Finite Element Analysis
E-mail Address: Please see my main page.
Return to Main Page
FEA and Optimization Introduction Page A Quick Overview of FEA
ANSYS® Tips Page My Collection of Tips on ANSYS Use.
Modeling issues include a host of topics. I will mention some that have been relevant to my experience. After almost six years of continuous use of the ANSYS program, I continue to learn new features of the software, discover more ways to represent or approximate features, and develop new ways to get useful output information from the models.
Example of Approximation: I wrote a macro to give the surface area (one side) of a previously selected set of shell elements. A force divided by this area can be applied as pressure over these shell elements, for smooth force application, if the elements are flat. Writing the macro required a few lines of code that: determine the number of elements, get the first element identity, create an array of correct size to hold data, put the areas of the elements into the array, sum the array entries, report the result, and delete the variables and array. NOTE: The user must be careful to apply the pressure to the CORRECT FACE of the set of shell elements. Force or pressure on a flat shell may require Large Displacement (geometrically nonlinear) analysis.
MODELING ISSUES that are faced include (but are by no means limited to):
FEA is Approximate.The first issue to understand in Finite Element Analysis is that it is fundamentally an approximation. The underlying mathematical model may be an approximation of the real physical system (for example, the Euler-Bernoulli beam ignoring shear deformation). The finite element itself approximates what happens in its interior with interpolation formulas. The interior of a 2-D or 3-D finite element has been mapped to the interior of an element with a perfect shape, so a severely distorted element can not deform in a manner that has an accurate match to the real physical response. Integration over the body of the element is often approximated by Gaussian Quadrature (depending on the element, an analytical integral can be either impractical or exceedingly difficult -- I've done a few with the computer algebra system MACSYMA and the number of terms can explode unless constants are extracted during the derivation and the integrand is kept factored; some elements are said to be more accurate with numerical integration at a limited number of points). The continuity of deformation between connected elements is interrupted at some level. Badly shaped (by distortion, warping or extreme aspect ratio) elements can give less accurate results. Elements approximate the local shape of the real body. Numerical analysis difficulties such as ill-conditioned matrices may reduce the accuracy of calculated results. A linear analysis is an approximation of the real behavior. The loading of the model is an approximation of what happens in the real world. The boundary conditions approximate how the structure is supported by the outside world. The material properties assumed are approximate. Flaws are not represented unless the analyst incorporates a model of a flaw. The overall dimensions of the model approximate real structures that are manufactured within a tolerance. Many details are idealized, simplified, or ignored. Element results may be reported at integration points or nodes, not continuously evaluated with the interpolation functions over the whole element interior. Stress and strain results are based on the derivatives of the displacement solution, amplifying the errors.
The result of an analysis contains the accumulated errors due to all of the contributing approximations. Good analysis and interpretation of results requires knowing what is an acceptable approximation, development of a complete list of what should be evaluated, appreciation of the need for margin of safety, and comprehension of what remains unknown after an analysis.
Meshing.Production of a good quality mesh is a major topic. The mesh should be fine enough for good detail where information is needed, but not too fine, or the analysis will require considerable time and space in the computer. A mesh should have well-shaped elements -- only mild distortion and moderate aspect ratios. This can require considerable user intervention, despite FEA software promotional claims of automatic good meshing. The user should put considerable effort into the generation of well-shaped meshes. This will include setting element densities, gradients in element size, concatenation of lines or areas to permit mapped meshing, playing with automatic meshing controls, and re-meshing individual areas and volumes until the result looks "just right".
In ANSYS, the command "LSEL,S,NDIV,,0" will select all the lines that have not had mesh density assigned. This can help find missed lines when setting mesh densities manually.
On a curved surface, quadrilateral shell elements should not be generated with a warped form. (The theory manual discusses shell element warping, but I suspect that the discussion is more relevant to element deformation under load, than to the initial un-deformed element shape. ANSYS will give warnings if there is more than very slight warping of the original un-deformed quad shell element shape.) Quad shell elements can sometimes be fitted to a cylindrical curve so that they are rectangular in shape and not warped. On other curved surfaces, finely meshed triangular 3-node or four-sided curved 8-node shell elements may be needed. Mid-side node elements can follow complex curved surfaces, so if they are capable of any nonlinearity that will be needed, they may be acceptable and preferred. The 8-node Shell93 shell element of ANSYS has mid-side nodes, follows curved surfaces, and supports nonlinearity.
Remember that most finite elements are stiffer than the real structure. For these elements, a coarse mesh generally results in a structure that underpredicts deflection, and overpredicts buckling load and vibration frequency. A coarse mesh is less sensitive to and "hides" stress concentrations. A fine mesh generally gives an answer closer to the exact solution. A fine mesh also results in larger models, more data storage, and longer model solution and display times.
Shell versus Solid versus Beam Elements.Ideally, structures would be represented for Finite Element Analysis by solid elements, for this would eliminate the problem of positioning the mid-plane of shell elements, exactly represent the sectional properties of components, and position welds in their design location. Unfortunately, there would have to be several solid elements through the thickness of sheets of steel or aluminum to capture local bending effects with any accuracy, and the other dimensions of the elements would have to be kept small so that the aspect ratios of the elements were acceptable. Consequently, the number of elements would be unbelievably large. It is not feasible to model many thin-wall structures with solid elements.
Shell elements were originally developed to efficiently represent thin sheets or plates of steel or aluminum, both flat and curved surfaces. They include out-of-plane bending effects in their fundamental formulation, as well as transferring shear, tension, and compression in the plane. Developing an interface between a shell portion and a solid element portion of a model has a difficulty: Most solid elements do not include rotational degrees of freedom at the nodes, and this results in a rotational "joint" if shell elements are connected to a solid. Even if a solid element with rotational degrees of freedom is used, the rotational stiffness at a solid's edge node is not appropriate for connection to shell elements -- these solid elements were intended to be connected to each other. In addition, high order solid elements like these are not usually capable of nonlinear analysis. A modeling trick that is often used is to overlap one shell element with the first element in a solid, and join the nodes in two locations in order to imply continuity of rotations, as well as deflections. This is not a perfect fix. Rigid regions with node pairs (rigid links with CERIG) may be used to enforce connection, although high local stresses will result. Some finite element software may have tools to address this problem.
Of course, beam elements are even simpler and more efficient, when structures employ beam-like details. There are occasions in FEA work when structural beams (including I, wide-flange, channels and angles) will be more fully represented as shells or solids, in order to examine in detail how they are behaving, or interacting with the structure where they are connected to other parts. Structural steel tubing and rolled sections can sometimes be simplified as beam elements. NOTE: Remember that when shapes are simplified as beam elements, we lose the possibility of predicting flange buckling, web buckling, and concentrated stresses, so caution must be used. Link elements will not show bending stress or Euler buckling of a link.
On the XANSYS listserver, I have seen the opinion that the ANSYS PCG solver is not significantly faster than the frontal solver with shell elements, because of the great stiffness difference between in-plane deflections of shell elements, and out-of-plane deflections. In the ANSYS manuals the PCG solver is not recommended where significant numbers of coupled nodes (CP) and rigid regions (CERIG) have been defined. Gap and contact elements may introduce the same problem. This has usually been my experience. However, when modeling a perforated flat plate with shell elements that were roughly square, all about the same shape and size, and as thick as they were wide, using about 200,000 degrees of freedom, I achieved good convergence with the PCG solver. The frontal solver could not fit this problem into my computer because of the size and large wavefront. Of course, you can speed up the "solution" of the PCG solver by accepting a larger convergence error. You know you are having PCG convergence trouble when the convergence error is not decreasing monotonically (when it goes up and down instead of dropping smoothly). The PCG solver is not recommended for use with nonlinear solutions. One time I tried it I got a negative on the diagonal, which would have resulted in bisection with the Frontal solver and adaptive time stepping, but crashed ANSYS with the PCG solver. However, for better behaved models, I have achieved apparently good results with the PCG solver, with shell elements, in nonlinear Large Displacement runs.
Reduction of the model to a shell structure.Shell elements are appropriate for many steel structures, since the plates of steel are thin in comparison with their other dimensions. (This applies to aluminum and other materials, too.) The ideal position for the shell element is on the mid-plane position of the sheet of steel. Consequently, a variety of approximations are needed to link parts of the model together, so that the surfaces act as if they are welded together.
ANSYS supports shell elements for which the element thickness varies within the element. This could require a REAL value for every element in order to input a different shell thickness at each node. Input from external programs such as CAD packages sometimes generates such elements and information. User-written macros are sometimes employed to generate elements with varying thickness, or to set up REAL values for existing elements, with the thickness that is assigned being based on node position.
There is a helpful if less-than-ideal fix for the case when somewhat thick shells overlap each other, and are welded together. Place the shell mid-surfaces correctly in space, and mesh them so that nodes where welds are used are positioned directly "above" one another on the two surfaces. Join those nodes in pairs with rigid regions (CERIG) or with massless high-stiffness beam elements. The beam elements have the advantage of working properly in large displacement (geometrically nonlinear) solutions. The problem with this technique is that it requires proper mesh control if the user wants to automate generation of the model, and it is tedious to implement manually. In some cases it will be desired to place gap or surface contact elements (with the gap set closed) between the nodes or elements in the interior of the pair of shells, requiring more work. The gap elements keep their original orientation in a large displacement solution, so they will not be applicable in large displacement analyses (unless you can live with the error), and surface contact elements will be needed. Surface contact elements on shell elements must be applied to the correct face of the shell elements.
The following figure shows two areas that are offset with one above the other. Lines have been created so that the CERIG command can be used to join them as if they were welded together. Mesh densities have been set so that the rigid region pairs can be created.
The next figure shows the same two areas after meshing and the creation of the rigid region pairs with CERIG. The shell elements have been plotted with the shell thickness shown, so that the positioning of the nodes in the center of the shell elements is visible, and the touching of the plates is implied. Remember that rigid regions only apply accurately with Small Displacement analysis.
Automating the creation of these CERIG pairs could be done with a macro that:
The macro would work as long as the nodes for the sets of lines are located "above" one another by appropriate mesh control on the lines. A similar macro could join the node pairs with the massless high stiffness beam elements mentioned. Alternatives to using a macro include applying the CEINTF or the EINTF commands with appropriate tolerance values. The reader is cautioned that this technique tells us little about the stresses in the weld, or about fatigue, crack growth and fracture. A prying load applied to the above example could tear the weld apart if the weld was small in comparison to the shell thickness. The example does not illustrate good design practice for handling certain loads. The FEA evaluation of loading of welds in shell structure models is a whole separate topic.
Pressure on Shell Elements.In ANSYS, shell elements have two sides. These are known as the TOP and the BOTTOM faces. They are also known as FACE 1 (the BOTTOM) and FACE 2 (the TOP). The nodes I,J,K,L form a path around the element. If the "right hand rule" is used on this path, the fingers of the right hand following the path, then the thumb points out of the TOP surface (FACE 2).
If positive (into the element) pressure is to be applied to FACE 2, a positive pressure vector points into FACE 2, the TOP. If positive pressure is to be applied to FACE 1, a positive pressure vector points into FACE 1, the BOTTOM. Areas act similarly.
If a simple primitive solid (for example a cube) is created in ANSYS, it is bounded by areas. The areas will have FACE 1 on the inside surface, while FACE 2 is on the outside of the solid. If the volume was deleted, and the areas that bounded the solid were to be pressurized on the interior of the box that was formed, the pressure should be applied to FACE 1 on all sides. In other models, where Boolean operations have been performed, the FACE 1 and FACE 2 orientations get very scrambled.
For the user to apply pressure, careful checking must be used to assure that the correct faces of shell element have been pressurized. ANSYS can plot elements or areas for which the positive vector points out of the screen (when coming out of FACE 2), or when it points into the screen. This lets the user plot only those areas or elements for which the user sees FACE 2, or for which the user sees only FACE 1. This helps in choosing whether to apply pressure to FACE 1 or FACE 2 when using picking to select areas or elements. Alternatively, ANSYS 5.3 (and presumably later) plots shell elements with different colors for FACE1 and FACE2 under PowerGraphics when the numbering options are set with "No Numbering" and with "Colors" or "Colors and Numbers".
To add to the challenge, the direction of the pressure arrows (choose arrows to be shown to indicate pressures under the SYMBOLS choice under PlotCtrls on the Utility Menu) for areas may differ from the direction of the arrows shown for the elements attached to those areas, depending on surfaces visible and sides to which the pressure was applied. The arrow plots for the elements are the ones to believe. Pressures have to be transferred from geometric entities to elements in order for these plots to take place. You have to activate plotting of arrows with the /PSF command -- by default surface symbols are used. ANSYS only plots pressure arrows on shell elements when the arrows point into the screen, so you have to look at a model from all directions when inspecting a shell model. Have fun!
Final notes on pressures: ANSYS can include a gradient in the applied pressure to show the effect of, for example, pressure increasing as a depth of water increases. "Suction" can also be applied by using a minus sign. Remember that "suction" in physically realistic models cannnot be applied beyond the point at which a liquid boils, or below zero absolute pressure. ANSYS, however, does not limit the negative pressure values that a user enters. The hydrostatic pressure of oil floating on water might be modeled by setting the "zero" position of the water pressure gradient above the position where the water starts, in order to include the pressure of the oil. A variety of other tricks can be applied.
Reflecting Part of a Model.Where symmetry in the design exists, only a partial model need be built; the rest can be created by reflecting (mirror imaging) the geometry. Where structure is repeated (e.g. a set of posts) multiple copies can be made.
Reflection in ANSYS can be done across the XY, YZ, or ZX planes of any ACTIVE Cartesian coordinate system. Since the active coordinate system can be any local system that the user has defined, any kind of reflection in 3D Cartesian space can be accomplished.
If the reflection included geometry, nodes, or elements that were on the XY, YZ, or ZX plane about which the reflection took place, copies of those entities will overlay the original copy on the plane of reflection. Entity appropriate merge (NUMMRG) commands will be needed to connect the original and reflected entities. Warning: As discussed elsewhere, elements lying in the plane of reflection get copied with the node order reversed, and will NOT merge with the element from which they were generated. These elements may have to be deleted, depending on your intentions.
Representation of Bolted Connections.This non-trivial item can be tackled at a simplified level, or with detailed 3-D representation. The simplest approximation is to represent the bolted (or riveted) connection of overlapping shell structures by locating a node of each surface at the location of the bolt. The nodes have to be located at the same X,Y,Z location in space. This means offsetting one or both shells from its nominal position so that the nodes and shells can touch. One then uses nodal coupling (the CP command in ANSYS) to tie the X, Y, and Z locations in space. It will generally be desirable to tie two of the three rotations as well. The only rotation that is free is that about an axis perpendicular to the planes of elements (about the axis of the bolt). When any rotations in a 3-D analysis are coupled (a result of the bolt clamping surfaces together) the rotation coupling is generally valid only in a small displacement (geometrically linear) analysis. Large displacement (geometrically nonlinear) analysis introduces an error based on the difference between "sin(theta) and theta" (expressed in radians). If contact surfaces are added between the shells that are bolted together, the coupling of rotation is not needed, but the solution becomes a nonlinear iterative process, taking several times longer. NOTE: Contact surfaces on shell elements have to be defined carefully, so that the correct surfaces (Face 1 or Face 2) of the shell elements are the ones in contact -- shell element orientation may need to be doctored to get this to work.
Another bolt representation is to use a rigid region to link pairs of nodes. Rigid regions in ANSYS assume small displacement (geometrically linear) analysis. The degree of freedom for rotation about the axis of the bolt must be free at one end of the rigid region node pair, for bolt representation. This representation has the advantage that the shells can be positioned properly in space. However, contact surfaces may become desirable, depending on the dimensions of the clamped parts. The ANSYS rigid region (CERIG) couples rotations about global axes, so the axis of the bolt would have to be along one of the global axes for the rotational degree of freedom to be correct. The analyst may do better to use a very stiff beam element, with incomplete nodal DOF coupling at one beam end and shell, and the other beam end attached to the other shell; the rotational degree of freedom about the beam axis is free at the end with the nodal coupling. A beam with arbitrary orientation may require the nodes at the coupled end to have their coordinate system rotated to have the rotational degree of freedom oriented properly (I haven't tried this). The problem of contact surfaces remains. It can be partially addressed by using gap elements at nearby nodes, for which the nodes of the two shell surfaces must be aligned "above" one another, so the gap elements are perpendicular to the two shell surfaces. Note: Gap elements keep their original orientation in a large displacement analysis, and will not be applicable where there is significant rotation. Contact surfaces (with the gap closed) may be needed where there will be large displacement. The previous warning about applying a contact surface to the correct side of a shell element applies.
Note that nodal coupling acts in the coordinate system of the nodes coupled. The nodal coordinates systems of the coupled nodes should, in general, be identical. The ability of nodal coupling to act in the nodal coordinate system means that the user is not restricted to coupling in global coordinate system directions.
Two of the previous bolt representation methods (nodal coupling and rigid region CERIG) are missing the possibility of representing bolt preload. Preload can be implied if a bolted connection is represented with a link or beam element that is capable of "initial strain". In ANSYS these include: Link1 (2-D Spar), Beam3 (2-D Elastic Beam), Beam4 (3-D Elastic Beam), Link8 (3-D Spar), and Link10 (Tension or Compression Only Spar). They must be squeezing surfaces together, which means that either nodal contact elements (gap elements) or surface contact elements must be in use between separated shell element surfaces, or that surface contact elements must be used on the interface between touching 3-D solid elements or touching shell element surfaces.
Other ways to represent bolt preload include:
Temperature setting, interference setting, and setting the "surface normal stiffness" value of surface contact elements in ANSYS must be carefully done to result in the intended preload. Setting the surface normal stiffness value appropriately is nontrivial. The intended preload must exist BEFORE the structure is loaded. An iterative process may help, but be time-consuming. If the bolts are not overloaded when the structure is loaded, the bolt preload will be nearly unchanged when the structure is loaded. Whether any gap or contact element friction coefficient should be included in the model needs to be considered carefully for it can hide or prevent shear loading on the bolts. For conservatism and safety, friction coefficients may need to be zero, so that the bolts take all the load. When postprocessing, loading on bolts should be assessed using established criteria.
My experience has been that if a full 3-D model of a bolted connection (bolt and materials represented with 3-D elements, and contact elements on the surfaces) starts out with the bolt loose and none of the contact elements touching, convergence may be difficult when the solver begins work. Various analyst "cheats" may help, such as moving the bolt or parts so that there is some contact, and/or using some very soft spring stiffness combination elements to keep the model from "flying off into space", when the solver is working to converge.
Warning about Nodal Coupling.Nodal coupling has its uses: one is a quick-and-dirty representation of a bolted or riveted connection with shell elements (see above). More exotic applications can be invented. When nodal coupling is used to represent a bolted connection of 3D shells, the nodes that are coupled must occupy the same position in space. Otherwise, body rotation at that part of the structure will result in an artificial mechanism acting on the structure. If the nodes were tied in the X,Y,Z directions, structure rotation would not result in the necessary change in the relative X,Y,Z positions of the two nodes. High local stresses, and an external couple would result if the coupled nodes were not located at the same position. This is not good!
Development of geometry in which surfaces cut each other with shared lines.The lines must be shared between different areas if the finite elements are to act as if the surfaces are welded together, when meshing takes place. Considerable care and checking is always necessary as a model is built, to see that connectedness is complete. I can still make errors of this type, for they sneak in even when being careful.
Hopefully, a beginning ANSYS user will have had some training in the development of ANSYS solid geometry within /PREP7. New revisions of ANSYS improve the capability of /PREP7, with not all improvements being publicized. I lived with ANSYS 5.0 and 5.1, and much prefer the more recent ANSYS versions. The solid modeling engine does not like singularities, e.g. you can't have a line that cuts half way through an area, the way that you can cut half way into a sheet of paper with a pair of scissors. It is necessary to cut an original area into two areas, in order to get a line that extends into the interior of the original area. Recent ANSYS versions appear to be more tolerant of cusps and some other difficulties. Development of complex structure solid-model geometry with /PREP7 calls on analyst creativity, intelligence, and puzzle-solving skills, as well as a good dose of patience. This tends not to be understood by those who have never done the work.
ANSYS does not assign the attributes (REAL, MAT, TYPE, and ESYS) of a parent geometric entity (Line, Area, or Volume) to the entities that are formed by a Boolean operation such as dividing the original entity into parts. I consider this unfortunate, since it increases the work required of the analyst who is developing the model. It is an easy way to forget to assign attributes.
Application of boundary conditions.Structural FEA displacement boundary conditions are the limitations on movement of the structure at places such as anchor locations. The boundary conditions in a finite element model must limit translation or rotation in a manner appropriate to the case at hand. Boundary conditions can be used to imply symmetric behavior in a structure that has symmetry, so that the model size can be halved, quartered, or similarly reduced, if the loading of the structure is also symmetrical. Boundary conditions can also be used to imply anti-symmetry, for example, where a warping displacement is applied to a symmetric structure (envision twisting a shoebox about the long axis -- a quarter model could be sufficient).
There are occasions when a displacement boundary condition needs to be applied to a single node so that the structure can rotate around the support point. This single node support, however, can result in a serious local stress spike. Depending on the model, the elements where the single node support will be applied might be artificially stiffened. Alternatively, if there is a surrounding "pad", an even pressure could be applied to the pad, that generates a force equal to the reaction otherwise found at the constrained node. Two stress runs could be used: (1) Run without the pressure on the "pad" and find the reaction at the constrained node. (2) Take the reaction, spread it smoothly over the pad as a pressure, and run again. The reaction could be spread over nearby nodes at stiffeners, instead of applied as a pressure, depending on the nature of the model and structure. The goal here is to approximate reality in an acceptable way, while avoiding the time-consuming use of contact and other non-linear elements. (Of course, in some cases, it will be necessary to exactly model a support complete with many non-linear complexities.) NOTE: If you do this, the reaction forces will no longer equal the previous applied load plus gravity load on the structure, because of the new load that has been introduced.
Application of loading in a manner that is of satisfactory accuracy, without becoming overly complex.It is often sufficient to apply forces directly to a small set of nodes. However, better representation of loading can be needed to avoid local stress spikes in some analyses. As discussed above, application of pressure over a region of elements, producing the desired force, can help avoid a local stress spike. Artificially stiffening a local region where a point force is applied can help, if this is acceptable.
The load to consider may need to be increased because of the possibility of dynamic effects, if you are doing only a static analysis. Your industry may have standards for this. Consider road vehicle design -- you wouldn't want the tires to blow out from the increased force due to a vehicle roll-over. (If they did, how would you prove that tire failure did not cause the accident?) This would call for the tires to stand at least twice the "normal max rating" without immediate failure. I once sighted a non-professional driver pulling a simple trailer grossly overloaded with crushed stone. It appeared that the wheel bearings failed before the tires let go (there was a lot of smoke so it was hard to tell). Somebody did good tire design! (Some transportation structures have to be limited in size under the knowlege that users will fill them to the maximum possible volume, without regard to the density and total weight of the material loaded.)
For structures that do not have a severe weight penalty (e.g. those that do not have to fly), getting a conservative result is often satisfactory. An analyst will develop a feel for this as the result of experience in a particular industry. However, where there are high material costs, or large volumes manufactured, extra modeling detail to reduce unjustified conservatism may be economically sound.
Pressure loading of a wall containing granular materialis particularly challenging. Earth, sand, grain, coal, or other granular material pressure is a civil engineering topic. Because of internal friction in the material, the lateral pressure on walls is usually less than simple hydrostatic pressure would be for a liquid of the same average density. For some dry materials, the pressure would be roughly 40 to 60 percent of hydrostatic pressure (look up a proper value) on a vertical wall. The pressure loading varies with the depth of the material, and varies if the slope of a wall changes (a horizontal surface could see hydrostatic pressure). On the other hand, in a long column filled with granular material, the pressure may be constant past a certain depth -- this affects the function of an hourglass. The ANSYS Finite Element program is capable of applying a pressure with a gradient, so pressure can ramp up smoothly as the depth increases. The pressure load must be applied to the correct face of a shell finite element. Considerable FEA checking is needed to assure that the whole structure model is properly loaded. Extra analyst work is needed to apply a series of gradient loads that increase smoothly in intensity if curvature of a wall or container surface causes change of slope. The Rankine formula describes granular material pressure on a vertical wall. Non-vertical sides might require the Coulomb formula to give a higher accuracy representation of how non-vertical slope affects granular material pressure on a wall (go visit a library, plus talk to a civil engineer). Take a look at EJGE/Magazine Feature for more information.
After creating loads that represent a granular material in a container, under a 1.0 g vertical load, the vertical component of the applied pressure should result in a total force that equals the weight of the granular material. It may be desired to scale the granular material pressures so that the total vertical force component under 1.0 g equals the weight of the contained material. This should be checked in reviewing the results of the analysis.
A perfect FEA model of containers (bin, hopper, hold, box, trailer, etc.) loaded by granular material may be impossible. The pressure required to push inward and deform a surface of a granular material is greater than the load with which the granular material pushes outward. This is because of the internal friction in the material. A finite element model of a loaded wall can include pressure on the inside surface that would result from contained material. However, that pressure will not be adjusted according to whether the wall moves inward, or expands outward, as the container deforms under various loads. Since an FEA analysis results in deformation of the walls, exact representation of the pressure loading will be unachievable. I have not been able to find an expert who would say that a granular material nonlinear solid element finite element model can be included inside a shell structure container model in a successful manner, using contact elements on the interface between the solid elements and shell elements (geotechnical engineers should know far more about this than I do). Material properties such as Drucker-Prager are included in ANSYS and some other FEA packages, but I don't know if they are applicable to this type of structure and granular material modeling. ANSYS manuals discuss this material option briefly. An engineer often settles for a model and design thought to be conservative or adequate, given industry experience. The worrying starts when a design departs significantly from previous practice.
Deformation of thin flat panels by pressure loading causes the panels to curve.When flat panels are loaded on one of their surfaces, the panels curve, then start to carry applied loading with membrane forces. The only way in which this can be represented is to activate large displacement (geometrically nonlinear) analysis. A rule of thumb is that membrane forces begin to be significant when the out-of-plane deflection exceeds half the thickness of the panel. Nonlinear analysis requires considerable experience, because of the difficulty in achieving converged solutions. Failure to use nonlinear analysis where it is appropriate can result in considerable ignorance of the real structural mechanics involved. Nonlinear analysis becomes very time consuming because of the iterative solutions needed. Fast computers are very desirable when doing this kind of work with a large model. Failure to consider that significant out-of-plane deflection can result during nonlinear analysis can, in some cases, lead to inadequate designs. In other cases, the curvature can lead to significant increases in strength of the structure. The designer needs to be aware of the need to include nonlinear effects in some work.
Use of Units.Vibration and transient analysis require that the mass of the structure be entered in units consistent with the other units in the model. Some North American industries normally work in inches-pounds-seconds. This requires that mass be represented as pounds/in/sec^2. Pounds here means "pounds force", the force with which 1.0 g of gravity pulls on the mass. This means dividing the weight in "pounds force", or the density in pounds/in^3, by the number 386.1 (more accurate than 32.2*12=386.4), which is the acceleration due to gravity expressed in inches per second squared (in/sec^2). In consequence, when mass and mass density have been defined this way (the density of steel, which depends on the alloy, if given as 0.2836 lb/in^3 would be entered into ANSYS as 0.0007345) it is necessary to enter 1.0 g of gravity as 386.1 in/sec^2 to let ANSYS apply the correct force due to gravity on the structure. Loads will be entered in pounds. Pressures and stresses will be referred to as pounds per square inch. ANSYS refers to these units as "BIN" (see the /UNITS command for "British system using inches", noting that the /UNITS command is for annotation of the database, and has no effect on the analysis or data).
In the metric world, fundamental units are meters-kilograms-seconds. However, in engineering work, analysts often use millimeters-kilograms-seconds. Forces are expressed in Newtons (1 Newton accelerates 1 kilogram at 1 meter per second squared). Pressure is Newtons per square meter (1 Newton/Meter^2 = 1 Pascal). A pressure of 1 Newton per square millimeter is referred to as 1 megapascal. When working in millimeters-kilograms-seconds, it is common to refer to pressures, stresses, and Young's modulus in megapascals or kilopascals. Acceleration due to gravity is 9.807 meters/sec^2, or 9807 mm/sec^2.
ANSYS does not care what units are used, nor does it issue warnings. The analyst must be consistent in the set of units in one model, to avoid errors. Getting the mass and mass density into the correct units is particularly important if any form of vibration, transient, or transient heat transfer work will be done. Tip: Check the values for typical materials in the ANSYS material library as a guide, even if you do not use these exact materials. A comparison will indicate if your values are in the right range. The ANSYS materials library includes material values in various systems of units. Many design codes will, for example, give densities in lb/in^3, where pounds is actually the weight expressed as "pounds force". This Imperial value cannot be used directly for vibration and transient work, and must be converted. (When I try to explain this to non-North American people, and even recent Canadian graduates, they think the whole Imperial units business is insane -- I can't blame them.)
The usual question on Imperial units is, "Why can't I enter density for steel as 0.2836 and 1.0 g of gravity as 1.0 ?" The answer is, "This would work for gravity loading on a structure, but if you ever do vibration or transient analysis on the same model in the future, your answer will be garbage." My own policy is to always use the "correct" units, similar to those that the ANSYS material library supplies for the BIN system, in case vibration or other work is done in future.
If densities have been entered "correctly" in Imperial units (e.g. 0.2836/386.1=0.0007345 for steel), then when ANSYS reports the "mass" of the model during the SOLVE process, that mass will have to be multiplied by "g" (386.1 in this example) to recover the weight of the model in "pounds force".
Buckling analysis and failurecan be pursued in two ways: Linear eigenvalue buckling, and geometrically nonlinear (Large Displacement) buckling analysis. Eigenvalue buckling (also known as Euler buckling or classical buckling) will be sufficient for some structures, but much greater detail about stress amplification and margin of safety can be found with geometrically nonlinear analysis. Note that margin of safety is not a simple concept in a nonlinear analysis. The margin of safety will be based on the difference between the intended design load and either the load that reaches failure conditions or the load that exceeds allowables set by design codes. The relationship between loading and consequent stress and deflection cannot be extrapolated linearly when a nonlinear analysis is used, or when it is needed. Design codes may address this concept with reference to combined compression and bending of beams, but many codes were written before the availability of nonlinear finite element analysis, so the analyst will need to comprehend the intent of the design code and interpret it, if this is permissible.
A difficulty here is to establish what level of loading has reached "failure" conditions. If the structure starts to buckle in a Large Displacement analysis, solution convergence will become slow, as the load is ramped up. The fact that the FEA solution stops converging at some level does not guarantee that the failure load has been reached -- it could be just a numerical analysis difficulty. The Arc-length method is useful here, since it will follow the load up and back down as the load/deflection curve first rises and then falls. An advantage to Large Displacement, Plastic material property analysis is that the failure can be followed in detail (if the model is small, or the computer is very fast). Defining margin of safety still requires a human decision as to what load "reaches" unacceptable stress and deflection, before complete collapse happens. Simply basing margin of safety on the highest load reached in a plastic, Large Deflection, Arc-length analysis would not satisfy the rules in most design codes, and usually not make good engineering sense.
A problem with eigenvalue analysis of some structures is that localized "popping" of panels or other components happens long before the whole structure begins to fail via buckling induced deformation. The problem with geometrically nonlinear analysis of the same structure and loading is that convergence troubles may make analysis exceedingly difficult and/or time consuming. This is particularly true when applied force is ramped up. Convergence of applied displacement is more successful in nonlinear studies, but applied displacement is not the most common way in which loads are analyzed. A possible advantage of a geometrically nonlinear Large Displacement run is that if convergence of the model is achieved, it may sometimes be shown that the structure will handle a load considerably greater than the first several eigenvalue buckling loads, without exceeding yield, or allowable stress, or undergoing deflection significant enough to merit concern. A geometrically nonlinear analysis with loads that exceed the eigenvalue buckling level should have loading ramped up, with substep information saved in fine detail. The substep results should be examined carefully to see whether sudden changes in the stress or deflection patterns develop. With a shell model, this should be done for both mid-plane and surface (use Powergraphics) stresses and for deflection plots. The ability of the ANSYS program to generate an animation file from the set of substep results is helpful here. Deflection can be set 1:1 or exaggerated using the /DSCALE command.
Ramping Loads in ANSYS.Loads are ramped up if the appropriate settings are used for time stepping. The fun starts when the user tries to ramp the loads back down (as when wanting to find the permanent deformation that results from plastic deformation). If the loads are deleted, there is nothing to ramp down to, the force drops immediately to zero, and convergence may be a problem. One solution is to reduce forces and pressures to an extremely small number. Another problem is that if the loading has been applied to geometric entities, it cannot be scaled down directly, for ANSYS lacks commands to do this.
An unsatisfactory but adequate fix is to transfer the loading to the nodes and elements, then delete the relationship between geometric entities using the MODMSH,DETA command from /PREP7 (Warning: make sure your model is saved before doing this -- MODMSH ruins the connection between your geometry and your FEA mesh), then scale down the loading on the nodes and elements. If you merely scale down the loading on the nodes and elements, it will be replaced by the loading on the geometric entities when the SOLVE command is executed.
A more satisfactory way to ramp loads that were originally applied to geometric entities will be to write and read load step files. The full loading on the geometric entities can be transferred to the elements, then a load step file written. The load step file includes pressures on elements, not information about loading on geometric entities. Then, the loading on geometric entities can be deleted. Next, the load step file can be read, bringing back in the pressures on the elements. Finally, that loading can be scaled down to an extremely small number. This method works in general for keeping the loading that geometric entities transferred to elements and nodes, while discarding the original assignment of loading to geometry, and so can be quite convenient.
Plotting resultscan show the stresses in the structure with colored contour maps. Plotting with stresses averaged at nodes (PLNSOL) results in smoother cleaner contours that are easier to study, and that tend to average out stress fluctuations due to local variations in element shape. However, such plots have the disadvantage that they average stresses at shell intersections (at corners, "Tee" intersections, thickness discontinuities, and material changes, for example). This results in considerable loss of information, and masking of high stress areas in some models. Either element stress plots with no nodal averaging must be used when this matters (PLESOL), or element selection must be limited to continuous panels of material, so that the averaging is not performed where it is not appropriate. This is a very common error in the reporting of results from shell models (and solid models with material type changes). I have seen stresses hidden that would cause fatigue troubles, because of nodal stress averaging with shell FEA models. In addition, fatigue-causing stresses often need to be shown at shell surfaces, not just at the mid-plane, so both mid-plane and surface stress plotting will often be required for complete model evaluation. In a complex model, components may need to be examined from a number of viewing angles, and with cutting planes, in order to inspect the stresses everywhere.
ANSYS has introduced its "Powergraphics" setting that can show VISIBLE SURFACE shell stresses with discontinuity at intersections, and changes in REAL and MATerial (see the AVRES command). However, a user often wants stress at the shell mid-plane. ANSYS keeps track of the surface stresses in its database, and calculates the mid-plane average when needed. I have written a macro that will move the mid-plane stress for each node of each shell element, element-by-element, to the top and bottom surfaces, so that the Powergraphics setting can show mid-plane shell stress with discontinuities and intersections. The problem with the macro is that it executes VERY slowly -- it was about two seconds per SHELL 63 element on a Pentium-Pro 180 under Windows NT in a 70,000 DOF model, taking 7 hours to process one load case. Surrounding macro executable lines with /NOPR and /GOPR speeded up the process by roughly a factor of 3. The database is permanently modified by this macro, so the analysis results database must be stored on disk BEFORE this macro is used. It must be used with caution.
The ANSYS contour map colors can be customized. I set them to shades of gray when I want to plot to a black-and-white laser printer (directly from ANSYS, not the DISPLAY program). The contour levels can be set automated to be evenly applied (default), or can be set by the user. I sometimes set all levels but the "red" contour to be evenly spread out up to the material yield, or the allowable stress, and let red color the region above. I wrote a macro to automate this, using the *GET command to find the max and min stresses, in order to calculate the custom levels. The macro has to be re-applied every time stresses are plotted for new elements, or for a different stress plot type. The automatic contour level mode should be returned to when done.
Shell mid-plane stresses are often preferred for review of structures. There are also good reasons to review shell surface stresses. They include checks on: direct shell bending, torque causing torsion stress in open sections, plastic hinge development and the onset of plastic failure, local stress concentrations, locations for possible fatigue or fracture, non-linear buckling, stresses from design errors or modeling errors, and prying loads. Torsion on an open section can cause substantial shell surface stresses at shell intersections such as corners -- an invitation to fatigue failure, fracture, or possible structure collapse. This phenomenon will be completely overlooked if only mid-plane stresses are plotted.
In limited testing I did, ANSYS gave me surprisingly good values for surface stress caused by torque applied to open sections modeled with shell elements. (I created equivalent solid models with a few solid elements through the wall thickness for the comparison runs that gave the "real" answer.) Mid-plane stress plots don't hint that torsional load is causing high shell stress on the surfaces of open sections. I wouldn't extrapolate my test result to any structure, but it suggests that shell surface stress plots will help to detect a class of design problems (shortcomings) that mid-plane stress plots will miss. ANSYS PowerGraphics plotting helps considerably.
Coping with Design Changes.A fun topic! The analyst must be able to modify existing models. The ability to do this can be enhanced if the model has been planned for later modification (see parametric design comments below). The commands that move keypoints can help a little... the keypoint moves will destroy curved lines, and only work if affected areas are not severely distorted, and topology does not try to change. KEEPING THE GEOMETRY on which the mesh was based is an important part of being able to do significant future modifications of models. It is easier to move a set of nodes than a set of keypoints, so under rare circumstances the elimination of geometry may be desired (nodes cannot be moved while they attached to underlying geometry; see the MODMSH command but do not use it without knowing exactly what you are doing). However, any substantial model changes become very difficult when only elements and nodes are available.
Computer Aided Engineering Environment.I often develop finite element models the "hard" way: Generate all the geometry from scratch in the pre-processor of ANSYS. For existing designs, I may get copies of a few dozen drawings, sometimes scaling dimensions off the drawings (I did say finite element analysis is approximate) when the dimensions are not explicit on the drawings (I don't like this). I adjust the position of parts in space to achieve a good mid-plane representation of steel sheets for shell element development. Adjustments and modeling tricks are used to approximate some connections of thick parts and of bolted parts. For a complex model it can become very time consuming to modify a model's fundamental dimensions after model development has progressed significantly. This makes exploration of cost-saving alternatives difficult on a tight time schedule (what other kind of time schedule is there?), even though significant money might be at stake. Significant money is involved with expensive structures, weight penalties, high-volume production, and with failures.
There exist CAD systems that can link the 3-dimensional CAD model to a complex shell finite element model (e.g. Pro/Engineer and SDRC IDEAS, probably others as progress is made). The CAD models can be parametrically defined so that overall dimensions can be updated quickly with all associated part and assembly prints, and the bill of materials being automatically updated, as well as the finite element model. This can make exploration of design alternatives much more sophisticated. Otherwise, the analyst may be limited to exploring shell thickness alternatives, and development of ANSYS models parametrically, so that the ANSYS log files can be re-run with different fundamental dimensions. Such a finite element model "program" requires careful planning and experience.
FEA versus Hand Calculations.This issue comes up when a new design needs to be configured. The "first cut" at a design must start with the invention of a configuration that supports the applied loads, and carries these loads to the support points of a structure. A variety of loads usually need to be supported, and structural details must be present that will handle each kind of load in a manner that is acceptable for the type of structure being considered (e.g. welded steel structures, bolted, pipes and pressure vessels, and others). The initial layout of the components of the structure, and the initial sizing of the parts has to begin with manual calculations.
Several concerns arise in the initial configuration, such as:
Given an initial structural concept, an FEA model can be created. If the model is only of moderate complexity, the geometry for the FEA model can be created parametrically, so that the log file can be reused in the future to regenerate the design with different dimensional values. This will require that there be no changes in the topology of the structure (e.g. varying the number of stiffeners, or shortening a part until it no longer meets another part) or else the parametric approach must include means to accommodate these changes. If the model is complex, it may not be feasible to create the geometry parametrically, and the finite element model will be created with exact dimensions entered numerically. During the finite element analyses that follow, the thicknesses of shells or beams can be varied in order to investigate the possibility of weight savings and cost reduction. The FEA package can be used to investigate stress, deflection, buckling, vibration, and nonlinear effects if these matter. Properly interpreted results will show where the structure is overdesigned, underdesigned, or if it has significant inadequate design details (e.g. complete lack of stiffeners where they are needed) and needs modification. Design sensitivity can be assessed with respect to variations in some dimensions. Optimization may be possible if time and sufficient skill are available.
Given modern CAD software, a parametric model can be built in the CAD system. An FEA model can be derived from the CAD model such that updating the CAD model leads to updating of the FEA model. This makes the modify-and-assess design loop much more effective and can lead to significant cost savings. Progress with development and deployment of these CAD systems continues.
Choosing an Appropriate Shell Element.There are several shell elements types available under ANSYS. The usual workhorse shell element is Shell63, a 4-node shell element. This element supports large displacement, but not plastic material properties. (If plastic material properties have been entered, they will be ignored by Shell63.) If your element type 1 was Shell63, you can directly enter (by hand) a command like "ET,1,181" to convert the elements to Shell181, which has plastic capability. You may want to modify the KEYOPT values after this command. Note that the effect of stress stiffening is activated with shell elements like Shell63 by adjusting one of the KEYOPT values for this element. Other 4-node elements that are capable of plasticity include Shell43, Shell143, and Shell181.
I have recently found Shell93, an 8-node shell element, to give satisfactory results for a problem I ran. This element is capable of plasticity (ANSYS manuals note that lower order elements (4-node in this case) may be preferred for nonlinear and plastic analysis), in addition to large displacement, so it gives "one size fits all" service. The advantage to this element is that mesh density does not have to be as great, and it follows curved surfaces very well, since it is a curved element. (4-node shell elements are flat, and any significant warping of their shape during meshing will cause the FEA program to complain, and presumably give degraded results.) Some user work is required with mid-side node elements, because they do not want to curve too much. Meshing an area fillet has to be carefully controlled. To change a model with 4-node elements, to 8-node elements with mid-side nodes, the usual thing to do would be to clear elements and re-mesh, after possibly modifying mesh density. Stress stiffening is activated for Shell93 in the Solution part of ANSYS, not by setting a KEYOPT value as with Shell63.
Using P-Elements.The use of P-elements can reduce the effort required to mesh models. The user is cautioned that the P-elements do not support large displacement or plasticity.
Harmonic Response.This is what ANSYS calls Steady State Frequency Response to constant harmonic input (an input forcing frequency that is sinusoidal steady state). There are three ways available in ANSYS: full, reduced, and modal. A damping ratio can be input using the DMPRAT command. The output is complex numbers that imply amplitude and phase. The phase differs from the phase of the input if the input is not at an eigenfrequency. Only the reduced and modal methods can handle stress stiffening. The /POST26 Time History postprocessor can plot amplitude for a node versus frequency (see the PLCPLX key value); the /POST1 postprocessor can use the SET command to load either the Real or the Imaginary component, but not both. The manuals say that the /POST26 postprocessor can do things with the components. As with all vibration and transient analyses, the units of mass must be input appropriately.
Failure Modes to Consider.Textbooks are written on this topic. There are many things an analyst may overlook. Just a few of the many things to think and worry about include:
Please send me your favorites, to add to this list of failure modes, as they relate to inadequacies and oversights in FEA.
Stress Limits and Margin of Safety.Two possible approaches to margin of safety are: (1) Amplify the loading, e.g. to twice the maximum static applied load (or far more with many civil engineering and other structures), and use the lesser of material yield or a fraction of ultimate tensile stress as the allowable limit, or, (2) Use the maximum static applied load, and the lesser of a fraction of material yield or a smaller fraction of ultimate tensile stress. The approach will depend on the industry and the codes followed; some industries may differ. Other factors may bear, e.g. stress allowables may be reduced by temperature and by high temperature creep considerations. Other considerations will be different allowables for thermal stresses, "secondary displacement-driven" stresses, and checks on vibration characteristics, buckling, fatigue, etc.
I noticed some recent discussion on ASME changes in the fraction of ultimate tensile stress (UTS) to be applied to some pressure vessel materials (some carbon and low alloy steels below creep temperatures in Section VIII, Div.1). The UTS fraction settings were said to put some ASME regulated designs at a competitive disadvantage on the world market. Steel producers note that the quality and uniformity of their steel is much better than two or three decades ago. Still, I have seen new steel plate that had laminar cracks more than a foot in size (roughly half a meter), and a spring that had a crack along the length of the wire from which it was produced. QC checking and conservative designs will not go away any time soon.
In discussing nonlinear material properties in these web pages, I am usually referring to checking for structure failure when loading leads to stresses that exceed material yield over regions of questionable size. This will usually NOT be strictly according to the rules laid out in design codes, but is added as a check that the intent of codes and safety needs are considered under severe or unusual loading, or under loading that is important but not included in codes. Some design codes have rules for "elastic-plastic" analysis, or for "fully plastic" analysis, which would have to be studied and applied during design and analysis.
Representation of a group of bolts (or rivets).A single bolt might be represented in an FEA model as preventing motion in the X, Y, and Z directions, as well as rotations, except rotation about the axis of the bolt. Contact elements may be wanted between the layers that are bolted together, at the expense of much slower solution. Friction with these contact elements might or might not be considered, depending on whether bolt preload or initial interference was included, and on whether it was acceptable to let friction carry any of the "in-plane" load -- it may be important or necessary (per codes or for safety) to let the bolts carry all the "in-plane" load, setting the contact element friction coefficient to zero. Because of looseness of fit, tolerancing of bolt diameter, and of hole position, diameter and alignment, not all bolts will act simultaneously when a real structure is loaded up. This would be true of structural tension, compression, and shear forces that produce shear forces in the bolts, and of moment applied to a "bolt circle." It may be decided in FEA to represent all bolts as being "tight" for the purpose of analysis. Note, this can introduce a problem: In the FEA model, the structural members undergo strain when they carry loads. Where members are bolted together, the overall structural strain will create high local forces as the bolts try to make one bolted member's strain match the other bolted member's strain. This makes the FEA report very high forces on the individual bolts, much of which may not be due to load path forces being transferred through the bolts.
I can't think of a simple way out of this dilemma. Your firm or industry may have "standard" ways of dealing with this analysis. It might be decided to average the reported forces acting on the full group of bolts for tension forces, and to use the standard analytical approaches to force on a group of bolts, and to a bolt circle with net moment on the group of bolts. If there is no significant load path force in one direction, some of the bolts could be modeled as "loose" in this direction. An alternative, possibly conservative, approach would be to consider a minimum number of bolts and directions of bolt action, to be acting to resist forces and moments, although this could result in FEA reporting overloaded bolts and high local stresses if the bolts are on the primary load path. (Usually, all the bolts should be "tight" in the direction in which they pull the joined materials together (the bolt axis direction).) The load on this reduced number of bolts could be considered to be spread over the group of bolts, and analyzed manually. In general, the user will want to consult codes and standards used in the appropriate industry, understand the concepts used in bolting, and discuss with people with expertise. It wouldn't hurt to review standard textbooks. Remember to avoid significant prying loads on bolts, rivets, welds, and other fasteners.
The presence of a bolt or group of bolts means that the crossectional area of the bolted materials is reduced by the presence of the bolt holes. If the holes are not represented in the finite element model, the analyst needs to do extra work to examine the stress in the zone of the bolt holes, using codes, standards, and good judgment to find the allowable net stress, bearing force, and total force in that zone.
Adequate Computer Hardware for FEA.I once heard of a product failing when highly loaded. An FEA analyst had limited modeling to a coarse FEA mesh with small-displacement elastic analysis, and plotted nodal averaged stresses, on an underpowered older computer. Proper computer equipment, some staff training, a finer mesh, nonlinear analysis (large displacement and material plasticity), and more thorough post-processing of results (PowerGraphics plots of shell element midplane and surface stresses) could have detected a structural weakness. Prevention would have been easier than modification. Such is life.
In an ideal world, adequate computer hardware would only rarely be an FEA modeling issue. A company may save thousands of dollars by using inadequate FEA hardware, and lose significantly more as a result. Computer hardware affects the mesh density possible in FEA models, the time to develop FEA models, to run solutions, and to save, process, review, and plot the results. Time saved by using better hardware makes it possible to use better resolution in a model when it matters, to take analyst "short cuts" that save model development time but increase computational expense, to check for errors, to check effects such as large displacement buckling and plastic deformation, to check unusual loadings, and to vary a design in attempts to reduce weight and costs. Convincing management of this can be another matter. A few thousand dollars not spent on computing hardware is a visible "saving". X million dollars in design errors that could be prevented remain hypothetical until they happen. Y million dollars in cost reductions also remain only a daydream if not proven in a non-rigged demonstration. In practice, funding for the computer hardware is often set by people who are either unfamiliar with FEA and engineering, or who have noticed that the analysis detail sometimes expands to fill the available computing capacity. (How's that for a euphemism?) When analysts living with deadlines spend an unacceptable amount of time waiting on computer hardware while performing FEA work, significant differences of opinion about computer hardware can develop between analysts and management. Analysts have been known to change employers over this issue.
Given the price of the ANSYS software, a computer costing only a fraction of the software cost can do a very substantial amount of analysis work given present (2004) hardware costs. In the Windows XP world, a few thousand U.S. dollars will purchase a computer with large RAM (2 GB or 4 GB), large hard drive (60 Gig or more), fast processor (2.4 or more GHz), cheap laser printer, colored ink-jet printer, 17" or larger monitor, graphics card with 32 Mbytes or more of RAM, and an adequate backup device -- a CD or DVD burner is often employed. A budget of several thousand dollars will allow a PC with a 2 CPU motherboard, 4 GB RAM, change the hard drive to a fast version of SCSI, monitor to a 21" CRT or a 19" to 21" LCD, and graphics card to an ANSYS tested powerful OpenGL card. Large budgets take the purchaser into the world of very fast Windows or UNIX machines with 64-bit operating systems and multiple processors. (My comments here will gradually become out of date.)
Hard drives have become very cheap. In FEA work, a hard drive should be able to store a significant amount of work-in-progress and recent completed work, with additional capacity to handle ANSYS solver temporary files for large models, including substantial results file storage. I can't say it with authority, but I have the impression that a SCSI hard drive will transfer information with less interruption of operation of the computer, for disk-intensive aspects of FEA work (e.g. working from an input file, and using the frontal solver on very large jobs). I have heard that having two SCSI drives, one for the operating system including the virtual memory swap file, and one for the model being run, can improve some FEA operations. I suspect that the money could be better spent on a larger RAM or dual-processor machine.
RAM is currently very cheap. A large RAM will permit larger models to be run with the SPARSE and PCG solvers in ANSYS; for this reason some companies have PC machines with 2 GB or 4 GB of RAM -- this will depend on your work. Models too large for a 32-bit operating system with the any solver will require a move to a 64-bit operating system and RAM larger than 4 GBytes. A large RAM will help your solutions work quietly in the background, with little swap file disk thrashing. Your ANSYS vendor can probably advise on high-end equipment.
FEA work is one of the numerically intensive applications that justifies the extra expense of a very fast processor. The availability of drivers for your operating system should also be checked before the purchase of extras.
I have found both 17" and 21" monitors to be sufficient for FEA modeling. Make sure that the cheapest monitor purchased supports at least refresh rates of 70 Hz or higher at resolutions of 1024 x 768 pixels or higher. Make sure that the graphics card matches or exceeds the monitor's resolution and refresh rates. A CRT monitor refresh rate lower than 70 Hz will cause the eye to perceive flicker of the image, and cause eye strain. Informed people prefer 75 Hz or more. Many PC computers are delivered running their monitors at a refresh rate of 60 Hz, and have to be properly set up by the end user. (I've known people who went to the optometrist because the computer screen was bothering their eyes. All that was wrong was that the refresh rate was at 60 Hz. The optometrist didn't know about this phenomenon or its fix.) I currently use a 17" LCD monitor at 1280 x 1024, so the refresh rate is not relevant for static images (60 Hz works with this LCD monitor and this display device does not flicker), but if using a CRT monitor, I would prefer that it be set to 1280 x 1024 pixels running at 85 Hz. A new monitor should support a resolution of at least 1280 x 1024 pixels at 75 Hz or higher, as should any decent modern graphics card. Today's graphics cards are cheap enough that this resolution should be supported with 24-bit color. The OpenGL cards that ANSYS suggests should result in much faster model graphics display. With large models, this should be a helpful investment.
Printers can be relatively inexpensive, although you can run up fairly high bills for colored ink if you generate large numbers of plots. A laser printer can be a fast inexpensive way to get black-and-white listings and plots during FEA work and report writing. I keep both a gray-scaled and a colored ANSYS color map on my toolbar to move quickly between black-and-white and color. A substantial amount of work can be done cheaply with gray-scaled plot prints, prior to developing a final report with color images. A color ink-jet printer is the least expensive way to get helpful colored plots. If a larger budget is available, consider an ink-jet that generates 11" x 17" plots, or a colored laser printer for high-volume high-priced work. In some companies the speed-up in analysis work will pay for the equipment in short order.
Top of Page
Return to Main Page
FEA and Optimization Introduction Page
ANSYS® Tips Page
© 1998 by Peter C. Budgell -- You are welcome to print and photocopy these pages (don't plagiarize or sell the contents).
E-mail Address: Please see my main page.
October 22, 1998; minor update in January 2004.
Link to: The ANSYS® Home Page at www.ansys.com
For more links, Return to Main Page.