The Algebraic Slip Model provides an alternative to IPSA for the modeling of truly multi-phase flows.
The model postulates that there exists one continuous medium in which there are dispersed various phase components. These may be droplets, bubbles or solid particles.
The mixture of the continuous and dispersed phases behaves as a single fluid, with fluid properties that may or may not depend on the dispersed phases.
This referred to as the mixture, and correspondingly its properties are referred to as the mixture density and the mixture viscosity.
Each dispersed phase is represented by a species concentration equation. The transport equation for each dispersed phase allows for relative movement between the dispersed phase and the continuous phase. This extra migration or drift of the dispersed phase is known as phase slip.
It is assumed that the slip velocity can be calculated from algebraic equations involving only local variables, rather than from the full partial differential equations, as is the case with IPSA.
The equations of motion for each particle group, treated as a distinct phase, involve the following terms:-
The algebraic-slip model assumes that the last three terms are dominant, eg small particles and viscous fluids.
Unimportance of d/dt and d/distance terms means that the relative velocity is a function of LOCAL variables only.
It can therefore be deduced from ALGEBRAIC rather than partial differential equations (PDEs).
The equations to be solved for the phase-concentration distributions are therefore:-
Assumption: dispersed phase is in quasi-steady state determined by local conditions
Requires: relaxation time for dispersed phase to be short compared with changes in the flow, i.e. the Stokes number << 1. The Stokes number is defined as the ratio of the particle relaxation time to the carrier flow time.
The precise condition depends on the drag relationship, and is considered below. In general terms, it will be satisfied if the particles/droplets are small, or if the viscosity of the fluid is high.
The model is thus suitable for the simulation of:
The frictional drag on the particle is given by
Fd = Cd * Ap * 0.5 * r * (Vs)2
where Ap is the projected area of the particle, r is the fluid density and Vs is the slip velocity.
The slip force is given by
Fs = B * Vp * Dr
where Vp is the volume of the particle, Dr is the density difference, and B is the body force per unit mass.
Hence,
(Vs)2 = K * Dr * d * B / r
where d is the particle diameter, and the coefficient K=4/(3*Cd) may be a function of the slip Reynolds number Re via Cd. The slip Reynolds number Re=d*Vs/n, where n is the kinematic viscosity.
The body force includes gravitational acceleration, rotational forces, magnetic or electric forces.
The slip velocity is added to the mixture velocity to construct the dispersed-phase convection fluxes.
The built-in drag coefficient is a simplified model which breaks the drag curve into two parts. At low slip Reynolds number the relationship is:
Cd = 24/Re;
at higher slip Reynolds number
Cd = 0.42
It is now possible to check the applicability condition described above, by considering the force balance on the dispersed phase, retaining the transient term:
Volume * du/dt = slip force - frictional drag.
The time constant for this equation (which is determined by the form of the frictional drag) gives an estimate of the relaxation time for the dispersed phase.
Using the low Reynolds number drag coefficient, Cd = 24/Re, for simplicity, this time constant becomes d2/18n. As an example, for a particle of 1mm diameter in water (viscosity approximately 10-6m2/s) the relaxation time is about 0.05s; this would be reasonable for a flow timescale of about 1s.
Solution for all volume fractions is carried out simultaneously at the end of the slab solution for the hydrodynamics. Simultaneous solution is required because of the strong links between the equations.
Iteration is used over each cell and over the whole slab.
For each cell iteration:
Mixture Density
rm = (1 - S(PTi)) * rc + S(PTi * ri)
Mixture Viscosity
nm = (1 - S(PTi)) * nc + S(PTi * ni)
In both cases m refers to the mixture, c to the continuous phase, and i to the i'th dispersed phase.
PTi is the volume fraction of the i'th phase.
The single phase continuity equation can be written as:
d(r)/dt + d( r*u )/dx = 0
This can also be written as:
D(ln(r))/Dt + d(u)/dx = 0
Assuming that all phases are incompressible:
d(u)/dx = 0
This implies that knowledge of the density is immaterial for the solution of the continuity equation if the flow is incompressible.
The continuity condition in terms of volumetric conservation is valid even when the density changes from point to point due to changes in volume fraction.
This is embodied in GALA (Gas And Liquid Algorithm), available in PHOENICS.
The Algebraic Slip Model can be activated from PHOENICS-VR. It can be selected in the Main menu, Models panel from the 'The simulation is' button. The number of particles and particle properties can then be specified from 'Settings'. The inlet and outlet object dialog boxes will allow the specification of inlet particle volume fractions.
Should the user wish to activate the model 'by hand' from the Q1 file, the following commands are required:
In Group 7
NAME (C1) = PT0 - volume fraction of the main carrier fluid
NAME (C2) = PT1 - volume fraction of disperse phase 1 ...
NAME (Cn) = PTn - volume fraction of disperse phase n
SOLVE (PT0, PT1, ..., PTn)
SOLVE (VFOL); STORE (DEN1, VISL)
The SOLVE command for the particles is required so that boundary conditions can be set for each particle. The actual simultaneous solution of the particle volume fraction equations is carried out in GXASLP.
The SOLVE for VFOL allows volume inflow/outflow conditions to be set.
In Group 8
GALA = T; TERMS(VFOL,N,N,N,N,P,P)
These settings activate the volume-continuity-satisfying flow field, and ensure that VFOL is not actually calculated.
The setting of an inflow value for VFOL is a mechanism which will satisfy the continuity equation, as in GALA the default source for inflows in the overall continuity equation is: Sv=mass inflow/(cell density)
If the cell density is different from that of the incoming flow, the volumetric source will not be correct. However GALA will recognise the inlet value of VFOL and set the source in the overall continuity equation as:
Sv= mass flow * incoming VFOL = (RHOM*Vel)*(1./RHOM) = Vel
In Group 9
RHO1 = GRND; RHO2 = density of the carrier fluid
ENUL = GRND
The above settings activate the calculation of the mixture density and viscosity in GXASLP. The formulae used were given above.
The densities, diameters of particles and viscosities of droplets are stored as follows;
PHINT (PTi) = Density of i'th phase
CINT (PTi) = Diameter of i'th phase
PRNDTL (PT0) = Laminar kinematic viscosity of carrier fluid
PRNDTL (PTi) = Laminar kinematic viscosity of i'th phase.
(if this phase is solid, set to a large number, say 1E3)
In Group 13
INLET (IN_1, AREA, IF, IL, JF, JL, KF, KL, TF,TL)
VALUE (IN_1, P1, RHOM*VEL)
VALUE (IN_1, U1, UIN)
VALUE (IN_1, V1, VIN)
VALUE (IN_1, W1, WIN)
VALUE (IN_1, PTi, Vol_frac_phase_i_in)
VALUE (IN_1, VFOL, 1./RHOM)
SPEDAT(SET,IN_1,ASLP,C,ASM)
Alternatively, Inflow PATCH names can start with the characters 'ASM', in which case the SPEDAT setting is not needed. The density used for calculating the inlet mass flux, RHOM, should be the mixture density, as defined in panel 9.
The setting for VFOL ensures that the correct volumetric flux enters the domain, in cases when the cell density is (already) different from that of the incoming flow.
Outflow conditions:
It is generally sufficient to employ the fixed-pressure type boundary condition for outflows. If there is any possibility of inflow through such a boundary, it is important to supply external values for all the dispersed phases, and also for VFOL. A typical outlet specification would be:
OUTLET (OUT_1, AREA, IF, IL, JF, JL, KF, KL, TF,TL)
VALUE (OUT_1, P1, Pext)
VALUE (OUT_1, PTi, vol_frac_phase_i_ext)
VALUE (OUT_1, VFOL, 1/RHOM_ext)
SPEDAT(SET,OUT_1,ASLP,C,ASM)
Alternatively, Outflow PATCH names can start with the characters 'ASM', in which case the SPEDAT setting is not needed.
The PATCH type for both inflow and outflow must be one of the area types.
For the present, the body forces which may be active in the flows simulated include the gravity, the centrifugal force and the Coriolis force. These are rendered available in GXASLP by calls to the GX-routines that are activated by settings in the Q1 file, by way of PATCH names with prefixes 'BUOY', and 'ROTA'.
In Group 15
LITER(PT0) = 2 - sets the number of iterations for each cell
LITER(PT1) = 5 - sets the number of iterations over a slab
ENDIT(PT0) = 1E-8 - set termination criterion for cell iterations
ENDIT(PT1) = 1E-5 - set termination criterion for slab iterations
In Group 16
RELAX (PT0, LINRLX, 0.5) - sets linear relaxation for cell iterations
RELAX (PT1, LINRLX, 0.5) - sets linear relaxation for slab iterations
In Group 19
ASLP = T - activate call to GXASLP
LASLPB = T - restrict slip velocity to direction of body force only. This can save cpu time by reducing the calculations required.
LASLPA = T - uses quicker but potentially less stable scheme for solution of volume fractions. This scheme should be tried first.
The present implementation of the Algebraic Slip model has the following limitations:
None of these limitations is fundamental to the method. It is planned to address them as time allows. GXASLP is provided in open source, so enthusiastic users could in principle make some of these changes themselves.
Library examples can be found in the Algebraic Slip Model (ASLP) section of the multi-Phase flow library, which can be accessed from the library option of the top menu, or from command mode by SEELIB(P).