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.