Issue 48

V. M. G. Gomes et alii, Frattura ed Integrità Strutturale, 48 (2019) 304-317; DOI: 10.3221/IGF-ESIS.48.30 309 Finite element modelling and parameters of the numerical models The tested bolted connections (1+1 and 4+4 bolts arrangements) were modelled. Good practice developed in a previous research by some of the authors was followed in this research [1]. Fig. 4 A and B show the FE models of the 1+1 and 4+4 connections, respectively. Due the physical and geometry symmetry, only 1/4 numerical models were modelled, in order to reduce the computational costs of the simulations. This step was possible by the imposition of null displacements in the direction perpendicular to the planes of the symmetry (X and Y axes). Regarding the mesh, a refinement of the finite element mesh was carried out in the proximity of the holes due to the expected higher stress concentration. In addition, full bolt geometry was considered, simplifying the bolt thread by a smooth cylindrical shape. Contact pairs were used for all the contact possibilities that exist in the numerical model. Moreover, surface-to-surface contact option was used to impose the contact among Gauss points of the elements. Before modelling the contact pairs, it is necessary to identify the potential interactions between bodies. In summary, the following contact pairs were established: the contact between cover plates and middle plate, contact between bolt head and superior cover plate, contact between washer and inferior cover plate and the bolt shank and the holes of the three plates (cover and middle plates). In addition, it should be highlighted that all middle plate surfaces were meshed with CONTA174 elements and all fastening bolt contact surfaces were meshed by TARGE170. However, the hole contact surfaces of cover plates were meshed with CONTA174 elements, while the cover plate surfaces in contact with middle plate were meshed with TARGE170 elements. The contact between elements was considered flexible-flexible. Simulations were performed using Lagrange contact algorithm. This requires the definition of the contact stiffness and the interpenetration tolerance of the contact pairs to be applied in the normal direction to the contact surface. The contact stiffness was estimated by ANSYS, and it was based on elastic properties of the contact bodies which could be affected by a multiplicative factor, defined by the FTOLN parameter and is also a multiplicative factor to be applied to the thickness of the first layer of solid elements in contact for penetration tolerance. According to Silva [5], the amount of penetration between the contact surfaces depends on the value of the normal contact stiffness. For high stiffness values, there is a reduction in penetration, increasing the convergence difficulties of the contact algorithm. Low stiffness values can lead to high penetrations, thus producing less precise solutions. In this way, a sufficiently high stiffness is intended to reduce interpenetration between elements to acceptable values, ensuring convergence to the solution in a timely manner. According to the study carried out by Silva [1][5], the optimal values for these parameters are as follows: FKN (contact stiffness factor) equal to 0.1 and FTOLN (penetration tolerance factor) equal to 0.1. These values were used in the present study. The initial penetration that may occur was ignored; anyway it is expected that does not exist any problems with this consideration because the finite elements are quadratic and can represent the real geometric hole. The materials (S355MC and S350GD) were modelled with elastoplastic behaviour. It was adopted the Von Mises yield criterion, with isotropic hardening defined by multilinear law. The uniaxial engineering stress-strain curve was adopted according to experimental data obtained by tensile tests performed in this research. As regards the bolts behaviour, elastic behaviour was adopted taking into account that the ultimate load of bolt is greater than plate materials and the failure occurred in the plates. Tab. 3 summarizes the parameters used in constitutive law of the materials. Regarding friction modelling, the Coulomb friction model was taken into account as provided by ANSYS 18.2 code. The friction law was based on Eqn. (4):       rel -Dc×v act dyn µ =µ × 1+ Fact-1 ×e (4) where act µ is the current friction coefficient, taking value equal to static friction coefficient, stat µ , before the sliding, dyn µ is the dynamic friction coefficient, Fact is the ratio between stat µ and dyn µ , Dc is the exponent of decay, and rel v is the relative velocity between element faces. Due to lack of knowledge of some data like the exponent of decay, the Eqn. (4) was simplified, considering the exponent of decay equals to 0, becoming the Eqn. (5) in: act dyn µ =µ ×Fact (5) The relationship between the static and dynamic friction coefficients, Fact , was estimated from experimental data. Thus, when the static friction load is reached, the sliding occurs. After this load level, the transition between static to dynamic friction coefficient is immediately, so the numerical sliding limit load can be incorrectly measured for situations where the Fact is relatively high. The static friction coefficient can be obtained from the first peak load on the experimental curve