Download - Arab Journal of Nuclear Sciences and Applications

Arab Journal Of Nuclear Science And Applications, 46(2), (276-286) 2013 

Experimental and CFD analysis of fluid flow and heat transfer in rod 

bundle geometry: I. steady state solution 

A. Salama, L.A. Shouman and A. Karameldin 

Reactor Departement, Nuclear Research Center, AEA, Egypt 

Received: 20/12/2012 Accepted: 29/1/2013 

ABSTRACT 

Experimental and CFD analysis was conducted to study steady state flow and 

heat transfer characteristics of a 4x4 square rod bundle. The experimental set up 

was designed to cover a variety of operating conditions and configurations. Data 

were collected using data acquisition. In this work we consider the steady state 

solution of the flow and heat transfer problem for this system. A 45o-sector of the 

square bundle was considered for CFD analysis. The shear-stress transport (SST) 

k 

model was chosen as the turbulence model, because it combines the power of 

the standard 

k in the main flow field and the standard 

276 

k model in the 

near wall regions. Fine meshes were considered in the boundary layer region to 

accurately capture the basic characteristics of the flow field. Comparisons between 

the measured inner clad temperatures and those simulated are in good agreement. 

Key Words: Steady state, forced convection, fluid flow, heat transfer, rod bundle geometry, the 

shear-stress transport (SST) 

k model 

INTRODUCTION 

Thermal hydraulics analysis is essential in order to evaluate safety features of nuclear reactors 

under various operating conditions. Because of the tremendous hazard associated with any 

malfunction in any of the essential working components of nuclear reactor systems, it is important to 

clearly understand the role of the different working circuits in relation to one another. The primary 

cooling system, for example, is responsible for cooling and moderating nuclear reactors cores. Any 

problem related to this particular system can cause serious damage to reactor’s core and consequently 

may lead to the release of radioactivity to the environment. Thus, it is important to study the behavior 

of nuclear reactors under different scenarios to shed light on the exact behavior of reactor systems. 

Thus, computational fluid dynamic techniques, CFD, can provide us with a valuable tool to 

comprehensively evaluate fluid dynamics behavior in nuclear reactors. However, several concerns 

related to the robustness of CFD modeling to a particular system can easily be raised. That is, without 

real comparison with measurements in similar systems, CFD results may be looked at with suspicion. 

Thus, it is important to build confidence in CFD modeling by comparing model’s results with 

measurements. In this context an experimental set up was constructed to evaluate the performance of a 

single, square fuel rod bundle of 4x4 fuel elements, as explained in the next section. The set up is 

capable of working under various steady state and transient conditions. Moreover, a CFD model was 

constructed to simulate the behavior of the system under the exact working conditions of the 

experimental set up. Thus by comparison with experiments, one would be able to build confidence in 

the resolution of the meshing technique as well as to suggest the appropriate turbulence model. Once 

this is done, the CFD model is expected be able to predict a variety of cases that was not included in 

the experimental set up and to be extrapolated to real system’s conditions.


THE EXPERIMENTAL SET UP 

The aim of the present experimental work was to study the effect of the thermal and hydraulic 

parameters on the fuel clad integrity of an electrically heated test section. This test section simulates a 

full square bundle of Egypt’s first research reactor (ET-RR1). A schematic diagram of the experimental 

set up with all its main components is shown in (Fig. 1). It is composed of two main loops namely the 

primary and secondary cooling circuits. In the primary loop, flow is induced in the fuel bundle (test 

section) downward through the plenum flange to the pump, through the ball valve, the orifice meter, 

the heat exchanger and finally to the lower plenum orifice flange where it flows upward in the core 

tube and back to the test section. In the secondary circuit, flow is induced by the circulating pump to 

the cooling tower, to the shell side of the heat exchanger and back to the pump. The core tube was mad 

of stainless steel with an inner diameter of 142 mm and a height of 940 mm. A manometer tapping was 

drilled at 700 mm from the base of the core tube and another tapping at about 750 mm from core tube 

base was constructed for thermocouples outlets. The coolant entrance and exit were located in the 

orifice flange (Fig.4) where they were separated by the test section body as shown in (Fig.1). The 

power header was constructed above the core tube to facilitate assembling and disassembling of the 

test section and its components and also to host the D.C. power grid to the heating elements within the 

test section. It was made of stainless steel tube of 148 mm in diameter and 185 mm in height. 

The square bundle consisted of the fuel rods, the upper grid and the lower grid (Fig.3). A set of 

16 rods of 10 mm outer diameter was used to simulate actual fuel rods. One of these rods, towards the 

center of the rod bundle, was instrumented with thermocouples for temperature measurements and was 

surrounded by 8 heating rods to mimic the ambient heating conditions of the instrumented rod. The 

other 7 rods were just used to provide the same hydraulic resistance in the actual square fuel bundle. 

The heating element (Fig. 2) was made of stainless steel and was machined to produce a heat 

generation function representing a distorted cosine with the maximum heat generation rate towards the 

lower half of the heating element. Direct electric current was supplied to the test section from a 100 

KVA electric power supply. Chromel-Alumel, type K thermocouples were used for temperature 

measurements. The thermocouple wires were 0.1 mm in diameter with each of its two wires wrapped 

with glass wool insulator. Moreover, the thermocouples were completely insulated from the DC power 

conducted to the heating rods as well as the cooling water. This was achieved by coating the 

thermocouples body and the junctions with a thin layer of a thermal paint to provide rapid response to 

temperature variations. The thermocouples were calibrated using the cold junction method and a third 

order polynomial was fitted to readily transform the measured voltage to temperature readings. The 

clad surface temperature distribution during steady state runes was determined by a set of nine 

thermocouples impeded at the outer surface of the insulator material between the heating element and 

the clad inner surface. 

The volumetric flow rate of the primary coolant circuit was measured using a standard 

calibrated sharp-edged orifice meter. The orifice plate was located around 110 cm away from the 

regulating valve to ensure fully developed flow conditions. Also the orifice meter was calibrated to 

relate the measured pressure drop across the orifice plate with the flow rate measurements. 

277


Fig.1. A schematic diagram of the experimental set up 

278


Fig. 2. Lower plenum orifice flange. 

Fig. 3. Sectional view of the test section. 

Fig.4. Sectional view of the heating element 

279


The data obtained from measuring instruments were collected and processed using data 

acquisition system. The raw data from measuring transducers are usually of low level and are thus 

prone to distortion. For example, the emf of the different thermocouples junctions was found to be 

ranging from 0 to 60.84 v/ o c (at 20 o c). A set of sequenced operations was introduced to make these 

signals amenable for recording in a computer. This includes amplifications, filtration, multiplexing, 

conversion to digital signal, demultiplexing, recording and finally processing. All these operations 

should take place in no time, hypothetically. However, there is indeed some time taken during these 

processes and if this time is larger than the time it takes for the physical phenomena to change, the 

automated measuring system will not be able to catch the actual changes of the studied phenomena. It 

is thus important to minimize these response times during each of the above mentioned processes. All 

cautions were taken to achieve this goal including the minimization of thermocouple diameter, the 

choice of a higher rate A\D converter, etc. After assembling the test rig, a cold run was carried out to 

check the consistency of the operating conditions, measuring devices and data acquisition system. 

MODELING APROACH 

The direct numerical solution of the momentum and energy equations in such a complex system 

which runs at moderately higher Reynolds number may not be attainable with the current available 

computing powers. The other alternative may be to adopt the RANS technique in order to make the 

system amenable to solution. In the RANS technique, one abandons the need for comprehensive, 

complete details of the instantaneous flow field and heat transfer, and is satisfied with the time 

averaged quantities that RANS determines. Albeit the fact that these averaged quantities provides us 

with somehow crude approximation to the real variables, they are, in most of our engineering 

applications, acceptable and can provide us with quite satisfying criteria for design purposes. The 

problem of using RANS approach, however, is that till now, there is no unifying set of equation to 

model all kinds of turbulent flows and heat transfer scenarios. The reason for this may be the fact that 

performing time averaging of the momentum and energy equations results in unclosed systems. In 

other words, the RANS equations contains terms that are related to the fluctuation components of the 

corresponding averaged quantities. There exist quite a number of models to close the system of 

equations and to propose relationships between the averaged fluctuating components and the mean 

field variables. On the other hand, since turbulence models are usually valid in the main flow field, 

special care need to be taken should there exist confining walls. The reason for that stems from the 

complex structure of the boundary layer in the vicinity of the confining walls. That is, while the flow 

in the main stream may be quite chaotic and turbulent, the flow right near to the wall is still laminar 

because of the viscosity effects. This layer, where viscous effects dominate inertial effects, is called the 

laminar sublayer and is confined closer to the wall boundaries. Right subsequent to this layer is a layer 

called the buffer zone in which a transition from laminar flow to the full turbulent flow is taking place. 

It is apparent that turbulence models are not applicable in this two regions and hence special treatment 

need to be devised. Two approaches are currently available to simulating the near-wall region. In the 

first approach, both the viscous sublayer and the buffer zone are not resolved and semi-empirical 

formulas are used to smoothly extend the turbulence models to wall. These formulas are called wallfunctions 

and they comprise law of the wall for mean quantities and formulas for near wall turbulent 

quantities. In the second approach, on the other hand, the turbulence models are modified in such a 

way as to be able to resolve the viscosity-affected region. The draw back of this approach, however, is 

that it requires a very fine mesh in the vicinity of the wall including nodes in the viscous sub layer. 

1-The choice of turbulence model. 

As stated earlier, the main focus of this research was to study the integrity of the clad material 

under different operating conditions. Hence, no measurements were taken to evaluate turbulence 

quantities (e.g., Reynolds stresses) that may help in suggesting the appropriate turbulence model. It 

280


was, thus, important to survey over the available turbulence models in terms of their criteria of 

applicability, limitations and restrictions in order to choose the one that might be appropriate to model 

this complex system. Moreover, literature surveys were conducted to explore on what other researcher 

have recommended for similar systems. It was found that substantial amount of research work have 

been done on rod bundle geometry using the standard k turbulence models over the past few 

decades for a recent in-depth review on CFD analysis on rod bundle geometries ( Tzanos 2001 (1) ). In 

general, there is a great deal of agreement between researchers that the standard k model may not 

be the turbulence model of choice in rod bundle geometries. On the other hand, most of these 

researches have considered periodic arrays of rods which allowed them to solving the flow in 

elementary sections and assuming symmetry across the boundaries (Rapley and Gosman 1986 (2) ; 

Baglietto and Ninokata, 2005 (3) ; and many others). However, as Chang and Tavoularis, 2007 (4) pointed 

out, this approach restricts the solution based on the fact that symmetry in geometrical configurations 

does not necessarily imply symmetry in the flow. In other words, simulating a full sector may be 

required to better capture the essential features of the flow field. It was reported the use of the shearstress 

transport (SST) k 

model to perform CFD analysis of flow field in a triangular rod bundle 

by Toth and Aszodi (2008) (5) . Chang and Tavoularis, 2005 (6) , on the other hand, used the unsteady 

Reynolds averaged Navier-Stokes equations supplemented by a standard Reynolds stress model to 

simulate the experimental work of Guellouz and Tavoularis 2000 (7) a,b and reported good agreement. 

In this work, we consider the use of the shear-stress transport (SST) 

Toth and Aszodi, 2008 (5) . Moreover, the two approaches to dealing with the near wall region were 

considered with the aim that if it is founded that the wall function approach provides reasonable 

approximation to the measured inner clad surface temperature, then it might be recommended for 

further investigation since it usually requires less computing resources. 

2-The Shear-Stress Transport (SST) 

k model 

281 

k model as suggested by 

k and SST models, which are basically two equation eddy-viscosity models, the 

In both the 

Reynolds stresses can be calculated from the eddy-viscosity hypothesis introduced by Boussinesq, 

(Pope, 2000 (8) ): 

2 

 

U 

uiu j k 

ij 

t 

3 

 

x 

j 

i 

U 

 

x 

i 

j 

 

 

 

 

As suggested by Menter, if it is possible to combine the standard 

shows to be relatively accurate if applied to the near wall region with the 

accurate in the far field, one may obtain a model that may be used in a variety of applications 

involving confining walls. This model is called the shear-stress transport 

basically the same formulation as the standard 

activate the 

region. In addition the definition of turbulent viscosity is modified to account for the transport of the 

turbulent shear stress. 

(1) 

k model, Wilcox, which 

k model which is also 

k model. It has 

k model but it includes blending function to 

k model in the near-wall region or the transformed 

k away from the wall 

In this model, the turbulent kinetic energy, k, and the specific dissipation rate, , may be 

obtained from the following transport equations (FLUENT, 2006 (9) ): 

k 

~ 

( k) 

( kui 

) ( 

k 

) Gk 

Yk 

S k 

(2) 

t 

xi 

x 

j 

x 

j


 

 

( ) ( u 

) 

G 

Y 

D 

S 

(3) 

 

 

i 

 

t xi 

x 

j x 

j 

where k 

G~ represents the generation of turbulence kinetic energy due to the mean velocity gradients, 

G the generation of , k 

and 

Y represents the dissipation of k and due to turbulence, 

S k , S 

are source terms. 

Now, k 

as 


 

t 

k , 

k 

represents effective diffusivity of k and , k 

282 

Y and 

D represents the cross-diffusion term, and 

represent the effective diffusivity of the k and , respectively, which are defined 

 

t 

with k 

 


are the turbulent Prandtl numbers and that is 

where the blending function is used to ensure that the model equations would work in both the nearwall 

and the far-field regions. 

On the other hand, the energy equation is modeled analogous to Reynolds treatment to 

turbulent momentum transfer. That is the energy equation as modeled in FLUENT takes the form: 

 

T 

E ui 

E p 

 

( ) [ ( )] keff 

u 

i ( ij ) eff S h 

(4) 

t 

xi 

x 

 

j x 

j 

k is the effective thermal conductivity, and eff 

( is the deviatoric 

Where E is the total energy, eff 

stress tensor. This term represents the irreversible dissipation of kinetic energy to heat energy. 

Moreover, the unified wall thermal treatment blends the laminar and logarithmic profiles according to 

the method of Kader (1981 (10) ) in which the convective heat flux is calculated as, (Koncar et al. 2005) 

C u 

q 

L pL W 

( TW 

T 

l, 

( nw) 

T 

y ( L) 

Here ) 

l, 

( nw 

) 

T is the liquid temperature in the near-wall computational cell, 

dimensional temperature at the non-dimensional distance from the near-wall cell, 

friction velocity. 

3-Mesh sensitivity analysis 

ij ) 

 

 

y (L) 

(5) 

T is the non- 

 

y nw and w 

u is the 

In this work we consider two kinds of meshes, in the first one both the viscous sublayer and the 

buffer zone are not resolved and hence wall function technique was assumed. Although this meshing 

strategy is considered coarse, it is amid at giving a rough estimation on the axial clad temperature 

profile based on the availability of less computing resources. In the other approach, a very fine mesh 

in the neighborhood regions of heating rods and basket wall were assumed. As Toth and Aszodi 

(2008 (8) 

) reported in their work that meshes with average y of approximately 1 and 20.1 were 

acceptable to capturing the basic flow field characteristic. Hence, meshes which are very fine near the 

wall may be difficult to implement, particularly for complicated, larger geometries. In this work, 

however, we consider a mesh with 

opportunity to get accurate estimation of the flow field at reasonable cost in terms of computing 

resources in addition to the fact that, this work is not primarily aiming at examining processes in the 

y in the order of 5. It is believed that this will also give us the

viscous sub-layer. 


Fig. 5-a,b show cross sectional grids for 45 o -sector of the complete rod bundle with Fig.5-a 

shows the coarse mesh and Fig.5-b represents the finer mesh. Fig. 6, on the other hand, shows the 3D 

mesh of a sectional cut of the simulated sector. 

RESULT AND DISCUSSION 

The steady state simulation was performed on a windows-based personal computer with Intel 

Quad dual processor. The commercial CFD code FLUENT 6.2.12, which solves the governing 

equations by the finite volume approach, was used for simulation. The convective terms were 

discretized using a second-order upwind scheme. The pressure field was coupled to the velocity field 

by the SIMPLE algorithm. Also, the energy equation was discretized by a second-order upwind 

scheme. Flow convergence was considered achieved when the residuals for all flow variables reaches 

lower than 10 -4 . Pressure inlet and outlet boundary conditions were set for the inlet and outlet sections, 

respectively, with the pressure gradient adjusted to match the desired mass flow rate. The side faces, 

on the other hand were considered symmetry faces. The present simulations were validated by 

comparing the measured inner clad surface temperatures with the result of simulation. As indicated 

earlier, the instrumented rod, which is the one near the centerline of the square bundle, was equipped 

with a set of 8 thermocouples impeded into the insulating material to measure the inner clad surface 

temperature. Temperature contours is shown in Fig 7. It is apparent that the hot spots are almost 

towards the lower half of the heating elements. Fig. 8, on the other hand, shows the comparison 

between measured inner clad surface temperatures with that simulated. The simulated, axial-wise 

average inner clad temperatures were extracted using a UDF. As the figure shows, quite good 

agreement is obtained between measurements and simulation which provide confidence in the 

modeling approach. It is apparent that the maximum inner clad surface temperature is shifted towards 

the center of the lower half of the heating element following the general trend of the heat generation 

function adapted to the heating elements. Fig. 9, also, depicts the axial average temperature variations 

at the surface of the heating element, and at the clad inner and outer surfaces. One can notice that there 

is a very little temperature drop within the clad material because of the higher thermal conductivity of 

its material. Velocity vector field at the plane z = 0.125 is shown in Fig. 10. It is apparent that the 

maximum velocity is at the middle of the gaps between heating rods. 

Fig. 5a. cross sectional grids for 45 o -sector 

( the coarse mesh ) 

283 

Fig. 5b. cross sectional grids for 45 o -sector (the 

finer mesh)


Fig.6. The 3D mesh of a sectional cut of the 

simulated sector. 

284 

Fig. 7. Temperature contours of the inner clad 

surface

T emperature, c 


160 

140 

120 

100 

80 

60 

40 

20 

0 

P ower 100% 

0 0. 1 0. 2 0. 3 0. 4 0. 5 0. 6 

Dista nc e from bottom, m 

285 

Measur ed 

SST- Si mul at ed 

Fig. 8. The comparison between measured inner clad surface temperatures and simulated. 

Fig. 9. the axial average temperature variations at the surface of the heating element, and at the 

clad inner and outer surfaces


Fig. 10. Velocity vector field at the plane z = 0.125 

REFERENCE 

k turbulence models in the simulation of LWR fuel-bundle 

1- Tzanos, C. 2001, Performance of 

flows, Trans. ANS 84, pp. 197-199. 

2- Rapley, C.W., and Gosman, A.D., 1986, The prediction of fully developed axial turbulent flow in 

rod bundles, Nuclear Engineering and Design, 97, pp. 313-325. 

3- Baglietto, E., and Ninokata, H., 2005, A turbulence model study for simulating flow inside tight 

lattice rod bundles. Nuclear Engineering and Design, 235, pp. 773-784. 

4- Chang, D., and Tavoularis, S., 2007, Numerical simulation of turbulent flow in a 37- rod bundle, 

Nuclear Engineering and Design, 237, pp 575-590. 

5- Toth, S. and Aszodi, A., 2008, CFD analysis of flow field in a triangular rod bundle, Nuclear 

Engineering and Design, 

6- Chang, D., and Tavoularis, S., 2005, Unsteady numerical Simulation of turbulence and coherent 

structures in axial flow near narrow gap. J. fluid Engineering, 127, pp 458-466. 

7- Guellouz. M, and Tavoularis, S., 2000, The structure of turbulent flow in rectangular channel 

contaning a cylindrical rod- part 1. Renolds averaged measurements, Exp. Thermal fluids, 23, pp 59- 

73. 

8- Pope, S., 2000, Turbulent flows, Cambridge university pres. 

9- Chang, D., and Tavoularis, S., 2008, Simulation of turbulence, heat transfer and mixing across 

narrow gaps between rod-bundle subchannel, Nuclear Engineering and Design, 238, pp 109-123. 

10- Kader, B.A., 1981, Temperature and concentration profiles in fully turbulent boundary layers, Int. 

J. Heat Mass Transfer 24, 1541-1544. 

286

Download - Arab Journal of Nuclear Sciences and Applications

Create successful ePaper yourself

Delete template?

Save as template?