Jurnal Pemodelan Matematika menggunakan CFD

1. CFD modeling of heat transfer and fluid flow inside a pent-roof type combustion
chamber using dynamic model☆
Yasin Varol a,
⁎, Hakan F. Oztop a,1
, Mujdat Firat a
, Ahmet Koca b
a
Department of Mechanical Education, Firat University, 23119 Elazig, Turkey
b
Technical Vocational School, Firat University, 23119 Elazig, Turkey
a b s t r a c ta r t i c l e i n f o
Available online 9 August 2010
Keywords:
Internal combustion engine
CFD
Heat transfer
Combustion chamber
A numerical work has been performed to analyze the heat transfer and fluid flow in a pent-roof type
combustion chamber. Dynamic mesh model was used to simulation piston intake stroke. Revolution of
piston (1000≤n≤5000) is the main governing parameter on heat and fluid flow. k–ε turbulence model was
used to predict the flow in the cylinder of a non-compressing fluid. They were solved with finite volume
method and FLUENT 12.0 commercial code. Velocity profiles, temperature distribution, pressure
distribution and velocity vectors are presented. It is found that the inclined surface of pent-roof type of
combustion chamber reduces the swirl effect and it can be a control parameter for heat and fluid flow.
© 2010 Elsevier Ltd. All rights reserved.
1. Introduction
Fluid flow, heat transfer and combustion in an internal combustion
engine are one of the important problems in thermofluid mechanics.
In recent years, Computational Fluid Dynamics (CFD) techniques are
used due to developing of numerical techniques and computer
capabilities. The CFD is an indispensable tool for engine development
with the increasing of computer capabilities. As well known that the
fluid motion inside a cylinder is turbulent, unsteady, cyclic and non-
stationary both spatially and temporally [1]. The fluid motion and heat
transfer inside the cylinder of an internal combustion engine is
strongly related with the performance of the engine efficiency. This
phenomenon is addressed by different researches as given in Ref.
[2,3].
There are two types of internal combustion engine; one is spark
ignition (SI) engines, where the fuel is ignited by a spark, the other is
compression ignition (CI) engines, where the rise in temperature and
pressure during compression is sufficient to cause spontaneous
ignition of the fuel. Analysis of flow and heat transfer in-cylinder is
performed with two different methods as CFD and visualization using
LDV [4], PIV etc. [5,6]. However, there have been numerous
computational techniques on this. In this field, there are many
computational commercial (FLUENT, KIVA, VECTICS, STAR-CD and so
on) or personal codes using finite volume [7], finite element methods
[8] C++ or FORTRAN. In this context, Akar [9] studied the flow
characteristics of some engine models in two-dimensional, three-
dimensional and dynamic model using FLUENT CFD solver. Numerical
models were carried out at various valve gaps for all models. They
showed that the flow structure is highly affected by the valve position
and cylinder length. Payri et al. [10] studied the three-dimensional
flow calculations of the intake and compression stroke of a four-valve
direct-injection Diesel engine with different combustion chamber.
Wu and Perng [11] studied the LES analysis of turbulent flow and heat
transfer in motored engines with different subgrid-scale models. They
tested the flow during the compression–expansion strokes in two
types of engine configuration under realistic engine conditions. As
indicated by Hong and Tarng [12] that the in-cylinder fluid motion is
so complex that it is of non-stationary turbulence. Thus, it is very
difficult to develop a model for turbulence in-cylinder. Moureau and
Angelberger [13] studied the cyclic variability in IC engines using 3D
CFD code. In their work, the Smagorinsky model was used in LES
simulations. Bilgin [14] made a numerical simulation of the cold flow
in an axisymmetric non-compressing engine-like geometry. He
compared the obtained results with the measurements of literature.
Milton et al. [15] investigated the two-phase fuel/air flow through an
internal combustion engine inlet valve both experimentally and
numerically. They indicated that simulation of the process for the gas-
phase flow using the proprietary code, FLUENT gives good agreement
with experiment. More recently, Song et al. [16] analyzed the three-
dimensional flow calculations of the in-cylinder flow for a direct-
injection Diesel engine for different combustion chambers. They
showed that the geometries of the piston have a significant effect on
International Communications in Heat and Mass Transfer 37 (2010) 1366–1375
☆ Communicated by W.J. Minkowycz.
⁎ Corresponding author.
E-mail address: ysnvarol@gmail.com (Y. Varol).
1
Visiting Professor, King Saud University, Department of Mechanical Engineering,
Saudi Arabia.
0735-1933/$ – see front matter © 2010 Elsevier Ltd. All rights reserved.
doi:10.1016/j.icheatmasstransfer.2010.07.003
Contents lists available at ScienceDirect
International Communications in Heat and Mass Transfer
journal homepage: www.elsevier.com/locate/ichmt

2. the distribution of the cross section-averaged swirl ratio. The
tangential velocity profiles at the cross sections are highly nonlinear,
and the rigid body rotation assumption is less admissible. Ceper [17]
studied the combustion and emission performance characteristics of
different percentage ratios of hydrogen–methane gas mixtures
experimentally and numerically. 100% CH4, 10% H2-90% CH4, 20%
H2-80% CH4 and 30% H2-70% CH4 gas mixtures were investigated at
2000 rpm engine speeds and excess air ratios on a model, which is
developed based on real engine diameters used in her numerical
study. In-cylinder pressure and temperature variations were given
based on crank angles. She found that numerical study were found
well-matched with experimental results.
The main purpose of the present study is to investigate the heat
transfer and fluid flow in a pent-roof type combustion chamber and
the effects of the combustion chamber shape on the flow during
intake stroke. The engine studied in this paper is a single-cylinder
spark-ignition gasoline engine with one intake port of the cylinder.
The study shows how flow acts inside of whole intake cycle and it
clarifies some places in which designer should consider some
geometrical innovations.
2. Definition of considered model
Fig. 1 (a) shows three-dimensional model of the combustion
chamber. This is drawn using Solid Works. It is a pent-roof type of
combustion chamber. In this study, flow and heat transfer is modeled
as two-dimensional. Thus, physical model is plotted in Fig. 1 (b) It
consists of real geometries which are used in two-dimensional
studies with their geometric values. Flow domains are created and
the models are meshed in the same code [18] as illustrated in Fig. 1
(c). The engine is simulated a four stroke engine with pent-roof
combustion chamber, and the engine parameters are listed in Table 1.
The piston has flat surface in these figures. As indicated from the
figures that the combustion chamber likes rectangular cavity
depends on piston position except roof of it.
3. Governing equations
Calculation of the temperature and flow field in a combustion
chamber of internal combustion engine requires obtaining the
solution of the governing equations. Compressible, unsteady and
turbulent in-cylinder flow can be described by differential equations
of continuity, momentum, energy, turbulence kinetic energy and its
dissipation rate. Radiation mode of heat transfer is neglected
according to other modes of heat transfer. Buoyancy forces are also
neglected and heat transfer regime is accepted as forced convection.
The mass conservation equation can be written as follows:
∂ρ
∂t
+ ∇⋅ ρVð Þ = 0 ð1Þ
Momentum equations can be written in two directions as:
∂ ρuð Þ
∂t
+
∂ ρu2
∂x
+
∂ ρuvð Þ
∂y
= −
∂p
∂x
+
∂
∂x
λ
∂v
∂x
+
∂u
∂y
V + 2μ
∂u
∂x
+
∂
∂y
μ
∂v
∂x
+
∂u
∂y
ð2Þ
∂ ρvð Þ
∂t
+
∂ ρv
2
∂y
+
∂ ρuvð Þ
∂x
= −
∂p
∂y
+
∂
∂x
μ
∂v
∂x
+
∂u
∂y
+
∂
∂y
λ∇V + 2μ
∂v
∂x
ð3Þ
Energy equation
∂ ρeð Þ
∂t
+ ∇ ρeVð Þ =
∂
∂x
k
∂T
∂x
+
∂
∂y
k
∂T
∂y
ð4Þ
The turbulence kinetic energy, k, and its rate of dissipation, ε, are
obtained from the following transport equations:
ρ
Dk
Dt
=
∂
∂xi
μeff +
μt
σk
∂k
∂xi
+ Gk + Gb−ρε−YM ð5Þ
ρ
De
Dt
=
∂
∂xi
μeff +
μt
σε
∂ε
∂xi
+ Cε1
ε
k
Gk + Cε3Gbð Þ−Cε2ρ
ε2
k
: ð6Þ
There are numerous alternative turbulence modeling approaches of
varying degree of complexity, but in this work, k–ε turbulence model
was used to forecast the flow in the cylinder of an incompressible fluid
[14]. In k–ε model, the turbulent or eddy viscosity concept, and
calculation of turbulent viscosity μt according to Prandtl–Kolmogorov
relation is given as
μt = ρCμ
k
2
ε
ð7Þ
Nomenclature
e internal energy per unit mass, J/kg
Gb the generation of turbulence kinetic energy due to
buoyancy
Gk represents the generation of turbulence kinetic energy
due to the mean velocity gradients
k thermal conductivity, W/mK
n engine speed, rpm
p pressure, Pa
T temperature, K
t time, s
u, v, w velocity magnitudes in direction −x,−y,−z, m/s
V volume, m3
Vc combustion chamber volume, m3
Greek symbols
θ crank angle
turbulent dissipation rate, m2
/s3
μ dynamic viscosity, Pa/s
μt turbulence viscosity
ρ fluid density, kg/m3
σk the turbulent Prandtl numbers for k
σ the turbulent Prandtl numbers for
1367Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

3. C1, C2 and C3 are model constant. These coefficients are,
C1 = 1:44; C2 = 1:92; Cμ = 0:09; μk = 1:0; σ = 1:3
Total effective viscosity of the flow is then, given by the
combination of the turbulent viscosity and laminar viscosity as
μeff = μt + μ ð8Þ
3.1. Boundary conditions
As indicated above that only time dependent intake valve situation
is presented in this work. The inlet boundary conditions were
obtained from the calculated instantaneous mass flow rate. This can
be done due to acceptation of the incompressibility. Also, no-slip
boundary conditions were applied for all velocities at walls. The fluid
velocity at the moving piston surface is equal to the instantaneous
piston velocity. Near wall region is treated by using well known wall
functions, based on the assumption of logarithmic velocity
Fig. 1. a) Solid model from different view, b) Physical models, c) Grid distribution.
1368 Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

4. distribution [19]. Boundary conditions for the considered physical
model (Fig. 1) are given as
Inlet temperature, Tinlet =303 K
Side temperature of combustion chamber, Tside =493 K
Temperature of piston head, Tpiston =493 K
Inlet velocities are V=14, 33 and 54 m/s for n=1000, 3000 and
5000 rpm, respectively.
Velocities at side of cylinder, u=0, v=0
Velocities at piston surface, u=0, v=vpiston
4. Numerical solution
The flow characteristics of engine models are considered as two-
dimensional. Dynamic models were investigated numerically by
means of FLUENT commercial code [18]. It is a well known
Computational Fluid Dynamic program that it is the science of
predicting fluid flow, heat transfer, mass transfer, chemical reactions,
and related phenomena by solving governing equations. This
program uses finite volume method in order to solve Navier-stokes
and energy equations and it is widely used in the field of internal
combustion engine design. The finite volume method can accom-
modate any type of grid. Thus, it is suitable for complex geometries,
like present study. The standard k–ε turbulence model was used as
engine model. The CFD code is based on the pressure-correction and
uses the SIMPLE algorithm of Patankar [20]. The first order upwind
difference scheme (UDS) is used to discretize the momentum, energy
and turbulence equations. The dynamic grid approach is used to treat
the moving piston in the computational area. In other words, the grid
generation approach was used to treat the moving piston as a moving
solid body in the computational domain without generating
completely new grids at each crank angle step [21]. Piston moves
towards to the bottom dead center (BDC). The calculations are
started with a crank angle of top dead center (TDC) and finished at
30° after bottom dead center (aBDC) in the compression stroke
for a different engine speed as 1000, 3000 and 5000 rpm. The model
structure is hybrid grid and to setup boundary condition for moving
piston. Total number of computational cells was used about 50,000 at
BDC and 10,000 cells at TDC. A typical grid distribution is shown in
Fig. 2.
5. Results and discussion
A computational study has been performed in this work for
different crank angles and revolution of pent-roof combustion
Fig. 2. Velocity vectors for different crank angle at n=3000 rpm, a) θ=30°, b) θ=60°, c) θ=90°, d) θ=120°, e) θ=150°, f) θ=180°, g) θ=210°.
Table 1
Engine geometry and parameters.
Bore/mm 82
Stroke/mm 90
Intake valve angle/deg 22
Crank period/deg 720
Engine speed/rpm 1000, 3000 and 5000
1369Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

5. chamber. In this part of the study, the results are present with velocity
vectors, pressure contours, velocity profiles and temperature con-
tours. As indicated above that standard k–ε model was carried out for
all two-dimensional model.
Fig. 2 presents the velocity vectors for different crank angle and
n=3000 rpm. Pent-roof cylinder model sweep out inside of cylinder
better than other models as indicated in literature [9]. There is no
swirl effect in this type. A jet effect is occurred near the valve gap
region due to very small area of this region of internal combustion
engines. Thus, the maximum velocity is formed at this part. For two-
dimensional model, the jet effect is seen at two sides of the valve and
it decreases as valve is getting down. Due to oval shaped of the roof of
combustion chamber, the flow distribution is not symmetric. The flow
generates stronger jet in both sides of the valve. At the beginning of
the intake stroke, the flow produced by the moving piston away from
the chamber head towards bottom dead center impinges to the piston
top surface at lower velocity according to inlet velocity. The flow is
probably laminar. Inlet flow impinges to left and right vertical walls
and two circulation cells were formed in clockwise and counterclock-
wise directions. It is an interesting result that the flow inlets from
right side of the valve become dominant with increasing of crank
angle. And, multiple cells were formed at the top oval shaped region
}
Fig. 2 (continued).
1370 Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

6. for higher crank angle. Impinging flow onto piston moves toward to
valve and again impinges to the valve. This is a characteristic flow
motion of a gas engines. For higher crank angles, the combustion
chamber looks a cavity. Please note that in case of crank angle of 210°,
the piston moves toward to TDC. Fig. 3 display the effects of revolution
for the same crank angle. Revolution number is not an effective
parameter on velocity direction. But boundary layer becomes thinness
on top of piston at higher revolution.
Fig. 4 illustrate the isotherms of the same case of Fig. 2. It is noticed
that temperature boundary conditions for combustion chamber was
Fig. 3. Comparison of velocity vectors for different revolutions at θ=90°, a) n=1000 rpm, b) n=5000 rpm.
Fig. 4. Isotherms for different crank angle at n=3000 rpm, a) θ=30°, b) θ=60°, c) θ=90°, d) θ=120°, e) θ=150°, f) θ=180°, g) θ=210°.
1371Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

7. measured from an exact engine and its temperature of cooling water.
Thus, constant temperature boundary conditions were kept as 493 K.
It is clearly seen from the isotherms that the temperature of fluid
inside the combustion chamber increases with increasing of crank
angle. Temperature rises at the cross section of rotated flow as given
in Fig. 2. It is an interesting result that temperature of two rotating
flows is almost equal to each other. Nevertheless, crank angle is
effective parameters on this value. Fig. 5 compare the effects of
revolution on temperature distribution. It is seen that revolution is an
effective parameter on temperature distribution. Temperature of
rotating fluid decreases with increasing of revolution number. The
temperature values are almost equal for both main eddies. The
strength of plume-like temperature distribution at the intersection of
clockwise and counterclockwise rotating fluid becomes higher for
n=5000 rpm. Pressure distribution inside the combustion chamber
is presented in Fig. 6 (a) to (d) for n=3000 rpm. It is an expected
result that low pressure is formed around the valve. Pressure values
are decrease with increasing of value of revolution. The sharp corner
disturbs the fluid and they may enhance the effectiveness of the
combustion. Finally, static pressure, velocity magnitude and tem-
perature values are illustrated in Fig. 7 (a), (b) and (c), respectively.
All results were presented for θ=90°. The profiles are taken at
y=Vc/2 (Fig. 1 (b)) and along the x-axis. Fig. 7 (a) showed that the
pressure is almost constant for n=1000 rpm. A sinusoidal variation
}
Fig. 4 (continued).
1372 Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

8. was obtained with increasing of revolution and pressure is also
increased. It is an interesting result that the pressure is lower at the
right-half section of the cylinder. The velocity magnitude is obtained
symmetrically according to middle x-axis as seen in Fig. 7 (b). The
value of revolution enhances the velocity of the fluid, as expected.
Temperature distribution is also obtained symmetrically and tem-
Fig. 5. Comparison of isotherms for different revolutions at θ=90°, a) n=1000 rpm, b) n=5000 rpm.
Fig. 6. Pressure contours for different crank angle at n=3000 rpm a) θ=30°, b) θ=60, c) θ=180°, d) θ=210°.
1373Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

9. Fig. 7. a) Static pressure, b) Velocity, c) Temperature for different revolution at θ=90°.
1374 Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375

10. perature is decreased with increasing of revolution due short intake
stroke.
6. Conclusions
A numerical work has been done in this study to see the how shape
and revolution of engine affects the flow and temperature fields. The
main conclusions drawn from the results of the present study may be
listed as follows:
• Two circulation cells were formed at different rotation directions for
all cases. This is a typical property of a gasoline engine. Flow
distribution inside the cylinder is almost symmetric for low values
of crank angles. But the flow at inclined side of the chamber
becomes dominant with increasing of crank angles.
• The pent-roof type of combustion chamber can be a control parameter
for heat and fluid flow.
• Temperature of the fluid increases with increasing of crank angle but
decreases with revolution.
• It is observed that the Reynolds averaged turbulence model k–ε gives
acceptable results for heat and fluid flow in pent-roof type combustion
chambers.
Acknowledgements
Authors thank Firat University Scientific and research fund for
their valuable financial support with a project number 1874.
References
[1] S.A. Basha, K.R. Gopal, In-cylinder fluid flow, turbulence and spray models-A
review, Ren. Sust. Energy Rev. 13 (2009) 1620–1627.
[2] G. Borman, K. Nishiwaki, Internal combustion engine heat transfer, Prog. Energy
Combust. Sci. 13 (1987) 1–46.
[3] J.B. Heywood, Internal Combustion Engine Fundamental, McGraw-Hill, New York,
1998.
[4] K.Y. Kang, J.H. Baek, Turbulence characteristics of tumble flow in a four-valve
engine, Exp. Therm. Fluid Sci. 18 (1998) 231–243.
[5] N. Kampanis, C. Arcoumanis, R. Kato, S. Kometani, Flow, Combustion and
Emissions in a Five-Valve Research Gasoline Engine, SAE Tech. Papers Series pp.
no. 2001-01-3556.
[6] R.F. Huang, C.W. Huang, S.B. Chang, H.S. Yang, T.W. Lin, W.Y. Hsu, Topological flow
evolutions in cylinder of a motored engine during intake and compression
strokes, Fluids Struc. 20 (2005) 105–127.
[7] N. Dinler, Numerical investigation of flow and combustion in a spark ignition
engine cylinder, MSc Thesis, Gazi University, Institute of Science and Technology,
2006.
[8] Z. Johan, A.C.M. Moraes, J.C. Buell, R.M. Ferencz, In-cylinder cold flow simulation
using a finite element method, Comp. Meth. Appl. Mech. Eng. 190 (2001)
3069–3080.
[9] R. Akar, Combustion chamber design with computational fluid dynamic, Inst. Nat.
Appl. Sci., MSc Thesis, 2005.
[10] F. Payri, J. Benajes, X. Margot, A. Gil, CFD modeling of the in-cylinder flow in direct-
injection diesel engines, Comput. Fluids 33 (2004) 995–1021.
[11] H.W. Wu, S.W. Perng, LES analysis of turbulent flow and heat transfer in motored
engines with various SGS models, Int. Heat Mass Transfer 45 (2002) 2315–2328.
[12] C.W. Hong, S.D. Tarng, Direct measurement and computational analysis of
turbulence length scales of a motored engine, J. Exp. Therm. Fluid Sci. 16 (1998)
277–285.
[13] V. Moureau, C. Angelberger, Towards Large Eddy Simulation in Internal
Combustion Engines: Simulation of a Compressed Tumble Flow, SAE 011995,
2004.
[14] A. Bilgin, Numerical simulation of the cold flow in an axisymmetric non-
compressing engine-like geometry, Int. J. Energy Res. 23 (1999) 899–908.
[15] B.E. Milton, M. Behnia, D.M. Ellerman, Fuel deposition and re-atomisation from
fuel/air flows through engine inlet valves, Int. Heat Fluid Flow 22 (2001) 350–357.
[16] J. Song, C. Yao, Y. Liu, Z. Jiang, Investigation on flow field in simplified piston bowls
for DI diesel engine, Eng. Appl. Comp. Fluid Mech. 2 (2008) 354–365.
[17] B.A. Ceper, Usability Of Hydrogen-Natural Gas Mixtures In Internal Combustion
Engines, PhD. Thesis, Erciyes University, Inst. Science Graduate School Natural and
Applied Sciences, 2009.
[18] FLUENT 12.0 User Guide, 2009.
[19] B.E. Launder, D.B. Spalding, Lectures in Mathematical Models of Turbulence,
Academic Press, London, 1972.
[20] S.V. Patankar, Numerical Heat Transfer and Fluid Flow, Hemisphere, New York,
1980.
[21] M. Firat, Modeling of fluid flow and heat transfer in new generation combustion
chambers, MSc Thesis, Firat University, Inst. Science Graduate School Natural
Applied Sciences, 2010.
1375Y. Varol et al. / International Communications in Heat and Mass Transfer 37 (2010) 1366–1375