ANSYS� Quick Reference

ANSYS™ Quick Reference www.come.tum.de Technical University of Munich Acknowledgements This paper is to a great extent based on the work by Prof. Dr.Ing. habil. Manfred Bischoff, Institute of Structural Mechanics, University of Stuttgart (http://www.ibb.uni-stuttgart.de), and Dipl.Ing. Moritz Frenzel M.Sc., Chair of Computational Mechanics, Technical University of Munich (http://www.lnm.mw.tum.de). We gratefully acknowledge their permission to use their work. Introduction This is not an ANSYS™ manual! ANSYS™ is a general purpose finite element package whose full documentation is available as ‘online help’ and would fill half a bookshelf when printed. There are numerous tutorials and sample problems available on the internet, but all of them serve different, and mostly specific purposes, reflecting the numerous areas of applicability of ANSYS™ (structural, thermal, electrical, etc.). This little quick reference collects hints to the most important features in the context of the courses “Modeling and Simulation I and II” within the Master Program in Computational Mechanics at the TU München. It is intended to serve as a help to get started with ANSYS™. After getting familiar with these basic steps it should be no problem to handle more complex applications with the help of the aforementioned online manual. Disclaimer: We do not take any responsibility for the information herein. This quick reference is not licensed, sponsored or connected in any other way to ANSYS™. If you downloaded this document and you are not a student of CoMe.TUM, please drop us a note (come@bv.tum.de). General Procedure ANSYS™ provides two principally different methods to issue commands: Either using a menu structure or a command line. Professionals who use ANSYS™ usually work with the command line because it is more efficient and provides an easy possibility to use readily prepared ‘macros’ (often used command sequences). To get started, however, it is recommended to use the menus. They help to lo lead you through the process of model creation, meshing, solving and plotting the results and provide a quick overview of the possibilities that the program offers. Note: depending on the ANSYS™ version, the menues might differ slightly from the examples herein. The main steps of a typical ANSYS™ session are: • • Create the geometrical model (keypoints, lines, areas, volumes and their combinations) Define the finite element model by choosing the element type (including “real constants”), material data, and applying boundary conditions and loads Choose a solver and compute the solution Review and analyze the results (output numbers or display plots) Preprocessing Preprocessing / Solution • • Solution Postprocessing It is recommended to always watch the output in the other (black) window to check if a command was accepted and how it is interpreted. All commands (whether written in the command line or specified over the menues) are written to a text file ("log file") which can be saved and used for a re-modeling. Note that "everything else" (for instance re-sizing of graphics) is also written to this log file so that it might become quite full with non-useful lines. The best is to delete unnecessary lines but it is sometimes difficult to guess which lines are important. But once you have understood most commands you will see that log files are an indispensible tool for quick and efficient modeling! Preprocessing commands Start Preprocessor To get into the preprocessing part of ANSYS™. From here all preprocessing commands are accepted. Main Menu > Preprocessor Command at the input line /prep7 Geometric Model Create Keypoint You can use keypoints as a geometric basis of the model. You can create the model bottom-up, which means first the keypoints then the lines, areas, etc. Alternatively, you can create the model top-down, for example directly create a rectangle resulting in an automatic generation of lines and keypoints. Keypoints are helpful for every geometric operation in complex structures and also, for instance, to apply concentrated loads and boundary conditions. They are defined by coordinates and are numbered automatically or user defined. Create > Lines Create Lines Create Arcs Modeling Create > Keypoints > On Working Plane > In Active CS > On Line K,NPT,X,Y,Z Defining Keypoints in the input line is very efficient and therefore recommended! L,KPstart,KPend Create Arbitrary Creates an arbitrary polygonal area. Create Rectangle Create Circle > Straight Line Create > Lines > Arcs > Through 3 KPs > By End KPs & Rad > By Cent & Radius > Full Circle Create > Area > Arbitrary > Through KPs > By Lines Create > Area > Rectangle > By 2 Corners > By Centr & Cornr > By Dimensions Create > Area > Circle > Solid Circle > Annulus > Partial Annulus A,KP1,KP2,KP3,… Copy Objects Easy modeling of repeated geometric objects or geometries with periodic properties. Offset depends on active coordinate system. Model Operations Boolean operations to merge geometric primitives or remove intersecting areas. > By End Points > By dimensions Copy > Keypoints > Lines > Areas Operate –Booleans> Add > Subtract > Divide > Glue Finite Element Structure Define Element Type Customize the list of required element types (beams, plates, shells, etc.) Provide Appropriate Constants for Individual Element Types For example the element thickness Define Material Properties For example Young´s modulus, Poisson’s ratio, etc. Assign Attributes Assign attributes (material properties, element types) to selected parts of the model. To make the attributes visible select numbering. Note: By default, all the elements that are created with the mesh command, obtain the “current” (i.e. last defined) attributes. Element Type > Add/Edit/Delete ET,ETNr,Ename Real Constants > Add/Edit/Delete Material Props > Material Models Meshing > Mesh Attributes > Keypoints > Lines > Areas R,SetNr,Value1,… Mesh the Model Create a finite element mesh for the model. Make sure to choose the appropriate dimensionality, i.e. one-dimensional for lines (beams), twodimensional for areas (plates, shells), three-dimensional for volumes (solid elements). Choose properties like element size, element shape, etc. prior to meshing. Usually, using the Mesh Tool instead of the individual commands in the mesh menu is recommendable! MeshTool Element Attributes Smart Size Size Controls Meshing > MeshTool Mesh Clear Refine Close Coupling / Ceqn > Coincident Couple Nodes Nodes The Meshes of all individual areas have to be compatible. If this is not the case one possibility would be to couple nodes at the intersections of individual mesh patches (areas) to connect these parts. Alternatively you can connect the areas by Boolean operations. Loads Loads and also boundary conditions are in general applied to the finite element model (i.e. after meshing). If the mesh is changed, all load data is lost! Loads > Define Loads > Apply > Displacement Boundary Conditions Displacement Defines boundary conditions for lines, areas, keypoints or nodes. All > On Lines degrees of freedom (DOF) can be addressed separately, the prescribed > On Areas displacement may be zero or non-zero. There is also a feature to > On Keypoints automatically generate symmetric and antisymmetric boundary > On Nodes conditions (Caution: The program needs to ‘guess’ the symmetry plane Define material number, element type, real constants,… Element size for ‘quick and dirty’ free meshing Specify mesh density via subdivision of lines (best to obtain structured and compatible meshes) or element lengths Generate the mesh, either free (automatic) or mapped (structured) with triangles or quads Clear the mesh. Has to be done for any changes in the finite element structure! Mesh refinement in the area of chosen elements, lines, keypoints, etc. Leave the MeshTool from the given model because it does, of course, not know the real structure. Always verify that that the generated boundary conditions are correct). Loads > Define Loads > Apply > Concentrated Loads and Moments Force/Moment > On Keypoints > On Nodes Loads > Define Loads > Apply > Pressure > On Lines > On Areas > On Nodes Loads > Delete > > All Load Data > Displacement > Force/Moment > Pressure Pressure Loads To apply pressure loads, i.e. loads that are perpendicular to the given geometric entity Delete Loads and Boundary Conditions Solution Commands Main Menu > Solution Start Solution Part Now only solution commands are accepted at the input line. Analysis Type > Sol´n Control Control the Solution Procedure Several solution options, mostly for non-linear computations Solve > Current LS Solve Problem Solves the current finite element system of equations (applying iterative incremental schemes in the case of non-linear problems). Be sure to select everything prior to solving! /Solu Postprocessing Commands Start Postprocessor Now only postprocessing commands are accepted at the input line Generate result plots After a successful computation you can create various plots of the results like deformations, stresses, etc. You can choose between nodal solutions mostly used for deformation results and element solutions, usually for stress plots. To change appearance of plots use plotctrls. Generate List of Results All data can also be listed as numbers, e.g. nodal values for the displacements etc. Work with sections / Path operations To display results at user defined sections, for example to perform equilibrium checks, paths have to be defined. Along these paths all data can be plotted and listed. It is also possible to do certain computations, for example to obtain a moment out of stress values and coordinates (i.e. the excentriticity). Note: All path data will be lost when leaving POST1 (but you can store the data in a file). To visualize a stress distribution on a path: - define a path - map the corresponding values onto the path by defining a name and the specified value, e.g. stress in x-direction (SX). Mind the option of average results over the element! - plot the corresponding path items either on the geometry (adjust the scale factor!) or on a special graph (which allows more items in one plot). - The following procedure is an example to obtain a moment for an equlibrium check: map the stresses on the path; do multiply this item with the geometry distance (e.g. YG) and give it a new item-name; do integrate this new item over the geometry; the result is shown in the output window (DOS-Box). Note: The number of intersections, defined in the specifications at the Main Menu > General Postproc Plot Results > Deformed Shape > Contour Plot > Nodal Solu > Contour Plot > Element Solu > -Vector Plot- Predefined List Results /Post1 Path Operations > Define Path > By Nodes > On Working Pl > By Location > Delete Path > Plot Paths > Recall Path > Map onto Path > Plot Path Item > On Graph > Plot Path Item > On Geometry > Plot Path Item > List Path Items > Various Calculations > Archive Path >Store/Retrieve beginning, control the accuracy of the plot and the subsequent computations (like integration). Work with Element Tables To visualize certain element results it is necessary to define element tables. They can be plotted, listed, sorted, etc. It is possible to select certain elements. Element Table > Define Table > Plot Elem Table > List Elem Table > Find Maximum/Find Minimum Utility Menu File Write DB Log File Read Input from List > Log File File controls, handling of job name. Creates a text file (ascii) with all commands of the whole history of the current session. It is sensible to save your work up to a certain stage once in a while (can be used later like an ‘undo’ option). Read commands out of text file (see above). View the current Log File. Selecting parts of the finite element model. All subsequently issued commands refer exclusively to the current selection. By default (at the beginning of your project) everything is selected. Select individual entities of the model (nodes, elements, lines, areas keypoints) either graphically (By Num/Pick) or with the help of certain properties (e.g. coordinates). Selects everything. Has to be done each time before starting a computation! Provides the possibility to list every kind of information like working-files, program-status, geometrical data, finite element data, etc. To plot all individual objects. Useful during modeling to organize the screen. To obtain a general replot. Controls all plot options. As there is a huge number of options, only the most important are listed below. Opens a window for easy controlling of zoom, viewing angle, etc. To view the entire model click Fit As all objects and attributes are numbered it is sometimes useful to plot the numbers. Especially for element attributes with different materials or real constants. Useful to display boundary conditions and forces (also as arrows instead of face outlines) Select Entities Everything List Plot Multi-Plots PlotCtrls Pan, Zoom, Rotate Numbering Symbols Style > Contours > It is possible to change the number of contours to control the quality of the plot. Uniform Contours Animate > Deformed Nice tool to animate your computation and see what happens (non-linear problems). Results Redirect Plots Capture Image MultiWindow Layout Export into other graphic standards. Redirect to screen to switch it back. For screenshots to compare different plots. More than one window. Work Plane controls WorkPlane Display Working Shows working plane triad. Plane WP Settings Tool to control working plane as grid, activate ‘snapping’, etc. Change Active CS to Changes coordinate system to cartesian, cylindrical or spherical for all modeling commands (lines, keypoints,…). During preprocessing the status is shown in the title of the graphics window. Parameters Scalar Parameters Parameters are used as variables. For example a load can be defined as a variable F and then set to different values. Useful in general, needed for optimization problems. Tool to define, set and check all parameters.