Under construction: Projected finish date: 5/18/2008 Sunday

CFD Simulation Scientific Paper (By: Jorge Rodriguez, Yong Sheng Khoo)

Title: Better Understanding of Flocculation Process through CFD Simulation

Abstract

Flocculation is an important process used by AguaClara to treat water. The process involves particle collisions and agglomeration to form flocs. Computational Fluid Dynamics was used to better understand the fluid dynamics in the reactor.  The standard k-e model was used for every simulation model.  The pressure coefficient drop over one baffle turn is 3.75, which agrees with literature estimates.  After a clearance height of one baffle width or greater, the pressure coefficient drop and the maximum velocity become approximately constant.  Most of the energy dissipation occurs in the region after the turn over a distance of two baffle widths.  An area of flow recirculation occurs near the center wall immediately after the turn.  The pressure drop is not sensitive to the Reynolds number for a large range of inlet velocities.  Better understanding of the flocculation dynamics will enable optimized particle agglomeration and break-up. 

1. Introduction

Flocculation is the process by which particles collide and agglomerate. Past research has shown that shear gradients play an important role during flocculation. This process was simulated using Computational Fluid Dynamics (CFD).  The main task of this research is to find the optimum strain rate in the reactor to influence particle collision. Gambit and FLUENT were utilized to model one baffle turn. Gambit was used to create the geometry of the flocculator, and to generate the mesh.  FLUENT was used set up the boundary conditions and to obtain the results.

2. Methodology

The real life flocculation tank used by AguaClara involves 180 deg turns over few dozens baffles.  To save computational effort, a simple 180 deg turn over two baffles was modeled. The first step was to set up the geometry of the turn.  For future comparison with the experimental data, the design parameters for the pilot plant were used. The modeling approach was to create the geometry, mesh it, set boundary conditions, and solve it using FLUENT.

2.1 Creating Geometry 

Figure 1. Geometry of Flocculator

The design parameters used are:

Height: 1 m
Clearance: 0.15 m
Baffle width: 0.1 m
Velocity inlet: 0.1 m/s

With the geometry, the mesh for the model can then be set up.

2.2 Setting up Mesh 

Figure 2. Meshing Parameters (Click on the figure to see the original size)

 
Figure 2 shows the meshing parameters that were used. The boundary layers was first established at all the wall surfaces. The boundary layer was set such that the solution would provide a result of y+ less than 5. After that, the mesh edges were set up such that they will provide higher mesh resolution near the turn.  With the initial meshing conditions set up, all the faces were then meshed.

 
   
Figure 3. Mesh of the Model (Click on figure for original size)

Figure 3 shows the overall mesh of the flocculator model. As can be seen, the mesh is fine near the turn and at the wall.  The final step at this point was to set up the boundary conditions of the system.

2.3 Setting up Boundary Conditions 

Figure 4. Boundary Conditions

Figure 4 shows the boundary condition that was used for modeling. For a flocculator, there is an in flow and out flow of the fluids. Since inlet velocity inlet was known from the experimental data, the inlet was set to the Velocity Inlet type boundary condition. The outlet was set to Pressure Outlet boundary condition type, the atmospheric pressure.

The mesh was then saved and exported to FLUENT for further obtaining solution and further analysis.  

2.4 Solve using FLUENT 

At this stage, the Standard k-ε turbulence model was set up.  Water was defined as the working material from the FLUENT database. The discretization method for the momentum, turbulent kinetic energy, and turbulent dissipation rate were set to the 'Second Order Upwind' scheme to obtain a 'Second Order Accurate' solution.  The boundary conditions were set according to the values shown in the table below.  The solution was obtained by iterating until the residuals converged to 10e-6.  Results were then analyzed and plotted.        

TABLE IN BCS TABLE 1

2.5 Mesh Sensitivity Analysis

The effect of the number of mesh elements on the result was also carried out. Coarse, medium and fine meshes were created and the pressure drop across the turn from each mesh was compared. This analysis will provide confidence on the accuracy of certain mesh. If the changes in mesh elements does not result in a lot of change in pressure coefficient drop, it is concluded that the mesh elements were refined enough that the truncation and discretization errors can be neglected. Table 2 shows the summary of 3 meshes created for mesh sensitivity analysis. Please refer back to figure 2 for corresponding meshing parameters.

Table 2. Mesh Meshing Parameters for Coarse, Medium and Fine Meshes

2.6 Effect of Reynolds Number

The effects of Reynolds number was examined. AguaClara water treatment plant is built in geographically diverse area where the flow rate into the flocculator is different. Hence, it is important to understand the effect of Reynolds number on the results.

2.7 Parameterization

At the later stage of project, after the confident on result of the model was built up, the effect of geometry on results was analyzed. Different clearance height was used for analyzing new results as a result of this effect. It would be tedious to individually recreate each geometry and mesh for different clearance height from scratch. For this reason, parameterization technique was used. The original Gambit journal file was modified to include the variable clearance height. Using this method, changes in corresponding clearance height was plug into the journal file and run using Gambit to obtain desired mesh and geometry. The journal files used for such parameterization is included in the Appendix.

2.8 Comparing Turbulence Model

Different turbulence model were also employed for comparing the effect of different turbulence model. Standard K-ε, K-ε Realizable and K-ω turbulence model were used and the results were compared.

3. Results and Discussions

Some of the important results are the velocity vectors, contour of pressure coefficient, contours of pressure coefficient, contours of strain rate and contours of turbulence dissipation rate.

Figure 5. Velocity Vectors (Click on figure for original size)
 
Velocity vector plot shows the velocity of the fluids throughout the flocculator.  As can be seen, there is a region of high velocity at the outer turn and recirculation at the inner turn. At the bottom of the flocculator, there is region of stagnant fluid.
 

Figure 6. Contours of Stream Function (Click on figure for original size)
 
Contours of stream function tell us how the fluid travel in the flocculator. As can be seen from figure 6, there is enclosed streamline at the inner turn. The enclosed streamlines means there are recirculating fluid which are trapped in the region.

 
 

Figure 7. Contours of Pressure Coefficient

Figure 7 shows most of the pressure coefficient drop occurs around the bend. There is a pressure coefficient drop of about 3.7 across the bend. (Talk about the experimental result. Literature review data)

Figure 8. Contours of Strain Rate

Contours of strain rate shows high strain rate right before and after the turn. There are also high strain rate near the wall. The region with high strain rate is the region where the flocculation occurs.

Figure 9. Contours of Turbulent Disssipation Rate

Contours of turbulent dissipation rate shows about the same trend as the contours the strain rate right after the turning. The region of high turbulence dissipation after the turn is about twice the length of baffle spacing (research literature). The high dissipation rate after the turn is because of the expansion of the fluid.

Figure 10. Wall Yplus

Figure 10 shows the yplus at wall was consistently less than 5.  FLUENT documentations mentioned that "the mesh should be made either coarse or fine enough to prevent the wall-adjacent cells from being placed in the buffer layer (yplus = 5~30)". Since the yplus from the model was consistenly less than zero and was in the region of viscous sublayer, the turbulence flow near the wall was able to be resolved properly.

Figure 11. Mesh Sensitivity Analysis

Figure 11 shows the pressure coefficient drop over one turn with different mesh densities. The pressure drop given by the fine mesh is the most accurate. This is because as the mesh get finer, the truncation error is reduced and provide more accurate result. However, as the mesh get finer, the computational times also increase. To determine is it worth extra time to obtain further accuracy, mesh sensitivity analysis is carried out. Pressure coefficient drop for three meshes is about the same. Hence it is concluded that coarse mesh is good enough to provide reasonable result.

Figure 12. Reynolds Number Effect on Pressure Coefficient Drop

It is important to take a look at the effect of Reynolds number on the results as water treatment plant built by AguaClara varies geographically. The flow rate into water treatment plant is different for different location. Reynolds number is changed by changing the inlet velocity boundary condition. The normal flow rate is of Reynolds number of 10,000. From figure 12, it is seen that the pressure coefficient drop changes only a little with big changes in Reynolds number. In other word, the pressure coefficient drop is not sensitive to the Reynolds number of the system. This is a good thing because in the design of flocculator, the flow rate of the geographical location can be neglected. One set of flocculator design can be used for different flow rate.
 
Figure 13. Clearance Height Effect on Pressure Coefficient Drop and Maximum Velocity

By adjusting clearance height, the effect on the pressure coefficient drop was also analyzed. It can be seen that the pressure coefficient drop is independent of the change in clearance height as long as the clearance height is greater than a certain critical value. Figure 13 shows that after a critical value of 1, the pressure coefficient drop is constant. This phenomena can be explained using figure 5. Figure 5 shows the clearance height of 0.15 m. However, from 0.1 m onward, the flow is mostly stagnant in the flocculator. This mean that 0.1 m is needed for the flow to navigate through the turn and after this point onward, there is not much activity happening. Clearance height of less than 0.1 m gave higher pressure coefficient drop as it created a constriction of flow and the frictional loss was increased. With this result, it is recommended for the design team that the clearance height must be at least the same of bigger than the baffle width to produce predictable pressure coefficient drop.

Figure 14. Comparison of Turbulent Dissipation Rate for Clearance height of 0.1 m and 0.15 m

To further validate that the result is not sensitive to the change in clearance height, the contours of turbulence dissipation rate of clearance height 0.1 m and 0.15 m was compared. The result showed that the region of active turbulent dissipation was the same, about two times the length of baffle spacing. With this result, it is concluded that the design team has the freedom of choosing clearance height according to their design constraint and not theoretical constraint as long as the clearance height is greater than the baffle spacing.

Figure 14. Effect of Turbulence Model on Pressure Coefficient Drop

 4. Conclusions