Ceiling fans are used to get thermal comfort, especially in tropical countries. With the increment of the usage of air conditioners, the emission of CO2 is increased. But ceiling fans are a limited solution, that saves much energy compared to air conditioners. Ceiling fans generate a non-uniform velocity profile, so that, there is a non-uniform thermal environment. That non-uniform environment does not imply lower thermal comfort, that will give enough thermal comfort with low energy cost by air velocity. Hence, there will be difficulties of analysing with simple modelling techniques in that environment. So, to predict the performance of the ceiling fan required more accurate models. The accurate model of a ceiling fan will generate complex geometry that makes difficulties for the simulation process and requires higher computational power. Because of that, there are several methods used to predict the performance of the ceiling fan using mathematical techniques but that will give an estimated value of properties in the surrounding.

1. Project Report
Transient three-dimensional CFD modelling
of ceiling fan

2. 1
1 Problem definition and objectives
Ceiling fans are used to get thermal comfort, especially in tropical countries. With the increment of
the usage of air conditioners, the emission of CO2 is increased. But ceiling fans are a limited solution,
that saves much energy compared to air conditioners. Ceiling fans generate a non-uniform velocity
profile, so that, there is a non-uniform thermal environment. That non-uniform environment does not
imply lower thermal comfort, that will give enough thermal comfort with low energy cost by air velocity.
Hence, there will be difficulties of analysing with simple modelling techniques in that environment. So,
to predict the performance of the ceiling fan required more accurate models.
The accurate model of a ceiling fan will generate complex geometry that makes difficulties for the
simulation process and requires higher computational power. Because of that, there are several methods
used to predict the performance of the ceiling fan using mathematical techniques but that will give an
estimated value of properties in the surrounding.
*
This project is inherited from a research paper that used momentum sources to model ceiling fan
geometry. In this project use fan boundary condition in ANSYS Fluent, for the modelling phase.
Main objectives of the project are as follows.
1. Develop 3D transient implicit CFD model of a typical ceiling fan using different RANS
models.
2. Get the velocity profile in each model to compare with each other
3. Compare results in the CFD model with the experimental results and select suitable RANS
model to model a ceiling fan
*
Babich, F., Cook, M., Loveday, D., Rawal, R. and Shukla, Y. (2017). Transient three-dimensional CFD
modelling of ceiling fans. Building and Environment, 123, pp.37-49.

3. 2
2 Problem domain and physical boundary
The environmental chamber that was used for the experimental setup in the literature was modelled
in the ANSYS Design Modeler. This domain is a closed one because there is no inlet or outlet. So that
all boundaries are stationary walls. The ceiling fan in the experiment was modelled using a circle, that
was a surface in the 3D domain. Since the fan is represented by a circle and the rotation is modelled
using fan boundary condition in ANSYS solver, so that there are no moving bodies in the domain.
Dimensions are in mm
Figure 2.1: Problem domain - top view (left) and front view (right)
x
x
x
x
north
west
south
east
x
x
x
x
x
x
r2000
r1200
r1700
r800
r200
Fan boundary condition
Profile specification of pressure jump – 3.3 Pa
Swirl velocity specification:
Fan hub radius – 0.1 m
Profile specification of tangential velocity – 1.2 m/s
Profile specification of radial velocity – 0.0 m/s
Wall boundary condition
Wall motion – Stationary wall
Shear condition – No slip
Roughness model - Standard
Figure 2.2: Applied boundary conditions

4. 3
3 Computational mesh
Figure 3.1: Isometric view of domain with mesh
Figure 3.2: Mesh view in XZ plane through fan surface
Figure 3.3: Mesh view in fan region using cross sectional views in XY, YZ and ZX
planes through fan center and fan surface

5. 4
Table 3.1: Mesh details
Statistics
Nodes 419016
Elements 404700
Mesh Metric Skewness
Min 1.3057e-010
Max 0.50002
Average 0.12616
Standard Deviation 0.14053
Mesh Metric Orthogonal Quality
Min 0.71075
Max 1.00000
Average 0.95871
Standard Deviation 6.3766e-002
Mesh Metric Aspect Ratio
Min 1.0171
Max 10.516
Average 2.5799
Standard Deviation 1.0672
Figure 3.4: Skewness of the mesh
Figure 3.5: Orthogonal quality of the mesh
Figure 3.6: Aspect ratio of the mesh

6. 5
4 Methods and governing equations solved
4.1 Governing equations
Governing equations that solved in the simulation are continuity equation and momentum equation.
As there is no need to evaluate the temperature in the domain, the energy equation is not used.
Continuity equation
𝜕𝜌
𝜕𝑡
+ 𝑑𝑖𝑣(𝜌𝒖) = 0 (1)
x-momentum equation
𝜕(𝜌𝑢)
𝜕𝑡
+ 𝑑𝑖𝑣(𝜌𝑢𝒖) = −
𝜕𝑝
𝜕𝑥
+ 𝑑𝑖𝑣(𝜇 𝑔𝑟𝑎𝑑(𝑢)) + 𝑆 𝑀𝑥 (2)
y-momentum equation
𝜕(𝜌𝑣)
𝜕𝑡
+ 𝑑𝑖𝑣(𝜌𝑣𝒖) = −
𝜕𝑝
𝜕𝑦
+ 𝑑𝑖𝑣(𝜇 𝑔𝑟𝑎𝑑(𝑣)) + 𝑆 𝑀𝑦 (3)
z-momentum equation
𝜕(𝜌𝑤)
𝜕𝑡
+ 𝑑𝑖𝑣(𝜌𝑤𝒖) = −
𝜕𝑝
𝜕𝑧
+ 𝑑𝑖𝑣(𝜇 𝑔𝑟𝑎𝑑(𝑤)) + 𝑆 𝑀𝑧 (4)
Since this simulation is transient,
𝜕(𝜌𝜙)
𝜕𝑡
term in equation 1,2,3 and 4 cannot be neglected. Convection
terms and diffusion terms in the momentum equation is considered to solve the problem.
4.2 Boundary conditions
Apart from the wall boundary condition, the fan is modelled using fan boundary condition in
ANSYS FLUENT. Here fan is considered as infinitely thin surface and there is discontinuous pressure
rise across the surface is specified as a velocity function given in equation 5.
∆𝑝 = ∑ 𝑓𝑛 𝑣 𝑛−1
𝑁
𝑛=1
(5)
where ∆𝑝 is the pressure jump, 𝑓 𝑛
are the pressure jump polynomial coefficient and 𝑣 is the local
fluid velocity normal to the fan. If the pressure jump across the fan is constant, the profile specification
of pressure jump option is used as in this project. The given momentum source is 55kgm-2
s-2
and the
thickness of the fan volume is 6cm, pressure jump is calculated as in equation 6.
𝑃𝑟𝑒𝑠𝑠𝑢𝑟𝑒 𝑗𝑢𝑚𝑝 =
𝑣𝑜𝑙𝑢𝑚𝑒 𝑜𝑓 𝑡ℎ𝑒 𝑓𝑎𝑛 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑦
𝐴𝑟𝑒𝑎 𝑜𝑓 𝑡ℎ𝑒 𝑓𝑎𝑛 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑦
× 𝑚𝑜𝑚𝑒𝑛𝑡𝑢𝑚 𝑠𝑜𝑢𝑟𝑐𝑒 (6)
𝑃𝑟𝑒𝑠𝑠𝑢𝑟𝑒 𝑗𝑢𝑚𝑝 = 3.3𝑃𝑎
Radial and tangential velocities in the fan are modelled using equation 7 and 8 respectively.
𝑈 𝜃 = ∑ 𝑔 𝑛 𝑟 𝑛
;−1 ≤ 𝑁 ≤ 6
𝑁
𝑛=1
(7)
𝑈𝑟 = ∑ ℎ 𝑛 𝑟 𝑛
; −1 ≤ 𝑁 ≤ 6
𝑁
𝑛=1
(8)
where 𝑈 𝜃 and 𝑈𝑟 are tangential and radial velocities on the fan surface in m/s, 𝑔 𝑛 and ℎ 𝑛 are
tangential and radial velocity polynomial coefficients and r is the radius of the fan from the centre. In
this project fan radial component is zero and tangential component and profile specified velocity is
selected as 1.2 m/s.
There are 4 turbulent models used in this project; k-ω standard, k-ω SST, k-ε standard, k-ε RNG.
The comparison of the results of each model is evaluated at the end of the project.

7. 6
4.3 The k-ε standard turbulence model
Here there are two additional transport equations of turbulent kinetic energy and dissipation to
model turbulent viscosity using
Turbulent
viscosity 𝜇 𝑡 = 𝜌𝐶𝜇
𝑘2
𝜖
(9)
Turbulence
kinetic energy
𝜕(𝜌𝑘)
𝜕𝑡
+
𝜕(𝜌𝑘𝑢𝑖)
𝜕𝑥𝑗
=
𝜕
𝜕𝑥𝑗
[(𝜇 +
𝜇 𝑡
𝜎 𝑘
)
𝜕𝑘
𝜕𝑥𝑗
] + 2𝜇 𝑡 𝐸𝑖𝑗. 𝐸𝑖𝑗 − 𝜌𝜖 (10)
Dissipation
rate
𝜕(𝜌𝜖)
𝜕𝑡
+
𝜕(𝜌𝜖𝑢𝑖)
𝜕𝑥𝑗
=
𝜕
𝜕𝑥𝑗
[(𝜇 +
𝜇 𝑡
𝜎𝜖
)
𝜕𝑘
𝜕𝑥𝑗
] + 𝐶1𝜖
𝜖
𝑘
2𝜇 𝑡 𝐸𝑖𝑗. 𝐸𝑖𝑗 − 𝐶1𝜖 𝜌
𝜖2
𝑘
(11)
4.4 The k-ε RNG turbulence model
This method is developed by Re-Normalisation Group (RNG) to normalise the Navier-Stokes
equations. Here 𝐶1𝜖 value is not fixed. That introduces strain-dependent relation to improve the
performance at low Reynolds number.
4.5 The k-ω standard turbulence model
This turbulence model, there are two additional equations to model the kinematic eddy viscosity.
Kinematic eddy viscosity 𝑣 𝑇 =
𝑘
𝜔
(12)
Turbulence kinetic energy
𝜕𝑘
𝜕𝑡
+ 𝑈𝑗
𝜕𝑘
𝜕𝑥𝑗
= 𝜏𝑖𝑗
𝜕𝑈𝑖
𝜕𝑥𝑗
− 𝛽∗
𝑘𝜔 +
𝜕
𝜕𝑥𝑗
[(𝑣 + 𝜎∗
𝑣 𝑇)
𝜕𝑘
𝜕𝑥𝑗
] (13)
Specific dissipation rate
𝜕𝜔
𝜕𝑡
+ 𝑈𝑗
𝜕𝜔
𝜕𝑥𝑗
= 𝛼
𝜔
𝑘
𝜏𝑖𝑗
𝜕𝑈𝑖
𝜕𝑥𝑗
− 𝛽𝜔2
+
𝜕
𝜕𝑥𝑗
[(𝑣 + 𝜎𝑣 𝑇)
𝜕𝜔
𝜕𝑥𝑗
] (14)
4.6 The k-ω SST turbulence model
The k-ω standard model is modified and there are 5 auxiliary equations apart from the equation
15,16 and 17. The Shear Stress Transport (SST) give
Kinematic
eddy
viscosity
𝑣 𝑇 =
𝑎1 𝑘
𝑚𝑎𝑥(𝑎1 𝜔, 𝑆𝐹1)
(15)
Turbulence
kinetic
energy
𝜕𝑘
𝜕𝑡
+ 𝑈𝑗
𝜕𝑘
𝜕𝑥𝑗
= 𝑃𝑘 − 𝛽∗
𝑘𝜔 +
𝜕
𝜕𝑥𝑗
[(𝑣 + 𝜎 𝑘 𝑣 𝑇)
𝜕𝑘
𝜕𝑥𝑗
] (16)
Specific
dissipation
rate
𝜕𝜔
𝜕𝑡
+ 𝑈𝑗
𝜕𝜔
𝜕𝑥𝑗
= 𝛼𝑆2
− 𝛽𝜔2
+
𝜕
𝜕𝑥𝑗
[(𝑣 + 𝜎 𝜔 𝑣 𝑇)
𝜕𝜔
𝜕𝑥𝑗
] + 2(1 − 𝐹1)𝜎 𝜔2
1
𝜔
𝜕𝑘
𝜕𝑥𝑖
𝜕𝜔
𝜕𝑥𝑖
(17)
4.7 Pressure velocity coupling method
The coupled algorithm is used for the above four turbulence models as that give some advantages
over non-coupled schemes or segregated approach. Higher performance, robust and efficient
implementation for single-phase problems can be obtained by using that algorithm. Also, this method
gives better results in transient problems with poor mesh quality and when large time steps are used.
Here 0.1s time step is used for all the simulations to reduce the computational time. So, the coupled
algorithm is used for the simulation.
Default values for the Relaxation factors of the parameters are used for simulation with residuals
convergence of 1e-6 for continuity, 1e-4 is used for three momentum equations and other turbulence
model-dependent parameters.

8. 7
5 Results
The generated airflow from the fan is highly turbulent. So that selection of the suitable turbine model
is essential to obtain accurate results. By analysing the results obtained by using four different turbulence
models, the k-ω SST turbulent model can generate more accurate results than others. These results are
shown in figure 5.1, 5.2, 5.3 and 5.45.1. RNG k-ε model provides good results second to the k omega
SST model.
Since the SS k-ω model can deal with high and low Reynolds number flow in adverse pressure
gradient conditions because of the cross-diffusion term in the equation. That model was developed by
combining the effect of k-ε and k-ω models.
By calculating the error of deviating the results from the experimental results, that scheme gives a
better understanding of the selection of the turbulence model.
Turbulence model Percentage of values within the error bar
SST k-ω model 78.52
RNG k-ε model 78.15
Standard k-ω model 64.97
Standard k-ε model 63.65
Figure 5.1: Measurements and CFD results comparison at increasing distance from the axis of the
ceiling fan (SST k-omega model)

9. 8
Figure 5.2: Measurements and CFD results comparison at increasing distance from the axis of the
ceiling fan (RNG k-ε model)
Figure 5.3: Measurements and CFD results comparison at increasing distance from the axis of the
ceiling fan (Standard k-omega model)

10. 9
Figure 5.4: Measurements and CFD results comparison at increasing distance from the axis of the
ceiling fan (Standard k-ε model)
Figure 5.5: Measurements and CFD results comparison - perimeter
points (SST k-ω model)

11. 10
Figure 5.7: Measurements and CFD results comparison - perimeter
points (RNG k-ε model)
Figure 5.8: Measurements and CFD results comparison - perimeter
points (Standard k-ε model)
Figure 5.6: Measurements and CFD results comparison - perimeter
points (Standard k-ω model)

12. 11
6 Conclusion
In this project, the ceiling fan is modelled as a surface in the domain and applied fan boundary
condition to get the required effect. That helps to simplify the problem and causes to reduce
computational cost compared with the sliding mesh arrangements.
Selection of the turbulence model to get results from modelling the ceiling fan is a critical parameter
as the flow generated by the fan is highly turbulent. By comparing k-ω SST, k-ω standard, k-ε RNG and
k-ε standard turbulence models, the k-ω SST model gives better results followed by k-ε RNG model. By
comparing the experimental data with the simulated results, 78.5 % of them are with the 5% error bar
limes in the k-ω SST model and 78.1% values are in the k-ε RNG model.
As a conclusion, the k-ω SST model is more suitable to model ceiling fan effect in the closed domain
than Standard k-ω and Standard k-ε models. The RNG k-ε model can also give accurate results compared
with the other two.
Figure 5.9: Airflow field generated by the ceiling fan at 10s time step in SST k-omega model