Abstract
Midfacial fractures rank first concerning maxillofacial traumatology. Collisions of two heads or head to object are the main causes for these fractures. An investigation based on a transient simulation using the finite element method was performed. A biomechanical head model was created and tested. A transient collision of two heads was simulated. The results were compared to a typical real patient case. This comparison revealed an identical fracture pattern, which can be interpreted as a clinical match of the simulation. The results of this study show the validity of biomechanical investigations, which may serve as a method to better understand maxillofacial fracture patterns. These results will be used for the optimization of fracture therapy or trauma prevention in the future.
Owing to their high incidence, midfacial fractures rank first amongst all maxillofacial fractures, demonstrating their high clinical importance . Collision of two heads or of a head and an object is a frequent cause of midfacial trauma. Typical fracture patterns occur in sports such as football, handball or in violence-related trauma . Scientific investigations in these trauma situations can be performed in two ways: cadaver studies; and through simulation in a virtual environment using finite element analysis (FEA). FEA is a numeric method used to solve partial derivatives in order to simulate the behaviour of solid bodies according to certain boundary conditions using an approximation method, is becoming increasingly popular as it can be adopted in a wide variety of investigations if an appropriate model is available. Cadaver studies can only deal with single questions and are limited by the availability of adequate cadaver specimens and the necessary equipment. FEA has been used in investigations on biomechanical simulation of isolated orbital wall fractures using defined objects to hit the infraorbital rim . The results of these studies are supported by the findings of several biomechanical experiments concerning orbital wall fractures and are confirmed by a case study . According to the high incidence of head collisions and the importance of the orbitozygomatic complex in complex midfacial and panfacial fractures , trauma studies on these fracture patterns are an interesting object of investigation. In contrast to their clinical importance, there have been no finite element studies regarding the collision of two heads.
This investigation aimed to design a more detailed and, in biomechanical respects, more appropriate model, compare it to earlier approaches and test it in the special trauma setting of head collision. The results would then be reviewed in a clinical context to decide whether the fracture patterns seemed realistic. If so, the next steps would be simulating further trauma modalities, investigating fracture patterns with respect to the probable impact, and considering different osteosynthesis strategies. The results could be used for trauma prevention, for example in the design of appropriate helmets as has been done in automobile safety studies or military investigations.
In order to gain further knowledge on the consequences following this particular trauma FEA can be used to calculate local stresses. These calculations could allow a better understanding of fracture genesis and permit statements on the requirements of osteosynthesis systems and reconstruction techniques. FEA allows clinicians to predict the biomechanical and anatomic consequences of any injury of the head more easily and cost-effectively than experimental methods and makes it possible to estimate a specific impact load according to an existing fracture pattern if an adequate model is available. Therefore the current finite element study with a collision of two heads was launched to investigate a computer simulation of a zygomatic trauma with respect to the occurring fracture pattern. These patterns are compared to the findings of a clinical case.
In order to simulate this trauma a transient analysis was conducted (i.e. simulating the whole trauma with smooth transition of all steps), which allows simulating the entire incident without additional calculation to determine the impact force and impact time . This type of analysis is more suitable for representing the realistic behaviour of the skull during trauma, as the effect of the viscoelastic response of bone due to a time dependent load has already been investigated for the upper limb in an experimental study . To assess the approach of this study, the biomechanical model was compared in two simulations with data taken from earlier investigations, which were concerned with geometrically defined impactors and test-bed settings . A specially defined load scenario was performed in a transient dynamic study of a head-to-head collision to understand the appearance of a typical maxillofacial fracture pattern; thus three simulations were performed.
Materials and methods
FE modelling
The central idea of FEA is to describe the mechanical behaviour of any given object by cutting it into small areas, the reactions of which can be individually computed. The individual reactions of these cells are later combined to calculate the reactions of the whole object. In order to do this some material properties are required (Young’s modulus and Poisson’s ratio), which are assigned to the individual cells. The great advantage is that FEA can be applied to almost any form or material, ranging from automobile design to surgical questions. In the medical fields, the main problem is to describe the detail required and decide which individual material parameters should be assigned. It is obvious that simple models like attributing one parameter to a complex anatomic structure such as the skull, as done in earlier work, is a very simplified approach and could lead to inappropriate results.
The authors describe their way of establishing a better model with respect to anatomic detail and biomechanical behaviour. In order to build the finite element model for the study a patient’s CT dataset (Siemens Volume Zoom Plus, 1 mm contiguous slicing) of a head without any pathological anomalies or any traumatic injury was used and segmented in the imaging software Vworks™ 4.0 Surgery (Cybermed Co., Seoul, Korea). During segmentation only bony structures are kept and soft tissue is discharged. The segmented bone was manually adjusted and holes in thin cortical bone areas were filled according to anatomical respects . The result was a very detailed 3D surface mesh. This optimized file was exported into VRML format, which is an exchange file format for 3D data and then imported into the finite element meshing module of the finite element software package ANSYS ICEM CFD 12.0.1 (ANSYS Inc., Canonsburg, PA, USA) ( Fig. 1 A) . In this module a finite element volume mesh with tetrahedral shaped 10-node elements was created according to the segmented 3D surface mesh of the bone with 736,934 volume elements ( Fig. 1 B). As the main focus lay on the midface, the mandible was omitted. For the two comparison studies, finite element models of impactors were built: one with a volume of 0.0481 cm 3 according to W aterhouse et al. and N agasao et al. ; and another with a volume of 0.0288 cm 3 based on A hmad et al. ( Fig. 2 A and B) . In the head collision study, a simplified finite element skull model with a less dense volume mesh of 86,187 elements was created in ICEM. This model was used as an impactor to simulate a realistic collision of two heads ( Fig. 2 C). All finite element models created in ICEM were transferred to ANSYS Classic ® v12.0.1 (ANSYS Inc.) (ANSYS) in order to carry out a transient nonlinear solution.
Material properties
The finite element model of the investigated skull of the collision study was assigned material parameters based on the patient’s CT dataset. The evaluation of the necessary Young’s modulus was done with the help of the programme BoneMat © developed by T addei et al. . For the calculation of Young’s modulus each pixel of the CT dataset was converted from Grey values to Hounsfield units. The Hounsfield units were converted into Young’s modulus based on the approach of M organ et al. . Each element of the volume mesh was assigned an individual material parameter with the help of an APDL script, which is a parametric programming language in ANSYS to optimize the FEM workflow ( Fig. 3 ). Poisson’s ratio, a unit-less ratio between the relative change of the thickness and the relative change of the length of a defined solid body was defined with 0.326 and the density of 1.591 g/cm 3 was taken from the literature ( Table 1 ). For a realistic numeric calculation of stresses, particularly at the surface of the bony structures, Young’s modulus of the skull model was reduced by limiting the lowest value to 11,000 MPa based on the minimum values for Young’s modulus of the literature . Young’s modulus is a material constant representing the structural stiffness of a solid body, in this case of the bone with the unit of pressure or stress (Pascal or MegaPascal). The mechanical stress is the product of Young’s modulus and the strain, which is the relative change of length of a solid body. This novel detailed approach covers all structural elements if they are represented by density values in CT imaging. Sutures of the skull are not specifically modelled because the assignment of the material parameters takes these structures into account by attributing particular values to these areas. For the impactors of the two comparison studies and the simplified skull model material properties of the literature were used. For the brass weight according to W aterhouse et al. a density of 8.4 g/cm 3 , a Young’s modulus of 100,000 MPa and a Poisson’s ratio of 0.37 were employed . These properties were also used to represent the impactor according to A hmad et al. . For the simplified skull model, which was utilized as an impactor in the collision study, a Young’s modulus of 13,500 MPa, a density of 1.591 g/cm 3 and a Poisson’s ratio of 0.32 were used based on the literature ( Table 1 ).
| Condition of the skull | Young’s modulus (MPa) | Poisson’s ratio | Density (g/cm 3 ) | Yield criteria (MPa) | Literature |
|---|---|---|---|---|---|
| Dry skull | 13,500 | 0.32 | None | 153 | N agasao et al. |
| Unembalmed skull, fresh | 13,050 | 0.29 | 1.591 | None | D echow et al. |
| Embalmed skull | 4000 | 0.2 | 0.88 | 79.3 | M c E lhaney et al. |
Boundary conditions
For the two comparison studies, the nodes of the external occipital protuberance of the investigated skull were fixed in all degrees of freedom. A local coordinate system along the axis of the impactor was created and a velocity of 4.85 m/s corresponding to a drop height of 1.2 m was applied to the impactor according to W aterhouse et al. and N agasao et al. ( Fig. 2 A). A velocity of 3.65 m/s corresponding to a height of drop of 0.68 m was applied along the axis of the impactor for the second study based on the studies of A hmad et al. ( Fig. 2 B). For an optimal hit of the impactor on the skull in both preliminary studies the skull was also placed at 20° from the sagittal plane . In both comparison studies the impactor was hitting the infraorbital rim of the right orbit. For the study of the head collision the impacting skull was assigned with a velocity of 6.5 m/s according to A rampatzis et al. in the distal direction, which corresponds to a velocity of running. The velocity was applied along an angle of 15° in the cranial direction with respect to the Frankfort horizontal plane of the impacting skull ( Fig. 2 C). To lock the model of the investigated skull the nodes of the occipital condyle were fixed in all degrees of freedom. This configuration of the model resulted in a hit of the zygomatic bone and the superolateral orbital rim of the right orbit of the investigated skull with the forehead of the impacting skull at the same time ( Fig. 3 ).
Contact modelling
For the simulation of the two comparison studies a contact pair between the skull and the impactors with a coulomb friction model was created , which is the solid body friction subdivided into sticking friction and sliding friction. The coefficient of friction for this contact was defined with 0.3 . The collision of the two skulls was also defined with a contact pair with a coulomb friction model between the two bodies. This contact pair was assigned a coefficient of friction of 0.4 .
Result evaluation
To evaluate the results of all three studies, the von Mises stresses were examined, which is a value of a virtual uniaxial stress calculated out of the 3D multiaxial stress condition with a unit of pressure. In this context the yield criteria of the skull bone of 153 MPa was used according to N agasao et al. ( Table 1 ), which is the limit where the material changes from elastic to plastic behaviour and therefore is highly at risk of failure. Stresses above the yield limit cause destruction of the bone, represented by the plastic deformation of the material. In order to analyse potential fractures and identify the region of the fractured bone, a theory of mechanical engineering was used. Based on this fracture theory, the examined part fails when two fronts of stress gradients above the yield limit hit each other. At this point the part has no more strength to resist the load .
Results
Owing to the novel modelling approach, a highly detailed model of the skull could be generated with a very dense volume mesh of 736,934 finite elements ( Fig. 1 A and B). Based on this method the details of the midface could be emphasized and successfully included into the transient analysis of the dynamic response of the skull to an impact ( Fig. 1 C).
The transient simulation of the three studies was carried out ( Fig. 2 ) and analysed and a dynamic response of the investigated skull under the action of the time-dependent load could be determined ( Fig. 4 ). In this way the von Mises stresses in the skull as well as the peak impact force could be evaluated.
