## Modeling Of Connections

2.1 Calibration of the finite element model

In the following, results of finite element (FE) analyses performed on a typical birdsmouth connection of Chestnut wood specie, are presented. In particular, calibration of FE model is performed on the base of available data which can be found in the relevant literature (Parisi et al. 1997, and Parisi & Piazza 1995, 1998, 2000). In this work, the connection behaviour is simulated with the use of the FE software package STRAUS7 (1999), and results are investigated in terms of both force-displacement and moment-rotation diagrams.

The geometric dimensions of the both main rafter and chord were: length of the elements L = 1.90 m; element cross section 190 x 225 mm and 200 x 200 mm, skew angle equal to 30°; rafter cross section notch depth tv = 35 mm and notch length lv = 200 mm.

Two loading pattern were considered. The first one consisted of a vertical pressure uniformly distributed at the free end of the rafter; subsequently a transverse force was applied perpendicular to the axis of the rafter. The second one consisted of an initial axial pressure uniformly distributed over the cross section of the rafter; from this, a linear pressure distribution over the cross section of the element was applied in order to simulate a bending moment at the end of the rafter. With reference to the axial compression stress in the rafter, two values were accounted: fwr equal to 1.0 MPa and 1.5 MPa, respectively. These stress were kept constant during the analysis.

Conventionally, transverse force, moment and rotations have been assumed positive as the skew angle was reduced. The main chord of the joint was constrained in the vertical displacements at the base, and in the horizontal displacements at the vertical right-side border. A structured mesh is used for the rafter and the chord, whereas an irregular transition mesh is used in the vicinity of the connection between rafter and chord.

It is worth noting that wood exhibits anisotropic elastic and inelastic behaviour, and the characteristic inner structure which include several defects (e.g. knots, slope grain). The use of refined non linear orthotropic criteria is essential for detailed numerical simulations of timber joint, since different strengths and softening/hardening characteristics in orthogonal directions can be accounted (Lourengo et al. 2007, 1997).

For the purposes of the paper, an elastic orthotropic model is accounted for wood elements (Parisi & Piazza 2000; Bodig & Jayne 1982). Strengths and elastic materials properties have been derived from available tests given in Parisi & Piazza (2000) and represent average values.

In order to properly fit elastic properties for the wood members, which are characterized by different grain directions, a local coordinate system was introduced. The 1-axis and 2-axis are related to the direction parallel and perpendicular to the grain, respectively; the 3-axis is orthogonal to the 1-2 plane.

Therefore, the elastic parameters included the elastic moduli Ei = 9200 MPa and E2 = 310 MPa parallel and orthogonal to the grain, respectively; the shear modulus G12 = 580 MPa and the Poisson's ratio v12 = 0.4. Nonlinearities were concentrated at the contact interfaces.

The rafter and the tie were connected by point contact elements which allowed relative tangential displacements of facing surfaces and limited normal displacements. In particular, the Normal type contact implemented in STRAUS7 was used, which provides stiffness in compression and not in tension. In addition, a friction coefficient was introduced in order to control the amount of lateral force that can be transferred thorough the contact surface.

Let a the angle between the horizontal direction and the normal of the contact, the axial elastic stiffness of the contact elements has been estimated as EaA/L, where A is the area of influence of each point contact, L is the distance between the rafter and the chord (1 mm) and Ea is the elastic modulus at the angle a. The modulus Ea is calculated for each contact by taking into account the elastic moduli E1 and E2 of the timber elements as follows (Lekhnitsii 1968):

Figure 8. Finite element mesh and boundary conditions.

Force [kN]

■ ■ Experimental curve k- Parisi & Piazza (2000) —STRAUS7

Displacement [mm]

Figure 8. Finite element mesh and boundary conditions.

In the following, the contacts are named as con-tact#1 and contact#2. Equation (1) gives: Ea1 = 1710 MPa, and Ea2 = 320 MPa, for contact#1 and contact#2 respectively, and for cross section dimensions of 190 x 225 mm. The axial stiffness of the inner point contacts were: EaiA[/L = 1943kN/mm; Ea2A2/L = 728kN/mm; for the contact points at the end of each contact were EaiA[/L = 971 kN/mm; Ea2A2/L = 364 kN/mm.

For cross section dimensions of 200 x 200 mm, Eai = 2209 MPa, and Ea2 = 416 MPa, for con-tact#1 and contact#2, respectively, are obtained. The axial stiffness of the inner point contacts were: Ea1A1/L = 1116 kN/mm; Ea2A2/L = 558 kN/mm; for the contact points at the end of each contact were Ea1A1/L = 445 kN/mm; Ea2A2/L = 223 kN/mm.

The study included two values of the compression stress in the rafter, fwr = 1.0 MPa and 1.5 MPa, respectively. It is worth noting that self-weight of the wood elements is considered in the analyses.

The Modified Newton-Raphson algorithm was used in the incremental iterative solution of the nonlinear problem. Figure 8 shows the finite element mesh, including loading and boundary conditions of the model.

### 2.2 Numerical results

Numerical results are showed in Figures 9-10 in terms of nodal force-displacement diagrams with reference to the cross section members 190 x 225 mm, and in Figure 11 in terms of moment-rotation diagrams for a cross section members 200 x 200 mm.

In addition, comparisons against both experimental and numerical reference curves provided by Parisi & Piazza (2000) are carried out. It is worth noting that the nonlinear behaviour of the numerical response occurred as the limit conditions of friction resistance were attained and the rafter started to rotate. However, numerical results have to be considered up to the elastic limit.

As shown in Figures 9 and 10, major differences between experimental and numerical results are found in the case of low axial stress. For a compression stress

Figure 9. Comparisons between numerical and experimental force-displacement curves for rafter 190 x 225 mm under fwr = 1.0 MPa.