Building on Finite Elements
About the Author
Over the past few decades traditional engineering analysis techniques have rapidly been replaced by computerised methods. Probably the most widely-used type of stress analysis software is based on the ‘finite element’ technique. These days there are very few design offices which do not have access to at least one of the many finite element programs on the market.
I think there is a general lack of understanding of the basic principal of finite element analysis.
These software packages can be very powerful in the hands of an experienced user. The potential drawback is that, especially in times of austerity, stretched training budgets mean that more and more engineers are being left to teach themselves how to use the software. This is in glaring contrast to other aspects of the industry – I’m sure you would be shocked, for example, if anyone on site was instructed to use a piece of construction equipment without proper training. For all the power of these programs, the results are entirely dependent on the engineer using them – if you put rubbish in, you will get rubbish out!
I first used finite element software as a fresh graduate, and found the whole experience thoroughly baffling. Apart from the book of worked examples provided with the software, I had no training, and the other engineers in my office were in the same situation. It was only by painstakingly working through the examples and making mistakes that I improved my abilities. I have no doubt that during this time some of my design work was based on dodgy analysis results.
Despite spending much of my time confused, I found using the software very interesting, and once I had reached a reasonable level of ability I applied for a job with the software company LUSAS. For the last couple of years I have been working for the LUSAS technical support team, so those of you who use this particular piece of software may well have had a conversation via phone or email with me at some point!
After starting at LUSAS I very quickly realised that I had developed some very bad habits during my period of self-teaching. Some of my ‘assumptions’ about the software had been completely wrong. My experience answering technical support queries quickly showed me that many (probably most) practicing engineers were in a similar situation – without any formal training and relying on the limited information provided in the worked examples or gleaned from colleagues. In particular, I think there is a general lack of understanding of the basic principal of finite element analysis – the way the element ‘mesh’ works. I think a good understanding of the basics of meshing will go some way to helping you become a good finite element user, so I would like to use this opportunity (thanks Tom!) to explain some of the basics of finite element analysis that every engineer should know before using this software. Because of my personal experience, this has been written using LUSAS-specific examples, but the information should be relevant to other programs as well.
My advice to any engineers using this type of software would be that if you are in any way unsure how to approach an analysis, simply contact the technical support team – that’s what they are there for!
I apologise for the departure from Tom’s usual entertaining posts! (Ed:I don’t know- this is one of the best thrillers I’ve ever read, i.e. “How many of these mistakes how you made?”)
So what is Finite Element Analysis?
Poor selection of element type or a poor arrangement of elements can provide incorrect and unconservative results.
In all finite element analysis a real structure is idealised to a (finite) number of ‘elements’ – hence the name. Stiffness matrix equations are formed and solved to ensure equilibrium between the elements, the applied loads and the structural supports. The resulting displacement matrix can be used to back-calculate forces, moments and stresses for use in design.
The type and arrangement of the elements used in an analysis will have a large influence on the results achieved. Poor selection of element type or a poor arrangement of elements can provide incorrect and unconservative results. Most finite element users are aware that they will get poor results if the mesh is not fine enough, but it is difficult to quantify exactly how fine a mesh should be. To a large extent this is analysis-specific, but there are a few general considerations which should be applied to every analysis.
There are many different element types available in LUSAS. Different geometric features (e.g. lines, surface or volumes) will require different element types, but there are many element options for each type of feature. Details of all of them can be found in the ‘Element Reference Manual’ which is accessible through the Help system, but I have provided a summary table at the end of this document.
A basic knowledge of the features of the various element options is very useful when planning an analysis. For example, there are (at time of writing) 7 different types of beam element. Depending on the analysis being undertaken some of these might be more suitable than others. If you are using more than one type of element in an analysis (for example beams and shells) compatibility between the specific beam element and the specific shell element must also be considered.
It is therefore important to be aware of whether your chosen mesh has quadratic (very good), linear (good) or constant (poor) variation of results across each element.
Some mesh types specify either thick or thin elements. The difference is that thick elements have out-of-plane shear flexibility, meaning that they undergo shear deformations and as a result can output shear forces. Thin elements do not have shear flexibility, and as a result do not output shear forces. This difference means that thick mesh types are applicable to any model, but thin meshes can be more efficient for structures where out-of-plane shear effects are minimal. For example, shear in a steel I-beam is primarily carried by in-plane shear in the web rather than out-of-plane shear in the flanges, so thin shells could be used for modelling such a component.
Another important consideration when selecting a mesh type is the force variation across each element. The ‘3D thick beam’ (BMS3) is probably the most commonly-used beam element and is very efficient because each individual element has a quadratic variation of bending moment across it. This means that the bending moment diagram across each element will form a nice smooth curve, resulting in good results even with relatively few BMS3 elements used:
Conversely, the ‘3D thick nonlinear beam’ (BTS3) has constant bending moment results across each element. This results in a ‘stepped’ bending moment diagram which can drastically underestimate moment results, especially at sharp changes such as hogging at supports. The diagram below shows how the hogging moment of 123kNm predicted by the BMS3 elements is underestimated by 23% when BTS3 is used.
It is therefore important to be aware of whether your chosen mesh has quadratic (very good), linear (good) or constant (poor) variation of results across each element. In LUSAS you can check this in the Element Reference Manual under the heading ‘Notes on Use’. For example, the entry for element type BMS3 states “The force variations along the beam are constant axial force, constant torsion, linear shear forces and quadratic moments.” Obviously an element with higher-order force variations is preferable.
All mesh types also have an interpolation order which is either linear or quadratic. This is distinct from the force variations discussed above. Linear order elements only have nodes at the ends (or corners) of each element, whereas quadratic order elements also have ‘midside’ nodes half way along each edge of the element. Quadratic order elements usually have higher-order force variations than the linear equivalent and therefore fewer are required to achieve accurate results. Linear order elements should not generally be mixed with quadratic order elements.
A summary of the structural (as opposed to thermal) mesh types available in LUSAS is presented below:
|Beams and bars||These mesh types are assigned to line features and are generally suitable for the analysis of structural members where the cross-section dimensions are much smaller than the length.|
|Bars||This mesh type only carries axial force. It is typically used for cables (use a single division only to prevent lateral mechanisms due to the lack of bending resistance) or for rebar in reinforced concrete structures.|
|Beams||Beams carry axial force plus torsion, bending moments and shear forces. There are various types of beam, the most generally-applicable of which is probably the ‘thick 3D beam’ (BMS3). These are very widely used for frame type structures and can also be connected to shell elements for beam-and-slab or stiffened plate structures.|
|Plates and shells||These mesh types are assigned to surface features and are generally suitable for the analysis of flat or curved structures where the thickness is much smaller than the plan dimensions.|
|Plates||These only carry out-of-plane forces and moments (i.e. no in-plane ‘membrane’ forces). They can be used for the analysis of simple flat structures such as concrete slabs.|
|Shells||These also carry in-plane forces so are more versatile than plate elements. They can be used for 3D structures such as the walls of box girders or the plates of I-beams.|
|2D continuum||2D continuum meshes are assigned to 2D surface features, which must be modelled in the XY plane. The 2D model represents a section through a 3D structure.|
|Plane stress||Plane stress elements only carry stress in the in-plane (XY plane) directions, but can experience strain in the out-of-plane direction. These assumptions make them suitable for analysis of planar structures of limited thickness. See example “Linear Elastic Analysis of a Spanner”.|
|Plane strain||Plane strain elements only undergo strains in the in-plane directions, but can carry stress in the out-of-plane direction. These assumptions make them suitable for analyses where the surfaces represent a slice through a long structure. A typical use is for embankments or cuttings in geotechnical applications. See example “Drained Nonlinear Analysis of a Retaining Wall”.|
|Axisymmetric||Similar to plane strain elements except that rather than a section through a long, straight structure, these elements are formulated to represent a section through a circular structure. Typical uses include the analysis of circular pressure vessels or mechanical components.|
|3D continuum||A 3D continuum mesh is used where it is necessary to represent the actual geometry of a structure in a finite element analysis. The number of elements required for this type of analysis usually makes it impractical and/or slow to use them for large-scale analyses (for example whole bridges or buildings).|
|Solids||Solid meshes are typically used for detailed analysis of mechanical components which cannot reasonably be represented by any of the other types of mesh.|
As well as an appraisal based on the judgment of the engineer, it is recommended that all analyses are evaluated with a mesh refinement check. This involves changing the mesh density, re-solving and checking whether the results are significantly affected. If increasing the mesh density significantly changes the results, this suggests that the mesh is not fine enough. Once the results start to converge then you can have confidence that the mesh density is sufficient.
In particular, be aware that any elements with ‘constant’ force variations will require very fine meshes to achieve accurate results. Quadratic order elements will generally provide good results with a coarser mesh than the equivalent linear-order element.
The golden rule is to keep the shape of the surface and volume features as simple as possible to allow a neat grid of elements to be used.
Once surfaces and volumes are introduced into an analysis, meshing becomes more complicated. As well as setting the number of mesh divisions, it is now necessary to ensure that the meshing pattern is reasonable. In the simplest terms, the following should be avoided:
- Elongated (high ‘aspect ratio’) elements
- Elements with acute-angled corners
In other words, the ideal element shape is as near to square (or cubic for volumes) as possible. The reason for this is that results are calculated at a number of locations (called ‘Gauss’ points) within the surface or volume elements. Results are extrapolated from the Gauss points to the element ‘nodes’ from where they can be read by the user. In the case of highly elongated or angular elements, the distance between the Gauss points and the nodes can be large relative to the size of the element, and errors can be introduced in the extrapolation process.
Meshing of surfaces and volumes is a complicated topic, but the golden rule is to keep the shape of the surface and volume features as simple as possible to allow a neat grid of elements to be used. Square elements are preferable to triangular elements for surface meshes, and hexahedral meshes are preferable to pentahedral or tetrahedral meshes for volumes.
To finish, here are some examples of poor meshing and preferable alternatives:
|Poor Example||Preferable Example|