Investigation of heavy water discharges via numerical modeling

Gravity currents are flows caused by the density difference between the current itself and receiving environment. There are three different types of density currents. If the density of the current is greater than its surroundings density, an underflow will occur. If the underflow reaches a depth within the reservoir where it becomes neutrally-buoyant, interflow will result. If the density of the current is lesser than its surroundings density, an overflow will occur. Gravity currents or in another terms density currents generally have two main parts: a head and a body. The body is the uniform, steady region behind the head. The head, unlike the body, is unsteady and non-uniform, it acts as a boundary condition for the body. Density difference can be caused by heat difference or the amount of the particles. We can observe gravity currents everywhere around us, even in daily life. For example, when pouring some cold milk in a hot black coffee, the density of cold milk is greater than the hot black coffee itself. So, denser milk will sink below the hot less dense coffee. Stirring increases the turbulence, hence it will reduce the density difference. Another example of density currents occur if you open the window when it's cold outside, dense cold air will flow along the floor and the warm less denser air will flow along the ceiling. We can also see density currents in nature. Snow avalanches are a good example for this. Avalanche is dense, contains a mixture of snow particles and air. The atmosphere surrounding the avalanche is only air so its density lesser than the avalanche. Despite everything, nature finds a way to heal itself, unlike man-made structures and scenes. In the industry, it becomes more important to understand density currents and their dynamics, because nature has a balance and we need to maintain the balance as it is. Heavy saline water is a waste that comes out at the end of a variety of industrial processes, such as fresh water treatment from sea water (desalination), cooling water intake and discharge for fossil fuel-fired power plants, etc. Also called as "brine", heavy saline water generally tends to settle on the seabed right after the initial mixing. Posing very serious threat against the marine life and marine ecosystem balance, the brine layer does not mix at all or mixes with a very slow rate once the initial mixing is completed. Brine layers are known to keep their coherence for very long timespans on the sea bottom. Although there are quite many studies to the understanding of brine mixing, by means of physical and numerical modeling, the phenomenon still keeps its mystery from many different aspects. Especially the effect of seabed slope, seabed topography, longitudinal and/or lateral currents as well as the role of wave activities and transverse current's effects are not completely understood yet. In this sense, density currents have studied by many researchers for a long while to find out how the fluid which is denser than its surroundings move and spread. Some of the researchers study with a laboratory experiment while the others set up a numerical model. In this master's thesis study, the primary purpose is to investigate the progress of brine via density current as well as the long-term mixing of brine in the marine environment by numerical modeling. To accomplish this, first, a benchmark case has modeled. As a reference model, Firoozabadi (2009) was studied as a paper and numerical model. As far as we know from the paper, they did laboratory experiments to investigate turbulent saline density current in a straight channel. They gathered data from this experiment and used it to create a numerical model of the flow. Thus, they can compare the results with laboratory experiments and the numerical model. In this master's thesis, when the validation of the numerical model with the reference model is done, the influence of the transverse currents into the process was studied parametrically via the numerical model. The numerical model was set by a CFD program called Fluent which is created by ANSYS. In order to set up models firstly, geometry was created. Due to limitations in the academic version of Fluent, the channel length is 6 meters, channel height is 0.6 meters and the channel width is 1.5 meters. Sluice gate width is 10 cm and height is 1.25 cm. The bottom slope was given as 1% and the flow rate was given as 20 l/min. Thus, the velocity for the heavy fluid was calculated as 0.2667 m/s. In the reference model channel length was 12 meters and the others remain the same. In the reference model, there is a table which shows the experimental conditions. In this table, they gave bed slopes, flow rates, initial concentration values, inlet Richardson numbers, inlet Reynolds numbers, and temperatures. According to this table, they did 7 runs in the laboratory, changing the slope and the flow rate. Next step was to create a mesh system for this geometry. In the reference model, the final grid was 200x60x73. Since our channel length is half of the channel which is in the reference model, the final grid for our numerical model was 100x60x73. After that, in the setup part, proper settings were made. All the models have two phases; the primary phase is the tap water (ro=998.83 kg/m3) and the secondary phase is the fluid mixture which is saline water (ro=1008.301 kg/m3). In order to model the benchmark case, 7 models were created to find an optimum model that represents the reference model. In the setup part, turbulent models, turbulence model constants and/or initial values were changed in these models. As a result, pressure-based, transient, Eulerian as a mixture model, dispersed RNG k-ε model as a turbulence model was used. Turbulent model constants were C-mu=0.09, C1- epsilon=1.44, C2- epsilon=1.92, C3- epsilon=0.2. Boundary conditions were set up as "wall" for the inlet, "velocity-inlet" for the mixture gate, "outflow" for the outlet, "wall" for the left and right walls and the bottom. For the mixture gate, the secondary phase velocity is 0.2667 m/s. All the initial values were set to zero. The calculation was started for 0.25 seconds as time step size and 3600 as the number of time steps. The benchmark case has modeled and the results have gathered. It is noticed that there are some differences between our model and the reference model. First of all, in the reference model, they did not mention the time period of the numerical model. In our case, our reference model worked for 900 seconds. Since we don't know the time period of the reference numerical model, it may have a huge difference. In the reference model, they developed a finite volume in-house CFD code. They modeled saline water by Boussinesq approximation and used SIMPLEC scheme as a pressure correction scheme. In this master's thesis, ANSYS Fluent has used as a CFD software and SIMPLE model has used as a pressure correction scheme. Differences like these can cause to get different results. After the benchmark case was modeled, the transverse current was added to the numeric model. Transverse current was created from left wall to right wall for 6 different velocities: 0.001 m/s, 0.005 m/s, 0.01 m/s, 0.015 m/s, 0.03 m/s and 0.05 m/s. Therefore, boundary conditions for the left wall were changed as "velocity-inlet" and the right wall as "outflow". Eventually, 6 numerical model was created for 6 different velocity values. The aim here is to investigate the effect of transverse current on the density currents. As the velocities are increased, the density current is deferred to the right. The results are showed us, transverse currents were increased the lateral spreading and reduced the vertical mixture.