Corresponding author: Aleksandra V. Voronina ( avvoronina@mephi.ru ) Academic editor: Boris Balakin
© 2021 Aleksandra V. Voronina, Sergey V. Pavlov.
This is an open access article distributed under the terms of the Creative Commons Attribution License (CC BY 4.0), which permits unrestricted use, distribution, and reproduction in any medium, provided the original author and source are credited.
Citation:
Voronina AV, Pavlov SV (2021) Selection of a turbulence model to calculate the temperature profile near the surface of VVER1000 fuel assemblies in the NPP spent fuel pool. Nuclear Energy and Technology 7(2): 7984. https://doi.org/10.3897/nucet.7.68939

The paper considers the problem of selecting a turbulence model to simulate natural convection near the surface of a VVER1000 fuel assembly unloaded from the reactor by computational fluid dynamics (CFD simulation) methods. The turbulence model is selected by comparing the calculated data obtained using the Ansys Fluent software package with the results of experimental studies on the natural convection near the surface of a heated vertical plate immersed in water, which simulates the side face of the VVER1000 fuel assembly in a first approximation. Twoparameter semiempirical models of turbulence, kε and kω, are considered as those most commonly used in engineering design. The calculated and experimental data were compared based on the excessive temperature of the plate surface and the water temperature profiles in the turbulent boundary layer for convection modes with a Rayleigh number of 8∙10^{13} to 3.28∙10^{14}. It has been shown that the best agreement with experimental data, with an average deviation not exceeding ~ 8%, is provided by the RNG kε model which is recommended to be used to simulate natural convection near the surface of VVER1000 FAs in the NPP spent fuel storage pool.
Natural convection, model, turbulence, laminarity, fuel assembly, temperature, Ansys Fluent
A longterm experience in testing fuel assemblies (FA) for pressurizedwater power reactors (PWR and BWR) on inspection benches in the NPP spent fuel storage pools has proved demonstratively its efficiency in such missions as providing the R&D basis for the FA operation, introducing new FA and fuel element designs, and justifying new fuel cycles (
A repair and inspection bench for the VVER1000 reactor FAs has been developed and is deployed at NPPs which makes it possible to examine closely the FAs, identify their form change, detect and remove leaky fuel elements, and perform eddycurrent radioscopy of the fuel cladding (
Right after the VVER1000 FA is withdrawn from the reactor core, its decay heat is rather high (reaching hundreds of kilowatts) due to which natural convection of water develops near the FA surface in the spent fuel pool. The convective layer is characterized by the thickness and the water temperature and velocity distribution in it, the convection parameters varying lengthwise the FA in a range from a laminar mode in the assembly’s bottom part to full turbulence at the top (
The convective layer formed near the FA surface with a noticeable water temperature gradient should be taken into account, specifically when using ultrasonic pulseecho techniques to measure the FA dimensions (
Numerical simulation based on CFD (Computational Fluid Dynamics) techniques can be used to estimate the parameters of the convection near the FA surface (
Hundreds of turbulence models have currently been developed of which none is however versatile. When there is a new item to be numerically simulated for convection, a problem therefore arises as to what particular turbulence model to select and how to estimate the confidence of the results obtained by simulation.
As a rule, the rationale for the turbulence model selection is provided through comparing the calculated data obtained using different models with experimental results. And the experiment can be conducted using the tested item as such or its model or the item’s convection processes which are physically close (identical) to same.
Literature does not contain experimental data on the parameters of natural convection near the surface of a VVER1000 FA with decay heat immersed in water. This leads to the need to search for examples of experimental studies on natural convection for items which are close, as far as possible, to the heated VVER1000 FA in terms of thermal physics. The convective layer along the FA’s outer surface results primarily from deposition of heat from the fuel elements in the peripheral row which can be simulated in a first approximation by a heated vertical plate with the width equal to the VVER1000 FA flat (~ 135 mm) and the height equal to the fuel element height (~ 4000 mm), and with the heat flux equal to the flux from the fuel elements and directed into the environment perpendicularly to the plate. In other words, the VVER1000 FA is simulated by a heated hexagon.
The paper presents the results of a CFD simulation using the Ansys Fluent software package (ANSYS Fluent) for the natural convection along a vertical heated plate immersed in water. Twoparameter semiempirical models of the kε and kω families were used as the turbulence models. The calculation results were compared with experimental results (
There is a great number of theoretical and experimental studies dealing with investigating the natural convection near a vertical heated surface. Since the phenomenon of natural convection is of most interest to scientists in calculation of structural elements and utility systems regarding the removal or supply of heat, many papers are concerned with studying the natural convection near a vertical surface uniformly heated in an air environment. Studies to investigate convection near a nonisothermal surface are much fewer. One of the earliest papers with published results from experiments to study laminar convection near a vertical surface with a constant heat flux in water is that by Lock and Trotter (
The experiments published in (
In a general form, the flow of a viscous liquid is described by a system of NavierStokes equations consisting of a mass conservation equation and the law of conservation of momentum (
$\begin{array}{l}\frac{\partial \rho}{\partial t}+\nabla \left(\rho \mathbf{v}\right)=0,\\ \end{array}\phantom{\rule{0ex}{0ex}}\frac{\partial \left(\rho \mathbf{v}\right)}{\partial t}+(\rho \mathbf{v}\xb7\nabla )\mathbf{v}=\nabla p+\mu \Delta \mathbf{v}+\mathbf{F},$ (1)
where v is the liquid velocity vector; μ is the dynamic viscosity; F is the vector of volume forces; р is static pressure; ρ is the density;▽ is the Hamilton operator; and Δ is the Laplace operator.
There are three approaches to simulation of turbulent flows:
DNS suggests solving complete unsteadystate NavierStokes equations. This method is hard to use to simulate actual physical flows, since it requires computational resources expected to become available by only 2080 (
Many studies were undertaken to simulate a free convective flow near a vertical heating surface for isothermal conditions (
The problem was simulated numerically in an unsteady twodimensional statement. A flow was studied along a heat emitting plate of the height 1.5 m immersed in a static liquid (water) with the constant temperature T_{∞}. The diagram of the computational region is presented in Fig.
The initial conditions have the following form:
u (x, y, 0) = v (x, y, 0) = k (x, y, 0) = ε(x, y, 0) = ω(x, y, 0) = 0;
T (x, y, 0) = T_{∞},
where u, v are the projections of the velocity vector on the x and y axes respectively; x, y are the coordinates, m; k is the kinetic energy of turbulence, m^{2}/s^{2}; ε is the dissipation rate of the turbulence kinetic energy, m^{2}/s^{3}; ω is the specific dissipation rate of the turbulence energy, s^{–1}; and T_{∞} is the water temperature, °С.
Temperature conditions of the second kind were defined as the boundary conditions on the plate surface FE
$\lambda \frac{\partial T}{\partial \mathbf{n}}=q$
as well as noslip and impermeability conditions for the velocity
v = 0,
where λ is the wall material’s thermal conductivity; n is the vector of the normal to the surface; q is the heat flux density, W/m^{2}; and v is the velocity vector.
A symmetry condition meaning the equality to zero of the boundarynormal liquid motion velocity component and of the temperature and pressure gradients has been defined for areas AE and FB:
v (x, y, t) = 0,
$\frac{\partial p}{\partial \mathbf{n}}=\frac{\partial T}{\partial \mathbf{n}}=0$.
The following boundary conditions are defined on boundaries AD, CD and BC for velocity, pressure and temperature:
u (x, y, t) = v (x, y, t) = 0,
p (x, y, t) = p_{∞},
T (x, y, t) = T_{∞}.
where p_{∞} and T_{∞} are the water pressure and temperature respectively.
The following kε and kω turbulence models implemented in Ansys Fluent were used for the turbulence simulation: Standard kε, RNG kε, Realizable kε, Standard kω, and SST kω. Due to a limited size, the paper does not describe in detail each of the models. The mathematical formulation and the peculiarities of the models are presented in (
Models of the kε family are not capable to simulate the effects taking place in the nearwall region. Semiempirical formulas, referred to as wall functions, are used for the quality simulation of the flow in the boundary layer using kε models. Ansys Fluent has the following models for nearwall turbulence: Standard Wall Functions, Nonequilibrium Wall Functions, and Enhanced Wall Treatment (ANSYS Fluent). Enhanced Wall Treatment was used in the study. The use of the Standard Wall Function and the Nonequilibrium Wall Function has shown a poor agreement in the simulation of a similar phenomenon (convection near an isothermal plate) (
Boussinesq approximation is used not infrequently to describe convective motion (
An equation solver, called PressureBased Solver, was used for solving. The Simple (SemiImplicit Method for PressureLinked Equations) algorithm was used to calculate the velocity field coupling with pressure involving a counterflow pattern of the second order accuracy (Second Order Upwind) for the convective members in the momentum conservation equation, for the kinetic turbulent energy equation, and for the turbulent energy dissipation equation. The convergence of the solution was regarded to be achieved in events when the difference between iterations in solving continuity, momentum, energy, turbulent kinetic energy, and dissipation rate equations reached 1×10^{–6}.
Regular meshes condensing towards the heated wall were used for the calculations. Ansys Meshing was used as the mesh generator. The mesh model was built with regard for the key criteria that characterize its quality (ANSYS Fluent).
Convection was simulated for the conditions of two experiments the results of which are published in (
Figs
It can be seen from the figures that the results for all of the turbulence models used are close to the experimental results in the laminar region and predict satisfactorily the laminarturbulent transition region (3∙10^{12} < Ra < 4∙10^{13}). In the developed turbulence region, Ra > 4∙10^{13}, the results of the calculations based on the Standard kω model stand out sharply against the overall picture giving the plate wall temperature overestimated by nearly 10 °C (Fig.
Fig.
The greatest discrepancies between the experimental and calculated data fall on the region near the plate wall being in the limits of ~ 0.1 mm. Here, the calculated data exceeds that obtained in the experiment. The possible reason for such discrepancies is that the water temperature is hard to measure correctly in the immediate vicinity of the plate, since the temperature sensors perturb the structure of the convective flow viscous sublayer.
Table
Turbulence model  Average deviation of calculated data, %  Maximum deviation of calculated data, % 

Standard kε  11.64  26.38 
RNG kε  8.07  22.16 
Realizable kε  14.70  26.44 
SST kω  14.32  26.34 
It can be seen from the table that the best result is achieved in the event of the RNG kε model with the average deviation from the experimental data being ~ 8%, as the Standard kε, Realizable kε, and SST kω models give 11.6, 14.7, and 14.3% respectively.
The Ansys Fluent code was used for the CFD simulation of the natural convection near a submerged vertical heated plate with a constant heat flux density. Five twoparameter semiempirical turbulence models, most often applied in engineering design, were used for the simulation, including Standard kε, RNG kε, Realizable kε, Standard kω, and SST kω.
The simulation results were compared with the experimental data obtained earlier for the excessive temperature of the plate surface and the water temperature profiles in the turbulent boundary layer for the three heat flux density values: ~ 4.5, 19.5, and 28.7 kW/m^{2}. The comparison results have shown the following.
All turbulence models used give the calculation results which are close to the experimental values in the laminar region and predict satisfactorily the laminarturbulent transition region.
To the exception of Standard kω, all models under consideration calculate satisfactorily the plate surface temperature in the developed turbulence area. As far as the temperature profile is concerned, the best result is provided by the RNG kε model with the average deviation from the experimental data being ~ 8%.
Therefore, it is recommended to use a twoparameter semiempirical turbulence model, RNG kε, as the turbulence model to calculate, using the Ansys Fluent code, the temperature profile in the laminar and turbulent boundary layers of natural convection near the outer surface of the irradiated VVER1000 FA immersed in water.