OpenFOAM 2.2.0: Physical Modelling

Particle Tracking

The particle injection modelling included as part of the Lagrangian intermediate library has been refactored to allow the specification of multiple (potentially different) injection models. The models are now specified as a list, e.g.

injectionModels
{
    model1
    {
        type            manualInjection;
        massTotal       0.0001;
        parcelBasisType mass;
        SOI             0;
        positionsFile   "particlePositions";
        U0              ( 0 0 0 );
        sizeDistribution
        {
            type        fixedValue;
            fixedValueDistribution
            {
                value           5e-06;
            }
        }
    }
    model2
    {
        type            coneNozzleInjection;
        SOI             0;
        massTotal       6.0e-6;
        parcelBasisType mass;
        injectionMethod disc;
        flowType        flowRateAndDischarge;
        outerDiameter   1.9e-4;
        innerDiameter   0;
        duration        1.25e-3;
        position        ( 0 0.0995 0 );
        direction       ( 0 -1 0 );
        parcelsPerSecond 20000000;
        flowRateProfile constant 1;

        Cd              constant 0.9;

        thetaInner      constant 0.0;
        thetaOuter      constant 10.0;

        sizeDistribution
        {
            type        RosinRammler;

            RosinRammlerDistribution
            {
                minValue        1e-06;
                maxValue        0.00015;
                d               0.00015;
                n               3;
            }
        }
    }
}

A new char oxidation model is available to the coalCombustion library, called COxidationHurtMitchell, based on the reference:

• Hurt R, Mitchell R, 1992. Unified high-temperature char combustion kinetics for a suite of coals of various rank. 24th Symposium in Combustion, The Combustion Institute, pp 1243-1250.

In addition, particle lift and virtual mass forces are now available.

A new cloud function object called particleCollector has been implemented that allows the collection of particle mass and mass flow rate to be captured across either:

• an arbitrary list of polygons
• sections of concentric circles

An example of the concentric circles variant is shown below, taken from the splashPanel tutorial case, in which the sectors are coloured by the total collected mass.

See $FOAM_TUTORIALS/lagrangian/reactingParcelFilmFoam/splashPanel

For particle tracking, the following modifications have been made to the solver applications:

• new simpleReactingParcelFoam: steady state version of the reactingParcelFoam solver
• The porousExplicitSourceReactingParcelFoam is deprecated; the equivalent functionality is now availabe in the reactingParcelFoam solver, combined with the new fvOptions functionality.

Example

• Vertical channel
  $FOAM_TUTORIALS/lagrangian/simpleReactingParcelFoam/verticalChannel

Surface Film Modelling

Many internal improvements have been made to the surface film modelling library, including new boundary conditions for inclined surfaces, e.g.

• inclinedFilmNusseltHeight, and
• inclinedFilmNusseltInletVelocity

In addition, the structure has been put in place to allow enhanced communication between region models, using the arbitrary mesh interface functionality.

Porosity Modelling

Porosity modelling in OpenFOAM has been redesigned to follow OpenFOAM’s standard approach for run-time model selection, creating a more flexible framework for future development of the modelling. The changes also make use of the new fvOptions framework, making porosity modelling available across a broad range of applications. The model selection are now specified in the $FOAM_CASE/constant/porosityProperties dictionary, e.g.

filter1
{
    cellZone        filter;
    active          true;
    type            DarcyForchheimer;

    DarcyForchheimerCoeffs
    {
        d   d [0 -2 0 0 0 0 0] (500000 -1000 -1000);
        f   f [0 -1 0 0 0 0 0] (0 0 0);

        coordinateSystem
        {
            e1  (1 0 0);
            e2  (0 1 0);
        }
    }
}

Examples

• Angled Duct (incompressible and compressible)
  $FOAM_TUTORIALS/incompressible/porousSimpleFoam/angledDuctImplicit
$FOAM_TUTORIALS/compressible/rhoPorousSimpleFoam/angledDuctImplicit

Turbulence Modelling

Incompressible and compressible variants of the v2–f turbulence model have been implemented. The model solves for turbulence k and epsilon, with additional equations for the turbulence stress normal to streamlines, v2, and elliptic damping function, f. The model includes appropriate wall functions for all variables.

The variant of v2–f is implemented from the following references. For Davidson et al., only the first correction is included, implemented using the davidsonCorrectNut function.

• Lien F-S, Kalitzin G, 2001. Computations of transonic flow with the v2-f turbulence model. Int. J. Heat Fluid Flow 22:53-61.
• Davidson L, Nielsen P, Sveningsson A, 2003. Modifications of the v2-f model for computing the flow in a 3D wall jet. Turbulence, Heat and Mass Transfer 4:577-584.

In addition, the turbulence wall function framework has been significantly updated to enable turbulence RAS wall functions to be applied to LES calculations.

Other

The combustion models library has been refactored to allow both finite-rate chemistry and single-step reaction models to coexist. This means that all combustion models are available at run-time without the need for specialised solver variants. For multiphase flows, a new cavitatingDyMFoam solver is included which is the dynamic mesh motion version of the cavitatingFoam solver.