In the CFD simulations meshing the model is the most important stage and the

meshing technique applied will have direct impact on the quality of the mesh. Desired fluid flow equations are solved by the mesh which creates the elements, and the size of the elements or grids will have key impact on computational time. This has direct connection with the cost of simulation. Also, convergence speed and accuracy of the solution depend on the quality and quantity of the mesh elements or grids. During meshing, inflation is applied in areas near the walls and boundary layer mesh. Figure 2(a) shows the meshing done without inflation option and Figure 2(b) is the detail sizing of the important areas in the Figure.

At the start the meshing process was done by the coarse mesh as shown in Table 2. The quality of the mesh was done by applying statistics shown in Table 3

Skewness and aspect ratio are among the most important parameters for quality check on the mesh. In order to avoid the solution to easily diverge the maximum skewness should be below 0.98 [5] [7]. Skewness value range varies from zero to one, where the best value is zero and worse is one. To make sure that the skewness is below 0.98, a medium or fine mesh is applied. A fine relevance center as well as other final settings shown in Table 3 will lower the maximum skewness below the most rigid limit. The aspect ratio is obtained when the longest edge length by the shortest edge is computed. Cells become square and have equal edge length of any shape when the aspect ratio is one. It is recommended that, the change in cell size be regular and should not exceed 20% change from one cell to another [6].

It is important to do mesh inflation as in Figure 3 in the areas which are close to the walls by adjusting setting shown in Table 3. The stings used to avoid collision of the meshing process are stair stepping or layer compression. For the 20 percent growth rate, there are 5 layers and maximum thickness of 2.0 mm. Air inlets and fuel inlets are very small. During meshing sweep method, face sizing and edge sizing have been considered.

The mesh independent test was performed to ensure high quality simulation and high accuracy of the modeling. In order to simulate the temperature profile in combustion chambers of the incinerator, grid independent test study was done for different mesh settings. The mesh sizes for grid A, B, C and D were 0.2 mm, 0.1 mm, 0.03 mm and 0.05 mm respectively. The ortho skew for grid A, B, C, and D was 0.6724, 0.7203, 0.7342 and 0.7499 respectively. In order to avoid

solution to diverge, the maximum skewness should be below. 0.98. Different grid sizes are shown in Figures 4(a)-(d) and temperature is compared for each specific grid size. The graph show that grid C and D have similar characteristics as can be seen in Figure 5. The temperature in the combustion chamber ranges between 930 K - 1700 K, which means that the grid was independent.

It is important to check the mesh quality and see if they are at the acceptable range. One of the quality checks is the orthogonal quality which ranges from 0 to 1, such that the lower values mean that the mesh is of low quality. In this study, the minimum orthogonal quality is 0.3177. Density based and pressure based is the settings selected depending on the type of solver. Solver should be selected for velocity formulation setting, that is absolute and relative, and also for the time between steady and transient. Pressure-based, absolute velocity and steady solver was used in this study. Also, the setting for gravitational acceleration was made at 9.81 m/s² in the Y direction. Table 4 shows the settings used to make the plane surface of the incinerator.

Other important settings for model such as energy, radiation, turbulent viscosity and species were done since these parameters are directly related to the simulation circumstances. The energy equation was turned on because during MSW combustion temperature is expected to change. For realizable k-epsilon, turbulent viscous model was selected applying standard wall function. The discrete ordinate (DO) and non-premix combustion was selected for radiation and species respectively. Table 5 shows the probability Density Function (PDF) and the boundary condition for the fuel and oxidant. ANSYS-FLUENT interpolates the PDF during solution of the non-premix combustion model.

In the simulation, methane (CH₄) is used as fuel to support the combustion process during MSW incineration. The oxidant consisted of 79 and 21 percent nitrogen and oxygen respectively and the temperature for fuel and oxidant was set at temperature of 315 K. The pressure was set at 101,325 Pa. The PDF table

was calculated and results were displayed by choosing the type of Figurewhether to be 2D or 3D and type of parameters to be displayed. For this case the default is 3D Figurehaving mean temperature, scaled variance and mean mixture fraction. Settings for the air inlets, fuel inlets, chimney and walls represent the boundary condition. In this study, the incinerator model consists of two air inlets, two fuel inlets, one chimney and twelve walls.

The momentum setting of air inlet and fuel inlets for velocity specification method applies the component method. Setting of velocity for air inlet was done in the X and Y direction and the air temperature was set at 315 K. The zero value was applied to species setting in the mean mixture fraction and the unity value was set for mean mixture fraction. The method used for the turbulence specification is intensity under the hydraulic diameter which was set to 5% and hydraulic diameter of 600mm according to model measurements. The setting of the air and fuel inlet velocity was set in meter per second because this is the most important parameters to consider during MSW combustion. “Stationary wall” method was used for the walls setting having no slip shear condition applying thermal heat flux of 0 w/m² and internal emissivity of 1.

Chemical reactions are involved in this model simulation as it is a non-premixed combustion process consisting of heat transfer, turbulent flows and species transport. The simulation applied the Navier-stokes equations which have been solved together with a realizable k-ε turbulence model. The model simulation was solved by using commercial CFD software ANSYS Fluent 16.1. The Discrete Ordinate (DO) radiation model involving absorption coefficient of the weighted sum of gas (WSGGM) was applied. The original and new setting for the solution in this case is shown in Table 6. Presto was used for pressure and the couple method was used for the pressure-velocity coupling scheme with at least square cell-based gradient.

The second order upwind is preferred for the momentum, turbulent kinetic energy, turbulent dissipation rate, pollutant no, energy, discrete ordinates, mean mixture fraction and mixture fraction variance during final running of the solution. Table 6 presents the solution control for flow courant number, explicit relaxation factor (ERF) and under-relaxation factor. Original values of the parameter settings are needed to run the simulation at the start and thereafter to evaluate the results. Simulations involving chemical reaction including combustion, sometimes the original setting can cause divergence error and therefore require more concentration. When there is a divergence, the flow courant number and relaxation factor should be changed depending on the type of error. Enthalpy was the error in this study and after applying the new settings the flow courant number was reduced from 200 to 50. Also, it reduced the relaxation factor for momentum, pressure and density as presented in Table 7.

The residual of convergence criteria is used for monitoring simulation and calculation process. The simulation was set up with time steps of 1e⁻³ s which led to 3000 iterations to ensure that convergence is reached and at the beginning, the hybrid was selected. Calculations were performed until convergence is reached, that means until when the species residuals were less 10⁻⁶ to make sure no concentration fields are developing. In this study, the patch is used for Y velocity, which is used to force the flow downward for the exhaust gas recirculation to the chimney. The patch for Y velocity is −9.81 m/s². The second patch is for temperature which is 315 K.

To ensure error free, a check case is performed before any calculation process is started. The mesh quality, models, boundaries and cell zone, materials and the

solver are checked by the check case. In the current study, the calculations were performed by setting 3000 iterations as indicated in Figure 6. During model simulation, the convergence is reached easily when a set of equations are solved. After solving the gas flow equations, the particles route interacting with the flue gas are also solved. Later, the chemical reaction and enthalpy equations for combustion are calculated. These calculations are repeated several times until the flow and temperature is converged.