# CFD Simulation of Solid Suspension for a Liquid-Solid Industrial Stirred Reactor
## 2 Materials and Methods
Geometry reconstruction of the industrial stirred reactor and its meshing were performed with the software Gambit 2.4. The mesh consists of approximately 1.1 million tetrahedral elements. As regards the mesh quality, we were restricted to use tetra mesh elements due to a greater number of previous case studies [2; 3]. For our numerical investigation, a very high quality of mesh (skewness < 0.6) was ensured throughout the computational domain. In order to use the sliding-mesh method, four fluid zones were defined: an inner rotating cylindrical volume centered on the impeller and three other volumes containing the rest of the reactor and the baffles. The interface is located at an equal distance from the blades of the impeller and the inside edge of the baffles. An illustration of the domain and the mesh of the domain is given in Figure 2, which shows that finer meshes were used around the impeller where the velocity spatial gradients are expected to be large. Good care was taken in keeping the same mesh dimension between the rotating and the stationary interface to ensure a good exchange of the hydrodynamic quantities between the two zones during calculation. A \"no-slip\" condition was applied on all walls of the geometry. Simulations of the turbulent multiphase flow were then performed with the help of the commercial CFD code Fluent 16 using the RNG \(k\)-\(\epsilon\) model. There are two working materials corresponding to the two phases, liquid and solid: liquid with density \(\rho_{l}=690\) kg\({}^{*}\)m\({}^{-3}\), powder with density \(\rho_{p}=1520\) kg\({}^{*}\)m\({}^{-3}\) and particle size \(d=0.000171\) m. At the liquid surface, a gas zone consisting of air was added at the free surface of water, a method that has been reported to dampen the instabilities, which means the top surface is exposed to atmospheric pressure. The flow resolution was unsteady, and the sliding-mesh approach was employed. At each time step, the position of the rotating zone relative to the stationary one was recomputed, and the grid interface of the rotating zone slid along the interface of the stationary zone. For all simulations, the time step was set as a function of the impeller speed, 65 rot/min, and the number of the cells from the interface surface, approximately 140 elements, so the time step was set to a value of 0.01 s.  
At the end of each time step, after a maximum of 5 iterations, the convergence criterion reached \(1-\) for the continuity, momentum and turbulence quantities. This value of the convergence criteria was set to have a total computational time of 120 h. Although the value of the criteria might be considered to be a course for complex Eulerian multiphase flow, the objective of the current research was to obtain an accurate enough result in a short period of time in order to make a practical decision. Simulations were performed in double precision with the segregated implicit solver. Transient formulation was of the first order, and the spatial discretization scheme for pressure was PRESTOI and for momentum and turbulence was QUICK. The SIMPLE algorithm was employed for the pressure-velocity coupling [15; 16; 17; 18; 19; 20]. The analysis of the results was performed after a total flow time of 90 s.