# Parametric Analyses of the Response of Masonry Walls with Reinforced Plaster
## 3 Numerical Simulations  
### Finite Element Model  
The numerical analyses were performed using 3D FE models of the specimens (Figure 5a), which were developed with the commercial software, Abaqus [35]. Since the analyses were restricted to wall specimens of limited dimensions, a simplified micro-modelling approach was adopted for the masonry by defining the individual mechanical properties of the units and the mortar, with no unit-mortar interfaces [8; 26].  
The size of the mesh and the typology of the elements were defined based on a sensitivity analysis. The interactions of the masonry components were fully compatible. Solid tetrahedral elements with mesh sizes of 20 mm and 10 mm were adopted for the brick and the mortar, respectively. The unit-mortar interface was not modeled in order to keep the computational time reasonable. For the retrofitted configuration, solid linear tetrahedral elements with mesh sizes of 20 mm and 5 mm were adopted for the plaster and nails, respectively. For the anchors, due to their curved geometry, a refined mesh was adopted compared to the other materials to avoid overclosure at the interface with the masonry and plaster. The interaction between the plaster and the wall surface was defined as normal hard contact and tangential behavior with friction coefficient \(\mu=0.1\). This assumption made possible the development of debonding mechanisms. The interaction between the anchors and the plaster was also defined as normal hard contact and tangential behavior, but with a friction coefficient of \(\mu=0.4\). The steel net was modeled by using  
Figure 4: Damage at collapse: (**a**) on the plaster; (**b**) on the masonry; (**c**) plaster detachment.  
Figure 5: (**a**) 3D model of the specimen; (**b**) FE mesh of reinforced masonry; (**c**) FE mesh of the anchor.  
beam elements embedded in the plaster region. A view of the reinforced specimen mesh is reported in Figure 5b, while a detail of the anchor's mesh is reported in Figure 5c.  
The numerical simulations followed the protocol suggested by ASTM-E519 [36]. The test setup is represented in Figure 6a. The steel shoes were modeled as rigid elements, and their interaction with the masonry was defined as normal hard contact and tangential behavior, with a friction coefficient of \(\mu=0.2\). The simulation of the load application was performed through the imposed displacements applied on one shoe, while the other shoe was considered fully constrained to the ground. Figure 6b shows the finite element model of the specimen, with the load and boundary conditions.  
The numerical solution was conducted by adopting a dynamic explicit solver, which uses the central difference time integration by considering the diagonal mass matrix of the system. Since the model is intrinsically nonlinear, the dynamic explicit solver can capture the nonlinear behavior of the specimen if a large number of small increments is adopted. Nevertheless, it should be considered that the real specimen is placed under static loading and not dynamic. For this reason, the time increment and the sizes of the meshes were optimized to solve the problem in a quasi-static manner, by diminishing the effects of the kinetic energy.