Group Title: 7th International Conference on Multiphase Flow - ICMF 2010 Proceedings
Title: 10.4.2 - Numerical Simulation of Air-Water Counter-current Two-phase Flow in a Model of the Hot-leg of a Pressurized Water Reactor (PWR)
ALL VOLUMES CITATION THUMBNAILS PAGE IMAGE ZOOMABLE
Full Citation
STANDARD VIEW MARC VIEW
Permanent Link: http://ufdc.ufl.edu/UF00102023/00256
 Material Information
Title: 10.4.2 - Numerical Simulation of Air-Water Counter-current Two-phase Flow in a Model of the Hot-leg of a Pressurized Water Reactor (PWR) Computational Techniques for Multiphase Flows
Series Title: 7th International Conference on Multiphase Flow - ICMF 2010 Proceedings
Physical Description: Conference Papers
Creator: Deendarlianto, A.
Höhne, T.
Lucas, D.
Vallée, C.
Publisher: International Conference on Multiphase Flow (ICMF)
Publication Date: June 4, 2010
 Subjects
Subject: numerical simulation
CFD
Counter-current flow limitation (CCFL)
Pressurized water reactor (PWR)
Algebraic interfacial area density (AIAD) model
 Notes
Abstract: In order to validate newly developed multiphase flow models in the code ANSYS CFX, a CFD simulation of the counter-current two-phase flow of 1/3rd scale model of the hot leg of a German Konvoi Pressurized Water Reactor with rectangular cross section was performed. A selected air-water Counter-current flow limitation (CCFL) experiment of Forschungszentrum Dresden-Rossendorf (FZD) at 0.153 MPa and room temperature was simulated with three-dimensional two-fluid Euler-Euler models of computer code CFX 12.0 (ANSYS CFX). The calculation was carried out in fully transient manner using a gas/liquid inhomogeneous multiphase flow model coupled with a shear stress transport (SST) turbulence model. In the simulation, the drag coefficient was approached by the Algebraic Interfacial Area Density (AIAD) model. The results indicated that quantitative agreement of the CCFL characteristics between calculation and experimental data was obtained. Next, a comparison with the high-speed video observations shows also a good qualitative agreement.
General Note: The International Conference on Multiphase Flow (ICMF) first was held in Tsukuba, Japan in 1991 and the second ICMF took place in Kyoto, Japan in 1995. During this conference, it was decided to establish an International Governing Board which oversees the major aspects of the conference and makes decisions about future conference locations. Due to the great importance of the field, it was furthermore decided to hold the conference every three years successively in Asia including Australia, Europe including Africa, Russia and the Near East and America. Hence, ICMF 1998 was held in Lyon, France, ICMF 2001 in New Orleans, USA, ICMF 2004 in Yokohama, Japan, and ICMF 2007 in Leipzig, Germany. ICMF-2010 is devoted to all aspects of Multiphase Flow. Researchers from all over the world gathered in order to introduce their recent advances in the field and thereby promote the exchange of new ideas, results and techniques. The conference is a key event in Multiphase Flow and supports the advancement of science in this very important field. The major research topics relevant for the conference are as follows: Bio-Fluid Dynamics; Boiling; Bubbly Flows; Cavitation; Colloidal and Suspension Dynamics; Collision, Agglomeration and Breakup; Computational Techniques for Multiphase Flows; Droplet Flows; Environmental and Geophysical Flows; Experimental Methods for Multiphase Flows; Fluidized and Circulating Fluidized Beds; Fluid Structure Interactions; Granular Media; Industrial Applications; Instabilities; Interfacial Flows; Micro and Nano-Scale Multiphase Flows; Microgravity in Two-Phase Flow; Multiphase Flows with Heat and Mass Transfer; Non-Newtonian Multiphase Flows; Particle-Laden Flows; Particle, Bubble and Drop Dynamics; Reactive Multiphase Flows
 Record Information
Bibliographic ID: UF00102023
Volume ID: VID00256
Source Institution: University of Florida
Holding Location: University of Florida
Rights Management: All rights reserved by the source institution and holding location.
Resource Identifier: 1042-Deendarlianto-ICMF2010.pdf

Full Text

7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010


Numerical simulation of air-water counter-current two-phase flow
in a model of the hot-leg of a pressurized water reactor (PWR)


Deendarlianto, Thomas H6hne, Dirk Lucas and Christophe Vallee

Forschungszentrum Dresden-Rossendorf e.V., Institute of Safety Research,
P.O. Box 510 119, D-01314 Dresden, Germany.
Email: d.deen@fzd.de

Keywords: Numerical simulation, Computational fluid dynamic, Counter-current flow limitation (CCFL),
Pressurized water reactor (PWR), Algebraic interfacial area density (AIAD) model


Abstract

In order to validate newly developed multiphase flow models in the code ANSYS CFX, a CFD simulation of the
counter-current two-phase flow of 1/3rd scale model of the hot leg of a German Konvoi Pressurized Water Reactor with
rectangular cross section was performed. A selected air-water Counter-current flow limitation (CCFL) experiment of
Forschungszentrum Dresden-Rossendorf (FZD) at 0.153 MPa and room temperature was simulated with three-dimensional
two-fluid Euler-Euler models of computer code CFX 12.0 (ANSYS CFX). The calculation was carried out in fully transient
manner using a gas/liquid inhomogeneous multiphase flow model coupled with a shear stress transport (SST) turbulence
model. In the simulation, the drag coefficient was approached by the Algebraic Interfacial Area Density (AIAD) model. The
results indicated that quantitative agreement of the CCFL characteristics between calculation and experimental data was
obtained. Next, a comparison with the high-speed video observations shows also a good qualitative agreement.


Introduction

The counter-current gas-liquid two-phase flow in the hot
leg of a pressurized water reactor (PWR) has received a
special attention for the nuclear reactor safety. One
hypothetical scenario is a loss-of-coolant-accident (LOCA)
in a PWR, which is caused by the damage at any position
of the primary circuit. During this scenario, it is considered
that the reactor will be depressurized and that vaporization
takes place. If the water level in the reactor falls below the
inlet nozzle of the hot leg, the saturated steam generated in
the reactor will flow through the hot leg and condense in
the steam generator.

In the reflux condenser mode, a part of the condensate will
flow back to the reactor core in counter-current to the
steam flow. The counter-current flow of steam and
condensate is only stable for a certain range of mass flow
rates. If the steam mass flow rate increases too much, the
condensate is clogged in the hot leg. Next, the condensate
is carried over by the steam and partially entrained in the
opposite direction to the steam generator. This
phenomenon is known as the counter-current flow
limitation (CCFL) or flooding, and could affect the cooling
of the reactor core. The detailed examples of such LOCA
scenarios leading to the reflux condenser mode can be
found in Jeong (2002).

There were a lot of experiments done to analyze and
understand the CCFL phenomena in a model of hot leg
PWR. Several experimental correlations were developed to
predict the CCFL on them, but they are valid only in
specified their experimental ranges (Deendarlianto et al.,
2008). Therefore, high resolution experimental data at


reactor typical boundary conditions is needed. In order to
improve the transient analysis of counter-current
two-phase flows, experimental studies were conducted at
Forschungszentrum Dresden-Rossendorf (FZD). A 1/3rd
scale model of the hot leg PWR of a German Konvoi
Pressurized Water Reactor with rectangular cross section
was used (Deendarlianto et al., 2008 & Vall6e et al.,
(2009).

The analytical simulation of this phenomenon is also an
essential element to understand safety-related issues in
nuclear power plants. The widely used analysis to model
the counter-current flow limitation in a model of hot leg
PWR is the used of the one dimensional two-fluid models
as reported by Ardron & Banerjee (1986), Bertadano
(1994) and Wongwises (1996). The switching point, where
the flow condition changes from sub to critical condition in
stratified flow was approached by the experimental
correlation in a specified flow direction. Therefore, the
simulated liquid flow does not split as observed in the
experiments (Kolev et al., 2001). Next, the use of this
empirical correlation is also far from the physic of the flow
phenomenon. In particular the CCFL conditions are
dominated by 3D effect, consequently, requires the use of
CFD approach. It is expected that the introduction of
computational fluid dynamics (CFD) tools will enhance
the accuracy of the simulation predictions compared to the
established one-dimensional thermal hydraulic analyses.

Wang & Mayinger (1995) simulated two-dimensional
analysis of counter-current model of UPTF Test A2 & Test
11 using a two-fluid model. They implemented the
interfacial friction factor proposed by Lee & Bankoff
(1983) and Ohnuki (1986) into the code FLOW3D. They









reported that satisfactory results were obtained, whereas,
under the reflux condensation conditions, numerical
computation reveals that different flow structures appeared
in the region away from flooding curve and in the region
near the flooding curve. Next, Minami et al. (2009) and
Murase et al. (2009) conducted a three dimensional CFD
simulation on the counter-current gas-liquid flow in a PWR
hot-leg air-water flow in a 1/15th scale model. They
implemented the VOF model on the commercial CFD code
FLUENT. In their simulations, the interfacial friction
factors were adopted from the empirical correlations
obtained from literatures for the cases of annular and slug
flow. Those correlations were obtained on the basis of one
dimensional analysis, which might affect the calculation
results; therefore, the accuracy of their CFD simulation
might limit to their experimental data.

This paper further provides a numerical study of the
air-water CCFL phenomena on the 1/3rd scale model of the
hot leg PWR of a German Konvoi PWR with rectangular
cross section under the FZD experimental condition. The
aim of this simulation is the validation of prediction of
CCFL in a model hot leg PWR with newly developed and
implemented multiphase flow models in the code ANSYS
CFX. In order to improve the physical meaning of this
CFD calculation, we have implemented the Algebraic
Interfacial Area Density (AIAD) model to solve the
Euler-Euler inhomogeneous mixture model available in
ANSYS CFX code. The drag coefficient obtained from this
model considered the 3D effects of the simulated
phenomenon. That is the gradients of gas/liquid velocities
between the phases in the direction of axis x,y,z, as an
example. Next, the effect of the change of flow
morphological as the function of volume fraction was also
considered in this model.

Nomenclatures
A Interfacial area density (m 1)
CD Drag coefficient (-)
d Diameter (m)
FD Interfacial friction force (N)
f Blending function (-)
g Gravitational constant (ms-1)
H Channel height (m)
Jk* Non dimensional superficial velocity by Wallis
(-)
p Pressure (Nm-2)
U Velocity (ms-1)

Greek letters
a Void fraction (-)
p Density (kg/m3)
p. Dynamic viscosity (Pa.s)
y Viscosity (Pas)
r Shear stress IN Imi

Subsripts
B Bubble
D Droplet
FS Free surface
G Gas phase
k Gas or Liquid phase
L Liquid phase


7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010

Experimental Apparatus & Procedures

The details of the experimental apparatus and procedure
used in the present study were described in the previous
papers (Deendarlianto et al., 2008 & Vall6e et al. 2009)
and only the main features are presented here. Figure 1
shows a diagram of the experimental facility. Two vessels
simulate the reactor pressure vessel (RPV) simulator and
steam generator (SG) separator are connected by a test
section that simulates the 1/3rd scale model of the hot leg
PWR of a German Konvoi Pressurized Water Reactor.
Both the RPV simulator and SG separator are identical
vessels with 0.8 m x 0.5 m x 1.55 m (D x W x H) cubic
shape. The water levels in both vessels were determined by
the measurement of the differential pressure between the
top and the bottom of the vessels with differential pressure
transducers. A vortex meter was used to measure the
injected water mass flow rate. The injected air mass flow
rate was measured and controlled using a thermal mass
flow meter.


Figure 1: Schematic diagram of the experimental apparatus
(dimension: in mm)

The test section is composed of a horizontal rectangular
channel, a bend that connects it to an upward inclined and
expended channel, and a quarter of a circle representing
the steam generator inlet chamber. The horizontal part of
test section is 2.12m long and has a rectangular
cross-section of 0.05 m x 0.25 m. The riser is 0.23 m long,
has an inclination of 50 to the horizontal plane and an
expansion angle of 7.5. The inner and outer bend radii of
curvature were 0.25 and 0.5 m, respectively. The test
section was made of stainless steel and was equipped with
glass windows to allow visual observation. The flow
behavior was recorded by a high-speed video camera at
frequencies of 60-100 Hz and a shutter speed of 1/1000 s.

In the experiment, a constant water flow rate was injected at
the bottom of the SG simulator from where it can flow
through the test section to the RPV simulator. The gas was
injected into the RPV simulator from the top and flowed
through the test section in counter-current to the water flow
to the SG separator. The increase of the water level in the
RPV simulator was used to determine the water flow rate
streaming over the test section (discharge flow). The onset
of flooding was defined as the limiting point of stability of
the counter-current flow, indicated by the maximum air
mass flow rate at which the down-flowing water mass flow
rate is equal to the inlet water mass flow rate.

This experimental apparatus is put in a pressure chamber,


air oulet




steam
gcearator
separator









where it was operated in pressure equilibrium with the
inner atmosphere of the tank. A compressor system allows
an increase of the air pressure in the chamber to a
maximum operation pressure of 5 MPa mainly for the
steam-water but here is of 0.153 MPa. The detailed
principle of the pressure equilibrium technique was
described by Prasser et al. (2006).


Physical & Numerical Model

In the present numerical study, both phases are assumed
adiabatic and incompressible. The flow is treated as
transient. Using the two-fluid model, general conservation
equations for mass and momentum can be respectively
given as:


( + V(akkUk) = 0 (1)



+(ap V(apUkUk)= -akVp, + apg +
dt (2)
+ Vak(r +T)+ D

where the subscript k denotes phase gas or liquid, p is the
density, u is the velocity vector, t is the time, p is the
pressure, g is the gravitational acceleration, a is the volume
fraction, ris the shear stress (f is the average viscous shear
stress, i is the turbulent shear stress) and TD is the interfacial
shear stress.

In simulation of CCFL phenomenon, the air bubble in the
water can be resulted by the drag force. The total drag force
is derived from the interfacial shear stress ( F = -D .A), is
most conveniently expressed in terms of the dimensionless
drag coefficient CD


7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010

momentum models. The separate models are also
necessary for dispersed particles and separated continuous
phases interfaciall drag etc.).

The suitable methodology within the Euler-Euler approach
is to use the momentum exchange coefficient depends on
the local morphology. For that reason, Yegorov (2004)
proposed an Algebraic Interfacial Area Density (AIAD)
model to solve the above problem. The basic conceptions
of the proposed model are:
The interfacial area density allows the detection of the
morphological form and the corresponding switching
for each correlation from one object pair to another.
It provides a law for interfacial area density and the
drag coefficient for full range 0 The interfacial area density in the intermediate range
is set to the interfacial area density for the free
surface.

The interfacial area density A also depends on the
morphology of the phases. For bubbles, the interfacial
area density is defined as follows


6aG
AB- =


Here dB is the bubble diameter and aG is the gas void
fraction. For a free surface, the interfacial area density is
defined as absolute value of the gradients of the liquid
fraction in x, y and z directions, and is written as


A =V = + \ + (5)
Nex, x Savy a z

Next, the average density pLG is defined as


PLG =PGa + L (1- )


FD = CD A PLG(UL UG)


where PLG is the average density, \(U, U )| is the relative
velocity and A is the projected area of the body in flow
direction / interfacial area density. In the present simulation,
CD is determined by using the Algebraic Interfacial Area
Density (AIAD) model and will be discussed later.


Free Surface & AIAD Model

Generally for the CFD modelling of large hydrodynamic
configurations with multiphase flow, the Euler-Euler
approach is used. In the previous experimental paper
(Deendarlianto et al., 2008) reported that there are three
morphologies at CCFL condition. Those are bubble flow,
stratified flow with a free surface and entrainment liquid
droplet. HOhne and Vall6e (2009) noted that the CFD
simulation of the free surface can be performed by using
the multi-fluid Euler-Euler modelling approach available in
ANSYS CFX. However it requires a careful treatment of
several aspects of the model. Those are interfacial area
density, turbulence model near free surface and inter-phase


where PL and pG are the liquid and gas densities,
respectively. In the bubble regime, where the a is low,
the average density according to Eq. (6) is close to liquid
phase density PL. According to the flow regime (bubbly
flow, droplet flow or stratified flow with a free surface),
the corresponding drag coefficients and area densities
have to be applied. This problem can be solved by
introducing a blending function f. Introducing void
fraction limits, the blending function and length scales for
bubbly and droplet regimes are respectively defined as


1
1+ eAB(I a G-aBimit)
1
fD
1D eAD(aG-aDimit)


Next, the blending function for the free surface is defined
as
fFs =1- f, fD (9)

Then, the area density and the drag coefficient are









respectively well defined in the domain by


7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010

of 248,610 hexahedral elements and 281,076 nodes.


A = fF AFS + fA, + fDAD


CD = fFSCD.FS + fBCD.B + fDCD.D


Ai vtocty urm arfsw


Normal vectors at
the free surface


Figure 3: Calculation meshes


Figure 2: Air velocity near the free surface (Hohne, 2009)

In simulation of free surface flows, Eq. (3) does not
represent the physics in the right way. It is reasonable to
expect that the velocities of both fluids in the vicinity of
the interface are rather similar. Hohne (2009) extended the
AIAD model to determine the drag coefficient of the free
surface. In their proposal, a shear stress like a wall shear
stress is assumed near the surface from both sides to
reduce the velocity differences of both phases as shown in
Fig. 2. Here, a viscous fluid moving along a "solid" like
boundary will incur a shear stress, the no-slip condition,
the morphology region "free surface" is the boundary
layer, the shear stress is imparted onto the boundary as a
result of this loss of velocity.


y~o


Finally, the drag coefficient of the free surface can be
obtained from the substitution of the Eqs. (5) and (12) and
is locally dependent on the fraction of both phases, liquid
density, and the slip velocity between the phases.


2(Lz-, +az-)
CD,FS -2(,L 2
PL U slp


where wall shear stresses of the gas and liquid zL and G
onto the free surface are a function of the viscosity of both
phases, the area of free surface and the gradient of void
fraction in x,y,z axes.:

In the simulation, the drag coefficient of the bubble, a
constant value of CD,B=0.44 is taken, based on the drag of
rigid spheres at the medium to high Reynolds number
regime. For the drag coefficient of the droplet, the
CD,D=0.44 is also taken. On the other hand, the drag
coefficient of the free surface, CD,FS, refers to Eq. (13).


Boundary Conditions

We have simulated the air-water CCFL phenomenon in a
hot-leg of PWR with Euler-Euler inhomogeneous mixture
model using a commercial CFD code of ANSYS CFX 12.0.
The calculation model is shown in Fig. 3. The grid consists


- 0.25 -


0.20 -


0.15



0 20 40 60 80 100
time [s]
Figure 4: Injected air mass flow rate as a function of time
of the experimental run of 30-09

An air-water CCFL experiment of experimental running
30-09 was chosen for the CFD calculation. The important
boundary conditions are as follows. The injected water
mass flow rate was constant of 0.283 kg/s. The system
pressure was 0.153 MPa. The injected air mass flow rate
used in the present calculation was a function of time as
shown in Fig. 4. It has six (6) levels of air mass flow rate
of 100 s of simulation time, ranges from 0.18 to 0.27 kg/s.
Both phases have treated as isothermal and incompressible,
at 25 'C and at a reference pressure of 0.153 MPa.
Buoyancy effects between the two-phase were taken into
account by the direction of gravity term. The turbulence
properties at the inlet of air and water were set using the
"turbulence intensity of 5% in both phases". The air outlet
was modelled with an opening boundary condition. The
inner surface of the channel walls has been defined as
hydraulically smooth with a non-slip boundary condition
applied to both gas and liquid phases. The SST turbulence
model and Upwind advection scheme were used in the
simulation. Drag coefficient, CD, was determined by the
AIAD model (Eq. (13)), and its implementation into CFX
was done via the command language CCL (CFX
expression language) and User FORTRAN Routines.

A time step 10-4 s and a maximum of 15 coefficient loop
were taken to model the flow. A convergence in terms of
the RMS values of the residuals to be less than 10-4 could
be assured most of the time. In order to simulate transient
calculation of 100 s of simulation time, four months of
calculation was required, whereas the simulations were
performed in parallel of 4 processors of FZD Linux cluster.






7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010


Results & Discussions

Figure 5 shows the calculated result of the average water
level inside the RPV simulator and the experimental data
of the stepwise increase of the injected air mass flow rate.
The water level and injected air mass flow rate are shown
by the blue and pink curves respectively. From this figure,
the phenomena can be explained as follows.


Region2 Regi.ni


Zero liquid

peiufratrn


0.30




0.20




0.10 1
'*


0.03 'L I. .' J 0.00
0.0 20.0 40.0 60.0 80.0 100.0
time [s]
Figure 5: Time variation of the calculated result of water
level in the RPV simulator (blue curve), and the
experimental data of the injected air mass flow rate (pink
curve) under a constant water mass flow rate of 0.283 kg/s.

1. The water level is divided into three regions. In the
first region, the water level in the RPV simulator
increases with a constant slope as air mass flow rate
increases. In the second region (at t=56 s and the
injected air mass flow rate of 0.232 kg/s), the slope of
the curve of water level in the RPV simulator begins to
decrease. It means that a part of the water injected in
the SG separator do not flow to the side of the RPV
simulator. This point is known as the onset of
flooding. From the figure, it shown also that around
the onset of flooding, there is a rapid fluctuation of the
water levels in RPV. It corresponds to the local
instability phenomenon, such as the entrainment of
liquid droplet in the interface of gas-liquid and wave
oscillations caused of the strong collision between the
interface of gas/liquid and the incoming liquid from
the hot-leg, due to the un-continue of the transported
liquid to the RPV simulator.
2. With further increasing of the air mass flow rate up to
0.26 kg/s (t=89 s), the calculated water level shows a
plateau (region 3). This means that all the injected
water in SG separator do not flow to the side RPV
simulator.
3. The characteristic of the water level described above
seems to confirm the experimental observations of
Deendarlianto et al. (2008). They defined the region 1,
region 2, and region 3 as the stable counter-current
flow, partial delivery region and zero penetration
respectively.


(a) Calculatedrwater volume fraction


(b) Visual observation obtained from experiment


Water Velocity Vector 1
[ms~l]
S1.548a+001

1 161e+0no


7.742e+000


3.871+0ooo0 Water

O.OOOe+00 /

ir


*
41%


(c) Calculated water velocity profile

Figure 6: Flow structure of the counter-current air-water
two-phase flow near the elbow near the elbow at t=5 s
(mG= 0.181 kg/s)


Figure 6 illustrates the flow structure of the counter-current
air-water two-phase flow near the elbow at t=5 s, thus
representing the flow structure at low air mass flow rate
(mG =0.181 kg/s) or before the onset of flooding. In the
figure, (a), (b) and (c) corresponds respectively to the
calculated water volume fraction, the visual observation
obtained from the experiment, and the calculated water
velocity profile. From Fig 6(a), the thin liquid film was
found in the bend region. Next, the flow pattern is a
supercritical stratified flow and a hydraulic jump as the
transition from supercritical to subcritical flow is observed
near the bended region, which agrees well with the
experimental observation shown in Fig. 6(b). In addition,
Fig 6 (c) indicates that both water and air flow in the
difference direction and a small water circulation (roll
wave) at the hydraulic jump locus is clearly visible.


Region




The oset offlooding


0.15



0.12



0.09



0.06






7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010

respectively to the time variation of the calculated water
volume fraction (At=0.1 s), the visual observation obtained
from the experiment, and the calculated water velocity
profile. Fig 7 (a) shows a bigger wave is generated by the
merging of small waves due to the interfacial drag. In
comparison between Fig. 7 (a) and 7 (b), it is noticed that
the computation agrees well with the experiment. In
addition, some part of water flows in the same direction
with the air, and a big roll wave is observed near the bended
region as shown in Fig. 7 (c).

Finally, a comparison of the CCFL characteristics between
the CFD calculation and experiment is shown in Fig. 8. For
a meaningful comparison, the non-dimensional superficial
velocity Jk', namely as Wallis parameter, is used to plot the
CCFL characteristics. Here the Wallis parameter in Fig. 8
is defined as follows.


1 pk
Jk ,H(pI-pc)
gH (p, pG


where H is the height of the channel. Close inspection of
Fig. 8, it is shown that the calculated CCFL points of the
CFD simulation are in good agreement with those from
experiment.


(a) (b)


0.2 -
0.00


11uter


Air


(c)
Figure 7: Flow behaviour during the counter-current
air-water two-phase flow flow near the elbow at high air
mass flow rate ( m =0.268 kg/s); (a) calculated water
volume fraction, (b) Visual observation obtained from
experiment, and (c) calculated water velocity profile


Figure 7 illustrates the flow structure of the counter-current
air-water two-phase flow near the elbow at high air mass
flow rate ( m =0.268 kg/s) or in the flooded regime (region
3 in the Fig.5). In the figure, (a), (b) and (c) corresponds


0.05
(JL*)1/2 [-


Figure 8: Counter-current flow limitation characteristics


Conclusions

Three-dimensional CFD simulations of the CCFL
phenomenon of air-water two-phase flow in a model of hot
leg a German Konvoi Pressurized Water Reactor with
rectangular cross section have been performed using the
Euler-Euler inhomogeneous mixture model. A selected of
air-water CCFL of FZD experiment was chosen for the
CFD simulation. The simulation was conducted in fully
transient manner. An Algebraic Interfacial Area Density
(AIAD) model on the basis of the implemented mixture
model was implemented. A picture sequence recorded
during the CCFL experiment was compared with CFD
simulation of the commercial code of ANSYS CFX 12.0.
The calculated results of the velocity profile and water
volume fraction indicate that the basic flow characteristics


-*- Experiment
-*- CFD simulation





-------

~i









of the experiment such as the hydraulic jump near the
bended region of the hot leg PWR and the occurrence of
slug flow were reproduced in simulation, while the
deviations require a continuation of the work. In addition,
the calculated CCFL points were also in an agreement with
the experiments.


Acknowledgements

This work is carried out within the frame work of a current
research project funded by the German Federal Ministry of
Economics and Technology, project number 150 1329.

Dr. Deendarlianto is an Alexander von Humboldt Fellow in
the Institute of Safety Research, Forschungszentrum
Dresden-Rossendorf e.V., Germany. The present research
is also supported by the Alexander von Humboldt
Foundation in Germany.


References

Ardron, K.H., and Baneerjee, S., Flooding in an Elbow
between a Vertical and a Horizontal or Near Horizontal
Pipe; Part II: Theory. International Journal of Multiphase
Flow, Vol. 12-4, pp. 543-558 (1986)

Bertadano, M.L., Counter-current Gas-liquid Flow in a
Pressurized Water Reactor Hot Leg. Nuclear Science and
Engineering, Vol. 117, pp. 126-133 (1994)

Deendarlianto, Vall6e, C., Lucas, D., Beyer, M., Pietruske,
H., Carl, H., Experimental Study on the Air/water
Counter-current Flow Limitation in a Model of the Hot
Leg of a Pressurized Water Reactor. Nuclear Engineering
and Design, Vol. 238-12, pp.3389-3402 (2008)

HOhne, T., Experiments and Numerical Simulations of
Horizontal Two-phase Flow Regimes, In: Proceeding of
the Seventh International Conference on CFD in the
Minerals and Process Industries, Melbourne, Australia
(2009)

HOhne, T., and Vall6e, C., Numerical Predicition of
Horizontal Two Phase Flow using an Interfacial Area
Density Model. In: Proceeding of the 13th International
Topical Meeting on Nuclear Reactor Thermal Hydraulics
(NURETH-13), Kanazawa, Japan (2009)

Jeong, H.Y., Prediciton of Counter-current Flow Limitation
at Hot Leg Pipe during a Small Break LOCA. Annals of
Nuclear Energy, Vol. 29-5, pp. 571-583 (2002)

Kolev, N.I., Seitz, H., Roloff-Block, I., Hot-leg injection:
3D versus 1D Three Velocity Fields Modelling and
Comparison with UPTF Experiment. In: Proceeding of the
4th International Conference on Multiphase Flow, New
Orleans, USA (2001)

Lee, S.C., and Bankoff, S.G., Stability of Steam-water
Counter-current Flow in an Inclined Channel: Flooding.
Journal of Heat Transfer, Vol. 105, pp. 713-718 (1983)


7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010

Minami, N., Utanohara, Y., Kinoshita, I., Murase, M.,
Tomiyama, A., Numerical Calculations on Counter-current
Gas-liquid Flow in a PWR Hot Leg (1) Air-water Flow in a
1/15th Scale-model. In: Proceeding of the 13th International
Topical Meeting on Nuclear Reactor Thermal Hydraulics
(NURETH-13), Kanazawa, Japan (2009)

Murase, M., Utanohara, Y., Kinoshita, I., Minami, N.,
Tomiyama, A., Numerical Calculations on Counter-current
Air-water Flow in Small Scale Models of a PWR Hot Leg
Using a VOF Model. In: Proceeding of the 17th
International Conference on Nuclear Engineering ICONE
17, Brussels, Belgium (2009)

Ohnuki, A., Experimental Study on Counter-current
Two-phase Flow in Horizontal Tube Connected to Inclined
Riser. Journal of Nuclear Science and Technology, vol. 23,
pp. 219-232 (1986)

Prasser, H.M., Beyer, M., Carl, H., Manera, A., Pietruske,
H., Schutz, H., Weiss, F.P., The Multipurpose Thermal
Hydraulic Test Facility TOPFLOW: an Overview on
Experimental Capabilities, Instrumentation and Result.
Kerntechnik, Vol. 71, pp. 163-173 (2006)

Vall6e, C., Seidel, T., Lucas, D., Beyer, M., Prasser, H.M.,
Pietruske, H., Schutz, P., Carl, H., Counter-current Flow
Limitation Experiments in a model of the Hot Leg of a
Pressurized Water Reactor Comparison between Low
Pressure Air/Water Experiments and High Pressure
Steam/water Experiments. In: Proceeding of the 13th
International Topical Meeting on Nuclear Reactor Thermal
Hydraulics (NURETH-13), Kanazawa, Japan (2009)

Wang, M.J., and Mayinger, F., Simulation and Analysis of
Thermal-hydraulic Phenomena in a PWR Hot Leg Related
to SBLOCA. Nuclear Engineering and Design, Vol 155, pp.
643-652 (1995).

Wongwises, S. Two-phase Countercurrent Flow in a Model
of a Pressurized Water Reactor Hot Leg. Nuclear
Engineering and Design, Vol. 166-2, pp. 121-133 (1996)

Yegorov, Y., Contact Condensation in Stratified
Steam-water Flow. EVOL-ECORA- D07.




University of Florida Home Page
© 2004 - 2010 University of Florida George A. Smathers Libraries.
All rights reserved.

Acceptable Use, Copyright, and Disclaimer Statement
Last updated October 10, 2010 - Version 2.9.7 - mvs