Issue 31

C.L. dos Santos et alii, Frattura ed Integrità Strutturale, 31 (2015) 23-37; DOI: 10.3221/IGF-ESIS.31.03 29 i) between the dowel and the surface of the hole of the side member; ii) between the dowel and the surface of the hole of the centre member; iii) between the centre and side members (interface). The Augmented Lagrange contact algorithm was adopted in the analysis. With respect to this contact algorithm, two important numerical contact parameters need to be defined, namely the normal penalty stiffness factor, FKN, and normal penetration tolerance factor, FTOLN [19]. For the proposed simulations, the following contact parameters were adopted: FTOLN=0.1 and FKN={1.0,0.1,0.006}, the latter respectively for wood-wood contact, dowel-central wood member contact and dowel-side wood member contact. These contact parameters were calibrated by authors on previous elastic simulations of embedding tests along the longitudinal and radial directions, performed on similar wood members [27]. Once the joint geometry admits two planes of symmetry, only 1/4 of the joint was modelled (1/2 of the side member and 1/4 of the centre member). The displacements of the nodes located at the planes of symmetry were restrained along the normal direction to these planes. Fig. 6 shows the FE mesh built for the T-connection, where a mesh refinement around of the dowel is observed. The clearance between the dowel and the holes was assumed equal to 0.1mm which is an average value from experimental measurements. The friction coefficient was assumed equal to 0.5, which has been considered a typical value for steel/wood contact. Figure 6 : Finite element mesh of the T-connection. With reference to the constitutive models used in the simulations, the steel dowel was modelled as a homogeneous and elastic material ( E = 210 GPa;  = 0.3). With respect to the wood, several constitutive modelling alternative approaches were tested in this investigation. As a first approach, wood was simulated assuming a fully elastic behaviour with orthotropic elastic properties, as presented in Tab. 1. However this first analysis revealed an unsatisfactory description of the experimental results since the observed experimental non-linear behaviour of the joint is not captured by the simulation. A literature review about numerical modelling of wood non-linear behaviour [11-13, 28] reveals plasticity constitutive models as a frequently adopted option. The ANSYS ® code [19] offers a constitutive plasticity model for anisotropic materials, based on Hill’s yield criterion. This model requires the definition of a reference non-linear uniaxial stress-strain curve and anisotropic stress ratios that allow the scaling of this reference curve in order to retrieve the material behaviour for each direction. The model does not distinguish tension from compression behaviours of wood. Therefore, the model calibration requires a compromise between these two distinct wood behaviours, taking into account the dominant stresses applied on wood members. This plasticity model, based on Hill’s yield criterion, was adopted to simulate the T-joint load- displacement behaviour. The material was assumed transversely isotropic and the reference curve was assumed perfectly plastic. Therefore, the anisotropic stress ratios required for the model identification corresponded to ratios between anisotropic yield stresses. Two alternative approaches were followed for the plastic analysis: i) The same plasticity model parameters were used for both wood members (see Tab. 3). This approach is physically more consistent since the materials of each specimen members are the same. ii) Distinct plasticity model parameters were used for each wood member (see Tab. 4). This approach try to use independent plasticity parameters adjusted for each wood member of the joint (central and lateral members) in a tentative to produce better global predictions of the mechanical behaviour of the joint.