Home

Management and Quality

Expertise

Contact Us

YOU ARE HERE: Home >> Analysis Basics >> FEA in Practice

Legal Statement

Theory and practice of FEA

FEA in Practice

This is the second page in the Technical Resources section on the ‘Introduction to FEA’, and is concerned with the theory and practice of basic FEA. Click here to go to the first page, which also has links to other FEA resources.

We are able to advise on best practice in developing your analysis strategies. Contact us if you are unsure about the best way to formulate a particular analysis problem.

Additional Sources of Information

The amazon website sells many titles on Finite Element Analysis. A good book giving practical tips on basic analysis is:

Building Better Products with Finite Element Analysis  
Vince Adams, Abraham Askenazi

 Follow this link to view this book at Amazon:

Building Better Products with Finite...

Theory and Practice of FEA

CAD Import Issues

It is usually sensible to generate a finite element model starting from a CAD model. Some of the issues that affect this are discussed below.

Transferring a model is strongly dependant on the organisation's CAD strategy. Some CAD and FEA packages are designed to work together, which can simplify the process. Cultural issues, i.e. the work practices of the design and analysis teams within an organisation, can raise issues when transferring models. For example: assigning additional write access for CAD models; and how and by whom the model should be transferred. In general, communication between CAD and analysis packages has become easier in recent years due to efforts from software companies in better standardisation of the file types (e.g. IGES or STEP) and import functions.

Traditionally, the model is imported into a finite element pre-processor. This can create the mesh, assign material properties, loads and constraints to the model. The pre-processor will have meshing capabilities to generate an automesh within the solid. This process is rarely straightforward however and further geometry modification from within the pre-processor will usually be required before it is possible to generate an automesh. The geometry will tend to have a number of problems like, for example, the presence of short lines or small areas causing very small elements to be created; acute angles causing very distorted elements; or discontinuous geometry preventing a solid from being formed. This latter problem often occurs and is sometimes caused by different tolerances between the CAD system and the pre-processor. Software tools such as CADfix (www.cadfix.com) can be used to resolve this problem.

An alternative for simple models often used by more experienced analysts and meshers is to generate the model from scratch in the finite element pre-processor, or to undertake modifications entirely in the pre-processor, having read in an unmodified solid from the source modeller. This approach is discussed further in the section ‘Mesh Generation’.

Modelling Strategy

Back to Top

The following sections describe the considerations to be borne in mind when deciding on the best form for the model.

Model Type - Two or Three Dimensional

A two-dimensional model will represent a substantial time saving over a three dimensional one: both run time and results interpretation time. In some cases a 2D model will give adequate results in its own right, and in others it will provide insights and a useful benchmark for checking a later 3D model. See the discussion of 2D element types.

Geometry

Consider if some of a component's features can be omitted from the model. Features away from load paths will have diminishing significance, as they will have lower stresses and less effect on other areas (St Venant's Principle.) Features directly in the load path however, even slight stress raisers, should be modelled in these critical regions. Determining where the load paths are may not be easy.

Back to Top

Symmetry Conditions

Decisions regarding whether symmetry conditions would allow a cyclic sector to be modelled or a reflected half or quarter of the full model also have to be made. If a symmetric model is used, it is not always obvious how to apply the restraints or loads, especially if the enigmatic 'anti-symmetry' is used and reference to a good textbook or a similar model will be useful.

Back to Top

Loads

The representation of loads can be a difficult one for many analyses. For example, local loads such as bolt or bracket forces can be considered as simple point loads if the area of interest is away from the load application points. Conversely, if these are thought to be critical stress areas, the accurate representation of all forces in such areas will be important.

Back to Top

The representation of bolt loads is a good example of a relatively simple physical situation that requires considerable thought when created in a finite element model. Local effects such as local radial loads arising from the bolt preload being reacted on the threads to the determination of bolt slip have to be considered when modelling and assessing such a joint. Similarly, the contact stresses around the bolt head, nut and between pairs of bolted parts may be important in joints with high or unusual loads: representing this accurately in FEA will require much extra thought, modelling and machine resource.

Back to Top

It is worth remembering that loads can be split up and do not have to be applied to the model in one loadcase' Creating different loadcases is a useful way to improve understanding of the problem where different types, directions or locations of load are applied to the same model, and usually have a negligible effect on run times. This adds flexibility so that loads can be summed factored, and combined to reproduce the original loadcase or variants thereof.

In static analysis, the loads that can be applied can be split into:

• Point loads applied to a node

• Pressure loads applied to an element face

• Body loads (such as gravity or acceleration), applied to element centres of gravity

These are applied in the pre-processor, usually to geometry if it exists. The pre-processor transfers the loads automatically to the relevant finite element entities at the start of the solution.

Back to Top

Restraints and Constraints

Restraints can cause problems because they can impair local stress accuracy. Theoretically, the stresses everywhere in a finite element model should be converging to the correct values. However, two examples follow of difficulties associated with assigning restraints:

1. Restraints all lying on a plane but fixing a direction normal to the plane effectively ensure this plane cannot deform in the area of the constraints. This may not be what is desired.

2. In assigning constraints to the system, one should ensure that no rigid body motion could occur, meaning there will be gross uniform deflection without deformation under the action of a load that tends to give very large displacements in some directions. Even if there appear to be sensible stresses, the very large displacements will indicate a poorly conditioned matrix that can produce either erroneous or inaccurate results. It is not always easy to remove all rigid body freedoms in the model without introducing over constraint that can damage stress accuracy.

Displacement boundary conditions are called constraints. Zero displacement boundary conditions (usually termed restraints) are usually required in any static analysis but sometimes, non-zero displacements are also specified, in what is often called displacement controlled loading. Although they specify a non-zero displacement, they eliminate rigid body displacements in the same way as restraints do.


Back to Top

Types of Finite Elements

There are several types of specialist elements, for example to model unusual constraint situations or to represent cracks, but only the 'continuum' types will be considered here; these are usually categorised according to the geometry they represent; namely 1D, 2D and 3D:

Back to Top

One-dimensional elements

'Rod' or 'tie-bar' elements are the names given to one dimensional elements which cannot sustain bending. They might be used for example to represent tie rods which cannot transmit bending at their ends due to a pinned fixing.

Be cautious of one important issue when using bar or truss elements which is worth mentioning because if nothing else, it helps illustrate a limitation of small displacement theory. If two truss elements are connected end to end, as shown below, then their stiffness in the vertical direction is zero. Any vertical load is sustained by the rods moving out of line and sustaining the load through tension in the rods. Small displacement theory will not update the geometry however as a result of the load application and so the vertical load will have no tensioning effect. This analysis will give no results unless large displacements are considered. See 'Non Linearity and Buckling'





'Beam' elements can sustain bending as well as axial loads; they can be used to model beam like parts of a structure but cannot represent local stress effects, where for example, a bracket is welded to the beam.

Back to Top

Two-dimensional elements for 2D analysis

These include plane strain, plane stress and axi-symmetric elements. They are all plane (i.e. flat) elements and are meaningless unless used in a two dimensional analysis, where the loads perpendicular to the plane of the 2D model are dependant and derived during the analysis, from the loads in the plane.

Back to Top

Two-dimensional elements for 3D analysis

These are not interchangeable with the elements for 2D analysis. They are used to model shell like structures, which can be curved in two directions. There are many different formulations, often grouped into two different types, namely thin shell and thick shell elements. Thin shell elements do not model through thickness shear, i.e. no variation in membrane stress through the thickness. They are suitable for modelling most shell structures however. Thick shell elements can represent through thickness shear and should be used where this may be significant. Thin shell-like structures (such as balloons or pressure accumulators) have very low stiffness normal to the plane of the shell; a strip of balloon material will have no noticeable bending (out of plane) stiffness but will have significant tensile stiffness.

The way in which an inflated balloon resists a normal load (such as a finger prodding it) is obviously not due to the bending stiffness of the material therefore. It is in fact due to the internal pressure that resists the load. Problems like this would require a non linear solution in a similar way to the rods problem discussed above. In this case however, as well as the geometry being updated during the analysis, the line of action of the forces would have to be recalculated as described in the 'Non Linearity and Buckling' section, for an accurate prediction of the deformation.

Back to Top

Three-dimensional elements

These are used for most general modelling problems. They can be linear or parabolic, tetrahedral or hexahedral (more commonly called bricks).

Element Order

Parabolic elements have mid-side nodes and can conform to a curved boundary. They will represent a parabolic (i.e. second order) displacement field through their volume and, since stress is proportional to strain, which is the derivative of displacement, this means that they can represent a linear stress field. Linear elements have no midside nodes and can only have straight edges. They model a linear displacement field and therefore a constant stress field through their length. Except in the case of contact analysis (where they there are unusual numerical problems) parabolic elements are more efficient than linear ones: for the same number of nodes in a model region, a parabolic mesh will have better accuracy. Their ability to represent curved boundaries also means that they will avoid most physical boundary approximations that the straight sided linear elements will make.

Be cautious of applying loads to parabolic element nodes directly. It is incorrect to represent uniformly distributed loads on a parabolic element by distributing the load uniformly over each node of the element. This sounds counter-intuitive, but is an important accuracy issue, the reasons for which will not be discussed here. The best procedure is to apply the loads using geometry in the pre-processor.

Shell or beam like parts or regions within a solid model can be represented by three dimensional elements but in order to have reasonable aspect ratios, very small elements (compared to other elements in the model) might be required and use of appropriate one or two dimensional elements might be preferable to model these parts.

Back to Top

H-Element methods

There are two different approaches to FEA: h-method and p-method. The h-method is the method used by most packages and despite increases in the popularity of Pro-Mechanica and other p-method approaches, the much greater majority of analysis is still achieved with the h-method. In the p-element method, a much coarser mesh can be used since each element has internal refinement, meaning the accuracy of elements is improved automatically during the analysis, along edges where stresses are high. Despite this automatic process, areas of the model that are of particular interest or with more complex geometry or loading could still benefit from the user specifying an increase in mesh density. Mesh refinement, distortion and convergence require separate consideration in relation to p-element meshes and will not be discussed here.

Mesh Generation

Hand or Auto Meshing

Back to Top

There are two distinct approaches to generating a mesh: automatic (computer) generation of a tetrahedral element mesh; or manual generation of a brick and wedge element mesh. Tetrahedral meshes have more elements and are not as accurate as the same sized brick or wedge elements.

Tetrahedral meshes are the only type of mesh that can be reliably generated within automeshers. Some brick and wedge element automeshers for general shapes are available but are not widely accepted and there still exist substantial problems with this area (visit http://sog1.me.qub.ac.uk/femgroup.html for a review of some of the best UK research in this area.) Although it is not difficult for an automesher to generate a brick mesh within a six sided solid, the problem of meshing any general solid is still difficult to automate and currently, a reliable tetrahedral automeshing algorithm is the most likely option for complex shapes with many section changes such as a cast component.

For 'slightly complicated' shapes, and depending on the nature of the pre-processor, it is worth considering creating and modifying the mesh by hand, using the pre-processor itself, rather than generate an automatic tetrahedral mesh from an imported solid model. This is usually achieved with a combination of geometry operations and manual node and element generation. A major advantage of creating manually created meshes is that they tend to be of better quality than tetrahedral meshes and generally have far fewer elements.

Despite many advances in mesh generation and links between modeller and analyses packages, a good deal of manual meshing still takes place, sometimes representing the bulk if a project's time. Some packages have better facilities than others for the often repetitive tasks involved in manual mesh generation.

The following table gives a listing of the relative merits of the two separate approaches to mesh generation:

Back to Top

Back to Top

Tips for a Good Mesh

Back to Top

General

The two mesh factors that affect accuracy are element quality and mesh density. Not all the features in a model will need the same level of accuracy and so a variation in mesh density through the model is usually appropriate; striking a balance between required accuracy and effort required to adjust the mesh. Element quality will tend to improve up to a point as mesh density is increased.

A coarse mesh is sufficient in areas where the stresses are expected to be fairly constant; i.e. in regions where the loads and geometry do not vary significantly across parts of the model.

Accuracy and the requirement for a refined mesh are dictated by the rate of change in stress with respect to distance through the component. The rate of change of stress is in turn dictated by the rate of change of load or geometry in the region of interest. Areas where the load or geometry change rapidly will require a more detailed mesh to give the same level of accuracy as a coarse mesh in a region of more uniform stress. Features like internal fillets or sudden changes in section will cause the stress distribution to be non–uniform, requiring a refined mesh in this area for accurate stress prediction.

Simplistically, a single finite element will represent a constant or linear variation in stress through its length, depending on whether it is linear or parabolic respectively. A finer mesh (or switching from a linear to a parabolic element type) therefore provides greater accuracy as it allows for a smoother variation of stress (with respect to distance) to be represented.

Aside from the inability of a coarse mesh to accurately model rapid changes in stress, such a mesh will inevitably have to suffer more distortion modelling a given shape than a fine one, where each element represents a smaller part of the varying boundary.

Although large elements should have no affect on the accuracy of distant small elements, mesh size changes should be achieved gradually through the model, as rapid element size changes can reduce the accuracy of nearby smaller elements and can also contribute to element distortion.

In defining a mesh, as well as conforming to the geometry, consideration should be given to the position of all loads and constraints to ensure that nodes are in a suitable position to apply these boundary conditions. Be wary of spending time creating the 'perfect' mesh, to find that the nodes are not near where the loads are to be applied.

Ideally, and especially if the model has not been verified by other means, a convergence test is a useful if long-winded method of determining a suitable mesh density. See the NAFEMS article on Convergence.

Back to Top

Stresses in corners, convergence

In reality, an internal corner with zero radius will have an infinite stress, if made from a perfectly elastic material. Generally, a radius must be created in the corner to achieve a measurable stress. The confusing issue with modelling this in finite elements is that sensible stresses can be predicted in the corner. This is just coincidence however; refinement of the mesh would see the stresses in the corner increase without limit. Internal corners should always be considered in any analysis as a potential failure area and these must have a realistic fillet radius inserted for convergent stress values to be predicted. Remember that the stress value reported in a non-filleted internal corner is only dependant on the size of the elements and has nothing to do with any real value that might occur there. See the NAFEMS article on Convergence.

Connecting differing element types (one way to avoid spurious displacements)

This can cause problems stemming from the mismatch of element degrees of freedom. For example, beam elements have three rotational and three translational degrees of freedom at each node whereas a brick element has only translational freedoms at each node (since these are all that are needed to fully define its position and deformation.) So, when beam and brick element are connected together, the beam's rotational freedoms are 'spare'. This may cause problems in the solution as the beam element is insufficiently constrained and could undergo unconstrained rotation. This may result in a singular stiffness matrix, which could not be solved and even it could, it is bad practice. If the software has no provision for checking and dealing with this type of issue, the analyst should ensure that 'spare' degrees of freedom are restrained out by the use of multi-point constraints or some other means.

Back to Top

Useful Model Checks

Pre Solution Checks

Material data required are Young's Modulus and Poisson's Ratio. For modal analysis, density is also required.

Useful checks that can be made prior to running the analysis include generating colour coded plots of all elements by type, and by material. Other checks will depend on the software features but element free edge checks and distortion checks should be available.

Very often, there will be some stipulated requirements for element distortion (quality) values which can be checked for. Acceptable levels of distortion depend on the situation and some types of distortion affect results more than others. However, elements with failed distortion values away from areas of interest can often be tolerated.

Back to Top

Post solution checks

Solving usually involves some crude checking of the model by the solver prior to analysis. Typical checks are for material assignment, and some application of restraints and loads. For a large, multiply connected model, it is often very useful to do a modal analysis to check for unconstrained movement and rigid body modes, prior to undertaking a static analysis. Animating the first few vibration modes can show if there are any cracks or rigid body modes in the model.

The analyst usually has access to a text file where all solver messages are reported. This should be checked to ensure there are no unforeseen problems with the model. Typical warnings are for poor element distortion, material data value omissions and nodal degrees of freedom that are not connected. For many solvers, there may be huge amounts of repeated data that tend to make this file difficult to digest and thus often ignored. However, this should be one of the first places to look to remedy any unexpected modelling problems.

Three reasons why checking is so important in finite element analysis are:

1.Model or analysis errors tend to not be revealed in the results.

2. FEA has many calculation steps, many of which are integral to the program and have been tested through benchmarking and so on. Many user controlled steps are no less important but without formal checking procedures, are likely to contain errors.

3. FEA is expensive and can only be cost effective if the risk of analysis errors is controlled with checking.

Checking should be part of a quality management system, involving documented procedures. This should encompass an appraisal of both the modelling and analysis process by an independent analyst.


Back to Top

Results Assessment - post-processing

This section only deals with stress, strain or displacement results plotting.

Back to Top

Verification

Simple hand calculations can be used to check the stress results obtained from an FE analysis. Simple errors in setting units or material data are common and some means should be used to independently verify the order (i.e. the right ‘ball park’) of the results to ensure they appear to be sensible. This is often known as a ‘sanity check’ and is cost effective (i.e. quick).

Result plots

Exaggerated deformation plots are further useful ‘sanity checks’. Animation of the result from zero to full load can be helpful in visualisation of the deformation.

Initial overall assessment of stress or strain result quantities can be best appreciated from contour plots. Stresses are often considered for proof loading strength assessment, using a Failure Criteria stress (such as Von Mises).

Alternatively, basic fatigue assessment is required; in which case maximum principal stress is usually used. Strain based assessment is sought for comparison with strain gauge data or for low cycle fatigue assessment. There are many 'bolt-on' packages for assisting the analyst to undertake fatigue analysis where raw finite element data is passed through a further set of sophisticated assessments to arrive at a fatigue life.

Back to Top

FE Results Calculation

All common structural finite element solvers use so called 'displacement based' solutions. This means that nodal displacements are the quantity solved directly from the matrix equations. Each node therefore will have a displacement result. Strains and stresses are obtained from a further calculation, carried out after the main matrix solution. Strain is a measure of rate of change of displacement (i.e. displacement gradient across an element) and these are obtained by differentiation of the displacements at internal calculation points within each element. The calculated strains and stresses are then extrapolated from these calculation points, to the nodes of the element.

Since a node connects two or more elements, it will have one set of stress results associated with it, for each element that it connects to. These values will not be the same and their variation will be an indication of model accuracy in this region, as displayed by an ‘unaveraged’ element stress contour plot. A difference of 10 to 15% is often taken to be a limiting value, indicating that the model is behaving well in this region. If the average of these values is taken, a smooth contour plot can be produced, often called an ‘average nodal stress’ plot. The values of these stresses are usually used for general stress assessments in preference to the discontinuous ‘unaveraged’ stress values.

Back to Top

Infrequent or Peak Loading (Proof and Ultimate Loads)

The aim of an analysis is to obtain stress or displacement results. Stiffness and displacements of a structure may often need to be assessed but stresses are the most likely criteria by which the integrity of a structure will be assessed. Stresses predicted by finite element analysis can be related to material properties, with consideration being given to the type and implications of failure and the consequent inclusion of safety factors or margins. Factors on stress and displacement can be obtained from Design Specifications (load documents), or standards.

Two types of in service loading are generally considered; namely proof and fatigue. These are idealised representations and any loadcase documentation should consider these types of loading as a minimum requirement.

A proof case can be considered a 'one-off' load, or an ‘overload’ case. It should encompass all reasonable foreseeable situations where the physical load on the structure exceeds the 'normal' operating loads. This situation should at most only occur a few times during the lifetime of the structure. The usual assessment of whether a structure has successfully endured such a loadcase (i.e. without failing) is if there is no gross distortion following the removal of the load. ‘No gross distortion’ implies that no significant regions of yield have occurred in the material of the structure.

The use of Von Mises stress as a measure of peak stress at a point is justified, if the stress is being compared with the failure strength or proof strength of the material. Ductile engineering materials will fail according to these criteria (maximum shear strain energy).

A fatigue case is meant to represent a typical in service load, and if only one load is applied this should represent the highest load the structure will see on a regular basis. If it is felt that fatigue loading is critical then, due to the cumulative nature of fatigue damage, all significant discrete load amplitudes will have to be considered, rather than just the maximum load. The consequent post-processing of this data will require some knowledge of fatigue lifing methods which are outside the scope of this document.

© 2002 Chalice Engineering Ltd