Computational Fluid Dynamics Modeling of Single Isothermal and Non-Isothermal Impinging Jets in a Scaled-Down High-Temperature Gas-Cooled Reactor Facility

Abstract

In the current work, the flow characteristics of single isothermal and non-isothermal jets discharging into the upper plenum of a 1/16th scaled-down high-temperature gas-cooled reactor (HTGR) facility were studied. ANSYS Fluent simulations were carried out in the central plane of the jet water flow and the upper plenum for different Reynolds numbers (Re) ranging from 3413 to 12,819. Then, the statistical jet water flow characteristics, such as the mean velocity, root-mean-square fluctuating velocity, Reynolds stress, and the mean temperature in the upper plenum, were computed and presented. The current study’s results showed that the flow maximum velocity occurred far from the jet inlet. Finally, the temperature profiles were plotted, and it was found that the maximum temperature of the flow occurred close to the plume inlet and after that decreased downstream.

1. Introduction

The development of generation IV (GEN IV) technologies is monitored and controlled by an organization, the Generation IV International Forum, which was founded in 2001. The organization publishes guidelines for GEN IV nuclear power plants as a roadmap for nuclear energy systems and a high-temperature gas-cooled reactor (HTGR). The HTGR is considered one of the promising future technologies to be used for reactors [1,2,3,4].

HTGRs can produce heat at high temperatures using hundreds-of-megawatts (MW) reactors. HTGRs are also known as high-temperature reactors (HTRs), and they have potential applications in solving various industrial issues such as process heat, electricity, etc. The elevated temperature from the HTGR allows for considering applications like the production of CO₂-free hydrogen or oil refining processes. Processes like desalination or district heating, which require lower temperature heat, may also benefit from the HTGR heat source. It is important to note that the heat residual from HTGRs has higher energy levels than the light water reactor (LWR) [5].

The HTGR uses tristructural isotropic (TRISO), which is coated with particle fuel, has a complete ceramic core structure, and uses helium as a coolant. All these features can withstand high-temperature conditions. In addition, the HGTR has inherent safety features since it uses function requirements like reactivity control, residual heat removal, and radioactive retention. The design features of the next-generation nuclear power plant reactor are based on the concept of modular HTGR. Therefore, the modular HTGR is designed to meet safety and design requirements [6].

Phenomena identification ranking table analysis has been used to identify specific accident scenarios for the HTGR as essential risks to core safety. Therefore, the in-depth analysis is always required for the use of HTGR technology. The two primary accident scenarios are a depressurized conduction cool down (DCC) and a pressurized conduction cool down (PCC) [7]. In the DCC scenario, also known as a loss-of-coolant accident (LOCA), the primary coolant experiences a sudden depressurization which causes a reactor scram. However, when the pump fails, a natural circulation occurs between the reactor vessel and the confinement.

On the other hand, the PCC scenario has been known as a loss of flow accident (LOFA), which occurs when an external force is lost during a reactor scram caused by power failure. In the situation of scram, the blowers and pumps will not function, but the primary system remains operational at full pressure with the natural convection pushing the heat from the reactor core to the cavity cooling system. Mixing hot plumes from the heated coolant channel of the reactor core will occur in the upper plenum [8]. Hot gas flow is usually transferred as a free shear flow from the core area into the upper plenum (hemisphere). A jet will be generated when the flow rate comes from massive heat fluxes and has high momentum-driven steaming. If the flow rate is density-gradient, the gas will flow upward to create a plume in the upper area of the plenum. Sometimes the emergence of the jet flow will change to a plume as it comes from the core coolant channels. The fundamental flow characteristics of jet and plume are different since jet flow involves mixing turbulent fluxes. In contrast, the plume flow consists of the buoyancy forces that cause the mixing. There is a development of warm or hot stratified gas layers in the upper plenum of the HTGR caused by the flow with plume characteristics. However, when the jet flow is largely momentum-driven, it will permeate through the stratified gas layers and negatively affect the upper hemisphere material. This penetration of jet flow and undesirable thermal gradients will result in material cracking since there will be poor cooling due to high-heat transfer rates in the flow. It is observed that the fundamental characteristics of both jet and plume flow in the PCC and DCC accident scenarios are a trade-off between the safety and operational aspects of the process.

Understanding the jet and plume flows in terms of their thermal-hydraulic characteristics, flow behavior, and heat transfers is crucial for studying the HTGR. In addition, high-fidelity experimental data with high spatial and temporal resolutions are essential for assessing and validating the simulation performance using the CFD models and system codes. Recently, the nuclear society utilized such simulations. Several researchers have studied flow experiments and numerical studies to examine the flow behavior for single and multiple jets in a scaled-down HTGR facility [9].

Three fields in the round jet can be defined as the near, intermediate, and far fields. Researchers have focused on turbulence around free jets, and they have studied the far-field areas and the near field of the potential core. Theory, experiments, and/or modelling and experiment were the three investigations used in the previous studies [10,11,12,13,14,15,16,17,18,19]. Moreover, numerous studies have been conducted over the last decade focusing on the flow behavior at different conditions in the scaled models for the lower and upper plenum of the HTGR [20,21,22,23,24]. Several researchers have studied nuclear reactors to examine the behavior of single and multiple jets flows in scaled-down HTGR facilities using CFD models [25,26,27,28,29,30].

The subcommittee for Verification, Validation, and Uncertainty Quantification in Computational Simulation of Nuclear System Thermal Fluids Behavior (VVUQ 30) of the American Society of Mechanical Engineering (ASME) is supporting a series of benchmark problems designed to study the scope and key ingredients of the VVUQ 30 subcommittee’s charter. One of the benchmark problems is the one that this research has investigated. This study used the CFD software ANSYS Fluent in analyzing 1/16th-scaled single isothermal and non-isothermal jets in high-temperature gas-cooled reactors (HTGR) with an upper plenum. The CFD model investigation was used for the measurements, characterization of flow behavior, and temperature distributions of a single jet together with heat transfer in a scaled-down HTGR facility.

There are several research studies on the behavior of a single jet/plume. However, there is no research specific for this geometry. The contribution of this research is an analysis of the characteristics of momentum and buoyancy flows in the hemispherical upper plenum of the reactor to support recent research on the advancement of nuclear technology reactors.

2. Physical Model

A 1/16th scaled-down version of the modular HTGR prototype was used in the current study. The HTGR core design and the scaled-down facility consist of 1020 fuel blocks and 25 pipe blocks, respectively. Both blocks have a hexagonal shape arrangement, and the scaled-down facility blocks simulated the coolant channels. Figure 1a is the visible view of the geometry model for a single jet, while Figure 1b shows the side view of the same jet. In Figure 1b, the coolant enters the lower plenum of the reactor from the inlet pipe (A) and is drawn up to the region of interest, the upper plenum (B). The water exits the upper plenum through the outlet groove (C) and flows downward through pipe (D) until it reaches the outlet pipe (E) [31].

In the numerical simulations, the lower plenum was not considered because a single vertical inlet channel has a total mass flow rate from the lower plenum. A recycling boundary condition was applied to generate a fully developed flow in a long vertical pipe (coolant channel). The model is a 1/16th scaled-down HTGR prototype that has been used in experiments to examine the behavior of single and multiple jet flows. Figure 2 shows the details of the model used in the simulations, and the inlet and outlet jet diameter for the model is 12.6 mm. Water was used as the fluid for the simulations, and the specific heat, thermal conductivity (k), density, and dynamic viscosity (μ) for H₂O are given as 4193 J/Kg-K, 0.66 W/m-K, 974.68 kg/m³, and 0.378 × 10⁻³ Kg/m s, respectively. The properties of water were set at the inlet of the coolant channels. This study applied the realizable k-ε turbulence model to accommodate different mesh sizes.

3. Numerical Model

In this present study, the two simulated cases were isothermal and non-isothermal models. The basic governing equations solved by ANSYS/FLUENT 19.1 are continuity, momentum, and energy. Equations (1) and (2) are the continuity and momentum equations. Equations (3)–(5) are the energy equations for the free flow, respectively:

$$\nabla . \left(\mu \stackrel{\rightharpoonup }{U}\right)=0,$$

(1)

$$\nabla . \left(\mu \stackrel{\rightharpoonup }{U}\stackrel{\rightharpoonup }{U}\right)=-\nabla p+\nabla .\stackrel{=}{\tau }+\mu \stackrel{\rightharpoonup }{g}+\stackrel{\rightharpoonup }{F},$$

(2)

$$\nabla . \left[\stackrel{\rightharpoonup }{U}\left(\mu E_f+p\right)\right]=\nabla .\left(K_f \nabla T\right),$$

(3)

$$\nabla . \left(k_s\nabla T\right)=0$$

(4)

$$\nabla . \left[\stackrel{\rightharpoonup }{U}\left(\mu E_f+p\right)\right]=\nabla .\left(k_{eff} \nabla T-\sum h_j{J}_j+({\tau }_{eff}.\stackrel{\rightharpoonup }{U}\right)),$$

(5)

All the equations are solved simultaneously by implementing the coupled flow and coupled energy models. The coupled flow gives the choice of integration and discretization methods, for which implicit and second-order upwind were chosen. The second-order upwind method has an advantage over the first method because of its reduced numerical diffusion. The implicit method was selected because it provides a wider stability margin but requires more system storage than the explicit scheme. All models were determined to be in turbulent flow, and the gravity model was implemented as a natural circulation in the non-isothermal model. The effects of gravitation acceleration were needed to model the forces used in a natural circulation flow accurately. However, a steady-state model was chosen to study the problem at the given time options.

3.1. Boundary Conditions

For the isothermal model, the boundary conditions selected in this study corresponded to the details of the experimental facility, operating conditions, and measured data provided in the work of Alwafi et al. [4] as shown in

Table 1. Setup and solver settings for the isothermal model.

Model		K-epsilon
Solver		Pressure-Based
Working Fluid		Water
Outlet		Pressure Boundary
Density Model		Constant (998.2)
Spatial Discretization	Pressure Solver	2nd Order Upwind
	Momentum	2nd Order Upwind
	Turbulent Kinetic Energy	2nd Order Upwind
	Energy	2nd Order Upwind
	Turbulent Dissipation Rate and	2nd Order Upwind
	Gradient	Least Squares Cell-Based
Pressure–Velocity Coupling		SIMPLE

. The non-isothermal model was used for the natural circulation with inlet temperature up to 75 °C. The Re number was set between 300 and 531 at the inlet. The average pressure was zero at the outlet of all simulated runs in the present study. Lastly, the pipe’s surface was assumed to have no-slip conditions.

3.2. Numerical Solution

The initial conditions were used for the isothermal model to test the numerical convergence at the inlet pipe. The number of iterations was between 3500 and 5000; for a high Re number, it converged between 2000 and 6300 iterations. Convergence criteria were set to be 1 × 10⁻⁵ for velocity, continuity, k, and epsilon. For a tighter criterion, the limit was 1 × 10⁻⁶ of energy to be used. The numerical solution is second-order, as shown in Table 1.

For the non-isothermal model, all the simulations were calculated under gravitational conditions, and flow was assumed to be turbulent. Moreover, several initial and boundary conditions were considered, as shown in

Table 2. Setup and solver settings for the non-isothermal model.

Model		Energy, K-epsilon
Solver		Pressure-Based
Gravity		−9.8
Working Fluid		Water
Density Model		Boussinesq
Coefficient of Thermal Expansion		0.0034
Spatial Discretization	Pressure Solver	Body Force Weighted
	Momentum	2nd Order Upwind
	Turbulent Kinetic Energy	2nd Order Upwind
	Energy	2nd Order Upwind
	Turbulent Dissipation Rate and	2nd Order Upwind
	Gradient	Least Squares Cell-Based
Pressure–Velocity Coupling		PISO

.

Most simulations were completed within 2–8 h in this work, but a high-power computer could improve the computational speed.

3.3. Mesh Parameters

Proper meshing is essential for the simulation to capture the thermal-hydraulic behavior, so ANSYS meshing was used to mesh the geometry. To ensure that the obtained results do not change according to cell size, five different mesh sizes were generated as follows: 3 M, 3.5 M, 4.1 M, 5.9 M, and 6.4 M for the velocity profiles, as shown in Figure 3. A small grid dependence was observed for 3 M nodes, and all results were identical for 5.9 M nodes and higher. For this reason, grids with 5.9 M nodes were selected for the rest of the simulations.

In the independent study, the number and type of the mesh were 5.9 M and tetrahedral mesh, respectively. The mesh’s geometry with natural circulation models is more complicated than force convection models. However, the fine mesh defined for all meshes had uniform size and slow transition. Moreover, close to the walls of the upper plenum, eight layers of inflated elements with a transition ratio of 0.1 and a growth rate of 1.2 were used. Figure 4 shows the inflation that was used next to the walls.

4. Results and Discussion

The results of the current study are divided into two sections. The isothermal and non-isothermal single-jet models were investigated in the first and second sections of the study, respectively. In the first section, three different single-jet simulations were modeled for given operating conditions, as shown in Figure 2. In addition, ANSYS Fluent was performed and analyzed for other Reynolds numbers from 3413–12,819. The selected Reynolds numbers were based on the operating conditions of the HTGR for the scenario of coolant accident loss. Furthermore, three various axial locations were investigated using ANSYS fluent, as shown in Figure 5 (y/d = 1, 5, and 10).

It is important to group various types of intrusion according to how they inject into the ambient fluid, either momentum, buoyancy, or both. These flows can be classified as partly turbulent as they cause higher turbulence levels in their intrusion vicinity than the surrounding fluid. When incoming fluid is mixed with its dormant fluid body, significant turbulence is created due to the velocity shear. However, when the incoming jet is mixed with the fluid body at rest, the momentum source is caused by the jet itself. Such momentum will remain unchanged along the downstream provided that external forces accelerating or decelerating are either minimal or nonexistent in the jet region [32]. The ANSYS Fluent results for a single-jet mixing in the upper plenum for different axial mean velocities against Reynolds numbers are presented in Figure 6, Figure 7 and Figure 8. The results show that the maximum values for jet velocity are attained at the y/D = 1, followed by a steady decrease downstream with expansion in the transverse direction due to the diagonal movement of the jet. The jet flow showed a higher momentum flux at a higher Re number of 12,819, causing large penetration depths compared to lower Re numbers.

Figure 9 shows the localized velocity decay rates for different Re numbers along the jet centerline. The results showed high fluctuations of the velocity decay profiles inside the jet-flow axial height. Further downstream, Re = 7912 and Re = 12,819 merge into one profile with similar decay rates. From the nozzle exit of y/D = 9.2, there was an exponential increase in the decay profile due to jet impingement on the upper plenum, thus resulting in reduced centerline velocity, which made the decay profiles increase.

Reynolds stress (u′v′) profiles for various horizontal lines, y/D equals 1, 5, and 10, have been shown in Figure 10. In this case, the jet flow was discharged from a circular pipe into the ceiling of the upper plenum, and there was also the development of wall-jet flow before exiting the plenum. The large-scale vortices caused the jet flow momentum to be exchanged within the shear layer. This scenario has shifted the maximum local peaks of the Reynolds stress to lower axial positions. The results showed that counter-rotating vortices in the longitudinal direction create oscillating positive and negative radial fluid patterns.

Figure 11 shows the results of the radial velocity ($\acute{U_{rms}}$) along different axial locations. The $\acute{U_{rms}}$ has nearly the same shape and peaks similar to the ones near the upper plenum inlet y/D = 1. These peaks were mainly located over shear layers where jet momentum was exchanged with the surrounding fluid. At y/D = 10, the turbulence intensities were anisotropic due to turbulence structure influences [10].

The second section examines the buoyancy flow characteristics of a single non-isothermal plume into the upper plenum of a 1/16th scaled-down HTGR. A heating source would create the plume buoyancy, circulating the flow via a closed loop. Thus, the non-isothermal simulation uses natural circulation and heat, and it will be analyzed by ANSYS Fluent. At the entrance of the jet pipe, the water temperature and Re number were set to 75 °C and 600, respectively. Additionally, the surface of the jet pipe was assumed to have non-slippery conditions. Figure 12, Figure 13 and Figure 14 show the mean velocity vector fields against the velocity magnitude contour v, u´_rms, fluctuating transverse velocity (m/s), and Reynolds stress ($\acute{U_{ }}\acute{V_{ }}$) (m²/s²), respectively, for the non-isothermal plume 1. The maximum value of the plume velocity was attained at V__Centerline = 0.119 m/s and y/D ≈ 1.85. The plume velocity showed a steady decrease along the axial position till the plume began to rise in a diagonal direction after reaching the upper plenum top wall. The transverse velocity $\acute{U_{rms}}$ has the maximum value close to the upper plenum center and after that began to decrease. In the isothermal study, the maximum velocities of the jet and the plume occurred close and away from the inlet. Turbulent regions caused by buoyancy force were observed at the plume center in both directions, and higher flow fluctuation occurred at the plume core. The normal jet flow with increased kinetic energy causes high turbulences close to the upper plenum wall [33]. The Reynolds stress color contour shows the shear layers with positive and negative peaks at similar elevations. The signs of Reynolds stress ($\acute{U_{ }}\acute{V_{ }})$ indicate the rotational signs of the counter vortex pairs formed along the axial position of the plume nozzle.

The interpolation and normalization of the statistical profiles were performed along the axial position, y/D = 0–8, and using the plume velocity (V center line), respectively. Figure 15 represents the profile of the normalized mean vertical velocity (V/V__centerline) obtained from the ANSYS Fluent measurements for the upper plenum plume mixing. Moreover, the velocity profiles started to increase from a y/D value of 0 to 5, where maximum velocity is attained, and after that peak began to have a steady decrease until y/D = 8. The velocity of the center line reached ~57% of the jet velocity, and there were minor changes in the axial velocity that occurred for x/D ≥ 3.

The temperature profiles from y/D = 0 to 8 were interpolated horizontally and plotted in Figure 16, which shows the mean temperature profiles for upper plenum plume mixing. The maximum temperature for the profile from y/D = 0 to 5 at the center of the core inlet shows a similar quick drop in temperature at the end of the core. However, there was a gradual drop in temperature from y/D = 2 to 7. The profiles at y/D = 8 show a decrease in a non-monotonic temperature pattern that could be assigned to the high-temperature flow from the upper plenum wall. On the other hand, Figure 17 shows the effects of the temperature profile on the Prandtl number (Pr). The Pr number increases as the fluid temperature is decreasing. Moreover, increasing the Pr number reduces the thermal boundary layer thickness.

Figure 18 shows the mean velocity-vector fields against the mean temperature. The flow moves in a horizontal direction to the heater plane, and there is a transfer of heat to the fluid due to flow molecular motion to form a dome-like temperature boundary layer. A convective jet is formed when the fluid rises at the center because a hot surface has gently heated it. When the convective jet phase has been attained, the plume’s uniform growth continues until the heat wave encounters the upper plenum wall top.

5. Conclusions

CFD simulations were performed to analyze single isothermal and non-isothermal jets in the 1/16th scaled-down HTGR upper plenum at Texas A&M University for different Re numbers from 3413–12,819. The CFD model was used for velocity vector fields for measurements close to the jet inlet and flow reaching the upper plenum wall. The flow characteristics, such as the mean velocity, u´_rms fluctuating velocity, and Reynolds stress, were examined and presented in the present study. The study simulated two cases for isothermal and non-isothermal models. The isothermal model corresponds to the details of the experimental facility at Texas A&M University, while the non-isothermal model represents the natural circulation and heat. The isothermal model results showed that the flow characteristics are similar for y/D = 0–5, and flow can be considered free jets. Confinement and impingement effects were observed in the y/D region greater than 5, and close to the upper plenum top wall the flow began to decrease and change its diagonal direction. The U_r.m.s peaks were identified downstream at y/D = 1 and 5 for Reynolds numbers Re1, Re2, and Re3. Decay profiles of local velocities along axial location showed an increase up to y/D = 9.2 and after that exhibited an exponential increase because of jet flow reaching the top wall.

For the non-isothermal case, the measurements, flow field characterizations, and temperature distributions of a jet flow inside the upper plenum with conjugate heat transfer were investigated for Re = 500. ANSYS Fluent was used to analyze the characteristics of momentum and buoyancy-driven flows in the hemispherical upper plenum. From the results of velocity vector fields, flow properties such as mean velocity, u´_rms fluctuating velocity, and Reynolds stress, the mean temperatures in the upper plenum were examined and reported in the current study. The results showed that the plume’s maximum velocity was attained away from the inlet, and after that the velocity decreased along the axial location. The flow had high turbulences close to the upper plenum wall. The Reynolds stress displayed the shear layers with positive and negative peaks that occurred at similar elevations. The signs of the Reynolds stress (u´v´) show the rotational signs of the counter vortex pair created downstream of the plume nozzle. These simulation results will be used as verification and validation tools for the system codes and CFD models. However, additional experimental measurements will be needed.

In the future, the standard k-ε turbulence model can be substituted for with the large eddy simulation (LES) model to analyze the flow mixing near the impingement region. Moreover, the current study can be extended to investigate the upper plenum surfaces with different accident scenarios. Furthermore, multiple jets for various flow configurations could be studied in the upper plenum for this geometry.