Development and Validation of an Ncap Simulation Using Ls-dyna3d

This paper describes a finite element computer simulation of a New Car Assessment Program (NCAP) full scale crash test. The full scale test selected for this study is a 30mph frontal impact of a 1993 Ford Taurus vehicle into a rigid flat wall. Finite element models of a Ford Taurus vehicle, a Hybrid III dummy, and a driver side airbag were combined to simulate the test. The vehicle, dummy, and airbag models are described in detail. The combined model validation against the full scale test is also presented. The combined model validation focuses on the comparison of the test and simulations in terms of crush depth in the front of the vehicle, the acceleration at different locations of the vehicle as well as the head and chest accelerations and the femur loads of the dummy. The simulation results are found to be consistent and in good agreement with the crash test data. Recommendations for further improvements of the model are also included in this paper. INTRODUCTION Computer simulations of vehicle collisions have improved significantly over the past few years. With advances in computer technology and non-linear finite element (FE) codes, full scale models and simulations of such sophisticated phenomena are becoming ever more possible. Finite element crash simulations have been primarily focused on the vehicle models and their crash characteristics. Recently, refined FE models of airbags and dummies have been added to the simulations. This allows direct evaluation of occupant risks and injuries using simulation data. In this paper, the development and validation of a FE model that incorporates a Ford Taurus vehicle, a 50 percentile Hybrid III dummy, and a driver side airbag models are presented. This FE model is used for the simulation of a frontal impact with a full rigid barrier using LS-DYNA3D crash code. A full scale crash test of a Ford Taurus impacting a frontal flat barrier at 30mph speed was used to validate the combined model. The model validation concentrated on the quantitative comparison of the test and simulation in terms of crush depth in the front of the vehicle, the acceleration at different location of the vehicle as well as the head and chest accelerations and the femur loads of the dummy. The simulation results are found to be consistent and in good agreement with the crash test data. Some deficiencies of the model were discussed and recommendations for the future improvement were also provided. FINITE ELEMENT MODEL The combined FE model used for the simulation of the NCAP full-scale crash test consists of a frontal-impact vehicle model, a Hybrid III dummy model, and a drive side airbag model. The following section describes the development and details of the three models. While the validations of the individual models are only discussed in brief, the full description of the validations can be found in their corresponding references. Vehicle Model Description The vehicle FE model used for the simulation is based a 1991 Ford Taurus. It was developed by EASi Engineering for the National Highway Traffic Safety Administration (NHTSA). Figure 1 shows the vehicle model of the Ford Taurus. The hood was removed in Figure 1 to display the detailed mesh of the front portion of the vehicle. Initially, the model was developed and validated for a frontal impact into a flat rigid wall, consequently the frontal portion of the vehicle was modeled in details while the center and rear of the portions were modeled with a coarse mesh or beam elements. Since the central and rear portions of the vehicle do not undergo significant deformations in such impact, modeling these parts of the vehicle with coarse mesh or beam elements does effect the accuracy of the results as long a the overall mass distribution and inertia of the model are consistent with those of the actual vehicle. Figure 1. Vehicle Model. The vehicle model is subdivided into 123 parts. Each part represents a component in the vehicle. Out of the 123 parts, 104 parts are used with shell elements to model the sheet metal components, 18 parts are assigned beam elements to represent the steel bars in the vehicle along with some of the connections between the sheet metal components, and one part is used with brick elements to model the radiator. Two types of shell elements are used in the model, quadrilateral and triangular. The formulation for both shell types is based on the Belytschko-Tsay shell theory which is the default shell formulation in LSDYNA3D. The material model assigned to these shell elements is a general isotropic elastic-plastic material (material type 24 in LS-DYNA3D). The stress-strain relation for the isotropic elastic-plastic material is defined with eight stress versus strain points. The beam elements in the vehicle model are based on Hughes-Liu beam formulation and use the isotropic elastic material model (material type 1 in LS-DYNA3D). The solid elements, are assigned material type 26, metallic honeycomb, and use the constant stress solid element formulation. The FE vehicle model components are connected to each other using the spot weld and rigid body constraint options in LS-DYNA3D. A total of 142 spot welds and 178 rigid body constrains are used in the model. The contact and friction between the components are modeled with one single surface sliding interface type 13; also known as automatic contact for beam, shell, and solid elements with arbitrary segment orientation. A summary of the FE vehicle model is listed in Table 1. Table 1. Vehicle Model Summary. Number of Parts 123 Number of Nodes 26,741 Number of Shell Elements 27,874 Number of Brick Elements 341 Number of Beam Elements 140 Several modifications were made to improve the vehicle model crash characteristics. The modified model was validated for several crash configurations using full scale crash test data. In this application, the model was further modified in order to incorporate the dummy and airbag models. The first modification involved adding a driver side seat and a dashboard for the purpose of accommodating the dummy. The geometry of these two components were obtained from a Ford Taurus vehicle. The newly added components were connected to the rest of the model components by merging coincident nodes and using rigid body constraints. The second modification consisted of replacing the original steering column, which was modeled with beam elements, with a more realistic one. The new steering column was connected to the rest of the model using the rigid body constraint option. The third modification entailed adding seven accelerometer models at the same locations and with the same orientations as of full scale test accelerometers. Dummy Model Description The dummy model used in the simulation is based on a 50 percentile Hybrid III. The model was developed and validated at the National Crash Analysis Center for application of injury assessment as shown in Figure 2. The components of the thorax and neck assemblies are modeled with flexible parts. The other components of the dummy are modeled with rigid body parts. The geometry of the different components of the dummy was obtained from design drawings of the Hybrid III. The overall mass as well as the mass and inertia of each component of the dummy match those of the 50 percentile Hybrid III. The joints at the ankles, knees, hips, shoulders, elbows, and wrists are modeled with spherical or cylindrical rigid body joints. Each rigid body joint is given properties that simulate those of the actual dummy. Table 2 shows the model information of the dummy. Figure 2. Dummy Model. Three experimental tests were used to validate the dummy model. The first test was a chest pendulum test and was used to validate the thorax assembly. In this test the dummy thorax was impacted with 150 mm diameter pendulum. The pendulum mass was 23 kg and its initial speed was 6.7m/s. The chest accelerations and deflections from the test were compared to the simulation and were found to be in good agreement. The second test was a head-neck pendulum test and was used to validate the dummy neck. In this test, the head an neck of the dummy were mounted at the free end of the pendulum. The pendulum was given an initial speed then subjected to a sudden stop. The neck and head responses were recorded. The third test was a full scale frontal impact into a flat wall test. This test was used to validate the overall kinematics as well as the chest and head accelerations of the dummy model. Table 2. Dummy Model Summary. Number of Parts 50 Number of Nodes 14,200 Number of Shell Elements 7,576 Number of Brick Elements 4,479 Airbag Model Description The airbag FE model was based on a Ford Taurus airbag. It was developed at the National Crash Analysis Center for the purpose of evaluating the interaction between the airbag and out-of-position occupants. The airbag chamber, the flaps, and steering wheel were digitized from a Ford Taurus vehicle. The airbag fabric was folded in a similar manner as the actual airbag using the PATRAN pre-processor. The airbag fabric folding pattern included 12 folds and a total of 56 layers of fabric stacked on top of each other . Special care was taken to ensure that there is no penetration between these layers especially at the corners where two or more folds intersect. Figure 3 shows the airbag model at three different stages of deployment. Figure 3. Airbag Model. The airbag fabric was modeled with membrane shell elements. The elements were assigned LS-DYNA3D material type 34 which is specifically formulated for fabric material under large deformations. The steering wheel and airbag chamber where modeled with shell elements and were assigned elastic materials. The airbag gas dynamics are modeled with the simple control volume formulation in LS-DYNA3D which is based on Cauchy’s first law of motion and ideal gas laws. The inflator characteristics are defined by a curve of the input mass flow rate versus time. The FE airbag model was validated against a test of an actual deployment of a Ford Taurus airbag. The validation consisted of comparing simulation pictures to the test high speed camera pictures at different stages of the deployment. In addition, motion analysis of the high speed film was performed to approximate the airbag volume at different times of the deployment. The motion analysis data and the simulation results correlate well. Table 3. Airbag Model Summary. Number of Parts 8 Number of Nodes 4,724 Number of Shell Elements 4,588 VEHICLE CRASH TEST The finite element model presented in this paper was validated against a frontal impact full scale crash test. The test was performed by the Transportation Research Center Inc. for the U.S. DOT National Highway Traffic Safety Administration under contract No. DNTH22-90-C-21003. The test involved a 1993 Ford Taurus 4-door sedan vehicle impacting a flat rigid wall. The vehicle gross weight was 3799 pounds (1725kg) and its initial speed was 30mph (48.3km/hr). Seven accelerometers were mounted on the left rear seat cross-member, right rear seat cross-member, top of the engine, bottom of the engine, right brake caliper, left brake caliper, and center of the instrument panel to measure the longitudinal accelerations of the vehicle at these locations. The vehicle included two 50 percentile Hybrid III dummies in the front driver and passenger seats. The dummies were restrained with only the airbags, the seat belts were unbuckled. Both dummies were instrumented with accelerometers at the head and the chest and with load cells at the right and left femurs. A SAE 60Hz filter was used to process all the measurements of the crash test. COMPUTER SIMULATION The simulation was performed on a Silicon Graphics Power Challenge XL super computer with 10 parallel processors. The Symmetric Multi-Processor (SMP) version of LSDYNA3D, version 936, was used. The case was run for 150 milliseconds of simulation time on 4 processors with a fixed time step of 1 microseconds. The total computation time required for the run was 35 hours. LS-DYNA3D accelerometer models were placed at seven locations in the vehicle as well as the dummy head and chest similar to the full scale crash test. In addition, the loads from both dummy femurs were outputted for comparison with the full scale load cell measurements. The simulation output data were also processed using a SAE 60Hz filter. Figure 4 shows a side view of the model at different stages of the simulation. A far and close-up views are shown side by side at each simulation stage. MODEL VALIDATION The fidelity and accuracy of the simulation can be evaluated both qualitatively and quantitatively. In general, qualitative evaluation examines the comparison between the test and simulation in terms of general crush profile in the impact zone, crash characteristics of main components in the model, and post-crash rigid body motion of the vehicle and dummy, while quantitative evaluation focuses on the comparisons of acceleration and impact load of various positions of the vehicle and dummy. The qualitative and quantitative comparisons are discussed in the following two sections. In the first section, the vehicle data collected during the test is compared to the corresponding results from the simulation. In the second section, the dummy full scale test data are compared to those obtained from the simulation.