OpenFOAM® v1606+: New Solvers

OpenFOAM® v1606+: New Solvers

30/06/2016

New multiphase solver for condensation and evaporation

The new interCondensatingEvaporatingFoam solver supports evaporation and condensation between a fluid and vapour for incompressible, non-isothermal immiscible fluids, employing Volume of Fluid (VoF) interface capturing

Fluid and vapour properties are set in the transportProperties dictionary, e.g. for the flow of FC-72 coolant:

vapour
{
    transportModel  Newtonian;
    nu              nu [0 2 -1 0 0 0 0]  5e-7;
    rho             rho [1 -3 0 0 0 0 0] 14.9;

    Cp              Cp [0 2 -2 -1 0 0 0] 895.2;   // FC72 vapour
    Cv              Cv [0 2 -2 -1 0 0 0] 870.4;   // Cv = Cp - R/w
    kappa           kappa [1 1 -3 -1 0 0 0] 0.01; // FC72 vapour
    hf              hf [0 2 -2 0 0 0 0] 93.0e3;   // heat of formation
}
The condensation and evaporation mass transfer model is described in the phaseChangeProperties file in the $FOAM_CASE/constant directory. Currently only the constant run-time selectable model is available. This calculates the rate of condensation and evaporation according to:

pict\relax \special {t4ht=

pict\relax \special {t4ht=

where:

  • TSat  \relax \special {t4ht= is specified in the thermophysicalProperties file
  • Cc  \relax \special {t4ht= and Ce  \relax \special {t4ht= are the condensation and evaporation coefficients [1/s/K]
  • T  \relax \special {t4ht= is the system mixture temperature
  • αv  \relax \special {t4ht= is the vapour volume fraction
  • αl  \relax \special {t4ht= is the liquid volume fraction
  • ρl  \relax \special {t4ht= is the liquid density
  • ρv  \relax \special {t4ht= is the vapour density

To include the pressure-work    ∙
p∇  (U )  \relax \special {t4ht= term into the energy equation, the pDivU switch must be set to true.

Examples
CondensatingVessel: $FOAM_TUTORIALS/multiphase/interCondensingEvaporatingFoam/condensatingVessel

Source code
interCondensatingEvaporatingFoam $FOAM_SOLVERS/multiphase/interCondensingEvaporatingFoam

New multiphase solver with particle modelling

The new MPPICInterFoam solver combines Multi-Phase Particle In Cell (MP-PIC) Lagrangian cloud modelling for particles with high volume loading, with two phase isothermal and immiscible fluids modelling using Volume of Fluid (VOF) interface capturing.

Particles are modelled using the same approach adopted in the MPPICfoam solver, including the effect of the volume fraction of particles on the continuous phase.

To limit the particles crossing the interface, typically from liquid to gas, a new interface force was introduced. This force acts in the direction normal to the interface and only near the interface according to the expression

pict\relax \special {t4ht=

where m  \relax \special {t4ht= is the particle mass, αw  \relax \special {t4ht= the liquid volume fraction, and C  \relax \special {t4ht= a model coefficient. These are specified in the particleForces sub-dictionary of the cloudProperties file.

...
subModels
{
    particleForces
    {
        WenYuDrag
        {
            alphac      alphac;
        }
        gravity;
        interface
        {
            C            -10;
            alphaName    alpha.water;
        }
    }
...
The solver includes support for Multiple Reference Frame (MRF) forces, specified via the MRFProperties file, and other forces via fvOptions. Turbulence modelling is generic, supporting RAS, LES/DES or laminar models.

The following animation shows the results from the tutorial case, showing particles being lifted as the column rises, and subsequently falling under the effect of gravity.

Example
twoPhasePachuka: $FOAM_TUTORIALS/multiphase/MPPICInterFoam/twoPhasePachuka

Source code
$FOAM_SOLVERS/multiphase/MPPICInterFoam

Acoustic damping

The new acousticDampingSource fvOption has been implemented to damp spurious pressure waves for acoustic analyses. The new acoustic damping, sometimes referred to as an acoustic sponge-zone, combines the theories of acoustic resistivity, porous resistance and inertial under-relaxation based on a reference solution taken from the far-field steady or mean flow. The new model is designed to:

  • damp acoustic waves generated from unsteady flow before they propagate to imperfect non-reflective inflow/outflow boundaries, and
  • damp the generation and propagation of spurious numerical acoustic waves in low-quality meshes and severe mesh coarsening/refinement interfaces.

The user supplies both a damping coefficient, targeting a frequency or frequency range, and a ramping distance based on characteristic wavelengths, e.g.

acousticDampingSource
{
    type            acousticDampingSource;
    active          yes;

    acousticDampingSourceCoeffs
    {
        timeStart        0.00;
        duration         1000.0;
        selectionMode    cellZone;
        cellZone         selectedCells;
        centre           (0 0 0);
        radius1          0.1;
        radius2          1.2;
        frequency        3000;
        URef             UMean;
    }
}
The following image shows how a 1-D acoustic wave of frequency, f  \relax \special {t4ht=, is damped using a cosine-ramping function within 2  \relax \special {t4ht= to 3  \relax \special {t4ht= wavelengths, λ =  c∕f  \relax \special {t4ht=.

[Picture]

Examples
Sine wave damping 1-D: $FOAM_TUTORIALS/compressible/rhoPimpleFoam/laminar/sineWaveDamping

A 3-D example of acoustic damping of a shedding cylinder is also available in OpenCFDs Exchange Platform Knowledge Base.

Source code
$FOAM_SRC/fvOptions/sources/derived/acousticDampingSource