Jamie Fogarty CFD FINAL DRAFT PRINT

ME6062 - Advanced Computational Fluid Dynamics – Spring 2015-2016 1

Abstract- This paper presents the comparison of 3
Computational Fluid Dynamics (CFD) models in the
computation of a conduction-convection conjugate heat
transfer problem. As no CFD model is universal to all
problems, their comparison can highlight the pros and
cons of each model and aid in the determination of the
most suitable for the specific problem. The
functionalities of turbulence models is introduced and
discussed to obtain an appreciation for the computed
results.
CFD Software, Star CCM+, is used to conduct an
analysis on a plate-fin heat sink with 6 fins. A heat load
of 160,000W/m2 is applied to the base plate of the heat
sink, and the heat sink is subjected to forced convection
corresponding to a channel Reynold’s number of 900, at
room temperature. The heat sink is modelled using PTC
Creo Parametric and imported into Star CMM+ where a
polyhedral mesh is applied and refined. 5 simulations
are conducted using the laminar model, Standard Low-
Reynolds Number k-ε model (low y+ & high y+ wall
treatment) and V2F Low-Reynolds Number k-ε model
(low y+ & high y+ wall treatment). Convergence was
gauged from the residual plots, maximum heat sink base
plate temperature monitor and pressure drop monitor.
The results were then benchmarked with theoretical
calculations for heat sink thermal resistance and
pressure drop to ensure their validity.
The results for all simulations conducted correlate with
theory to within 10% for the heat sink thermal resistance
and 20% for the pressure drop over the heat sink, and
also correlate extremely close one another. The most
efficient model for the problem was deemed to be the
laminar solver, as it yielded the same accuracy as the
turbulence models in the least amount of time. It was
also found that in the cause of a fine, refined mesh, the
low y+ wall treatment enables the turbulence models to
iterate faster.
22/04/16 10100598@studentmail.ul.ie
I. INTRODUCTION
fluid flow and it’s physical aspects are governed by
three fundamental principles, that is the
conservation of mass, the conservation of energy and
Newton’s second law (F=ma). These principles can be
expressed in terms of, usually, partial differential
equations. In basics terms, Computational fluid
dynamics (CFD) is, in part, the art of replacing the
governing partial differential equations of fluid flow
with numbers, and advancing these numbers in space
and/or time to obtain a final numerical description of
the complete flow field of interest (Wendt and Anderson
2009). In saying so, this is not the inclusive limit of CFD
capabilities, as there are some problems that allow for an
immediate solution without advancing in space or time,
and also contain integrals as opposed to differentials.
The CFD software used to conduct the analysis in this
paper is called Star CCM+. This software provides a
comprehensive engineering physics simulation,
inclusive of an entire engineering process for solving
problems involving flow (of fluids or solids), heat
transfer, and stress (CD-Adapco, 2016). This software
will be used to obtain a physical description of a
conductive-convective conjugate-heat transfer problem.
Conjugate heat transfer is the interaction of at least two
mediums or subjects (Dorfman 2010). This problem will
be the interaction of a cooling fluid, air, flowing over a
heat sink with applied heat flux at the base. A heat sink
is a device to effectively absorb thermal energy from one
location and dissipate it to the surroundings (air)
through use of extended surfaces, such as fins. Heat
sinks are used in a wide range of applications where
efficient heat dissipation is required; major examples
included refrigeration, heat engine, and cooling
electronic devise (Lee 2010). The most common heat sink
design will be considered, a heat sink with longitudinal
rectangular fin array as the extended surface. This type
of heat sink has the benefit of simple design, low
fabrication costs and high thermal performance
achievable.
Comparison of Turbulence Models in Predicting
Heat Transfer Parameters of a Finned Heat Sink
under Forced Convection
Jamie Fogarty
Department of Mechanical, Aeronautical & Biomedical Engineering, University of Limerick
A

This paper will outline the procedures for modelling
such a problem using that CFD software, and will aim to
compare three different turbulence models used by the
software, in order to arrive at a numerical solution of the
problem at hand. Turbulence models, their
functionalities and differences will be introduced,
discussed and compared. The abilities of each
turbulence model will be benchmarked by theoretical
calculations and solutions, to determine the most
suitable model for this conjugate heat transfer problem.
The models will be compared to theoretical calculations
for heat sink thermal resistance and pressure drop.
II. OBJECTIVES
The main objective of this paper is to provide a platform
of understanding on the functionalities of CFD software
and turbulence modelling. This will be achieved through
the analysis and benchmarking of a conjugate heat
transfer problem of a heat sink under forced convection.
The objectives are as follows;
 Introduce and use correlations to determine the
theoretical values for the heat sink:
o Thermal Resistance
o Pressure Drop
 Model the heat sink in CAD software
 Import software into Star CCM+ develop an
adequate mesh
 Introduce the concept of turbulence modelling
and develop its concept
 Determine the most suitable turbulence model
to use in conduction of a mesh sensitivity study
 Introduce the turbulence models to be
considered, highlighting the reason for choice
and the differences and similarities between the
models, in the context of equations used by each
 Conduct a mesh sensitivity study to determine
the most sufficient mesh, in terms of cell count,
size, etc.
o Mesh sensitivity will be bench marked
from the theoretical calculations of
thermal resistance and pressure drop
 Once an adequate mesh has been generated and
correlates with theoretical calculations, the
model used will be compared to other slected
models to gauge how they compare.
o The comparison will be drawn from
theoretical calculations, Resistance and
Pressure drop, and also to determine
which turbulence model best captures
the behavior of the forming boundary
layers between the plates.
III. GEOMETRY
In order for the reader to gain an appreciation for the
theory and theoretical calculations, it is effective to
firstly define visually the heat sink under consideration.
The heat sink under analysis is a plate-fin heat sink with
6 fins. The modelled heat sink has two fins, Figure 1, and
advantage was taken of the symmetry plane options
when defining the boundary conditions of Star CCM+.
The heat sink was modelled using PTC Creo Parametric
and imported into Star CCM+.
Figure 1: Front,side andangledviewof plate-fin heat sink modelled.
The dimensions of the total heat sink, with the
symmetry planes implemented, are presented in Table 1.
Note, that the heat sink will have half a channels width
at the fins closest to the either side of the width (when
looking from a front view).
Dimension (mm)
Base Height 6
Fin Height 30
Channel Thickness 1.5
Fin Thickness 1
Base Width 15
Length 60
Table 1: Plate-FinHeat sinkdimensions, with the symmetry planes in
mind.
The heat sink was enclosed in a bounding box of width
15mm, height 31mm and length 360mm. The bounding
box was placed on the top of the base plate, and just
encloses the fins and the exposed area of the base plate
top surface. This can be seen in Figure 2. The heat sink
was positioned 120mm from the defined inlet, and
180mm from the defined outlet. The heat sink is not
equidistant from either let, as the effect of the heat sink
wake would like to be visualised.

Figure 2: Heat-sink including bounding box.
IV. FLUID & SOLID MATERIAL PROPERTIES
The material properties of both the fluid and solid
region (air and aluminium heat sink) are presented in
Table 2. These values were used for both the theoretical
calculations and for the CFD analysis.
Property Air Aluminum Units
ρ 1.18415 2702 Kg/m3
k 1.85508 237 W/m-K
Cp 0.0257 - J/Kg-K
μ 0.9 - Pa-s
α 1003.62 - /K
Pr 0.0333 - -
Table 2: Fluid and solid material properties used in both theoretical
calculations and CFD analysis
V. THEORY
The theoretical calculations conducted were aimed to
obtain the; heat sink thermal resistance and the pressure
drop through the heat sink. This section outlines the
theoretical equations used.
The heat sink thermal resistance is given by;
Rtot = Rhs +
H−Hf
kbase .w.L
(Eqn. 1)
(Simons, 2003)
The second term is the thermal resistance of the base,
where H is the total height of the heat sink, Hf is the
height of the fins, kbase is the thermal conductivity of the
base, w is the width and L is the length. The first term,
Rhs, is the thermal resistance of the heat sink fins and is
given by;
Rhs =
1
h .(Abase +NfinηfinAfin)
(Eqn. 2)
(Simons, 2003)
Where Abase is the exposed area of the base (between the
fins), Nfin is the number of fins, ηfin is the fin efficiency,
and Afin is the surface area per fin taking into account
both sides of the fin.
The pressure drop, ΔP (Pa), across the heat sink is given
by:
ΔP = (Kc + 4. fapp .
L
Dh
+ Ke). ρ.
V2
2
(Eqn. 3)
(Culham & Muzychka, 2001)
Where Kc and Ke are coefficients that represent the
pressure losses due to sudden contraction channels and
expansion of the flow entering and leaving the heat sink
respectively. fapp is the apparent friction factor, that takes
into account the developing and developed regions of
the flow in the heat sink channels.
Appendix A presents a full representation of the
equations and correlations used to calculate both the
thermal resistance and pressure drop.
VI. FLOW CONDITIONS
Firstly, it is necessary to state that two flow conditions
will be present. That is, the flow condition of the fluid in
the bounding box, and the flow condition of the fluid
through the heat sink channels. The air will be
introduced into the inlet at a temperature of 293K and a
velocity of 2.9m/s, corresponding to a Volume Flow
Rate 𝑉̇ of 1.35x10-3 m3/s. Dividing the Volume Flow Rate
by the open cross sectional area of the heat sink (i.e.
between the fins and the bounding box) gives a velocity
of 5m/s through the heat sink channels. The Reynold’s
number corresponding to the bounding box is Re=3740,
which is in the turbulent regime, and the channel
Reynolds number is Rech=900, which is in the laminar
regime.
The problem under consideration is one of a conductive
-convective heat transfer. A heat flux 𝑄̇ of 16,000W/m2
will be applied to the bottom of the heat sink base plate,
corresponding to a heat load q of 14.4W. This will
conduct through the heat sink base and fins, where it
will be subjected to forced convection by the working
fluid.
VII. TURBULENCE MODELLING
This section aims to briefly describe the concept of
turbulence modelling and present some of the
fundamental equations used in aid to develop a basis for
which turbulence models under consideration may be
compared.
Firstly, consider a laminar flow. In the computation of a
laminar flow, the Navier-stokes equations are solved
directly. For the computation of a turbulent flow, the
starting point for any CFD software is the conservation
of mass and continuity. Making the assumption that the
fluid is incompressible, with constant-property
following the continuum hypothesis, no thermal

interaction and no other body-forces, the conservation of
mass and momentum can be denoted in its conservation
form, after the addition of a time-averaging. The time-
averaging process takes the Navier-Stokes equations for
the instantaneous velocity and pressure fields are
decomposed into a mean value and a fluctuating
component (Wilcox, 2010). This equation is otherwise
known as the Reynolds-Averaged Navier Stokes (RANS)
equation and is;
𝜌
𝜕𝑈 𝑖
𝜕𝑡
+ 𝜌𝑈𝑗
𝜕𝑈 𝑖
𝜕 𝑥 𝑗
= −
𝜕𝑃
𝜕𝑥𝑖
+
𝜕
𝜕𝑥 𝑗
(2𝜇𝑆𝑖𝑗 − 𝜌𝜇 𝑗
′ 𝜇 𝑖
′̅̅̅̅̅̅) (Eqn. 4)
Where 𝜇 𝑗
′ 𝜇 𝑖
′̅̅̅̅̅̅ is a time-averaged rate of momentum
transfer due to turbulence, and 𝜌𝜇 𝑗
′ 𝜇𝑖
′̅̅̅̅̅̅ is known as the
Reynolds-stress tensor. The time-averaged Navier stokes
equations are identical to the instantaneous equations
aside from the replacement of instantaneous variables
with mean values and the addition of a time-averaged
rate of momentum transfer due to turbulence.
The Reynolds stresses arise from the velocity
fluctuations associated with the turbulence of the flow.
The purpose of a turbulence model is to compute the
Reynold’s stress tensor in terms of the mean flow
quantities, and provide closure for the governing
equations (Griffin, 2016). Various methodologies exist to
try achieving this end goal. The one of interest in this
project is the eddy viscosity method.
Every turbulence model begins with the Boussinesq
eddy-viscosity approximation to compute the Reynolds
stress tensor as the product of an eddy viscosity and the
mean strain-rate tensor. For computational simplicity,
the eddy viscosity, in turn, is often computed in terms of
a mixing length that is analogous to the mean free path
in a gas. Because of this, the eddy viscosity and mixing
length must be specified in advance, most simply, by an
algebraic relation between eddy viscosity and length
scales of the mean flow. Thus, each turbulence model
computes a different algebraic relation for eddy
viscosity (Wilcox, 2010). Boussinesq’s eddy-viscosity in
mixing length form is given as:
𝜇 𝑡 = 𝐶 𝜇 𝜌𝜐𝑡 𝑙 𝑡 (Eqn. 5)
Where Cµ is a constant, νt is the averaged eddy transport
velocity around the flow field (velocity scale) and lt is
the distance an eddy travels before it exchanges it
original mean momentum (length) scale) (Griffin, 2016).
Turbulence models are then categorised by the number
of equations used to compute the eddy viscosity into
mean flow parameters. Two-equation models are the
most popular choice loaning to their effective balance
between computational cost and accuracy. The
turbulence models used in the analysis will be two-
equation models. Two-equation models are reliant on
the Boussinesq hypothesis to evaluate the Reynolds
stresses, and are based around the transport for
turbulent kinetic energy defined k, and in the case of the
turbulence models of interest, the turbulence dissipation
rate per unit mass ε.
The combination of k- ε brings us to the k- ε turbulence
models and its variants. Recalling Eqn. 27, we can infer
that the velocity of the large eddies is proportional to √𝑘,
defining the turbulence velocity scale as;
𝜐𝑡 = √𝑘 (Eqn. 6)
The time scale associated with the turbulence is given by
the length scale divided by the velocity scale (eqn. 6),
and the dissipation rate per unit mass can be expressed
as (eqn. 7):
𝑡𝑡 =
𝑙 𝑡
√𝑘
(Eqn. 7) 𝜀 =
𝑘1 .5
𝑙 𝑡
(Eqn. 8)
Using this, the turbulence length scale can be expressed
in terms of k and ε;
𝑙 𝑡 =
𝑘1.5
𝜀
(Eqn. 9)
Now substituting into Prandtl’s turbulence viscosity
expression gives;
𝜇 𝑡 = 𝜌𝐶 𝜇
𝑘2
𝜀
(Eqn. 10)
This is used to compute the turbulent viscosity in the k-
ε model, and then the turbulence viscosity is used in
conjunction with the Boussinesq approximation to
calculate the Reynolds stresses. In order to arrive at a
numerical solution, it is necessary for the model to also
use a modified transport equation for k and ε consisting
of semi-empirical correlations and approximations for
the unknown/immeasurable terms, along with closure
coefficients. The model describe is called the Standard k-
ε model. Although this model is reasonably accurate for
a wide range of flows, it performs poorly for flows with
large swirls, pressure gradients and separation.
Let’s consider two other variations of this turbulence
model. Standard Low-Reynolds Number k-ε (Lien et al.
1996) and the V2F Low-Reynolds Number k-ε (Durbin
1991, Lien at al. 1998).
The first, Standard Low-Reynolds number k-ε, is
identical to the standard model except for the additional
turbulence production term in the modelled ε equation.
Also, this model computes the eddy viscosity the same
way, with addition of a damping function, fμ:
𝜇 𝑡 = 𝜌𝑓𝜇 𝐶 𝜇
𝑘2
𝜀
(Eqn. 11)

This damping function is present to ensure that the
turbulent viscosity attenuates accordingly in the near-
wall region (Griffin, 2016). It should be noted that both
the standard model and low Re model cannot be
implemented directly to the wall, as the ε- equation
contains a term which cannot be computed at the wall.
As a result, it is necessary for the models to use wall
functions.
The law of the wall is one of the most famous
empirically-determined relationships in turbulent flows
near solid boundaries. Measurements show that, for
both internal and external flows, the stream wise
velocity in the flow near the wall varies logarithmically
with distance from the surface. This behaviour is known
as the law of the wall (Wilcox, 2010). This behaviour can
be categorised into three sections:
 The viscous or linear sublayer – viscous stresses
dominate in this region
 The buffer layer –both viscous and turbulent
shear stresses are of equal magnitude.
 The log-law layer– influence of turbulent shear
(Reynolds) stresses is strongest and viscous
stresses are small.
In order to compute the near wall region, Star CCM+
offers three alternative wall treatments. These are Low
y+, High y+ and all y+ wall treatment. y+ is a
dimensionless parameter that defines the central
distance of a wall bounded cell. Low y+ is used when
the centre of the near-wall cell is as a y+ value of under 1
(viscous sublayer), high y+ is between 5-30 (buffer layer)
and the all y+ is a hybrid model that attempts to provide
a more realistic modelling than either low or high Re
wall treatments if the wall adjacent cell lies in the buffer
layer.
The V2F model is also a low Reynold number k- ε model
variant that can model the anisotropy of near-wall
turbulence. The model is similar to the standard model
but rather than use the turbulent kinetic energy to
calculate the eddy viscosity it used a velocity scale 𝑣′2̅̅̅̅.
The V2F model is able to provide the correct scaling for
the representation of the damping of turbulence in the
near-wall region without actually using exponential
damping or the wall functions (Griffin, 2016).
Anisotropic turbulent behaviour close to the walls is
modelled through an elliptic relaxation function f. The
model solves this, along with 𝑣′2
, k and ε making it
essentially a four equation model. The V2F model was
originally developed for attached or mildly separated
boundary layers but can simulate with reasonable
accuracy flows that are dominated by separation
(Griffin, 2016). The eddy viscosity is given by:
𝜇 𝑡 = 𝜌𝐶 𝜇2 𝑣′2
T (Eqn. 12)
Where T is a turbulent timescale. The V2F model can
accurately model anisotropic flow and heat transfer
effects in wall-bounded, channel and jet flows, and has
been chosen as one of the models to compare.
VIII. PROCEDURE
A. Mesh Generation
This section outlines the meshing procedure, in order to
enable the conjugate heat transfer solution. The mesh
generation procedure was as follows:
 Once imported, the heat sink model was
sectioned into two parts; Heat Sink and Fluid
Region. The Heat sink was then broken further
into two subgroups; fins and base plate.
 The base plate of the heat sink was split (by
patch) so that the base plate of the heat sink
could be considered an individual part among
the heat sink sub-group. This was conducted in
order to create a boundary where a heat flux
could be applied. This will simulate a heat flux
from a heater matt/component/etc.
 Next, the fluid region was extracted by the
subtract function. This function would separate
the region where the fluid will flow from the
heat sink fins.
 Next an imprint function was executed. This
function allows for the option of a conformal
mesh i.e. the mesh faces match one-to-one at
interfaces to ensure heat transfer occurs
smoothly.
 Next it was necessary to apply parts to regions.
The subtract was assigned fluid region, and the
heat sink was assigned solid region, with each
part surface having a boundary.
 Next it was necessary to create interfaces
between certain faces within the model. The
boundaries were created were:
o Heat sink Base plate – Heat sink Base
o Heat sink Base – Heat sink Fins
o Fluid Region: Heat sink fin faces – Heat
sink: Fins
o Fluid Region: Heat Sink Base Faces –
Heat sink: Base
 This was done so that the mesh of the solid and
fluid region could communicate at these
interfaces and exchange values, in order for the
conjugative heat transfer (conduction-
convection) to solve correctly.
 Two automated mesh operations were used for
the fluid region and the solid region. This was

done to have the option of turning the prism
layers on or off for the fluid region.
 A coarse polyhedral mesh was applied initially,
and then further refined as necessary, ensuring
correlation with theory and ensuring
consistency through visual inspection.
A mesh sensitivity study was conducted and is in
Section IX. The resulting refined mesh is shown in
Figure 3. This figure presents a top view of plane section
taken across the heat sink, displaying the mesh
concentration at the fin’s leading edge and in between.
The image below it shows a plane section taken to
display the mesh through the middle of the entire
section. This displays the concentration of the mesh
approaching, and leaving the heat sink region. The final
image at the bottom illustrates the mesh concentration at
the trailing edge.
Figure 3: Top (plane sectioncut through the heat sinkfins and fluid domain),
middle (plane sectiontaken to present a side view of mesh), bottom (cross
sectional plane to show mesh concentration at trailing edge)
B. Physics models and Continua
In order to arrive at a full solution of the flow field, it is
necessary to enable various models, in addition to the k-
ε- models, to aid the solution. The following models
were used:
Fluid Continua Solid Continua
Boussinesq Model -
Constant Density Constant Density
Gas Multi-part Solid
Gradients Gradients
Gravity -
Segregated flow -
Segregated fluid
temperature
Segregated solid energy
Steady Steady
Three Dimensional Three Dimensional
Turbulent -
Table 3: Physics continua models usedin addition tothe k- ε models in
order to arrive at a full description of the flow field
 Boussineq model
o This model provides a buoyancy source
term that only applies when there are
small variations of density due to
temperature variations.
 Segregated Fluid/Solid Temperature
o This model solves the total energy
equation with temperature as the solved
variable.
 Gradients
o This model accounts for:
 Secondary gradients for
diffusion terms
 Pressure gradients for pressure-
velocity coupling in the
segregated flow model
 Strain-rate and rotation-rate
calculations for turbulence
models
 Segregated Flow Model
o This model solves the flow equations
(one for each component of velocity,
and one for pressure) in a segregated, or
uncoupled, manner.
 Gravity
o The Gravity model accounts for the
action of gravitational acceleration in
STAR-CCM+ simulations.
o For fluids, it provides two effects:
 The working pressure becomes
the piezometric pressure.
 The body force due to gravity
can be included in the
momentum equations.
Note the descriptions of each models purpose are
sourced from Cd-Adapco’s Star CCM+ User Manual.
C. Benchmarking
In order to ensure the validity of the model, the
computed results will be benchmarked from the theory
presented earlier. This will be conducted in conjunction
with a mesh sensitivity study. Initially, the mesh
sensitivity study will only factor in the heat sink thermal
resistance and pressure drop. This will ensure the
validity of the model. After hand, as the boundary layer
is also of interest, a visual sensitivity study will be
conducted in which the essential mesh to model the
development of the boundary layer will be conducted.
The Theoretical calculations are as follows:

Channel Reynold’s
number (Rech)
Thermal
Resistance (Rhs)
Pressure
Drop (ΔP)
900 1.03 K/W 53.32 Pa
Table 4: Theoretical calculations correspondingtoan inlet velocity of
2.9 m/s, a channel average velocityof 5 m/s anda channel Reynolds number
of 900.
D. Numerical Methods and Convergence
To monitor convergence, the software automatically
creates a residual monitor plot. This plot computes the
error in the solution of the solved equations. The
software takes an initial guess and solves discrete
equations for each cell. From this, the error is computed
and processed into a residual to then be normalized so
that it varies between 0 and 1. Although it can be said
that the solution is converged when the residuals tend
towards a small number, it is more effective to ensure
convergence by monitoring quantities of interest. To
help assess the stability and extent of convergence of the
solution, a maximum temperature monitor (of the base
plate) and pressure drop monitor (between the inlet and
the outlet) were set up.
The convergence of the solution was achieved when the
residuals stabilised under a residual value of 1x10-3 and
the maximum temperature monitor’s, and pressure drop
monitor’s slope tended towards 0 and preceded in a
stable manor. Figure 4 and 5 present a residual plot and
a maximum temperature monitor respectively for the
laminar simulation run. The residuals consist of 5
components, 4 residuals resulting from the solved
transport equations and another residual from the
solved energy equation with temperature as the
variable. Convergence can be identified from the
maximum temperature plot as the slope tends to 0, and
the temperature remains constant.
Figure 4: Residual plot example, correspondingtothe laminarsolution
whose results are presented in the next section
Figure 5: Maximum temperature monitor plot, corresponding to the
laminar solution previous mentioned
IX. MESH SENSITIVITY STUDY
In the conduction of the mesh sensitivity study, the
Standard Low-Reynolds Number k-ε Model (Lien et al.
1996) was used, as it is effective in conjugate heat
transfer and also computationally efficient in
comparison to the V2F model. This model will give a
good representation of the validity of the simulation.
In the study, the initial wall treatment was set to low y+.
Low y+ wall treatment was used as the y+ values
corresponding to each base size used were in the range
of 1-2. The wall y+ values were obtained from a surface
average monitor on the fins alone. Appendix A contains
the settings used in the mesh sensitivity study. In
general, within the heat sink volume a polyhedral mesh
was used. In the fluid region the same mesher was used,
with addition of the surface repair, thin mesher and
prism layer option. The thin mesher maximum thickness
was set to the heat sink channel thickness. This allowed
for a consistent mesh through the channels. The prism
layer mesher was used in the fluid region and between
the heat sink fins. In the fluid region only one prism
layer was used, and between the fins 5 were originally
used. The prism layer gap fill percentage was increased
to the maximum in order to enable the prism layers to
fill the gap between the fins. Custom controls enabled
the mesh to be concentrated at the leading and trailing
edge of the heat sink fins. At the leading edge this allows
for a smooth transition of the mesh into the restricted
flow area and at the trailing edge to facilitate the wake
left by the fins. The results obtained are as follows:

With the applied settings, the base size was varied from
30-5mm in increments of 5mm. The results are presented
in Table 5.
Base
Size
(mm)
Rhs Error
(%)
ΔP Error
(%)
y+ Cell
Count
30 1.1736 14.08 43.59 18.25 1.4 24187
25 1.1240 9.26 43.35 18.70 1.4 31084
20 1.1295 9.80 43.42 18.57 1.41 46727
15 1.1356 10.38 42.98 19.40 1.41 75764
10 1.1396 10.77 39.81 25.34 1.39 156072
5 1.14 10.81 38.15 28.45 1.38 617042
Table 5: Mesh sensitivity study results for a base size varied from
30mm-5mm in 5mm increments
Studying Table 5, it is evident that the initial mesh
correlated quite close with theory. As the mesh base size
decreases the thermal resistance sits around 10% error
from theory, which is sufficiently close. On the other
hand, as the base size decrease the pressure drop
digresses from the theoretical value. This may be due to
the fact that the pressure drop correlation used does not
facilitate the flow conduit that the heat sink is in, and is
an idealisation. With the given results it was decided to
take the base size of 15mm and add some additional
refinements. This was selected in consideration of the
iteration time and accuracy. The number of prim layers
between the fins was increased to 10, while their
stretching was changed to 1.15. The results are as
follows:
Base
Size
(mm)
Rhs Error
(%)
ΔP Error
(%)
y+ Cell
Count
15 1.1387 10.69 41.57 22.03 0.5 247623
Table 6: Refinement to the 15mm base size mesh used in the initial
mesh sensitivity study
With further refinements conducted, Table 6 displays
that the percentage error increases slightly. It should be
noted that the validity of either the computational model
or theory is undermined by experimentation. However,
no experimental results are available for this heat sink
under the given conditions. Regardless, the
benchmarking conducted indicates agreeance in
particular with the heat sink thermal resistance, and
some agreeance in regards to pressure drop.
X. RESULTS
The refined mesh was used the compare the results of 3
different models; V2F Low-Reynolds Number k-ε model
(Low Re), V2F Low-Reynolds Number k-ε model (V2F)
and laminar model. The results are presented in Table 7.
Model (wall
function)
Rhs Error
(%)
ΔP Error
(%)
Iterations
to
converge
Low Re (low y+) 1.13875 10.69% 41.57 22.03% 120
Low Re (all y+) 1.13889 10.70% 41.56 22.06% 120
Laminar (none) 1.13986 10.80% 41.54 22.10% 140
V2F (low y+) 1.13875 10.69% 41.60 21.98% 200
V2F ( all y+) 1.13375 10.20% 41.71 21.78% 200
Table 7: Results obtainedfrom three different models; Low Re, V2F
andLaminar. Forthe LowRe andV2F the wall treatment was variedbetween
low y+ and all y+.
Note in Table 7, Convergence was determined as the
number of iterations for all plots to stabilise i.e. Thermal
Resistance, Pressure Drop and Residuals.
Each model, and associated wall function option, was
run for 100 iterations and a solver iteration time elapsed
monitor was generated. This was then exported to excel,
where an average time was obtained. This average time
was then normalised about the laminar model, as it was
the shortest, to gauge the comparison of the models in
terms of iteration time. Table 8 presents the results.
Low Re
(Low y+)
Low Re
(all y+)
Laminar V2F
(Low y+)
V2f
(All y+)
1.19 1.35 1.00 1.31 1.46
Table 8: Iterationtime elapsed(seconds) normalisedby the laminar iteration
time elapsed (1.375s) for each simulation conducted.
Multiply the normalised iteration time by the number of
iterations to convergence, yields a time scale for
comparison between the simulations. Table 9 presents
the results:
Low Re
(Low y+)
Low Re
(all y+)
Laminar V2F
(Low y+)
V2f
(All y+)
142.8sec 162sec 140sec 262sec 292sec
Table 9: Number of iterations multiplied by the normalised iteration time
(sec).
The boundary layer was visualised between the fins
through use of a section plane. Figure 5 and 6 present
the scalar planes for the Low Re model for low y+ and
high y+. These plots were generated for each simulation,
and the rest are available in Appendix B.

Figure 5: Standard Low Reynold’s Number, all y+. Scalar plot of a plane
section cut through the flowdomain. Y direction coming out of page and Z
direction is from bottom to top.
Figure 6: Standard Low Reynold’s Number, low y+. Scalar plot of a
plane sectioncut through the flow domain. Y direction coming out of page
and Z direction is from bottom to top.
XI. DISCUSSION
Firstly, considering the heat sink thermal resistance
computed from each simulation in Table 7 and rounding
up to two decimal places, each model computes the
same value of 1.14 K/W. This is around 11% error from
theory. Next, considering the pressure drop through the
heat sink, each model is computing a value of 41.6 Pa,
plus or minus 0.1 Pa, corresponding to around 22% error
with theory. The percentage errors may arise from the
fact that the theory used is an idealisation and does not
consider as much variables in the flow field as the
computational model. Regardless, the correlation is
adequate and the validity of the model is sound.
Considering the time per iteration, it would be expected
that the quickest would be laminar (as it solves 5
equations), then the standard low Reynold’s number
model (as it solves the same 5 equations as the laminar
plus 2 more), and finally the V2F model (as it solves the
same 7 equations as the low re model plus an additional
2). The Laminar simulation solves the 4 transport
equations, being continuity and x, y, & z momentum.
The standard Low Reynold’s model solves these in
addition to the turbulence dissipation rate and the
turbulent kinetic energy. Finally the V2F model solves
the stated in addition to an elliptical function f, which is
a redistributed term used to solve the last variable
required, 𝑣′2
. Analysing Table 7, it is clear that this
trend is satisfied, except however that the V2F (low y+)
simulation had a quicker iteration time that the Low Re
(all y+). Considering this, and the fact that the low y+
was quicker for both simulations than the associated all
y+ for the same model, displays the additional
computational requirement needed to use the ‘hybrid’
wall function. The all y+ attempts to merge the low y+
and high y+ wall treatment. It should be noted that the
all y+ is designed for a more coarse mesh, with a y+
value ranging from 5-30. If used in this range, the
computation time may have been reduced to lower than
the corresponding low y+ values, at the potential
expense of accuracy.
Table 9 presents the normalised iteration time as a
product of the number of iterations to convergence.
These figures enable the comparison of the computation
time for each simulation. The shortest convergence time
being laminar, following to Low Re (low y+ first and all
y+ after), and finally the V2F model (low y+ first and all
y+ after). Recalling the proximity of the variables of
interest (thermal resistance and pressure drop), the most
efficient model is the laminar. The accuracy of the
laminar model may loan itself to the fact that the flow is
laminar between the heat sink channels, which is the
area of interest. Therefore, the model is capable of
competing with the more complex turbulence models.
For the purpose of this heat transfer problem, the

laminar model or Low Reynold’s models provide a
sufficient solution in the shortest time.
Analysing Figure 5 and 6, the scalar plot of a plane
section cut through the flow domain, it can be seen that
the development of the hydrodynamic and thermal
boundary layer of both the all y+ and low y+ are in
agreeance. Studying the fins leading edge in both plots
(Z direction runs from bottom to top), the all y+
simulation displays a higher reduced velocity than the
low y+, while at the trailing edge the low y+ model
illustrates a larger wake than the all y+. Considering the
V2F scalar plots, Appendix B, the same trend is evident
for the V2F simulations. In comparison to these
simulations, the laminar scalar plot, Appendix B,
experiences a leading edge reduced velocity analogous
to the low y+ simulations and has the smallest wake at
the trailing edge. All in all, the scalar plots of all the
simulations are near identical.
XII. CONCLUSION
The most significant conclusion that can be drawn from
the analysis is that each model used correlates, with
nearly the same proximity, with theory. Further from
this;
 The laminar model provided the quickest
solution, in terms of time per iteration and
iterations to convergence, when compared to the
Low Re and V2F models.
 For both the Standard Low Reynold’s model
and the V2F model, the low y+ option reached
convergence quicker than the corresponding all
y+. This was determined to be an effect of the all
y+ wall treatment attempting to emulate both
the low y+ and high y+ wall functions.
 Despite the fact that the V2F model solves 9
equations and the Low Reynold’s number 7, the
low y+ V2F simulation had a quicker time per
iteration than the high y+ Low Re model.
However, the high y+ simulation reached
convergence quicker.
 Analysing the scalar plot of a plane section cut
through the flow domain, it was seen that
o All simulations agreed upon the
development of the hydrodynamic and
thermal boundary layer.
o The all y+ simulations generated a
higher reduced velocity at the leading
edge than the low y+ model, while the
low y+ model generated a larger wake
at the trailing edge than the all y+
model.
o The laminar plot displayed a leading
edge velocity analogous to the low y+
simulations and a lower wake than all
simulations.
It is evident from the conduction and analysing of the
simulations, that for a conduction-convection conjugate
heat transfer problem of a plate-fin heat sink under the
given flow conditions, the laminar model is just as
adequate at achieving a thermal resistance and pressure
drop value than the other turbulence models.
APPENDIX
A. Appendix A
The Reynold’s number is a ratio of inertial forces to
viscous forces used to categorise a flow into three
regimes. The Reynolds number is given by:
𝑅𝑒 𝐷ℎ
=
𝜌𝑢𝐷ℎ
𝜇
(Eqn. 13)
Where ρ= density of fluid (kg/m3), μ=dynamic viscosity
(Pa-s), u=fluid velocity (m/s), and finally Dh=hydraulic
diameter, which is a diameter measure defined to
correlate the flow in a non-circular duct to that of a
circular duct, and is given by:
𝐷ℎ =
4𝐴
𝑃
(Eqn. 14)
Where A=Cross sectional area (m2) and P=wetted
perimeter (m).
The Nusselt number is defined as the ratio of convection
heat transfer to fluid conduction heat transfer. This
dimensionless parameter is dependent on the flow
regime. It should be noted that when the flow constricts
to the heat sink channels, the fluid will have to
redevelop and entrance length effects may not be
omitted. Therefore it is appropriate to use a Nusselt
number correlation that accounts for both developing
and developed flow. The correlation proposed by
Teertstra et. al. (1999) factors both criteria and is given
by:
𝑁𝑢 𝑖 =
[
1
(
𝑅𝑒
𝑏
∗ 𝑃𝑟
2
)3
+
1
(0.644√𝑅𝑒 𝑏
∗
𝑃𝑟1/3
√
1+
3.65
√𝑅𝑒
𝑏
∗
)
3
]
−1/3
(Eqn. 15)
Where Nui=Ideal Nusselt Number (η=1), Pr=Prandtl
Number and Reb* is defined as a modified Reynolds
number and is aimed to combine the channel width,
length and Reynolds number, otherwise known as
Elenbass Rayleigh number for natural convection:

𝑅𝑒 𝑏
∗
= 𝑅𝑒 𝑏 .
𝑏
𝐿
(Eqn. 16)
The convective heat transfer coefficient can be related to
the ideal Nusselt Number by:
ℎ = 𝑁𝑢 𝑖 .
𝑘 𝑓
𝑏
(Eqn. 17)
where kf is the thermal conductivity of the fluid, and b is
the channel width.
The heat sink thermal resistance, Rhs (K/W) i.e. the
resistance of the heat sink to, under the given flow
conditions, the flow of heat and is given by:
𝑅ℎ𝑠 =
1
ℎ .(𝐴 𝑏𝑎𝑠𝑒+𝑁 𝑓𝑖𝑛 𝜂 𝑓𝑖𝑛 𝐴 𝑓𝑖𝑛)
(Eqn. 18)
Abase is the exposed area of the base (between the fins),
Nfin is the number of fins, ηfin is the fin efficiency, and
Afin is the surface area per fin taking into account both
sides of the fin.
The fin efficiency, ηfin, is given by:
𝜂 =
tanh(𝑚𝐻)
𝑚𝐻
(Eqn. 19)
Where H is the height of the fins, and m is defined as:
𝑚 = √
ℎ𝑃
𝑘𝐴 𝑐
(Eqn. 20)
Where P is the perimeter (P=2t+2L), h is the heat transfer
coefficient, k is the thermal conductivity of the fins, and
Ac is the cross sectional channel area of the fins (Ac=tL).
It may be noted that the relationship for Nusselt number
(Eqn. 3) includes the effect of the temperature rise in the
air as it flows through the fin passages. To obtain the
total thermal resistance, Rtot, to the base of the heat sink
it is necessary to add in the thermal conduction
resistance across the base of the heat sink. For uniform
heat flow into the base Rtot is given by:
𝑅𝑡𝑜𝑡 = 𝑅ℎ𝑠 +
𝐻−𝐻 𝑓
𝑘 𝑏𝑎𝑠𝑒 .𝑤.𝐿
(Eqn. 21)
The pressure drop, ΔP (Pa), across the heat sink is given
by:
Δ𝑃 = ( 𝐾𝑐 + 4. 𝑓𝑎𝑝𝑝 .
𝐿
𝐷ℎ
+ 𝐾𝑒) . 𝜌.
𝑉2
2
(Eqn. 22)
Where Kc and Ke are coefficients that represent the
pressure losses due to sudden contraction channels and
expansion of the flow entering and leaving the heat sink
respectively. These coefficients are given by:
𝐾𝑐 = 0.42(1 − 𝜎2) (Eqn. 23)
𝐾𝑒 = (1 − 𝜎2
)2
(Eqn. 24)
Where σ is the ratio of the area of the flow channels to
that of the flow approaching the heat sink.
fapp is the apparent friction factor, that takes into account
the developing and developed regions of the flow in the
heat sink channels. It is defined as:
𝑓𝑎𝑝𝑝 =
[(
3.44
√𝐿∗
)
2
+( 𝑓.𝑅𝑒 𝐷ℎ
)
2
]1/2
𝑅𝑒 𝐷ℎ
(Eqn. 25)
Where L* is a dimensionless length defined as:
𝐿∗
=
𝐿/𝐷ℎ
𝑅𝑒 𝐷ℎ
(Eqn. 26)
The Poiseuille number is given by:
𝑓. 𝑅𝑒 𝐷ℎ
= 24 − 32.527𝜀 + 46.721𝜀2
− 40.829𝜀3
+
22.954𝜀4
− 6.089𝜀5
(Eqn. 27)
Where ε is defined as the fin aspect ratio:
𝜀 =
𝑏
ℎ
(Eqn. 28)
Where b is the channel width, and h is the channel
height (fin height).
B. Appendix B
Figure B1: Laminar.Scalar plot of a plane section cut through the flow
domain. Y direction comingout ofpage andZ directionis frombottomtotop.

Figure B2: V2F LowReynold’s Number, all y+. Scalar plot of a plane
Figure B3: V2F LowReynold’s Number, lowy+. Scalar plot ofa plane
NOMENCLATURE
ρ Density Kg/m3
Pressure drop Pa-s
Volume Flow rate m3/s
heat flux W/m2
A Area
Cp Specific heat capacity J/Kg-K
D Diameter m
h heat transfer coefficient
H Height m
k Thermal conductivity W/m-K
K contraction/expansion
coefficnet
-
N number -
Pr Prandtl number -
q heat load W
R Thermal Resistance K/W
Re Reynold's number -
v velocity m/s
α Thermal expansion
coefficient
/K
η fin efficiency -
μ Dynamic viscosity Pa-s
Subscripts
hs heatsink
ch channel
tot total
f fins
base base
c contraction
app apparent
e expansion
h hydraulic

XIII. REFERENCES
[1] Culham, J.R., and Muzychka,Y.S. “Optimizationof Plate FinHeat
Sinks Using Entropy Generation Minimization,” IEEE Trans.
Components and Packaging Technologies, Vol. 24, No. 2,pp.159-
165, 2001.
[2] Dorfman, A. (2010) Conjugate Problems In Convective Heat
Transfer, CRC Press: Boca Raton.
[3] Lee, H. (2010) Thermal Design, Wiley: Hoboken, N.J.
[4] Simons, R.E., “Estimating Parallel Plate-Fin Heat Sink Thermal
Resistance,” ElectronicsCooling, Vol. 9, No. 1, pp. 8-9, 2003.
[5] Simons, R.E., and Schmidt, R.R., “A Simple Method to Estimate
Heat Sink Air Flow Bypass,”ElectronicsCooling, Vol. 3, No. 2, pp.
36-37, 1997.
[6] Teertstra, P., Yovanovich, M.M., and Culham, J.R., “Analytical
Forced Convection Modeling of Plate Fin Heat Sinks,”
Proceedings of 15th IEEE Semi-Therm Symposium, pp. 34-41,
1999.
[7] Wendt, J., Anderson, J. (2009) Computational Fluid Dynamics,
Springer: Berlin.
[8] Griffin, P. (2016) Advanced Computational Fluid Dynamics.

Jamie Fogarty CFD FINAL DRAFT PRINT

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to Jamie Fogarty CFD FINAL DRAFT PRINT

Similar to Jamie Fogarty CFD FINAL DRAFT PRINT (20)

Jamie Fogarty CFD FINAL DRAFT PRINT