Group Title: 7th International Conference on Multiphase Flow - ICMF 2010 Proceedings
Title: 7.3.1 - Assessment of NEPTUNE_CFD code for some free surface flows interesting fluvial hydraulic
ALL VOLUMES CITATION THUMBNAILS PAGE IMAGE ZOOMABLE
Full Citation
STANDARD VIEW MARC VIEW
Permanent Link: http://ufdc.ufl.edu/UF00102023/00179
 Material Information
Title: 7.3.1 - Assessment of NEPTUNE_CFD code for some free surface flows interesting fluvial hydraulic Industrial Applications
Series Title: 7th International Conference on Multiphase Flow - ICMF 2010 Proceedings
Physical Description: Conference Papers
Creator: Méchitoua, N.
Jennesson, B.
Schneider, J.-P.
Luck, M.
Valette, E.
Publisher: International Conference on Multiphase Flow (ICMF)
Publication Date: June 4, 2010
 Subjects
Subject: fluvial hydraulic
Eulerian simulations
stratified and dispersed flows
VOF method
multi-fluid model
 Notes
Abstract: The paper presents an evaluation of the multiphase CFD solver NEPTUNE_CFD for the computation of free surface flows involved in fluvial hydraulic. The numerical model of NEPTUNE_CFD is based on separate Eulerian transport equations for mass, momentum, energy and turbulent quantity of the different fluids, which are coupled through inter-phase transfer terms (Ishii et al, 2006). This model is primarily dedicated to the simulation of multiphase flows containing one continuous fluid always present, which carries dispersed fluids present in the form of inclusions, whose dimensions are much smaller than the spatial resolution length of the model. Liquid/ gas stratified flows represent challenging cases for multiphase volume averaged flow models. Numerical assessments of such flows have been already performed (Méchitoua et al, 2003, Pigny et al, 2004, Bartosiewicz et al, 2008) and show that it is possible to get an acceptable description of complex stratified flows with a general multi-fluid flow solver (Coste et al, 2007, Laviéville et al, 2008). The paper deals with a supplementary assessment, concerning free surface flows interesting hydraulic engineering. The numerical results obtained with NEPTUNE_CFD are compared with experimental data and numerical results arising from two other flow solvers FLOW3D and CFX5 (Valette et al, 2009), using respectively VOF and pseudo-VOF methods, widely used for free surface numerical simulations.
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: VID00179
Source Institution: University of Florida
Holding Location: University of Florida
Rights Management: All rights reserved by the source institution and holding location.
Resource Identifier: 731-Mechitoua-ICMF2010.pdf

Full Text

Paper No 7th International Conference on Multiphase Flow
ICMF 2010, Tampa, FL USA, May 30-June 4, 2010


Assessment of NEPTUNECFD code for some Free
Surface Flows interesting Fluvial Hydraulic


Namane Mechitoua1, Benjamin Jennesson Jean-Pierre Schneider,
Marilyne Luck1 and Eric Valette2


Electricity de France, Research & Development 6, Quai Watier 78400 Chatou Cedex, France
ENSEEIHT Engineering School, Toulouse, France Student internship from March to September 2009
2 Electricity de France, Hydraulic Engineering Centre, Savoie, Technolac 73373 Le Bourget du Lac Cedex, France
namane.mechitoua@iedf.fr, marilyne.luck@iedf.fr, eric.valetteA@iedf.fr

Keywords: Fluvial Hydraulic, Eulerian simulations, stratified and dispersed flows, VOF method, multi-fluid model

Abstract

The paper presents an evaluation of the multiphase CFD solver NEPTUNE_CFD for the computation of free surface flows
involved in fluvial hydraulic. The numerical model of NEPTUNE_CFD is based on separate Eulerian transport equations for
mass, momentum, energy and turbulent quantity of the different fluids, which are coupled through inter-phase transfer terms
(Ishii et al, 2006). This model is primarily dedicated to the simulation of multiphase flows containing one continuous fluid
always present, which carries dispersed fluids present in the form of inclusions, whose dimensions are much smaller than the
spatial resolution length of the model. Liquid/ gas stratified flows represent challenging cases for multiphase volume averaged
flow models. Numerical assessments of such flows have been already performed (M6chitoua et al, 2003, Pigny et al, 2004,
Bartosiewicz et al, 2008) and show that it is possible to get an acceptable description of complex stratified flows with a general
multi-fluid flow solver (Coste et al, 2007, Lavieville et al, 2008). The paper deals with a supplementary assessment,
concerning free surface flows interesting hydraulic engineering. The numerical results obtained with NEPTUNE_CFD are
compared with experimental data and numerical results arising from two other flow solvers FLOW3D and CFX5 (Valette et al,
2009), using respectively VOF and pseudo-VOF methods, widely used for free surface numerical simulations.


Introduction

Design of spillways are mainly studied with experimental
models, representing at a reduced scale the real
configurations. In the field of hydraulic engineering, the use
of such models is often preferred, because of the complex
geometries of the configurations and encountered complex
physical phenomena (three dimensional flows, turbulence,
multiphase transport of scour and sediment,...). Nevertheless,
efficient numerical techniques have been developed since
one or two decades, and become today suitable to
complement physical modelling, thanks to the progress of
high performance computers.
Since several years, studies are done at EDF to analyse the
relevance of numerical models in the field of free surface
flows interesting hydraulic engineering and multiphase
flows interesting nuclear engineering.
The free surface numerical models are based on the shallow
water approximation of the Navier-Stokes equations leading
to the Saint-Venant based model. This model is
implemented in the multi-dimensional Finite Element code
TELEMAC (Hervouet, 2007) and the one dimensional
Finite Volume code MASCARET (Goutal et al, 2002).
More recently, a fully Lagrangian method applied to the
Navier Stokes equations has been implemented in the
Smooth Particle Hydrodynamic (SPH) code SPARTACUS
(Violeau et al, 2007). This method, which has a wider range
of use than the Saint-Venant based models, has interesting
capabilities for modeling complex free surface flows.
The multiphase approach, developed at EDF in the


NEPTUNE_CFD code (M6chitoua et al, 2003) for nuclear
engineering, is based on separate Eulerian transport
equations for mass, momentum, energy and turbulent
quantity of the different fluids, which are coupled through
inter-phase transfer terms (Ishii et al, 2006, Simonin et al,
2000). This model is primarily dedicated to the simulation
of multiphase flows containing one continuous fluid always
present, which carries dispersed fluids present in the form of
bubbles, droplets or solid particles, whose dimensions are
much smaller than the spatial resolution length of the model.
Liquid/ gas stratified (or separated) flows, which can be
encountered in nuclear PWR circuits and pipes under
nominal or incidental conditions, represent challenging
cases for multiphase volume averaged flow solvers, as
NEPTUNECFD jointly developed by EDF, CEA, AREVA
and IRSN in the frame of the NEPTUNE project (Guelfi et
al, 2007). Numerical assessments of such flows have
already been performed on some configurations
representative of industrial ones (M6chitoua et al, 2003) or
representative of academic ones (Bartosiewicz et al, 2008).
These results show that it is possible to get an acceptable
description of complex stratified flows with a general
multi-fluid flow solver (Coste et al, 2007, Tobita et al, 2006,
Pigny et al, 2004, Lavieville et al, 2008), originally
designed for dispersed flows.
The paper deals with a supplementary assessment of
NEPTUNE_CFD, concerning free surface flows
encountered in fluvial hydraulic. These flows generally
present a very large interface between the gas (air) and the
liquid (water). Compared to the characteristic length scale





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


of the fluvial hydraulic configuration, this interface can be
considered as smooth. The friction of the gas on the liquid is
generally negligible and the large interface can be replaced
by a free surface, upon which a constant constraint
corresponding to the pressure in the gas is imposed.
Neglecting the presence of the gas in the simulation,
Saint-Venant based models or free surface single phase
Navier-Stokes based models if the hydrostatic pressure
approximation is not valid are well suited for the simulation
of such flows. The paper, which compares results obtained
with NEPTUNE CFD and VOF based models on cases
representative of fluvial hydraulic configurations, is
organised as follows. The paper firstly describes the main
features of the VOF based models and of the multi-fluid
volume averaged models. Then, it describes the test cases,
presents the numerical simulations and the discussions
about the results. The last part concerns the concluding
remarks and the perspectives upon this work.

Volume of Fluid (VOF) based models

The motion of an isothermal fluid obeys to the classical
momentum and mass conservation equations. For
incompressible stratified (or separated) flows, the density
remains constant along the streamlines and the mass
equation is then reduced to a steady volumetric equation:
dp= 0 or divU = 0
dt
Liquid and gas flows encountered in the nature as for
example water and air making up sea and atmosphere or
flows encountered in industry, as for example bubbles
columns containing gas dispersed in the liquid obey to this
equation. The application of the above equation to the
mentioned geophysical and industrial flows implies that
P=Pliquid or P=pgas, depending on whether the streamline
contains liquid or gas. The above equation can be replaced
by an equation on the volume fraction, the liquid volume
fraction, for instance:
dL = with LL=1 in the liquid and 0 elsewhere.
dt
Then, density is calculated through the equation of state:
S=a LPiquid +(1 -L)Pgas with L= 1 or 0 strictly.

In summary, the derived model for incompressible stratified
flows, containing two immiscible fluids consists of the
following set of equations.
A momentum equation:
3pu +div(UpU-p( W+tVU)) +VP=pg+po (1)
at
where p, uL, P andu stand respectively for density, dynamic
viscosity, static pressure and the velocity vector. The right
hand side contains the buoyancy and tensile accelerations
respectively represented by vectors g and o .

A steady conservation equation on the volume flow-rate.
divU = 0 (2)

A transport equation on the volume fraction of the liquid
associated with an equation of state giving the density.
dL =0 (3)
dt


P= LPliquid +(1-uL)Pgas
with aL=1 or 0 strictly


The above model, which looks like the Navier-Stokes
equations for incompressible mono-species fluid, is not so
easy to handle numerically. The condition on the volume
fraction aL=1 or 0 strictly is quite difficult to obtain for
industrial flows. For instance, the capture of the smallest
flow structures, whose dimensions are of the order of the
tensile force characteristic length, necessitate to build very
fine mesh or to use a lot of particles, respectively with an
Eulerian or a Lagrangian approach. Hopefully, such detailed
descriptions of the flows are not often necessary for an
engineering use of numerical simulations. The VOF and
pseudo-VOF methods, more tractable and mature than other
methods, can be used at a coarser level of spatial
discretization, compatible with an industrial need.

Pseudo- VOF methods

If our physical interest or our domain of studying concerns
stratified flows containing some very large interfaces
between two immiscible fluids, methods similar to the basic
one, succinctly presented above, can handle them with a
cost compatible with an engineering use.
This consists to solve the flow structures at a coarser level,
and in particular to slightly relax the strict condition on the
liquid volume fraction: the condition aL=l or 0 strictly is
replaced by the condition 0< La .
The interface capturing methods, widely used in CFD codes
solving the Navier-Stokes equations with an Eulerian
approach (Ubbink, 1997, Benkenida, 1999, Muzaferija et al,
1998) consider the transition between the liquid and the gas
as a continuous medium. The interface is captured at best
with a layer containing one to three cells, by the use of
compressive convection schemes (Ubbink, 1997) for the
transport of fluid volume fraction.

The two fluids (liquid and gas) are solved on a fixed mesh,
with the same velocity field. As the numerical method takes
into account the motion of the liquid and the gas in a
symmetric way, this method named pseudo-VOF is able to
simulate relative complex liquid/ gas flows. We can cite:
- breaking flows with draining and re-flooding zones,
- trapping of gas bubbles in the liquid or trapping of the
droplets in the gas, provided that the number of cells be
sufficient for representing the bubble pocket or the
liquid droplet.
The discrete systems obtained with such methods are stiff.
For stratified water/air flows, we have to solve the
momentum equation and the mass equation (through a
pressure correction equation), presenting respectively a
viscosity gradient in the range of 1 up to 100 and a density
gradient in the range of 1 up to 1000.

Figure 1 shows such an example of flows computed with a
pseudo-VOF method, using a structured mesh of
quadrilaterals. In order to mimic at best the conservative
form of the momentum and the mass equations on coarse
meshes, the spatial discretization on structured or
unstructured mesh with a Finite Volume method is often
preferred. Such a model can be coupled with an adaptive


Paper No






Paper No


mesh technique which refines the mesh around the interface.
This procedure generally improves the resolution of the
interface, even if this coupling is not yet robust, when used
with the automatic mode of mesh refinement.


Figure 1
Two Dimensional example of a liquid/gas
Interface obtained with a pseudo-VOF method


VOF modeling offree surface flows

The front tracking methods constitute an other alternative
for solving some classes of free surface flows. As these
techniques directly take into account the discontinuous
nature of the interface separating two stratified fluids, they
are theoretically able to numerically solve the multi-phase
problems given by the set of equations (1), (2), (3) and (4)
(Zaleski, 1995). But a fine spatial resolution and a precise
convection scheme are needed, entraining significant
computational costs and numerical difficulties.

Provided additional hypotheses authorizing some
simplifications of the basic model, these techniques can also
be used for engineering purposes.
Among the modeling hypotheses, the following ones,
concerning the water/air stratified flows representative of a
large class of flows involved in fluvial hydraulic:
- The flow is characterized, at first order, by some very
large interfaces separating two immiscible fluids.
Moreover, the friction of the gas onto the liquid at the
level of the free surface is negligible because the
separation surface is quite smooth with a small
interfacial area and because the density ratio between
the liquid and the gas is large.
- From an engineering viewpoint, the heaviest fluid
(water) is of a much greatest interest than the lightest
fluid (air): forces acting on the structures,
environmental needs, ...

The above assumptions authorize the computation of the
liquid flow only. The interface between the liquid and the
gas is considered as a free boundary for the liquid, upon
which the gas pressure is imposed. In general, this pressure
remains almost the same everywhere, because of the great
difference between the pressure inside the liquid and the gas


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

averaged pressure. The mesh moves with the free surface,
with respect to the kinematics and dynamic conditions
imposed upon the separation surface. This procedure allows
a precise tracking of the interface, since it is treated as a
boundary of the solution domain. This technique is
implemented in the TELEMAC3D code (Razafindrakoto et
al, 2009) and is coupled with a Finite Element discretization
for the propagation operators (Hervouet et al, 2007). It can
also be coupled with Finite Volume discretizations on
unstructured meshes (Muzaferija et al, 1998).
But this approach can be efficiently used for smooth free
surface, for which the shape of the mesh near the interface
remains smooth during the computation. Moreover,
re-flooding and drying zone are difficult to model with this
technique, except if the cells are added or removed during
the course of the numerical simulation.
The use of fixed meshes, as in the VOF method, is an other
way for tracking free surface flows and remove some
difficulties encountered with deformable mesh techniques.
The VOF method (Hirt, 1981), originally implemented in
the FLOW3D code (FLOW3D, 2009), can be described as
an intermediate technique between:
- the methods of front tracking based on the motion of
the mesh with the free surface, as in TELEMAC 3D or
other codes using FE or FV discretizations,
- and the methods of interface capturing, similar to that
implemented in commercial CFD packages or R&D
codes and named pseudo-VOF.
The motion of the free surface is proceeded in a geometrical
manner. The volumes containing liquid fluid are displaced
on a time step with the velocity of the fluid. Then, the
volumes are re-distributed on the traveled cells. This
procedure looks like to a Lagrangian one applied to the
movement of liquid volumes, whose the boundaries are the
surfaces of the mesh cells and the free surface. Figure 2
shows such an example of displacement of discrete surfaces,
as it is implemented in VOF codes.



SVoid (or gas)






Uquld undMr bJe soid lines (initial)
Liould under red dashed llnes Iiall




rounilt (n roonm)


Figure 2
Two dimensional example of a liquid/gas
interface obtained with a VOF method

This part of the VOF method, probably the most difficult in
terms of implementation, is representative of the knowledge
acquired as and when the evolution of the numerical method,
from a one dimensional approach (operator separation by





Paper No


space direction) to a full three dimensional approach
(FLOW3D, 2009). The displacement of the free surface,
whose accuracy for Cartesian mesh is comparable with the
front tracking techniques, needs some numerical cares in
order to maintain smooth the free surface:
- The translation of the new position of the interface in
terms of volume fractions can lead them to have values
slightly less than 0 or slightly above 1: these values are
then clipped.
- Pockets of liquid or void respectively isolated in the
emptiness or in the liquid can be carried out in areas
where the spatial discretization is insufficient for
describing the motion of these inclusions: these pockets
are then cleaned.
The volume added or destroyed by clipping, cleaning or
re-distribution is accumulated during the simulation and
compared to the total volume of fluid. The level of
conservation is considered as acceptable if the difference
does not exceed a few percent of the total volume for the
duration of the simulation.

The equations of momentum and mass are then solved in the
part of the mesh containing the liquid, like in the front
tracking methods. The interfaces between the liquid and the
"void", evaluated with the VOF method, constitute the
boundaries of the simulation, upon which suitable constraint
type boundary conditions are imposed (atmospheric
pressure for geophysical flows). The discrete system of
equations to solve is much less stiff than that obtained with
an interface capturing method or with a multi-fluid model
(presented below), since the gradient of the dynamic
viscosity and the density of water and air does not appear in
the equations.

Multi-fluid volume averaged models

General equations

Multi-fluid volume averaged models play a central role for
numerically handling multi-phase flows having complex
and rapidly changing topology of the interface separating
two immiscible fluids. In order to avoid description of the
small scales that may appear in multi-phase flows, a volume
(or time) averaging of the Navier-Stokes equations lead to a
set of separate mean balance equations for each phase (Ishii
et al, 2006, Simonin, 2000), which looks like to the single
phase conservation equations of mass, momentum, energy
and turbulent quantities. The averaging procedure in time
and/or space introduces additional coupling inter-phase
transfer terms between phases, which have to be modeled.
NEPTUNECFD code solves the general compressible or
incompressible multi-field balance equations, which is an
extension of the "two fluid-one pressure" model to the case
of m phases (up to 20 envisaged). In the case of two
incompressible isothermal phases without mass transfer as
air and water involving in fluvial hydraulic, the model
reduces to the following mass and momentum equations for
each phase (k=1,2):


ak + div(akPk k)=0 (5)
at


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

akPk Uk
k +di(Uk akPkUk)= (6)

div( ak+k +"k) -ak P + 1k +akPk +akgk

where k, ak and Uk represent respectively the number of
fluid (1 or 2 in our case), the volume fraction and the
velocity of phase k at the same given spatial point.

The global volume and momentum conservation imply:


2
Zak =1
k-1


1k=o
k=1


Notice that:
Tk is the laminar viscous constraint tensor:

k =k(VUk + Uk )-2/3divk(8)
k is the turbulent constraint tensor:

-k (kPk k k) (9)

I k represents the momentum interfacial transfer of all
phases p onto the phase k (drag, added mass, turbulent
contributions to drag and added mass, ...):
Ik- 1 -' (10)
Ik= 2I p-ik
p k

Additive equations for each field can be used in order to
model physics, such as turbulence, phase separation,
diameter of the inclusion, nucleate boiling near walls and
radiation heat transfer. The influence of turbulence between
phases is taken into account through correlations which
modify the turbulent viscosity. The correlations depend on
turbulence quantities of each phase, such as turbulent kinetic
energy and turbulent dissipation, the covariance of the
fluctuating velocities and the turbulent characteristic time
scale of the droplet and bubbles.

Numerical procedure

A segregated procedure is used for advancing in time
(M6chitoua et al, 2003). The first step consists of predicting
velocity for each phase from the momentum equations. This
step solves an implicit equation for velocity, all other
variables as pressure and volume fractions being frozen.
Then, a reduced form of the momentum equations containing
the predicted velocity, the implicit part of the pressure and
volume fractions gradients are coupled with the mass
equations. This system is solved using sub cycles, combining
mass predictions and pressure corrections. The convergence
of the non linear system is assessed if the predicted volume
fractions obey to the volume conservation (7). This criterion
is very strong since it applies to the maximum volume
conservation constraint over the computation domain. The
elliptic feature of the overall algorithm is due to the elliptic
form of the pressure correction equation. The taking into
account of the non linear coupling between pressure and
volume fractions within the sub-cycles and the symmetric
treatment of all fields make this algorithm tractable for all the
range of void fraction, without any artificial numerical need.






Paper No


Spatial discretization follows a 3D full unstructured finite
volume approach, with a collocated arrangement for all
variables. A face based data structure allows the use of
arbitrary shaped cells (tetrahedron, hexahedron, prisms,
pyramids, ...), including non matching meshes. Numerical
consistency and precision for diffusive and convective
fluxes for non orthogonal and irregular cells are taken into
account through a gradient reconstruction technique. A
careful treatment of gradient terms of momentum equations,
similar to a Rhie & C lho interpolation, is needed in order
to avoid spurious oscillations of pressure, velocity
components and volume fractions.

Interfacial drag modeling

Among the different forces including in the momentum
interfacial terms, the interfacial drag between the two
phases has a key role in the modeling of momentum transfer.
This term can be written in the following form:

I = aza2F12(U2 -U1) kaza2 I (U2 -U1) (11)
D
It depends on the relative velocity and a coefficient F12
homogeneous to a dynamic viscosity divided by the square
of a length D characteristic of the two phase flow.
In dispersed flows modeling, physical considerations show
that this length scale is proportional to the diameter of the
inclusion. Formulas and correlations corresponding to the
drag of a non deformable sphere by a continuous fluid
surrounding it are generally used (bubble and droplet laws).
For liquid/ gas flow covering all the range of void (0 up to
1), the translation of the volume fraction values in terms of
drag modeling is not unique. Figure 3 shows an example of
choice of models for a volume fraction close to 0.5. We can
consider a stratified flow with two continuous phases and
two types of dispersed flows (dispersed droplets in a
continuous gas or dispersed bubbles in a continuous liquid).
The standard choice provided in NEPTUNE_CFD is the
SIMMER flow chart (Tobita et al, 2006), for which
dispersed droplets in a continuous gas are considered for a
void fraction greater than 0.7, dispersed bubbles in a
continuous liquid are considered for a void fraction smaller
than 0.3. For intermediate values taken between 0.3 and 0.7,
the drag law is continuously interpolated between a bubble
and droplet drag law. This quite simple model gives
acceptable results for a quite wide range of applications, as
it can be shown in (Tobita et al, 2006, Pigny et al, 2004,
M6chitoua et al, 2003).


Reahb de la surface libre Bulles d'a uda.u 1'e Gouties d'eau dars l'a

Figure 3
Flow chart choices for a volume fraction-0.5

Nevertheless, for pure stratified flows, the model described
above may lead to a significant over-evaluation or
under-evaluation of the friction between the gas and the
liquid. Indeed, the drag model based on the friction between
a dispersed and a continuous phase is sensitive to the
diameter value. Interfacial area modeling, which gives


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

information about the dimensions of the inclusions, still
remains a challenging task for two-phase flows simulation.
Instead, the recognition of large interfaces within a volume
averaged model represents a viable alternative for
improving the modeling of the friction. A three layers model,
named Large Interface Model or LIM, has been
implemented in NEPTUNE_CFD (Coste et al, 2007,
Lavibville et al, 2008). If the void fraction varies between 0
and 1 on three contiguous cells, a specific friction law is
applied in the intermediate cell in which the void fraction is
far from 0 and 1. Figure 4 shows a scheme of such a
configuration of flows. The dispersed/ continuous drag law
(11) projected on the recognized separation surface is
replaced by a continuous/continuous friction law, taking into
account the laminar and turbulent contributions on both
sides of the interface. The other part of the dispersed/
continuous drag law acting along the strongest gradient of
the volume fraction is conserved, even if it has no longer
physical signification. It links the residual phase velocity to
the most present phase velocity and hence avoids the
apparition of too large relative velocities, which may induce
numerical difficulties.




Intermediate
Cell





Figure 4
Recognition of a surface of separation
between two stratified flows (red and blue)

Boundary conditions

No external boundary condition is imposed upon the free
surface separating the liquid and the gas since it is simulated
by the model, using the two friction laws described above.
The friction between the liquid and the ground is modelled
through wall log laws, coupled with a turbulence model
(generally a k-e one). For other kind of surfaces (as
vegetation, stones, ...), ad hoc specific laws are necessary,
provided by heuristic or hydraulic engineering.
Two types of boundary conditions are considered at the inlet,
depending if the discharge or charge is known. The first one
consists to give the known flow-rate of liquid on boundary
surface, which is wetted by the liquid contained in the cells
adjacent to the surface boundary. The inlet velocities and
water height (which represents the wetted surface) converge
to fixed values, as the computation reaches the steady state.
The second one consists to give the pressure (or water
height) at the inlet, representing the known charge.
Stagnation pressure condition is preferred to static pressure
one, since it is numerically stable and more physical,
provided the condition is imposed rather far from the weir.
A normal derivative pressure condition is imposed at the
outlet, with a global or local rescaling in order to avoid the
drift of the pressure (the pressure in the gas far from the free
surface does remain close to the atmospheric pressure).






Paper No


Free surface flow over a Creager spillway

The flow over a Creager spillway is extensively described in
the technical and engineering literature (Sinniger et al, 1989,
US corps of Engineers, 1990). The geometry is defined for a
hydraulic design upstream head Hd which corresponds to a
pressure profile of zero along the spillway. The geometry of
the studied spillway, presented in figure 5, is defined using
the following parameters: Weir height=0.4 m and design
upstream head Hd=0.3 m.
The available data provide the position of the free surface
over the weir and the distribution of static pressure on the
facing of the weir, for three hydraulic head upstream (H/Hd
= 0.5, 1 and 1.33). Furthermore, the discharge of the
spillway is analysed using the flow rate coefficient Cd taken
from the following semi-empirical formula.:


Q= CLH42gH wherecd = Cp(H/Hd)0'12


where L is the width of the weir, H is the upstream water
height. The coefficient Cp is generally taken to 0.494,
assuming that the height of weir is high comparing to the
hydraulic head. Here, Cp 0.485 .


1115,5 mm


594,3 mm 490,25 M


A


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

mesh) used for the 3 models are of the same order.
The numerical results obtained with the 3 models are in
good agreements with experimental data. The main
discrepancies concern the following points:
- the multi-fluid model slightly under and over-evaluates
the water height respectively upstream and downstream
the weir.
- The multi-fluid and the pseudo-VOF models
respectively slightly under and over-evaluates the
discharge as the upstream increases.

The computed global friction between water and air
(normalised by the integrated pressure gradient) obtained by
the multi-fluid model is less than 2%. This confirms the
validity of the VOF model, which gives very good results,
when applied to this type of weir.
The two drag interfacial models available in
NEPTUNECFD were used for computing the friction
between liquid and gas. In this case, these models give quite
comparable results. The Large Interface Model (LIM),
which has a wider range of application, is generally
preferred to the dispersed flow drag model, even if its use
for complex situations (mixed flows) and for full
unstructured meshes remains perfectible. The diameter of
the inclusions is fixed, ranging between 0.1 mm up to 2 mm,
which is much smaller than the discretization grid.


1200



-


Figure 5
Geometry of the experimental configuration
of the Two Dimensional Creager spillway


-CFQaXsBfrQ-,O% NEPTUKEUM S0% -Flu.D Fa Ea.. tLSBR

Figure 7
Comparison of the water level obtained with 3 methods for
an imposed charge H/Hd= (pseudo-VOF with CFX, VOF
with FLOW3D, multiphase model with NEPTUNE_CFD)


Wl I
-ll |
J'MuaH U


i n-tn
- 4%.O U
-lio'tai


Figure 6
Liquid volume fraction and pressure of the 2D
Creager spillway obtained with NEPTUNECFD

Figures 7 and 8 respectively show the mean position of the
free surface for a given charge H/Hd= 1 and the correlations
water discharge versus upstream charge obtained by the 3
methods presented above. The pseudo-VOF, the VOF
(Valette et al, 2009) and the multi-fluid models are
associated here with CFX, FLOW3D and NEPTUNE CFD
codes. The cells number (hexahedra, tetrahedron, Cartesian


0.5 0.6 0.7 0.8 0.9 1 1,1 1,2 1.3 1.4
Hydraulic Charge H/Hd

Figure 8
Comparison of the Discharge versus Hydraulic charge
obtained with 3 methods (pseudo-VOF with CFX, VOF
with FLOW3D, multiphase model with NEPTUNE_CFD)


Free Surface
H -


400 mm Creager






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


Free surface flow over a 3D gated Creager spillway

The flow upon a Creager spillway equipped with 3 segment
gates has been investigated by the use of a reduced scale
experiment at EDF R&D (Cic6ro et al, 2004). The
experimental tests performed in a current channel allowed:
- To measure the discharge for different geometrical
configurations (number of the gates in service, position
of the gates with respect to the highest level of the
spillway, opening, ...) and two types of pile.
- To show hysteresis phenomenon due to the transition
between a free surface flow and a partially confined
flow controlled by the gate.
This case is particularly interesting for the evaluation of a
CFD code (Luck et al, 2009), since non linear phenomena
drive the transition when the water level touches the gate.
Moreover, a predictive evaluation of the free surface level is
capital, since it determines if there is or not air entrainment
under the gate.
The configuration contains three Creager weirs separated by
two piles and three fixed gates, opened of 15 mm. Half of
the geometry is simulated, provided that the flow remains
symmetric in average according to a vertical plane located at
the middle of the intermediate bump. Figure 9 shows the
experimental setup viewed of front and behind and the
unstructured mesh composed of hexahedra and prisms.


IJ-


Figure 9
Reduced scale model of the Creager spillway equipped with
3 sector gates. Corresponding mesh of the configuration.

The hysteresis phenomenon has been reproduced by
imposing an inlet flow-rate corresponding to the hysteresis
zone and two initial different water levels, respectively
slightly lower and higher than the level of the gate. The
numerical simulations then give two steady water levels,
corresponding respectively to a free surface flow and to a
mixed flow controlled by the gate. Figure 10 shows on the
coarsest mesh the initial water levels (white line) and the
final water levels (green) corresponding to a discharge for
which a hysteresis phenomenon can be observed.


Figure 10
Reproduction of the hysteresis phenomena at 80 1/s
White and green lines represent initial and final levels

Figure 11 shows a mixed flow (free surface and partially
confined) obtained for a charge of H/Hd=2, for which the
sector gate is submerged.


Figure 11
3D flow with sector gate submerged with water (H/Hd=2)
Liquid volume fraction field (red=liquid and blue=air)

Figure 12 shows the relation of the computed discharges by
passes with the imposed upstream charge. The computations
have been performed with the following boundary
conditions:
- the charge (corresponding to the stagnation pressure)
and the level of liquid and air (through volume fractions
of the two phases) at the inlet,
- a pressure condition at outlet; the computed pressure is
prolonged to the boundary faces and rescaled in order
to remain close to the atmospheric pressure far from the
liquid flow.
The computed discharges are in good agreement with the
experimental data, only available for non dimensional
charges ranging from 0.6 up to 1. The first slope
corresponds to a free surface flow passing under the sector
gate, the second slope to a flow controlled by the sector gate
and the third slope to a flow submerging the sector gate. The
Large Interface Model (LIM) model gives here much better
results than the dispersed drag model.


180
IBO
140
S120
so
sc
W~


40 4


slope 1


Flow touches
the gate


0. 0.6 0.7 0.8 09 1 1.1 1.2 1.3 1.4
Hydraulic Charge H/Hd


Figure 12
Flow-rate by passes with respect to the imposed charge


Paper No


slope 3




Row sumerges
the gte


1.5 1.6 1.7 1. 1.9 2






Paper No


3D flow through a breach of a dam in clay

Free surface flows through breaches inside embankment
dams have been extensively studied (US Corps of
Engineering, 1990), including several different geometries
(height, breach length). The available experimental data
corresponding to the case n 37 provide the discharge versus
upstream hydraulic charge. The discharge coefficient Cf is
obtained through the following correlation


Q= CLHF2gH


TOP VIW
A __



z


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

The numerical results presented in figure 15 suggest to
share the flow in two parts. In the first part upstream the
bump, numerical results show that it is necessary to have a
refined mesh at the highest level of the bump in order to
correctly capture the upstream water height for low
discharge. In this way, a refinement mesh technique driven
by a criterion based on the upstream water height would be
useful. In the second part downstream the bump, thanks to
the multi-fluid model, the main physical features are found
by the computations, with a reasonable spatial discretization.
The liquid jet is simulated as a mixed dispersed/ stratified
flow along its falls (green, blue sky) and then again as a
stratified flow in the bottom of the configuration.


ap


licttIo 1.vE
SeCMHALVIEWAA


YBO \ ^ Si .---- ----- '-. -------------



Figure 13
Geometry of a reduced model of
the breach of an embankment dam

The computations with NEPTUNECFD have been
performed with the following parameters:
- Large Interface Model (LIM) for the friction modeling
between liquid and gas,
- fixed diameter of 1 mm, which is much smaller than the
grid size,
- k-E turbulence model for each phase,
- half of the geometry is simulated, provided that the
flow is symmetric in average according to the vertical
plane AA defined in figure 13.

Figure 14 shows a three dimensional view of the flow
obtained numerically. The complexity of the flow
necessitates to reduce the geometry and to refine the mesh
around the bump, in order to capture at best the hydraulic
charge (480 000 cells).


Figure 15
Liquid (red), Gas (blue) and mixing (green, yellow)
obtained by NEPTUNE_CFD code

Figure 16 shows the discharge coefficient versus the
discharge obtained by the code and experimental tests.
NEPTUNE_CFD results compare fairly well with
experimental data, for the reduced and refined mesh, as well
as for the low discharge corresponding to low upstream
charge and for high discharge. The simulation with the
coarsest mesh presents a non monotone behavior for low
discharges, probably due to the use of the non linear LIM
model with a coarse mesh.


0,9


0,6

A 0,5


0,3
0


25 50 7'5
Discharge (l/s)


100 125 150 175


Figure 16
Discharge coefficient versus discharge


Figure 14
3D view of the flow obtained with NEPTUNE CFD


)!


bW_ f


Ir





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


Acknowledgements


The paper presents an evaluation of the multiphase CFD
solver NEPTUNECFD for the computation of free surface
flows involved in fluvial hydraulic.
The evaluated numerical model is based on separate
Eulerian transport equations for mass, momentum, energy
and turbulent quantity of the different fluids, which are
coupled through inter-phase transfer terms (Ishii et al, 2006).
This model is primarily dedicated to the simulation of
multiphase flows containing one continuous fluid always
present, which carries dispersed fluids, present in the form
of bubbles, droplet or solid particles, whose dimensions are
much smaller than the spatial resolution. Liquid/ gas
stratified flows, which can be encountered in nuclear
pressurized water reactor (PWR) circuits and pipes under
nominal or incidental conditions, represent challenging
cases for multiphase volume averaged flow models.
Numerical assessments of such flows have been already
performed on some configurations representative of
industrial ones (MWchitoua et al, 2003, Pigny et al, 2004) or
of academic ones (Bartosiewicz et al, 2008). These results
show that it is possible to get an acceptable description of
complex stratified flows with a general multi-fluid flow
model (Coste et al, 2007, Lavi6ville et al, 2008).
The paper deals with a supplementary assessment,
concerning free surface flows interesting hydraulic
engineering. Two and three dimensional flows upon
spillways and through a breach inside an embankment dam
have been computed with NEPTUNECFD. The obtained
results have been compared with experimental data and
numerical results arising from two other flow solvers using
methods different from that NEPTUNECFD (Valette et al,
2009). On one hand, FLOW3D simulates only the liquid and
uses a VOF method for tracking the interface between the
liquid and the "void", upon which free type boundary
conditions are imposed. On the other hand, CFX-5 uses a
pseudo-VOF method without reconstruction of the interface
and simulates the two fluids, with an adaptive mesh
technique for sharpening the interface. The numerical results
obtained by NEPTUNE_CFD compare fairly well with
experimental data and with numerical results obtained with
methods widely used for free surface flows simulation.
However, the computation of flows characterized by large
and smooth interfaces between two immiscible fluids show
that it can be necessary to take into account the laminar and
turbulent friction between the two stratified fluids with laws
similar to wall laws, clearly separating the two fluids by a
plane, instead of using friction laws between a dispersed
fluid contained in a continuous fluid. Future work will deal
with the simulation of more complex flows interesting the
environment domain and hydraulic engineering. A
predictive simulation of such flows, characterized by the
presence of dispersed and separated fluids in the same
computational domain, still remains a challenging task and
will bring us to propose variants of the multi-fluid model
implemented in NEPTUNE CFD.


The work presented here has been achieved in the framework
of the EDF R&D project "Suret6 hydraulique et maitrise des
6coulements", concerning experimental and numerical
simulations of free surface flows upon dams and weirs,
interesting hydraulic engineering. The financial support
comes from EDF (Electricit6 de France).
The authors are grateful to Alexandre Douce and Jr6rme
Lavi6ville of the NEPTUNE_CFD development team for
their support to the use of this code.
In the frame of the NEPTUNE project, NEPTUNECFD
code is jointly developed by EDF (Electricit6 de France) and
CEA (Commissariat A l'Energie Atomique). The project is
also funded by AREVA-NP and IRSN (Institut de
Radioprotection et de Sfiret6 Nucl6aire).


Paper No


Concluding remarks






Paper No


References

Bartosiewicz, Y, Lavidville, J., Seynhaeve, J.M. A first
assessment of the NEPTUNE CFD code : instabilities in a
stratified flow comparison between the VOF method and a
Two Field Approach. International Journal of Heat and Fluid
Flow 29, pp. 460-478 (2008)

Benkenida, A. Ddveloppement et validation d'une m6thode
de simulation d'6coulements diphasiques sans
reconstruction d'interfaces. Application a la dynamique des
bulles de Taylor. PhD Thesis, Institut National
Polytechnique de Toulouse, France (1999)

Cic6ro, G.M., Boursiquot, D., Br6mont, O.,Menon, J.M.,
Project Maitrise de la D6bitance des Ouvrages Synthese des
essais sur module r6duit de vannes segment sur seuil
Creager. Internal Report EDF R&D LNHE HP-75/04/014/A
(2'"'4)

Coste, P., Pouvreau, J., Morel, C., Lavidville, J., Boucker,
M., Martin, A. Modeling Turbulence and Friction around a
large interface in a three dimensional-two velocity Eulerian
code. NURETH'12, Pittsburgh, Pennsylvania, USA,
September 30- October 4 (2007).

FLOW3D: documentation of the FLOW3D code available
at the internet site Imp \ \\ \ llo \\ D.com (2009)

Goutal, N., Maurel, F. A finite volume solver for one
dimensional shallow water equations applied to an actual
river. International Journal of Numerical Methods in Fluids
(2002)

Guelfi, A., Bestion, D., Boucker, M.,Boudier, P., Fillion, P.,
Grandotto, M., H6rard, J.M., Hervieu, E., P6turaud, P.
NEPTUNE A New Software Platform for Advanced
Nuclear Thermal-Hydraulics. Nuclear Engineering and
Design, Vol. 156, pp. 281-324 (2007)

Hervouet, J.M. Hydrodynamics of free surface flows.
Modelling with the Finite Element Method. John Wiley and
Sons Ltd (2007)

Hirt, C.W., Nichols, B.D. Volume of Fluid (VOF) method
for dynamics of free boundaries, Journal of Computational
Physics, Vol. 39, pp. 201-221 (1981)

Ishii, M., Hibiki, T Thermo-Fluid Dynamics of Two Phase
Flows. Springer Science Business Media, New York (2006)

Lavieville, J., Coste, P., Numerical modeling of liquid-gas
stratified flows using two phase Eulerian approach,
Proceeding 5th International Symposium on Finite Volumes
for Complex Applications, Aussois, France, June 08-13,
2008 (2008)

Luck, M., Eun-Sug, L., Mechitoua, N., Violeau, D., Laugier,
F., Blancher, B., Valette, E., Guyot, G. Physical and 3D
modeling of spillways discharge capacity and design.
Colloque SHF "Modeles physiques hydrauliques", Lyon,
November 24-25 (2009)


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

M6chitoua, N., Boucker., M., Lavieville, J., H6rard, J.M.,
Pigny, S., Serre, G. An unstructured FV Solver for Two
Phase Water/ Vapor Flows Modelling based on an elliptic
Oriented Fractional Step Method, NURETH'10, Seoul,
October 5-9 (2003)

Muzaferija, S., Peric, M. Computation of free surface flows
using interface-tracking and interface-capturing methods.
Comput. Mechanics Publication. O. Mahrenholtz and M.
Markiewicz editors, Non linear Wave Interaction (1998)

Pigny, S., Boucker, M., Lavidville, J., M6chitoua, N.,
Benchmarks for the NEPTUNE 3D code, Proceedings
International Conference on Multiphase Flows, Yokohama,
Japan, May 31- June 03, 2004

Razafindrakoto, E., Martin, L., Hervouet, J.M., 3D
modeling of long term hydrodynamics and water quality in
the Berre Lagoon, Proceeding 33rd IAHR Congress: water
engineering for a sustainable environment (Vancouver,
British Columbia, August 2009 (2009)

Simonin, O. Statistical and continuum modelling of
turbulent reactive particulate flows. Theoretical and
Experimental Modelling of Particulate Flows. Lecture
Series 2000-06, Von Karman Institute for Fluid Dynamics,
Rhode Saint Genbse, Belgium (2000)


Sinniger, R.O, Hager, W.H. TraitW de g6nie civil, Volume 15,
p. 152, Construction hydraulique de l'Ecole Polytechnique
F6d6rale de Lausanne, Ecoulements stationnaires (1989)

Tobita, Y, Kondo S., Yamano, K., Morita, W., Maschek, P.,
Coste, P., Cadiou, T The Development of SIMMER-III, An
advanced Computer Program for LMFR Safety Analysis,
and its application to Sodium Experiments. Nuclear
Technology, Vol. 153, pp.245-255 (2006)

Ubbink, O. Numerical prediction of two fluid systems with
sharp interfaces, PhD Thesis, University of London (1997)


US Corps of Engineers, Hydraulic Design Criteria, Volume
I, Overflow spillway crest equation, p. 68, Over flow
spillway crests upper nape profiles and high overflow dams
crest pressures, p. 98-109 (1990)

Valette, E., M6chitoua, N., Spennato, B. Which software for
which 3D Hydraulic Simulation ? Hydro 2009, France,
October 26-28 (2009)

Violeau, D., Issa, R. Numerical modeling of complex
turbulent free surface flows with the SPH method: An
overview. International Journal of Numerical Methods in
Fluids, 53(2),pp. 277-304 (2007)

Zaleski, S., Li, J., Succi, S. Two dimensional Navier-Stokes
simulation of deformation and break up of liquid patches,
Physical Review Letter, Vol. 75, pp. 244-277 (1995)




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