Vehicle Load Area Division Wall Integrity during Frontal Crash

Transcription

1 Vehicle Load Area Division Wall Integrity during Frontal Crash H. Türkmen TOFAS Türk Otomobil Fabrikasi A.S. Abstract : This study addresses design efforts of a vehicle load area division wall and the verification of its integrity under frontal crash conditions. One of the purposes of such an activity is investigating the performance of ABAQUS/Explicit. The test to be simulated is a High-g Sledge Crash Test, which comprises of accelerating the vehicle body with a velocity curve equivalent to that recorded in a full scale crash test with three standard blocks simulating cargo inside the vehicle. The load area has to contain these boxes within a specified intrusion value and without rupture of critical components. ABAQUS/Explicit has been used by TOFAS R&D throughout the project and results have been verified with those obtained by other colleagues using the existing explicit solver as well as physical tests themselves. Keywords: Load Retention, Division Wall, Occupant Safety 1. Introduction : This paper discusses analyses performed by TOFAS R&D Department in order to check the possibility of implementation of ABAQUS/Explicit for simulations of automotive crash applications. The case under investigation is the load retention test of a special version. This is a high-g sledge test where three blocks of specified size and mass collide with the load area division wall as the vehicle body with the mentioned blocks inside is accelerated with a time history equivalent to that of a full-scale frontal crash scenario. Also investigated for the first time with this activity is the FASTENER method used for modeling mesh-independent spotwelds, which might prove useful also for implicit analyses to be performed by TOFAS R&D Dept ABAQUS Users Conference 1

2 The simulation study has actually been launched after the initial design solution has been tested in the crash laboratory, in order to understand the shortcomings of the first design solution and investigate improvement possibilities. Therefore the steps for the activity have been defined as : 1. Construction of an FE model to represent the initial design solution, and performing the retention test model virtually, therefore obtaining a correlation of virtual test results with those of the physical test and validating the FE model. 2. Modeling and testing of different design modifications in order to help design people develop an improved final solution to perform better in the test. 3. Correlation of results obtained from virtual and physical tests for this final solution. As an outcome of such activity planning, results correlation has been performed twice with different configurations of the two solutions, therefore acting as a kind of double-check. The mentioned correlation has not only been checked between the results of ABAQUS/Explicit and physical test, but also between the results of the ABAQUS/Explicit and the established explicit solver. 2. Migration from ABAQUS/Standard to ABAQUS/Explicit : This study has been the first encounter of TOFAS CAE team, who hare already users ABAQUS/Standard, with ABAQUS/Explicit. Therefore it is important to note that the migration has been quite smooth, as the input file structure is almost identical to that of the ABAQUS/Standard, save for some specific details explained further in the following section. 3. Model and Analyses : 3.1 File Structure : BODY_IN_WHITE : the model of the body-in-white of the vehicle in ABAQUS format, previously prepared for other implicit analyses on the body. It contains around a total of elements. It is called by the launch file as it is, hence requiring no migration effort from Standard to Explicit. BOXES : the file that contains the 3 blocks of required dimensions and mass. (figure 1) DIVISION_WALL : the model of the load area division wall assembly as defined by the designers. This model, constructed only for this study, is prepared with a finer mesh with respect to that of the body, as it is the primary area of importance in the load retention test. It contains around a total of elements, exact element number depending on different design solutions. (figure 2) SPOTWELD : the file that contains the node definitions related to spotweld locations in the division wall model as well as the *FASTENER PROPERTY and *FASTENER definitions ABAQUS Users Conference

3 Therefore, once called, this file welds together the components of the division wall assembly. Fasteners have been divided into three sub-groups based on the total shell thicknesses of the components they are to join, and they have been assigned proper search radii values to detect the components in the proximity of the nodes. No additional components-to-connect information has been provided. MATERIALS : contains the material definitions. LAUNCH-FILE : This is the master file that calls all the others and manages the parameters of the analysis such as the type of analysis, time period of simulation, minimum allowed time increment size (so mass scaling), boundary conditions, contact definitions and output requests. (figures 3 & 4) Such file structuring allows modularity between Standard and Explicit analysis applications as the file containing bulk data can be called by either an implicit run or an explicit one. Furthermore it renders utilization of the standard blocks for different crash analyses easier. However, care is necessary for these files in order not to have coincident node or element numbers, which will cause errors later as the analysis is launched. 3.2 Elements : Sheet metal parts at any part of the models are modeled by reduced integration shell elements and structural adhesives are modeled by solid hexahedrons. Welds are modeled by two different approaches, as the classical node-to-node rigid connection method has been inherited with the model of the Body-in-White, and the components of the newly modeled division wall have been welded using FASTENER feature. It has been noted that ABAQUS had successfully handled this mixed approach. Each block geometry, after being discretized using shell elements, has been assigned a proper RIGID BODY definition in order to represent better their relatively higher stiffness with respect to the components of the body and the division wall. Their masses have been adjusted to the required value by adding lumped mass elements. 3.3 Materials : The definition of materials differs from the definition of non-linear material properties for an implicit analysis in the following ways : Utilization of a different unit system (kg-ms-mm) Definition of rate dependent stress-strain curves in the plastic zone by using additional *PLASTIC cards for the same material with the addition of RATE option indicating proper strain rate values ABAQUS Users Conference 3

4 3.4 Analysis parameters : The analysis procedure is DYNAMIC, EXPLICIT with a simulation time period of 150 ms. FIXED MASS SCALING has been used with BELOW MIN option so that the mass would be added only to the elements requiring time increment sizes less than ms. The minimum time increment size has been determined after a couple of trial runs to find a value that will yield a reasonable mass change in the model. With time increment size set to the aforementioned value, the change in total mass of the model is 0.2 %. Elements in the primary area of interest have been checked to ensure they do not get very high mass scaling values that could have significant effect on the results. (figure 5) Boundary conditions have been applied in the form of velocity as a function of time in the direction of acceleration on the sledge. The nodes on which the boundary conditions have been defined are displayed in figure 3. Contact definition has been made including all elements in the model, although the inclusion of only the components in the proximity of the collision area could also be sufficient. Abaqus has handled initial penetrations with success except a few points on the body where extremely large offsets have been encountered, but this situation has been related primarily to local poor modeling practices that could have been avoided using a more careful approach and with a finer mesh size. Good handling of the slight initial penetrations on the division wall, where the mesh size is finer, can be considered as a proof of this statement. 4. Results and Conclusions : The analyses have yielded results that are in correlation with the results of the physical test and those of the established explicit solver, therefore proving ABAQUS/Explicit to be a reliable tool in the simulation of crash analyses. (figures 6 & 7) The ease of migration from Standard to Explicit and possibility of using common FE models for very different simulation applications is another notable strong point. Further evaluation in terms of performance may be performed by simulating a full-scale crash test that will include complexities such as more varied material constitutive models, barrier and dummy finite element models etc. Following notes point out some of the lessons learned as well as additional improvement possibilities in the conduction of such study : During the test runs it has been noted that a node of the slave surface (representative division wall) was falling behind the convex master surface (block) after which the contact would be active, therefore practically sticking rigid block to the representative division wall at one node. In this study, this problem (also addressed in v6.4 Analysis User s Manual - Section ) has been ABAQUS Users Conference

5 overcome by using finer mesh in modeling the blocks. If the same problem might have been avoided by using a more detailed contact definition is worth verifying with further investigations. In order to shorten analysis times, only a portion of the body has been utilized for the first runs. However, due to excessive and unrealistic oscillations of the roof panel, whole body model had to be included instead of only a portion in the consecutive runs even if the body itself had not gone under notable deformation. As a solution to this, implementation of submodeling technique has been considered, where an initial run with the whole body-in-white could be followed by other runs necessary through the design iterations with much smaller portion of the body. However, the utilization of such technique has been left to be verified with another study. Bolted joints between the division wall and body have been modeled using rigid stars which do not convey information about the forces transmitted through such connections. However, it is also necessary to check these values to ensure the integrity of bolted joints under the loads caused by the impact. At the time of preparation of this paper, studies were still underway to check usability JOINT elements with proper ORIENTATION definitions at the connections. 5. References 1. Türkmen, H., Simulations of High-g Sledge Crash Tests with ABAQUS/Explicit, Internal report, ABAQUS Inc., ABAQUS Analysis User s Manual, Version 6.4, ABAQUS Inc., ABAQUS Keywords Reference Manual, Version 6.4, Figures Figure 1. Blocks with specified size and mass by the standard 2005 ABAQUS Users Conference 5

6 Figure 2. Division wall model Figure 3. Part of assembled model ABAQUS Users Conference

7 Figure 4. Nodes of boundary condition Figure 5. Element Mass Scaling Factor (EMSF) at t=0 ms ABAQUS Users Conference 7

8 Figure 6. Plastic equivalent strain distribution at t=150 ms. Figure 7. Relative displacement distribution at t=150 ms ABAQUS Users Conference