65 Application Of Finite Volume Method

Implementation of the basic steps of the finite volume method discussed above to solve the governing equations of a flow model requires development of a computer

FIGURE 6.11 SIMPLE family of algorithms for unsteady flows.

program. Development of a computer program involves many issues and is outside the scope of this work. It is assumed that suitable computational tools are available to a reactor engineer. Key issues which need to be considered when selecting suitable computational tools, are discussed in Chapter 8. In this section, various issues relevant to computational flow simulations are discussed with the help of a simple example. Consider a cubical vessel with rectangular inlet and outlets as shown in Fig. 6.12a. Geometrical and other details are given in Table 6.1. Simulations were carried out for four different viscosity fluids (in the range 0.001 Pa.s to 100 Pa.s) to determine the possible influence of viscosity on the numerical solution of model equations.

Inlet iA\

outlet

Inlet

outlet

FIGURE 6.12 Outline of vessel (isometric and two-dimensional approximation).

TABLE 6.1 Data Used for Simulation Example

Three-dimensional vessel (Fig. 6.12a): Volume = 1m3

Length = Depth = Breadth = 1m Inlet area = 0.1 x 1.0 = 0.1m2

(Distance between top edge of inlet to vessel edge = 0.1m) Outlet area = 0.1 x 1.0 = 0.1m2

(Distance between bottom edge of outlet to vessel bottom = 0.1m)

Two-dimensional approximation (Fig. 6.12b):

Inlet velocity = 1ms-1

Fluid viscosity = 0.001 Pa.s, 1 Pa.s, 10 Pa.s and 100 Pa.s

6.5.1. Solution Domain and Computational Grid

The first task in initiating a numerical simulation is to select an appropriate solution domain and formulate appropriate boundary conditions to specify the influence of the environment on flow processes in the considered solution domain. Flow in a cubical vessel with rectangular inlet and outlet can be conveniently modeled by considering a two-dimensional geometry, if the end effects are assumed not to be important. In any case, it can be seen that the most important flow processes occur in the x-y plane. It is, therefore, useful to examine various numerical issues such as the required number of grids, discretization schemes etc., by carrying out two-dimensional simulations. If necessary, after identifying an adequate number of grid points, a complete three-dimensional simulation may be carried out to verify the adequacy of the two-dimensional approximation. A two-dimensional solution domain was therefore considered for numerical simulation of the flow in a cubical vessel (Fig. 6.12b).

The next issue is the formulation of appropriate boundary conditions. The availability of suitable boundary conditions may also affect the decision concerning the extent of the solution domain. Obviously in practice, the inlet and outlet of any vessel will be connected to the associated pipe work. It is essential to decide the extent of the solution domain in such a way that it does not affect the simulated results. Generally for high velocity inlets, conditions in the process vessel do not affect the flow characteristics of the inlet pipe, and therefore it is acceptable to set the inlet boundary conditions right at the vessel boundary. More often than not, some piping at the outlet section may have to be considered if the outlet boundary condition is to be used. Alternatively, one may use constant pressure boundary conditions. Possible boundary conditions and solution domain are shown in Fig. 6.13. Before examining the influence of the solution domain on the simulated results, it is necessary to identify an adequate number of grids to resolve all the major features of the flow.

Flow simulations in the simplest solution domain (Fig. 6.13a) were carried out with different numbers of grids: 10 x 10, 20 x 20, 40 x 40, 80 x 80. Commercial CFD code, FLUENT (Fluent Inc., USA) was used for these simulations. Since the geometry of the proposed solution domain was simple, it was possible to generate a suitable computational grid using the tools provided within FLUENT, and a separate grid generation tool was unnecessary. For all of these four grid levels, uniform grids were used. Typical grids used for simulations (for the 40 x 40 case) are shown in Fig. 6.14. Typical flow results in the form of vector and contour plots are shown in Fig. 6.15. The influence of grids on predicted results is shown in Fig. 6.16. All of these results were obtained for fluid with viscosity 100 Pa.s. It can be seen that there is almost no change in the predicted results for grids beyond 40 x 40. Therefore, 40 x 40 grids (for square geometry) were used to examine the influence of length of the outlet pipe and corresponding boundary conditions. Comparison of predicted results for different configurations is shown in Fig. 6.17. Since the difference in predicted results with and without outlet pipes is not significant, for all further simulations, a solution domain without extensions of inlet or outlet pipes was considered.

Inlet o

Outlet

FIGURE 6.13 Different solution domains.

6.5.2. Convergence and Error Analysis

As mentioned in the earlier part of this chapter, the overall solution procedure is iterative and an adequate degree of convergence needs to be ensured before further processing of simulated results. Usually a measure of how closely each discretized equation is balanced is used to decide convergence. For this, generally the imbalance in the governing equations is summed over all computational cells in the solution domain. Such a sum is called the residual and for a general conservation equation can be written (from Eq. (6.12)):

R = |aePe + awpw + awwPww + aNPn + asps + asspss + sC - aPpP

all nodes

0 0