 This realigns the WP with the global coordinate system K200206126 Keypoints K20106126 K202206130 KWPLAN1200201202 Shift working plane CSYS4 Change active coordinate system K2031290577352600 Keypoints K204 12905773526 38 sqrt32760 A200203204 Create area from keypoints VOFFST720 Volume from area VADD ALL Add it together Solid Model Creation Introduction This tutorial is the last of three basic tutorials devised to illustrate commom features in ANSYS Each tutorial builds upon techniques covered in previous tutorials it is therefore essential that you complete the tutorials in order The Solid Modelling Tutorial will introduce various techniques which can be used in ANSYS to create solid models Filleting extrusionsweeping copying and working plane orientation will be covered in detail Two Solid Models will be created within this tutorial We will create a solid model of the pulley shown in the following figure We will also create a solid model of the Spindle Base shown in the following figure University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTSolidPrinthtml Copyright 2001 University of Alberta ANSYS Command Listing Pulley Model PREP7 BLC420155 Create rectangles BLC43251 BLC480055 AADDALL Add the areas together CYL435505 Create circles CYL4850202 ASBA41 Subtract an area AGEN2246 Mirrors an area AGEN2105 AADDALL Adds all areas LFILLT22701 Create a fillet radius of 01mm between lines 30 LFILLT26701 AL369 Creates fillet area arbitrary area using lines AL101114 AADDALL Sweep K1001000 Keypoints K1002050 VROTAT3 10011002360 Sweep area 4 about axis formed by keypoints 1001 K2001030 K2002130 K2003031 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTSolidPrinthtml Copyright 2001 University of Alberta KWPLAN1200120022003 Align WorkPlane with keypoints CSYS5 Change Active CS to Global Cartesian Y CYL455005 1 Create circle VGEN85 45 0 Pattern the circle every 45 degrees Subtract areas vsbvall5 vsbv136 vsbvall7 vsbv48 vsbvall9 vsbv210 vsbvall11 vsbv212 Spindle Base Model PREP7 BLC400109102 Create rectangle K52082 Keypoints K62020 K7082 K8020 LARC45720 Line arcs LARC16820 L56 AL4567 Creates area from 4 lines AADD12 Now called area 3 CYL402010 Area 1 AGEN21 69 Mirrors area 1 AGEN212 62 Mirrors again ASBA3ALL Subtracts areas VOFFST626 Creates volume from area K1001091020 Keypoints K10110920 K102159102sqrt3002 KWPLAN1100101102 Defines working plane BLC400102180 Create rectangle CYL45118051 Create circle AADD2526 Add them together VOFFST2726 Volume from area VADD12 Add volumes AADD333438 Add areas AADD323637 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTSolidPrinthtml Copyright 2001 University of Alberta CYL45118032 60 Create cylinder VADD13 Add volumes CYL451180185 60 Another cylinder VSBV21 Subtract it WPCSYS10 This realigns the WP with the global coordinate system K200206126 Keypoints K20106126 K202206130 KWPLAN1200201202 Shift working plane CSYS4 Change active coordinate system K2031290577352600 Keypoints K204 12905773526 38 sqrt32760 A200203204 Create area from keypoints VOFFST720 Volume from area VADD ALL Add it together University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCBTSolidPrinthtml Copyright 2001 University of Alberta Effect of Self Weight on a Cantilever Beam Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the required steps to account for the weight of an object in ANSYS Loads will not be applied to the beam shown below in order to observe the deflection caused by the weight of the beam itself The beam is to be made of steel with a modulus of elasticity of 200 GPa ANSYS Command Listing Title Effects of Self Weight PREP7 Length 1000 Width 50 Height 10 K100 Create Keypoints K2Length0 L12 ET1BEAM3 Set element type R1WidthHeightWidthHeight312Height exponent MPEX1200000 Youngs Modulus MPPRXY103 Poissons ratio MPDENS1786e6 Density LESIZEALLLength10 Size of line elements LMESH1 Mesh line 1 FINISH SOLU Enter solution mode ANTYPE0 Static analysis DK1ALL0 Constrain keypoint 1 ACEL98 Set gravity constant SOLVE FINISH POST1 PLDISP2 Display deformed shape Effect of Self Weight on a Cantilever Beam Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the required steps to account for the weight of an object in ANSYS Loads will not be applied to the beam shown below in order to observe the deflection caused by the weight of the beam itself The beam is to be made of steel with a modulus of elasticity of 200 GPa ANSYS Command Listing Title Effects of Self Weight PREP7 Length 1000 Width 50 Height 10 K100 Create Keypoints K2Length0 L12 ET1BEAM3 Set element type R1WidthHeightWidthHeight312Height exponent MPEX1200000 Youngs Modulus MPPRXY103 Poissons ratio MPDENS1786e6 Density LESIZEALLLength10 Size of line elements LMESH1 Mesh line 1 FINISH SOLU Enter solution mode ANTYPE0 Static analysis University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITDensityPrinthtml Copyright 2001 University of Alberta DK1ALL0 Constrain keypoint 1 ACEL98 Set gravity constant SOLVE FINISH POST1 PLDISP2 Display deformed shape University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITDensityPrinthtml Copyright 2001 University of Alberta Application of Distributed Loads Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data Please note that this material was also covered in the Bicycle Space Frame tutorial under Basic Tutorials A distributed load of 1000 Nm 1 Nmm will be applied to a solid steel beam with a rectangular cross section as shown in the figure below The crosssection of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa ANSYS Command Listing title Distributed Loading of a Beam PREP7 K100 Define the keypoints K210000 L12 Create the line ET1BEAM3 Beam3 element type R110083333310 Real constants areaIheight MPEX1200000 Youngs Modulus MPPRXY1033 Poissons ratio ESIZE100 Mesh size LMESHALL Mesh line FINISH SOLU ANTYPE0 Static analysis DK1UX0UY Pin keypoint 1 DK2UY0 Roller on keypoint 2 SFBEAMALL1PRES1 Apply distributed load SOLVE FINISH POST1 PLDISP2 Plot deformed shape ETABLESMAXINMISC 1 Create data for element table ETABLESMAXJNMISC 3 PLLSSMAXISMAXJ10 Plot ETABLE data Application of Distributed Loads Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data Please note that this material was also covered in the Bicycle Space Frame tutorial under Basic Tutorials A distributed load of 1000 Nm 1 Nmm will be applied to a solid steel beam with a rectangular cross section as shown in the figure below The crosssection of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa ANSYS Command Listing title Distributed Loading of a Beam PREP7 K100 Define the keypoints K210000 L12 Create the line ET1BEAM3 Beam3 element type University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITDistributedPrintht Copyright 2001 University of Alberta R110083333310 Real constants areaIheight MPEX1200000 Youngs Modulus MPPRXY1033 Poissons ratio ESIZE100 Mesh size LMESHALL Mesh line FINISH SOLU ANTYPE0 Static analysis DK1UX0UY Pin keypoint 1 DK2UY0 Roller on keypoint 2 SFBEAMALL1PRES1 Apply distributed load SOLVE FINISH POST1 PLDISP2 Plot deformed shape ETABLESMAXINMISC 1 Create data for element table ETABLESMAXJNMISC 3 PLLSSMAXISMAXJ10 Plot ETABLE data University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITDistributedPrintht Copyright 2001 University of Alberta UofA ANSYS Tutorial ANSYS UTILITIES BASIC TUTORIALS INTERMEDIATE TUTORIALS ADVANCED TUTORIALS POSTPROC TUTORIALS COMMAND LINE FILES PRINTABLE VERSION Creating Files Features Basic Tutorials Intermediate Tutorials Advanced Tutorials PostProc Tutorials Radiation Index Contributions Comments MecE 563 Mechanical Engineering University of Alberta ANSYS Inc Copyright 2001 University of Alberta Contact Element Example The ANSYS contact element CONTACT48 allows friction to be modelled as a normal force only or as a normal force and a shear force In this model there are two blocks one above top of the other with a small separation The top block is cantilevered while the bottom block is tied to ground The top block experiences a load and comes into contact with the lower block This command file is also useful to demonstate the use of sets or selections to group nodeskeypoints or to select a single nodekeypoint to which boundary conditions will be applied titleSample of CONTACT48 element type prep7 RECTNG01002 define rectangular areas RECTNG257524 aplot define element type ET1plane4232 element type 1 plane stress wthick nodal strs out type1 activate element type 1 R 1 001 thickness 001 define material properties MPEX 1 200e3 Youngs modulus MPNUXY1 03 Poissons ratio MPEX 2 20e3 Youngs modulus 10 times less rigid MPNUXY2 03 Poissons ratio meshing esize05 set meshing size mat1 turn on material set 1 real1 real set 1 amesh1 mesh area 1 esize035 mat2 amesh2 pnummat1 turn on material color shading eplot ET2contac481 defines second element type 2D contact elements keyo271 r220e3000510 TYPE2 activates or sets this element type real2 define contact nodes and elements first the contact nodes aselsarea2 select top area nslas1 select the nodes within this area nselrlocy199201 select bottom layer of nodes in this area cmsourcenode call this group of nodes source then the target nodes allsel relect everything aselsarea1 select bottom area nslas1 select nodes in this area nselrlocy199201 the top layer of nodes from this area cmtargetnode call this selection target gcgensourcetarget3 generate contact elements between defined nodes finish solution antypestatnew Ground upper left hand corner of top block kselslocx25 kselrlocy4 dkallall0 Ground bottom nodes on bottom block allsel nselslocy0 when vmin vmax 0 here a small tolerance is used dallall0 Give top right corner a vertical load allsel kselslocx75 kselrlocy4 fkallfy100 allsel time1 nsubst20100 autotson auto time stepping predon predictor on nroptfullon NewtonRaphson on solve finish NonLinear Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam shown below There are several causes for nonlinear behaviour such as Changing Status Material Nonlinearities and Geometric Nonlinearities change in response due to large deformations This tutorial will deal specifically with Geometric Nonlinearities To solve this problem the load will added incrementally After each increment the stiffness matrix will be adjusted before increasing the load The solution will be compared to the equivalent solution using a linear response ANSYS Command Listing prep7 start preprocessor titleNonLinear Analysis of Cantilever Beam k1000 define keypoints k2500 5 beam length l12 define line et1beam3 Beam r10031254069e50125 area izz height of beam mpex1300e6 Youngs Modulus mpprxy103 Poissons ratio esize01 element size of 01 lmeshall mesh the line finish stop preprocessor solu start solution phase antypestatic static analysis nlgeomon turn on nonlinear geometry analysis autotson auto time stepping nsubst510001 Size of first substep15 of the total load max substeps1000 min substeps1 outresallall save results of all iterations dk1all constrain all DOF on ground fk2mz100 applied moment solve post1 pldisp1 display deformed mesh PRNSOLUX lists horizontal deflections NonLinear Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam shown below There are several causes for nonlinear behaviour such as Changing Status Material Nonlinearities and Geometric Nonlinearities change in response due to large deformations This tutorial will deal specifically with Geometric Nonlinearities To solve this problem the load will added incrementally After each increment the stiffness matrix will be adjusted before increasing the load The solution will be compared to the equivalent solution using a linear response ANSYS Command Listing prep7 start preprocessor titleNonLinear Analysis of Cantilever Beam k1000 define keypoints k2500 5 beam length l12 define line et1beam3 Beam r10031254069e50125 area izz height of beam mpex1300e6 Youngs Modulus mpprxy103 Poissons ratio esize01 element size of 01 lmeshall mesh the line finish stop preprocessor University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITNonLinearPrinthtml Copyright 2001 University of Alberta solu start solution phase antypestatic static analysis nlgeomon turn on nonlinear geometry analysis autotson auto time stepping nsubst510001 Size of first substep15 of the total load max substeps10 outresallall save results of all iterations dk1all constrain all DOF on ground fk2mz100 applied moment solve post1 pldisp1 display deformed mesh PRNSOLUX lists horizontal deflections University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITNonLinearPrinthtml Copyright 2001 University of Alberta Buckling Introduction This tutorial was created using ANSYS 70 to solve a simple buckling problem It is recommended that you complete the NonLinear Tutorial prior to beginning this tutorial Buckling loads are critical loads where certain types of structures become unstable Each load has an associated buckled mode shape this is the shape that the structure assumes in a buckled condition There are two primary means to perform a buckling analysis 1 Eigenvalue Eigenvalue buckling analysis predicts the theoretical buckling strength of an ideal elastic structure It computes the structural eigenvalues for the given system loading and constraints This is known as classical Euler buckling analysis Buckling loads for several configurations are readily available from tabulated solutions However in real life structural imperfections and nonlinearities prevent most realworld structures from reaching their eigenvalue predicted buckling strength ie it overpredicts the expected buckling loads This method is not recommended for accurate realworld buckling prediction analysis 2 Nonlinear Nonlinear buckling analysis is more accurate than eigenvalue analysis because it employs nonlinear large deflection static analysis to predict buckling loads Its mode of operation is very simple it gradually increases the applied load until a load level is found whereby the structure becomes unstable ie suddenly a very small increase in the load will cause very large deflections The true nonlinear nature of this analysis thus permits the modeling of geometric imperfections load perterbations material nonlinearities and gaps For this type of analysis note that small offaxis loads are necessary to initiate the desired buckling mode This tutorial will use a steel beam with a 10 mm X 10 mm cross section rigidly constrained at the bottom The required load to cause buckling applied at the topcenter of the beam will be calculated ANSYS Command Listing Eigenvalue Buckling FINISH These two commands clear current data CLEAR TITLEEigenvalue Buckling Analysis PREP7 Enter the preprocessor ET1BEAM3 Define the element of the beam to be buckled R110083333310 Real Consts type 1 area mm2 I mm4 height mm MPEX1200000 Youngs modulus in MPa MPPRXY103 Poissons ratio K100 Define the geometry of beam 100 mm high K20100 L12 Draw the line ESIZE10 Set element size to 1 mm LMESHALLALL Mesh the line FINISH SOLU Enter the solution mode ANTYPESTATIC Before you can do a buckling analysis ANSYS needs the info from a static analysis PSTRESON Prestress can be accounted for required during buckling analysis DK1ALL Constrain the bottom of beam FK2FY1 Load the top vertically with a unit load This is done so the eigenvalue calculated will be the actual buckling load since all loads are scaled during the analysis SOLVE FINISH SOLU Enter the solution mode again to solve buckling ANTYPEBUCKLE Buckling analysis BUCOPTLANB1 Buckling options subspace one mode SOLVE FINISH SOLU Reenter solution mode to expand info necessary EXPASSON An expantion pass will be performed MXPAND1 Specifies the number of modes to expand SOLVE FINISH POST1 Enter postprocessor SETLIST List eigenvalue solution TimeFreq listing is the force required for buckling in N for this case SETLAST Read in data for the desired mode PLDISP Plots the deflected shape NonLinear Buckling FINISH These two commands clear current data CLEAR TITLE Nonlinear Buckling Analysis PREP7 Enter the preprocessor ET1BEAM3 Define element as beam3 MPEX1200000 Youngs modulus in Pa MPPRXY103 Poissons ratio R110083333310 area I height K1000 Lower node K201000 Upper node 100 mm high L12 Draws line ESIZE1 Sets element size to 1 mm LMESHALL Mesh line FINISH SOLU ANTYPESTATIC Static analysis not buckling NLGEOMON Nonlinear geometry solution supported OUTRESALLALL Stores bunches of output NSUBST20 Load broken into 5 load steps NEQIT1000 Use 20 load steps to find solution AUTOTSON Auto time stepping LNSRCHON ESHAPE1 Plots the beam as a volume rather than line DK1ALL0 Constrain bottom FK2FY50000 Apply load slightly greater than predicted required buckling load to upper node FK2FX250 Add a horizontal load 05 FY to initiate buckling SOLVE FINISH POST26 Time history post processor RFORCE21FY Reads force data in variable 2 NSOL32UY Reads ydeflection data into var 3 XVAR2 Make variable 2 the xaxis PLVAR3 Plots variable 3 on yaxis AXLABYDEFLECTION Changes y label AXLABXLOAD Changes X label REPLOT Buckling Introduction This tutorial was created using ANSYS 70 to solve a simple buckling problem It is recommended that you complete the NonLinear Tutorial prior to beginning this tutorial Buckling loads are critical loads where certain types of structures become unstable Each load has an associated buckled mode shape this is the shape that the structure assumes in a buckled condition There are two primary means to perform a buckling analysis 1 Eigenvalue Eigenvalue buckling analysis predicts the theoretical buckling strength of an ideal elastic structure It computes the structural eigenvalues for the given system loading and constraints This is known as classical Euler buckling analysis Buckling loads for several configurations are readily available from tabulated solutions However in reallife structural imperfections and nonlinearities prevent most real world structures from reaching their eigenvalue predicted buckling strength ie it overpredicts the expected buckling loads This method is not recommended for accurate realworld buckling prediction analysis 2 Nonlinear Nonlinear buckling analysis is more accurate than eigenvalue analysis because it employs nonlinear largedeflection static analysis to predict buckling loads Its mode of operation is very simple it gradually increases the applied load until a load level is found whereby the structure becomes unstable ie suddenly a very small increase in the load will cause very large deflections The true nonlinear nature of this analysis thus permits the modeling of geometric imperfections load perterbations material nonlinearities and gaps For this type of analysis note that small offaxis loads are necessary to initiate the desired buckling mode University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITBucklingPrinthtml Copyright 2002 University of Alberta This tutorial will use a steel beam with a 10 mm X 10 mm cross section rigidly constrained at the bottom The required load to cause buckling applied at the topcenter of the beam will be calculated ANSYS Command Listing Eigenvalue Buckling FINISH These two commands clear current data CLEAR TITLEEigenvalue Buckling Analysis PREP7 Enter the preprocessor ET1BEAM3 Define the element of the beam to be buckled R110083333310 Real Consts type 1 area mm2 I mm4 height mm MPEX1200000 Youngs modulus in MPa MPPRXY103 Poissons ratio K100 Define the geometry of beam 100 mm high K20100 L12 Draw the line ESIZE10 Set element size to 1 mm LMESHALLALL Mesh the line FINISH SOLU Enter the solution mode University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITBucklingPrinthtml Copyright 2002 University of Alberta ANTYPESTATIC Before you can do a buckling analysis ANSYS needs the info from a static analysis PSTRESON Prestress can be accounted for required during buckling analysis DK1ALL Constrain the bottom of beam FK2FY1 Load the top vertically with a unit load This is done so the eigenvalue calculated will be the actual buckling load since all loads are scaled during the analysis SOLVE FINISH SOLU Enter the solution mode again to solve buckling ANTYPEBUCKLE Buckling analysis BUCOPTLANB1 Buckling options subspace one mode SOLVE FINISH SOLU Reenter solution mode to expand info necessary EXPASSON An expantion pass will be performed MXPAND1 Specifies the number of modes to expand SOLVE FINISH POST1 Enter postprocessor SETLIST List eigenvalue solution TimeFreq listing is the force required for buckling in N for this case SETLAST Read in data for the desired mode PLDISP Plots the deflected shape NonLinear Buckling FINISH These two commands clear current data CLEAR TITLE Nonlinear Buckling Analysis PREP7 Enter the preprocessor ET1BEAM3 Define element as beam3 MPEX1200000 Youngs modulus in Pa MPPRXY103 Poissons ratio R110083333310 area I height K1000 Lower node K201000 Upper node 100 mm high L12 Draws line ESIZE1 Sets element size to 1 mm LMESHALL Mesh line FINISH SOLU ANTYPESTATIC Static analysis not buckling NLGEOMON Nonlinear geometry solution supported OUTRESALLALL Stores bunches of output University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITBucklingPrinthtml Copyright 2002 University of Alberta NSUBST20 Load broken into 5 load steps NEQIT1000 Use 20 load steps to find solution AUTOTSON Auto time stepping LNSRCHON ESHAPE1 Plots the beam as a volume rather than line DK1ALL0 Constrain bottom FK2FY50000 Apply load slightly greater than predicted required buckling load to upper node FK2FX250 Add a horizontal load 05 FY to initiate buckling SOLVE FINISH POST26 Time history post processor RFORCE21FY Reads force data in variable 2 NSOL32UY Reads ydeflection data into var 3 XVAR2 Make variable 2 the xaxis PLVAR3 Plots variable 3 on yaxis AXLABYDEFLECTION Changes y label AXLABXLOAD Changes X label REPLOT University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITBucklingPrinthtml Copyright 2002 University of Alberta NonLinear Materials Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model For instance the case when a large force is applied resulting in a stresses greater than yield strength In such a case a multilinear stressstrain relationship can be included which follows the stressstrain curve of the material being used This will allow ANSYS to more accurately model the plastic deformation of the material For this analysis a simple tension speciment 100 mm X 5 mm X 5 mm is constrained at the bottom and has a load pulling on the top This specimen is made out of a experimental substance called WhoKilledKenium The stressstrain curve for the substance is shown above Note the linear section up to approximately 225 MPa where the Youngs Modulus is constant 75 GPa The material then begins to yield and the relationship becomes plastic and nonlinear ANSYS Command Listing finish clear prep7 Enter Preprocessor k100 Keypoints k20100 l12 Line connecting keypoints ET1LINK1 Element type R125 Area of 25 MPEX175000 Youngs modulus MPPRXY103 Poissons ratio TBMELA1112 Create a table of 12 data points to map the stressstrain curve TBPT00175 Data points TBPT002150 TBPT003225 TBPT004240 TBPT005250 TBPT025300 TBPT06355 TBPT1390 TBPT15420 TBPT2435 TBPT25449 TBPT275450 ESIZE5 Element size 5 LMESHall Line mesh all lines FINISH SOLU Enter solution phase NLGEOMON Nonlinear geometry on NSUBST2010001 20 load steps OUTRESALLALL Output data for all load steps AUTOTSON Auto timesearch on LNSRCHON Line search on NEQIT1000 1000 iteration maximum ANTYPE0 Static analysis DK1all Constrain keypoint 1 FK2FY10000 Load on keypoint 2 SOLVE FINISH POST1 Enter post processor ESHAPE1 Show element shape PLNSOLUY01 Plot deflection contour FINISH POST26 Enter time history RFORCE21FY Reads force data in variable 2 NSOL32UY Reads ydeflection data into var 3 XVAR2 Make variable 2 the xaxis PLVAR3 AXLABYDEFLECTION Changes y label AXLABXLOAD Changes X label REPLOT NonLinear Materials Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model For instance the case when a large force is applied resulting in a stresses greater than yield strength In such a case a multilinear stressstrain relationship can be included which follows the stressstrain curve of the material being used This will allow ANSYS to more accurately model the plastic deformation of the material For this analysis a simple tension speciment 100 mm X 5 mm X 5 mm is constrained at the bottom and has a load pulling on the top This specimen is made out of a experimental substance called WhoKilledKenium The stressstrain curve for the substance is shown above Note the linear section up to approximately 225 MPa where the Youngs Modulus is constant 75 GPa The material then begins to yield and the relationship becomes plastic and nonlinear ANSYS Command Listing finish clear prep7 Enter Preprocessor k100 Keypoints k20100 l12 Line connecting keypoints ET1LINK1 Element type R125 Area of 25 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITNonLinearMatPrin Copyright 2003 University of Alberta MPEX175000 Youngs modulus MPPRXY103 Poissons ratio TBMELA1112 Create a table of 12 data points to map the stressstrain curve TBPT00175 Data points TBPT002150 TBPT003225 TBPT004240 TBPT005250 TBPT025300 TBPT06355 TBPT1390 TBPT15420 TBPT2435 TBPT25449 TBPT275450 ESIZE5 Element size 5 LMESHall Line mesh all lines FINISH SOLU Enter solution phase NLGEOMON Nonlinear geometry on NSUBST2010001 20 load steps OUTRESALLALL Output data for all load steps AUTOTSON Auto timesearch on LNSRCHON Line search on NEQIT1000 1000 iteration maximum ANTYPE0 Static analysis DK1all Constrain keypoint 1 FK2FY10000 Load on keypoint 2 SOLVE FINISH POST1 Enter post processor ESHAPE1 Show element shape PLNSOLUY01 Plot deflection contour FINISH POST26 Enter time history RFORCE21FY Reads force data in variable 2 NSOL32UY Reads ydeflection data into var 3 XVAR2 Make variable 2 the xaxis PLVAR3 AXLABYDEFLECTION Changes y label AXLABXLOAD Changes X label REPLOT University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITNonLinearMatPrin Copyright 2003 University of Alberta Creation of the Cantilver Beam used in the Dynamic Analysis Tutorials This file shows the command line codes necessary to create the following cantilever beam in ANSYS TITLE Dynamic Analysis FILNAMEDynamic0 This sets the jobname to Dynamic PREP7 K100 K210 L12 ET1BEAM3 R100001833e10001 MPEX12068e11 MPPRXY1033 MPDENS17830 LESIZEALL10 LMESH1 FINISH Close this window to return to the Dynamic Analysis Tutorials Creation of the Cantilver Beam used in the Dynamic Analysis Tutorials This file describes the GUI Graphic User Interface steps to create the following cantilever beam in ANSYS 1 Open preprocessor menu 2 Give example a Title Utility Menu File Change Title 3 Give example a Jobname Utility Menu File Change Jobname Enter Dynamic for the jobname 4 Create Keypoints Preprocessor Modeling Create Keypoints In Active CS We are going to define 2 keypoints the beam vertices for this structure as given in the following table Keypoint Coordinates xy 1 00 2 10 5 Define Lines Preprocessor Modeling Create Lines Lines Straight Line Create a line between Keypoint 1 and Keypoint 2 6 Define Element Types Preprocessor Element Type AddEditDelete For this problem we will use the BEAM3 Beam 2D elastic element This element has 3 degrees of freedom translation along the X and Y axiss and rotation about the Z axis With only 3 degrees of freedom the BEAM3 element can only be used in 2D analysis 7 Define Real Constants Preprocessor Real Constants Add In the Real Constants for BEAM3 window enter the following geometric properties i Crosssectional area AREA 00001 ii Area Moment of Inertia IZZ 833e10 iii Total beam height HEIGHT 001 This defines an element with a solid rectangular cross section 001 m x 001 m 8 Define Element Material Properties Preprocessor Material Props Material Models Structural Linear Elastic Isotropic In the window that appears enter the following geometric properties for steel i Youngs modulus EX 2068e11 ii Poissons Ratio PRXY 03 To enter the density of the material double click on Linear followed by Density in the Define Material Model Behavior Window Enter a density of 7830 Note For dynamic analysis both the stiffness and the material density have to be specified 9 Define Mesh Size Preprocessor Meshing Size Cntrls ManualSize Lines All Lines For this example we will specify 10 element divisions along the line 10 Mesh the frame Preprocessor Meshing Mesh Lines click Pick All Close this window to return to the Dynamic Analysis Tutorials Modal Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple modal analysis of the cantilever beam shown below ANSYS Command Listing FINISH CLEAR TITLE Dynamic Analysis PREP7 K100 Enter keypoints K210 L12 Create line ET1BEAM3 Element type R100001833e10001 Real Const areaIheight MPEX12068e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh line FINISH SOLU ANTYPE2 Modal analysis MODOPTSUBSP5 Subspace 5 modes EQSLVFRONT Frontal solver MXPAND5 Expand 5 modes DK1ALL Constrain keypoint one SOLVE FINISH POST1 List solutions SETLIST SETFIRST PLDISP Display first mode shape ANMODE1005 0 Animate mode shape Modal Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to do a simple modal analysis of the cantilever beam shown below ANSYS Command Listing FINISH CLEAR TITLE Dynamic Analysis PREP7 K100 Enter keypoints K210 L12 Create line ET1BEAM3 Element type R100001833e10001 Real Const areaIheight MPEX12068e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh line University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITModalPrinthtml Copyright 2001 University of Alberta FINISH SOLU ANTYPE2 Modal analysis MODOPTSUBSP5 Subspace 5 modes EQSLVFRONT Frontal solver MXPAND5 Expand 5 modes DK1ALL Constrain keypoint one SOLVE FINISH POST1 List solutions SETLIST SETFIRST PLDISP Display first mode shape ANMODE1005 0 Animate mode shape University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITModalPrinthtml Copyright 2001 University of Alberta Harmonic Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to explain the steps required to perform Harmonic analysis the cantilever beam shown below We will now conduct a harmonic forced response test by applying a cyclic load harmonic at the end of the beam The frequency of the load will be varied from 1 100 Hz The figure below depicts the beam with the application of the load ANSYS provides 3 methods for conducting a harmonic analysis These 3 methods are the Full Reduced and Modal Superposition methods This example demonstrates the Full method because it is simple and easy to use as compared to the other two methods However this method makes use of the full stiffness and mass matrices and thus is the slower and costlier option ANSYS Command Listing FINISH CLEAR TITLE Dynamic Analysis PREP7 K100 Enter keypoints K210 L12 Create line ET1BEAM3 Element type R100001833e10001 Real Const areaIheight MPEX12068e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh line FINISH SOLU ANTYPE3 Harmonic analysis DK1ALL Constrain keypoint 1 FK2FY100 Apply force HARFRQ0100 Frequency range NSUBST100 Number of frequency steps KBC1 Stepped loads SOLVE FINISH POST26 NSOL22UY UY2 Get ydeflection data STOREMERGE PRVAR2 Print data PLVAR2 Plot data Harmonic Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to explain the steps required to perform Harmonic analysis the cantilever beam shown below We will now conduct a harmonic forced response test by applying a cyclic load harmonic at the end of the beam The frequency of the load will be varied from 1 100 Hz The figure below depicts the beam with the application of the load ANSYS provides 3 methods for conducting a harmonic analysis These 3 methods are the Full Reduced and Modal Superposition methods University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITHarmonicPrinthtml Copyright 2001 University of Alberta This example demonstrates the Full method because it is simple and easy to use as compared to the other two methods However this method makes use of the full stiffness and mass matrices and thus is the slower and costlier option ANSYS Command Listing FINISH CLEAR TITLE Dynamic Analysis PREP7 K100 Enter keypoints K210 L12 Create line ET1BEAM3 Element type R100001833e10001 Real Const areaIheight MPEX12068e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh line FINISH SOLU ANTYPE3 Harmonic analysis DK1ALL Constrain keypoint 1 FK2FY100 Apply force HARFRQ0100 Frequency range NSUBST100 Number of frequency steps KBC1 Stepped loads SOLVE FINISH POST26 NSOL22UY UY2 Get ydeflection data STOREMERGE PRVAR2 Print data PLVAR2 Plot data University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITHarmonicPrinthtml Copyright 2001 University of Alberta Transient Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to show the steps involved to perform a simple transient analysis Transient dynamic analysis is a technique used to determine the dynamic response of a structure under a time varying load The time frame for this type of analysis is such that inertia or damping effects of the structure are considered to be important Cases where such effects play a major role are under step or impulse loading conditions for example where there is a sharp load change in a fraction of time If inertia effects are negligible for the loading conditions being considered a static analysis may be used instead For our case we will impact the end of the beam with an impulse force and view the response at the location of impact Since an ideal impulse force excites all modes of a structure the response of the beam should contain all mode frequencies However we cannot produce an ideal impulse force numerically We have to apply a load over a discrete amount of time dt After the application of the load we track the response of the beam at discrete time points for as long as we like depending on what it is that we are looking for in the response The size of the time step is governed by the maximum mode frequency of the structure we wish to capture The smaller the time step the higher the mode frequency we will capture The rule of thumb in ANSYS is timestep 1 20f where f is the highest mode frequency we wish to capture In other words we must resolve our step size such that we will have 20 discrete points per period of the highest mode frequency It should be noted that a transient analysis is more involved than a static or harmonic analysis It requires a good understanding of the dynamic behavior of a structure Therefore a modal analysis of the structure should be initially performed to provide information about the structures dynamic behavior In ANSYS transient dynamic analysis can be carried out using 3 methods G The Full Method This is the easiest method to use All types of nonlinearities are allowed It is however very CPU intensive to go this route as full system matrices are used G The Reduced Method This method reduces the system matrices to only consider the Master Degrees of Freedom MDOFs Because of the reduced size of the matrices the calculations are much quicker However this method handles only linear problems such as our cantilever case G The Mode Superposition Method This method requires a preliminary modal analysis as factored mode shapes are summed to calculate the structures response It is the quickest of the three methods but it requires a good deal of understanding of the problem at hand We will use the Reduced Method for conducting our transient analysis Usually one need not go further than Reviewing the Reduced Results However if stresses and forces are of interest than we would have to Expand the Reduced Solution ANSYS Command Listing finish clear TITLE Dynamic Analysis FILNAMEDynamic0 This sets the jobname to Dynamic PREP7 Enter preprocessor K100 Keypoints K210 L12 Connect keypoints with line ET1BEAM3 Element type R100001833e10001 Real constants MPEX12068e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh the line FINISH SOLU Enter solution phase ANTYPE TRANS Transient analysis TRNOPTREDUC reduced solution method DELTIM0001 Specifies the time step sizes At time equals 0s NSELS211 select nodes 2 11 MAllUY Define Master DOFs NSELALL Reselect all nodes D1ALL Constrain left end F2FY100 Load right end At time equals 0001s TIME0001 Sets time to 0001 seconds KBC0 Ramped load step FDELE2ALL Delete the load at the end At time equals 1s TIME1 Sets time to 1 second KBC0 Ramped load step LSSOLVE131 solve multiple load steps FINISH POST26 Enter time history FILEDynamicrdsp Calls the dynamic file NSOL22UY UY2 Calls data for UY deflection at node 2 STOREMERGE Stores the data PLVAR2 Plots vs time Please note if you are using a later version of ANSYS you will probably have to issue the LSWRITE command at the end of each load step for the LSSOLVE command to function properly In this case replace the found in the code with LSWRITE and the problem should be solved Transient Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to show the steps involved to perform a simple transient analysis Transient dynamic analysis is a technique used to determine the dynamic response of a structure under a timevarying load The time frame for this type of analysis is such that inertia or damping effects of the structure are considered to be important Cases where such effects play a major role are under step or impulse loading conditions for example where there is a sharp load change in a fraction of time If inertia effects are negligible for the loading conditions being considered a static analysis may be used instead For our case we will impact the end of the beam with an impulse force and view the response at the location of impact httpwwwmeceualbertacatutorialsansysCLCITTransientPrinthtml Copyright 2003 University of Alberta Since an ideal impulse force excites all modes of a structure the response of the beam should contain all mode frequencies However we cannot produce an ideal impulse force numerically We have to apply a load over a discrete amount of time dt After the application of the load we track the response of the beam at discrete time points for as long as we like depending on what it is that we are looking for in the response The size of the time step is governed by the maximum mode frequency of the structure we wish to capture The smaller the time step the higher the mode frequency we will capture The rule of thumb in ANSYS is timestep 1 20f where f is the highest mode frequency we wish to capture In other words we must resolve our step size such that we will have 20 discrete points per period of the highest mode frequency It should be noted that a transient analysis is more involved than a static or harmonic analysis It requires a good understanding of the dynamic behavior of a structure Therefore a modal analysis of the structure should be initially performed to provide information about the structures dynamic behavior In ANSYS transient dynamic analysis can be carried out using 3 methods httpwwwmeceualbertacatutorialsansysCLCITTransientPrinthtml Copyright 2003 University of Alberta The Full Method This is the easiest method to use All types of nonlinearities are allowed It is however very CPU intensive to go this route as full system matrices are used The Reduced Method This method reduces the system matrices to only consider the Master Degrees of Freedom MDOFs Because of the reduced size of the matrices the calculations are much quicker However this method handles only linear problems such as our cantilever case The Mode Superposition Method This method requires a preliminary modal analysis as factored mode shapes are summed to calculate the structures response It is the quickest of the three methods but it requires a good deal of understanding of the problem at hand We will use the Reduced Method for conducting our transient analysis Usually one need not go further than Reviewing the Reduced Results However if stresses and forces are of interest than we would have to Expand the Reduced Solution ANSYS Command Listing finish clear TITLE Dynamic Analysis FILNAMEDynamic0 This sets the jobname to Dynamic PREP7 Enter preprocessor K100 Keypoints KZ10 Connect keypoints with line L12 Connect keypoints with line ET1BEAM3 Element type R100001833e10001 Real constants MPEX12e68e11 Youngs modulus MPPRXY1033 Poissons ratio MPDENS17830 Density LESIZEALL10 Element size LMESH1 Mesh the line FINISH SOLU Enter solution phase ANTYPE TRANS Transient analysis TRNOPTREDUC reduced solution method DELTIM0001 Specifies the time step sizes At time equals 0s NSELS211 select nodes 2 11 MALLUY Define Master DOFs NSELALL Reselect all nodes D1ALL Constrain left end F2FY100 Load right end At time equals 0001s TIME0001 Sets time to 0001 seconds KBC0 Ramped load step FDELE2ALL Delete the load at the end At time equals 1s TIME1 Sets time to 1 second KBC0 Ramped load step LSSOLVE131 solve multiple load steps FINISH POST26 Enter time history FILEDynamicrdsp Calls the dynamic file NSOL22UY UY2 Calls data for UY deflection at node 2 STOREMERGE Stores the data PLVAR2 Plots vs time Please note if you are using a later version of ANSYS you will probably have to issue the LSWRITE command at the end of each load step for the LSSOLVE command to function properly In this case replace the found in the code with LSWRITE and the problem should be solved httpwwwmeceualbertacatutorialsansysCLCITTransientPrinthtml Copyright 2003 University of Alberta Simple Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple conduction problem The Simple Conduction Example is constrained as shown in the following figure Thermal conductivity k of the material is 10 WmC and the block is assumed to be infinitely long ANSYS Command Listing title Simple Conduction Example PREP7 define geometry length10 height10 blc400length height area one corner then width and height mesh 2D areas ET1 PLANE55 Thermal element only MPKXX110 10 WmC ESIZElength20 number of element subdivisionsside AMESHALL FINISH SOLU ANTYPE0 STEADYSTATE THERMAL ANALYSIS fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500C NSELALL NSELSLOCX0 select nodes on three sides NSELALOCXlength NSELALOCY0 DALLTEMP100 apply fixed temp of 100C NSELALL SOLVE FINISH POST1 PLNSOLTEMP0 contour plot of temperatures Simple Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple conduction problem The Simple Conduction Example is constrained as shown in the following figure Thermal conductivity k of the material is 10 WmC and the block is assumed to be infinitely long ANSYS Command Listing title Simple Conduction Example PREP7 define geometry length10 height10 blc400length height area one corner then width and height mesh 2D areas ET1 PLANE55 Thermal element only MPKXX110 10 WmC ESIZElength20 number of element subdivisionsside AMESHALL University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITConductionPrinth Copyright 2001 University of Alberta FINISH SOLU ANTYPE0 STEADYSTATE THERMAL ANALYSIS fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500C NSELALL NSELSLOCX0 select nodes on three sides NSELALOCXlength NSELALOCY0 DALLTEMP100 apply fixed temp of 100C NSELALL SOLVE FINISH POST1 PLNSOLTEMP0 contour plot of temperatures University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITConductionPrinth Copyright 2001 University of Alberta Thermal Mixed Boundary Example Conduction ConvectionInsulated Introduction This tutorial was created using ANSYS 70 to solve simple thermal examples Analysis of a simple conduction as well a mixed conductionconvectioninsulation problem will be demonstrated The Mixed ConvectionConductionInsulated Boundary Conditions Example is constrained as shown in the following figure Note that the section is assumed to be infinitely long ANSYS Command Listing title Simple Convection Example PREP7 define geometry length10 height10 blc400length height area one corner then width and height mesh 2D areas ET1 PLANE55 Thermal element only MPKXX110 10 WmC MAT1 TYPE1 ESIZElength20 number of element subdivisionsside AMESHALL FINISH SOLU ANTYPE0 STEADYSTATE THERMAL ANALYSIS fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500C NSELALL NSELSLOCX0 select nodes on three sides DALLTEMP100 apply fixed temp of 100C NSELALL convection BCs NSELSLOCXlength right edge SFALLCONV10100 apply fixed temp of 100C NSELALL Insulated BCs NSELSLOCY0 bottom edge SFALLCONV0 insulate edge NSELALL SOLVE FINISH POST1 PLNSOLTEMP0 contour plot of temperatures Thermal Mixed Boundary Example ConductionConvectionInsulated Introduction This tutorial was created using ANSYS 70 to solve simple thermal examples Analysis of a simple conduction as well a mixed conductionconvectioninsulation problem will be demonstrated The Mixed ConvectionConductionInsulated Boundary Conditions Example is constrained as shown in the following figure Note that the section is assumed to be infinitely long ANSYS Command Listing title Simple Convection Example PREP7 define geometry length10 height10 blc400length height area one corner then width and height mesh 2D areas ET1 PLANE55 Thermal element only MPKXX110 10 WmC MAT1 TYPE1 ESIZElength20 number of element subdivisionsside httpwwwmeceualbertacatutorialsansysCLcitconvectionprinthtml Copyright 2003 University of Alberta AMESHALL FINISH SOLU ANTYPE0 STEADYSTATE THERMAL ANALYSIS fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500C NSELALL NSELSLOCX0 select nodes on three sides DALLTEMP100 apply fixed temp of 100C NSELALL convection BCs NSELSLOCXlength right edge SFALLCONV10100 apply fixed temp of 100C NSELALL Insulated BCs NSELSLOCY0 bottom edge SFALLCONV0 insulate edge NSELALL SOLVE FINISH POST1 PLNSOLTEMP0 contour plot of temperatures httpwwwmeceualbertacatutorialsansysCLcitconvectionprinthtml Copyright 2003 University of Alberta Transient Thermal Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple transient conduction problem Special thanks to Jesse Arnold for the analytical solution shown at the end of the tutorial The example is constrained as shown in the following figure Thermal conductivity k of the material is 5 W mK and the block is assumed to be infinitely long Also the density of the material is 920 kgm3 and the specific heat capacity c is 2040 kJkgK It is beneficial if the ThermalConduction tutorial is completed first to compare with this solution ANSYS Command Listing finish clear title Simple Conduction Example PREP7 Enter preprocessor define geometry length10 height10 blc400length height area one corner then width and height mesh 2D areas ET1 PLANE55 Thermal element only MPDens1920 Density mpc12040 Specific heat capacity mpkxx15 Thermal conductivity ESIZE005 Element size AMESHALL Mesh area FINISH SOLU ANTYPE4 Transient analysis time300 Time at end 300 nroptfull Newton Raphson full lumpm0 Lumped mass approx off nsubst20 20 substeps neqit100 Max no of iterations 100 autotsoff Auto time search on lnsrchon Line search on outresallall Output data for all substeps kbc1 fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500K NSELALL NSELsLOCY0 DALLTEMP100 apply fixed temp of 100K NSELALL ICallTemp100 Initial Conditions 100K SOLVE FINISH POST1 Enter postprocessor CONT18100500 Define a contour range PLNSOLTEMP Plot temperature contour ANTIME2005020500 Animate temp over time Transient Thermal Conduction Example Introduction This tutorial was created using ANSYS 70 to solve a simple transient conduction problem Special thanks to Jesse Arnold for the analytical solution shown at the end of the tutorial The example is constrained as shown in the following figure Thermal conductivity k of the material is 5 WmK and the block is assumed to be infinitely long Also the density of the material is 920 kgm3 and the specific heat capacity c is 2040 kJkgK It is beneficial if the ThermalConduction tutorial is completed first to compare with this solution ANSYS Command Listing finish clear title Simple Conduction Example PREP7 Enter preprocessor define geometry length10 height10 blc400length height area one corner then width and height University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITTransCondPrinthtml Copyright 2003 University of Alberta mesh 2D areas ET1 PLANE55 Thermal element only MPDens1920 Density mpc12040 Specific heat capacity mpkxx15 Thermal conductivity ESIZE005 Element size AMESHALL Mesh area FINISH SOLU ANTYPE4 Transient analysis time300 Time at end 300 nroptfull Newton Raphson full lumpm0 Lumped mass approx off nsubst20 20 substeps neqit100 Max no of iterations 100 autotsoff Auto time search on lnsrchon Line search on outresallall Output data for all substeps kbc1 fixed temp BCs NSELSLOCYheight select nodes on top with yheight DALLTEMP500 apply fixed temp of 500K NSELALL NSELsLOCY0 DALLTEMP100 apply fixed temp of 100K NSELALL ICallTemp100 Initial Conditions 100K SOLVE FINISH POST1 Enter postprocessor CONT18100500 Define a contour range PLNSOLTEMP Plot temperature contour ANTIME2005020500 Animate temp over time University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITTransCondPrinthtml Copyright 2003 University of Alberta Modelling Using Axisymmetry Introduction This tutorial was completed using ANSYS 70 This tutorial is intended to outline the steps required to create an axisymmetric model The model will be that of a closed tube made from steel Point loads will be applied at the center of the top and bottom plate to make an analytical verification simple to calculate A 34 cross section view of the tube is shown below As a warning point loads will create discontinuities in the your model near the point of application If you chose to use these types of loads in your own modelling be very careful and be sure to understand the theory of how the FEA package is appling the load and the assumption it is making In this case we will only be concerned about the stress distribution far from the point of application so the discontinuities will have a negligable effect ANSYS Command Listing finish clear title Axisymmetric Tube prep7 triadoff Turns off origin triad marker rectng02005 Create 3 overlapping rectangles rectng15200100 rectng02095100 aaddall Add the areas together et1plane2 Define element type keyopt131 Turns on axisymmetry mpex1200000 Youngs Modulus mpprxy103 Poissons ratio esize2 Mesh size ameshall Mesh the area finish solu antype0 Static analysis lselslocx0 Select the lines at x0 dlallsymm Symmetry constraints lselall Reselect all lines nselslocy50 Node select at y50 dalluy0 Constrain motion in y nselall Reselect all nodes fk1fy100 Apply point loads in center fk12fy100 solve finish post1 nselslocy4555 Select nodes from y45 to y55 prnsolscomp List stresses on those nodes nselall Reselect all nodes expand27axis10 Expand the axisymmetric elements view1123 Change the viewing angle replot Modelling Using Axisymmetry Introduction This tutorial was completed using ANSYS 70 This tutorial is intended to outline the steps required to create an axisymmetric model The model will be that of a closed tube made from steel Point loads will be applied at the center of the top and bottom plate to make an analytical verification simple to calculate A 34 cross section view of the tube is shown below As a warning point loads will create discontinuities in the your model near the point of application If you chose to use these types of loads in your own modelling be very careful and be sure to understand the theory of how the FEA package is appling the load and the assumption it is making In this case we will only be concerned about the stress distribution far from the point of application so the discontinuities will have a negligable effect ANSYS Command Listing finish clear title Axisymmetric Tube University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITAxisymmetricPrint Copyright 2003 University of Alberta prep7 triadoff Turns off origin triad marker rectng02005 Create 3 overlapping rectangles rectng15200100 rectng02095100 aaddall Add the areas together et1plane2 Define element type keyopt131 Turns on axisymmetry mpex1200000 Youngs Modulus mpprxy103 Poissons ratio esize2 Mesh size ameshall Mesh the area finish solu antype0 Static analysis lselslocx0 Select the lines at x0 dlallsymm Symmetry constraints lselall Reselect all lines nselslocy50 Node select at y50 dalluy0 Constrain motion in y nselall Reselect all nodes fk1fy100 Apply point loads in center fk12fy100 solve finish post1 nselslocy4555 Select nodes from y45 to y55 prnsolscomp List stresses on those nodes nselall Reselect all nodes expand27axis10 Expand the axisymmetric elements view1123 Change the viewing angle replot University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCITAxisymmetricPrint Copyright 2003 University of Alberta Application of Joints and Springs in ANSYS Introduction This tutorial was created using ANSYS 571 This tutorial will introduce G the use of multiple elements in ANSYS G elements COMBIN7 Joints and COMBIN14 Springs G obtainingstoring scalar information and store them as parameters A 1000N vertical load will be applied to a catapult as shown in the figure below The catapult is built from steel tubing with an outer diameter of 40 mm a wall thickness of 10 and a modulus of elasticity of 200GPa The springs have a stiffness of 5 Nmm ANSYS Command Listing title Catapult PREP7 ET1PIPE16 Element type 1 ET2COMBIN7 Element type 2 ET3COMBIN14 Element type 3 R14010 Real constants 1 R21e91e91e9 Real constants 2 R35 Real constants 3 MPEX1200000 Youngs modulus Material 1 MPPRXY1033 Poissons ratio Material 1 N 1 0 0 0 Node locations N 2 0 01000 N 31000 01000 N 41000 0 0 N 5 010001000 N 6 01000 0 N 7 700 700 500 N 8 400 400 500 N 9 0 0 0 N10 0 01000 N11 0 0 500 N12 0 01500 N13 0 0500 TYPE1 Turn on Element 1 REAL1 Turn on Real constants 1 MAT1 Turn on Material 1 E 1 6 Element connectivity E 2 5 E 1 4 E 2 3 E 3 4 E10 8 E 9 8 E 7 8 E12 5 E13 6 E1213 E 5 3 E 6 4 TYPE2 Turn on Element 2 REAL2 Turn on Real constants 2 E 1 9 11 Element connectivity E 2 10 11 TYPE3 Turn on Element 3 REAL3 Turn on Real constants 3 E58 Element connectivity E86 PNUMKP0 Number nodes PNUMELEM1 Number elements REPLOT FINISH SOLU Enter solution phase ANTYPE0 Static analysis NLGEOMON Nonlinear geometry on NSUBST5 5 Load steps of equal size D3ALL041213 Constrain nodes 341213 F7FY1000 Load node 7 SOLVE FINISH POST1 PLDISP2 GETVERT7NODE7UY Application of Joints and Springs in ANSYS Introduction This tutorial was created using ANSYS 571 This tutorial will introduce the use of multiple elements in ANSYS elements COMBIN7 Joints and COMBIN14 Springs obtainingstoring scalar information and store them as parameters A 1000N vertical load will be applied to a catapult as shown in the figure below The catapult is built from steel tubing with an outer diameter of 40 mm a wall thickness of 10 and a modulus of elasticity of 200GPa The springs have a stiffness of 5 Nmm ANSYS Command Listing title Catapult PREP7 ET1PIPE16 Element type 1 ET2COMBIN7 Element type 2 ET3COMBIN14 Element type 3 R14010 Real constants 1 R21e91e91e9 Real constants 2 R35 Real constants 3 MPEX1200000 Youngs modulus Material 1 MPPRXY1033 Poissons ratio Material 1 N 1 0 0 0 Node locations N 2 0 01000 N 31000 01000 N 41000 0 0 N 5 010001000 N 6 01000 0 N 7 700 700 500 N 8 400 400 500 N 9 0 0 0 N10 0 01000 N11 0 0 500 N12 0 01500 N13 0 0500 TYPE1 Turn on Element 1 REAL1 Turn on Real constants 1 MAT1 Turn on Material 1 E 1 6 Element connectivity E 2 5 E 1 4 E 2 3 E 3 4 E10 8 E 9 8 E 7 8 E12 5 E13 6 E1213 E 5 3 E 6 4 TYPE2 Turn on Element 2 REAL2 Turn on Real constants 2 E 1 9 11 Element connectivity E 2 10 11 TYPE3 Turn on Element 3 REAL3 Turn on Real constants 3 E58 Element connectivity E86 PNUMKP0 Number nodes PNUMELEM1 Number elements REPLOT FINISH SOLU Enter solution phase ANTYPE0 Static analysis NLGEOMON Nonlinear geometry on University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATJointsPrinthtml Copyright 2001 University of Alberta NSUBST5 5 Load steps of equal size D3ALL041213 Constrain nodes 341213 F7FY1000 Load node 7 SOLVE FINISH POST1 PLDISP2 GETVERT7NODE7UY University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATJointsPrinthtml Copyright 2001 University of Alberta Design Optimization Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to introduce a method of solving design optimization problems using ANSYS This will involve creating the geometry utilizing parameters for all the variables deciding which variables to use as design state and objective variables and setting the correct tolerances for the problem to obtain an accurately converged solution in a minimal amount of time The use of hardpoints to apply forcesconstraints in the middle of lines will also be covered in this tutorial A beam has a force of 1000N applied as shown below The purpose of this optimization problem is to minimize the weight of the beam without exceeding the allowable stress It is necessary to find the cross sectional dimensions of the beam in order to minimize the weight of the beam However the width and height of the beam cannot be smaller than 10mm The maximum stress anywhere in the beam cannot exceed 200 MPa The beam is to be made of steel with a modulus of elasticity of 200 GPa ANSYS Command Listing prep7 title Design Optimization setH20 Set an initial height of 20 mm setW20 Set an initial width of 20 mm K100 Keypoint locations K210000 L12 Create line HPTCREATELINE10RATI75 Create hardpoint 75 from left side ET1BEAM3 Element type R1WHWH312H Real consts areaI note not height MPEX1200000 Youngs modulus MPPRXY103 Poissons ratio ESIZE100 Mesh size LMESHALL Mesh line FINISH SOLU ANTYPE0 Static analysis DK1UX0 Pin keypoint 1 DK1UY0 DK2UY0 Support keypoint 2 FK3FY2000 Force at hardpoint SOLVE FINISH POST1 ETABLEEVolumeVOLU Volume of single element SSUM Sum all volumes GETVolumeSSUMITEMEVOLUME Create parameter Volume for volume of beam ETABLESMAXINMISC1 Create parameter SMaxI for max stress at I node ESORTETABSMAXI01 GETSMAXISORTMAX ETABLESMAXJNMISC3 Create parameter SMaxJ for max stress at J node ESORTETABSMAXJ01 GETSMAXJSORTMAX SETSMAXSMAXISMAXJ Create parameter SMax as max stress LGWRITEoptimizetxtCTEMP Save logfile to CTempoptimizetxt OPT OPANLoptimizetxtCTemp Assign optimizetxt as analysis file OPVARHDV10500001 Height design variable min 10 mm max 50 mm tolerance 0001mm OPVARWDV10500001 Width design variable min 10 mm max 50 mm tolerance 0001mm OPVARSMAXSV1952000001 Height state variable min 195 MPa max 200 MPa tolerance 0001 MPa OPVARVOLUMEOBJ200 Volume as object variable tolerance 200 mm2 OPTYPEFIRS Firstorder analysis OPFRST3010002 Max iteration Percent step size Percent forward difference OPEXE Run optimization PLVAROPTHW Graph optimation data AXLABXNumber of Iterations AXLABYWidth and Height mm REPLOT Design Optimization Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to introduce a method of solving design optimization problems using ANSYS This will involve creating the geometry utilizing parameters for all the variables deciding which variables to use as design state and objective variables and setting the correct tolerances for the problem to obtain an accurately converged solution in a minimal amount of time The use of hardpoints to apply forcesconstraints in the middle of lines will also be covered in this tutorial A beam has a force of 1000N applied as shown below The purpose of this optimization problem is to minimize the weight of the beam without exceeding the allowable stress It is necessary to find the cross sectional dimensions of the beam in order to minimize the weight of the beam However the width and height of the beam cannot be smaller than 10mm The maximum stress anywhere in the beam cannot exceed 200 MPa The beam is to be made of steel with a modulus of elasticity of 200 GPa ANSYS Command Listing prep7 title Design Optimization setH20 Set an initial height of 20 mm setW20 Set an initial width of 20 mm K100 Keypoint locations K210000 L12 Create line HPTCREATELINE10RATI75 Create hardpoint 75 from left side ET1BEAM3 Element type R1WHWH312H Real consts areaI note not height MPEX1200000 Youngs modulus MPPRXY103 Poissons ratio University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATOptimizationPrint Copyright 2001 University of Alberta ESIZE100 Mesh size LMESHALL Mesh line FINISH SOLU ANTYPE0 Static analysis DK1UX0 Pin keypoint 1 DK1UY0 DK2UY0 Support keypoint 2 FK3FY2000 Force at hardpoint SOLVE FINISH POST1 ETABLEEVolumeVOLU Volume of single element SSUM Sum all volumes GETVolumeSSUMITEMEVOLUME Create parameter Volume for volume of beam ETABLESMAXINMISC1 Create parameter SMaxI for max stress at I nod ESORTETABSMAXI01 GETSMAXISORTMAX ETABLESMAXJNMISC3 Create parameter SMaxJ for max stress at J nod ESORTETABSMAXJ01 GETSMAXJSORTMAX SETSMAXSMAXISMAXJ Create parameter SMax as max stress LGWRITEoptimizetxtCTEMP Save logfile to CTempoptimizetxt OPT OPANLoptimizetxtCTemp Assign optimizetxt as analysis file OPVARHDV10500001 Height design variable min 10 mm max 50 mm to OPVARWDV10500001 Width design variable min 10 mm max 50 mm tol OPVARSMAXSV1952000001 Height state variable min 195 MPa max 200 MPa OPVARVOLUMEOBJ200 Volume as object variable tolerance 200 mm2 OPTYPEFIRS Firstorder analysis OPFRST3010002 Max iteration Percent step size Percent forwar OPEXE Run optimization PLVAROPTHW Graph optimation data AXLABXNumber of Iterations AXLABYWidth and Height mm REPLOT University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATOptimizationPrint Copyright 2001 University of Alberta Substructuring Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the how to use substructuring in ANSYS Substructuring is a procedure that condenses a group of finite elements into one superelement This reduces the required computation time and also allows the solution of very large problems A simple example will be demonstrated to explain the steps required however please note that this model is not one which requires the use of substructuring The example involves a block of wood E 10 GPa v 029 connected to a block of silicone E 25 MPa v 041 which is rigidly attached to the ground A force will be applied to the structure as shown in the following figure For this example substructuring will be used for the wood block The use of substructuring in ANSYS is a three stage process 1 Generation Pass Generate the superelement by condensing several elements together Select the degrees of freedom to save master DOFs and to discard slave DOFs Apply loads to the superelement 2 Use Pass Create the full model including the superelement created in the generation pass Apply remaining loads to the model The solution will consist of the reduced solution tor the superelement and the complete solution for the nonsuperelements 3 Expansion Pass Expand the reduced solution to obtain the solution at all DOFs for the superelement Note that a this method is a bottomup substructuring each superelement is created separately and then assembled in the Use Pass Topdown substructuring is also possible in ANSYS the entire model is built then superelement are created by selecting the appropriate elements This method is suitable for smaller models and has the advantage that the results for multiple superelements can be assembled in postprocessing ANSYS Command Listing BottomUp Substructuring GENERATION PASS Build the superelement portion of the model FINISH CLEAR START FILNAMEGEN Change jobname PREP7 Create Geometry blc4040100100 Creates rectangle Define material properties of wood section ET1PLANE42 Element type MPEX1 10000 Youngs Modulus MPPRXY1029 Poissons ratio meshing AESIZE110 Element size amesh1 Mesh area FINISH SOLU ANTYPESUBST SUBSTRUCTURE GENERATION PASS SEOPTGEN2 Name GEN and no printed output NSELSEXT Select all external nodes MALLALL Make all selected nodes master DOFs NSELALL Reselect all nodes NSELSLOCY140 Select the corner node NSELRLOCX0 FALLFX5 Load it NSELALL Reselect all nodes SAVE Saves file to jobnamedb SOLVE GENSUB created FINISH USE PASS FINISH CLEAR FILNAMEUSE Change jobname to use PREP7 Create Geometry of non superelements blc40010040 Creates rectangle Define material properties ET2PLANE42 Element type TYPE2 Turns on element type 2 MPEX2 25 Second material property set for silicon MPPRXY2041 Meshing AESIZE110 Element size mat2 Turns on Material 2 real2 Turns on real constants 2 amesh1 Mesh the area Superelement ET1MATRIX50 MATRIX50 is the superelement type TYPE1 Turns on element type 1 GETMaxNodeNODENUMMAX determine the max number of nodes SETRANGENMaxNodeGEN2 node number offset SEGEN2 Read in superelement matrix NSELSLOCY40 Select nodes at interface CPINTFALL Couple node pairs at interface NSELALL FINISH SOLU ANTYPESTATIC Static analysis NSELSLOCY0 Select all nodes at y 0 DALLALL0 Constrain those nodes NSELALL Reselect all nodes ESELSTYPE1 Element select SFEALL1SELV1 Apply superelement load vector ESELALL Reselect all elements SAVE SOLVE FINISH POST1 Enter post processing PLNSOLUSUM01 Plot deflection contour FINISH EXPANSION PASS CLEAR Clear database FILNAMEGEN Change jobname back to generation pass jobname RESUME Restore generation pass database SOLU Enter SOLUTION EXPASSONYES Activate expansion pass SEEXPGEN2USE Superelement name to be expanded EXPSOL11 Expansion pass info SOLVE Initiate expansion pass solution Full superelement solution written to GENRST FINISH POST1 PLNSOLUSUM01 Plot deflection contour Substructuring Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to show the how to use substructuring in ANSYS Substructuring is a procedure that condenses a group of finite elements into one superelement This reduces the required computation time and also allows the solution of very large problems A simple example will be demonstrated to explain the steps required however please note that this model is not one which requires the use of substructuring The example involves a block of wood E 10 GPa v 029 connected to a block of silicone E 25 MPa v 041 which is rigidly attached to the ground A force will be applied to the structure as shown in the following figure For this example substructuring will be used for the wood block The use of substructuring in ANSYS is a three stage process 1 Generation Pass Generate the superelement by condensing several elements together Select the degrees of freedom to save master DOFs and to discard slave DOFs Apply loads to the superelement 2 Use Pass Create the full model including the superelement created in the generation pass Apply remaining loads to the model The solution will consist of the reduced solution tor the superelement and the complete solution for the nonsuperelements 3 Expansion Pass Expand the reduced solution to obtain the solution at all DOFs for the superelement Note that a this method is a bottomup substructuring each superelement is created separately and then assembled in the Use Pass Topdown substructuring is also possible in ANSYS the entire model is built then University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATSubstructuringPrin Copyright 2001 University of Alberta superelement are created by selecting the appropriate elements This method is suitable for smaller models and has the advantage that the results for multiple superelements can be assembled in postprocessing ANSYS Command Listing BottomUp Substructuring GENERATION PASS Build the superelement portion of the model FINISH CLEAR START FILNAMEGEN Change jobname PREP7 Create Geometry blc4040100100 Creates rectangle Define material properties of wood section ET1PLANE42 Element type MPEX1 10000 Youngs Modulus MPPRXY1029 Poissons ratio meshing AESIZE110 Element size amesh1 Mesh area FINISH SOLU ANTYPESUBST SUBSTRUCTURE GENERATION PASS SEOPTGEN2 Name GEN and no printed output NSELSEXT Select all external nodes MALLALL Make all selected nodes master DOFs NSELALL Reselect all nodes NSELSLOCY140 Select the corner node NSELRLOCX0 FALLFX5 Load it NSELALL Reselect all nodes SAVE Saves file to jobnamedb SOLVE GENSUB created FINISH USE PASS FINISH CLEAR FILNAMEUSE Change jobname to use PREP7 Create Geometry of non superelements blc40010040 Creates rectangle Define material properties ET2PLANE42 Element type TYPE2 Turns on element type 2 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATSubstructuringPrin Copyright 2001 University of Alberta MPEX2 25 Second material property set for silicon MPPRXY2041 Meshing AESIZE110 Element size mat2 Turns on Material 2 real2 Turns on real constants 2 amesh1 Mesh the area Superelement ET1MATRIX50 MATRIX50 is the superelement type TYPE1 Turns on element type 1 GETMaxNodeNODENUMMAX determine the max number of nodes SETRANGENMaxNodeGEN2 node number offset SEGEN2 Read in superelement matrix NSELSLOCY40 Select nodes at interface CPINTFALL Couple node pairs at interface NSELALL FINISH SOLU ANTYPESTATIC Static analysis NSELSLOCY0 Select all nodes at y 0 DALLALL0 Constrain those nodes NSELALL Reselect all nodes ESELSTYPE1 Element select SFEALL1SELV1 Apply superelement load vector ESELALL Reselect all elements SAVE SOLVE FINISH POST1 Enter post processing PLNSOLUSUM01 Plot deflection contour FINISH EXPANSION PASS CLEAR Clear database FILNAMEGEN Change jobname back to generation pass jobname RESUME Restore generation pass database SOLU Enter SOLUTION EXPASSONYES Activate expansion pass SEEXPGEN2USE Superelement name to be expanded EXPSOL11 Expansion pass info SOLVE Initiate expansion pass solution Full superelement sol FINISH POST1 PLNSOLUSUM01 Plot deflection contour University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATSubstructuringPrin Copyright 2001 University of Alberta Coupled StructuralThermal Analysis Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to outline a simple coupled thermalstructural analysis 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 attemp to expand However since it is pinned this cannot occur and as such stress is created in the link A steadystate 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 degrees Celsius The link is steel with a modulus of elasticity of 200 GPa a thermal conductivity of 605 WmK and a thermal expansion coefficient of 12e6 K Preprocessing Defining the Problem According to Chapter 2 of the ANSYS CoupledField Guide A sequentially coupled physics analysis is the combination of analyses from different engineering disciplines which interact to solve a global engineering problem For convenience the solutions and procedures associated with a particular engineering discipline will be referred to as a physics analysis When the input of one physics analysis depends on the results from another analysis the analyses are coupled Thus each different physics environment must be constructed seperately so they can be used to determine the coupled physics solution However it is important to note that a single set of nodes will exist for the entire model By creating the geometry in the first physical environment and using it with any following coupled environments the geometry is kept constant For our case we will create the geometry in the Thermal Environment where the thermal effects will be applied Although the geometry must remain constant the element types can change For instance thermal elements are required for a thermal analysis while structural elements are required to deterime the stress in the link It is important to note however that only certain combinations of elements can be used for a coupled physics analysis For a listing see Chapter 2 of the ANSYS CoupledField Guide located in the help file The process requires the user to create all the necessary environments which are basically the preprocessing portions for each environment and write them to memory Then in the solution phase they can be combined to solve the coupled analysis ANSYS Command Listing finish clear title Thermal Stress Example prep7 Enter preprocessor k100 Keypoints k210 l12 Line connecting keypoints et1link33 Element type r14e4 Area mpkxx1605 Thermal conductivity esize01 Element size lmeshall Mesh line physicswritethermal Write physics environment as thermal physicsclear Clear the environment etchgtts Element type mpex1200e9 Youngs modulus mpprxy103 Poissons ratio mpalpx112e6 Expansion coefficient physicswritestruct Write physics environment as struct physicsclear finish solu Enter the solution phase antype0 Static analysis physicsreadthermal Read in the thermal environment dk1temp348 Apply a temp of 75 to keypoint 1 solve finish solu Reenter the solution phase physicsreadstruct Read in the struct environment ldreadtemprth Apply loads derived from thermal environment tref273 dk1all0 Apply structural constraints dk2UX0 solve finish post1 Enter postprocessor etableCompStressLS1 Create an element table for link stress PRETABCompStress Print the element table Coupled StructuralThermal Analysis Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to outline a simple coupled thermalstructural analysis 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 attemp to expand However since it is pinned this cannot occur and as such stress is created in the link A steadystate 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 degrees Celsius The link is steel with a modulus of elasticity of 200 GPa a thermal conductivity of 605 WmK and a thermal expansion coefficient of 12e6 K Preprocessing Defining the Problem According to Chapter 2 of the ANSYS CoupledField Guide A sequentially coupled physics analysis is the combination of analyses from different engineering disciplines which interact to solve a global engineering problem For convenience the solutions and procedures associated with a particular engineering discipline will be referred to as a physics analysis When the input of one physics analysis depends on the results from another analysis the analyses are coupled Thus each different physics environment must be constructed seperately so they can be used to determine the coupled physics solution However it is important to note that a single set of nodes will exist for the entire model By creating the geometry in the first physical environment and using it with any following coupled environments the geometry is kept constant For our case we will create the geometry in the Thermal Environment where the thermal effects will be applied University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATCoupledPrinthtml Copyright 2003 University of Alberta Although the geometry must remain constant the element types can change For instance thermal elements are required for a thermal analysis while structural elements are required to deterime the stress in the link It is important to note however that only certain combinations of elements can be used for a coupled physics analysis For a listing see Chapter 2 of the ANSYS CoupledField Guide located in the help file The process requires the user to create all the necessary environments which are basically the preprocessing portions for each environment and write them to memory Then in the solution phase they can be combined to solve the coupled analysis ANSYS Command Listing finish clear title Thermal Stress Example prep7 Enter preprocessor k100 Keypoints k210 l12 Line connecting keypoints et1link33 Element type r14e4 Area mpkxx1605 Thermal conductivity esize01 Element size lmeshall Mesh line physicswritethermal Write physics environment as thermal physicsclear Clear the environment etchgtts Element type mpex1200e9 Youngs modulus mpprxy103 Poissons ratio mpalpx112e6 Expansion coefficient physicswritestruct Write physics environment as struct physicsclear finish solu Enter the solution phase antype0 Static analysis physicsreadthermal Read in the thermal environment dk1temp348 Apply a temp of 75 to keypoint 1 solve finish solu Reenter the solution phase physicsreadstruct Read in the struct environment ldreadtemprth Apply loads derived from thermal environment tref273 dk1all0 Apply structural constraints dk2UX0 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATCoupledPrinthtml Copyright 2003 University of Alberta solve finish post1 Enter postprocessor etableCompStressLS1 Create an element table for link stress PRETABCompStress Print the element table University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATCoupledPrinthtml Copyright 2003 University of Alberta Using PElements Introduction This tutorial was completed using ANSYS 70 This tutorial outlines the steps necessary for solving a model meshed with pelements The pmethod manipulates the polynomial level plevel of the finite element shape functions which are used to approximate the real solution Thus rather than increasing mesh density the plevel can be increased to give a similar result By keeping mesh density rather coarse computational time can be kept to a minimum This is the greatest advantage of using pelements over helements A uniform load will be applied to the right hand side of the geometry shown below The specimen was modeled as steel with a modulus of elasticity of 200 GPa ANSYS Command Listing finish clear title PMethod Meshing pmethon Initialize pmethod in ANSYS prep7 Enter preprocessor k100 Keypoints defining geometry k20100 k320100 k44552 k55552 k680100 k7100100 k81000 k9800 k105548 k114548 k12200 a123456789101112 Create area from keypoints et1plane145 Element type keyopt133 Plane stress with thickness option r110 Real constant thickness mpex1200000 Youngs modulus mpprxy103 Poissons ratio esize5 Element size ameshall Mesh area finish solu Enter solution phase antype0 Static analysis nsubst2010020 Number of substeps outresallall Output data for all substeps time1 Time at end 1 lselslocx0 Line select at x0 dlallall Constrain the line all DOFs lselall Reselect all lines lselslocx100 Line select at x100 sflallpres100 Apply a pressure lselall Reselect all lines solve finish post1 Enter postprocessor setlast Select last set of data plesolseqv Plot the equivalent stress Using PElements Introduction This tutorial was completed using ANSYS 70 This tutorial outlines the steps necessary for solving a model meshed with pelements The pmethod manipulates the polynomial level plevel of the finite element shape functions which are used to approximate the real solution Thus rather than increasing mesh density the plevel can be increased to give a similar result By keeping mesh density rather coarse computational time can be kept to a minimum This is the greatest advantage of using pelements over helements A uniform load will be applied to the right hand side of the geometry shown below The specimen was modeled as steel with a modulus of elasticity of 200 GPa ANSYS Command Listing finish clear title PMethod Meshing pmethon Initialize pmethod in ANSYS University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATPElementPrinthtml Copyright 2003 University of Alberta prep7 Enter preprocessor k100 Keypoints defining geometry k20100 k320100 k44552 k55552 k680100 k7100100 k81000 k9800 k105548 k114548 k12200 a123456789101112 Create area from keypoints et1plane145 Element type keyopt133 Plane stress with thickness option r110 Real constant thickness mpex1200000 Youngs modulus mpprxy103 Poissons ratio esize5 Element size ameshall Mesh area finish solu Enter solution phase antype0 Static analysis nsubst2010020 Number of substeps outresallall Output data for all substeps time1 Time at end 1 lselslocx0 Line select at x0 dlallall Constrain the line all DOFs lselall Reselect all lines lselslocx100 Line select at x100 sflallpres100 Apply a pressure lselall Reselect all lines solve finish post1 Enter postprocessor setlast Select last set of data plesolseqv Plot the equivalent stress University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCATPElementPrinthtml Copyright 2003 University of Alberta Using PElements Introduction This tutorial was completed using ANSYS 70 This tutorial outlines the steps necessary for solving a model meshed with pelements The pmethod manipulates the polynomial level plevel of the finite element shape functions which are used to approximate the real solution Thus rather than increasing mesh density the plevel can be increased to give a similar result By keeping mesh density rather coarse computational time can be kept to a minimum This is the greatest advantage of using pelements over helements A uniform load will be applied to the right hand side of the geometry shown below The specimen was modeled as steel with a modulus of elasticity of 200 GPa ANSYS Command Listing finish clear title Convection Example prep7 Enter the preprocessor define geometry k100 Define keypoints k20030 k3003003 k40003 a1234 Connect the keypoints to form area mesh 2D areas ET1Plane55 Element type MPDens1920 Define density mpc12040 Define specific heat mpkxx118 Define heat transfer coefficient esize00005 Mesh size ameshall Mesh area finish solu Enter solution phase antype4 Transient analysis time60 Time at end of analysis nroptfull Newton Raphson full lumpm0 Lumped mass off nsubst20 Number of substeps 20 neqit100 Max no of iterations autotsoff Auto time search off lnsrchon Line search on outresallall Output data for all substeps kbc1 Load applied in steps not ramped ICalltemp268 Initial conditions temp 268 nselsext Node select all exterior nodes sfallconv10368 Apply a convection BC nselall Reselect all nodes gstoff Turn off graphical convergence monitor solve finish post1 Enter postprocessor setlast Read in last subset of data etablemeltytemp Create an element table eselsetabmelty273 Select all elements from table above 273 finish solu Reenter solution phase antyperest Restart analysis ekillall Kill all selected elements eselall Reselect all elements finish post1 Reenter postprocessor setlast Read in last subset of data eselslive Select all live elements plnsoltemp Plot the temp contour of the live elements Using PElements Introduction This tutorial was completed using ANSYS 70 This tutorial outlines the steps necessary for solving a model meshed with pelements The pmethod manipulates the polynomial level plevel of the finite element shape functions which are used to approximate the real solution Thus rather than increasing mesh density the plevel can be increased to give a similar result By keeping mesh density rather coarse computational time can be kept to a minimum This is the greatest advantage of using pelements over helements A uniform load will be applied to the right hand side of the geometry shown below The specimen was modeled as steel with a modulus of elasticity of 200 GPa ANSYS Command Listing finish clear title Convection Example prep7 Enter the preprocessor define geometry k100 Define keypoints k20030 k3003003 k40003 a1234 Connect the keypoints to form area University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysATBirthDeathprinthtml Copyright 2003 University of Alberta mesh 2D areas ET1Plane55 Element type MPDens1920 Define density mpc12040 Define specific heat mpkxx118 Define heat transfer coefficient esize00005 Mesh size ameshall Mesh area finish solu Enter solution phase antype4 Transient analysis time60 Time at end of analysis nroptfull Newton Raphson full lumpm0 Lumped mass off nsubst20 Number of substeps 20 neqit100 Max no of iterations autotsoff Auto time search off lnsrchon Line search on outresallall Output data for all substeps kbc1 Load applied in steps not ramped ICalltemp268 Initial conditions temp 268 nselsext Node select all exterior nodes sfallconv10368 Apply a convection BC nselall Reselect all nodes gstoff Turn off graphical convergence monitor solve finish post1 Enter postprocessor setlast Read in last subset of data etablemeltytemp Create an element table eselsetabmelty273 Select all elements from table above 273 finish solu Reenter solution phase antyperest Restart analysis ekillall Kill all selected elements eselall Reselect all elements finish post1 Reenter postprocessor setlast Read in last subset of data eselslive Select all live elements plnsoltemp Plot the temp contour of the live elements University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysATBirthDeathprinthtml Copyright 2003 University of Alberta Contact Elements Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to utilize contact elements to simulate how two beams react when they come into contact with each other The beams as shown below are 100mm long 10mm x 10mm in crosssection have a Youngs modulus of 200 GPa and are rigidly constrained at the outer ends A 10KN load is applied to the center of the upper causing it to bend and contact the lower ANSYS Command Listing finish clear titleContact Elements prep7 Top Beam X10 Y115 L1100 H110 Bottom Beam X250 Y20 L2100 H210 Create Geometry blc4X1Y1L1H1 blc4X2Y2L2H2 define element type ET1plane42 element type 1 keyopt133 plane stress wthick type1 activate element type 1 R 1 10 thickness 001 define material properties MPEX 1 200e3 Youngs modulus MPNUXY1 03 Poissons ratio meshing esize2 set meshing size ameshall mesh area 1 ET2contac48 defines second element type 2D contact elements keyo271 contact timeload prediction r220000010 TYPE2 activates or sets this element type real2 activates or sets the real constants define contact nodes and elements first the contact nodes aselsarea1 select top area nslas1 select the nodes within this area nselrlocyY1 select bottom layer of nodes in this area nselrlocxX2X2L22 select the nodes above the other beam cmsourcenode call this group of nodes source then the target nodes allsel relect everything aselsarea2 select bottom area nslas1 select nodes in this area nselrlocyH2 select bottom layer of nodes in this area nselrlocxX2X2L22 select the nodes above the other beam cmtargetnode call this selection target gcgensourcetarget3 generate contact elements between defined nodes finish solut antype0 time1 Sets time at end of run to 1 sec autotson Auto timestepping on nsubst100100020 Number of substeps outresallall Write all output neqit100 Max number of iterations nselslocxX1 Constrain top beam nselrlocyY1Y1H1 dallall nselall nselslocxX2L2 Constrain bottom beam nselrlocyY2Y2H2 dallall nselall nselslocxL12X1 Apply load nselrlocyY1H1 fallfy10000 nselall solve finish post1 dscale11 CVAL120408016032064012802560 PLNSOLSEQV01 Contact Elements Introduction This tutorial was completed using ANSYS 70 The purpose of the tutorial is to describe how to utilize contact elements to simulate how two beams react when they come into contact with each other The beams as shown below are 100mm long 10mm x 10mm in crosssection have a Youngs modulus of 200 GPa and are rigidly constrained at the outer ends A 10KN load is applied to the center of the upper causing it to bend and contact the lower ANSYS Command Listing finish clear titleContact Elements prep7 Top Beam X10 Y115 L1100 H110 Bottom Beam X250 Y20 L2100 H210 Create Geometry blc4X1Y1L1H1 blc4X2Y2L2H2 httpwwwmeceualbertacatutorialsansysCLCATcontactprinthtml Copyright 2003 University of Alberta define element type ET1plane42 element type 1 keyopt133 plane stress wthick type1 activate element type 1 R 1 10 thickness 001 define material properties MPEX 1 200e3 Youngs modulus MPNUXY1 03 Poissons ratio meshing esize2 set meshing size ameshall mesh area 1 ET2contac48 defines second element type 2D contact elements keyo271 contact timeload prediction r220000010 TYPE2 activates or sets this element type real2 activates or sets the real constants define contact nodes and elements first the contact nodes aselsarea1 select top area nslas1 select the nodes within this area nselrlocyY1 select bottom layer of nodes in this area nselrlocxX2X2L22 select the nodes above the other beam cmsourcenode call this group of nodes source then the target nodes allsel relect everything aselsarea2 select bottom area nslas1 select nodes in this area nselrlocyH2 select bottom layer of nodes in this area nselrlocxX2X2L22 select the nodes above the other beam cmtargetnode call this selection target gcgensourcetarget3 generate contact elements between defined nodes finish solut antype0 time1 Sets time at end of run to 1 sec autotson Auto timestepping on nsubst100100020 Number of substeps outresallall Write all output neqit100 Max number of iterations nselslocxX1 Constrain top beam nselrlocyY1Y1H1 dallall nselall nselslocxX2L2 Constrain bottom beam httpwwwmeceualbertacatutorialsansysCLCATcontactprinthtml Copyright 2003 University of Alberta nselrlocyY2Y2H2 dallall nselall nselslocxL12X1 Apply load nselrlocyY1H1 fallfy10000 nselall solve finish post1 dscale11 CVAL120408016032064012802560 PLNSOLSEQV01 httpwwwmeceualbertacatutorialsansysCLCATcontactprinthtml Copyright 2003 University of Alberta ANSYS Parametric Design Language APDL Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to familiarize the user with the ANSYS Parametric Design Language APDL This will be a very basic introduction to APDL covering things like variable definition and simple looping Users familiar with basic programming languages will probably find the APDL very easy to use To learn more about APDL and see more complex examples please see the APDL Programmers Guide located in the help file This tutorial will cover the preprocessing stage of constructing a truss geometry Variables including length height and number of divisions of the truss will be requested and the APDL code will construct the geometry ANSYS Command Listing finish clear prep7 askLENGTHHow long is the truss100 askHEIGHTHow tall is the truss20 askDIVISIONHow many cross supports even number2 DELTAL LENGTHDIVISION22 NUMK DIVISION 1 COUNT 1 XCOORD 0 doi1NUMK1 COUNT COUNT 1 OSCILATE 1COUNT XCOORD XCOORD DELTAL ifOSCILATEGT0THEN kiXCOORD0 else kiXCOORDHEIGHT endif enddo KEYP 0 doj1DIVISION1 KEYP KEYP 1 LKEYPKEYP1 ifKEYPLEDIVISION1THEN LKEYPKEYP2 endif enddo et1link1 r1100 mpex1200000 mpprxy103 esize1 lmeshall finish ANSYS Parametric Design Language APDL Introduction This tutorial was completed using ANSYS 70 The purpose of this tutorial is to familiarize the user with the ANSYS Parametric Design Language APDL This will be a very basic introduction to APDL covering things like variable definition and simple looping Users familiar with basic programming languages will probably find the APDL very easy to use To learn more about APDL and see more complex examples please see the APDL Programmers Guide located in the help file This tutorial will cover the preprocessing stage of constructing a truss geometry Variables including length height and number of divisions of the truss will be requested and the APDL code will construct the geometry ANSYS Command Listing finish clear prep7 askLENGTHHow long is the truss100 askHEIGHTHow tall is the truss20 askDIVISIONHow many cross supports even number2 DELTAL LENGTHDIVISION22 NUMK DIVISION 1 COUNT 1 XCOORD 0 doi1NUMK1 COUNT COUNT 1 httpwwwmeceualbertacatutorialsansysclcatapdlapdlhtml Copyright 2003 University of Alberta OSCILATE 1COUNT XCOORD XCOORD DELTAL ifOSCILATEGT0THEN kiXCOORD0 else kiXCOORDHEIGHT endif enddo KEYP 0 doj1DIVISION1 KEYP KEYP 1 LKEYPKEYP1 ifKEYPLEDIVISION1THEN LKEYPKEYP2 endif enddo et1link1 r1100 mpex1200000 mpprxy103 esize1 lmeshall finish httpwwwmeceualbertacatutorialsansysclcatapdlapdlhtml Copyright 2003 University of Alberta Viewing XSectional Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to view cross sectional results Deformation Stress etc of the following example ANSYS Command Listing FINISH CLEAR Title CrossSectional Results of a Simple Cantilever Beam PREP7 All dims in mm Width 60 Height 40 Length 400 BLC400WidthHeightLength Creates a rectangle ANGLE 1 60000000YS1 Rotates the display REPLOTFAST Fast redisplay ET1SOLID45 Element type MPEX1200000 Youngs Modulus MPPRXY103 Poissons ratio esize20 Element size vmeshall Mesh the volume FINISH SOLU Enter solution mode ANTYPE0 Static analysis ASELSLOCZ0 Area select at z0 DAAllALL0 Constrain the area ASELALL Reselect all areas KSELSLOCZLength Select certain keypoint KSELRLOCYHeight KSELRLOCXWidth FKAllFY2500 Force on keypoint KSELALL Reselect all keypoints SOLVE Solve FINISH POST1 Enter post processor PLNSOLUSUM01 Plot deflection WPOFFSWidth200 Offset the working plane for crosssection view WPROTA0090 Rotate working plane CPLANE1 Cutting plane defined to use the WP TYPE18 QSLICE display WPCSYS10 Deflines working plane location WPOFFS00116Length Offset the working plane CPLANE1 Cutting plane defined to use the WP TYPE15 Use the capped hidden display PLNSOLSEQV01 Plot equivalent stress Animation ANCUT430150050017142 Animate the slices Viewing XSectional Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to view cross sectional results Deformation Stress etc of the following example ANSYS Command Listing FINISH CLEAR Title CrossSectional Results of a Simple Cantilever Beam PREP7 All dims in mm Width 60 Height 40 Length 400 BLC400WidthHeightLength Creates a rectangle ANGLE 1 60000000YS1 Rotates the display REPLOTFAST Fast redisplay ET1SOLID45 Element type MPEX1200000 Youngs Modulus MPPRXY103 Poissons ratio esize20 Element size vmeshall Mesh the volume University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPSlicePrinthtml Copyright 2001 University of Alberta FINISH SOLU Enter solution mode ANTYPE0 Static analysis ASELSLOCZ0 Area select at z0 DAAllALL0 Constrain the area ASELALL Reselect all areas KSELSLOCZLength Select certain keypoint KSELRLOCYHeight KSELRLOCXWidth FKAllFY2500 Force on keypoint KSELALL Reselect all keypoints SOLVE Solve FINISH POST1 Enter post processor PLNSOLUSUM01 Plot deflection WPOFFSWidth200 Offset the working plane for crosssection view WPROTA0090 Rotate working plane CPLANE1 Cutting plane defined to use the WP TYPE18 QSLICE display WPCSYS10 Deflines working plane location WPOFFS00116Length Offset the working plane CPLANE1 Cutting plane defined to use the WP TYPE15 Use the capped hidden display PLNSOLSEQV01 Plot equivalent stress Animation ANCUT430150050017142 Animate the slices University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPSlicePrinthtml Copyright 2001 University of Alberta Advanced XSectional Results Using Paths to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to create and use paths to provide extra detail during post processing For example one may want to determine the effects of stress concentrators along a certain path Rather than plotting the entire contour plot a plot of the stress along that path can be made In this tutorial a steel plate measuring 100 mm X 200 mm X 10 mm will be used Three holes are drilled through the vertical centerline of the plate The plate is constrained in the ydirection at the bottom and a uniform distributed load is pulling on the top of the plate ANSYS Command Listing finish clear title Defining Paths PREP7 create geometry BLC400200100 cyl4505010 cyl41005010 cyl41505010 asba1all et1plane23 Plane element R110 thickness of plane mpex1200000 Youngs Modulus mpprxy103 Poissons ratio esize5 mesh size ameshall area mesh finish solu apply constraints lselslocy0 select line for contraint application dlallUY constrain all DOFs on this face allsel apply loads allsel restore entire selection lselslocy100 SFLallPRES200010 apply a pressure load on a line allsel solve solve resulting system of equations finish plot results window1top define a window top half of screen POST1 PLNSOLSeqv21 plot stress in xx direction deformed and undeformed edge window1off noerase window2bot define a window bottom half of screen nselall define nodes to define path nselslocy50 choose nodes half way through structure pathcutline21000 define a path labeled cutline ppath1050 define endpoint nodes on path ppath220050 PDEFSeqvAVG calculate equivalent stress on path nselall PLPAGMSEQV200NODE show graph on plot with nodes Advanced XSectional Results Using Paths to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to create and use paths to provide extra detail during post processing For example one may want to determine the effects of stress concentrators along a certain path Rather than plotting the entire contour plot a plot of the stress along that path can be made In this tutorial a steel plate measuring 100 mm X 200 mm X 10 mm will be used Three holes are drilled through the vertical centerline of the plate The plate is constrained in the ydirection at the bottom and a uniform distributed load is pulling on the top of the plate ANSYS Command Listing finish clear title Defining Paths PREP7 create geometry BLC400200100 University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPAdvancedXSecRes Copyright 2003 University of Alberta cyl4505010 cyl41005010 cyl41505010 asba1all et1plane23 Plane element R110 thickness of plane mpex1200000 Youngs Modulus mpprxy103 Poissons ratio esize5 mesh size ameshall area mesh finish solu apply constraints lselslocy0 select line for contraint application dlallUY constrain all DOFs on this face allsel apply loads allsel restore entire selection lselslocy100 SFLallPRES200010 apply a pressure load on a line allsel solve solve resulting system of equations finish plot results window1top define a window top half of screen POST1 PLNSOLSeqv21 plot stress in xx direction deformed and undeformed edge window1off noerase window2bot define a window bottom half of screen nselall define nodes to define path nselslocy50 choose nodes half way through structure pathcutline21000 define a path labeled cutline ppath1050 define endpoint nodes on path ppath220050 PDEFSeqvAVG calculate equivalent stress on path nselall PLPAGMSEQV200NODE show graph on plot with nodes University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPAdvancedXSecRes Copyright 2003 University of Alberta Data Plotting Using Tables to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to plot Vertical Deflection vs Length of the following beam using tables a special type of array By plotting this data on a curve rather than using a contour plot finer resolution can be achieved This tutorial will use a steel beam 400 mm long with a 40 mm X 60 mm cross section as shown above It will be rigidly constrained at one end and a 2500 N load will be applied to the other ANSYS Command Listing finish clear title Use of Tables for Data Plots prep7 elementsize 20 length 400 et1beam3 Beam3 element r12400320e340 AreaIHeight mpex1200000 Youngs Modulus mpprxy103 Poissons Ratio k100 Geometry k2length0 l12 esizeelementsize Mesh size lmeshall Mesh finish solu antypestatic Static analysis dk1all Constrain one end fully fk2fy2500 Apply load to other end solve finish post1 Note there are 21 nodes in the mesh For the procedure below the table must have nodes 1 rows rows lengthelementsize 1 1 DIMgraphTABLErows21 Creat a table called graph 22 rows x 2 columns x 1 plane vgetgraph11nodealllocx Put node locations in the x direction in the first column for all nodes vgetgraph12nodealluy Put node deflections in the y direction in the second column setgraph210 Delete data in 21 which is for x 400 otherwise graph is not plotted properly setgraph220 Delete data in 22 which is for UY x 400 otherwise graph is not plotted properly vgetgraphrows1node2locx Reenter the data for x 400 but at the end vgetgraphrows2node2uy of the table vplotgraph11graph12 Plot the data in the table axlabxLength Change the axis labels axlabyVertical Deflection replot Data Plotting Using Tables to Post Process Results Introduction This tutorial was created using ANSYS 70 The purpose of this tutorial is to outline the steps required to plot Vertical Deflection vs Length of the following beam using tables a special type of array By plotting this data on a curve rather than using a contour plot finer resolution can be achieved This tutorial will use a steel beam 400 mm long with a 40 mm X 60 mm cross section as shown above It will be rigidly constrained at one end and a 2500 N load will be applied to the other ANSYS Command Listing finish clear title Use of Tables for Data Plots prep7 elementsize 20 length 400 et1beam3 Beam3 element r12400320e340 AreaIHeight mpex1200000 Youngs Modulus mpprxy103 Poissons Ratio k100 Geometry k2length0 l12 esizeelementsize Mesh size University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPDataPlottingPrinth Copyright 2003 University of Alberta lmeshall Mesh finish solu antypestatic Static analysis dk1all Constrain one end fully fk2fy2500 Apply load to other end solve finish post1 Note there are 21 nodes in the mesh For the procedure below the table must have nodes 1 rows rows lengthelementsize 1 1 DIMgraphTABLErows21 Creat a table called graph 22 rows x 2 columns x 1 plane vgetgraph11nodealllocx Put node locations in the x direction in the first column for all nodes vgetgraph12nodealluy Put node deflections in the y direction in the second column setgraph210 Delete data in 21 which is for x 400 otherwise graph is not plotted properly setgraph220 Delete data in 22 which is for UY x 400 otherwise graph is not plotted properly vgetgraphrows1node2locx Reenter the data for x 400 but at the end vgetgraphrows2node2uy of the table vplotgraph11graph12 Plot the data in the table axlabxLength Change the axis labels axlabyVertical Deflection replot University of Alberta ANSYS Tutorials wwwmeceualbertacatutorialsansysCLCPPDataPlottingPrinth Copyright 2003 University of Alberta