Methodology for Validation and Documentation of Vehicle Finite Element Crash ModelS for Roadside Hardware Applications

 

ABSTRACT

Researchers involved in finite element method (FEM) crash simulation of Roadside Hardware need efficient, validated FE models of vehicles. The National Crash Analysis Center (NCAC) funded by the US Department of Transportation have been developing and releasing to the public domain numerous vehicle FE models. These models are modified and combined with other models to develop specific simulation scenarios. Users of the models regularly make modifications to the basic vehicle model according to their particular simulation requirements. A cooperative effort between the National Transportation Research Center (NTRC), Oak Ridge National Laboratory (ORNL), Battelle, and NCAC was initiated to explore the possibility of updating and enhancing the kinematic and structural accuracy of these basic vehicle models. This document outlines the methodology used in evaluating, validating against experimental data and updating NCAC's Ford F800 Single Unit Truck FE model. A new Hypertext Markup Language (HTML)-based documentation has been developed to facilitate the model adoption and understanding of prospective users. The overall methodology used by the participants - from evaluation to validation to documentation - is outlined here can be applied to other basic vehicle FE model currently available to users, and in our opinion could further facilitate crashworthiness research.

 

INTRODUCTION

It has become a standard practice in roadside hardware research to evaluate new and existing designs with computational simulations using large and complex models based on the Finite Element Method (FEM) [1].

Building a FE model of an entire vehicle of any kind is a considerable undertaking. A significant technical expertise and FEM tradecraft is needed to develop a computationally feasible and practical model that replicates the main kinematics of the vehicle and the deformation response due to the impact loads.

The most challenging aspect of model development is the constant tradeoff between the real world complexity of the vehicle and engineering simplification of its model that should not compromise the final goal of a sufficiently accurate model suited for its purpose. This tradeoff process evolves with advances in computing and, therefore, the already developed models may need to be updated not only to remedy some of their drawbacks, but also to bring them up to the ever-improving levels of computational capabilities.

A FE model of a representative Single Unit Truck (SUT) was developed by the FHWA [2]. The model has been released to public use and has been used for numerous computational studies of roadside hardware. The model's primary purpose is to be used as a bullet object for computational evaluation of road safety hardware, and as such it does not warrant the complexity ordinarily employed in vehicle crash analysis models. In fact, too much complexity in a bullet model may be detrimental to its primary purpose because of an increased computational burden and structural failures in the bullet that may overshadow the target's response. Therefore, possible modifications of the vehicle model must always be evaluated within the context of the roadside model development.

The objectives of this research were to conduct an evaluation of the SUT model with respect to its ability to accurately simulate its interaction with roadside safety hardware, to identify areas of possible improvements based on comparison of simulations with crash experiments, and consequently modify and update the model to improve its accuracy and take advantage of current advances in FEM.

To be able to use the model efficiently and appropriately, a prospective user has to understand its structure and modeling decisions made during its development. The traditional user's manual format is not very effective for describing a three-dimensional model, the interconnections between different parts and their participation in different sub-modeling entities. Therefore, a long lead-time is necessary for a new user to be able to use the model with sufficient confidence to know that the perceived impact configuration is indeed the modeled one. We have developed an interactive, web-based User's Manual of this vehicle FE model to simplify this learning process and make the model more transparent to new users.

This vehicle model is fairly well suited to its purpose as a bullet vehicle. For example, on a 2-cpu 1.8 MHz. Dell workstation with the Linux operating system, the truck-model-only run time using LS-DYNA 970 [3] was 2 hours 40 minutes clock time to run 226 milliseconds of simulation time. The nominal time step was about 4 microseconds. This appeared to be a good trade-off between mesh refinement and speed.

 

Representative Single Unit Truck for Roadside Hardware Analysis

Due to practical considerations in roadside hardware analysis, the number of vehicle FE models used and developed is limited. The process involves selection of a representative vehicle for each vehicle class, and developing respective FE models. Therefore, the model and available experimental data may not always coincide but it is assumed that the differences in the structural behavior between models of the same class are negligible with respect to the roadside hardware response and performance. The Ford F800 Series Truck was selected as representative of the SUT vehicle class. The available experimental data for the SUT category were obtained using a variety of similar size trucks including; GMC, Chevrolet, Freightliner, and International. The vehicle is ballasted to the correct weight for the test level requirements.

A cursory inspection of several makes and models of SUT's at a truck dealership revealed generally more similarities than differences. The chassis were all parallel-rail frame types with front and rear leaf spring suspension. They all had V-8 diesel or gasoline engines, and all had dual-wheel rear axles. The cargo bodies are mounted on a series of lateral C- or I-Beams which are welded to C-Channels that run parallel and directly atop the chassis main frames. There typically is a wooden member as a buffer between the Parallel C-Channels and the main chassis frame rails. Large U-Bolts fasten the Cargo-body C-Channels to the chassis main rails. The GMC 7000 SUT used in the TTI test 7147-17 was typical of this design and had an empty weight of 11470 lb. The NCAC F800 Model was also of this general design and had an empty weight of 11051 lbs.

 

Outline of the SUT Model Analysis Process

The analysis of the SUT model was conducted on evolving model versions as they were being developed by NCAC. The initial analysis of the model resulted in several suggestions and modifications that were subsequently implemented by the NCAC. The evaluation of the early versions of the SUT model consisted of the following steps:

 

• Preliminary evaluation of the SUT models using FEM simulations
• Comparison of the simulations with the crash experiments
• Identification of the model areas critical for its performance in roadside hardware analysis
• Analysis of the SUT service manuals with respect to FEM modeling approaches
• Analysis of the SUT model material models
• Analysis of the connectivity and joint models
• Analysis of the suspension and its possible failure modes
• Model modification - analysis of the new results and recommendations for updates in the model

 

The analysis and simulations of the early model versions lead to recommendations for the model updates that were later implemented by the original developers. The updated model was then used as a platform on which the final analysis and modifications were performed.

 

SUT Material Models

Even the FEM models with large numbers of elements will not be able to produce realistic results without realistically modeled material behavior. One of the important areas of the SUT model update is the implementation of more detailed material model assignment and material properties. An exploded view of the SUT parts that are assigned materials is shown in Figure 1.

 

Figure 1 SUT computational parts

 

The vehicle is built on a main longitudinal rail structure that acts as its backbone. It is therefore important to accurately model the geometry and the material of the rails. The material of the rails is specified in the Service Manual as the High Strength Low Alloy (HSLA) steel of yield point 350 MPa. The material data available from the Auto/Steel Partnership [4] and American Iron and Steel Institute [5] was used to enhance the existing material model.

The new material model includes the effects of strain rate sensitivity, which is very important in steels. Mild low-carbon steel (DQSK) is primarily used in body structures and, by volume, constitutes the largest part of the vehicle. The new model also adds a strain rate sensitivity effect. Other significant material models implemented were the SAE 5160 bracket and spring steel, SAE 1541 forged axle steel, Hot Rolled bumper steel and medium Carbon alloyed SAE Grade 8 steel for nuts and bolts. Parts made of each of these materials can be interactively viewed using the Virtual Reality Markup Language (VRML) version of the documentation.

The most commonly used approach to modeling strain-rate sensitivity of steels in automotive crash simulations is to use isotropic plasticity models with a rate sensitivity component that has moderate requirements on the experimental program. The types of material models that are frequently used are the Johnson-Cook model [6], the Zerilli-Armstrong model [7] and the piecewise linear strain rate sensitive material model [3]. The models are appealing because they have been implemented in commercial codes used for crash simulations and have a relatively small number of material parameters that must be determined by experiments.

The most commonly used strain rate dependence material model in crashworthiness simulations of steel structures is the piecewise linear plasticity model. In this approach, effective strain-stress curves from experiments are directly used in the computational material models and require the least amount of effort for material model development. In simulations, for a given rate of strain, the resulting stress in the plastic region is linearly interpolated between the stress-strain values that were experimentally determined in strain rate tests.

The computational model fits experimental data exactly, but whatever testing artifacts or errors are contained in the experimental data will be carried over to the simulations. The highest strain rate in the experimental data acts as a saturation plateau for strain rate effects. The strain rate dependent model for the HSLA 350 steel used in the main rails of the SUT were developed by the Auto/Steel Partnership [4] and are shown in Figure 2. The dashed curves show the results from the quasi-static uniaxial tensile experiments.

 

 

Figure 2 Material parameters for HSLA350

 

 

 

Vehicle – Infrastructure Asset Interaction

An FHWA-funded study was undertaken by Battelle and ORNL to model and assess different scenarios of truck vehicle run-off-road collisions with roadway infrastructure elements, vehicle structural modes of failure, and subsequent vehicle stability. The focus of this work was to identify areas of the NCAC Ford F800 Single Unit Truck (SUT) model that was available at the time that could be improved to make it more immediately useful as-downloaded from the NCAC Finite Element Model archive. To accomplish this, Battelle worked with Oak Ridge National Laboratory, the FHWA-sponsored National Crash Analysis Center (NCAC) and other Centers of Excellence (COE) in Finite Element Crash Analysis.

The vehicle model improvement study focused on impacts with rigid barriers because this kind of test captures the vehicle model behavior rather than the barrier response. Several simulations were run by Battelle and ORNL during the course of this work and a number of vehicle model improvements were suggested and implemented. The procedure that was established to validate and verify the SUT model also will provide the methodology for validation and verification of other heavy-vehicle models currently under development at NCAC.

The experimental data collected on Single Unit Truck (SUT) came from full scale tests performed by the Texas Transportation Institute (TTI). The crash analysis simulations of the Texas Transportation Institute (TTI) Crash Test No. 7147-17 – SUT impacting Single Slope Concrete Bridge Rail, were performed. The crash test vehicle was an 18,000 lb. GMC 7000 Single Unit Truck (11470 lb curb weight plus 6530 lb ballast load). The vehicle was impacted into a single-slope bridge rail at 51.3 mph, at an impact angle of 17.9 degrees

Figures 3 through 5 show (in very abbreviated form) of the general level improvement achieved in this vehicle model's fidelity. Figure 3 shows one snapshot in time (0.672 seconds after impact) from the crash test experiment. Figure 4 shows the original vehicle model's response at 0.672 seconds after impact and Figure 5 shows the improved model's response at 0.672 seconds after impact.

 

 

 

 

Figure 3 TTI Test at Time = 0.672 Seconds After Initial Impact

 

 

Figure 4 Original F800 SUT Simulation at Time = 0.672 Seconds After Initial Impact

 

 

 

 

Figure 5 Improved F800 SUT Simulation at Time = 0.672 Seconds After Initial Impact

 

 

SUT Model Documentation

Vehicle and roadside hardware FEM models from DOT and NCAC are available in public domain so that they can be modified and combined with other models. The availability of verified FEM models greatly facilitates research in the transportation field. Perhaps the biggest obstacle in adoption of the FEM models is their complexity and the respective startup time before they can be confidently used in new impact scenarios. Since the computer simulations are very tolerant to modeling errors, even the verified FEM models can be inappropriately used if they are not fully understood.

Ever increasing computing capability leads to correspondingly larger and more detailed FEM models so that the written documentation cannot efficiently convey the model's structure and development considerations and keep up with inevitable model updates. One of the objectives of this research was to introduce new internet-based technologies to the model documentation and presentation. The FEM vehicle modeling is inherently complex and three-dimensional so the ability to effectively view the model's information is very important.

To view the vehicle models, a combination of Virtual Reality Modeling Language (VRML) and Hypertext Markup Language (HTML) was used to build the Visualization Module of the documentation package. Additionally, the Visualization Module allows for easy access of other tools within the documentation package. Although new languages for three-dimensional computer environments have been proposed, VRML with all its limitations is still prevailing standard. A VRML file format is a plain text format that describes the shapes and their properties within a 3D world. This file only specifies objects and shapes within a virtual environment; it does not handle the navigation and the interaction. Moving through the world, rotating objects, and similar functions are handled through a VRML player, an application that displays the VRML file.

Other important considerations are the size of model documentation and the ability to efficiently transmit that information in today's network environment. The dynamics of computing development will inevitably lead to faster networks and better ways of model presentation, but it is reasonable to expect that they will be based on three-dimensional modes of data display. The VRML mode of interaction with the automotive crashworthiness models was also explored in Reference [8] and briefly reviewed below.

Vehicle geometry is converted into a VRML file by a Perl script that sorts the parts, assigns them positions and rotations, colors them, and assigns them appropriate behaviors. Due to this automated process it is possible to quickly export new versions of the vehicle model to VRML format and post them for viewing and analyzing on the World Wide Web. A virtual control panel constantly follows the user inside the VRML world (Figure 6). The panel allows the user to select individual vehicle parts, examine their mesh makeup, move, rotate, and eventually call up an information page about the part and further cross-referencing as its participation in different contact sets, element types, etc. The explode feature separates the individual parts, allowing the user to get a good idea about the interconnectivity of the vehicle (Figure 7).

 

 

 

 

Figure 6 VRML Interface to the Documentation

 

 

Figure 7 Exploded View with Selected Part

 

 

The name of the part and the subsystem it belongs to are also displayed in the control panel. By using this control panel, the user can easily navigate through the vehicle and gather information about it. The delete function allows the user to remove any parts that are obstructing the area of interest. This is a common occurrence - especially if user wants to examine a cramped area such as the engine compartment. Additionally, the user is able to examine a part's mesh composition by selecting it. These features are easy to add, delete, or alter, due to the object-oriented design of the VRML interface.

 

We have organized the model documentation in 5 categories

1. Part sets (subsystems)
2. Parts
3. FEM element types
4. Material models
5. Contacts

 

Other groupings are clearly possible (i.e. connectivity models) and can be added to the existing documentation.     

The part sets categories are selected based on their organization in SUT Service Manuals. The parts sets can be viewed in both HTML and VRML modes. The HTML documentation is programmed as the staring point due to the low data transfer requirement. As the user searches for more details, the VRML interactive environment is offered to clarify the details of spatial information.

 

SUMMARY

The main objectives of this research were to conduct an in-depth evaluation of the Single Unit Truck (SUT) finite element model with respect to its ability to accurately simulate its interaction with roadside safety hardware and to identify areas of possible improvements. The model's primary purpose is to be used as a bullet object for computational evaluation of road safety hardware. The modifications of the vehicle model were evaluated within the context of the roadside hardware model development.

            The analysis of the model and comparison between simulations and tests lead to recommendations for the SUT model modifications that were implemented by the original developers of the model, National Crash Analysis Center (NCAC) and participants in this project, Battelle, Oak Ridge National Laboratory and University of Tennessee. The goal of the project was also to establish a methodology for validation and verification of the finite element models used in roadside hardware analysis so that it could be applied to other vehicle finite element models currently under development.

The model and the project developments are documented in an HTML based environment that allows for dynamic visualization and interaction with the model. The user can view and analyze all the main components of the model and their interactions. The goal of the interactive 3D environment is to make the model more transparent to the end users and to facilitate transfer of the developed models and technologies to the end users.

Acknowledgements

This Heavy Vehicle Safety Research project was sponsored by the U.S. Department of Transportation/Federal Highway Administration under cooperative agreement #DTFH61-03-X-00030 with NTRCI.

Use of the supercomputers at the ORNL Center for Computational Sciences (CCS) is gratefully acknowledged.

Our thanks to Roger Bligh of the Texas Transportation Institute for his generous contribution of the experimental test data that was essential to this study

Our thanks to NCAC staff – Dr. Leonard Meczkowski, Dr. Dhafer Marzougui, and Dr. Cing-Dao (Steve) Kan for their continuing support, help and advice on this vehicle model.

 

References

 

1.     Belytschko, T., Liu, W. K., Moran, B., Nonlinear Finite Elements for Continua and Structures, Wiley, 2000.

2.     National Crashworthiness Analysis Center Model Archive, http://www.ncac.gwu.edu/archives/model/index.html, 2003.

3.     Hallquist, J. O., LS-DYNA3D, An explicit finite element nonlinear analysis code for structures in three dimensions, LSTC Manual, 1995.

4.     Mahadevan, K., Fekete, J. R., Schell B., McCoy, R., Faruque, O., Strain-Rate Characterization of Automotive Steel and the Effect of Strain-Rate in Component Crush Analysis, SAE paper 982392, 1998.

5.     Simunovic, S., Shaw, J., Aramayo, G., Material modeling effects on impact deformation of ultra light steel auto body, SAE Paper 2000-01-2715, 2000.

6.     Johnson, G. R. and Cook, W. H., A Constitutive Model and Data for Metals Subjected to Large Strains, High Strain-rates and High Temperatures, Proceedings of the Seventh International Symposium on Ballistic, The Hague, The Netherlands, 1983, pp. 541-547.

7.     Zerilli, F. J. and Armstrong, R. W., Dislocation-Mechanics-Based Constitutive Relations for Material Dynamics Calculations," Journal of Applied Physics V 61 (5), pp. 1816-1825, 1987.

8.     Bobrek, A., Simunovic, S., Aramayo, G., Collaborative Toolkit for Crashworthiness Research HICSS-34, Minitrack on Developing and Deploying Collaborative Problem Solving Environments 2001.