Progressive Failure Analysis of Thin-Wall Aluminum Extrusion - APSSDC

under the quasi static loading

Created on 2020.06.17 170 views
Objectives In this example problem we consider the overall deformation and failure behavior of a thin-wall, double-chambered aluminum extrusion under quasi-static three-point bending and dynamic axial loading conditions. The following Abaqus features are demonstrated Using ductile, shear, and Müschenborn-Sonne forming limit diagram (MSFLD) damage initiation criteria to study the initiation of failure due to three different mechanisms: ductile fracture, shear band formation, and necking instability, respectively. Modeling progressive failure of components using damage evolution and element removal. Application description New materials such as aluminum and magnesium alloys and high-strength steels are being introduced increasingly in automotive components to reduce weight and, hence, to increase overall vehicle performance. These materials typically have low ductility at fracture compared to traditional steels and may suffer damage and failure under crash loading conditions. A typical component made of sheet metal may undergo damage due to a number of mechanisms including void nucleation and coalescence, shear band formation, and necking instability. Thus, to obtain reliable predictions from crashworthiness simulations, it is essential to model damage initiation and progressive failure due to various failure mechanisms as well as modeling accurate plastic deformation behavior. Geometry The overall dimensions of the aluminum extrusion are L=500 mm, W=95 mm, and H=68 mm for the three-point bending case and L≈396.5 mm, W=95 mm, and H=68 mm for the axial crushing case. The thickness of the sheet is 2.5 mm for both cases. Materials The material used in this study is an extruded aluminum alloy EN AW-7108 T6. This material behaves in an elastic-plastic manner and can undergo damage due to either one or a combination of the following damage mechanisms, nucleation and coalescence of voids, shear band formation, and necking instability. Boundary conditions and loading The three-point bending configuration consists of the aluminum extrusion supported on two rigid cylinders and loaded in the transverse direction by another rigid cylinder (Figure 2.1.16–1). In the axial crushing simulation, one end of the aluminum extrusion is supported by a fixed rigid base and the other end is subjected to an instantaneous velocity by a planar rigid impactor. Abaqus modeling approaches and simulation techniques Two loading cases are considered. The first case consists of a quasi-static three-point bending configuration where the part is loaded transversely to the extrusion direction. In the second case the part is subjected to a dynamic loading in the axial (extrusion) direction. Summary of analysis cases Case 1 Quasi-static three-point bending simulation. Case 2 Dynamic axial crushing simulation. The sections that follow discuss the analysis considerations that are applicable to both cases. Mesh design The aluminum extrusion is meshed with a uniform mesh consisting primarily of 4-node shell elements. In the axial crushing case some 3-node shell elements are also used. The planar dimensions of the elements are an order of magnitude larger than the shell thickness. The simulations with this mesh yield results in agreement with the experimental observations. No mesh refinement studies were conducted. Initial conditions For the axial crushing simulation a velocity initial condition is specified at the reference node of the planar rigid impactor in the global 1-direction. Boundary conditions For the three-point bending simulation all the degrees of freedom at the reference node of the rigid supports are constrained. A velocity boundary condition in the global 2-direction is specified at the reference node of the rigid punch with all the remaining degrees of freedom constrained. For the axial crushing simulation all the degrees of freedom at the reference node associated with the rigid support are constrained. Furthermore, all of the degrees of freedom except that associated with the global 1-direction are constrained at the reference node of the planar rigid impactor. Loads The velocity boundary condition at the rigid punch applies the load in the three-point bending simulation. In the case of the axial crushing simulation the initial velocity of the planar rigid impactor loads the component. Constraints Rigid body constraints are specified in both cases to form element-based rigid bodies. These rigid bodies form the support and apply loads to the aluminum extrusion.   Discussion of results and comparison of cases The overall deformed shape of the aluminum extrusion obtained from the three-point bending simulation is shown, and the experimentally observed deformed shape is shown. The elements that have failed at the end of the simulation are presented, mapped into the undeformed configuration. Good qualitative agreement is seen between the simulation results and experimental observations. The load-displacement history of the punch obtained from the simulation is compared with three different experimental results. Again, a very good match is observed, indicating the reliability of the simulation results. . The overall deformed shape including the failure patterns obtained from the axial crushing simulation is uploaded. The deformed shape and the failure patterns are qualitatively similar to those observed experimentally. The overall force-displacement response from the simulation (filtered using the Butterworth filter with a cutoff frequency of 1500) is compared with the results from three different experiments. Again, a good qualitative match is seen, and the numerical results are within the experimentally observed scatter. In conclusion, the results from both the quasi-static three-point bending and the dynamic axial crushing simulations match the experimental data very well. It is also concluded that the use of progressive damage and failure is essential to capture the overall deformation and failure behavior of thin-wall aluminum extrusion.  
Discover the team
Who’s behind this project
sp sai vikas paruchuri
Discover the solution
Software used for this project
Project Timeline
Project Timeline