FEA Basics

Imaging

Imaging and 3D Reconstruction

The complex and free-form organic shapes of biological structures pose a challenge in finite element modeling. It is extremely difficult, if not impossible, to manually reconstruct complex organic shapes within FE or CAD software. These engineering tools are not designed to handle the highly irregular, complex geometric shapes of organics systems. The most efficient methodology for realizing FE models of biological systems is the process of 3D digital reconstruction from serial image data, usually obtained using computer topography (CT) technology.

Shown here is a single ct-scan slice through the skull, forearms, and fingers of the wrinkle-faced bat, Centurio senex.

Recent innovations in computerized tomography (CT), magnetic resonance imaging (MRI), and confocal microscopy have revolutionized biological imaging. It is now possible to capture serial sections of virtually any structure and generate exquisitely detailed 3D reconstructions. We use 3D surface reconstructions created from CT scans as templates for 3D finite element models. We work on small animals and are fortunate to have access to a micro-CT scanner in Dr. J. W. Hagadorn’s lab (http://www.amherst.edu/~jwhagadorn/) at Amherst College. Another well-known resource for micro-CT scanning is the Digital Morphology group (www.digimorph.org) at the University of Texas at Austin.

Initial 3D surface reconstructions are typically quite rough and require significant editing before they can be imported into an FE tool and successfully meshed as a finite element model. 3D surface representations can be saved in a number of different file formats depending on the software that you use. In our experience, the Standard Tessellation Language (stl) file format is the most portable and thus the easiest for taking 3D surface representations from a reconstruction program to the next phase of FE model building – editing the 3D Image.

Essentially, STL is a simple triangulation of the surface of a volumetric body. It is no surprise that the STL file format is most appropriate for this application. This file format was developed by engineers to support the stereo lithography rapid prototyping and manufacturing process. In stereo lithography a part is manufactured directly from a 3D CAD model by transmitting it to an automated STL rapid prototyping machine as a stack of 2-D slices of geometric data that collectively define the volumetric shape of the part. The machine then builds the part layer by layer. The process of digitally reconstructing the geometry of an organic system from a stack of 2-D image data is essentially the reverse of this process. This suggests that file formats and engineering software tools used to support rapid prototyping will work the best for this application.

Back to flow chart

Image Processing

Editing the 3D Image

At this point in time, editing 3D images is the most time intensive step in building FE models of biological structures. It is critical to think though the sequence of editing tools and file formats you plan to use before starting the process. File format incompatibilities and software interoperability issues are common (if not rampant). We have experimented with many different combinations of image reconstruction, surface editing, and FE analysis packages before identifying a set of file formats and programs that can be used to produce a FE model in a series of relatively simple steps.

We have had good success with keeping files in .stl format and using VGStudio Max (www.volumegraphics.com) for building 3D surface models from ct scans, Geomagic Studio (www.geomagic.com) for “cleaning” the 3D images, and Strand7 ( www.strand7.com) for generating finite element models and running analyses. There are undoubtedly other suites of tools and file formats that “play well” together; finding them and determining how to use them efficiently simply requires time and a good supply of patience.

The ultimate goal of 3D image processing is to generate a “water-tight” surface model that can be imported into and successfully manipulated in FE software. To envision a water-tight model, think of a 3D surface representation as a skin that covers all surfaces of a model. In the case of a skull, this would include not only the external surfaces but also the internal surfaces such as the nasal and middle ear cavities and any sinuses or canals. In reality, the spaces between the surfaces are filled with bone. The surfaces must be continuous in order to model the volume they define using finite elements. To complete the analogy, if you could immerse the surface model in water, the spaces between the surfaces should remain dry - the model should be “water-tight”.

3D surface representations derived from modern serial imaging techniques can be spectacularly detailed – a morphologist’s dream. The unfortunate reality is that the geometric complexity and size of these images are invariably too much for current FE modeling and analysis software to handle. We have found that the most efficient way to deal with these problems is to simplify the 3D representations using a combination of 3D reconstruction and reverse engineering software (i.e., VGStudio Max and Geomagic Studio).

The most important aspect of the simplification process involves smoothing and removing details in selected areas of the model (Figure 1). The decision of where and to what extent to simplify a model rests with the investigator. In general, any area that is not likely to be load carrying is a good candidate for simplification. For example, in developing models of bat skulls we routinely remove the nasal conchae, smooth the walls of the nasal cavity, and treat the semicircular canals and much of the middle ear cavity as solid structures. We are willing to assume that these alterations will not affect the results of our loading experiments. At the same time we retain complex structures that we suspect are structurally significant. These include structures such as the sinuses, nasal septum and the pterygoid plates.

Figure 1 (click to enlarge): Progressive simplification and decimation of the skull of Centurio senex, the wrinkle-faced bat.

Another important goal of simplification is to significantly reduce the overall size of the surface representation. This vastly decreases the computational resources required to manipulate the FE model and conduct loading experiments. 3D surface representations are composed of connected polygons and are often referred to as ‘polygon models’. The more polygons a model contains, the greater it’s fidelity to the object it represents but the larger its size. The easiest way to reduce, or decimate, the number of polygons in a model is to use the polygon reduction/decimation tools available in either 3D reconstruction or reverse engineering software (Figure 1).

Determining the extent to which a surface model should be decimated requires balancing the capabilities of the FE software against the need for a geometrically accurate model. There is a strong correlation between the number of polygons in a surface model and the number of elements in, and therefore the size of, the subsequent FE model. Therefore, it’s important to know the limits of your FE software and computational resources. (Our favorite FEA tool, Strand7 (www.strand7.com) easily handles FE models containing more than 1 million elements.) 

Even if computational resources are not an issue, larger models will almost certainly contain larger numbers of errors that will need to be fixed during FE mesh construction. Moreover, it is important to keep in mind that complex models are not necessarily “better” than simpler models. Finite element models are analysis models, and like any analysis model a finite element model constitutes an idealized (i.e. simplified) representation of the physical world. The goal is not to develop the most accurate analysis model. Rather, the goal should be to develop the simplest model that still represents structural relationships with accuracy and/or resolution required to answer the question of interest. Again, the decision of how simple to make a model lies with the investigator.  .

Choosing the right software for smoothing and decimating surface models in preparation for FE model-building is absolutely critical. Image processing is the most labor-intensive aspect of conducting FE analyses of biological structures. One of our goals has been to streamline this process in order to make FE analysis more readily available to comparative biologists. Our software recommendations are based on our experiences in working to attain that goal.  

In our experience , VGStudio Max (www.volumegraphics.com) is good for simplifying areas of complex morphology when it is useful to refer to cross-sectional images to differentiate between scanning artifacts and morphological details. For skulls this includes the nasal cavity, sinuses and teeth. We find Geomagic Studio ( www.geomagic.com) to be indispensable when it comes to filling holes in, smoothing surfaces on, and decimating surface models. We have taken the approach of starting with as rich a data set as possible and then simplifying it as needed in each subsequent step. Therefore, we decimate our polygon models as a final step before saving polygon models in stl format and importing them into our FEA tool of choice – Strand7.

Back to flow chart

Finite Element Modeling

The modeling process is made up of 4 important steps:

• Importing 3D representations into FEA tools
• Assigning material properties
• Constraining the model
• Loading the model

Importing 3D representations into FEA tools

The ease or difficulty of importing a 3D surface model into FEA software and generating an FE mesh depends upon the quality of your 3D surface model and your choice of FE software.

The first hurdle in importing a 3D surface model is file format compatibility. Most FEA tools can import water-tight surface meshes that are saved in stl ( Standard Tessellation Language) format. Stl models are recognized by Strand7 as a plate models from which a solid mesh can be generated. Many FE tools also have the ability to import models proprietary Computer Aided Design (CAD) formats. This is particularly useful if you are building FE models with CAD software rather than directly from surface representations derived from CT-scans. CAD models are generally recognized by FE software are “geometric models.” Even if the FE tool does not support the proprietary CAD format, CAD programs can also export geometry data in a standard file format called IGES which most commercial FEA tools support. Unfortunately, we have found that CAD tools are not able to handle the complexity of 3-D stl models created by our 3-D digital reconstruction process.

Once an stl surface model is imported successfully into FE software, flaws in the surface model can cause problems. These flaws can include poorly formed plates (angles excessively acute or obtuse), overlapping plates/nodes, t-junctions between plates, duplicate plates/nodes, and small gaps between adjacent plates. In our experience these kinds of errors are common in surface models built from CT-scans. In the worst-case scenario, some FE software is very sensitive to errors and simply can’t open models containing errors. In other cases, stl files with errors can be opened but attempts to generate a solid mesh from them will fail. The key to solving these problems is to use FE software that can either fix or help to pinpoint the problems.

Our FE tool of choice, Strand7 (www.strand7.com), will import stl files that contain significant errors. A built-in mesh cleaning tool is effective in removing duplicates plates/nodes and zipping together adjacent plates. It can also point out t-junctions. These must be fixed by going back into the stl model with editing software (e.g. Geomagic), manually reworking the area, and then re-importing the stl. Once a solid mesh is generated and an analysis is underway, Strand 7 (and most other FE tools) provides warnings to identify malformed element in the mesh. Again these must often be fixed by making changes to the stl model and re-importing it.

Assigning material properties

Material property information for the system being modeled must be known a priori.  This means that fundamental material property behavior is an input - not an output - to a finite element analysis.

Any single FE model can include groups of elements with distinct material properties. Thus, virtually any complex composite structure can be modeled. Most commercial finite element tools support the specification of many different material behavior models. These include: linear elasticity, nonlinear elasticity, nonlinear inelastic, viscoelastic, isotropic, orthotropic, anisotropic, etc. Some tools (including Strand7) even permit the user to write macros or subroutines for the purposes of defining unique material models for specific applications. This is particularly important for comparative biologists as no commercial FE software provides default material properties databases for tissues such as bone, ligament, cartilage or muscle. We are developing a Strand7 material properties library that includes the data listed in the material properties database on this site. We will post it on biomesh.org as soon as it is complete.

Constraining the model

All finite element models must be kinematically constrained before they can be analyzed. In rigid body static analysis, we use Newton’s laws to deduce the set of forces necessary to keep a body in static equilibrium and often graphically represent this with a rigid “free body diagram.” The deformation of the body is not of interest in rigid body static analysis. In contrast, predicting deformation is the goal of finite element analysis and it is mathematically impossible to predict deformation without imposing kinematic constraints. FE models must be fixed in space in order to predict how they will deform under load (i.e. before one can compute stresses and strains). For FE analysis this means that there must be sufficient constraints on a model to prevent all possible modes of rigid body motion. A rigid body in space has 6 rigid body modes of motion - translation in each of three mutually orthogonal directions and rotation about each of the three axis that define the three mutually orthogonal directions.

Choices about constraints can have a significant impact on the patterns of stress and strain predicted through FE analyses. The figure below compares two FE analyses of a skull that differ only in how constraints were applied. The skull of the left skull was constrained at 3 nodes: one at each of the centers of the left and right jaw joints and another on the upper left. The model on the right was constrained at the same node on the upper left molar and at one node on each of the occipital condyles. In both cases, the node at the tooth was constrained against all movement while the other two nodes were free to rotate but fixed against displacement.

There are clear differences in both the magnitude and distribution of stress under the two loading regimes. If one is interested in stresses generated during feeding, we would argue that the constraints on the left (the center of the mandibular condyles and the tooth) are “better” because they more closely model how the lower jaw contacts the skull. Note that kinematic constraints are another example of an analysis idealization. If a single point defined by a node is rigidly constrained against motion, stresses predicted at this point are not realistic. The constraint results in what is called a “stress singularity.” This means that if a series of analyses were conducted with increasing mesh density surrounding the constrained node, the predicted stresses at this point would keep increasing without bound. The singularity in stresses merely reflects the physical impossibility of constraining a real physical object at a point. Where to place constraints on an FE model is clearly an important decision that should be made carefully and with as much prior knowledge about how a system works as possible.

Back to Flow Chart

Loading the model

The final step before FE analysis is to apply loads to the model. As the primary goal of FE analyses is to predict how systems will perform, it is important that loads be applied as realistically as possible. For example, engineers who want to use FEA to predict how an earthquake will affect a new building design would need to define the amplitude, frequency and direction of shock waves of a range of seismic events. Similarly, a biomechanist interested in the peak compressive stresses within the femur of a runner would need to define the magnitude and direction of forces acting on the bone. FE tools offer many different ways to apply loads. These include the ability to apply loads as forces acting on individual nodes (point-loads), forces distributed over groups of nodes or element surfaces, pressures, loads per unit volume such as due to gravity or acceleration, or initial stresses or strains that result in nodal loads. The problem in modeling biological systems isn’t so much what method to use, but knowing how the loads should be applied.

In contrast to many man-made structures, the forces acting on biological systems can be extremely complex. Take, for example, the relatively simple situation of a muscle applying a load to a bone. For an FE model of a bone under load a researcher would want to know something about the areas over which muscles are attached, the magnitude of the force it produces by the muscles, the direction in which muscle forces are applied, and loads imposed by ground reaction forces (in the case of locomotion) or contact with other bones.

A great deal of thought and, in some cases effort, need to be put into loading FE models of biological systems. In our lab we have addressed the problem of loads imposed by muscles that wrap around their surfaces by writing a program. The program requires basic input regarding muscle forces and directions and can apply a combination of tangential tractions and normal loads due to muscle attaching to and wrapping around irregularly shaped bone surfaces. You can download a copy of the program here.

Back to Flow Chart

Interpreting Results

Once an FEA solution has been obtained, it is critical to assess its accuracy. Inaccuracies due to erroneous modeling assumptions are difficult if not impossible to assess without valid empirical data or expert knowledge about the analysis.

Other sources of errors can be effectively assessed and controlled. As a numerical method, finite element analysis results are approximations to the theoretically exact (and usually intractable) solutions to the underlying equilibrium equations that govern the physical behavior of a system. In reality, the continuum of a system has an infinite number of degrees of freedom. The discretization of the continuum with a finite element mesh results in a finite number of nodal degrees of freedom that approximates the solution behavior. Fortunately, through a series of properly constructed meshes involving increasingly more nodal degrees of freedom and separate analyses, one can come arbitrarily close to the theoretically exact solution. This is process of controlling the inherent finite element discretization error is called a convergence study. Consider the simple bar fixed at the left face and under a distributed axial load q (i.e. load per unit length) as shown in the figure. The next two figures show the uniaxial deflection and stress in the bar for the exact solution compared to a single finite element solution.

In the next four figures the exact solutions are compared to the finite element solutions for the case of the bar meshed with two and four elements. Note how the finite element solution is approaching the exact solution as the bar is meshed with more elements, and hence nodal degrees of freedom. Also note that the displacement solution is more accurate for a given mesh than the stress solution. This is typically the case. As always, larger and more complex models require more computational resources.

Typically, one expects a quantity of interest, such as maximum deflection, principal strain, or von Mises stress, to converge asymptotically to the theoretically exact value. This means at least three different analyses are required to generate a plot of the quantity of interest versus some measure of degrees of freedom in the system that shows a converging trend to an asymptotic value. Unfortunately, given the large number of nodes and elements required to model some biological systems, it may not be possible to develop a series of models with increasing mesh refinement. However, while convergence studies and comparison to experimental data is always preferred methods of validating FE analyses, we can still gain some confidence in the results from single analyses. In this case one can examine the results of a finite element model for lack of local equilibrium. For example, on a free external surface (i.e. an external surface with no forces acting on it), the FE model should predict that the component of stress normal to the surface to be essentially zero. Similarly, each finite element admits different states of stress. But in a theoretically exact solution certain stress components must be continuous across inter-element boundaries. Observing the degree of lack of continuity in certain stress components across inter-element boundaries is another way to help assess how accurate the model is.

Copyright - biomesh.org, 2007

Back to Flow Chart