# OpenFOAM® v1606+: New Solvers

## 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:

{

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

}

where:

- is specified in the thermophysicalProperties file
- and are the condensation and evaporation coefficients [1/s/K]
- is the system mixture temperature
- is the vapour volume fraction
- is the liquid volume fraction
- is the liquid density
- is the vapour density

To include the pressure-work 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

where is the particle mass, the liquid volume fraction, and 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 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.

{

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;

}

}

- 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