Numerical Simulation of Turbulent Fountains with Negative Buoyancy

Abstract

This paper investigates the flow dynamics of a turbulent fountain with negative buoyancy using a Computational Fluid Dynamics (CFD) model, developed using OpenFOAM^® and calibrated against laboratory experiments. The simulations effectively replicate the geometry and buoyancy fluxes of the fountain, showing a fairly good agreement between the numerical and experimental velocity fields. These simulations are then used to investigate momentum and buoyancy fluxes for various source fluid densities. We find a dominant out-upward momentum transfer in the body of the fountain, while it is mainly out-downward below the inlet section. Furthermore, the vertical flux is almost twice the radial flux, while the tangential components are negligible on the inner side of the fountain. For small density differences between the fountain and the surrounding environment, we find a greater diffusion of the source fluid, while both the vertical and radial salt fluxes increase with increasing density of the fountain. The data generated serve as a significant resource for the development of future CFD models.

1. Introduction

Fountains are defined as localized vertical flows where a source fluid is introduced into an ambient fluid of a different density. The result is a buoyant jet, which is very common in the industry as well as in nature [1,2]. In fluid mechanics, fountains differ from jets, which are flows where fluid is expelled with significant momentum and spreads primarily due to inertia, with minimal buoyancy effects. Thus, jets are driven mainly by momentum, while fountains are characterized by the interaction of momentum and opposing buoyancy forces. Some examples are represented by smoke emerging from chimneys, heating or cooling from building floors or ceilings, rising marine oil spill plumes, underwater hydrothermal plumes, and rising gases during explosive volcanic eruptions.

Depending on various factors, the dominant forces governing the behavior of a fountain can vary significantly. These factors include the nature of the release, whether the flow is laminar or turbulent, the geometry of the source (circular or rectangular), the direction of fluid injection (vertical or inclined), and the physical properties of both the source and ambient fluids, such as their density and viscosity. This study specifically examines axisymmetric miscible fountains formed by a continuous release of denser fluid into a calm, uniformly less dense ambient fluid. The injection occurs vertically upward from a circular tube, with the density contrast between the fluids small enough to apply the Boussinesq approximation [3].

The most common classification of fountains depends on the source Froude number [4], denoted as $F{r}_0=w_0/\sqrt{g_0^{\prime }{r}_0}$, where $w_0$ is the initial velocity of the fluid, $r_0$ is the radius of the source, and $g_0^{\prime }$ is the buoyancy of the source fluid, defined as $g_0^{\prime }=g\left({\rho }_0-{\rho }_a\right)/{\rho }_a$. ${\rho }_0$ and ${\rho }_a$ are the densities of the source and ambient fluid, respectively. The dynamics of a forced fountain ($F{r}_0>4$, which is the present case) exhibit distinct stages. At the beginning, there is an initial pulse of fluid, represented by a starting plume which rises until the opposing buoyancy arrests it and induces a counter-flow, see Figure 1. Then, the fountain stabilizes into a nearly steady state, featuring a rise and fall behavior. The peak height, $z_i$, is reached before the development of the counter-flow, and it exceeds the mean rise height, $z_{ss}$ (that is, the average height of the fountain during the nearly steady state).

In a turbulent fountain, there is a direct and complex exchange of momentum between the outward flow from the source and the counter-flow. Accessing detailed internal dynamics of turbulent fountains has traditionally been challenging, especially in experiments. Recent developments in computational power have paved the way for numerical models which solve the Navier–Stokes equations in order to simulate complex flow fields, making it possible to analyze numerous fluid processes [5], including turbulent fountains, as a complement to physical testing. Unlike physical experiments that rely on probes and cameras at specific locations, numerical simulations provide comprehensive 3D data anywhere in the domain, including instantaneous velocity, density, and turbulent kinetic energy. Moreover, numerical modeling is cost-effective and overcomes limitations such as equipment availability and operational complexity associated with physical testing [6].

Previous research studied turbulent fountains employing Direct Numerical Simulation (DNS) [7,8,9,10,11] or Large Eddy Simulation (LES) [12,13,14,15]. Valero and Bung [16] employed FLOW-3D for full 3D RANS modeling of two turbulent jet-to-crossflow cases, including free surface jet impingement. Following comparison with experimental data, they underlined the importance of using the appropriate turbulent Schmidt number to achieve more accurate reproduction of the concentrations.

A wide range of software is available for numerical modeling. In addition to commercial software packages and in-house programs, open-source CFD software has grown in popularity and is frequently supported by active communities thanks to the free license and the availability of the source code. An excellent example of such an open-source CFD package is open-source field operation and manipulation, commonly known as OpenFOAM^® [17,18]. The standard package of this software comes with numerous solvers and utilities designed to address a wide range of problems. OpenFOAM^® has already been utilized for several studies on turbulent fountains [19,20]. Suzuki et al. [21] performed an inter-comparison study of three-dimensional models of volcanic plumes, but for this particular phenomenon, direct measurements were not available to validate the model. Gildeh et al. [22,23] performed numerical simulations of inclined dense jets in still water, while Yan and Mohammadian [24] studied laterally confined vertical buoyant jets. More recently, Yan et al. [25] simulated the mixing characteristics of vertical buoyant jets released from multiport diffusers.

This work aims (i) to present the ability of a CFD model, developed in OpenFOAM^®, to reproduce turbulent fountain dynamics and (ii) to use the results of the numerical simulations to show new aspects of the flow field. As an advancement from the previous research, we were able to exactly replicate a set of laboratory tests and to directly compare the experimental velocity, density, and flux profiles with those obtained from the CFD model (for this purpose, we have used accurate experimental measurements by Addona et al. [26]). Then, more insights are provided by the numerical models, in particular to describe mass fluxes due to turbulent fluctuations, where measurements could not be obtained through experiments or were compromised by the invasiveness of the probes.

This paper is structured as follows: Section 2 describes the experiments that will be used to calibrate the numerical model (both the facility and instruments are illustrated along with the data processing and methodology). Section 3 details the computational domain, the boundary and initial conditions, and the mesh sensitivity analysis. The results are discussed in Section 4, and the main conclusions are summarized in Section 5.

2. Experiments

All the experiments were performed at the Hydraulic Laboratory of the University of Parma, Italy. The activity aimed to produce a turbulent fountain of a denser source fluid which propagates into a lighter ambient fluid and is therefore subjected to a negative buoyancy [26].

2.1. Apparatus

The experimental apparatus consists of a tank with a height of $800\mathrm{mm}$ and a square horizontal section measuring $400\times 400{\mathrm{mm}}^2$. A vertical pipe with an inner diameter of $7.8\mathrm{mm}$ was fixed at the bottom of the tank, protruding upwards for $300\mathrm{mm}$, and it was connected to a pump, which allowed for the generation of the fountain by injecting the source fluid into the ambient fluid (i.e., freshwater). Furthermore, a feedback control system was implemented to regulate the flow rates. In fact, the rotation speed of the pump was adjusted based on real-time flow measurements taken using a turbine meter. The entire system was managed by custom software developed in LabVIEW, allowing for the generation of either a constant or variable flow rate over time. In this study, we present the experiments with a constant discharge of $15.3\mathrm{mL}/\mathrm{s}$. The source fluid was saline water (brine) with density values given in

Table 1. Parameters of the experiments for turbulent plume.

Test Name	${\mathit{\rho }}_{\mathit{a}}$ ${\mathrm{kg}/\mathrm{m}}^3$	${\mathit{\rho }}_0$ ${\mathrm{kg}/\mathrm{m}}^3$	Q $\mathrm{mL}/\mathrm{s}$	${\mathit{Re}}_0$ -	${\mathit{Fr}}_0$ -
test 1	1000	1028	15.3	1180	9.6
test 2	1000	1040	15.3	1130	8.0
test 3	1000	1051	15.3	1110	7.2
test 4	1000	1060	15.3	1080	6.6
test 5	1000	1070	15.3	1060	6.1

, while the ambient fluid was homogeneous quiescent freshwater as stated above.

A schematic of the experimental setup is shown in Figure 2.

2.2. Data Recording

A FHD video camera was used to detect the interface between the ambient fluid and the source fluid. For this purpose, the brine was colored with aniline dye to facilitate the automatic processing of the images using MATLAB-based software. Before each test, a grid with known coordinates was inserted inside the tank (in the midsection) and recorded by the camera for calibration. This step is necessary to transform the coordinate system from pixels to meters and to obtain quantitative results.

An Acoustic Doppler Profiler (ADP) was used to measure the instantaneous velocity profiles at a data rate of 50 Hz. For this purpose, the probe was axially aligned with the vertical pipe, and it was in a fixed position approximately $150\mathrm{mm}$ above the inflow section. A second instrumental setup was also used, with the ADP mounted on a traverse system alongside a conductivity probe (Conduino [27], which works as a density meter). The traverse was continuously moved up and down during the test in order to obtain density data over the entire profile, as the Conduino, unlike the ADP, takes measurements only within a small control volume surrounding its primary sensor (i.e., the electrodes). The inset in Figure 2 shows the density meter and the ADP on the moving support.

Further information on the experiments can be found in Addona et al. [26].

3. Numerical Model

A CFD model was developed in OpenFOAM^® to replicate the experiments on turbulent fountains. Therefore, the simulation parameters were chosen to match the experimental conditions.

3.1. Model Setup

The CFD modeling of turbulent fountains involves the irreversible mixing of different fluids. The solver used for the simulation, interMixingFoam, is designed to handle a tri-phasic approach with three incompressible fluids, two of which are miscible. In this case, only two liquid phases are considered: the ambient fluid (freshwater) and the source fluid (brine), while air is neglected. The solver considers the three-dimensional Unsteady Reynolds-Averaged Navier–Stokes (U-RANS) equations for each fluid phase (see Appendix A) with a Volume of Fluid (VoF) [28] interface capturing method [29]. The algorithm used to solve the governing equations is called PIMPLE, which combines the SIMPLE (semi-implicit method for pressure-linked equations) and PISO (pressure implicit with the splitting of operators) algorithms as an improvement over previous versions of the code [30]. The main structure of the PIMPLE algorithm is inherited from the original PISO, but it allows for under-relaxation of the equation to ensure convergence at each time step. The LES scheme was adopted to simulate turbulence dynamics using the SubGrid-Scale (SGS) model kEqn-cubeRootVol, which is particularly effective for complex geometries with non-uniform mesh resolutions and for capturing multiscale turbulence. The LES model is chosen for its ability to resolve large turbulent structures while modeling smaller eddies, providing a more accurate description of the dynamic behavior of fountains and their interaction with the surrounding environment. In contrast, the $k-ϵ$ model, while computationally less expensive, simplifies turbulence and may struggle to accurately capture the intricate flow features at the interface between the involved fluids. The $k-\omega$ model, which excels in modeling near-wall turbulence, can be useful in predicting the behavior of water at the pipe exit or the surrounding boundary layer, but it may not handle larger-scale flow dynamics as well as LES [31,32,33].

The time step was chosen using the Courant–Friedrichs–Lewy (CFL) criterion, defined by the following equation:

$$C_{\mathrm{FL}}={\displaystyle \frac{u\mathrm{\Delta }t}{\mathrm{\Delta }x}}\le C_{\max }$$

(1)

where u is the velocity at the pipe outlet, $\mathrm{\Delta }t$ is the time step, and $\mathrm{\Delta }x$ is the average distance between two cell centers in the pipe. The Courant number (CFL) quantifies the relationship between the time increment $\mathrm{\Delta }t$ and the time required for a fluid element, moving at velocity u, to traverse a cell with size $\mathrm{\Delta }x$ [31]. The constant $C_{\max }$ depends on the type of equation being solved and the numerical scheme used for its solution. Generally, it is recommended to maintain $C_{\mathrm{FL}}$ below 1 to ensure the stability of the numerical scheme and the accuracy of the results. For Large Eddy Simulations (LES), even stricter conditions may be necessary, with the Courant number typically around 0.5 [34]. In the present case, the maximum $C_{\mathrm{FL}}$ is 0.63, and it rapidly decreases with the velocity as the plume expands in the ambient fluid.

3.2. Computational Domain, Boundary, and Initial Conditions

The mesh of the water tank has dimensions of $400\times 400\times 550{\mathrm{mm}}^3$ and includes a $300\mathrm{mm}$ vertical pipe at its center. This setup represents just a portion of the experimental water tank, ensuring the maximum rise height of the fountain is within the domain while reducing computational costs. The outer diameter of the pipe, $D_o$, is $10\mathrm{mm}$, and the inner diameter, $D_i$, is $8\mathrm{mm}$, resulting in a tube thickness of $1\mathrm{mm}$. Figure 3 shows a sketch of the numerical domain.

The interMixingFoam solver requires the definition of three fluid phases; thus, three fluid phase fractions, ${\alpha }_{air}$, ${\alpha }_0$, and ${\alpha }_a$, are used (with the subscripts 0 and a denoting the source and ambient fluids, respectively). For each simulation, the initial conditions are set with the entire domain occupied by the ambient fluid (at rest) and the source fluid inside the pipe. The value of ${\alpha }_{air}$ is set to zero throughout the entire domain.

The top boundary of the tank domain is designated as an open boundary, where inlet–outlet boundary conditions are applied to allow excess fluid within the tank to flow out, thereby preventing fluid compression. In contrast, no-slip conditions are enforced at the lateral and bottom boundaries. The pipe is numerically treated as a solid boundary, with the no-slip condition applied to both its inner and outer walls. Furthermore, at the inlet boundary (where the source fluid enters the domain) a constant volumetric flow rate Q of $1.5\times {10}^{-5}{\mathrm{m}}^3/\mathrm{s}$ is imposed, giving the outflow velocity of 298 mm/s. This value shows a slight deviation from the experimental one, primarily due the difficulty of generating exactly the nominal flow rate in the laboratory. Nevertheless, the results will be presented in dimensionless form, ensuring their comparability.

3.3. Mesh Sensitivity Analysis

To achieve grid-independent results, a mesh sensitivity analysis was conducted initially. Several meshes were developed with decreasing cell sizes, labeled as coarse, medium, fine, and fineR. The details of the tested meshes are provided in

Table 2. Parameters of the different tested meshes.

Mesh	Total Number of Cells (No.)	Minimum Grid Size (mm)	Mean Rise Height (mm)
Coarse	754,416	0.91	65.3
Medium	1,184,183	0.74	63.2
Fine	1,901,232	0.59	60.6
FineR	3,063,808	0.48	60.8

, including the total number of cells, the minimum cell dimensions, and the quasi-steady mean rise height for each mesh. Figure 4 illustrates the details of the different meshes at the inlet section, located at the bottom of the tank.

To select the optimal mesh for the simulations, we used the Grid Convergence Index (GCI) method, as suggested by Roache [35]. This method was applied to the case with an intermediate density of $1051{\mathrm{kg}/\mathrm{m}}^3$, using the average velocity near the base of the fountain as the reference variable.

In our study, the constant refinement ratio was $r=1.24$, while the order of convergence, p, was calculated using three grids at a time, resulting in $p=0.46$ for the coarse, medium and fine meshes, and $p=3.67$ for the medium, fine and fineR meshes. In particular, for $p=0.46$, the GCI values were found to be $GC{I}_M=1.70\%$ and $GC{I}_F=1.54\%$ for the medium and fine meshes, respectively. For $p=3.67$, the GCI values were within the acceptable range, with $GC{I}_F=0.04\%$ for the fine mesh and $GC{I}_{FR}=0.02\%$ for the fineR mesh. This indicates that the results are grid-independent. Furthermore, since the GCI for the fineR mesh was the smallest, this mesh was eventually used for the numerical modeling of the turbulent fountains. A safety factor of $F_s=1.25$ was assumed in the analysis.

To confirm this, it was observed that as the mesh density increases, the quasi-stationary rise height values tend to converge, with the mean rise height for the fine and fineR meshes being nearly equal. Furthermore, the value for the fineR mesh is the closest to the experimental value, as shown in Figure 5a. Note that the GCI approach ensures a robust and reliable selection of the mesh, as it is based on a quantitative measure of grid independence rather than a mere comparison with experimental values.

Since the present study focuses on the fluid domain above the source, we note that the external wall of the tube and the internal surfaces of the tank are located far from the fountain and do not interact with the region under investigation. Therefore, no particular attention was paid to the reproduction of the boundary layer at these elements. Furthermore, although this study addresses turbulent fountains, it is important to note that the Reynolds number inside the tube is approximately 2300, indicating that the flow is laminar or, at most, at the very onset of the transition regime.

The minimum duration of the simulations was determined by analyzing the stability of the turbulence statistics after the initial plume had dissipated. This was achieved by calculating the root mean square (RMS) of the velocity fluctuations over progressively larger time intervals. Figure 5b shows the evolution of the velocity fluctuations, $w_{\mathrm{rms}}^{\prime }/w_0$, above the pipe, along a vertical profile aligned with its axis. It was observed that for simulations lasting at least 25 s, the statistics within the main body of the fountain exhibit a variability of approximately $5\%$, which is comparable to the experimental uncertainties.

4. Results

The results of the numerical model are compared with the experiments by Addona et al. [26] in order to estimate the capabilities of the software to reproduce the details of the physical phenomenon.

Table 3. Geometric parameters of the fountain from the numerical model. $z_{ss}$ and ${\sigma }_{ss}$ are the mean value and the standard deviation of the rise height, respectively. $z_{pe}$ and $z_{tr}$ represent the mean peak height and mean trough height, while $2b_{ss}$ is the fountain-top width.

Sim. No.	$\mathit{\rho }$ kg/m3	${\mathit{z}}_{\mathbf{ss}}$ mm	${\mathit{\sigma }}_{\mathbf{ss}}$ mm	${\mathit{z}}_{\mathbf{ss}}+{\mathit{\sigma }}_{\mathbf{ss}}$ mm	${\mathit{z}}_{\mathbf{ss}}-{\mathit{\sigma }}_{\mathbf{ss}}$ mm	${\mathit{z}}_{\mathbf{pe}}$ mm	${\mathit{z}}_{\mathbf{tr}}$ mm	$2{\mathit{b}}_{\mathbf{ss}}$ mm
1	1028	86.6	6.4	93.0	80.1	95.5	76.8	18.8
2	1040	68.4	6.3	74.7	62.1	78.5	57.4	18.2
3	1051	59.1	5.8	64.9	53.2	68.6	50.4	17.2
4	1060	53.7	5.2	58.9	48.4	61.6	45.9	15.7
5	1070	48.1	4.6	52.7	43.4	55.1	41.1	14.0

reports some geometrical parameters derived from the CFD simulations.

4.1. Fountain Statistics

The statistics of the forced fountain are shown in Figure 6 as a function of the source Froude number $F{r}_0$. Panel (a) illustrates the mean rise height $z_{ss}$, normalized by the radius of the source, $r_0$. The numerical data appear well-aligned with the trend of the experiments by Burridge and Hunt [36] and Addona et al. [26]. In panel (b), the fluctuation in fountain height $(z_{pe}-z_{tr})$ is shown, normalized by the fountain-top width $2b_{ss}$, where $z_{pe}$ and $z_{tr}$ represent the mean peak height and mean trough height, respectively [36]. Again, the numerical results show reasonable agreement with the literature, though they tend to be slightly higher on average. This discrepancy may arise from the different techniques used to extract information from the numerical model and from the experiments.

4.2. Mean Flow and Turbulence

Figure 7a shows the profiles of the non-dimensional vertical velocity $w/w_0$, where the coordinate z is scaled with $2r_0$. All the data collapse near the outflow section, where $w/w_0$ must be equal to one. As the distance from the source increases, reasonable agreement is observed if the numerical and experimental Froude numbers are comparable, with curves exhibiting the same slope, which in turn represents the rate of vertical velocity reduction. Panel (b) shows the non-dimensional vertical velocity fluctuations, $w_{\mathrm{rms}}^{\prime }/w_0$, as a function of $z/\left(2r_0\right)$. The CFD simulation aligns with the experimental data, especially in the inner region, with values between 0.1 and 0.2. Measurements are not available near the outlet, where the simulation shows that turbulent fluctuations are negligible up to a distance from the pipe equal to two or three times its diameter. A sharp reduction of $w_{rms}^{\prime }/w_0$ is then observed around $z/\left(2r_0\right)\approx 10$, whereas the data from [37], which correspond to much higher source Froude numbers, decrease more gradually. The mean velocities are essential to determine the dynamics of the fountain, the recirculation of the surrounding ambient fluid, the entrainment by the forced fountain (since the entrainment is usually assumed as proportional to the radial velocity), and the mean buoyancy fluxes.

The results of the numerical model were then used to obtain further information regarding the characteristics of the turbulent field. The Reynolds stresses provide information regarding momentum exchange, which in turn modifies the entrainment and the mixing by the forced fountain. Figure 8 shows the Reynolds stress map in the $xz$ plane, when $\rho =1051\mathrm{kg}{\mathrm{m}}^{-3}$. The maximum values of the momentum transport due to the fluctuations are concentrated in the main body of the fountain, and we can infer that the direction of transport in this portion of the domain is out-upward. The down-flow region is characterized by more modest stresses, with a prevailing out-downward transport. Despite the system being axially symmetric, the symmetry of the contour is not perfect because the fluctuations are calculated from simulations with finite durations, and the data are exported at a frequency comparable to that of the ultrasound probes used in the experiments. Consequently, the statistics may show slight asymmetries due to sampling effects. These considerations hold for any vertical plane in which the axis of the inlet pipe lies. The results of the other simulations (i.e., relative to other densities of the source fluid) are similar and are therefore omitted for the sake of brevity.

4.3. Density Profile and Mass Exchanges

Figure 9 shows the results of measurements taken with the Conduino salinity probe alongside the corresponding numerical data.

Panel (a) displays the vertical profile of non-dimensional density $(\overline{\rho }-{\rho }_a)/({\rho }_0-{\rho }_a)$, where $\overline{\rho }$ is the time average of the density, ${\rho }_0$ is the density of the source fluid, and ${\rho }_a$ is the density of the ambient fluid (freshwater). The density gradient is the balancing term determining the negative buoyancy, i.e., the balancing force against the momentum of the uprising fountain. The density variations are also strictly related to the salt transport and the mixing processes between the source and the ambient fluids. The numerical results overestimate the experimental ones in the main body of the fountain. However, it is important to emphasize that the density measurement technique is particularly invasive, as it involves a probe moving vertically within the fountain. This movement can create additional mixing due to the turbulence generated by the probe, leading to a reduction of the bulk density. Furthermore, a closer examination of the results reveals that for $z/z_{ss}>0.35$, the experimental and numerical data exhibit the same slope. This suggests that most of the entrainment observed in the laboratory likely develops near the inlet. On the contrary, near the mean rise height, the agreement between the data improves, culminating in a very good overlap at $z/z_{ss}=0.35$. It must also be noted that the experimental data do not approach zero above $z/z_{ss}$; this can be attributed to the drag effect exerted by the probe on the fluid, with traces of brine that may remain on the sensor even after it has entered the fresh water domain.

Panel (b) demonstrates a good qualitative agreement between the density fluctuation profile ${\rho }_{rms}/({\rho }_0-{\rho }_a)$ and the experimental data, both displaying a pronounced peak at $z/z_{ss}=1$.

The agreement improves if we look at the correlation between density fluctuations and vertical velocity fluctuations (see Figure 10). In this case, the experimental evidence is available for only one density of the source fluid ($\rho =1028\mathrm{kg}{\mathrm{m}}^{-3}$), and it is possible to observe that the position and the value of the peak are almost the same in both the numerical results and the laboratory data. This result supports the use of simulations to extend the study of mass exchanges due to turbulence in the entire investigated domain.

Figure 11 shows the map of $\overline{{\rho }^{\prime }{w}^{\prime }}$ in the $x-z$ plane for two different densities (tests 1 and 5). Such a correlation can be interpreted as the vertical buoyancy flux per unit of area [38], and it is possible to observe that, for low densities of the source fluid, the highest positive values are recorded near the inlet area (at $z/z_{ss}\lesssim 0.5$). When ${\rho }_0$ increases, the maximum values tend to move towards the mean rise height (at $z/z_{ss}\approx 1$), where the injected fluid has already mixed with the ambient one. The density of the source significantly influences the shape of the mass down-flux due to fluctuations, with the region affected by the exchange widening as ${\rho }_0$ decreases. For ${\rho }_0=1070\mathrm{kg}{\mathrm{m}}^{-3}$, the minimum values of $\overline{{\rho }^{\prime }{w}^{\prime }}$ are observed in a narrow band close to the lateral wall of the pipe.

The different extensions of the domain affected by the mass fluxes can also be observed in Figure 12, which shows the maps of the correlation $\overline{{\rho }^{\prime }{u}^{\prime }}$ for the lowest and highest density. This quantity represents the horizontal mass exchange due to turbulence, with positive and negative values indicating a net flux to the right and to the left, respectively. The maximum and minimum values are equal to half of those observed in the case of vertical flux. The results present axial symmetry, as expected in any vertical plane on which the axis of the inlet pipe lies.

Figure 13 illustrates the dynamics of $\overline{{\rho }^{\prime }{v}^{\prime }}$, reveling a very complex pattern characterized by a continuous alternation of positive and negative values. Notice that, in this case, the average value of the correlation is computed with reference to the horizontal velocity component normal to the plane, so it represents the exchange in the tangential direction, which appears to be one order of magnitude lower than the radial one. We also observe that, in the case of correlations involving horizontal velocities in the outer region of the domain and when $z/z_{ss}<0$, very small positive or negative values are detected, leading to an irregular pattern.

4.4. Practical Applications

Once the CFD model is built and calibrated, broader implications of the findings that are out of the scope of the present work can be explored, and we report some examples below. In environmental systems, it would be possible to enhance the comprehension of cumulus cloud top dynamics. In fact, at the top of stratocumulus clouds, water can evaporate, resulting in denser cold air falling at the edge of the clouds, mixing with the surrounding air which is going up in the inner side of the cloud tower. This behavior has been shown to depend on the buoyancy, geometry, and velocity of the plume, which can be thoroughly investigated through an adequate CFD model, such as the one that has been described in this manuscript [39]. In industry processes, numerical models allow for the optimization of processes such as the discharge of waste brine water from desalinization plants, which can have a severe impact on oceans, rivers, or other water bodies. The discharged fluid consists of saline water and results in a negatively buoyant jet. To minimize the impact on the marine environment, it is compulsory to effectively design the geometric parameters that influence the dilution of the waste brine water [40,41]. Further implications of the desalinization plant discharges include the accumulation of heavy metals, which can greatly affect the surrounding ecosystem [42]. Recent LES studies have shown that the density ratio and the salinity Froude number play a critical role in the impact of the discharged saline water [43]. In human activities, the understanding of turbulent fountains has become increasingly relevant in the design of ventilation systems. A significant example is represented by underfloor air distribution systems, where cooling air is driven by a pressure gradient from the floor and balanced by a reverse buoyancy [44]. In this context, it is also crucial to understand the effects of such ventilating systems on the dispersion of contaminants in enclosed environments, which can be sensitive areas where indoor air quality must be preserved (houses and offices) and contamination by pollutants must be avoided (hospitals) [45]. The use of a CFD model, in this case, would help investigate all the variables and dimensional groups involved, whereas invasive experimental apparatuses may be difficult to utilize and may provide only limited information.

5. Conclusions

We developed a numerical model using OpenFOAM^® to simulate forced fountains in an enclosed environment, aiming to replicate a recently published set of experiments. A detailed description of the CFD model is provided, and the results were compared with data from the literature, focusing on flow statistics such as fountain rise height, vertical velocity, and density profiles, including both mean values and fluctuations. In particular, the mean rise height and the average flow are well-reproduced, while some discrepancies are observed in density profiles, especially in the main body of the fountain. However, the numerical model captures the key characteristics of forced fountains, and it allows for the extension of experimental findings to a broader domain. The instrumentation used by Addona et al. [26] was limited to data acquisition along a single vertical profile, making it difficult to repeat tests by repositioning the probes to obtain data in 3D space. Therefore, once calibrated, the CFD model serves as a powerful tool for conducting an in-depth analysis of the phenomenon under investigation.

The momentum transfer is mainly out-upward in the main body of the fountain and out-downward below the inlet section, and the maps of the Reynolds stresses are useful to define the regions where the different cases occur (i.e., to resolve the exchange directions). Furthermore, the analysis of the results focuses on mass flux due to velocity fluctuations, which is a significant contributor to the mixing and possible propagation of any pollutants or pathogens from the source fluid to the ambient fluid. The values of the vertical flux are more significant (about double) than the radial ones, while the tangential component shows a complex pattern with negligible values also within the main body of the fountain. A strong dependence on ${\rho }_0$ can be observed, with the region affected by momentum and mass exchange widening as the density of the source fluid decreases, even if the maximum values of the correlations $\overline{{\rho }^{\prime }{w}^{\prime }}$ and $\overline{{\rho }^{\prime }{u}^{\prime }}$ are higher in cases of greater ${\rho }_0$ values. Therefore, it is expected that turbulence leads to a wider diffusion of the source fluid when the difference ${\rho }_0-{\rho }_a$ is small.

Possible future works will include the realization of a numerical model with an ambient fluid characterized by a shear flow, which represents a particularly realistic case study with numerous applications in both natural and artificial environments.