Sensitivity study of diffuser angle and brim height parameters for the design of 3 kW Diffuser Augmented Wind Turbine

Abstract The Diffuser Augmented Wind Turbine (DAWT) is an innovative mean to increase the power harvested by wind turbine. By encompassing the rotor with a diffusershaped duct it is possible to increase the flow speed through the turbine by about 40-50%. The study presents the development of a numerical model and its validation by the experiments performed in the wind tunnel of the Institute of Turbomachinery, TUL. Then, the numerical model is used for the geometry sensitivity study to optimize the shape of a diffuser. The paper presents that the DAWT technology has the potential to even double the power outcome of wind turbine when compared to a bare rotor version.


Introduction
An increasing demand for reliable green energy source leads to a vast development in wind power sector. However, optimisation of rotor geometry may only be done within the so-called Betz limit, stating that no more than about 60% of wind's kinetic energy may be harvested and converted into a mechanical power on the shaft. In practice, the conversion rate is on average 30% for majority of the Horizontal Axis Wind Turbines (HAWTs). One possible solution to increase energy production rate over this limit is to force more air to move through the working section of turbine. This can be achieved by equipping the rotor with The Shrouded Wind Turbine concept may be traced back to as early as 1970s. Gilbert and Foreman [1] mainly concentrated on a long divergent channel structure with a turbine placed inside, while Igra [2] proved that a compact shroud may be equally interesting. However, the idea has not remained commercially exploited until the results of numerous studies performed at Japanese Kyushu University were published (see for example [3,4]). The research conducted at Kyushu University proposed a more compact form of a shroud, called "wind lens", in which the outlet of a di user is equipped with a brim. The experiments showed numerous advantages of this solution: signi cant rise in the power output, increase of safety by housing the rotor or decrease of acoustic noise [3,5].
The general operation principle of a shrouded wind turbine may be explained with uid mechanics principles. The brim is an obstacle for the oncoming ow that creates a low-pressure zone downstream. The low-pressure zone draws more air into the channel to equalize the pressure gradient. By increasing the mass ow through the di user, a signi cant ow acceleration is observed at the inlet of a divergent duct where the turbine is placed [6][7][8]. This theory becomes insu cient to explain the ow acceleration in the di user outlet region that is observed for di user angles of about 20°and higher, a phenomenon that the "wind lens" compact designs are based on.
In order to broaden knowledge of ow nature around brimmed di users and, further, a Di user-Augmented Wind Turbine (DAWT), a series of numerical analysis were conducted. Based on an experimentally validated numerical model, a sensitivity study of two parameters describing the geometry of an isolated di user was made in order to identify a design which can further increase the ow velocity through the channel. Results of this study are presented in the following document.  mined via a model independence study. To limit the size of the computational task the domain encompassed an axisymmetric 1°section of a ow eld, where rotational periodicity boundary condition around the X axis was imposed. The di using channel was placed at the distance equal to three diameters from the inlet cross-section. A combination of boundary conditions was used to mimic the ow in the Institute of Turbomachinery (IMP) wind tunnel. Hence, the free slip wall condition (no through ow allowed) was used to adhere to an open wind tunnel test section and the outlet cross-section imposing a perpendicular out ow, where an ambient pressure of 101325 Pa was used. The ow was treated as isothermal, steadystate type with air treated as an ideal gas. A low (1%) turbulence intensity was set at the inlet, which corresponds to a value measured in IMP wind tunnel (see for example [9]). The turbulence model independence test including the SST and k − ε closure were performed and will be presented in Chapter 3. Care was taken to assure that nearwall mesh elements provide y+ values around 1 in order to use the ω-based equation to compute boundary layer ows. For places where this was not possible, a velocity pro le from at plate experiment was imposed.

Numerical model
The key geometrical parameters of the modelled diffuser are grouped in Table 1. The inlet diameter-based Reynolds number was calculated to be 6.61· and corresponds to a small ducted 3 kW turbine operating at wind speed of 4 m/s (annual average wind speed at 2/3 of territory of Poland 10 m above ground, [10]). In the wind tunnel measurement, the model in a smaller scale was tested to limit the blockage coe cient to 0.05.
The proposed mesh was envisaged so as to favour the regions of interest: di user boundary layer and inside region and generally the region downstream the brim-di user structure. The mesh was swept face-to-face around the X axis. Meshing statistic parameters are listed in Table 2, while the general overview of the mesh is visible in Figure 2.

Numerical model validation . Experimental stand
Experimental study has been carried out in the subsonic wind tunnel at the Institute of Turbomachinery at the Lodz University of Technology. The investigated di user model was placed in the free stream inside the test section (downstream the circular wind tunnel outlet nozzle). To limit the blockage e ect of the model, an open test section was used with the model size frontal area equal to 5% of the contraction nozzle area supplying the air into the test area.
Particle Image Velocimetry (PIV) and pneumatic probe measurements have been made.
Unauthenticated Download Date | 3/6/17 6:34 AM . °R eynolds number based on D . E+ . E+  PIV measurement plane was aligned with the ow direction. It was positioned vertically and passed through the axis of a channel, perpendicular-wise to the brim of diffuser. Two cameras in 2D measurement mode were used in order to obtain large velocity ow eld downstream the DAWT (see Figure 3).

. Pneumatic measurements
To supplement the PIV tests, pneumatic measurements have been performed. Pitot-static pressure probe connected to a pressure di erence transducer was used. By measuring the pressure di erence between output signals of probes (total and static pressure), dynamic pressure was obtained allowing for the calculation of the ow velocity. Measurement system was equipped with an automatic data acquisition system in order to perform multiple measurement for one location of the probe. Information about the temperature have been gathered with a thermocouple, while an ambient pressure was measured with a mercurybased barometer.

. Comparison of results with the experimental data
Velocity distribution at the locations, where pressure measurements have been taken, are presented in Figures 4 and  5. A comparison of results obtained by means of numerical simulations with two di erent turbulence models as well as experimental data from PIV and pneumatic probe measurements are shown. No data was recorded by PIV in the region upstream the di user thus only pneumatic measurements and CFD results are compared for that zone in  surements con rm the observed velocity trends. The simulation results are indi erent despite that two varying turbulence models were used and clearly show an over 40% of velocity rise at the di user inlet (x/D=0). Velocity gradually returns to the free stream value at the distance of two diameters downstream the di user. The simulation results are about 6% lower than the experimental ones. This may be attributed to the fact that the reference value of U was measured directly at the outlet of the wind tunnel nozzle, at a location laden with ow turbulence. The tunnel is of blow-down type and, at the moment of the experiment, was equipped with a nozzle of a crude design which could additionally intensify local ow unsteadiness. Tests of a new nozzle, based on Witoszynski formula, are planned shortly, and this phenomena should not be visible in the future studies. Because the di erence observed between experimental and numerical results is quite consistent in the ow domain presented in Figure 4, it could have been reduced by using an appropriate correction. However, it was not judged as crucial for the numerical model used in the sensitivity study since the character of the measured ow is nearly exactly mimicked by the simulation. This proves the representative character of the model.
A very good quantitative agreement between simulation and the experiment was found downstream the diffuser, where some of the measurements were made inside the wakes. The inner dashed lines mark the di user outlet diameter, while the outer dashed lines locate the ends of the brim. Therefore, the numerical models are validated for ows laden with aerodynamic wakes. For further analysis, the SST turbulence model was used. Figure 6 compares the distribution of ow velocity in the domain, as seen in the PIV experiment and in the simulation. The two images present very good qualitative correlation of both cases con- cerning the size and location of the observed ow phenomena.

Numerical model for DAWT simulation
The described numerical model was used in a sensitivity study process of a di user geometry for 3 kW Di user-Augmented Wind Turbine with inlet diameter of D = 2.5 m. To simulate the rotor's presence an actuator disc was placed at the distance of 0.05 m from the di user inlet in place, where the maximum velocity occurs (refer to Figure 4). The disc was allowed to rotate at the rotational speed of 150 rpm, while a pressure drop of 7 Pa was imposed across its boundaries to simulate the rotor load. Figure 7 presents the other boundary conditions used in the study: inlet velocity was equal to 6 m/s with inlet turbulence Tu = 5%. In total 48 geometries were examined, covering 3 di erent brim heights (0.1D, 0.3D and 0.5D) and 16 di user angles (from 0°to 30°with interval 2°).
In order to determine the imposed pressure drop across the rotor plane, the experimental results as presented by Abe and Ohya [11] were used. Pressure coecient cp di erence due to the load exerted on the rotor by  the uid was determined by using the plot data available in Figure 8. Abe and Ohya [11] reported that the cp drops from about -0.78 to -1.22 producing ∆cp = . when loading coe cient C t = . . The following de nition of the loading coe cient was proposed by [11]: which di ers from standard C t de nition, and where p1 is the pressure immediately upstream the rotor plane, p and U denote pressure and velocity immediately downstream the rotor. The aforementioned values of cp di erence were next employed in the standard formula de ning the pressure coe cient: where U describes free stream velocity of 5 m/s at which Abe and Ohya [11] performed tests in the wind tunnel, air density was assumed as in own CFD simulations (ρ = . kg/m ). The obtained numerical result is about ∆p = Pa. Next, the ∆p value was imposed across the actuator disc model in own CFD simulations of the small DAWT (D = 2.5 m). The results of this study are visible in Figure 8 as well and correspond well to the reference data, which concerns the pressure drop in rotor plane. Therefore, for the further analysis presented herein the value of ∆p = Pa was assumed.
The di erence in quantitative relationship between the implemented model in own simulation and the experimental values is due to the existence of a sharp entry edge at the di user inlet. In numerical simulation this leads to the creation of sudden pressure drop, extending from the di user inlet to about x/D = 0.4, as visible also in Figure 8. At the same time, the experimentally investigated di user in [11] is not explicitly described to possess either sharp inlet edge or aerodynamically optimal inlet. The implication that this particular geometrical feature could have on the sensitivity results presented in the following sections is minimal as the same numerical e ect occurs in all simulations. Figure 9 shows typical features of the considered ow. The velocity rise of about 50% can be observed at the turbine inlet and potentially even more at about 0.2D downstream the di user inlet.

Sensitivity study of DAWT's di user angle and brim height
The region downstream the brim is a low-pressure zone, and the ow behaviour in this region is di erent with varying geometry. Low brim and low di user angle result in creation of only small wake. Augmenting these two geometric parameters results generally in the creation of two vortices -one, nearer to the stream exiting the di user, directed counter clockwise, and another oneabove, turning clockwise. Very high di user angles may result in the creation of a boundary layer separation which causes energy losses. In case of the considered ows, for angles above 26°, the boundary-layer vortices connected Unauthenticated Download Date | 3/6/17 6:34 AM with the vortex behind the brim creating a massive separation zones and ow instabilities. Figure 10 presents the results of the sensitivity study where the in uence of the di user angle and the brim height on the velocity at the rotor inlet can be estimated. The velocities were area-averaged and then divided by the free stream value.
Generally, the test results show that the ow velocity gain, regardless of the brim height, is as high as even 1.6 for di user angles of about 6°. Another observation is that smaller di user angles favour higher brims. On the other hand, the angles from the range 18°-26°show equally satisfactory ow velocity increase. However, in these cases, the areas in which the ow accelerates are usually shifted towards the di user outlet where, as described earlier, larger ow separation regions form due to increasing di user angles. These structures may potentially amplify the vibrations of the channel and the turbine itself, presenting a challenge from a structural, control and safety points of view. The brim of reduced height is generally preferred in these cases. Despite the unsteady character of the ow, these geometries may be of signi cant interest, as a ow velocity rise even of magnitude 2 was observed.
The proposed rotor modelling technique assumes a constant pressure drop across the virtual rotor plane. This would not be the case in reality, especially when the geometrical changes introduced lead to the increase of the streamwise velocity at the rotor inlet (see Figure 10). Namely, the pressure drop is expected to rise according to the rise of dynamic pressure upstream the rotor. However, the DAWT geometry models in the sensitivity study were not identical as in Abe and Ohya [11] to directly impose pressure drop characteristics as based on experiment. At the time own CFD study was prepared no experiment existed to derive representative pressure drop in own model. Therefore, this point leaves place for a potential improvement in ow modelling.
For further analysis, the dimensionless streamwise velocity U/U plots for angles 2α = 6°and 22°are presented in Figure 11 and Figure 12. In case of the 6°, the distribution of the axial velocity reveals that the maximum velocity in rotor plane occurs for the brim with mediocre height (h = 0.3D). Additionally, the velocity ow eld downstream the DAWT is in uenced by the size of the brim as the velocity plot shows the return of the exit velocity to the free stream value only in the case of the smallest brim. At a higher di user angle, 2α = 22°, the DAWT with the highest brim leads to a slightly higher U/U ratio at rotor plane as in the case of the brim with h = 0.1D. At these di user angles, ow instabilities complicate interpretation of the numerical results due to its unsteady character. Nevertheless, some observations agree with the literature data. For   example [11] observed higher turbine power values for diffuser angles 2α = 30°. However, computations were made at higher loading coe cient.
Furthermore, what is likewise interesting, in both cases the maximum ow acceleration is observed at locations inside the di user rather than directly at the inlet (x/D = 0). As the di user angles rise, the in uence of the di user leading edge becomes lower with the boundary layer separations growing larger. Thus, the velocity peak zone may be shifted further downstream the di using channel, as seen for example in Figure 12. This may favour a second contra rotating turbine rotor to harvest the remaining energy and increase overall power production of the plant. This investigation is a subject of another scienti c study conducted at the Institute of Turbomachinery, at the Lodz University of Technology.