# Numerical Analysis of a Moderate Fire inside a Segment of a Subway Station
## 4 Thermomechanical Simulation at Selected Time Instants  
The load-carrying behavior of the tested structure was analyzed by means of three-dimensional Finite Element simulations, using Abaqus FEA 2016. The chosen Finite Element mesh was similar to the one used for the thermal simulations; see Figure 10. The concrete structure was modeled by 139,040 hexahedral elements of type \"C3D8R\", i.e., eight-node linear elements with reduced integration and hourglass control, with three translational degrees of freedom per node. The steel rebar was considered by 18,035 line elements of type \"T3D2\", i.e., two-node linear three-dimensional truss elements, with an axial displacement degree of freedom per node. Perfect bond between concrete and steel rebar was assumed by attaching the nodes of the steel elements to the nodes of the concrete elements.  
The supports of the structure were accounted for by means of prescribing displacement boundary conditions. Four sets of such boundary conditions were prescribed in order to prevent displacements of the bottom ends of the walls and of the columns, in the direction of the axes of the columns; see Figure 6. Two additional sets of displacement boundary conditions were prescribed in order to  
Figure 14: Comparison of the simulated evolutions of the temperature inside the analyzed structure, obtained by prescribing three piecewise spatially-uniform temperature histories along the inner surface, with experimental data: (**a**) top slab, at the midspan of the middle cell, (**b**) top slab, at the midspan of the right cell, (**c**) top slab, at the midspan of the left cell, (**d**) center of the right wall (**e**) bottom slab, at the midspan of the middle cell, and (**f**) core of the right column.  
Figure 15: Temperature distribution obtained by prescribing three piecewise uniform surface temperature histories, 30 min after the start of the thermal loading: detail showing the central cross-section of the right column.  
prevent horizontal displacements of the left wall, in the direction orthogonal to the axes of the columns; see Figure 6.  
The external mechanical loads, imposed on the structure, were accounted for by means of prescribing traction boundary conditions. The six concentrated forces, acting on the top slab, and two loads, acting on the right wall (Figure 6), were prescribed by means of equivalent pressures amounting to \(13.3\,\mathrm{MPa}\).  
The thermomechanical simulation was organized by analogy to the sequence of actions during the analysis of the experiment. At first, the external forces were applied. While they were kept constant thereafter, the temperature fields, computed in Section 3, were prescribed as a time-dependent input, resulting in a transient thermomechanical loading of the structure.  
Combined sensitivity analyses were carried out, in order to study the sensitivity of simulation results with respect to uncertainties regarding the thermal loading and the material behavior of concrete. As for the first type of sensitivity analysis, the two different temperature field histories, computed in Section 3, were imposed on the structure, by way of two different simulations. As for the second type of sensitivity analysis, two different types of material models were used for the simulation of concrete. It was either modeled as a linear-elastic material with temperature-independent material properties or as an elasto-plastic material with temperature-dependent material properties, as described in the following.