report

Centre for Modeling and Simulation
Savitribai Phule Pune University
Master of Technology (M.Tech.)
Programme in Modeling and Simulation
Project Report
Conjugate Heat Transfer for Electronic
Cooling using OpenFOAM
Avinash Gorde
CMS1310
Academic Year 2014-15

Certiﬁcate
This is certify that this report, titled
Conjugate Heat Transfer for Electronic Cooling using OpenFOAM,
authored by
Avinash Gorde (CMS1310),
describes the project work carried out by the author under our supervision during the
period from January 2015 to June 2015. This work represents the project component
of the Master of Technology (M.Tech.) Programme in Modeling and Simulation at the
Center for Modeling and Simulation, Savitribai Phule Pune University.
Dr. Vikas Kumar, Principal Technical Oﬃcer
Computer Aided Engineering Group, Centre for
Development of Advanced Computing Pune,INDIA
Mr. Mohan Labade, Project Engineer
Centre for Development of Advanced
Computing Pune,INDIA
Dr. Sukratu Barve, Faculty
Pune 411007 India
Prof. Anjali Kshirsagar, Director
Pune 411007 India

Author’s Declaration
This document, titled
Conjugate Heat Transfer for Electronic Cooling using OpenFOAM,
authored by me, is an authentic report of the project work carried out by me as part
of the Master of Technology (M.Tech.) Programme in Modeling and Simulation at the
Center for Modeling and Simulation, Savitribai Phule Pune University. In writing this
report, I have taken reasonable and adequate care to ensure that material borrowed from
sources such as books, research papers, internet, etc., is acknowledged as per accepted
academic norms and practices in this regard. I have read and understood the University’s
policy on plagiarism (http://unipune.ac.in/administration_files/pdf/Plagiarism_Policy_
University_14-5-12.pdf).
Avinash Gorde
CMS1310

Abstract
The cooling is necessary for the proper functioning of Electronic instruments. Unless proper
cooling arrangement is designed, the operating temperature exceeds permissible limit, hence
it chances of failure get increased. Traditional models like conduction, convection etc often
solve one type of physics and heat transfer problem consisting of single material and governing
equations. Conjugate heat transfer problems it contain convection and conduction both. where
the convection equation of fluid zone is coupled with the conduction equation of solids. Modeling
of these systems is a difficult problem and involves many types of physics and usually did not
interact with other models. As increased in High Performance Computing (HPC) platforms it
has allowed more and more interactions of these various models.
The objective of this project is to study conjugate heat transfer in electronics cooling system
using OpenFOAM tool. For this purpose first solves simple problems like 2D planewall, IC
cooling of board for getting confiden e on OpenFoam tool. Finally solves the conjugate heat
transfer in server cooling of HPC system. Commercially available software has been readily
available as of late to solve complex fluid- solid heat transfer problems. This project investigates
the effectiveness of using the open source software OpenFOAM to effectively model conjugate
heat transfer of solid and fluid domain for electronic cooling. It having solid parts 24 RAM , 2
Socket, 1 PCB in solid domain and other parts comes in air domain, it solves conjugate heat
transfer equations using chtMultiRegionSimpleFoam steady state solver. The turbulence model,
mesh, numerical schemes, boundary and initial conditions were carefully chosen and adapted
to in this case.
7

Acknowledgements
In particular, the past six months of thesis work would not have been possible without the
help and support of many people. I would like to thank my Project Institute Centre for
Development of Advanced Computing Ganeshkhind, Pune University Campus, Pune,INDIA
provide me project opportunity.
I would like to thanks Principal Technical Oﬃcer Dr. Vikas Kumar, project engineer
Mohan Labade and Sai Meher, for their valuable guidance on a daily basis during this
project. I am thankful to this people for providing with me wonderful environment and
availability of computing facility for this project.
Special thanks to my internal guides Prof. Sukratu Barve giving me guidance and
direction, every time during this project,without his advices and help I would not have gone
too far. I am thankful to internal guide Prof. Mihir Arjunwadkar support giving direction
for project.
I would like to thanks Dr. Deepak Bankar, Mrs. Sutapa Chattopadhay, Shrinivas(CMS),
guided about computing facility. Last but not the least I would like to thank my friend Alok,
Umesh, Ashish, Sandeep, Akshay, Ashish, Jaydeep, Ajay for their encouragement and help
during my tenure at CMS. Big thanks to my parents, brother whom without I would not have
been able to accomplish anything.
9

List of Tables
2.1 Constant values for turbulence model . . . . . . . . . . . . . . . . . . . . . . . . . 22
4.1 Boundary conditions for AIR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33
4.2 Solid thermophysical properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
4.3 Fluid thermophysical properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
4.4 Numerical Scheme . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37
4.5 Residual Error tolerance for SIMPLE algorithm . . . . . . . . . . . . . . . . . . . 38
5.1 Comparision of Socket & Ram Temp(K) . . . . . . . . . . . . . . . . . . . . . . 42
11

List of Figures
2.1 Example of one dimensional control volume. . . . . . . . . . . . . . . . . . . . . . 24
3.1 Model of server . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
3.2 topoSet for create region . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
3.3 blockMesh of server . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
3.4 Sink of Socket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30
4.1 SIMPLE Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32
5.1 Temperature colour legends . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
5.2 Temperature distribution in sink . . . . . . . . . . . . . . . . . . . . . . . . . . . 40
5.3 Temperature distribution in passage of sink . . . . . . . . . . . . . . . . . . . . . 40
5.4 Temperature distribution inlet outlet . . . . . . . . . . . . . . . . . . . . . . . . . 41
5.5 Temperature distribution socket and ram . . . . . . . . . . . . . . . . . . . . . . 41
5.6 Temperature distribution socket and ram . . . . . . . . . . . . . . . . . . . . . . 42
A.1 Case structure for server . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48
13

Contents
Abstract 7
Acknowledgments 9
1 Introduction 17
1.1 Previous Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
1.2 Need of Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
1.2.1 Objectives . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
2 Therotical Background 19
2.1 Fluid Mechanics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
2.1.1 Governing Equation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
2.2 RANS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
2.2.1 Turbulence Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
2.3 Heat Transfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
2.3.1 Non Dimensionless Number . . . . . . . . . . . . . . . . . . . . . . . . . . 23
2.4 Finite Volume Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23
3 CFD Modeling 25
3.1 General introduction of OpenFOAM . . . . . . . . . . . . . . . . . . . . . . . . . 25
3.1.1 Case . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
3.1.2 Case structure for chtMultiRegionSimpleFoam (Electronic Cooling) . . . . 26
3.2 Equation Used by OpenFOAM chtMultiregionSimpleFoam Solver . . . . . . . . . 26
3.2.1 Governing equations in ﬂuid regions . . . . . . . . . . . . . . . . . . . . . 26
3.2.2 Governing equations in Solid regions . . . . . . . . . . . . . . . . . . . . . 26
3.2.3 Conjugate Heat Transfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27
3.2.4 ParaView for postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . 28
3.3 Geometry and Meshing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
4 Solution Methodology 31
4.1 Solution Algorithm SIMPLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31
4.2 Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33
4.2.1 Thermophysical Properties . . . . . . . . . . . . . . . . . . . . . . . . . . 34
4.3 Numerical Schemes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36
4.3.1 Linear Solvers in OpenFOAM . . . . . . . . . . . . . . . . . . . . . . . . . 36
4.3.2 Numerical Schemes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37
4.3.3 Convergence Criteria . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38
15

16 CONTENTS
5 Results 39
5.1 Graphs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
5.1.1 Temperature colour legends . . . . . . . . . . . . . . . . . . . . . . . . . . 39
5.1.2 Temperature distribution Heat Sink . . . . . . . . . . . . . . . . . . . . . 40
5.1.3 Temperature distribution passage of Heat Sink . . . . . . . . . . . . . . . 40
5.1.4 Inlet Outlet Temperature Distribution . . . . . . . . . . . . . . . . . . . . 41
5.1.5 Temperature distribution along Socket and Ram . . . . . . . . . . . . . . 41
5.1.6 Velocity of air inlet to Outlet . . . . . . . . . . . . . . . . . . . . . . . . . 42
5.1.7 Validation of OpenFOAM Results with Experimental Results . . . . . . . 42
6 Conclusion 43
6.1 Future Scope . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44
Bibliography 45
A Heat Source with fvOption 47
A.1 Structure for OpenFOAM case . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48

Chapter 1
Introduction
In the industry today, Computational Fluid Dynamics (CFD) codes are widely used as a tool
of thermal analysis. CFD solutions of high spatial and temporal resolutions can be obtained
on a desktop computer or even a laptop. The relatively recent adoption of CFD simulation
studies in electronic cooling applications has prompted some interest in validation.Conjugate
heat transfer is simulated for all the electronic devices and packages by solving Navier-Stokes
equations.Whenever electrical current flows through a resistive element, heat is generated.[2]
This project involves building a model of server which having 2 sockets, 24 rams and 1 printed
circuit board. Geometry using open-source software, creating a suitable mesh, setting up the
cases (choosing solvers, numerical schemes methods, etc.), making the CFD calculations with
OpenFOAM.
The geometry and flow domain consists of a flat circuit board with a heat generating element
socket and ram mounted on it. Heat is conducted through the source (chip) and the board on
which it is mounted. A stream of air flows over the board and the chip, causing simultaneous
cooling of the solid components and heating of the air stream due to convection. Thermal
energy is also transported due to the complex flow field. For RANS the Low Reynolds number
RNGk-epsilon turbulence model was chosen for its accuracy at the near wall region.[5]
1.1 Previous Work
The previous work was done in the field of forced convection conjugate heat transfer
for laminar flow conditions was discussed in Peterson and Ortega (1990).[12] Baker (1972)
conducted an analytical and experimental investigation of cooling of microelectronic devices by
free and forced convection. His study included small isothermal heat sources mounted on an
insulated board in a turbulent boundary layer with uniform properties and universal velocity
profile using Freon 113 as the coolant. Brosh et al. (1982) numerically solved the problem of
a two dimensional laminar incompressible flow over a conducting plate with a line heat source
(a point source in the two dimensional sense) located at the solid-fluid interface perpendicular
to the flow direction. An investigation on conjugate analysis of forced convection heat transfer
from small isothermal heat sources embedded in a large substrate for hydro dynamically fully
developed laminar channel flow was performed by Ramadhyaniet al. (1985).
Mahaney H. V. , Ramadhyani S., and Incropera, F. P (1989) Numerical Simulation of
Three-Dimensional Mixed Convection Heat Transfer from an Array of Discrete Heat Sources
in a Horizontal Rectangular Duct. They conducted both experimental and theoretical studies
17

18 CHAPTER 1. INTRODUCTION
of this problem. They compared their numerical investigations with data from single square
sources and an array of twelve such sources in water and FC77.[11] They concentrated their
effort on understanding the behavior of the surface conductance on the surface of the heat
source. Culham et al. (1991) conducted a study of conjugate heat transfer from square flush
mounted heat sources by implementing an iterative scheme in which the thermal boundary
conditions are applied on the conduction solution based upon the analytical solution of the
boundary layer energy equation
In (1994)Ramesh Sugavanam studied the problem of A Numerical investigation of conjugate
heat transfer a flush heat source on a conductive board in laminar channel flow.[13]
1.2 Need of Project
A very limited conjugate heat transfer case studies have been analyzed using OpenFOAM
CFD software. Since the popularity of OpenFOAM is increasing day by day among researchers,
considering these aspects, the current project was undertaken with the following objectives:
1.2.1 Objectives
• To develop a CFD model for conjugate heat transfer analysis of an electronics cooling
system
• Validation of CFD model with experimental results

Chapter 2
Therotical Background
2.1 Fluid Mechanics
This chapter will content a brief introduction to the theory used in this thesis. A fluid is a
substance that is unable to support shear stresses [2], though in reality they can withstand
some because of viscosity. The study of fluids is called fluid mechanics, and the part of fluid
mechanics used here is called fluid dynamics. It studies forces in conjunction with fluids. Basic
concepts of heat transfer and a description of the finite volume method are also presented.
2.1.1 Governing Equation
Fluid flows are well described by the Navier-Stokes equations for continuity and momentum
for an incompressible fluid make up a system with 4 equations and 4 unknowns: 3 velocity
components (u, v, w) and the pressure p.
Continuity Equation
The continuity equation, also known as the mass balance equation is based on the physical
principle that mass can be neither destroyed nor created [2]. This physical principle states that
the mass flow into a control volume equals the rate of change of mass inside the control volume.
∂ρ
∂t
+
−→
· (ρ−→u ) = 0 (2.1)
which is know as the continuity equation.
Momentum Equation
The momentum equation, also known as the force balance equation, it is based on Newtons
second law of motion, that is, the sum of all forces acting on a body is equal to the rate of change
of momentum of it (mass acceleration) . The forces acting on the body can be divided into to
groups. The first is the body forces fi acting inside the body e.g. centrifugal or gravitational
forces. The second group is the surface forces acting on the surface of the body e.g. pressure
or viscous forces.The governing equation for momentum from [4] can then be expressed as
∂(ρui)
∂t
+
∂[ρuiuj]
∂xj
= −
∂p
∂xi
+
∂τij
∂xj
+ ρfi (2.2)
Strain rate tensor
τij =
1
2
∂xi
∂xj
+
∂xj
∂xi
(2.3)
19

20 CHAPTER 2. THEROTICAL BACKGROUND
Energy Equation
The energy equation, also known as the energy balance equation, is based on the conservation
of energy principle. This principle states that energy can neither be created nor destroyed, it
can only change form. It follows from the first law of thermodynamics and states that the
rate of change of total energy is equal to the rate heat is added minus the rate of work done.
The temperature field T is calculated using the energy equation (2.3) once the velocity field is
known.The energy equation can be expressed in terms of the specific enthalpy
ρ
D
Dt
h +
1
2
uiui =
∂p
∂t
+
1
2
[ui + τij] −
∂qi
∂xi
+ ρgui (2.4)
D
Dt represents ∂
∂t + ui + ∂
∂xI .
Enthalpy h = cpT
Heat flux q using Fouriers law becomes −κ ∂T
∂xi
The system of equations is complete, it seems that we could directly discretize the equations
and calculate the fluid properties at every grid point. But solving Navier-Stokes equations
numerically is not a simple task, it would require a very fine grid to resolve all the turbulent
scales and a fine resolution in time (turbulent flow is always unsteady)
2.2 RANS
The three commonly used methods for turbulence modeling are Direct Numerical Simulation
(DNS), Large Eddy Simulation (LES), and Reynolds Averaged Navier-Stokes (RANS) modeling.
Solving all scales in a turbulent flow is only possible using high computational power. For most
practical purposes it is enough to calculate the time-averaged properties of a flow. This can be
solved by solving a time-averaged version of the Navier-Stokes equations.They are obtained by
introducing the Reynolds decomposition of the pressure and velocity and then time-averaging
the equations [5]. The Reynolds decomposition consists of dividing the instantaneous pressure
and velocity into one time-averaged and one fluctuating part,the decomposition of the velocity
would be as:
u (x, t) = ¯u (x) + u (x, t) = U + u (2.5)
similarly p = P + p
Where the average value calculated from:
¯u (x) = lim
1
T
u (x, t) dt (2.6)
After insertion of the decomposition and time-averaging of the Navier-Stokes equations one
additional term appears, −ρui uj This term is called the Reynolds stress tensor and means
additional unknowns have been introduced. Since the number of equations has not increased,this
creates a closure problem.
2.2.1 Turbulence Modeling
In laminar flow the adjacent layers slide past each other in an orderly fashion.Turbulent flow
on the other hand is random and chaotic in its nature. There are six main characteristics for

2.2. RANS 21
turbulent flow:
• Irregular
• Diffusive
• Has a relatively high Reynolds number
• Three-dimensional
• Dissipative
• Property of the flow (i.e. not the fluid)
In turbulence unsteady vortices called eddies appear. The largest eddies extract energy from
the mean flow, called turbulent kinetic energy. This energy is then transferred to smaller and
smaller eddies until it reaches the smallest ones where it is dissipated into heat. This process
of energy transfer is called the cascade process.To solve this the Reynolds stress tensor can
be model using an eddy viscosity and the velocity gradients. This is called the Boussinesq
assumption (Eq.2.6) and the basic idea behind it is to model the small-scale eddies with a
viscosity term.
−ρuiuj = µt
∂ui
∂xj
+
∂uj
∂xi
−
2
3
∂uk
∂xk
δij −
2
3
kδij (2.7)
2
3kδij is the turbulent viscosity or eddy viscosity and k is the turbulent kinetic energy
defined as
k =
1
2
u 2
+ v 2
+ w 2
(2.8)
There are plenty of models to describe the turbulent quantities including one-equation models,
two-equation models and algebraic models.
RNG κ − model
The RNG κ− model was derived using a rigorous statistical technique (called renormalization
group theory). It is similar in form to the standard κ − model.The RNG model has an
additional term in its equation that significantly improves the accuracy for rapidly strained
flows. While the standard κ − ε model is a high-Reynolds-number model, the RNG theory
provides an analytically-derived differential formula for effective viscosity that accounts for
low-Reynolds-number effects. Effective use of this feature depend on an appropriate treatment
of the near-wall region. The RNG theory provides an analytical formula for turbulent Prandtl
numbers, while the standard κ − model uses user specified, constant values.[1]
∂ (ρk)
∂t
+
∂ (ρkui)
∂xi
=
∂
∂xj
αkµeff +
∂k
∂xj
+ Gk + Gb − ρ − Ym + Sk (2.9)
above equation is turbulent kinetic energy for RNG κ − model.
∂ (ρ )
∂t
+
∂ (ρ ui)
∂xi
=
∂
∂xj
αkµeff +
∂
∂xj
+ C1
k
(Gk + C3 Gb) − C2ρ
2
k
− R + S (2.10)

above equation is dissipation rate for RNG κ − model.
where,
Gk is the generation of turbulent kinetic energy that arises due to mean velocity gradients.
Gb is generation of turbulent kinetic energy the arises due to buoyancy.
Sk, S are source terms defined by the user.
αk, α are inverse effective Prandtl numbers for the turbulent kinetic energy and its dissipation.
C1 , C2 and Cµ are constants that have been determined experimentally.
C1 is replaced by C∗
1 which is no longer a constant, but is determined from an auxiliary
function as
C∗
1 = c1 −
η 1 − η
η0
1 + βη3
(2.11)
where,
η =
k√
τijτij (2.12)
is the expansion parameter (ratio of the turbulent to mean-strain time scales). The model
constants are [1]:
Table 2.1: Constant values for turbulence model
C1 C2 C3 Cµ η β σk σ
1.42 1.68 -0.33 0.085 4.38 0.012 0.7194 0.7194
2.3 Heat Transfer
Heat Transfer
Energy in transit due to temperature difference. In heat transfer the exchange of thermal
energy in a physical system is the subject of study. Heat exchange always occur when there
exist a temperature difference in a medium or between media. Heat transfer is categorized
depending on the conditions in which it take place. The fundamental modes of heat transfer
are conduction or diffusion, convection and radiation.[2]
Conduction
Conduction is the transfer of energy from the more energetic particles of a substance to the
adjacent less energetic ones as a result of interactions between the particles. conduction is due
to the collisions and diffusion of the molecules during their random motion .[2]
Convection
Convection is the mode of energy transfer between a solid surface and the adjacent liquid or
gas that is in motion, and it involves the combined effects of conduction and fluid motion.The
faster the fluid motion, the greater the convection heat transfer.In the absence of any bulk fluid
motion, heat transfer between a solid surface and the adjacent fluid is by pure conduction.[2]
Radiation
Radiation is the energy emitted by matter in the form of electromagnetic waves (or photons)
as a result of the changes in the electronic configurations of the atoms or molecule .[2]
Conjugate heat transfer

2.4. FINITE VOLUME METHOD 23
Process which involves variation of temperature within solid and fluid due to thermal interaction
between solid and fluid.
It may be combination of conduction + convection
conduction + radiation
In convective heat transfer motion of fluid is the dominant mechanism for transfer of the heat.
Convection can further be divided into natural convection and forced convection. In a forced
convection system the fluid motion is maintained by external force,like blower or a fan whereas
in natural convection it is maintained by buoyancy forces. The system that will be modeled in
this thesis consist of forced convection in a server casing with heated socket and ram.[10]
2.3.1 Non Dimensionless Number
Study of systems with turbulent flow and heat transfer there are many ways to estimate basic
concepts. For this purpose there exist a wide range of dimensional numbers that describe
the different properties of a system [10].Theory will be helpful for make use of following
dimensionless number:
Reynolds Number
The Reynolds number (Re) is defined as the ratio between inertial forces and viscous forces.
It can be calculated by Re = ρul
µ , were u is the average velocity of the fluid and l is the
characteristic length,in circular section used diameter. The Reynolds number is used for
estimate if a flow is turbulent(if Re > 4000) ,transitional(if 4000 > Re < 2000) or laminar(if
Re < 2000).
Prandtl Number
It is the ratio of kinematic viscosity to thermal diffusivity.It can be calculated according to
µCp
K .
Nusselt Number
The Nusselt number (Nu) is defined as the ratio between convective and conductive heat
transfer across a boundary, it is the dimensionless temperature gradient normal to the heated
surface.It can be calculated using hl
K h is convective heat transfer coefficient and K is the
thermal conductivity of solid.
2.4 Finite Volume Method
The finite volume method is a technique to go from continuous differential equation to a
discrete algebraic equation.[14] The fundamental idea is to divide the computational domain
into a number of smaller control volumes of geometrical shapes like cuboid or tetrahedrons.
This is done by defining a number of node points in the domain and then divide the domain
between the node points resulting in a structure called mesh. In the solution procedure, the
refinement of the mesh is a compromise between the solution accuracy and the computational
cost. The differential equation is then discretized by integration over each control volume. The
integrations make use of Gauss theorem stating that
Ω
· ψdV =
∂Ω
ψ · ndS (2.13)
Ω is the arbitary control volume.
∂ω is the surface.
let n be the outward unit normal on a small area dS.

With this technique the integrated terms of the differential equation only needs to be given
at the boundary of the control volume. The boundary is divided into faces defined as parts of
the boundary where the normal do not change. Since the values at the faces are normally not
known they are interpolated from the node points. This is done with an interpolation scheme
of which there exist a wide range to chose from depending on what is suitable for the equation
to be solved.
As an example, to solve the one-dimensional differential equation:
d2ψ
dx2
+ S = 0 (2.14)
over a domain D first divide D into a suitable number of control volumes, see below figure. At
each control volume by Gauss theorem it follows that
Ω
d2ψ
dx2
+ S dV =
Ω
d
dx
dψ
dx
dV +
Ω
SdV =
∂Ω
dψ
dx
dS+S∆x =
dψ
dx e
−
dψ
dx w
+S∆x
(2.15)
The subscripts e and w corresponds to the faces between node P and node E and W
respectively and S is the average of S over the control volume.To achieve the final discretized
equation the first order derivative terms need to be interpolated on the faces in terms of the
node points. One such scheme is the central differencing scheme which gives
dψ
dx e
=
ψE − ψP
δxe
,
dψ
dx w
=
ψP − ψW
δxw
(2.16)
Inserting Equation 2.14 in Equation 2.13 and rearranging yields,
aEψE − aPψP + aWψW = −Su (2.17)
aE =
1
δxe
, aW =
1
δxw
, aP = aE + aW (2.18)
Performing the previous discretization at each node gives a linear system of equation, with an
equation per node. Such a system of equation can be solved by existing algorithms like Thomas
Diagonal Matrix Algorithm (TDMA) and Gauss-Seidel Method.
∆ x
δxw δxe
• •
W
•
PE
Figure 2.1: Example of one dimensional control volume.

Chapter 3
CFD Modeling
OpenFoam is open source software for CFD. We can say it is C++ template base library,
It included various type of solvers for different physics e.g. compressible, incompressible,
multiphase, heat transfer etc.. OpenFOAM is preferably used in a Linux environment, it is
open source so user can adjust their own way. Basic concepts of developing solvers and setting
up cases are presented. In this project OpenFOAM version 2.3.1 used. OpenFOAM uses finite
volume discretization schemes.
3.1 General introduction of OpenFOAM
The OpenFOAM software contains tools for pre-processing and the solver tools. Useful
features in the pre-processing tools are the meshing tool like blockMesh, snappyhexMesh,
Dynamic mesh. In the solving procedure in OpenFOAM there are two main parts. The first
is the applications which are executables referred to as solvers and utilities. The solvers are
algorithms for solving systems of differential equations mainly with the finite volume method.
In OpenFOAM to solve problem is to located in entity called case. In case given detail of
which solver is to be used for solving the partial differential equations. The solver and cases
briefly explained in following sections. [7]
3.1.1 Case
The case is set up with appropriate name of folders. It contain three sub folders i.e. system,
constant and 0. In 0 directory initial conditions and boundary conditions for all the fields in
the problem are defined. The commonly used boundary conditions in OpenFOAM is set with
keywords. The Dirichlet boundary condition is defined with fixedGradient [8]
The constant folder contains problem specific files defining constant properties of the
case. The other files, that depend on the specific problem, if fluid is present can be
turbulenceProperties properties,RAS properties,RAS model,thermophysical properties of that
domain. In this folder contain polymesh folder in which mesh(blockMesh) is stored, it contains
boundary patch.[8]
The system folder contains files relevant to solvers e.g.fvScheme it contains numerical schemes
for that solvers. When simulation is transient then ddt scheme will be Euler and simulation
is steady state then ddt scheme will be Steady State. fvSolutions contains algorithm(SIMPLE,
PIMPLE) for solver, convergence criteria for numerical scheme.contolDict contain start time,
end time, Courant number, we can add run time utilities.
25

26 CHAPTER 3. CFD MODELING
3.1.2 Case structure for chtMultiRegionSimpleFoam (Electronic Cooling)
In this case contain AIR, BOARD, 24RAM, SOCKET, small boxes smps, splitter,mesion in
appendix
3.2 Equation Used by OpenFOAM chtMultiregionSimpleFoam
Solver
chtMultiRegionSimpleFoam solver is the combination of heatConductionFoam and
buoyantFoam for conjugate heat transfer between a solid region and fluid region, including
steady-state turbulent flow of compressible fluids.
3.2.1 Governing equations in fluid regions
The continuity equation and the NavierStokes equations for compressible laminar flows in
vector forms same as above mentioned equation(2.1).
Momentum equation used by OpenFOAM
∂ (ρu)
∂t
+ · (ρuu) = − p + · τ − ρg (3.1)
where u is the velocity vector, p is the thermal pressure, g is the gravitational acceleration, and
τ is the stress tensor given by
τ = µ u + uT
−
2
3
· uI (3.2)
where µ is the molecular viscosity, and I is the unit tensor. Here the compressible perfect gas
is used instead of the Boussinesq approximation because of the large temperature difference
between the cold wall and hot wall in the present study.
Energy equation used by OpenFOAM
∂(ρE)
∂t
+ · (ρuE) = · (α e) − · [u (p − ρgr)] + Sh (3.3)
α =
µCp
κ is the thermal diffusivity.
Sh is the thermal source term.
e is the specific internal energy.
E is the specific total energy of the gas defined as:
E = e + u2
2
3.2.2 Governing equations in Solid regions
For making of solid region requires properties of solid like Moles weight, Specific heat, thermal
conductivity of solid and density of solid.[3]
∂ (ρh)
∂t
= · (α h) + Sh (3.4)

3.2. EQUATION USED BY OPENFOAM CHTMULTIREGIONSIMPLEFOAM SOLVER 27
α =
µCp
κ is the thermal diffusivity.
Sh is the heat source term.
h is the sensilbe enthalpy.
when analysis is steady state then equations will be
− · (α h) = Sh (3.5)
3.2.3 Conjugate Heat Transfer
The fluid domain and the solid domain are simulated simultaneously for the conjugate heat
transfer problem. The constant temperature boundary condition is given for the outside surfaces
of the solid regions in the model.In order to provide boundary condition for the fluid governing
equation, on the interface between the fluid domain and the solid domain, the no-slip wall
boundary condition is assumed.
In CHT computational domain is divided into fluid and solid regions. The NaviereStokes
equations and the energy equation in the fluid regions are solved first. Then the heat transfer
equation in the solid regions is solved. The coupling between the fluid and solid regions is
achieved by exchanging information at the fluid/solid interfaces to ensure the continuity of
temperature and the conservation of energy.
Coupling at the solid-fluid interface
The coupling between the fluid and the solid regions can be illustrated using fig. When solving
the energy Eqn. in the fluid region, a temperature should be specified at the interface.[3] The
temperature on the interface Tw can be calculated as follows:
Tw =
ks
δxs
Ts
kf
δxf
+ ks
δxs
+ (1 − k) Tf +
Tref
δxf
=
kf
δxf
Tf + ks
δxs
Ts
kf
δxf
+ ks
δxs
(3.6)
Where Tf and Ts are the temperatures from the neighboring fluid and solid regions
respectively. kf and ks are the heat conductivities of the fluid and solid regions respectively,
and Tref is a reference temperature. An interpolation coefficient k is defined as follows:
k =
ks
δxs
kf
δxf
+ ks
δxs
(3.7)
where δxf and δxs are the distances between the cell centers and the interface.
The temperature gradient at the interface can be calculated by following equation:
TI
f = k
Ts − Tf
δxf
+ (1 − k) Tref =
ks
δxs
kf
δxf
+ ks
δxs
Ts − Tf
δxf
(3.8)
For the solid side, similar gradient relation exists. To ensure energy conservation near the
interface the following condition is required
ksTI
s = kf TI
f (3.9)

3.2.4 ParaView for postprocessing
This is the third party post-processing open Source software distributed with OpenFOAM. It
is an open-source data analysis and visualization tool and it can either be invoked by using
paraFoam script or by converting the data to VTK format and open with ParaView. Data
processing can be done either interactively in a 3D environment or using command line batch
processing.[8]
3.3 Geometry and Meshing
Following ﬁgure shows the geometry of server,it contain 24 RAMS PCB, 2 SINKS 2 SOCKETS
2 BOXES, 2 SMPS
Figure 3.1: Model of server
topoSet
Figure 3.2: topoSet for create region

3.3. GEOMETRY AND MESHING 29
topoSet create cylindrical, rectangular, geometry inside of meshed block and extract cells of
that block. splitMeshregion utility create polymesh for region created by toposet and put into
constant folder contains different regions folders. The sample topoSet format given below:[9]
In this case for pre-processing blockMesh utility make generalized mesh geometry having
length 0.41 m X width 0.46 m X height 0.09 m it will start from inlet of the Fan. The velocity
inlet condition take instead of Fan. Meshing done with blockMesh utility, creating different zone
for multiregion using topoSet it requied to create the fluid and solid domain for the solver to
solve the domain. The checkMesh utility can be used for problem occured it shows fail report,
various type of error occur like negative volume cell detected. To diagnose problems with the
blockMesh dictionary and evaluate the quality of the mesh always used checkMesh utility.[8]
Figure 3.3: blockMesh of server

Heat Sink
The heat sink should be selected with high thermal conductivity materials like Copper or
Aluminium. It have low thermal resistance, heat sink increase the surface area for the dissipation
of heat and lowers the operating temperature of heat generating element. Heat sinks must be
designed in a way that air can easily and quickly flow through it, and reach all cooling fins.
The part of the heat sink that is in contact with the heat source must be perfectly flat. A
flat contact area allows you to use a thinner layer of thermal compound, which will reduce the
thermal resistance between heat sink and heat source.
Figure 3.4: Sink of Socket

Chapter 4
Solution Methodology
In this chapter Numerical Schemes, Solution Algorithm, Boundary conditions mentioned
4.1 Solution Algorithm SIMPLE
chtMultiregionSimpleFoam is compressible solver for steadystate heat transfer. SIMPLE is
Semi Implicit Pressure Linked Equation.When the RANS approach for turbulence is used, a
stationary problem arises. RANS and many other methods for steady problems in computational
fluid dynamics can be regarded as unsteady problems until a steady state is reached. If an
implicit method is used in time, the discretized momentum equations at the new time step are
non-linear. Due to this the underlying differential equations are coupled, the equations system
resulting from discretization cannot be solved directly hence solution methods are the only one
choice to solve equation.
The momentum equations are usually solved sequentially for each component. The pressure
used in each iteration is obtained from the previous time step and therefore the computed
velocities normally do not satisfy the discrete continuity equation. In order for the velocities
to fulfill this equation one have to modify the pressure field. This can be done by solving a
discrete Poisson equation for the pressure.
After solving this new equation for the pressure the final velocity field at the new iteration
is calculated. This new velocity field satisfies the continuity equation, but the velocity and
pressure fields do not satisfy the momentum equations. Therefore, the procedure described
above is iterated until a velocity field is obtained that satisfy both the momentum and continuity
equations.
Methods of this kind which first construct velocity fields that do not satisfy the continuity
equation and then correct them are known as projection methods. The SIMPLE algorithm is
such a method, and it is the solving procedure used in OpenFOAM for our computations
The algorithmic representation for SIMPLE algorithm is following way. In algorithm p is the
pressure, u, v, w, velocities in 3 direction, t is the Temperature.[14]
31

32 CHAPTER 4. SOLUTION METHODOLOGY
The steps in the SIMPLE algorithm, as shown in Figure 12, are summarized as:
START
Estimate a starting guess for the pressure field p*.
Initial guesses for p*, velocity components u*, v*,
w*, and other scalar properties φ* (i.e. T).
STOP
START
STEP 1: Solve discretised
momentum equations
STEP 2: Solve for pressure
correction equation
STEP 3: Correct
pressure and velocities
STEP 4: Solve the other
discretised transport equations
Convergence?
Yes
No
Set solved values equal
to new initial guesses.
p*=p, u*=u, v*=v,
w*=w, φ= φ*
Figure 12. The SIMPLE Algorithm [Versteeg and Malalasekera, 2007]
p’
p, u, v, w, φ*
φ
u*, v*, w*
[Hjertager, 2007]
Figure 4.1: SIMPLE Algorithm

4.2. BOUNDARY CONDITIONS 33
4.2 Boundary Conditions
In server cooling case have 31 different domain like 24 RAMS, AIR, BOARD, 2 SMPS, 2
BOXES, 2 SINKS, FLAPPER so 1 fluid and 32 solid domain, firstly
Boundary Conditions for AIR
Table 4.1: Boundary conditions for AIR
Boundary Conditions
Field INLET OUTLET F&B TOP AIR to
p
(Pa)
type
calculated
type
calculated
symmetry type
calculated
type calculated
value uniform
100000
value uniform
100000
value uniform
100000
value uniform
100000
p rgh type
fixedFluxPressure
type fixedvalue symmetry type
fixedFluxPressure
type
fixedFluxPressure
(Pa) value uniform
100000
value uniform
100000
value uniform
100000
value uniform
100000
U
(m/s)
type fixedvalue type
inletOutlet
symmetry type fixedvalue type fixedvalue
value uniform
2.1
value uniform
2.1
value uniform
0
value uniform 0
T
(K)
type fixedvalue type
inletOutlet
symmetry type
zeroGradient
type fixedvalue
value uniform
299
value uniform
299
value uniform
0
type compressible
turbulentTemperatureCoupledBa
value uniform 300
Tnbr T
kappa
fluidThermo
kappaName none
k type fixedvalue inletOutlet symmetry fixedValue type compressible
kqWallFunction
value uniform
0.1
value uniform
0.1
value uniform
0.1
value uniform 0.1
epsilon type fixedvalue inletOutlet symmetry fixedValue type compressible
epsilonWallFunction
value uniform
0.1
value uniform
0.1
value uniform
0.1
value uniform 0.1
Boundary Condition for Solid region
In solid region 24 RAMS, BOARD, 2 SMPS, 2 BOXES, 2 SINKS, FLAPPER are included.

Boundary Conditions for BOARD
Field INLET OUTLET F & B BOTTOM BOARD to
T
(K)
type
zeroGradient
type
zeroGradient
symmetry zeroGradient type compressible
turbulentTemperatureCoupledBaﬄeMixed
value uniform
299
value uniform
299
value
uniform
299
value uniform 299
Tnbr T
kappa
solidThermo
kappaName none
4.2.1 Thermophysical Properties
Solid thermophysical Properties
The data sheet for this material give the following properties
Table 4.2: Solid thermophysical properties
Solid name κ(W/mK) Cp(J/kgK) rho(kg/m3) Material
SOCKET 1 & 2 124 702 2325 Silicon
SINK 1 & 2 220 903 2700 Aluminium
RAM 124 702 2325 Silicon
SMPS 1 & 2 53 450 8000 Steel
BOX 1 & 2 53 450 8000 Steel
FLAPPER 53 450 8000 Steel
BOARD 0.02 1800 1500 FR4

4.2. BOUNDARY CONDITIONS 35
Thermophysical properties for air
The properties of air at 299K is deﬁned as follows density of air change with temperature, as
temperature increases density of air decreases
Table 4.3: Fluid thermophysical properties
Parameter value
Cp (J/kg K) 1000
µ 1.8e−05
Pr 0.7

Heat Source
In OpenFOAM heat source apply using fvOptions in terms of watt. The syntax for fvOptions
is mensioned in appendix:
4.3 Numerical Schemes
Numerical schemes is very important for solving various type of partial diﬀerential, integral
equations. The correct numerical scheme gives faster convergence for solution.
4.3.1 Linear Solvers in OpenFOAM
The chtMultiRegionSimpleFoam solver using the RNG κ turbulence model solves equations
for velocity, pressure, turbulent kinetic energy, and turbulent kinetic energy dissipation.
Every discretization equation uses linear solvers to solve a set of linear equations. The
Generalized Geometric-Algebraic Multi-Grid (GAMG) linear solver would have been more
ideal. This method generates a fast solution for a selection of cells, which is then mapped
on to the ﬁner mesh as the initial guess for the solution. The Preconditioned Conjugate
Gradient (PCG) linear solver is used to solve the symmetric pressure matrix equation using
a Diagonal Incomplete-Cholesky (DIC) preconditioner. The velocity, turbulent kinetic energy,
and turbulent kinetic energy(κ) dissipation rate( ) all use the Gauss Seidel smooth solver. Gauss
Seidel method is one of the more reliable smooth solvers, it is relatively slow due to its sequential
nature. A preconditioner, such as Preconditioned bi-Conjugate Gradient (PBiCG), could have
considerably reduced the number of iterations for solving these sets of equations.[6]

4.3. NUMERICAL SCHEMES 37
4.3.2 Numerical Schemes
For solid and fluid regions have soving numerical schemes as follows
Numerical schemes
Table 4.4: Numerical Scheme
Calculation Scheme
Time steadyState
Gradient Gauss linear
Divergence bounded Gauss upwind
Laplacian Scheme Gauss linear corrected
interpolationScheme Linear
Surface normal gradient uncorrected
Gradient terms , are discretized using the standard finite volume discretization method
of Gaussian integration, requiring interpolation of values from cell centers to face centers. In
this chtMultiregionSimpleFoam case, linear interpolation, more commonly known as central
differencing, is used. The divergence scheme . , which determines the convection term of a
fluid, (ρuu), can only be discretized using the Gauss scheme, along with an interpolation
scheme. Generally, simulations were initialized using upwind (first order) interpolation to
calculate a more stable flow field before upgrading to the more accurate linear (second order)
interpolation scheme. Furthermore, the positive turbulent kinetic energy and turbulent kinetic
energy dissipation scalars are bounded. Limited linear differencing is used for the velocity
vector to account for direction.Laplacian schemes discretize the Laplacian term, .(α h). The
interpolation scheme specified for the diffusion coefficient is Gauss linear. The surface normal
gradient corresponds to limited non-orthogonal correction.Surface normal gradient scheme
specifies the gradient of two adjacent cell centers normal to the face between the two cells.
This scheme uses explicit non-orthogonal correction. [6]

4.3.3 Convergence Criteria
Every iteration of the solvers, the residual error is evaluated. The solver stops when one of the
following is satisfied
• The ratio of current to initial residuals drops below the solver relative tolerance.
• The residual falls below the solver tolerance
• The number of iterations exceeds the specified maximum number of iterations
The tolerance and residual control for various fields specified below:
Table 4.5: Residual Error tolerance for SIMPLE algorithm
Parameter Relative Tolerance Absolute Tolerance
p rgh 0 1e−7
Velocity U 0.1 1e−7
Enthalpy h 0.1 1e−7
k 0.1 1e−7
epsilon 0.1 1e−7
ρ 0 1e−7

Chapter 5
Results
The results showing here cover tenperature distrubution profile in the server. Several probes
are inserted made line plot along SOCKET, RAM, Heat sink;
• Contours of temperature in server
• Plot of Temperature distrubution along heat sink.
• Plot of Temperature distrubution between passage between 2 heat sink fins.
• Plot of inlet to outlet temperature distribution in server.
• Plot of Temperature distrubution along RAM and SOCKET.
• Plot of inlet to outlet velocity distribution in server.
5.1 Graphs
5.1.1 Temperature colour legends
Below figure shows temperature distribution in server the red color portion is SOCKET and
SINK regions. Next to the sink it is observed the air temperature increases with the colour
variations.
Figure 5.1: Temperature colour legends
39

40 CHAPTER 5. RESULTS
5.1.2 Temperature distribution Heat Sink
This graph is plot along the z direction of geometry. Plot line passes through first and last fins,
first point coordinate is (0.1 0.02 0.28) and (0.1 0.02 0.360). following graph shows temperature
of sink. Lowerer line shows passage temperature.
298
300
302
304
306
308
310
312
314
316
318
320
0 0.01 0.02 0.03 0.04 0.05 0.06 0.07 0.08
TemperatureinKelvin
distace along z-axis
SinkTemp betn fins
Figure 5.2: Temperature distribution in sink
5.1.3 Temperature distribution passage of Heat Sink
Socket and RAM generate heat, sink is placed above the socket. It has low thermal resistance,
so it conduct heat faster and dissipate due to larger surface area. This plot taken along x-axis
first point is (0.06 0.02 0.332) before of heat sink and second point is (0.19 0.02 0.0332) after
the heat sink.
298
300
302
304
306
308
310
312
314
316
0 0.02 0.04 0.06 0.08 0.1 0.12 0.14 0.16 0.18 0.2
Temp.inKelvin
distace along x-axis
HeatsinkTemp
Figure 5.3: Temperature distribution in passage of sink

5.1. GRAPHS 41
5.1.4 Inlet Outlet Temperature Distribution
Following graph shows temperature distribution from inlet to Outlet in the server. This graph
is taken along x-axis with mid of the geometry.
299
299.5
300
300.5
301
301.5
0 0.05 0.1 0.15 0.2 0.25 0.3 0.35 0.4
TemperatureinKelvin
OutletTemp
Figure 5.4: Temperature distribution inlet outlet
5.1.5 Temperature distribution along Socket and Ram
Sockets are containing processors of server it has main heat generating source in the server. If
processing load on socket is increases then generation of heat increases. So it is necessary to
require more surface area for dissipation of heat. This graph is taken along z-axis ﬁrst point is
(0.095 0.0075 0) and second point is (0.09 0.0075 0.46).
295
300
305
310
315
320
325
0 0.05 0.1 0.15 0.2 0.25 0.3 0.35 0.4 0.45 0.5
Temp.inKelvin
distace along z-axis
SOCKET & RAM Temp
Figure 5.5: Temperature distribution socket and ram

42 CHAPTER 5. RESULTS
5.1.6 Velocity of air inlet to Outlet
In graph velocity showing some dropping down nature due to increase in volume of geometry.
This graph is taken along x-axis with mid of the geometry:
0
0.5
1
1.5
2
2.5
3
3.5
4
0 0.05 0.1 0.15 0.2 0.25 0.3 0.35 0.4
Velocitym/s
Velocity
Figure 5.6: Temperature distribution socket and ram
5.1.7 Validation of OpenFOAM Results with Experimental Results
The experimental results of server taken from sensor sensors reading which is available in the
server. OpenFOAM result based on same boundary conditions taking average of temperature
along socket.
Table 5.1: Comparision of Socket & Ram Temp(K)
Region OpenFOAM Result Experimental Result
SOCKET 319.838 318
RAM 301.43 303

Chapter 6
Conclusion
To study the Conjugate Heat Transfer in electronic cooling system
chtMultiRegionSimpleFoam OpenFOAM based steady state solver used. It simulatate
heat transfer mode conduction and convection simultaneously for the cooling electronics
server. CFD result which is obtained from simulation is good validate with experimental result
of server data. Hence OpenFoam tool is given good prediction for conjugate heat transfer
simulations.
This CFD analysis of server gives three dimensional temperature distribution in server
components such as RAMS, PROCESSORS, BOARD. It will be very significant in design of
electronics parts of server. This simulation is given heat dissipation profile along the components
which also important for choosing right material designing.
However a number of recent studies have observed that experimental data confirms the
continuum theory. The theory governing the fundamentals of CHT has been introduced and
the case for server has been developed. This will save time in the future work.
43

44 CHAPTER 6. CONCLUSION
6.1 Future Scope
The following works can be suggested as future work
• To implement Fan boundary condition for mass ﬂow rate.
• To implement microthickness baﬄe for sink region.

Bibliography
[1] ANSYS. Fluent 6.3 users guide. www.sharcnet.ca/Software/Fluent6/html/ug/
node479.htm.
[2] Y. A. Cengel. Heat Transfer A Practical Approach. McGraw-Hill, forth edition, 2003.
[3] Y. L. Chaolei Zang. Conjugate heat transfer analysis using simplified household refrigerator
model. Technical report, Department of Mechanical Engineering University of Lousville
USA, June 2014.
[4] J. D.Anderson. Computational Fluid Dynamics Basic with application. Mc GrawHill, 2000.
[5] W. D.C. Turbulence Modeling for CFD. DCW Industries, 3 edition, 2006.
[6] D.E.Dwyer. Defining ventilation boundary condition for green house climate model.
Master’s thesis, Delft University of Technology, August 2014.
[7] O. Foundation. Openfoam programmer guide. www.openfoam.org.
[8] O. Foundation. Openfoam user guide. www.openfoam.org.
[9] O. Foundation. Openfoam wikipedia. www.openfoamwiki.net.
[10] F. Incropera and D. DeWitt. Fundamentals of Heat and Mass Transfer. Wiley, Essex,
England, fifth edition, 2002.
[11] H. V. Mahaney, S. Ramadhyani, and F. P. Incropera. Numerical simulation of
three-dimensional mixed convection heat transfer from an array of discrete heat sources in
a horizontal rectangular duct. Numerical Heat Transfer, 16(part A):267–286, 1989.
[12] G. P. Peterson and A. Ortega. Thermal control of electronic equipment and devices.
Advance in heat transfer, 20(N5):181–245.
[13] C. Y. C. Ramesh Sugavanam, Alfonso Ortega. A numerical investigation of conjugate
heat transfer from a flush heat source on a conductive board in laminar channel flow.
InterSociety Conference on Thermal Phenomena, 1994.
[14] W. M. Versteeg H. K. An Introduction to Computational Fluid Dynamics, A Finite Volume
Method. Pearson Education Limited, Essex, England, second edition, 2007.
45

Appendix A
Heat Source with fvOption
heatSource
{
type scalarSemiImplicitSource;
active true;
selectionMode cellSet;
cellSet SOCKET1; //name of cellSet
scalarSemiImplicitSourceCoeffs
{
volumeMode absolute; // Values are given as <quantity>
//volumeMode specific; // Values are given as <quantity>/m3
injectionRateSuSp; // Semi-implicit source term S(x) = S_u + S_p x
{
h (103 0);
}
}
}
47

48 APPENDIX A. HEAT SOURCE WITH FVOPTION
A.1 Structure for OpenFOAM case
Figure A.1: Case structure for server

report

Recomendados

Recomendados

Más contenido relacionado

La actualidad más candente

La actualidad más candente (20)

Destacado

Destacado (6)

Similar a report

Similar a report (20)

report