OpenFOAM® v2.0.0: New Thermophysical Modelling

OpenFOAM® v2.0.0: New Thermophysical Modelling

16th June 2011

View Factor Radiation Model

In addition to the P1 model and finite volume discrete-ordinate method (fvDOM), OpenFOAM now has an implementation of a view factor model for radiative heat transfer, specifically between surfaces. The method begins with the generation of rays between discrete faces of the surfaces, using the viewFactorsGen utility in OpenFOAM. Radiative heat transfer is then calculated by summing energy exchanges between ray end-points. A major benefit of this approach is that energy is only exchanged between parts of surface that are directly visible to one another, giving a representative solution to complex problems where some surfaces are shielded from radiative sources by others.

The view factor is the geometric function that describes the radiative contribution for the ray that accounts for ray length and face size/orientation. The model takes no account of any absorption, emission, or scattering of radiation. The computational time and memory requirement of the modelling is largely determined by the number of faces from which the rays emanate. In OpenFOAM, the cost can be reduced by grouping faces together using the faceAgglomerate pre-processing utility.

Source code
radiationModels library - $FOAM_SRC/thermophysicalModels/radiationModels
viewFactorsGen utility - $FOAM_UTILITIES/preProcessing/viewFactorsGen
faceAgglomerate utility - $FOAM_UTILITIES/preProcessing/faceAgglomerate
Example
multi region heater with radiation -
$FOAM_TUTORIALS/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeaterRadiation

New Thermophysical Properties Syntax

Prior to this release of OpenFOAM, the syntax for specifying model coefficients in the thermophysicalProperties dictionary has been a little confusing since it involved a string of numbers, e.g. 

fuel
fuel 1 44.0962 200 5000 1000
7.53414 0.0188722 -6.27185e-06 9.14756e-10 -4.78381e-14 -16467.5 -17.8923
0.933554 0.0264246 6.10597e-06 -2.19775e-08 9.51493e-12 -13958.5 19.2017
1.67212e-06 170.672;

In the latest release the syntax has been changed to include keywords to enable the user to identify what each coefficient is. The above entry in the new (v2.0.0) syntax is:

fuel
{
    specie
    {
        nMoles       1;
        molWeight    16.0428;
    }
    thermodynamics
    {
        Tlow         200;
        Thigh        6000;
        Tcommon      1000;
        highCpCoeffs (1.63543 0.0100844 -3.36924e-06 5.34973e-10 -3.15528e-14 -10005.6 9.9937);
        lowCpCoeffs  (5.14988 -0.013671 4.91801e-05 -4.84744e-08 1.66694e-11 -10246.6 -4.64132);
    }
    transport
    {
        As           1.67212e-06;
        Ts           170.672;
    }
}

Further information
User Guide: Thermophysical models
Examples
Any tutorial with a thermophysicalProperties dictionary, e.g. type
find $FOAM_TUTORIALS -name thermophysicalProperties

Thermal Baffles

A new thermal baffle functionality has been added that enables the effects of heat transfer between the main flow and thin walls to be modelled. Two types of thermal baffle have been implemented:

  • as a new boundary condition, that employs 1 dimensional, steady-state heat transfer across a thickness, with the option to include an additional heat source; can be used with most heat transfer solvers;
  • as a separate mesh region, for which 3 dimensional heat transfer is modelled using thermodynamics specified using the new solids-based thermodynamics packages; incorporated into a new buoyantBaffleSimpleFoam solver.

Source code
buoyantBaffleSimpleFoam solver - $FOAM_SOLVERS/heatTransfer/buoyantBaffleSimpleFoam
thermoBaffleModels library - $FOAM_SRC/regionModels/thermoBaffleModels
thermal baffle BC - $FOAM_SRC/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/temperatureThermoBaffle1D
Example
cooling of a circuit board, $FOAM_TUTORIALS/heatTransfer/buoyantBaffleSimpleFoam/circuitBoardCooling

Thermal Porous Zones

The functionality of porous zones has been extended to include the handling of thermal effects, through the implementation of a new thermalPorousZone library. The library currently offers a fixed temperature model for the porous region but can be extended for more complex models.

Source code
thermalPorousZone library - $FOAM_SRC/thermophysicalModels/thermalPorousZone
rhoPorousMRFSimpleFoam solver -
$FOAM_SOLVERS/compressible/rhoSimpleFoam/rhoPorousMRFSimpleFoam
Examples
Angle duct examples in $FOAM_TUTORIALS/compressible/rhoPorousMRFSimpleFoam

Thermodynamic Packages including Solids

A new SLGThermo library has been created for cases that involve thermodynamics of solids, liquids and gases. It is incorporated into solvers that involve thermodynamics and reactions between solid, liquid and gas phases, such as those that include pyrolysis, surface film modelling and reacting particles.

Source code
buoyantBaffleSimpleFoam solver - $FOAM_SOLVERS/heatTransfer/buoyantBaffleSimpleFoam
thermoBaffleModels library - $FOAM_SRC/regionModels/thermoBaffleModels
thermal baffle BC - $FOAM_SRC/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/temperatureThermoBaffle1D
Examples
fireFoam cases - $FOAM_TUTORIALS/combustion/fireFoam

A new basicSolidThermo library has been created for thermodynamics of solids. It is now used in all conjugate heat transfer solvers and can include temperature dependent properties with anisotropy effects (direction dependency).

Source code
basicSolidThermo library $FOAM_SRC/thermophysicalModels/basicSolidThermo
chtMultiRegionFoam solver - $FOAM_SOLVERS/heatTransfer/chtMultiRegionFoam
Examples
chtMultiRegionFoam cases - $FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam