(1)
M-K. Bouras,
Cemagref, hydrology-hydraulic division, Lyon, France
J-B. Faure,
Cemagref, hydrology-hydraulic division, Lyon, France
N.Buil
Abstract: We present a tridimensional model for a free surface flow in natural river and experimental canal using CFX Software from AEA Technology. Our essential work was, on one hand to define initial and boundary conditions, and on the other hand to choose a model which allows to find the free surface without adding simplification as hydrostatic pressure hypothesis. This last kind of hypothesis allows to construct shallow water equations.
The aim of the work presented here is to build a 3D numerical tool for prediction of pollutant concentra-tions in the vicinity of its injection point in the river.
In such situation, 1D and 2D models are not suitable for seeing concentration’s heterogeneities vertically (in 2D) and in cross section (in 1D). Particularly, it’s not possible to watch the influence of the injection point position in cross section on pollutant dispersion, if the concentration field is probably strongly inhomogenous due to geometry variability as meander, fairway or weir for example.
If such heterogeneity in spacial distribution of a pollutant was easy to be predicted with good accuracy, one would think out some disposal management capable of predicting the pollutant dispersion by the flow, and by the way, able to avoid that, locally, pollutant concentrations exceed letal quantity for aquatic animal life even though the mean values are under the maximum prescribed.
We present here the first results.
We study concurrently the two following complex test cases :
- 3D simulation in a channel (length 4 m, slope 0.4% and trapezoid cross section).
- 3D simulation on flow in a meander (length 4m, width 0.25m, depth 0.5m, slope 0%, rectangular cross section).
The first step, which is
actually reaching completion, is to test the practicability of that kind of
numerical simulation in unsteady flow with conservative pollutant. The main
difficulties are :
- the choice of boundary conditions that are compatible with the natural flow in a river.
- the free surface : the water depth is unknown and varies with time.
- the CPU time.
The second step will be to add more realistic pollutant, that is more complex geochemical and mechanical phenomena. For example several interacting pollutant or thermal stratification.
Our choice has been the use of a general CFD code instead of developing our proper solver. The main reasons are:
l it is needless to do twice the same things.
l we have already the code for another study.
l saving developing effort even if a proprietary solver is, a priori, more flexible and easy to use.
Comparing with other codes on the market, CFX has the following characteristics:
l solve Navier-Stokes equations with turbulence, including multiphasic flows ;
l wide choice of equations and models.
l use of Finite Volume Method ;
l opening of the software which allows to act on some points of the model, particularly on initial and boundary conditions and wall roughness ;
l availability of a double precision version.
For the first step the basic hypothesis are :
(1) The flow consists of two continuous phases without mixing. Each phase is taking up his own space region and is described by his volume fraction, the sum of all volume fractions in a cell being always equal to one. The phases being continuous, turbulent dispersion of volume fractions are assumed negligible.
(2) The two phases are isotropic and newtonian fluids which are supposed to be incompressible.
(3) There is no mass transfer between phases.
(4) The flow is isothermal.
(5) As a general rule, the flow is unsteady. For example it may be controlled by time varying inflow.
(6) The only volume force which is modeled is the gravity: the Coriolis and centrifugal forces are assumed negligible due to the small spacial area taken up by the flow.
(7) The pollutant does not modify water density.
(8) The molecular viscosity is assumed to be constant for each phase.
(9) The flow being turbulent in each phase, the turbulence is modelled by the k-e model.
(10) The flow being stratified with sharp boundary between air and water, we choose the homogeneous version of used multi-fluid model which assumes that the solution fields for each phase are identical except for volume fractions which are found by solving separate continuity equations for each phase.
Under theses assumptions, Navier-Stokes equations in terms of mean variables and with summation convention that repeated indices are summed on, can be expressed in the following form:
Continuity :
(1)
where ra is the volume fraction and r0a the density for phase a and
U = (Ui,Uj,Uk) = (U,V,W) the mean velocity.
Momentum (for i =1,2,3) :
(2)
Where P* = P + r0 k and r0 and m are linear combinations of r0a, ma for each phase weighted by volume fractions ra.
mt = Cm r0 where Cm is semi empirical coefficient with value 0.09.
Turbulence kinetic energy :
(3)
Turbulence dissipation rate :
(4)
sk, se are turbulent Prandtl numbers associated to each variable with sk = 1 and se = 1,3 ;
Sk = r1Sk1 + r2Sk2 and Se = r1Se1 + r2Se2 are source terms :
Ska = Ha - r0.e and Sea = Ct1 Ha - Ct2 r0 for phase a , with :
and Ct1 = 1,44 and Ct2 = 1,92 being empirical constants.
Pollutant :
(5)
where YA is mass fraction of species A (it may be several species), GA is the molecular mass dispersion coefficient, sA is Prandlt number for species A and SA is a source term.
There are three different boundary conditions:
l Upstream boundary condition (Inlet) for air and water.
l Downstream boundary condition (Outlet) for air and water.
l
Symmetry plane
condition at the top of the domain that is in the region taken up only by air.
These last kinds of boundary conditions are standard in the code and don’t have to be coded by the user.
On the other hand, upstream and downstream boundary conditions have to be carefully coded.
The upstream boundary condition is defined in an analogous manner to inlet condition in 1D simulation by a time varying inflow from which one can construct a uniform longitudinal velocity if one assumes that transverse and vertical velocities are zero. One must add a boundary condition of the same kind for volume fractions. It is the same as to specify water depth at inlet, but water depth is controlled by downstream flow conditions: one only has to add a weir so that the depth, at inlet, goes up with the same inflow.
The solution is to transfer at inlet the last known values of volume fractions in the first (y,z) plane of cells. The calculation of boundary conditions being done at each iteration of each time step, one obtains in this way a good coupling of boundary and interior of domain.
V and W are fixed to zero in water and air while U in air exponentially decreases from free surface in order to preserve velocity’s continuity.
In water and in air, turbulence kinetic energy at inlet is fixed at 0,002 · U .
Turbulence dispersion rate e is estimated by the formula:
e =
where A is the fluid cross section and Pm
his perimeter. ( CFX Release 4.3 1995 and Versteeg H.K. & al. 1995).
In the same way, the downstream boundary condition of the river section is defined in a manner analogous to outlet condition in 1D rivers simulations: one specifies the pressure through the medium of depth discharge function (rating curve): the outflow is estimated by integrating the longitudinal velocity in the last plane (y,z) of cells. The water depth obtained from this value of outflow allows defining a pressure field if one assumes it to be hydrostatic. Of course the downstream boundary condition needs to be sufficiently distant in order that supplementary hypothesis don’t modify the flow too far toward the upstream.
The rating curve used is a classical curve of uniform flow in a channel with rectangular cross section:
Q =
(6)
Where K is roughness coefficient from Strickler, L the channel width, y the water depth and I the bottom slope.
For the other variables (velocities, k, e, scalars) we prescribe a homogeneous Neumann condition at outlet.
The selected method
comes from the analogy with 1D simulation ( Faure & Buil Hic 98 ).
The free surface is the boundary between air and water and we find its position comparing the volume fractions of the two phases ( Faure & Buil Hic 98, Buil 99) .
Now we present the results obtained adding to the simulation one advection-dispersion equation for a passive scalar.
The boundary conditions are of the same kind as for the other transported variables: zero prescribed value at inflow, homogeneous Neumann condition at outflow and symmetry plane at and z = zmax.
The pollutant injection, simulated by adding a source term, is done into the domain in only one cell far enough from upstream in such a way that velocity field is not disturbed by uniform velocity prescribed at inflow. The injection cell is situated at mean depth.
Fig.1 Isoconcentration in the transverse plane
Fig.2 isoconcentration in the horizontal plane
Numerical model is used to simulate flow in a trapezoidal cross section. Channel. This test case is more realistic than a flow in a rectangular cross section channel.
In fact, the modeling should be capable of representing the totality of phenomena which take place in a river bend.
The results obtained confirm the satisfactory behavior of the numerical model.
CFX (1995) Release 4.3 User Manual , AEA Technology , Harwell Laboratory , Oxfordshire OX11 ORA , United Kingdom.
Patankar S.V. (1980) Numerical Heat Transfer and Fluid Flow, Hemisphere Publishing Corporation , Mc Graw Hill Book Co. , New York, USA.
Versteeg H.K. & Malalasekera W. (1995) An introduction to Computational Fluid Dynamics. The Finite Volume Method. Longman Scientific & Technical. Essex, United Kingdom.
Zakrzewski Ch. - (1993) Cahier de validation du code MAGE. Cemagref, France.
Giraud F.M, Faure J.B, Zimmer D, Lefeuvre J.C, Skaggs R.W - (1993) Hydrologic modeling of a complex drained watershed. ASAE International Winter meeting, Chicago, USA, 14-17 décembre 1993.
Giraud F.M, Faure J.B, Zimmer D, Lefeuvre J.C, Skaggs R.W. - (1997) Hydrologic modeling of a complex wetland. Journal of Irrigation and Drainage Engineering, Vol 123, No. 5, September/October, 1997, p. 344-353.
Schlichting - (1979) Boundary-layer theory , 7th edn, McGraw-Hill, New York.
Faure J B & Buil N (1998) Proceedings of the third international conference on hydroinfor-matics , Copenhagen , Danemark ,24-26 august.
Buil N (1999) Modélisation tridimensionnelle du transport de polluants dans les écoulements à surface libre Thèse de l’université Lyon1 et du Cemagref.