1. Introduction
In small countries with mostly flat terrains, the explotation of medium- and large-scale hydropower has become prohibitive, due to the great impact of flooding large areas. Nowadays, new hydropower stations in these countries are preferably of mini and micro scales, for which conventional turbines are very expensive [
1,
2,
3].
The evaluation of new devices for micro hydropower schemes usually does not justify the investment that represents the use of commercial CFD codes or the excecution of model tests. On the other hand, a lot of time and money could be spent while trying different designs in the exact location of the scheme. To assess the performance of these new devices, CFD simulations could be performed through open source and freely available fluid flow solvers, which represent a great opportunity to save on investment costs in this kind of projects. If the design and/or evaluation take part within a university research or academic project, the use of this kind of tools becomes even more convenient. Researchers, professors and students benefit from the use of open source fluid flow solvers by having the opportunity to understand and even modify the original codes in order to solve particular issues. Nevertheless, within industrial environments, the use of commercial packages is mostly preferred [
4,
5]. Among a few examples of open source fluid flow solvers, OpenFOAM is by far the most used around the globe, having a great community of developers who help to improve its capabilities. OpeanFOAM was initially developed by Henry Weller in 1989 [
6] and it was made freely available in 2004 [
7].
In this work, we chose to use the open source and freely available fluid flow solver named
caffa3d [
8,
9], developed from a family of 2D flow solvers included in [
10] by researchers of the Computational Fluid Mechanics Group of the Faculty of Engineering of Universidad de la República (Uruguay). It shares several characteristics with other open source flow solvers and it is coded in Fortran 90, demanding lesser programming skills than other packages. The most common and successful applications of
caffa3d are simulation of blood flow to predict the rupture of an intracranial aneurysm [
11,
12], simulation of the wake produced by wind turbines [
13] and evaluation of wind farms, atmospheric boundary layer simulation to analyze wind flows in urban environments and pollutant dispersion [
9], and the development of a numerical wind tunnel [
14]. There was an incipient use of the solver to simulate the performance of a rotating device, specifically a Hydrostatic Pressure Machine (a type of water wheel [
15,
16]), although in this first attempt some difficulties aroused which did not allowed to obtain correct results [
17].
Turbulence modelling is the main issue to solve in most common CFD simulations, included turbomachinery flows. Most researchers use RANS (Reynolds Average Navier Stokes) to model turbulence, along with several closure models such as
and
, meanwhile others prefer the use of LES (Large Eddy Simulation) along with closure models such as Smagorinsky for sub-grid scales. RANS solves the turbulence by time averaging of Navier–Stokes equations, while LES does it by averaging in space while maintaining time accuracy of fluid turbulence, making it more convenient for unsteady simulations. In the field of turbomachinery simulations, RANS is the preferred choice for most researchers [
5,
18], despite of its poor accuracy, due to higher computational cost and the use of not enough fine grids for LES [
19].
When dealing with turbomachinery simulations in CFD, rotating parts are other important part of the problem. The rotation of the machine within the fluid domain could be solved by several methods, such as MRF (Multiple Reference Frames), SM (Sliding Meshes) or IBCM (Immerse Boundary Condition Method). Among the first two, that work with body fitted grids to model the solid surface of the machine, MRF (also called frozen-rotor) handles the rotation by solving the equations in a rotating reference frame (using relative velocities and considering Coriolis and transport forces) for those blocks close to the machine and in an absolute reference frame for the rest of the blocks [
20], while SM solves the equations for the entire domain in an absolute reference frame but it needs to rotate the block grids around the machine and solve the connectivity between the cells of the interface [
8]. In MRF method all the mesh blocks of the domain remain stationary in their respective reference frames, and a steady flow condition must exist at the interface between the subdomains, so it is not useful for transient simulations. In the IBCM [
21], there is no special treatment for the grid, as the solid is represented by an external mass force field acting like the real solid body and imposing a velocity equal to the body’s one in the grid cells lying within it’s surface. For rotating bodies, one need to re-calculate the distance between cells and body’s surface at every time step, making the method computationally expensive.
In addition, in those turbomachines working partially submerged under water, the simulation of two very distinct fluids (air and water) is another challenging task. In order to simulate two phase flows, the methods are devided into Lagrangian approaches, such as SPH (Smoothed Particle Hydrodinamics) described in [
22,
23], and Eulerian approaches which in turn are divided into interface-tracking and interface-capturing methods [
10]. Among the latter, VOF (Volume Of Fluid), proposed by [
24], is the most popular method.
Section 2 presents some details of
caffa3d (including its main equations and discretization schemes), a description of the HPM chosen as case study, the computational domain and mesh, initial and boundary coinditions, solver parameters and fluid properties and method for power and efficiency calculation. In addition, a convergence study and grid sensitivity analysis is presented.
In
Section 3, the use of
caffa3d to simulate a hydropower device is validated through the analysis of the performance of a medium-scale HPM with straight radial blades. Some turbulence characteristics of the flow in the channel are shown. The generated power and efficiency for different discharges are compared with previous experimental results and a qualitative comparison of the flow across the wheel for two distinct conditions is presented. Similar analyses were conducted in the past by other researchers using commercial CFD codes [
25].
The main emphasis of the present study was not to perform a rigurous analysis of the turbulent quantities, but to evaluate the use of caffa3d to assess the global performance of a hydropower device.
3. Results and Discussion
The analysis of the simulation results is divided into four parts. Before presenting the data involved in the validation of the simulation and the characterization of the flow field, some characteristics of the turbulence of the resolved flow are shown. Regarding the validation of the simulations, a quantitative study is presented, where the calculation of the instantaneous power is carried out for different operating discharges of the HPM obtained from the numerical simulations. Then, the average power and efficiencies for each discharge were calculated and compared with the values presented in the HYLOW project. Finally, a qualitative study of the flow in the channel around the HPM is presented, with images of the behavior of the flow and streamlines colored by velocity and pressure.
3.1. Turbulence Charactaristics of the Flow
The main turbulence quantities of the flow were evaluated at one of the operating points of the HPM (
58.9 L/s and
rpm). The Reynolds number calculated from the mean velocity of the cross section of the channel downstream of the HPM and the height of the water in the same section, resulted in
. The Reynolds number of the subgrid scales defined in
Section 2.1.1 took values between 400 and 4000. In addition, the friction Reynolds number calculated from the shear velocity and half of the water height resulted in values around 3000.
In order to obtain an idea of how well the turbulence of the flow was modeled, the spectrum of the turbulent velocity of a given cell element was obtained. The cell under study is an hexaedron of 51 mm × 7.3 mm × 14 mm (in longitudinal, transversal and vertical direction, respectively, and it is located downstream and close to the HPM (at 97 mm above the floor). The spectrum shows the turbulent kinetic energy distribution among all the scales of the flow, from the production to the dissipation scales, as well as the inertial subrange in between. Following Kolmogorov’s hypothesis [
29], a decay of the energy in a rate of −5/3 is expected in the inertial subrange. For a correct spectral analysis, the mean velocity must be steady in the analysed period, conditioned that is satisfied for the three velocity components (longitudinal-
u, vertical-
v and transversal-
w), as shown in
Figure 11 for a period of 86 s.
The power spectrum of the longitudinal component of velocity is calculated by means of the fast Fourier transform, as described in [
40]. For a better definition of the spectrum, the frequency range was divided in three subranges. For the low frequency range (between
and 0.191 Hz), the entire set of data was used to calculate the spectrum. For the medium frequency range (between 0.191 Hz and 2.06 Hz), the data were divided in two subsets and the average of both spectrums was calculated. Finally, for the high frequency range (between 2.06 Hz and
), the data were divided in four subsets and the average of all four spectrums was calculated. The result was normalized by the square of the standard deviation
(representing a power spectral density) and plotted against frequency in
Figure 12, together with the −5/3 decay law. Because the number of data points used to compute the spectrum has to be a power of 2, it was necessary to cut the data to 52.4 s (
data points). The minimum frequency is related to the total time of the data and is assessed as
Hz, while the maximum frequency depends on the average horizontal velocity (
m/s) and the length of the cell element (
mm) and is assessed as
Hz.
From the value of the spectrum at
one can obtain an estimate of the longitudinal integral length scale (characteristic of the energetic vortices) as [
29]:
which in this case resulted in
m (similar to half the height of the water in the channel downstream of the HPM). The turbulence intensity (
) resulted as high as 94%, supporting the choice of LES over RANS to model the turbulence in this study.
3.2. Instantaneous Power
The maximum discharge in the simulations was 120 L/s (higher discharges yielded great instabilities that did not represented the actual performance of the HPM), and the working point L/s was added, which, although it was not included in the experimental tests, was useful to obtain smoother operating curves in a zone of unsteady performance of the HPM. In addition, the point corresponding to L/s was included, which was not part of the experimental tests either. A simulation was carried out in order to evaluate the leakage flow through the HPM (), for which the wheel was left stationary and the same discharge as in the experimental tests (25 L/s) was considered. It was found that the water levels before and after the HPM remained constant for a considerable time (20 s), so it was possible to conclude that L/s in the simulations of the analyzed HPM.
Figure 13 shows time evolution of the instantaneous power of the HPM for discharges 58.9 L/s (
Figure 13a), 97.8 L/s (
Figure 13b) and 120 L/s (
Figure 13c). The first few seconds are not shown, because from the beginning of the simulation up to the first blade passage, a power peak was observed followed by a transient behaviour where the power does not stabilize. The time interval that is plotted in each graph corresponds to four turns of the HPM. In each graph, the red line corresponds to the mean power and the broken black lines represent the intervals corresponding to the standard deviation of the power.
The waveform with the highest frequency presented by the power curves responds to the blade pass frequency of the HPM. In the curves corresponding to discharges greater than 97.8 L/s, this waveform is superimposed with another of lower characteristic frequency associated with a complete turn of the wheel. This last wave increases its amplitude as the discharge increases, even causing the HPM to present time intervals with negative power (see
Figure 13c).
3.3. Mean Power and Efficiency
From the time evolution of the instantaneous power, the average power for each discharge was calculated and the efficiency for each working point was assessed.
Table 2 summarizes the main parameters and results of the operation of the HPM at different discharges. The rotating speeds, which differ from those presented in
Figure 3b and in
Table 1, were selected in such a way that during the simulations the water level before the HPM remained constant at the upper edge of the hub (the level after the HPM is controlled by the height of the weir).
Figure 14,
Figure 15 and
Figure 16 show the Power—Discharge, Efficiency—Discharge and Discharge—Rotating speed curves (respectively), obtained from the numerical simulations, along with the operating points surveyed in the previous experimental tests summarized in
Table 1.
From the previous figures, a very good correlation between the numerical and experimental results can be seen, for discharges between 25 L/s (minimum discharge) and 97.8 L/s (maximum power), concluding that the simulations carried out in caffa3d managed to reproduce the operation of the HPM in this working range. However, for higher discharges, the numerical simulations yielded much lower power and efficiency values, possibly explained by overestimated turbulence modelling. Although it is an aspect to be solved in the model and the numerical simulations, it is still acceptable that it can reproduce the global variables of the real operation between the minimum discharge and that corresponding to the maximum power, including the best efficiency point. It would be very rare to have discharges outside this range in actual operation of this HPM.
Figure 17 shows the comparison error between the values of the different magnitudes (power, efficiency and rotating speed) obtained numerically with
caffa3d and those obtained experimentally in the HYLOW project. The error is expressed relative to the experimental value and it is shown for various discharges.
It is clear that the comparison error in power and efficiency increase rapidly when the discharge goes from 97.8 L/s to 120 L/s. However, for discharges up to 97.8 L/s, the error in power and efficiency remained below 6%, indicating a good correlation. On the other hand, the comparison error in the rotating speed remains low for the entire range of analyzed discharges. This behaviour reaffirms the above comments about the adequacy of the model and the numerical simulations to analyze the performance of the HPM in the operating range between the point of minimum discharge and the point of maximum power.
3.4. Channel Flow Analysis
In order to complement the previous analysis, images of the water flow in the channel through the HPM are presented below, for two operating points. Due to the transient nature of the HPM operation, instantaneous images of the flow are shown for a specific time instant. Such instant was chosen in order to appreciate the characteristic behaviour of the flow through the HPM for each operating point.
The maximum efficiency (from experimental tests) operating point is considered first, with
L/s and
rpm. The following figures show the instantaneous streamlines through the HPM (the images correspond to the same instant of time).
Figure 18 shows the streamlines colored by the magnitude of the velocity vector, while
Figure 19 shows the streamlines colored by pressure.
In both images, several eddies are observed inside the buckets downstream the bottom shroud, possibly due to the interaction of the main flow with the bottom flow coming from the gap between the channel bed and the HPM, which, as it can be seen in
Figure 18 has a higher velocity with respect to the average flow. Another eddy formation can also be seen in the flow inside the bucket that has just entered the water, which could explain the presence of the air bubbles observed in
Figure 20. For the analyzed operating point, there are no low pressure zones associated with the core of these eddy structures, so their presence does not seem to alter the normal operation of the HPM.
Figure 20 shows an image of the flow of water through the HPM obtained by simulations in
caffa3d (left) and presented in HYLOW reports of the experimental tests (right), for similar discharges. The section on
Supplementary Material has the video of the simulation for a complete turn of the HPM.
The previous images show bubbles of air trapped inside the bucket that has just entered the water, which in this case manage to be expelled before the bucket passes through the bottom of the channel (at higher discharges, the air is transported downstream of the channel). Water recirculation is not appreciated, that is to say that all the water transported by the HPM manages to evacuate towards downstream of channel (a desirable situation in an optimal behavior of the machine).
Next, the operation of the HPM with a high discharge is analyzed, specifically
L/s and
rpm, where abnormal phenomena begin to be observed that introduce inefficiencies reducing the absorbed power and the efficiency of the HPM. The following figures show the instantaneous streamlines through the HPM (the images correspond to the same instant of time).
Figure 21 shows the streamlines colored by the magnitude of the velocity vector, while
Figure 22 shows the streamlines colored by pressure.
In the previous images, larger eddy structures can be observed than at the point of operation of maximum efficiency. Furthermore, in the bucket about to exit the water and on the pressure side of the blade, significant negative pressure values occur. This blade in particular is working with a negative torque with respect to the rotation of the HPM, reducing the net absorbed power. This depression together with the delay in the entry of air (and evacuation of water) are responsible for the recirculation of water towards the entrance of the channel.
Figure 23 shows an image of the flow of water through the HPM obtained by simulations in
caffa3d (left) and presented in HYLOW reports of the experimental tests (right), for similar high discharges. The section on
Supplementary Material has the video of the simulation for a complete turn of the HPM.
In particular, it can be seen how the buckets do not empty completely when they exit the water, taking with them some water towards the entrance, which generates a contrary torque that reduces the absorbed power. In addition, noteworthy is the high turbulence produced when the blades enter the water and the large amount of air trapped in the bucket that has just entered, which is not evacuated entirely, reducing the volume of water transported and the force exerted on the blades.
4. Conclusions
In this paper. the operation of a simple Hydrostatic Pressure Machine (a type of hydraulic turbine) with radial straight blades was analyzed by means of the use of caffa3d code, which is an open source and freely available flow solver for incompressible viscous fluid flow that implements the finite volume method in Fortran 90, and has been developed by academic researchers from the Computational Fluid Mechanic Group of the Faculty of Engineering of Universidad de la República (Uruguay). The solver implements the Large Eddy Simulation method to model the flow turbulence, the Volume of Fluid method to simulate open channel flows and the Sliding Mesh method to simulate rotating machinery.
A convergence study was performed in order to assess the adequacy of the total number of iterations used in the simulations. From this study, it was concluded that the actual number of iterations enable to reach a steady value of the residuals of the equations. In addition, a grid sensitivity analysis was conducted, comparing the results for three different total number of elements in the mesh.
The suitability of the simulations to model the turbulence characteristics of the flow was studied, highlighting the distribution of the power spectral density of the longitudinal velocity along the frequencies presented in the flow. For the inertial subrange, the spectrum quite follows the −5/3 decay law predicted by Kolmogorv. The longitudinal integral length scale in the channel downstream of the HPM resulted close to half the height of the water in that section. The high values obtained for the turbulence intensity suggest that the use of LES was adequate.
The time evolution of the absorbed power over a few turns of the wheel for various discharges were presented, showing oscillatory phenomena related to the blade pass frequency and the rotating frequency. The power–discharge and efficiency–discharge curves (both with fixed head and variable rotating speed) were plotted, presenting a good correspondence with the experimental curves previously found in the framework of a research project. This was true at least up to the discharge corresponding to the maximum power, after which the simulations yielded lower values than the experiments. The comparison error in power and efficiency remained below 6% for discharge lower than 97.8 L/s.
Instantaneous images of the streamlines near the blade that was about to exit the water showed eddy structures that increased in size with increasing discharge, resulting also in higher negative pressure (and torque) over the pressure side of the blade, reducing the absorbed power. In addition, short animations of the flow through the HPM were created with the numerical results for two distinct discharges, and a qualitative comparison with the experimental behaviour was performed, concluding that the simulation managed to reproduce the main features of the flow for increasing discharge. These features are the difficulty to expel the air inside the bucket of the HPM that was entering the water upstream, and the difficulty to drain the bucket that was getting out of the water downstream.
It is proposed as future work to carry out numerical simulations of the operation of other HPM models, which have been developed in order to increase the maximum power and efficiency. Likewise, the possibility of simulating the operation of other types of turbines is also proposed.