3D crack propagation study of a railway component using XFEM method

This work develops a methodology to study the crack propagation through ABAQUS simulation. This simulation study uses the service condition of the mechanical component and the complex geometry of a manufacturing defect obtained by microtomography. It was concluded that the XFEM method is an essential tool in predicting crack propagation of a railway component. Furthermore, the type of criteria used in the XFEM method allowed the analysis of the propensity of the manufacturing defect to initiate crack propagation. The C3D4 elements were essential in realising the crack propagation simulation, considering a manufacturing defect. Having the pore’s complex geometry was crucial to developing the methodology presented in this study. The static analysis results indicated that the maximum stress concentration value in the pore is in a zone that can be identified as a hot spot. In addition, the pore showed a higher concentration of Von-Mises stresses than in the static simulation performed without a pore and of the material’s ultimate strength. In conclusion, the methodology presented in this work shows that developing a more realistic simulation study is possible. For a complete structural integrity study, the mechanical design simulation studies must include some complex geometries of intrinsic manufacturing defects.


Introduction
Due to the advantage of manufacturing components with complex geometries and the low cost of raw materials, added to the fact of recycling of the moulding sands, the casting process by green sand moulding continues to be widely used in obtaining mechanical components for the industry.
The existence of manufacturing defects is inherent to all manufacturing processes.The most common defects of this casting process are Porosities, Inclusions, Oxide films, Hot cracking, and Cold cracking [1,2,3].
It is crucial to study these defects since they can promote initiation points for crack propagation during the component´s service and consequently provoke premature failure [4,5,6].Therefore, knowing the location, distribution, and geometric dimensions of defects in parts is essential.
The objective of this work is to study the crack propagation from a 3D intrinsic casting defect on a cast component of manganese steel using Extended Finite Elements Method.The simulation software used was the ABAQUS.The mechanical proprieties of the railway component object of this study are presented in the Infante et al. work [7].The 3D defect geometry was obtained by microtomography.

Extended Finite Elements Method
Conventional finite element methodologies use polynomial functions that cannot describe discontinuities, using as the only alternative to model discontinuities the coincidence of the same with the finite elements mesh used.Such coincidence requires constant mesh refinements, which leads to high computational time.Thus, one can deduce that a problem of the conventional method (Contour Integral) is that the crack depends on the mesh used.A method used to avoid this problem is the Extended Finite Elements Method (XFEM).This method, developed in 1999 by Belytschko and Black, is an extension of the conventional method and is based on the unit partition principle developed by Melenk and Babuska in 1996 [8].The Extended Finite Element Method allows representing discontinuities and singularities independent of the mesh type defined by enriching traditional shape functions with other functions.This advantage makes this method attractive for crack propagation simulations since it does not require constant mesh refinements.
For the study of fracture mechanics, asymptotic functions are used at the crack tip to represent the singularity and discontinuous functions are used at the crack tip to represent the singularity, and discontinuous functions, such as the Heaviside function, describe the discontinuity when cracks open.
Figure 1 shows a crack that is not aligned with the mesh.It is possible to verify the enriched elements (in red) coming from the intersection made by the discontinuity.There are two types of enrichment: the asymptotic function at the crack tip, which describes the behaviour of the crack tip, and the Heaviside function, which describes the behaviour of the rest of the crack.Figure 2 presents an example of an arbitrary crack in a mesh; the nodes enriched by the Heaviside function are those that are intersected by the crack geometry (red), while the nodes surrounding the crack tip are enriched by the asymptotic function at the crack tip (green).Considering all nodes of the mesh in a group named A, the nodes around the crack tip in group B, and the nodes that are intersected by the crack in group C (except the nodes of group B).The finite element equation, displacement is given by equation 1, where Ni(s,t) is the shape function at node i with coordinates (s,t), and ui is the nodal displacement vector, ai characterizes the nodal vector enrichment of degrees of freedom with the Heaviside function, and bi is the vector of the nodes enriched with asymptotic function at the crack tip.H(s,t) is Heaviside given by equation (2).The solutions of the asymptotic function at the crack tip are represented by ψi (equation 3), where r and a are the local polar coordinates at the crack tip with a varies between [-π, π].

Experimental Procedure
The typical cast defect appeared in the concentration zone of a coupling railway component studied by Morgado [2,3].Therefore, railways component samples were analysed in detail using A high-resolution Skyscan 1172 micro-tomograph to obtain the 3D dimensions of intrinsic manufacturing defects.In this dimensional characterization, the analytical data resulting from the combination of the microscopic system of radiographs and a computer with tomographic reconstruction (NRecon), visualization and analysis software (Dataviewer, CTAn, and CTVox).Samples were observed with a voltage of 85 kV and a current of 116A for a pixel size of 4.80 μm.The biggest porous obtained by tomography was modelled in ABAQUS, as shown in Figure 3.
The in-service requests [6] to which the rail component is subject have been re-created in a simplified model.For this purpose, one of the flared ends was considered, and the other was subjected to pressure to simulate the axial force, with a value of 20.8 MPa.A compensation pressure of 1.2 MPa was also applied due to the symmetry conditions.Moreover, the mechanical properties of the material, obtained experimentally  A quarter ellipse crack, visualized through macrography whose shape factor is 0.75, was incorporated in the highest zone of concentration of stresses in the pore (see Figure 4).Through this crack, it is possible to perform a numerical simulation of propagation through the XFEM method to determine the crack propagation path, considering the conditions of loading and frontier.Given the length of the pore, it is expected that the processing time of this simulation will be excessive, considering the possible convergence errors.Several simulations were carried out to reduce the convergence problems encountered.The methodology used was based on finding hypotheses that could influence the convergence of results.The hypotheses to overcome the convergence problems were the follows: 1) Attention to the complexity of the model: One of the principles that must be considered in modelling is that the component should be simple enough to describe the desired behaviour.
2) Check boundary conditions: One of the causes of convergence difficulties is inadequate boundary conditions, which can lead to extreme local deformations.Thus, a model can be under-constrained when not all the body's degrees of freedom are constrained, or it can be over-constrained, leading to an error known as a "zero-pivot warning".3) Include static dissipation in the Step: One of the ways to achieve convergence is to include a static dissipation stabilization in the analysis, as recommended by the programme manual [9,10].One way to introduce this dissipation is to include an automatic stabilisation in the Step module that applies a viscous force proportional to the nodal displacement; this is divided among all the nodes at all simulation times, creating a stabilisation effect.One way to check whether this viscous dissipation influences the results is to check whether the ALLSD (static dissipation, stabilisation) and ALLIE (internal energy) parameters have similar values.
4) Damage stabilisation: It is possible to use a viscous regularisation tool to have a more stable response during the damage evolution characteristic of the XFEM process.
5) Add plasticity to the model: Non-convergence in a simulation can occur when the stress developed in a component does not increase as the deformation increases.In other words, by specifying the stress for each instant of deformation can make it easier for the results to converge.At this stage, the software no longer aborts due to the error "System error in timeup.Dtime=zero"; however, it cannot converge from a particular step time.
6) Add the "discontinuous analysis" option: This option allows the software to perform more iterations by increasing the I0 and IR parameters.With this option, more iterations are allowed before the solution needs to approach each iteration, i.e., it allows the programme to be less rigid in deciding if a calculation does not converge.It can be beneficial for non-linear problems such as those using the XFEM method, but it has the disadvantage of requiring more computational time.
7) Remove parameters from the simulation outputs (request outputs): Sometimes, the nonconvergence of the simulation is because there are specific simulation output parameters that can be difficult to determine at certain periods of the simulation.
8) Use other types of elements: After checking that none of the hypotheses described above would solve the convergence problem, it was decided to use another type of element, in this case, 4-node linear tetrahedral elements C3D4.

Results and Discussion
Figure 5 presents the Von-Mises stress distribution results in the pore in the elastoplastic regime.And Figure 6 shows the result of propagation through the pore and a detailed view of the crack propagation with fractured and damaged elements by applying the tool STATUSXFEM.
From the study developed it can be affirmed the following: • The XFEM method is a valuable tool for predicting the possible propagation of a crack in a railway component considering a manufacturing defect.• The type of criteria used in the XFEM method made it possible to analyse the propensity of the manufacturing defect to initiate crack propagation.• The type of elements used, in this case, the C3D4 elements, proved to play an essential role in realising the numerical simulation of crack propagation considering a manufacturing defect.The final number of elements was 266237, and the nodes number was 55091.• The static analysis results indicated that the maximum stress concentration in the pore is in a zone that can be identified as a hot spot.• The presence of the pore meant a more significant stresses concentration.The highest value of Von-Mises's stress is in the pore; this emphasises the importance that a manufacturing defect has on the structural integrity of a component.• The ALLSD static dissipation used in Step did not influence on the results.
• The ALLVD viscous stabilisation used in Damage evolution did not influence on the results.

Conclusions
With this study, it is concluded that reconstructing a complex pore mesh by finite elements is possible.Nevertheless, it is laborious and time-consuming.It is also concluded that it is possible to incorporate a manufacturing casting defect into a solid component and mesh it.
The stress analysis study shows that the highest stress value is in the manufacturing defect, and its complex geometry presents zones of stress concentration that promote crack propagation.So, manufacturing defects must be considered in the finite elements' crack propagation studies.
It is also concluded that the Extended Finite Elements Method can be applied in complex studies of crack propagation using defects with complex geometries.
The methodology proposed by the authors for the 3D crack propagation numerical simulations was successful.It is concluded that the proposed method is a valuable tool in future 3D numerical simulations of crack propagation using intrinsic manufacturing defects.

Figure 1 .
Figure 1.Crack not aligned with the mesh.

Figure 2 .
Figure 2. Arbitrary crack in the mesh.

Figure 3 .
Figure 3. Railway component mesh with the manufacture defect inserted in the surface.

Figure 4 .
Figure 4. Crack inserted in the stress concentration zone of the pore.

Figure 5 .
Figure 5. Von-Mises stress distribution results in the pore in the elastoplastic regime.

Figure 6 .
Figure 6.Crack propagation with the detail of crack inserted in the stress concentration zone of the pore.