Fluent Is a Commercially Available Software That Uses Computational Fluid Dynamics (CFD)

1.1.1CFD Analysis

1.1.1.1Introduction

Fluent is a commercially available software that uses Computational Fluid Dynamics (CFD) to analyze and solve 2D and 3D flow fields. CFD uses conservation of mass, conservation of energy and transport equations, otherwise known as Navier-Stokes equations, at points in the flow field to calculate pressures, velocities, temperatures and other flow characteristics based on specified boundary conditions. There are two main sections to complete the CFD analysis.

The first section is gambit, a pre-processor where the geometry is built, meshed and the boundary entities are defined. The model is built based on a xyz coordinate system. Points, edges, faces and volumes are created to form the geometry. The geometry is then carried through Boolean operations such as splitting, uniting or subtracting to obtain a physical connection between intersecting parts. Once the geometry configuration has been established, it is a good practice to connect all the points, lines (edges), and faces to avoid mesh complications. One can locate the critical areas in the geometry by obtaining the location of the shortest edge. This technique will be useful to visualize where the meshing operation might fail. The next operation in pre-processing is meshing the geometry. Knowing the model’s unit scale, one must choose appropriate size intervals at the critical regions and stretch the mesh at the less critical regions. Gambit provides structured and unstructured meshing techniques. Structured mesh uses quadrilateral elements while unstructured mesh uses triangular elements. Unstructured mesh is used for geometries that have significant obstructions. The use of structured mesh is recommended to minimize the maximum element skew level. It is important to check the element skew level upon completion of mesh. Desired maximum element skewness for a typical 3D model with an unstructured mesh is 85% or below. Values greater than 95% might affect the computational results. The final step for completing the pre-processing section is to define the boundary entities. For example: inlets, outlets, boundaries that will behave as walls, rotating fluid regions, stationary solid regions, etc. Finally, the meshed model is exported to be used in the post-processing section.

The second part of a CFD analysis uses Fluent, a post-processor where the meshed geometry is imported and the boundary conditions are defined so that the model can be solved. Typically, the imported geometry is scaled to the appropriate unit that it was built in. Then the domain is reordered to reduce or simplify the bandwidth of the matrix formed to solve the model. The user must then setup the operating conditions, such as the reference working pressure, gravitational effect, and working temperature condition. The solver is chosen based on the flow characteristic. There are two types of solvers that Fluent uses. The Coupled solver, typically used for compressible flow (M>0.3), and the segregated solver, usually used for incompressible flow (M<0.3). The segregated solvers solve each of the transport equation separately, whereas coupled solvers solve all the transport equations simultaneously. The working fluid’s materialistic properties are defined in the materials panel. Fluent has capabilities of running different types of working fluids or gases depending on the desired design operation. Viscous effects can be modeled by different turbulence models provided by Fluent. Standard  (turbulence kinetic energy-turbulence dissipation rate) model is a widely used turbulence model that uses two equations. It is an empirical model, however the approximations obtained are reasonably accurate. Boundary conditions are defined at locations where the fluid is entering, leaving, or rotating in the domain. Unless appropriate boundary conditions are defined, the results will not be correct.

Fluent uses iterative techniques to solve the flow fields. The solution is typically initialized with the inlet conditions where the pressure, directional velocities, temperature and turbulence values are entered. The solution is defined as converged when pressure, momentum, energy, and turbulence residuals are below a defined relative error limit. Typical values for convergence are: pressure, momentum, and turbulence residuals below 1e-03, and energy residual below 1e-06. The solution is controlled and stabilized by using under-relaxation factors for the residuals. By default, Fluent assigns under-relaxation values for each of the residuals. They are well approximated working values for most of the analyses, however there are times that the values must be reduced or increased based on the behavior of the solution. Under-relaxation factors can have great impact on the solution convergence. For example, a low under-relaxation value will make the solution stable, however it will increase the time of the convergence due to smaller iterative steps. A high under-relaxation value will speed the convergence time, but could make the solution unstable and diverge. Therefore, the analyst must make the appropriate selection to stabilize the solution while maintaining a reasonable convergence time (Fluent 6.0 User Guide).

1.1.1.2Analysis

The design team performed 2D CFD analyses to conceptually visualize the flow inside the miniature turbine’s casing. The goal of the analysis was to attain the most efficient flow path to extract the fluid from the domain. The CFD analyses were performed using commercially available pre-processor Gambit 2.0, and post-processor Fluent 6.0. The team’s initial step was to validate that the CFD could be efficiently used to solve models in small scales, such as millimeters. The team contacted Fluent university support engineer Ashish A. Kulkarni and validated that the software was capable of solving problems in these small scales.

Initial design of the casing and the turbine consisted of single inlet, and single outlet with four blades mounted on the turbine. The casing was of a circular design to help the flow gain smooth transition from one section to the other. The model was meshed with triangular elements at 0.25mm interval size. The figure below displays the initial geometry and the mesh.

Figure 5.6 was used as an initial design model to test the forces on the top blade shown in the 12 o’clock position. As observed in the figure, a uniform mesh was used throughout the geometry. The tip clearances of the blade to casing surface were kept large in order to extract the flow easily since there was no rotation defined for the blades. The meshed model was imported and solved in Fluent 6.0. The summary of the setup and the boundary conditions are summarized in the table below.

Table 5.1: Summary of boundary conditions
Solver / Coupled Implicit
Viscous Model /  standard
Temperature / (constant)
Fluid Properties / Air
- ideal gas
Cp – 1006.43J/kg.K (constant)
k – 0.0242W/m.K (constant)
 - Sutherland Law
Operating Conditions / Pressure – 101325Pa (static)
Under-Relaxation / Solid – 0.8 (combination of pressure and momentum residuals)
Turbulence Viscosity – 0.6
- 0.3
 - 0.3
Inlet / M=0.7
a= 347.22m/s
Velocity Inlet – 243.05m/s
Outlet / Pressure Outlet – 0Pa (gauge)
Solution Initialization / Pressure-0Pa
x-velocity: 243.05m/s
y-velocity: 0.1m/s
z-velocity: 0.1m/s
- 0.025m2/s2
 - 0.025m2/s3

Using the above conditions, the model was solved in steady state. The static pressure contours, velocity contours, and velocity vectors were obtained (See Appendix F). Knowing the length of the blade and the pressure difference between the upstream and the downstream side of the top blade, the force per unit depth was calculated by Fluent to be 111.94 N/m-depth. Figure 5.7 above show the static pressure contours in the casing. Notice that at steady state, high-pressure region is observed at the root of the blade.

To obtain the forces on the top blade at different angles of rotation the model was modified by rotating the blades 10°, 20° and 45° clockwise. At those configurations the forces on the top blade was calculated as:

10°: F=142.13N/m-depth

20°: F=122.04N/m-depth

45°: F=112.82N/m-depth

The pressure contours revealed that the maximum force on the blade was at 10° configuration. This analysis was conducted to approximate the torque that would be generated due to the forces on the blades. Assuming a 1mm depth, the forces on the turbine blades were sufficient to overcome the estimated torque needed by the generator. Another reason the forces on the blades were calculated was to observe the stagnation points, which might cause structural failure.

The models presented in figures 5.8, 5.9, and 5.10 display the gauge pressures inside the casing and the turbine assembly. As one might expect, the forces on the top blade decreased as the geometry was rotated. The pressure contours illustrate the shift of the high-pressure regions due to the rotation. Since there were no rotational effects in these steady-state solutions, the casing behaved as a pressure tank. This behavior is clear in figure 5.9. Once again, the purpose of the analysis observed above was to obtain the forces on the blades at different turbine configurations. Therefore, pressure contours were the key components in obtaining the forces and the stagnation points on the blades.

The mass-flux balance showed that the total mass flow coming into the domain was not efficiently balancing the mass flow that was exiting. One of the reasons for this problem was the location of the outlet. The design team’s next step was to modify the geometry so that the maximum torque could be achieved with an optimum flow performance. The multiple-jet concept was a candidate to achieve this goal. The figures 5.11 and 5.12 show the modifications made to the initial model that was used in the preceding analyses.

The geometry show in figure 5.11 is similar to the initial design, with the addition of a second inlet and outlet introduced in the lower section. The second inlet was located at the lower right quadrant and the outlet pertaining to the second inlet was located at the lower left quadrant. Figure 5.12 shows a modified version of the geometry of figure 5.11. The outlets were relocated to extract the mass flow efficiently. The boundary layers were also meshed at a lower interval size (0.1mm) to capture the turbulence effects.

As it is observed from the figure 5.13, the velocity vectors do not exit the domain effectively. In order to obtain an optimum flow performance, the flow entering the control volume must exit efficiently. Any disturbed flow in the casing will cause losses that will affect the performance of the design. The mass-flux balance of the model shown in figure 5.13 was on the order of 1e-02kg/s, which signified that there was still some mass-flow remaining in the domain. An ideal mass-flux balance would be 0 kg/s, but for these analyses the limit was set to 1e-05 kg/s.

As it will be observed in the next sections of the analysis, the multiple-jet concept led to flows that were more symmetrical than the single jet design.

An option that the design team had was to introduce a rotating reference frame that would simulate a steady-state performance of the rotating blades, which simulates actual condition of the rotating turbine. In Fluent 6.0 this approach is referred to as Multiple Reference Frame (MRF). The model in figure 5.14 below was used to experiment with MRF. The boundary conditions for the rotating fluid region were defined as a moving wall with an angular velocity of 50,000rpm (optimum rotational velocity for the generator). The inlet speed was reduced to 10m/s because the speeds that were used in earlier models exceeded the desired rotational speed of the generator (50,000rpm). Velocity vectors illustrated in figure 5.14 show the flow behavior when rotational effects are taken into account. The new configuration for the outlets enhanced the flow performance by extracting the mass-flow much more efficiently. In this model the mass-flux balance was reduced to 1e-6.

The model analyzed to the left contained a large tip clearance to simplifying the convergence. Traditionally, the tip clearances in turbines are at their minimum to increase efficiency. Therefore, the next step taken by the design team was to modify the geometry of the turbine and the casing to strengthen the design by reducing the tip clearance.

The model to the right, figure 5.15, is composed of eight blades separated by 45°. The geometry was meshed using 0.1mm interval size. The inlet boundary condition was modified due to the changes in the geometry. The new inlet velocity was 28.6m/s. The rotational velocity remained at 50,000 rpm. The results obtained from this analysis did not illustrate a symmetric flow pattern within the structure and therefore raised the concern of the team.

As it is observed from both the pressure contours and the velocity vectors of figures 5.16, and 5.17, the behavior of the flow was not realistic. The team expected a symmetric pressure and velocity distribution along the flow field. Boundary conditions were re-checked to make sure that both inlets had the same velocity rates. The entropy contours, figure 5.18, were inspected to see if the grid had a discontinuity, but none were observed. Finally, the team had discovered the problem that lead to unrealistic results. The solution initialization for x-velocity was the cause. Typically, the solution is initialized with the velocity rate observed at the inlet. In this model, both inlets were initialized with an x-velocity of 28.6m/s. When the solution was initialized using very low value for x-velocity (1m/s) the results were much better. The figures 5.19 and 5.20, which are the static pressure contours and velocity vectors, show a symmetric pressure and velocity distribution.

The team’s final modifications were to increase the inlet velocity slightly to obtain a free spinning turbine and to reduce the tip clearances to an absolute minimum. Figure 5.21 displays the geometry with reduced tip clearance. The reason to reduce the tip clearance is to be able to move the air more effectively. This in terms will increase the flow performance and hence increasing the efficiency of the turbine. The velocity vectors displayed in figure 5.20 illustrates that the rotation of the blades was driving the flow rather than the nozzle. This meant that the team needed to increase the inlet velocity to make sure the nozzle was causing the turbine to rotate.

The static pressure contours in figure 5.22 validates a free spinning turbine. The velocity vectors in figure 5.24 illustrates that the inlet speed is driving the rotational flow. The reduced tip clearances increased the efficiency of the turbine by preventing the air from flowing around the blades. However, reducing the tip clearances increased the tip velocities significantly. The maximum velocity observed at the tip was approximately 104 m/s. Even though the tip velocities increased significantly, the flow was still incompressible (M<0.3 subsonic/incompressible). To validate the grid independence, the future models will be meshed with finer meshes at the tip clearances. All the models observed in this analysis section are presented in detail in Appendix F.

The 2-dimensional CFD simulations helped the team to visualize and optimize the flow inside the casing. The steady state analyses helped gain an understanding of the forces observed at the blades. To maintain the structural integrity of the blades the stagnation points are important key factors for the designer. The configuration of the inlets and the outlets were obtained based on the model performance using iterative steps. The team observed the model performance, brainstormed the variables that would impact the efficiency, and modified the geometry predicting better results than the previous model. The CFD simulations were preliminary steps to design an optimization tool. The design team’s goals for the future are to validate the 3D CFD simulations with the experimental data, and also to optimize the existing model to obtain an ideal flow performance. Due to close interaction between the blades and the casing, sliding mesh technique was suggested by the Fluent technical support. The team will explore this technique in future analyses.