Keyword

1 Introduction

As one of the Generation-IV advanced nuclear energy systems, Lead-based Fast Reactor (LFR), has appealed to many international research institutions owing to its excellent inherent safety and nuclear sustainability [1]. The Lead Bismuth Eutectic (LBE) coolant employed in LFR with special characteristics (such as better heat conduction) different from the water (conventional coolant), as well as its integrative pool-type configuration may give rise to complicated three-dimensional thermal hydraulic phenomena in the large space plenum, such as thermal stratification and coolant mixing [2], making the thermal-hydraulics and safety problems of LFR always the research highlights. Computational fluid dynamics (CFD)-based commercial programs for simulating, owing to its mature technologies (plentiful models and algorithms) as well as the powerful pre-processing (modeling and mesh generation of complex geometric structures) capability, is considered as an effective method to overcome the multi-dimensional complicated thermal hydraulic problems involved in the liquid metal pool-type reactors [3].

At present, some commercial CFD tools, such as ANSYS Fluent, Star-CCM +, ABAQUS, have been widely used for simulations of liquid metal pool-type reactors, particularly the multi-scale coupling simulations with other reactor core physical models. For example, Gu Z. developed an advanced two-dimensional fuel pin heat transfer model, then integrated it with the self-developed PK model into ANSYS Fluent to conduct multi-physics coupling [4]. Deng J. developed a three-dimensional transient nuclear thermal coupling solution program based on OpenFOAM platform [5]. Narayanan developed the numerical models that deal with lead thermal hydraulics and solidification with ANSYS Fluent and Star-CCM + software [2].

As we summarized above, CFD tools are popularly used for multi-physics coupling simulation on liquid-metal-cooled reactors, but such commercial CFD programs are incapable to conduct the advanced coupling algorithms due to their closed source codes. OpenFOAM, as a free open-source CFD code, has a unique advantage of direct contact with the source code of existing solvers, making it relatively convenient for us to develop a new solver by modifying its source code from existing solver to vitally design its core computing functions.

In order to conduct the multi-physics coupling simulation with a high degree of customization based on complex coupling algorithms, a solver for simulating the coupled flow and heat transfer behaviors of fluid (coolant) and fuel pin in LFR was developed, and the fuel pin HC model was coupled to the modified icoFoam solver of OpenFOAM in this study. Verifications were conducted by the steady-state coupled simulation of coolant and fuel pin heat transfer behaviors, comparing with the MPC-LBE code which has been verified by the benchmarks for LFR fuel pin channel [6]. The simulation results agree well with the results provided by the MPC-LBE code, which shows the feasibility and accuracy of the solver.

2 Coupling of HC Code with Modified IcoFoam Solver

For LFR, the fuel pin channel consists of a slender cylindrical fuel pin and LBE coolant. Especially, the fuel pin constitutes of a centra hole, pin fuel pellet made of mixed oxides of uranium and its proliferator plutonium, gas plenum filled with Helium (under high pressure) and cladding mainly made of Zr-4 alloy. All the features above can be found in the benchmark reports [7].

2.1 CFD-Based Modifications of IcoFoam Solver

The new solver developed in this paper is based on the icoFoam solver of OpenFOAM, which can simulate the laminar flow by solving the incompressible Newtonian fluid N-S equations shown in Eq. (1) with the finite volume method.

$$ \frac{{\partial \rho {\varvec{U}}}}{\partial t} + \nabla \cdot (\rho {\varvec{UU}}) = \rho {\varvec{g}} - \nabla p + \nabla \cdot (\mu \nabla {\varvec{U}}) $$
(1)

In icoFoam, the fluid flow model is simplified by the neglect of gravity as well as the assumption of constant fluid density and kinematic viscosity. As shown in Fig. 1, the coupling solution of velocity and pressure, based on the simplified N-S equations and continuity equations, is obtained by using the transient PISO algorithm.

Fig. 1.
figure 1

Coupling solution of velocity and pressure

Full size image

However, icoFoam is incapable of simulating the heat transfer phenomena in fluid (coolant) region due to the neglecting of energy conservative equation for fluid. To conduct the simulation coupled flow and heat transfer behaviors in coolant region, corresponding energy equation containing the heat source term, shown as Eq. (2), is added to icoFoam source code.

$$ \frac{{\partial \rho_{LBE} c_{p,LBE} T_{LBE} }}{\partial t}{ + }\nabla \cdot \left( {\rho_{LBE} c_{p,LBE} T_{LBE} {\varvec{U}}} \right) = \nabla \cdot \left( {\lambda_{LBE} \nabla T_{LBE} } \right) + q_{V} $$
(2)

The velocity-based solution of energy conservative equation using the existing solver in OpenFOAM, is carried out after the coupling solution of velocity and pressure, as shown in Fig. 2.

Fig. 2.
figure 2

Velocity-based solution of temperature

Full size image

What’s more, the new variables involved in this new equation, such as temperature, specific heat, conductivity etc., indispensably need to be added to the solver as mesh-based variable fields just, which is similar to the pressure and velocity. Meanwhile, these newly added variable fields should be defined and initialized in include files, source code and running environment, including internal meshes and boundary conditions.

In particular, with the consideration of temperature changes caused by the energy change in coolant channel, it should be noted that most of the coolant parameters (density, conductivity, kinematic viscosity) are no longer constants as before but variables changing with temperature, whose calculation formulas can be obtained in detail from the benchmark reports [7]. Consequently, it is necessary to calculate then update these variables as feedbacks to corresponding mesh-based variable fields after the temperatures are solved in each time-step. In this paper, as shown in Fig. 3, only the kinematic viscosity (involved in N-S equations), density and conductivity (involved in energy equation) are regarded as variables with the feedbacks from continuous update.

Fig. 3.
figure 3

Mesh-based variable fields update

Full size image

2.2 Coupling Strategies with HC Code and Modified IcoFoam Solver

The modified icoFoam can simulate both the flow and heat transfer phenomena in coolant region, a three-dimensional mesh system based on OpenFOAM, after the works we did in the last section. As for the fuel pin region, its heat conduction process can be described by using the fully implicit finite volume method to discretize then solve the Heat-Conduction Equation in fuel pin sub-mesh system based on two-dimensional cylindrical coordinate system, which is already in our previous research work [4].

Through the convective heat transfer process at the interface (cladding outer surface) between fuel pin and LBE coolant, the heat transfers in these two regions are coupled as each other's dynamic boundary conditions with the explicit calculating strategy as shown in Fig. 4.

Fig. 4.
figure 4

Heat transfer explicit coupling strategy

Full size image

Firstly, the average convective heat transfer coefficient and average coolant temperature at specific axial position are provided to the fuel pin heat transfer module within the same axial position after the temperatures are solved in each time-step. Especially, the calculations of these two average variables are conducted by modifying icoFoam source code.

After that, the fuel pin region gives a heat source to coolant region in return. Generally, this heat source is transferred in the form of heat flux as a boundary condition, nevertheless, in this study we tried a new method to conduct this transfer. By the heat flux calculated in fuel pin region, the power transferred from cladding outer surface to LBE coolant can be also obtained, which is applied to the meshes at the inner wall of coolant channel as its volume power density (external heat source). Many mesh related parameters need to be obtained then used for calculations above.

Importantly, the fuel pin heat transfer module (HC code) is added after the coolant module to icoFoam source code based on the integral coupling framework shown in Fig. 5, so as to realize the coupling calculations in each time-step. These two modules use the same time-step size (0.02s) to coupled calculate, which has been already proved that this size of time-step can guarantee numerical stability. In each time-step, the temperatures of fuel pin module and coolant module are calculated iteratively, until the calculated time-steps meet the steady-state establishment.

Fig. 5.
figure 5

Integral coupling framework

Full size image

3 Verifications on Coupled Solver

3.1 Description and Mesh Generation for Computational Domain

In this paper, only a single fuel pin channel model is considered as the computational domain, whose composition is shown in Fig. 6 [6].

Fig. 6.
figure 6

Model of fuel pin channel [6]

Full size image

The computational domain is treated as a hexagon prism by its symmetrical characteristic. For the convenience of calculations of steady-state process, the inlet coolant temperature and velocity are constantly equal to the initial value, and the heat decay power is neglected. The geometry data and material properties of the fuel pin channel can be found with details in the benchmark report [6].

The fluid region in fuel pin channel is only the coolant channel, which is a complex digging hexagonal prism with a central hole. Therefore, such complicated channel is meshed by ANSYS instead of the existing meshing tool (blockMesh) of OpenFOAM. Then, this three-dimensional mesh system, shown in Fig. 7, is imported into OpenFOAM, whose quality analysis meets the service conditions.

Fig. 7.
figure 7

Mesh generation of coolant channel

Full size image

3.2 Computation Results and Code Verification Compared with the MPC-LBE

The steady state of the fuel pin channel is simulated by using the HC-coupled modified icoFoam solver code (coupled solver) developed in this paper. In Figs. 8 and 9, the coolant temperature spatial distributions, both at the mid-plane and outlet of the coolant channel, occur the thermal stratification, and the high-temperature heat ring on the inner wall of coolant channel is thicker, owing to the better heat transfer performance of LBE (liquid metal) coolant compared with other general coolants (such as water). And it is obvious that the overall level of the outlet temperature is higher than that of the mid-plane, and the trend of the former gradually decreasing outward along the radial direction is slower than that of the latter.

What’s more, as shown in Fig. 10, four axial distribution related temperature curves, representing the fuel pellet inner surface, fuel pellet outer surface, cladding outer surface and coolant temperatures (arranged from high to low), are drawn and compared with the ones by the MPC-LBE code whose feasibility and accuracy have already been verified [4]. Since the power generated from fuel pellet will heat the coolant channel around with coolant continuously flowing through the channel, the coolant temperature will gradually rise during the process from inlet to outlet. Obviously, such good agreements are achieved in terms of both the trends and values among the results provided by the HC-coupled modified icoFoam solver code and by the MPC-LBE code [4] in Fig. 10.

Fig. 8.
figure 8

Temperature spatial distribution at mid-plane of coolant channel

Full size image
Fig. 9.
figure 9

Temperature spatial distribution at outlet of coolant channel

Full size image
Fig. 10.
figure 10

Material axial temperature distribution of fuel pin channel at steady state

Full size image

4 Conclusions

In this paper, a single fuel pin channel model is established for the reactor core of LFR, so as to analyse the coupled flow and heat transfer behaviors in coolant and fuel pin. Multi-physics simulation system is built by coupling the fuel pin heat transfer model (two-dimensional HC module) to the three-dimensional open-source CFD code OpenFOAM by its icoFoam. This coupled simulation system for reactor thermal-hydraulics and safety analyses is abbreviated as the HC-coupled modified icoFoam solver code (coupled solver), which copes with the key data transmission problems of multi-physics coupling strategy within the framework of OpenFOAM platform. Mathematics models and methods as well as the coupling strategy of two modules are elaborated.

Verifications were conducted by the steady-state coupled simulation of flow and heat transfer behaviors between coolant and fuel pin regions in fuel pin channel of LFR, including the comparison with the benchmarks-verified MPC-LBE code [4]. The results simulated by the HC-coupled modified icoFoam solver code proposed in this paper agreed well with the ones provided by benchmarks-verified MPC-LBE code. It is testified that the HC-coupled modified icoFoam solver code is capable to perform the multi-physics simulations involved in thermal-hydraulics and safety analyses of LFR with enough accuracy.

However, only a simple single fuel pin model is considered to preliminarily verify the basic coupling strategies and schemes of reactor core heat transfer behaviors. Therefore, the coupling simulation of the whole fuel assembly channel of reactor core should be further studied in the future work, which can describe the reactor core more carefully and comprehensively. Meanwhile, for the heat transfer calculation coupled with coolant and fuel pin regions, the implicit iteration can be considered instead of the explicit calculating strategy used in this study. All in all, this study already verified the initial steady state, laying a foundation for the further development of transient safety analysis code to conduct transient simulation for LFR in our future work.