Transient three-dimensional CFD modelling of ceiling fans

Ceiling fans have been used for decades as a means of providing thermal comfort in tropical countries such as India. However, recent years have witnessed a signi ﬁ cant increase in the use of air conditioning as a means to achieve comfort, and therefore in the total energy consumption and related CO 2 emissions. Ceiling fans are still viable options to limit use of air conditioners or in combination with air conditioners without compromising on thermal comfort and still achieving energy savings. Ceiling fans generate non- uniform velocity pro ﬁ les, and therefore relatively non-uniform thermal environments, whose characteristics may be tough to analyse with simple modelling methods. This issue can be investigated using CFD. However, to date, there are few works on ceiling fans, CFD and thermal comfort. More accurate models are therefore required to predict their performance. The research presented in this paper aimed to develop and validate a three-dimensional transient implicit CFD model of a typical ceiling fan available in India by comparing simulation results obtained using different URANS turbulence models with measured data collected in controlled environment. The results highlight that this ceiling fan model is able to replicate the predominant characteristics of the air ﬂ ow generated by the fan such as the meandering plume and the local ﬁ ne free shear layers. The best results are achieved when the SST k- u turbulence model is used, with 83% of the simulated values being within the error bars of the respective measured value.


Introduction
Ceiling fans have been used for decades as a means of providing thermal comfort in tropical climates. In Indian residences, ceiling fans are as common as electric light bulbs, being present in almost every habitable space. They are part of most of Indian residences, and they are widely used in both old and more recent buildings [1,2]. In the event of growing economy and rising percentage of population which can afford purchase and operation of air conditioner for higher want of thermal comfort India has experienced rise in sales of air conditioners [3]. Cities such as Delhi, Mumbai and Kolkata, having Cooling degree days in range of 3000 and 3500, are replacing fans with air conditioners despite possibility of use of fan during certain part of year. It is important to note that most air conditioners have low-efficiency and use high-GWP refrigerants [4]. The electricity demand for space cooling comprises up to 60% of summer peak load in large cities such as Delhi [5]. Unless the use of energy-intensive air conditioning is limited only to periods of extremely hot weather, then overall Indian energy consumption and related CO 2 emissions will significantly increase, leading to severe implications for the global climate and also challenging the reliability of the Indian electricity grid.
Air conditioning usually provides uniform thermal environmental conditions, therefore designers can predict with confidence its performance using traditional thermal comfort models [6]. On the other hand, ceiling fans generate non-uniform velocity profiles, and therefore relatively non-uniform thermal environments. This does not imply a lower thermal comfort for the occupants, but could possibly lead to more thermally comfortable environments with lower energy cost due to air velocity, as research on alliesthesia suggests [7]. The positive effect of air movement on thermal comfort in warm and hot conditions has also been included in international standard such as the current version of ASHRAE 55 [8]: for operative temperature above 25.5 C, the air speed limits have been raised to 1.2 m/s with occupant control and 0.8 m/s without occupant control. However, accurate models of the ceiling fans are required to predict their ability to generate air velocity and their effect on occupant comfort using newer and more advanced thermal comfort models such as the IESD-Fiala model [9,10] coupled with a commercial CFD software [11]. Traditional thermal comfort models, namely the PMV-PPD model developed by Fanger [6] and the more recent adaptive approach [12,13], are indeed not suitable to investigate thermal comfort in non-uniform thermal environments. The former is applicable only to uniform steadystate conditions, while the adaptive model uses only the outdoor temperature as input parameter, and therefore it cannot be used to study the effect of a specific device such as a fan on thermal comfort.
The IESD-Fiala model is a model of human thermal physiology and comfort that predicts passive [9] and active [10] reactions of a human body in response to certain environmental conditions. It has been successfully coupled in real-time with a commercial CFD software [11], where real-time means that at each time step of a transient simulation there is an exchange of information between the two parts of the system. Thus, this coupled system can accommodate transient and asymmetrical environments [14], and can therefore be used to model the usage of ceiling fans, for instance identifying the best location for their installation. In the literature, there are other advanced models such as the model developed at UCB by Huizenga [15], but their capabilities are lower. Like the IESD-Fiala model, the UCB model is based on the multinode model developed by Stolwijk for aerospace applications [16,17], and it has been used together with CFD software [18e20]. However, in these studies there is only a manual coupling, with no real-time automated procedure.
To date, there are few existing reports on the use of CFD to model ceiling fans. Bassiouny et al. [21] implemented simple 2D models. Thus, the truly three-dimensional behaviour of air flow generated by a ceiling fan is not captured. Momoi et al. [22,23] developed too complex modelling approaches that are limited in their application because many measurements are needed due to the required input data. Adeeb et al. [24] focused on the effect of the different numbers of blades, but their work did not provide sufficient information to build a 3D model of a ceiling fan in CFD to be used for thermal comfort studies within the Fiala-IESD and CFD coupled system. To do so, the most important thing is accurate modelling of the environment around the occupants, but keeping the CFD model as simple as possible for two reasons: reducing the time and computational power required to achieve a converged solution, and avoiding potential sources of error due to the use of an unnecessary complex model. For instance, the use of a moving mesh used by Zhu et al. [25] to study the effect of the ceiling fans on air mixing and UR-UVGI disinfection efficacy [25] would not guarantee more accurate thermal comfort predictions, but would certainly increase the computational time, especially when transient and steady-state simulations are used.
Thus, the research presented in this paper aimed to develop and validate a three-dimensional transient CFD model of a typical ceiling fan predominantly used in India by comparing simulation results and measured data. This model combines accuracy with efficient computation, and can be used for accurate thermal comfort studies.
This paper is divided in to five parts: (1) Introduction (2) Methods, this has two sub sections one deals with experiment and second modelling (3) Results from experiment and modelling (4) Discussion (5) Summary, including key findings and limitation of work.

Methods
Detailed measurements of the air movement generated by a typical Indian ceiling fan have been collected in an environmental chamber in controlled environment, and the same experimental set-up has then been modelled using a commercial CFD program, ANSYS CFX [26]. In this model, the fan is modelled as a momentum source that is specified by radial components and applied to a thin cylindrical sub-domain of the CFD model which has the same diameter as the fan used in chamber experiment. Measured values and computer-generated predictions have been compared analysed, and the reasons for any deviation discussed.

Experimental set-up
Environmental chambers have been extensively used to collect data for validating CFD models [27]. Within an environmental chamber, most of the variables can be controlled, and the state of the uncontrolled variables ought to be accurately determined. Thus, the number of required assumptions due to the lack of measurements or better information, and therefore the number of potential sources of uncertainties, are minimised.
For this research, an environmental chamber located at CEPT University, Ahmedabad, in India was used to generate validation data (see Fig. 1). Chamber is located in basement with only one side exposed to outdoor environment. Internal (thickness 200 mm) and external (thickness 350 mm) walls have U-value of 0.29 and 0.28 W/m 2 K, respectively. Roof, false ceiling, and floor have U-value of 0.29, 0.55 and 2.80 W/m 2 K, respectively. External window facing West direction has U-value of 1.79 W/m 2 K. At no point in time direct solar radiation hit this window as it is well protected outside. The mechanical ventilation system comprises four supply grilles and two return grilles, which are located in the ceiling. The chamber ventilation system was turned off during any experiment, and the diffusers were sealed during both the second and third repetition of the measurements. This did not produce any significant difference in the measured values, but allowed to more accurately set the boundary conditions in CFD. Moreover, since the objective was to obtain data of velocity profiles under uniform and stable environmental conditions, the experiment was conducted once the chamber stabilized at constant air and surface temperatures. The stability of chamber was determined based on less than 0.1 C change in air and surface temperature for more than 12 h. A typical 3-blade 1200 mm sweep Indian ceiling fan [28] with a 4step regulator was installed on the ceiling of the chamber. The diameter of central part is 190 mm and the length of the blade is 500 mm. Other than measuring equipment, no other objects were present in the room.
Air speed measurements were recorded in three horizontal planes in the chamber: 0.1 m, 0.7 m and 1.3 m above the floor. In each plane, 12 measurements were recorded. These were located (see Fig. 2) below the centre of the fan ("centre"), below the perimeter of the fan ("north, east, south, west"), and on a radius at increasing distance from the centre of the fan. For instance, "r 800" means 800 mm away from the fan centre. Thus, in total, measurements were taken at 36 points (see Table 1).
Measurements were recorded simultaneously at these three heights in each of the 12 horizontal locations using three air speed probes (see Table 2 and Fig. 1). After the recording was completed in one location, the measurement equipment was moved to the next spot, but the new recording period always started a few minutes after having moved the equipment. The logging duration per location was 300 s and the logging period 1 s. It is important to point out that both types of probe used for measuring air speed are omnidirectional, which means that only air speed is recorded, rather than the three components of air velocity separately. Their measuring range is 0e10 m/s, in À20 to þ70 C range. Instantaneous measurements of room air temperature and relative humidity, room surface temperatures, and fan rotational speed have also been taken (see Table 3). In this study, the highest available fan rotational speed setting has been chosen based on an on-going field study in India and in the UK on air movement in domestic buildings [29].
A complete set of measurements was taken three times to ensure the quality of the data and repeatability of the experiment.

Modelling approach and assumptions
The identical configuration used during the experiments was then recreated within the CFD program. In this study, the chosen software is ANSYS CFX [26] primarily because the coupling between the IESD-Fiala model and CFD was completed using ANSYS CFX due to its customization features which facilitate the connection with other software [11]. Thus, this facilitates the use of this ceiling fan modelling approach in thermal comfort applications. However, the modelling approach presented in this paper could be     implemented in most CFD programs. The geometry (see Fig. 3) was created in ICEM CFD [30], a general purpose geometry and mesh generator for CFD. Air diffusers, windows and door were not included since they were all closed during the experimental work, and because only isothermal simulations were conducted to reduce the required computational power. This has been done because the surface temperatures and the air temperature were similar, being 31.8 C and 31.9 C, respectively (see Table 3). Thus, the magnitude of any buoyancydriven air flow would have been negligible compared with the air speed generated by the fan.
The ceiling fan has been modelled as a momentum source. Modelling the actual blades would require very detailed information about their geometry, and would lead to a much higher number of mesh elements and to the use of a moving mesh. Both these features would significantly increase the demand for computational power, and the possible sources of uncertainty, without guaranteeing better results, but limiting the usability and applicability of the model. Thus, the fan has been modelled as a ring with the same diameter, 120 cm, and distance from the ceiling, 30 cm, as the actual fan, and with a central cylindrical solid element, since in a real ceiling fan no air emanates from the centre [31]. The momentum source has been applied to this ring (see Figs. 3 and 4, in which the ring is highlighted in yellow).
In this study, an unstructured mesh was used because it is more flexible and it can be used with any complex shape such as a human body, easing the wider applicability of the proposed modelling approach. Similarly to previous studies [14], both the surface and the volume mesh were initially generated in ICEM CFD using the Octree algorithm, then the volume mesh was deleted, and finally regenerated using the Delaunay algorithm (see Fig. 5). This procedure ensures the robustness of the mesh and a smoother transition from smaller elements to larger ones. Ten prism layers were added adjacent to the walls to accurately model the boundary layer near surfaces.
Transient simulations have been performed to better model the real behaviour of the ceiling fan. Moreover, considering this ceiling fan model as a component that can be used with advanced transient thermal comfort models, running transient simulations from the very beginning makes its applicability easier and more reliable. A second order backward Euler scheme, and high resolution advection scheme and turbulence numerics have been used. The double precision option was also used to enhance accuracy and robustness of the results. Convergence criteria have been set equal to 1e-05 for the RMS residuals and 0.01 for the conservation target. Since there are no inlets and outlets in this model, the conservation target does not have any influence. Furthermore, the sub-domain used to model the fan simply acts as a momentum source, but cannot generate any mass imbalance as there are no physical barriers (real surfaces) between this sub-domain and the remaining part of the room, and there is no mass generation or dissipation within this sub-domain. Moreover, an adaptive time step as a function of RMS Courant number was chosen, with the limit for the RMS Courant number set equal to 1. Since it is an implicit code, CFX does not require the Courant number to be small for stability, but this still leads to more accurate results. The initial time step was 0.1s, with the maximum and minimum values set equal to 1s and 0.01s, respectively.
The momentum source that simulates the actual fan has been applied to the subdomain using cylindrical components: axial component 55 kgm À2 s À2 , radial component 0 kgm À2 s À2 and theta component 8 kgm À2 s À2 . The axial component pushes air downwards while the theta component generates rotational movement. The sign of each component depends on the orientation of the defined local system of coordinates (see Fig. 4), while the absolute figures have been defined with an iterative process by comparing simulation results with measured values and by comparing the qualitative features of the flow field with qualitative previous studies. A study by Jain [31] provided with very useful qualitative information about the flow field generated by a ceiling fan. Using smoke from thick incense sticks, the flow field created by the ceiling fan was visualised, identifying the main regions of the flow and its key behaviours such as the swirling movement.
Due to the intrinsic turbulent nature of the air flow generated by the fan, the correct choice of the turbulence model is fundamental. In this study, four of the most widely used Unsteady Reynolds Averaged Navier-Stokes (URANS) eddy-viscosity turbulence models have been fully tested: the SST (Shear Stress Transport) k-u  [32e36], the RNG (Re-Normalisation Group) k-ε [37], the standard k-ε [38] and the standard k-u [39e42]. Two Reynolds-stress models have also been considered, namely the SSG (Speziale-Sarkar-Gatski) [43] and the BSL (Menter Baseline Model) [44], for their potential higher accuracy for simulating swirling flows and boundary layers [45].
Before running the main simulations, a mesh sensitivity analysis has been completed, with the purpose of estimating the discretization error and calculating the numerical uncertainty in the fine-grid solution, and thus identifying the most suitable mesh for the main simulations. To do so, three meshes of varying density have been used (see number of elements n i in Table 4), a representing dimension h i to be calculated, and a significant simulated value 4 i has to be used to quantify this uncertainty [46]. In this research, the air speed at a point below the centre of the fan at 1.5 m above the floor has been chosen. The mesh chosen for the main simulations comprises 1,996,278 elements and a numerical uncertainty equal to 15.80%.

Model validation -criteria for agreement
Measured and simulated values were compared in 36 points (see the yellow marks in Fig. 3) and considered to be in agreement when the respective error bars overlapped. For the simulated values, the upper and lower limits of the error bars are the mean over the simulated period plus and minus the discretization error, respectively. For the measurements, since the experiment has been repeated three times, the upper limit of the error bars is the highest of the three measurements plus the measurement error, while the lower limit of the error bars is the lowest of the three measurements minus the instrument error.
Statistics such as root mean square error (RMSE) and the mean absolute error (MAE) have not been employed in this research for two key reasons. Firstly, using RMSE and MAE with n ¼ 36 might be misleading as they would spread the error across all points. However, in this study, it is more important to evaluate the accuracy of the model in the different regions (centre, perimeter, along a radius), separately. Secondly, all statistics are less useful when there are only a limited number of error samples [47]. Thus, in this research, presenting the values of the errors themselves (as error bars) is more appropriate.

Results
In this section, qualitative and quantitative simulation results are presented. The former are compared with previous qualitative research, while the latter are compared with the measurements taken in this study.

Qualitative analysis of the air flow generated by the ceiling fan
Previous research [31] investigated the major flow regions observed in a room with an operating ceiling fan, identifying eight regions (Fig. 6). The comparison between previous research and the developed CFD model is summarised in Table 5. Region one is the area below the fan, and, in good agreement with previous research, in the CFD model presented in this paper air speed reaches the highest values in this region (Fig. 7). The diameter of downward flow immediately below the fan is smaller than the diameter of the fan, the flow then starts to diverge, and there is a significant swirling component (see Fig. 8). In the qualitative study [31], the half cone angle is about 10 , while in the CFD results this varies depending on which time-step is analysed. This is due to the fact that in this region the flow is highly turbulent, and therefore the angle of the meandering plume and the characteristic of the local fine free shear layers vary over time (see Fig. 9).  Similarly to previous research [31], in region two, the air speed near walls and ceiling is very low, air is moving upwards near the walls, and as soon as it is again in proximity of the fan, in region three, its speed increases and it starts to redevelop a swirling component. Moreover, the CFD model accurately predicts the small region below the ceiling fan where air is not driven downwards due to the blockage caused by the motor of the fan. In agreement with the qualitative study [31], the wide region (number four) between the surfaces of the room and region one is characterised by very low air speed and negligible effectiveness of the fan. Thus, the CFD model is able to accurately replicate all the occupied regions of the room.
The major differences between the CFD results and previous qualitative studies are located in the two small regions near the ends of the blades, where the local air recirculation is underestimated by the CFD model. This is due to the fact that the actual blades are not modelled, but it is not a significant limitation of the model in this case since the aim is to model the air movement generated by the ceiling fan in the room with particular interest in the occupied zone.

Quantitative validation of the CFD model
In this study, four turbulence models have been fully tested and the CFD results significantly vary depending on the chosen model (see Table 6).
Taking into account the uncertainties in measurement and the discretization error in CFD, measured and simulated values are in excellent agreement when the SST k-u was used, with 83% of the simulated values being within the error bars of the respective measured value. There is an excellent agreement in the three points below the centre of the fan (see Fig. 10, three "centre" points) and in the 21 points located on a radius at increasing distance (see Fig. 10, points from "r200" rightwards). Only in six perimeter points (see Fig. 14), namely "Est 700" and "Est 1300", "North 700" and "North 1300", and "West 700" and "West 1300", the respective error bars do not overlap. In three of them, namely "North 700" and "North   1300", and "West 700", the difference between measured and simulated values is wide, while it is significantly smaller in the others. This is likely to be due to the fact that these six points are in the most turbulent and critical region of the flow, where air speed is characterised by rapid spatial and temporal variations (see Fig. 9). The other three turbulence models did not reach the same high level of agreement with the measured values (see Table 6). In the three points below the centre of the fan, the RNG k-ε (see Fig. 11) and the k-u (see Fig. 12) turbulence models are as good as the SST ku, while the k-ε fails to predict the air speed at 0.1 m above the floor, being 0.1 m/s the difference between the error bars (see Fig. 13). In the 12 perimeter points, 50% or less of the simulated values are within the error bars of the respective measured value (see Table 6, and Figs. 15e17). On the radial points, k-u and k-ε models have limited capability of predicting the correct air speed, the percentage of agreement with the measurements being below 50%, and there is no clear pattern that can explain why, at certain points, the prediction is correct and in others it is not. When the RNG k-ε model is used, the agreement is excellent between r200 and r800 at any given height (see Fig. 11), while it weakens farther away from the fan, where air speed is lower.

The importance of the choice of the turbulence model
The air flow generated by a ceiling fan is highly turbulent. As shown in the previous section, it is characterised by elevated air speed variations, and therefore by significant Reynolds number (Re) variations. For this reason, choosing the most appropriate turbulence model is essential in order to obtain accurate results.
The SST k-u turbulence model produced the most accurate and realistic results, being superior to the other three eddy-viscosity turbulence model considering both qualitative and quantitative results. This is in agreement with findings from previous research which used the IESD-Fiala model to investigate the effect of air movement generated by desktop fans on human thermal comfort [14]. This can be explained by analysing the nature of the four eddyviscosity turbulence models in relation to the application presented in this paper.
Turbulence occurs when the inertia forces in the fluid become significant compared to the viscous forces. The Re is defined as the ratio between inertia and viscous forces, and therefore the higher the Re, the more turbulent the fluid flow becomes. Navier-Stokes equations could be used to describe any fluid flow, regardless of its turbulence level, but the required computational power to fully solve a given problem significantly exceeds the power that is currently available. For this reason, several turbulence models have been developed which simplify the original unsteady Navier-Stokes equations by the introduction of time-averaged quantities and a turbulent viscosity to produce the Reynolds Averaged Navier-Stokes (RANS) equations. In these time-averaged equations, the fluctuating quantities, called Reynolds turbulent stresses, are taken into account by adding some extra terms in order to achieve closure. Additional equations are then required to balance the added unknowns. The equations used to close the system and their numerical coefficients define the type of turbulence model [48].
The four turbulence models tested in this research are twoequation eddy-viscosity models, which means that the Reynolds stresses are assumed to be proportional to mean velocity gradients. In the k-ε models, the two additional transport equations are used to describe the kinetic energy k and the rate of dissipation of k per unit mass ε, respectively: The equations contain five coefficients, whose value in the standard k-ε model are constant [38]:  C 1ε ¼ 1.44, C 2ε ¼ 1.92. In the RNG k-ε model [37], the C 1ε is not fixed, and it represent a strain-dependent correction term introduced to improve the performance at low Re. In the k-u model developed by Wilcox [39e42], the turbulence frequency u ¼ ε/k is used as the second variable, and the two additional equations are: The models constants are: s k ¼ 2.00, s u ¼ 2.00, g 1 ¼ 0.553, b 1 ¼ 0.075, b * ¼ 0.09. Subsequently, an improved k-u model was suggested, namely the SST k-u model [32e35], which is a combination of the standard keε model used in the fully turbulent region Table 6 Comparison between measured and simulated air speed values.

Location
Number of points Agreement measurements -simulations SST k-u RNG k-ε k-u k-ε There is an extra source term on the right hand side of the equation, and the numerical coefficients are [36]: s k ¼ 1.00, s u,1 ¼ 2.00, s u,2 ¼ 1.17, g 2 ¼ 0.44, b2 ¼ 0.083, b* ¼ 0.09. Moreover, blending functions are used to achieve a smooth transition between the two models, namely k-ε and keu.
Considering the three-dimensional transient ceiling fan model proposed in this paper, it is now easier to understand why the SST k-u model produced the best results followed by the RNG k-ε model, while the other two turbulence models generated less accurate results. By combining the strengths of k-ε and k-u models, the SST k-u can deal with higher and lower Re, and it is able to accurately model the boundary layers and the flow separation under adverse pressure gradient conditions thanks to the extra cross-diffusion term on the right hand side of equation (5). The CFD results indeed demonstrate that this turbulence model is more accurate in all considered locations, namely below the centre of the fan, on the perimeter, and on a radius at growing distance for any given height and therefore air speed. On the other hand, the RNG kε is as good as the SST k-u in the central and perimeter points, where the flow is more turbulent and air speed is higher, while it  shows its main limitations by failing to predict the air speed farther away from the fan.
In view of the fact that in none of these four turbulence models the agreement between measured and simulated values exceeded 50% in the 12 perimeter points, two more advanced turbulence models have been considered, namely the BSL [44] and SSG [43] Reynolds stress models. Theoretically, these models are more suitable for complex flows, such as the swirling flow generated by a ceiling fan. Practically, their application proved to be fairly difficult. Without changing any other input data or element of the model, the simulation immediately stopped due to fatal overflow in linear solver using both models. Two relatively easy-to-test changes were then tried: reducing the time step by setting a limit for the maximum, rather than the RMS, Courant number equal to 1, and using the best available results, namely those calculated with the SST k-u model, as initial conditions. Even combining the two things, the simulation stopped due to the same overflow error after some iterations. Also a finer mesh was used, but unsuccessfully. Both using a finer mesh and reducing the time step would also have the disadvantage of exponentially increasing the time required to reach a converged solution. Thus, evidence suggests that more advanced turbulence models such as Reynolds stress models and also Large Eddy Simulations (LES) require a complete explicit model of the fan, the use of a moving mesh, and therefore higher computational power. However, this would significantly limit the applicability of the model and increase the potential sources of uncertainties.

Required computational power
In this study, simulations have been run on the High    Performance Computer System at Loughborough University, a 2460-core 64-bit Intel Xeon cluster. Two nodes and 20 cores per node, therefore 40 cores in total, have been used in these simulations in order to make efficient use of the cluster architecture, and reduce the computational time. In the pre-processing, the meshes have been generated using a work station equipped with an Intel Xeon E5520 CPU and 24 GB of RAM. All the other pre-and postprocessing activities have been completed using a laptop with an i5-3320M CPU and 8 GB of RAM.
Due to extra terms in the two additional k and ε, or u, equations, the CPU time required to achieve a converged solution using the SST k-u and RNG k-ε models is twice the time required when the ku model is chosen, and three times higher than the time required when the standard k-ε model is selected (see Table 7). In detail, the SST k-u and RNG k-ε are both able to predict the meandering behaviour of the plume over time (see Fig. 9), which means that there are relevant differences between each time step and the following one, and therefore more iterations per time step are required to reach convergence. On the other hand, when the other two simpler models (standard k-u and standard k-ε) are used, the differences between each time step and the following one become negligible after the initial time steps, and therefore only a few iterations per time step are required thereafter.
Although there is no direct linear relationship between the number of cores and the CPU time due to the time required to split, and then recombine, the results which increases with the number of cores, these total CPU times (see Table 7) could be reduced if more cores were available. Considering the CPU time and the accuracy of the results, the SST k-u model is still the best choice.

Usability of the developed model
Compared with the models previously developed [21e24], the model presented here is applicable to a wider range of fluid flow problems due to the small number of input parameters required, the reasonably low CPU time required, and the use of an unstructured mesh, which can accommodate complex geometries. This implicit model can therefore be used whenever a given piece of research requires a focus on the flow field generated by a ceiling fan, not on the actual design of the fan.
When assessing the effect of air movement on human thermal comfort using advanced thermal comfort models such as the IESD-Fiala model [9,10], this CFD model is able to effectively predict the air flow generated by the fan at any distance from the fan and therefore it reliably estimates the air flow on a person. The limited agreement between measurements and simulated values at the perimeter of the fan has little implication on the applicability of this model in thermal comfort studies, since this perimeter region is less than 10 cm wide, while any human body, regardless of age, gender, height, and weight, is significantly bigger. Moreover, it is almost always possible for a person to then move a short distance to increase or decrease the air movement on their body. Similarly, if the spread of pollutants in a room is to be investigated, then any error in the perimeter region does not affect the overall distribution of the contaminants in the space, but only their concentration and movement in that narrow perimeter region.

Conclusions
This paper presents research findings on a transient threedimensional CFD implicit model of a ceiling fan. The research question was whether a simple implicit model, that combines accuracy with efficient computation, can be used for accurate thermal comfort studies. In order to validate the simulation results and therefore to fully address the research question, a comparison with experimental data has been presented.
The results confirm that the model developed is able to accurately, qualitatively and quantitatively, predict the air flow generated by a typical Indian ceiling fan in a room. When using the SST ku turbulence model, 83% of the simulated values are within the error bars of the respective measured value, and both the swirling and downward air movements are effectively modelled.
Due to the small number of input parameters required, the relatively low CPU time required, and the use of an unstructured mesh, this model can be effectively used in any study in which it is important to accurately model the air movement generated by the fan, such as thermal comfort or air quality and contaminant distribution research. The choice of the most appropriate turbulence model is essential, and the best results have been achieved using the SST k-u turbulence model, which is available in most of the CFD packages.
Due to the use of a simplified implicit model and RANS turbulence models, the major differences between measurements and simulated values occur in the narrow region below the perimeter of the fan, where there are rapid temporal and spatial variations in the flow field. Further work is required to investigate the possibility of using more advanced Reynolds stress turbulence models and LES, balancing the accuracy of the results and the computational effort required to achieve a reliable converged solution.
More advanced measurement techniques such as particle image velocimetry could be used in the future to provide a better understanding of the flow field generated by the ceiling fan and better validation data, including data for lower fan rotational speeds. This would also ease the use of more advanced turbulence models.