
Modelling Capabilities
 Problem dimensionality: one, two and three dimensions.
 Time dependence: steady state and transient processes.
 Grid systems: Cartesian, cylindricalpolar and curvilinear coordinates; rotating
coordinate systems; multiblock grids and fine grid embedding.
 Compressible/incompressible flows.
 Newtonian/nonNewtonian flows.
 Subsonic, transonic and supersonic flows.
 Flow in porous media, with directiondependent resistances.
 Convection, conduction and radiation; conjugate heat transfer, with a library
of solid materials and automatic linkage at the solid fluid interface.
 A wide range of builtin turbulence models for high and lowReynolds number flows;
LVEL model for turbulence in congested domains and a variety of KE models, including
RNG, two scale and twolayer models.
 Multiphase flows of three kinds with a variety of builtin interphasetransfer models:
 Interpenetrating continua, including turbulence and modulation;
 Particle tracking, including turbulence dispersion effects;
 Freesurface flows.
 Finitevolume approach on staggered or collocated grids, with 13 choices of
discretisation schemes for convection.
 Combustion and Nox models, with a range of diffusion and kinetically controlled
models including the unique MultiFluid Model for turbulent chemical reaction.
 Chemical kinetics including multicomponent diffusion and variable properties.
Builtin interface to the CHEMKIN chemical database.
 Advanced radiation models, including surfacesurface model with calculated view
factors, a sixflux model and composite radiosity model for radiative heat transfer,
known as IMMERSOL
 Mechanical and thermal stresses in immersed solids can be computed at the
same time as the fluid flow and heat transfer.
PHOENICS Numerics
PHOENICS is a generalpurpose commercial CFD code which is applicable to steady or unsteady, one , two or threedimensional turbulent or laminar, multiphase, compressible or incompressible flows using Cartesian, cylindricalpolar or curvilinear coordinates. The code also has a spatial marching integration option to handle parabolic and hyperbolic flows, as well as transonic free jets in the absence of recirculation zones.
The numerical procedure is of the finitevolume type in which the original partial differential equations are converted into algebraic finitevolume equations with the aid of discretisation assumptions for the transient, convection, diffusion and source terms. For this purpose, the solution domain is subdivided into a number of control volumes on a monoblock mesh using a conventional staggeredgrid approach. All field variables except velocities are stored at the grid nodes, while the velocities themselves are stored at staggered cellface locations which lie between the nodes.
For curvilinear coordinates, the default option is to solve the momentum equations in terms of the covariant projections of the velocity vector into the local grid directions on a structured, monoblock, staggered mesh. An alternative exists to employ the GCV (General Collocated Velocity) method for curvilinear coordinates, whereby cellcentred Cartesian velocities or covariant velocity projections are solved on a structured monoblock or multiblock mesh. The link description for the latter can handle arbitrary block rotations, and therefore can accommodate an unstructured multiblock grid made from relatively simple, structured blocks.
For complex geometries, PHOENICS by default actually uses a Cartesian cutcell method named PARSOL (PARtial SOLid) which provides an automatic, efficient, and flexible alternative to traditional boundaryfitted grid methods using curvilinear coordinates. The Cartesian cutcell approach uses a background Cartesian or cylindricalpolar grid for the majority of the flow domain with special treatments being applied to cells which are cut by solid bodies, thus retaining a boundaryconforming grid. Specifically, the method computes the fractional areas and volumes, and employs a collection of special algorithms for computing interfacial areas, evaluating wall shear stresses, and for computing advection and diffusion near solid boundaries, etc.
The finitevolume equations for each variable are derived by integrating the partial differential equations over each control volume. Fully implicit backward differencing is employed for the transient terms, and central differencing is used for the diffusion terms. The convection terms are discretised using hybrid differencing in which the convective terms are approximated by central differences if the cell face Peclet number is less than 2 and otherwise by upwind differencing. At faces where the upwind scheme is used, physical diffusion is omitted altogether. In addition to the upwind and hybrid differencing schemes, PHOENICS is furnished with an extensive set of higherorder convection schemes, which comprise five linear schemes and twelve nonlinear schemes. The linear schemes include CDS, QUICK, linear upwind and cubic upwind. The nonlinear schemes employ a flux limiter to secure boundedness. These schemes include SMART, HQUICK, UMIST, SUPERBEE, MINMOD, OSPRE, MUSCL and vanLeer harmonic.
The integration procedure results in a coupled set of algebraic finitevolume equations which express the value of a variable at a grid node in terms of the values at neighbouring grid points and the nodal value at the old time level. For unsteady flows, PHOENICS by default solves each of these equations by an implicit method, but the option exists to revert to an explicit method which is stable only when the Courant number is less than or equal to unity. The explicit method uses oldtime neighbour values, whereas the implicit method uses values at the new time level. Although implicit methods allow a much larger Courant number than the explicit methods, it is not unconditionally stable since the nonlinearities in the equations often limit numerical stability.
The finitevolume equations are solved iteratively using the SIMPLEST and IPSA algorithms of Spalding, which are embodied in PHOENICS for the solution of singlephase and twophase flows, respectively. These algorithms are segregated solution methods which employ pressurevelocity coupling to enforce mass conservation by solving a pressurecorrection equation and making corrections to the pressure and velocity fields. Multiphase flows are accommodated using either an EulerianLagrangian method using particle tracking, or an algebraicslip model. The latter solves mixture continuity and momentum equations, and a volumefraction equation is solved for each dispersed phase. Algebraic relationships are used for slip velocities relative to the mixture.
The default calculation procedure is organised in a slabbyslab manner in which all dependent variables are solved in turn at the current slab before attention moves to the next higher slab. The slabs are thus visited in turn, from the lowermost to the uppermost, and a complete series of slab visits is referred to as a sweep through the solution domain. For parabolic and hyperbolic calculations, only one such sweep is required, with many iteration cycles at each slab for parabolic cases, and no outflow boundary condition is required because this is an outcome of the solution. For elliptic calculations, many such sweeps are conducted until convergence is attained at the current time level; in addition, the pressurecorrection equation is solved in a simultaneous wholefield manner at the end of each sweep. Thereafter the solution proceeds to the next time level where the iterative process is repeated. The option exists to solve each finitevolume equation in a wholefield manner, and this is actually the default when using the automatic convergence control. The default linear equation solver for each finitevolume equation is a modified form of Stone's strongly implicit solver, but the option exists to use a Conjugate Gradient Residuals solver for each equation.
The GCV method solves the system of algebraic finitevolume equations by using a conjugateresidual linear solver with LU preconditioning, and it uses a segregated pressurebased solver strategy with an additional correction of the cellcentred momentum velocities. This provides faster convergence than conventional onestep facevelocity corrections.
The numerical solution procedure requires appropriate relaxation of the flow variables in order to procure convergence. Two types of relaxation are employed, namely inertial and linear. The former is normally applied to the velocity variables, whereas the latter is applied to all other flow variables, as and when necessary.
The PHOENICS Parallel solver subdivides the solution domain into subdomains (spatial domain decomposition) and assigns each subdomain to one processor on a multicore computer. Each subdomain has storage overlap ("halo" cells) for data exchange between the various subdomains. The CFD code then runs simultaneously on all the processors, on its own set of data, and data is exchanged between the various subdomains ( via the "halo" cells ) using MPI (messagepassing interface). A point solver is used for wholefield solution of each of the finitevolume equations.
The convergence requirement is that for each set of finitevolume equations the sum of the absolute residual sources over the whole solution domain is less than one percent of references quantities based on the total inflow of the variable in question. An additional requirement is that the values of monitored dependent variables at a selected location do not change by more than 0.1 percent between successive iteration cycles. It is also possible to monitor the absolute values of the largest corrections to each variable anywhere in the domain. Once the largest correction falls to zero, or at least a negligible fraction of the value being corrected, then it can be assumed that convergence has been achieved, even if the sum of the residuals has not fallen below the cutoff.

Latest NEWS
PHOENICS News:
The Spring Edition, will be circulated in the near future.
The Summer Edition is in progress.
If you would like to contribute please send articles (in word format only) to cik@cham.co.uk.
Thank you.
AGENT NEWS
ACFDA, CHAM's Agent in North America has submitted a paper and presentation for the 2014 ASSE_MEC Conference. These give a brief review of recent validated PHOENICS CFD models applied for risk and safety assessments (flammable gas release and dispersion , atmospheric pollutant dispersion and twophase plumes from cooling towers and other industrial installations).
These materials show the PHOENICS modeling capabilities and underline the beneficial use of CFD in risk and safety analyses. More information on the models and training/consulting options can be obtained by contacting info@acfda.org
CLICK HERE FOR PRESENTATION
CLICK HERE FOR PAPER
