Natural convection heat transfer flow visualization of perforated fin arrays by cfd simulation

IJRET: International Journal of Research in Engineering and Technology eISSN: 2319-1163 | pISSN: 2321-7308
__________________________________________________________________________________________
Volume: 02 Issue: 12 | Dec-2013, Available @ http://www.ijret.org 483
NATURAL CONVECTION HEAT TRANSFER FLOW VISUALIZATION
OF PERFORATED FIN ARRAYS BY CFD SIMULATION
Dhanawade Hanamant S1
, K. N. Vijaykumar2
, Dhanawade Kavita3
1
Professor, Smt. Indira Gandhi College of Engineering, Navi Mumbai, Maharashtra, India
(Research Scholar JJT University), dhanashri_hd@rediffmail.com
2
Professor and Head of Dept. of Mechanical Engineering, D. J Sanghvi College of Engineering, Mumbai, Maharashtra,
India, kotturvijaykumar@gmail.com
3
Assistant Prof. Department of Mechanical Engineering, Lokmanya Tilak College of Engineering, Navi Mumbai,
Maharashtra, India, nikhil_kd@rediffmail.com
Abstract
The present paper reports, the validation of results of modeling and simulation in CFD by experiment on the fluid flow and heat
transfer characteristics of a fin arrays with lateral circular perforation and its external dimensionally equivalent solid fin arrays
equipped on horizontal flat surface a problem of natural convection. The simulation is carried out using the fluid flow (CFX)
workbench of ANSYS 12.0. In this study, results shows that formation of the stagnant layer around the solid fin array which slow-
downs the heat dissipation rate. Increase in the fluid flow movement around the fin results increase in the heat dissipation rate. It can
be achieved by adding perforation to the fins. Natural convection is a buoyancy driven phenomenon; the state of the art of CFX was
used to carry the study of fluid flow separation and velocity field over a fin array. New designed perforated fins have an improvement
in average Nusselt number, over its external dimensionally equivalent solid fin arrays.
Keywords: CFD simulation, perforated fins, Natural convection, Heat sink, Nusselt number, Flow Visualization
----------------------------------------------------------------------***------------------------------------------------------------------------
1. INTRODUCTION
The enhancement of heat transfer is an important subject of
thermal engineering. Removal of excessive heat from system
components is essential to avoid the damaging effects of
burning or overheating. Basically flow is nothing but
circulation of the air around the heated fins surface which
occurs due to the change in density of air after getting heated
when it comes in contact with heated fin. Thus cold air gets
sucked inside from the bottom and heated air goes up causing
the natural convection currents. Mainly three types of the flow
pattern are mentioned in the literature.
i) Single chimney flow pattern: Fig.1 a) this pattern is
observed in lengthwise short arrays. It is formed by the cold
air entering from the two ends of the arrays, traveling
lengthwise and coalescing at the center of the arrays. This
flow pattern is the most favorable from the heat transfer
standpoint.
ii) Sliding Chimney Flow Pattern: Fig. 1 b) as the length of the
arrays is increased keeping the height and spacing unaltered.,
it is observed that beyond a certain value of the length, the air
entering from the ends is not sufficient to cool the entire arrays
and leaves the array before reaching the central zone, and the
resulting flow pattern is sliding chimney flow pattern, which is
unsteady in nature.
a) Single chimney flow pattern
b) Sliding chimney

__________________________________________________________________________________________
c) Down and up
Fig-1: Types of Flow Patterns
iii) Down and Up Flow Pattern: Fig1 c) if the length of the
array is further increased so that the array can be considered
infinite in the longitudinal direction, the resulting flow pattern
has cold air entering at the central portion of the array, turning
through 180o
, developing boundary layers along the height of
the fin flats and leaving the array in the upward direction.
It has been reported that the cross component of velocity
(along the direction of the spacing) is negligible in single
chimney flow pattern. The down and up flow pattern are
mostly hypothetical situation and hence has little practical
significance.
Abdullah H. AIEssa et al. [1-2] studied the heat dissipation
from a horizontal rectangular fin embedded with square
perforation, rectangular perforations with an aspect ratio of
two, equilateral triangular perforations of bases parallel and
towards its fin tip, by using the finite element technique under
natural convection. They compared the results of the
perforated fin with its external dimensionally equivalent solid
fin. They showed that perforation in the fins enhances heat
dissipation rates and at the same time decreases the
expenditure for the fin material. Sanjeev D. Suryawanshi and
Narayan K. Sane [3] investigated experimentally the heat
dissipation from a fin array with an inverted notch at the
central bottom portion of the fin to modify its geometry for the
enhancement of heat transfer on normal and inverted notched
fin arrays. Also they observed the single chimney flow pattern
for INFAs. C. B. Sobhan [4] on free convection heat transfer
from fins and fin arrays attached to a heated horizontal base by
applying the differential interferometry technique. They have
calculated the heat transfer coefficient, Nusselt number,
considering the fin spacing and the thermal conductivity as
parameters. The correlations are presented concerning the
overall Nusselt number with the relevant parameters. The
optimum fin spacing depends on the thermal conductivity of
the material. They observed the different flow patterns by
using the interfometry technique. Suneeta Sane et.al [5] has
performed the studies on the rectangular notched fin arrays;
they observed that total heat flux and the heat transfer
coefficient increase as the notch depth increases. The area
removed due to notch is compensated by the air entry at the
ends of the fin it provides fresh cold air to bring in contact
with hot fin surfaces. They also carried the flow visualization
of the fluid flow around the fin by using the simple smoke
technique using the Dhoop stick. They found that the cold air
is sucked inside from the bottom of the fin and leaving from
the central portion of the fin forming the single chimney
pattern. Vinod M. Wankar S.G. Taji [6] in their experimental
investigation of flow pattern on rectangular fin arrays under
natural convection carried the flow visualization studies by
simple smoke technique using the Dhoop stick on the
rectangular fin arrays of varying the fin spacing they obtained
for 2mm, 4mm, 6mm fin spacing, the scattered flow pattern.
While for 12mm fin spacing they observed the single chimney
flow pattern which gives the higher heat transfer coefficient.
The present paper reports, CFD modeling and simulation
using ANSYS 12.0 in the workbench of fluid flow (CFX), of
the fluid flow and heat transfer characteristics of a rectangular
fin arrays equipped with circular perforation on a horizontal
flat surface and its external dimensionally equivalent solid fin
arrays. The studies were carried by varying the diameter (8mm
and 12mm) of circular perforations and heat inputs. Geometric
dimensions of the perforated fin arrays and its external
dimensionally equivalent non perforated fin arrays were same
and those were H=65mm, L=100mm, S=30mm. The
simulation results are validated by experimentation by taking
repeated steady state readings.
2. EXPERIMENTAL SETUP
The main requirement of the natural convection heat transfer
experiment is controlled environmental conditions. The
experiment must be away from fans and flow of outside air.
Hence to provide natural convection conditions, the
experiment were conducted in a room where the fan was off
and windows were closed so that readings should not affect by
the outside atmosphere and to provide similar atmospheric
conditions for all experiments.
Fig-2: Photograph of the experimental setup

__________________________________________________________________________________________
Initially the supply voltage was set to 230V on the stabilizer.
The dimmer-stat was adjusted to get the desired input to the
electric heater which multiple of voltage and current. A total
of 16 Copper constantan k type thermocouple junctions (Fig.2)
were fixed on different points of the fin arrays, on and beneath
of the base plate and in the insulating bricks at some distance,
this was done to note the temperature at various points of the
fin arrays as well as to find out various heat losses to the
surrounding. One thermocouple was suspended to measure the
surrounding temperature. The calibrated digital temperature
indicator having 0o
C to 600o
C range was used to measure the
temperature. The heating was continued till the steady state is
reached; it took 4 to 5 hours to reach steady state. Only one set
of reading very carefully taken on one day, after achieving the
steady state all the 16 temperature readings were noted. This
procedure was repeated for all heater inputs of 40, 60, 80 and
100 Watt. Observations were repeated to confirm the validity
and the readings obtained were found to be similar.
3. DATA PROCESSING
Net heat transfer can be calculated as
QN = ha ACΔT (1)
Where,
QN = QInput – QCond (2)
To find heat loss by conduction (heat loss through the base)
thermocouples were inserted through insulating bricks up to
distance dxb from the base plate.
b
b
Cond
dx
TAk
Q bb 
 (3)
Similarly, conduction loss through sides of base plate is also
calculated by noting the temperature of side of the base plate.
Average convective heat transfer coefficient,
 as TTAc
NQ
ha

 (4)
Nusselt number,
k
Hah
Nu  (5)
Rayleigh Number is given by


k
HTCg
Ra P
32
)(
 (6)
Where, β =
1
Tm
and Tm= (Ts+Ta)/2
Properties of air were taken from the standard table of air
properties at mean Temperature Tm.
4. CFD MODELING AND SIMULATION
The CFD modeling, simulation and post processing are carried
out in an ANSYS 12.0, Workbench environment with an
ANSYS system of fluid flow (CFX) [7]. It has the capability
of solving the convective transport of energy by fluid flow
along with the conjugate heat transfer (CHT) capability to
solve the thermal conduction in solids.
In the any CFD simulation, the steps in performing fluid
analysis are
1) Create or import a geometry
2) Create a mesh
3) Set up the analysis that will be sent to the solver
4) Control and monitor the solver to achieve a solution
5) Visualize the results in a post-processor and create a report.
These steps are briefed below.
4.1. Create a Geometry
Geometry was created using ANSYS Design Modeler
software which is specifically designed for the creation and
preparation of a geometry for simulation. A domain has to be
built around the fin to study mass flow and thus the heat flow
from the fin, because the area of interest is the outside of fin,
which is the interface between the air and fin surface. Thus,
connections are required between the solid fin surface and the
fluid domain consisting of air.
Fig-3: Domains Fluid and Solid and boundary conditions
applied, the12mm perforated fin array

__________________________________________________________________________________________
Initially the domain of fin including base was created and
required domain of fluid of size 172x140x130mm (Fig.3)
created with the help of the „Enclosure‟ option around the fin.
The setup was modeled with full geometry so that maximum
physics of experimental analysis can be included. Hence it is
logical to assume that the behavior of the created system
domains is similar to the behavior of the experimental system.
4.2 Create a Mesh for the Geometry
The standard volume Mesher in a CFX-Mesh is the Advancing
Front Volume Mesher. It enables an automatic tetrahedral
mesh generation using efficient mesh generation techniques,
meshes were created with high contact sizing relevance (dense
meshing near the fin surface), inflation growth rate 1.2 and
total number of tetrahedral elements between 3.0 to 3.5
million.
4.3 Setup the Analysis that will be sent to the Solver
Under the set up of CFX of the ANSYS Workbench, selected
Analysis type „Steady State‟. The appropriate boundary
conditions were applied to the domains (refer Fig. 3).
Materials Aluminum and Air were assigned to the created
solid and fluid domain respectively. The interface between
solid fin surface and fluid was created by using the option
„Domain Interface‟, having chosen „Fluid Solid‟ interface
under the basic settings. Activated buoyancy in Y direction,
chosen Turbulence model as Laminar.
Through the use of the boundary condition of „opening‟ to all
sides of the enclosure faces except the bottom face (set to
adiabatic) the size of the fluid domain can be reduced to a
great extent and it can be assumed to be as the atmospheric
conditions. Under fluid domain a layer adjacent to the bottom
face of fin base was set to adiabatic. Under the domain fin and
base, bottom surface of a base of the fin, set the boundary
condition to „Heat Flux‟. The heat flux was applied equal to
the QN/Ab of the experimental readings. Other vertical sides of
base plate set to boundary condition as adiabatic.
4.4 Control and Monitor the Solver to Achieve a
Solution (Convergence)
The most important measure of convergence is the residual.
The CFX-Solver will terminate the run when the equation
residuals (Root Mean Square (RMS) type of residual)
calculated are below the residual target value. The target was
set to 1.0x10-6
. It was observed that most solutions were
getting converged between 240 to 270 iterations. In a few
cases, residuals of the energy equations remain constant (about
4.8x10-6
). Hence, to optimize the computational time the
maximum number of iterations was set to 300. It took 8 to12
hours to get solutions converged.
4.5 Visualizing the Results in a Post-Processor and
Creating a Report.
When the solver was terminated, the results were examined
which is the post processing step. Temperature distribution
and heat flux along the fin surface as well as parameters like
Nusselt Number, heat transfer coefficient, Rayleigh number
and changes in other parameters can also be predicted by
computational analysis. Fig.4 and Fig.5 shows the temperature
contours over the convective surface area of the non
perforated and perforated fin arrays respectively. It can be
seen that the perforated fin arrays are pumping out the more
heat from the base, as the average fin temperatures are higher
than that of the equivalent solid fin array. The end fins and top
ends of the all fins are cooled faster.
Fig-4: Contours of Temperature Solid Fin array 80W input
Fig-5: Contours of Temperature perforated Fin array 80W
input

__________________________________________________________________________________________
5. FLOW VISUALIZATION
The Fig.6 shows the velocity vectors of the solid fin array at
80 watt heat input. The air has only chance to come in from
the ends of the fin as seen in the interspacing of the fin. The
air entering from the ends is not sufficient to cool the entire
arrays and leaves the array before reaching the central zone,
hence the resulting sliding chimney flow pattern. From the
Fig.7 and Fig.8 it is observed that air is sucked from the ends
of the fin as well as from the sides through the perforation and
goes up through the central portion of fin array.
Fig-6: Vectors of velocity on XY plane at Z=0.02m solid fin
array
Fig-7: Vectors of velocity on XY plane at Z=0.02m
12mm perforated fin array
Fig-8: Vectors of velocity on YZ plane at X=0.06m 12mm
perforated fin array
Fig-9: Contours of temperature on XY plane at Z=0.04m solid
fin array
Fig-10: Contours of temperature on XY plane at Z=0.04m

__________________________________________________________________________________________
Fig-11: Contours of temperature on YZ plane at X=0.103m
Showing the single chimney flow pattern, the space between
middle fins showing the negligible down flow but it is better
than solid fin arrays. Yet there is scope to improve the flow
pattern by increasing the size of the perforation. Fig.9 shows
the contours of the temperature around the solid fin, it clearly
shows the formation of the stagnant hot layer. It is eased by
adding the perforation to the fins as it is seen from Fig.10 the
contours of temperature in the fluid domain of the 12mm
perforated fin. Similarly Fig.11 shows the contours of the
temperature 12mm perforated fin array clipped on the YZ
plane at X=0.103m all contour and velocity vectors are
clipped to local range correspond to 80W heat input. The
Fig.12 shows the streamlines of velocity in fluid domain of
12mm perforated fin array. The air entering in the fluid
domain from the bottom sides of the fluid domain which
comes in contact with the heated fin surface then passes
through perforation resulting in an upward flow of air by
natural convection.
Fig-12: Streamlines of flow velocity of 12mm perforated fin
array at 80W heat input
The attempt was made to visualize the flow pattern of the
perforated fin array with simple smoke technique by using the
Dhoop sticks. It was observed that the flow pattern obtained
was a single chimney at the height above the fin, and slight
curling of the smoke at the edge of perforation.
6. GRID INDEPENDENCY AND VALIDATION OF
RESULTS
A Grid independency test was carried out by varying the
number of elements from 2.8 million to 3.5 million. It was
observed that, a very minute variation (< 1o
c) in various output
temperatures and < 3w/m2
in conserved heat flux values
existed. Even though, as time was not a constraint and for
accurate results the total number of tetrahedral elements in a
grid were chosen to be approximately 3.0 to 3.5 million.
Comparison among the CFD simulation results and
experimental values of various temperatures, heat transfer
coefficient and Ra and Nu with a maximum variation of 7.5%
was observed. The uncertainty analysis was carried it was
found that uncertainty remains below ±5%, during the
experimentation.
7. RESULTS AND DISCUSSION
Experimental analysis and CFD simulation of performance
characteristics of the perforated fin arrays with 12mm
perforation and its external dimensionally equivalent solid fin
arrays is presented.
From the presented Figs.4, 8 and 9 vectors of velocity and
temperature zones around the solid fin array clears that, the air
coming inwards from the bottom, gets heated as it moves

__________________________________________________________________________________________
towards the centre of the fin, rises up due to a decrease in
density, the central portion of the fin becomes ineffective
because the hot airstream passes over that part and therefore it
does not bring about large heat transfer through that portion.
When perforation is added, Figs.7, 8, 10, 11 and 12, vectors of
velocity, temperature zones and streamlines of velocity around
the perforated fin revels that the area removed by the
perforation from the fin is compensated by the entry of more
fresh cold air through the perforation and also from the ends of
the fin resulting in the enhancement of the heat transfer.
Fig- 13: Performance in Nu Vs Ra of 12 mm Perforated and
corresponding external dimensionally equivalent solid fin
arrays CFD and Experimental analysis
Fig.13 shows the performance of Nu against Rayleigh number
(Ra) at the same heat input the Nu of the perforated fin array is
higher than the Nu of the solid fin array of the experiment as
well as of the simulation and heat dissipation rate increases
with an increase in the size of the perforation.
8. CONCLUSION
The experimental analysis as well as the CFD simulation on a
solid and a perforated fin array is carried out. The
enhancement in the heat dissipation rate due to the perforation
is noted and heat dissipation rate increases with an increase in
the size of the perforation because of more free convection
due to the perforation. The flow pattern observed in case of
solid fin array was more or less in a sliding chimney in nature
and that of the perforated fin array was of single chimney in
nature, a significance of enhanced heat dissipation rate due to
perforation.
REFERENCES
[1]. Abdullah H. AIEssa and Fayez M.S. Al-Hussien, 2004.
The effect of orientation of square perforations on the
heat transfer enhancement from a fin subjected to natural
convection. Springer-Verlag, Heat and Mass Transfer,
40, pp. 509-515.
[2]. Abdullah H. AIEssa and Mohmmed I. Al-Widyan, 2008.
Enhancement of natural convection heat transfer from a
fin by triangular perforations of bases parallel and toward
its tip. Applied Mathematics and Mechanics, Shanghai
University and Springer-Verlag 29 (8), Pp.1033-1044.
[3]. Sanjeev D. Suryawanshi and Narayan K. Sane, 2009.
Natural convection heat transfer from horizontal
rectangular inverted notched fin arrays, ASME, J. Heat
Transfer, 131(8).
[4]. C. B. Sobhan, S.P. Venkateshan and K. N. Seetharamu,
(1990),“Experimental studies on steady free convection
heat transfer from fins and fin arrays”, Wärme- and
Stoffübertragung, Springer-Verlag, Vol. 25, pp. 345-352.
[5]. Suneeta Sane, Gajanan Parishwad, Narayan Sane, 2009,
Experimentatal Analysis of Natural Convection Heat
Transfer from Horizontal Rectangular Notched Fin
Arrays, International journal of Heat and Technology,
Vol.27, pp11-16
[6]. Vinod M. Wankar, S.G. Taji, 2012, Experimental
Investigation of Flow Pattern on Rectangular Fin Arrays
under Natural Convection, International Journal of
Modern Engineering Research (IJMER), Vol.2, Issue.6,
pp-4572-4576.
[7]. ANSYS CFX-Solver Modeling Guide, April 2009,
Release 12.0 ANSYS, Inc. Southpoint.
BIOGRAPHIES
Dhanawade Hanamant S. is Professor in Smt.
Indira Gandhi College of Engineering, Navi
Mumbai and Research scholar of JJT
University, Rajasthan, has 24 years of
teaching experience and more than eleven
papers in the national, international
conferences and Journals in his credit. Life member of ISTE
and Associate Member of IIIE
Dr. K. N. Vijaykumar is Professor and Head
of the Department of Mechanical Engineering,
D J. Sanghvi College of Engineering,
Mumbai, has 24 years of teaching experience
and more than 21 papers in the national and
international conferences and Journals in his
credit. Life member of ISTE and Associate Member of IIIE
Dhanawade Kavita H. is Assistant
Professor in the Department of Mechanical
Engineering, Lokmanya Tilak College of
Engineering, Navi Mumbai, Sixteen years
of teaching experience and she has in credit
more than 12 papers in the national and
international conferences and journals, She is the life member
of the ISTE.
28
33
38
43
48
11 16 21
Nu
Ra x 100000
12PR CFD
12PR EXP
PL CFD
PL EXP

__________________________________________________________________________________________
NOMENCLATURE
Ab Surface area of bottom of the base, m2
Ac Convective heat transfer area, m2
CP Specific heat capacity at constant pressure, Ws/kgK
dxb Distance of thermocouple from base plate in the
brick, mm
g Gravity, m/s2
H Fin height, mm
ha Average heat transfer coefficient, W/m2
K
k Thermal conductivity of air, W/mK
kb Thermal conductivity of insulating brick, W/mK
L Length of fin, m
Nu Nusselt number, dimensionless
Ta Ambient temperature, K
Tm Mean temperature, K
Ts Average surface temperature of a fin, K
ΔT Difference of average surface temperature and
ambient temperature, K
ΔTb Difference of temperatures at bottom of the fin and
temperature in a brick at dxb distance,K
QCond Heat loss by conduction, W
QInput Electrical heat input, W
QN Heat transfer by Convection, W
Ra Rayleigh number, dimensionless
S Fin spacing, mm
Greek Symbols
β Coefficient of thermal expansion of air, 1/K
ε Emissivity
ρ Density of air, kg/m3
µ Viscosity of air, kg/ ms

Natural convection heat transfer flow visualization of perforated fin arrays by cfd simulation

More Related Content

Similar to Natural convection heat transfer flow visualization of perforated fin arrays by cfd simulation (20)

More from eSAT Journals (20)

Recently uploaded (20)

Natural convection heat transfer flow visualization of perforated fin arrays by cfd simulation