Prediction of B-Pillar Failure in Automobile Bodies
- Friday, 27 February 2009
Simulation of deformation, failure, and contact conditions help determine B-pillar quasi-static strength.
The B-pillar is an important load-carrying component of any automobile body. It is a primary support structure for the roof, and is typically a thin-walled, spot-welded, closed-section structure made from high-strength steels. As part of the validation process, the B-pillar can be experimentally loaded at quasi-static rates until failure. The force and displacement of the impactor are measured to get valuable insight into the stiffness characteristics of the structure. During the past two decades, crashworthiness simulation of automotive structures has proven to be remarkably good, largely because the finite element codes being used can accurately predict the plastic bending and stretching deformation mechanisms that occur in stamped metal parts.
Abaqus/Explicit simulation software was used to predict the onset and evolution of damage in ductile metals. The Müschenborn-Sonne forming limit diagram (MSFLD) damage initiation criterion allows for the prediction of necking instability in sheet metal. When combined with appropriate damage evolution criteria, sheet metal rupture initiated by necking can be captured in an Abaqus/ Explicit simulation.
The B-pillar failure test is not required by any federal regulations. The purpose of this test is to determine the load carrying capacity and stiffness of the structure, which is deliberately loaded to failure.
All sheet metal parts are modeled with small-strain shell elements for computational efficiency. Parts are joined together with mesh-independent spot welds. Turnbuckles, which constrain the vehicle body to the rigid floor, are modeled with truss elements. The experimental loading is applied quasi-statically, at a rate of 2 mm/s. An Abaqus/Explicit quasi-static analysis conducted in its natural time scale would result in an excessive run time. To increase the efficiency of the analysis, the loading event is accelerated by prescribing a velocity boundary condition of 2.5 m/s to the reference node of the rigid impactor.
A tensile load of 3 kN is applied to each turnbuckle in the first 10 ms to prestress the structure. To bring the structure into equilibrium, no load is applied on the B-pillar for the next 10 ms. The velocity boundary condition is then applied to the impactor. The impactor reaction force and displacement histories are monitored. General contact is defined for the entire model.
The material properties for all the sheet metal components are characterized by Mises plasticity with isotropic hardening. Three separate damage initiation criteria are used: ductile, shear, and MSFLD. Each damage initiation criteria has an associated displacement-based damage evolution criteria.
An initial simulation was done with only the shear and ductile damage initiation criteria; the MSFLD criterion was not included. A mesh of typical size used in crashworthiness analyses (characteristic element length of 6-8 mm) was employed. The force displacement curve from the simulation compares reasonably well with that from the experiment. However, in the absence of the MSFLD initiation criterion, the simulated structure does not fail completely and continues to carry load throughout the analysis.
In a second simulation using the same mesh, the MSFLD initiation criterion was included in the material model, so that all three initiation and evolution criteria were active. Representative Mises stress and equivalent plastic strain results show how the development of the crack initiation zone is captured by the simulation.
For extremely large displacement of the impactor, a mesh with regular element sizing does not capture the complete separation of the structure that is observed in the experiment. To evaluate the effect of mesh refinement on the crack propagation and failure, the region of the B-pillar where the crack initiates was re-meshed, with an average local element size of 1.5 mm.
The figure shows the separation of the B-pillar in the simulation with the refined mesh and in the experiment. The results with the refined mesh show improved correlation with the physical test. The results indicate that a mesh size of 6 to 8 mm is appropriate to predict the area of stress concentration and the crack initiation, but a refined mesh may be necessary to predict crack propagation accurately.
This work was done by Sridhar Sankar, Manager, Crash Engineering Specialists, and Biswanath Nandi, Crash Engineering Specialist, for Dassault Systemes SIMULIA Corp. For more information, click here.