## 2 Methods
### Adopted Model  
In the present paper, the CIRCE-HERO facility is simulated adopting a coupled STH/CFD approach. In particular, the CFD code ANSYS Fluent simulates the pool while the STH code RELAP5/Mod3.3 is adopted for the simulation of the internal loop. In addition, the top region of the pool, where the LBE free surface is in contact with Argon, is modeled through RELAP5 to avoid two-phase simulation in the CFD domain. Figure 2 reports a scheme of the considered approach, the location of the interfaces between the regions and the relevant information transferred in their correspondence is reported as well. This subdivision was chosen, in similarity with other works, in order to exploit the advantages of both codes and, on the other hand, to avoid their drawbacks. In fact, in this way RELAP5 is used for the regions in which the fluid flow may be approximated by a mono-dimensional approach and in the regions where multiphase phenomena occur. ANSYS Fluent, instead, provides predictions for the intrinsically 3-dimensional environment of the pool, dealing with regions in which LBE only is present. The improved modelling capabilities of CFD are thus taken into account for the pool environment only; the introduction of the CFD domain, in fact, dramatically increases the computational cost of the performed calculation and thus must be limited as far as possible. Comparing to STH stand-alone applications, in fact, the coupled STH/CFD calculations are definitively more time consuming; nevertheless, the improved capability of the model and the quality of the information and lessons that can be drawn from the obtained results are often worth the additional computational cost  
Figure 2: Coupling scheme and spatial discretization. In the following, some of the most relevant information about the considered coupling approach is provided. It is worth noticing that, regarding the CFD domain, the inlet/outlet definitions are actually reversed; that is, the outlets of the real facility and the RELAP5 nodalization correspond to the inlets of the CFD computational domain and vice versa. Concerning the spatial discretization, a non-overlapping approach was adopted: RELAP5 and ANSYS Fluent solve autonomously their corresponding domains and only communicate at some selected boundaries. In particular, fluid-dynamic boundaries are imposed at the FPS inlet and at the HERO-SGBT outlet. On the CFD side, the HERO-SGBT outlet, which represents the main inlet surface for the CFD pool environment, is modelled adopting an imposed mass flow inlet condition. At the FPS inlet, instead, an imposed velocity condition is applied: the needed information is provided by the RELAP5 calculation at each time step. According to [14], defining the velocity distribution, it is one of the most practical ways to impose a mass flow rate at an outlet section; in addition, this assumption also allows for addressing possible backflow conditions which may appear in the numerical analysis owing to oscillations caused by the abrupt changes in the imposed Argon mass flow and was consequently selected in the present application. Eventually, at the top of the pool, a pressure inlet condition is applied. This was necessary in order to provide a suitable pressure value at the inlet and outlet sections which, after each internal iteration, provide these values to RELAP5. On the RELAP5/Mod3.3 side, instead, the fluid dynamic coupling with the CFD domain is obtained by mean of Time-Dependent Volumes and single junctions. At each time step, the CFD code updates the pressure and temperature information in these volumes, thus providing RELAP with suitably updated boundary conditions. Figure 3 resumes the thermal-hydraulic boundary conditions for the CFD side of the coupled calculation. The coupled application performed by UniPi in Ref. [14] was here furthermore updated with the introduction of thermal boundaries between the CFD and the STH domain for the most relevant heat structures of the internal loop.