Conference PaperPDF Available

Crash Simulation of an F1 Racing Car Front Impact Structure

Authors:

Abstract and Figures

Formula 1 motorsport is a platform for maximum race car driving performance resulting from high-tech developments in the area of lightweight materials and aerodynamic design. In order to ensure the driver’s safety in case of high-speed crashes, special impact structures are designed to absorb the race car’s kinetic energy and limit the decelerations acting on the human body. These energy absorbing structures are made of laminated composite sandwich materials - like the whole monocoque chassis - and have to meet defined crash test requirements specified by the FIA. This study covers the crash behaviour of the nose cone as the F1 racing car front impact structure. Finite element models for dynamic simulations with the explicit solver LS-DYNA are developed with the emphasis on the composite material modelling. Numerical results are compared to crash test data in terms of deceleration levels, absorbed energy and crushing mechanisms. The validation led to satisfying results and the overall conclusion that dynamic simulations with LS-DYNA can be a helpful tool in the design phase of an F1 racing car front impact structure.
Content may be subject to copyright.
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
Crash Simulation of an F1 Racing Car Front Impact
Structure
S. Heimbs, F. Strobl, P. Middendorf, S. Gardner, B. Eddington, J. Key
* EADS Innovation Works, 81663 Munich, Germany
** Force India Formula One Limited, Northamptonshire, UK
Summary:
Formula 1 motorsport is a platform for maximum race car driving performance resulting from high-tech
developments in the area of lightweight materials and aerodynamic design. In order to ensure the
driver’s safety in case of high-speed crashes, special impact structures are designed to absorb the
race car’s kinetic energy and limit the decelerations acting on the human body. These energy
absorbing structures are made of laminated composite sandwich materials - like the whole
monocoque chassis - and have to meet defined crash test requirements specified by the FIA. This
study covers the crash behaviour of the nose cone as the F1 racing car front impact structure. Finite
element models for dynamic simulations with the explicit solver LS-DYNA are developed with the
emphasis on the composite material modelling. Numerical results are compared to crash test data in
terms of deceleration levels, absorbed energy and crushing mechanisms. The validation led to
satisfying results and the overall conclusion that dynamic simulations with LS-DYNA can be a helpful
tool in the design phase of an F1 racing car front impact structure.
Keywords:
Formula 1; crash simulation; energy absorption; composite sandwich material
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
1 Introduction
Formula 1 is the top class of motorsports, demonstrating maximum race car driving performance
resulting from high-tech developments in the area of lightweight materials and aerodynamic design
(Fig. 1). Since extreme racing speeds may lead to severe accidents with high amounts of energy
involved, special measures are taken in order to ensure the driver’s safety in case of high-speed
crashes. Besides the driver’s protective equipment (like helmet, harness or head and neck support
device) and the circuit’s safety features (like run-off areas or barriers), the F1 car itself is designed for
crashworthiness and possesses special sacrificial impact structures, which absorb the race car’s
kinetic energy and limit the decelerations acting on the human body. The FIA as the governing body of
motorsports imposes strict regulations for the performance of these energy absorbing structures,
which are updated each racing season [1]. The main philosophy behind those crashworthiness
regulations is to assure that the driver is enclosed within a strong survival cell, surrounded by energy-
absorbing structures in the front, back and sides. Besides static tests (nose push-off test, side
intrusion test etc.), the vehicle structure has to withstand dynamic impact tests (frontal impact test, rear
impact test, side impact test and steering column test) [2]. Such tests are documented in [3-5].
Today almost the whole F1 racing car is made of lightweight composite materials, including the energy
absorbing structures [6-10]. While metals absorb energy by plastic deformation, composites do so by
braking and crushing into small fragments. The basic energy absorption capabilities of a composite
laminate for the design of a crash box are typically evaluated in drop tower tests on cylindrical,
rectangular or conical specimens. The design process of the final F1 racing car crash absorbers is
also primarily based on experimental crash test series.
One efficient tool in the design of composite structures are numerical simulations based on the finite
element (FE) method. The commercial explicit FE code LS-DYNA has been used in many past
investigations for crushing simulations of composite cylinders or crash boxes [11-19] and even for
crashworthiness studies of racing cars [20-22].
The aim of the following study is to apply the FE code LS-DYNA for the crushing simulation of an F1
racing car front impact structure in a frontal crash against a rigid wall. This composite structure
consists mainly of the nose box, which is mounted to the chassis. Attached are the nose tip and a
representative front wing with certain wing pillars (Fig. 2). The focus of this investigation is on the
modelling of the composite material crushing. Simulation results are compared to experimental crash test
data in a qualitative and quantitative way with respect to crush front propagation and deceleration
curves.
Figure 1: Force India F1 racing car of 2008 season (photo: Sutton Motorsport Images)
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
Figure 2: Illustration of F1 racing car front structure components
2 Frontal impact crash testing
The frontal impact crash test specified by the FIA aims at assuring that the nose box is able to
dissipate the kinetic energy involved in the crash and the driver is protected from injurious deceleration
forces. The crash tests were performed at the Cranfield Impact Centre according to FIA regulations
(Fig. 3). Those demand a total weight of 780 kg and an impact velocity of 15 m/s [1]. This velocity
obviously is much lower than typical race track speeds, but before a racing car frontally strikes a rigid
wall its speed is usually reduced by gravel run-off areas and the deformable tire barriers.
The chassis with a 75 kg dummy was mounted on a test sled, which was accelerated to the specified
velocity. When the test sled strikes an immovable steel plate, mounted on a huge concrete block, the
peak deceleration over the first 150 mm of deformation may not exceed 10 g, the peak deceleration
over the first 60 kJ of energy absorption may not exceed 20 g and the average deceleration of the
chassis may not exceed 40 g. These values are measured by accelerometers mounted on the sled.
Figure 3: Frontal impact crash test setup
Representative wing
Wing pillar
Nose tip
Nose box
Chassis
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
3 Model development
3.1 Mesh generation and boundary conditions
The FE model for crash simulations of the F1 racing car front impact structure consists of the nose
box, nose tip, wing pillar and wing. The mesh was generated in Hypermesh based on CAD data. In a
preliminary study a full model was compared to a half model using symmetrical boundary conditions.
Since the influence on the simulation results was negligible, the half model was prioritised due to the
significantly lower computational cost. The model in Fig. 4 has been mirrored for visualisation
purposes. It consists of 58 different part definitions, resulting from numerous assembly parts and
different composite laminate lay-ups. The influence of different mesh sizes was investigated in a
further preliminary study. Finally, an element size of 3 mm was used, which leads to approx. 78000
elements in the half model. The chassis with its respective mass was modelled as a rigid body dummy
plate of solid elements connected to the nose box. Displacements of this part are only possible in x-
direction, representing the requested fixture to the test sled.
The connection of different parts like wing and wing pillar or wing pillar and nose tip is achieved by the
utilisation of contact algorithms, partly with and without failure option, allowing for realistic energy
absorption due to debonding. An additional global single-surface contact is used to avoid penetrations
between different parts. An initial velocity of 15 m/s is ascribed to the whole model to impact a fixed
rigid wall.
Figure 4: LS-DYNA model of F1 front impact structure
3.2 Material modelling
Nose box and nose tip are made of a lightweight sandwich structure consisting of carbon fibre/epoxy
skin laminates and an aluminium and Nomex® honeycomb core. During the crash test the nose box is
literally converted into a cloud of dust and fragments within one tenth of a second with matrix cracking,
fibre breakage and delaminations in the crush front mainly contributing to the energy absorption. Two
modelling approaches come into consideration for such sandwich composites:
The first option is to model the honeycomb core with homogenised solid elements and the skins with
shell elements, connected by a contact formulation (‘shell-solid-shell’ approach) [24]. Lamb [25] has
adopted this approach for his crash simulations of an F1 racing car front impact structure with PAM-
CRASH. In general, this rather expensive technique enables to cover skin/core debonding, a better
representation of core shear deformations and core indentation in thickness direction. However, since
those effects play a less important role in axial crushing of the sandwich structure and the reduction of
computational cost was of higher importance to establish crash simulations as an efficient tool in the
fast moving F1 development process, this approach was not adopted here.
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
The second option, which was used in this study, is to model the whole sandwich structure within a
multi-layered shell element (‘layered shell’ approach). A certain number of integration points are
defined through the thickness of the shell element in a user-defined integration rule, representing the
core and skin laminate layers (Fig. 5). For the sandwich materials in this study, this led to a maximum
of 23 integration points across the thickness. For this purpose, underintegrated Belytschko-Tsay
elements based on the first order shear deformation theory were used. Different material models may
be ascribed to the individual integration points.
Figure 5: Illustration of honeycomb sandwich structure and layered shell modelling
For the carbon fibre/epoxy skins the composite material model MAT54 was used. This orthotropic,
linear elastic material law is based on the Chang/Chang failure criteria, which control failure in
longitudinal and transverse direction under compressive, tensile and shear loads [26]. In addition,
failure strain parameters DFAILx were used to control the erosion of individual layers and the total
absorbed energy. Since delaminations, occurring ahead of the crushing zone under crash loads,
cannot be represented physically in the model, the so-called crash-front algorithm of MAT54 was
adopted: The crash-front parameter SOFT of the material model reduces the strength of those
elements neighbouring failed elements to capture this pre-damage effect and allow for a continuous
crushing. It turned out that SOFT=0.8 is sufficient for the generation of a stable crush front.
The inner honeycomb layers were also modelled with MAT54 since it allows for orthotropic linear
elastic-perfect plastic stress-strain behaviour, which is characteristic for the in-plane compression of
honeycomb structures [27].
Mass scaling was used to speed up the simulation: 1% increase of mass increased the time step from
0.17E-6 to 2.25E-4 ms and led to a total CPU time of 8 hours on twelve parallel processors for a
simulation time of 110 ms.
4 Simulation results and validation
The front impact crash simulation begins with the nose tip hitting the wall, being compressed and
partly being fractured. Then the lower structure of the nose tip and the wing pillar are detached
through a debonding failure under shear loads covered by the chosen contact definition. Afterwards,
the nose box strikes the wall and is crushed continuously until all kinetic energy is absorbed. An image
sequence of the crash simulation results is shown in Fig. 6. For comparison reasons, a sequence of
images taken from the high speed film in the crash test at corresponding time steps is also shown.
The qualitative correlation appears to be very good. The only difference is in the detachment of the
front wing, which is highly affected by the erosion of specific elements. However, this was proven to
have no influence on the global results. Almost all elements of the nose box are eroded in a
continuous crushing process, which is illustrated in Fig. 7, where all eroded elements are dark shaded.
A comparison of the deceleration curves vs. crushing displacement in Fig. 8 – both being recorded
with a sampling frequency of 20 kHz and filtered with an SAE 60 filter – also shows a good
quantitative correlation with noticeable discrepancies only occurring between 200 mm and 400 mm
crushing displacement, which might make an enhanced modelling of the stiff wing pillar attachment
section necessary.
L
W
T z
y
x
Honeycomb core
Composite skins
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
Figure 6: High speed image sequence of front impact crash test vs. simulation results
Figure 7: Illustration of eroded elements due to fracture (dark colour)
Figure 8: Deceleration-displacement diagram for frontal impact: test vs. simulation
The initial kinetic energy of 88 kJ is mainly absorbed by material deformation and fracture (internal
energy) and friction between the impact structure and the rigid wall (sliding energy). The hourglass
energy, resulting from the underintegrated shell elements, is less than 5% of the total energy.
Deceleration [g]
0 100 200 300 400 500 600 700 800 900 1000
Displacement [mm]
Crash Test
LS-DYNA Simulation
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
5 Summary and conclusions
Crushing simulations of an F1 racing car front impact structure striking a rigid wall have been
conducted and validated against experimental crash test data. Since it is very difficult to represent the
crushing and fragmentation of the composite material with relatively coarse finite elements, the crash-
front algorithm was used as a substitute numerical method to cover the continuous crushing of the
structure in a layered shell model. A fair correlation with respect to qualitative and quantitative results
could be obtained with this model. Those results relate to only one configuration of the front impact
structure. Different designs with different laminate lay-ups have been analysed in the framework of this
study with comparisons of crash simulations and experimental data to evaluate the robustness of the
model. The validation led to satisfying results and the overall conclusion that dynamic FE simulations
with LS-DYNA can be a helpful tool for an evaluation of the crash performance of different
configurations in the design phase of an F1 racing car front impact structure, although this method is
not qualified for a replacement of crash tests.
6 Literature
[1] 2008 Formula One Technical Regulations, FIA, Paris, 2008.
[2] Mellor, A.: Impact testing in formula one. International Journal of Crashworthiness, 7(4), 2002,
475-486.
[3] Feaboli, P.; Norris, C.; McLarty, D.: Design and certification of a composite thin-walled structure
for energy absorption. International Journal of Vehicle Design 44(3/4), 2007, 247-267.
[4] Savage, G.; Bomphray, I.; Oxley, M.: Exploiting the fracture properties of carbon fibre
composites to design lightweight energy absorbing structures. Engineering Failure Analysis, 11,
2004, 677-694.
[5] Browne, A.; Fuchs, H.; Johnson, N.; Watling, P.; Melvin, J.; Pierce, J.: Side-impact testing of
race car sandwich panels. Automotive Engineering, 105(3), 1997, 99-104.
[6] Wright, P.: Formula 1 technology. Society of Automotive Eng., Warrendale, 2001.
[7] Macknight, N.: Technology of the F1 car. Hazleton Publishing, Richmond, 1998.
[8] O'Rourke, B.P.: The uses of composite materials in the design and manufacture of formula 1
racing cars. Proc. of the Inst. of Mechanical Engineers, 204, 1990, 41-48.
[9] Savage, G.: Composite materials in formula 1 racing. Metals and Materials, 7(10), 1991, 617-
624.
[10] BMW Team: Materials in the BMW Sauber formula 1 race car. Advanced Materials &
Processes, 166(11), 2008, 59-62.
[11] Hörmann, M.; Wacker, M.: Simulation of the crash performance of crash boxes based on
advanced thermoplastic composite. 5th Eur. LS-DYNA Users Conference, Birmingham, UK,
2005.
[12] El-Hage, H.: Numerical modelling of quasi-static axial crush of square aluminium-composite
hybrid tubes. Int. Journal of Crashworthiness, 9(6), 2004, 653-664.
[13] Schweizerhof, K.; Maier, M.; Matzenmiller, A.; Rust, W.: Energy absorption with composite
crash elements in frontal crash - an analysis with LS-DYNA3D. 11th CADFEM user meeting,
Bamberg, 1993.
[14] Papapostolou, D.: Finite element modelling of the static axial compression and impact testing of
square CFRP tubes in LS-DYNA3D. 5th Eur. LS-DYNA Users Conf., Birmingham, UK, 2005.
[15] Mamalis, A.G. et al.: The static and dynamic axial collapse of CFRP square tubes: finite element
modelling. Composite Structures, 74(2), 2006, 213-225.
[16] Agaram, V.; Bilkhu, S.S.; Fidan, S.; Botkin, M.E.; Johnson, N.L.: Simulation of controlled failure
of automotive composite structures with LS-DYNA3D. Proc. 12th ESD/SAE Advanced
Composites Conference, Detroit, MI, 1997, 181-190.
[17] Botkin, M.E.; et al.: Numerical simulation of post-failure dynamic crushing of composite tubes.
2nd International LS-DYNA Conference, San Francisco, 1994.
[18] Matzenmiller, A.; Schweizerhof, K.: Crashworthiness simulations of composite structures - a first
step with explicit time integration. In: Nonlinear Computational Mechanics: State of the Art,
Springer, Berlin, 1991, 643-670.
7th European LS-DYNA Conference
© 2009 Copyright by DYNAmore GmbH
[19] Kerth, S.; Ostgathe, M.; Dehn, A.; Maier, M.: Experimental investigation and numerical
simulation of the crush behaviour of composite structural parts. 41st SAMPE Symposium and
Exhibition, 1996, Anaheim, CA, 1397-1408.
[20] Bisagni, C.; et al.: Progressive crushing of fiber-reinforced composite structural components of a
formula one racing car. Composite Structures, 68(4), 2005, 491-503.
[21] Siegler, B.P.; et al.: The application of finite element analysis to composite racing car chassis
design. Sports Engineering, 2(4), 1999, 245-252.
[22] Williams, T.D.; et al.: The prediction of frontal impact crashworthiness of a space-frame
sportscar. International Journal of Crashworthiness, 4(2), 1999, 147-158.
[23] Borg, R.: Simulation of delamination initiation and growth in fiber composite laminates. PhD
Thesis, Linköping University, Sweden, 2002.
[24] Heimbs, S.; Middendorf, P.; Maier, M.: Honeycomb sandwich material modeling for dynamic
simulations of aircraft interior components, 9th International LS-DYNA Users Conference,
Dearborn, MI, 2006.
[25] Lamb, A.J.: Experimental investigation and numerical modelling of composite-honeycomb
materials used in formula 1 crash structures. PhD Thesis, Cranfield University, UK, 2007.
[26] Chang, F.K.; Chang, K.Y.: A progressive damage model for laminated composites containing
stress concentrations. Journal of Composite Materials, 21, 1987, 834-855.
[27] Heimbs, S.; Schmeer, S.; Middendorf, P.; Maier, M.: Strain rate effects in phenolic composites
and phenolic-impregnated honeycomb structures. Composites Science and Technology, 67(13),
2007, 2827-2837.
... The design must incorporate lightweight material [6]. In addition, the design must be built to absorb kinetic energy from a race car and minimize the deceleration acting on the human body in case of a collision [7]. To provide optimum safety to the driver, aluminum, composite, and other metal alloy foil are generally used [4,8]. ...
... The comprehensive impact event and the contribution of each component were determined. Heimbs et al. [7] examined the cone collision condition of the impact structure of F1 racing cars, using LS-DYNA to control the modeling of composite materials. The numerical findings were compared to the crash test data in terms of crush, energy absorbed, and deceleration rates. ...
Article
Full-text available
The impact attenuator is a safety vehicle system designed to absorb the kinetic energy from a collision that is converted into deformation and ensures the deceleration level acting on the human body remains low. In this paper, we propose that the impact attenuator be fabricated with used cans, which are easy to obtain. Compared to fabricating cylinders through machining and other production processes using new material, the application of used cans may reduce production costs by approximately IDR 500,000 (USD 34.50) for one attenuator structure, while the attenuator still meets the weight criterion, i.e., it has to be light to improve acceleration and fuel efficiency. As a type of metal waste product, food cans are often fabricated from aluminum and other metal alloys. These products are widely used in our lives; if they are not recycled, they can potentially pollute the environment as waste. Given these problems and considering the use of environmentally friendly materials, lightweight used cans were chosen as materials for the proposed impact attenuator design. In the initial study, the verification and validation tests of the impact attenuator shell and used cans show good agreement between the numerical and experimental impact tests. The proposed impact attenuator design under the predetermined parameters showed that used cans of aluminum 6063 series can be recommended as an alternative material in this system.
... The controlled crush behavior offered by the Carbon fiber Epoxy composite has found an important application in survival cells and nose cones which protect the driver in the event of the crash. McLaren produced the first composite motor sports car made from Carbon fiber monocoque [13]. Figure 8 shows a racing car that uses a Carbon fiber monocoque chassis. ...
... Racing car with a Carbon fiber monocoque chassis.[13] ...
Thesis
Composite materials reinforced by carbon and/or glass fibers offer a set of attractive properties such as high strength and stiffness, excellent corrosion resistance and improved fatigue properties, making them suitable for a variety of structural applications. The use of these composites is becoming critical for applications where the structures may be subjected to dynamic loading conditions. Therefore, it is important to investigate the effect of strain rate on the mechanical response of these lightweight composite materials when subjected to dynamic loading conditions. In this thesis, woven carbon and glass fiber reinforced composites based on an epoxy matrix were tested under tensile loading using a screw-driven Instron universal testing machine, a high-speed servo-hydraulic MTS test system and an in-house pneumatic system in order to achieve strain rates of 0.0025 s-1, 0.25 s-1, 10 s-1,100 s-1, 500s-1 and 1000s-1. Furthermore, to investigate the mechanical behavior of these materials under such loading conditions a high-speed DIC (Digital Image Correlation) system was also used consisting of two high-speed cameras capable of recording over 200,000 frames per second. Experimental results revealed that these materials maintained their high strength properties even under high strain rates and could be the material of choice for lightweight structures that may be subjected to dynamic loading conditions. Furthermore, the high speed DIC system revealed local and global strain distributions within the woven composites highlighting their failure mechanisms.
... Several studies have been carried out in the past decades to understand the behavior of composite materials during crash and to compare different materials. Even though at present a wide literature on crash mechanisms (Thornton (1979); Farley and Jones (1989); Hull (1991)) and design of energyabsorbing elements (Bisagni et al. (2005); Heimbs and Strobl (2009);Dalli et al. (2020); Obradovic, Boria, and Belingardi (2012); Lescheticky, Barnes, and Schrank (2013)) is available, comparing different studies is a hard task because of the absence of a standard for testing composite materials in crash conditions (Feraboli, Deleo, and Garattoni (2007)). ...
Article
The effectiveness of composite materials in crashworthiness applications is well-known in the literature. In most cases, the Specific Energy Absorption (SEA) of composite structures is higher than that of metallic structures, but at present there is no standard available to characterize their crash behavior. A new fixture to test flat composite samples in in-plane impact conditions has been used to investigate the effect of the impact speed and of the friction on the SEA of carbon fiber/epoxy flat plates. Tests have been carried out in impact conditions. The effect of the friction has been studied varying the clamping force given by the fixture. The force-displacement curves have been acquired in all tests and used to calculate the SEA of the material. The tested specimens have shown a splaying failure mode and values of SEA that increase with the clamping force given by the testing fixture.
... The lightweight design will improve the vehicle acceleration performance and fuel economy [6]. An attenuator must be specially made to absorb the collision's energy-namely the vehicle's kinetic energy -and reduce the driver's deceleration acting [7]. The technical requirements of an attenuator are that: 1. ...
Article
Full-text available
The impact attenuator is an essential system in both race cars and urban vehicles. The structure of an impact attenuator serves as a safety barrier between the impacted surface and the driver in an accident. Attenuator materials tend to have a high price; thus, alternative materials were explored in the current work, i.e., used cans from food and beverage containers. The study deployed a nonlinear finite element algorithm to calculate a series of impacts on the attenuator structures. The thickness of the cans and velocity of the impact were considered as the main parameters. Analysis results concluded that the attenuator's average energy was 16,000 J for a can thickness of 1 mm. This value is more than two times the 0.5 mm thick used cans. The attenuator's new design was then matched with an attenuator regulation, and the results surpassed the standard value of 7350 J.
... At the same time, the determination of an optimal design in the case of composite structures can represent a rather complicated task, since it does not only depend on the inherent complexity introduced by the adoption of composite materials with their own anisotropic properties, but also on the possible complication due to the components' geometry. For instance, in [5] the Ansys Finite Elements (FE) code was used on composites structures to investigate the effect of a frontal impact in the case of a F1 racing car. ...
Article
The effects of vibrations in vehicles range from simple noise and reduced comfort, to decreased performance, from wear and material fatigue to irreversible failures and danger. A study of the dynamic behaviour of reinforced composite panels is here presented, applied to the construction of an ultralight photovoltaic roof in the case of a solar sport car. This is an extreme race prototype where design and materials solutions, as high strength carbon fiber reinforced polymers and sandwich-structured composites, were addressed to optimize the stiffness-to-weight ratio. A modal analysis was performed considering materials anisotropies by a layered-shell finite element model and through-the-thickness integration points with the scope to discretize the multi-layered sandwich structure. Additional aspects, as gravity force and external constrains, were also included. Experimental evidences were used for validating the numerical model and underscored an outstanding accuracy. The same design procedure was finally applied to change the preexisting structural solution achieving an optimized roof that was manufactured, installed and tested.
... Finite Element (FE) modeling of honeycomb structures have been performed using a detailed representation of the hexagonal cells by shell elements [7,17] or by an orthotropic solid continuum based on its homogenized elasto-plastic properties [18][19][20][21]. ...
Article
Full-text available
A honeycomb impact attenuator for a Formula SAE (FSAE) prototype vehicle is examined using both experimental and numerical analyses. Two common FSAE impact attenuators were compared to a new design concept, combining four layers of hexagonal honeycomb. The comparison aimed to obtain the combination of the lowest mass and highest energy absorption. The attenuator must comply with both the FSAE championship rules and further internally-defined design constraints. The work continues addressing the numerical-experimental correlation of the applied materials. Finally, the finite element models for virtual crash testing are presented and were validated through the experimental tests.
Article
Full-text available
The objective of this paper is focused on detailed analysis of the crash behavior of the Impact attenuator structure that was designed to equip the formula SAE car is presented. The design of the energy absorbing structure has to allow a progressive force evolution, avoiding force peaks (i.e. deceleration peaks). It is very important to design impact attenuators in order to protect the driver from any serious wound, in case of any mishap. The impact attenuator serves dual purpose, it protects the race car structures as well as the driver. It absorbs the crash energy in a controlled manner, thus offering the required protection. So, the goal of crashworthiness is an optimized vehicle structure that can be absorbed the crash energy by a controlled vehicle deformations while maintaining adequate space so that the residual crash energy can be managed by the restraint systems to minimize crash loads transfer to the vehicle occupants. This paper is dealing with the study of different material for impact attenuator using honeycomb structured sandwich panel and its analysis by using Hypermesh and explicit solver LS-DYNA. The results of this paper show that the impact attenuator absorbs the total kinetic energy at the time of collision.
Article
The diffusion of fiber reinforced plastics in crashworthiness applications is continuously growing thanks to the excellent balance between high mechanical performances and low weight, resulting in most cases in a Specific Energy Absorption (SEA) of composite structures higher than that of the corresponding metallic structures. In this paper, a new fixture to test composite plates applying an in-plane load has been used to investigate the effect of the impact velocity and of the friction caused by the fixture on the SEA of carbon fiber reinforced epoxy plates. The tests have been carried out using a drop tower testing machine and the effect of the friction has been studied varying the clamping force given by the fixture. Splaying is the main failure mechanism found in the specimens during the tests; SEA values (43.6 kJ/kg in average) increase with the clamping force due to the higher friction level induced by higher clamping force; impact velocity does not significantly influence the results. To avoid an overestimation of the SEA due to the excessive friction force (+5.6% when the clamping force increases from 0.8 kN to 8 kN), a Polytetrafluoroethylene (PTFE) coating has been applied to the anti-buckling supports to reduce the friction. The effect of this modification has been studied by carrying out a new test in which the specimen slides between the anti-buckling supports with a given clamping force. A significant reduction (-48% with same clamping force) of the friction force is obtained when the lubricant is applied.
Article
A constitutive damage model is proposed in order to investigate the crushing response of crossply and 0 ° plies composite laminates, using a VUMAT subroutine implemented in ABAQUS/Explicit. This damage model predicts five failure modes commonly observed in unidirectional (UD) carbon fibres reinforced composite structures: fibre failure in tension, fibre failure in compression, matrix cracking in tension, matrix cracking in compression and in-plane shear failure. Its formulation is based on an energy framework which combines stress-based fracture mechanics and damage mechanics approaches within a unified way, enabling the prediction of the five failure modes aforementioned in terms of damage initiation and damage propagation. In this work a new fibre kink formulation is proposed taking into account the stresses degradation on the matrix fracture plane inside the kinking band. An experimental test campaing is proposed for verification of the numerical models. Additional comparisons between predictions obtained using the proposed model and experimental results taken from the open literature are also presented and discussed. An overall good correlation between numerical predictions and experimental data, taken from literature and in-house experimental results for wedge-shaped tip composite, was obtained.
Chapter
Full-text available
An overview over recent progress in the numerical simulations of composite damage is presented. The paper first concentrates on failure criteria for fiber-reinforced composites, indicating various failure mechanisms to model the post-failure behavior. Computational aspects for the crash worthiness analysis of laminated composite shell structures under low velocity impact are given next. Numerical results for the axial crushing of composite tubes and conical shells are presented and compared to experimental investigations. Finally the limits and merits of the implemented material and shell models are discussed.
Conference Paper
Full-text available
An approach for modeling sandwich structures with a Nomex® honeycomb core and phenolic composite faces in the commercial finite element code LS-DYNA with solid elements for the core and shell elements for the thin faces is presented, which accounts for the major sandwich failure modes. Extensive material testing was conducted to determine the parameters for the composite face material model and for the orthotropic honeycomb material model. Strain rate dependency of the material parameters as well as face-to-core debonding phenomena were also investigated and included in the model. In order to design aircraft interior components for dynamic loads, finite element models of lateral and center bins of a widebody aircraft cabin were created and simulations of different load cases were performed. A good correlation to experimental dynamic test results could be achieved.
Article
Full-text available
In this paper, we have used finite element method to study the quasi-static axial crush behaviour of aluminium-composite hybrid tube containing filament wound E glass-fibre reinforced epoxy over-wrap around an aluminium tube. The fibre orientation angle in the overwrap was ±45° to the tube axis. A modified Chang-Chang failure model was used for the composite layers. The effects of adhesion and friction between the aluminium tube and the composite overwrap were examined. Excellent correlation was observed between the numerical and experimental results.
Article
The energy absorption and failure behaviour of composite structural parts under crush load will be discussed. It will be focused on crush elements with double hat geometry. Double belt press and stamp forming technique have been chosen for economic industrial scale manufacturing of thermoplastic composite parts. Various specimens with different fibre/matrix combinations have been tested. Their crush behaviour has been compared to thermoset composite parts. The paper points out the good crush behaviour and energy absorption capacity of composite parts with thermoplastic matrix systems. A first approach to numerical crush simulation of thermoplastic composite structures is presented and discussed. The philosophy beyond this paper is to provide a system solution for the development of crush worthy structures.
Article
General Motors Corp. has studied the impact mechanics of composite structures used in Indianapolis-type cars and has evaluated alternative side-panel designs for injury reduction. To assess the effect of several proposed countermeasures, engineers have developed a drop-tower impact test procedure for assessing the performance and damage of composite race car structures in localized impacts by the wheel. Peak normal loads measured were between 25 and 35 kN. Results showed that wheel penetration into the cockpit occurred with a peak lateral acceleration of 3 to 4 g for a 900 kg combined mass of race car and driver. Good correspondence was observed between the damage induced by the test procedure and that observed in motorsport vehicle side impacts involving wheel penetration into the cockpit.
Article
A progressive damage model is presented for notched laminated composites subjected to tensile loading. The model is capable of assessing damage in laminates with arbitrary ply-orientations and of predicting the ultimate tensile strength of the notched laminates. The model consists of two parts, namely, the stress analysis and the failure analysis. Stresses and strains in laminates were analyzed on the basis of classical lamination theory with the consideration of material nonlinearity. Damage accumulation in laminates was evaluated by proposed failure criteria combined with a proposed property degradation model. A nonlinear finite element program, based on the model, was developed for lami nates containing a circular hole. Numerical results were compared with the experimental data on laminates containing an open circular hole. An excellent agreement was found be tween the analytical prediction and the experimental data.
Article
In recent years a new application for advanced composite materials has been in the construction of load-bearing components for Formula 1 racing cars. Their use has been progressively extended and they currently comprise a major part of the vehicle assembly for all competing Formula 1 designs. Here the experiences gained with these materials at Williams Grand Prix Engineering are described. The initial interest in this technology was for optimization of structural efficiency. A wide range of component design criteria are covered and advantages have also been found in the areas of strength, impact performance, geometric accuracy and speed of manufacture.
Article
This paper describes the CAE predictions and verifications performed whilst investigating the response of a low volume, niche market spaceframed British sportscar to a standard frontal impact test. In considering the options for crashworthy design solutions, it was essential to understand and have confidence in the complex crash behaviour of the standard vehicle. A detailed knowledge of the construction and ‘real world’ observations have led to the simulation of a complex and highly nonlinear response including rapidly changing contact surfaces and tyre compression. An experimental test programme supported the finite element predictions and included the impact testing of typical brazed tubular structures and an automotive wheel and tyre.