OpenFOAM v14 User Guide

[version 14][version 13][version 12][version 11][version 10][version 9][version 8][version 7][version 6]

[chapter contents][previous topic][next topic][index]

6.6 Thermal boundary conditions

For solutions involving thermal energy, boundary conditions are required for the temperature ﬁeld $\text{[math]}$ in the 0/T ﬁle. While conventional conditions can be used at inlet and outlet patches, e.g. ﬁxedValue and zeroGradient, respectively, the following bespoke conditions are available for wall patches.

externalTemperature : models heat transfer at an external wall, with various options to specify the heat ﬂux.
coupledTemperature : models heat transfer between regions (ﬂuid or solid) in a conjugate heat transfer simulation.

The externalTemperature condition, illustrated in Figure 6.5 , can include one or more of the following heat ﬂuxes.

Prescribed power Q (W) or power ﬂux q (W m $\text{[math]}$ ).
Thermal radiation from inside the domain, qr speciﬁes the radiation ﬁeld name.
Convective heat transfer with a coeﬃcient h and ambient temperature Ta, both a Function1 of time.
The coeﬃcient h can alternatively be conﬁgured using a specialised externalWallLayersHeatTransferCoefficient ﬁeld function, which can emulate conduction through additional layers of material on the outside of the wall patch.
External thermal radiation with a speciﬁed emissivity.

$PICT\relax \special {t4ht=$

Figure 6.5: The externalTemperature boundary condition.

The foamInfo script provides further details and examples of the use of the externalTemperature condition.

foamInfo externalTemperature

The following example shows the use with a straightforward heat transfer coeﬃcient h.

    wall
    {
        type    externalTemperature;
        Ta      constant 300;
        h       constant 10;
        value   uniform  400;
    }

The example below demonstrates the externalWallLayersHeatTransferCoefficient ﬁeld function which includes conduction through layers of material. The conducting layers are described by a list of thicknesses and corresponding conductivities via the thicknessLayers and kappaLayers lists, respectively.

    wall
    {
        type    externalTemperature;
        Ta      constant 300;
        h
        {
            type             externalWallLayersHeatTransferCoefficient;
            h                10.0;
            thicknessLayers  (0.1 0.2 0.3 0.4);
            kappaLayers      (1 2 3 4);
        }
        value   uniform  400;
    }

The coupledTemperature condition calculates the heat ﬂux between regions in a conjugate heat transfer simulation. It is shown in Figure 6.6 with regions labelled 1 and 2. The condition is applied at the interface patches of both regions. If we imagine the condition applied to region 1 in the ﬁgure, qr speciﬁes the name of the variable for thermal radiation from within region 1, and qrNbr is the name of the variable in the neighbour region, i.e. region 2.

$PICT\relax \special {t4ht=$

Figure 6.6: The coupledTemperature boundary condition.

The condition is similar it externalTemperature and can include additional conducting layers at the interface between the regions, e.g. to simulate a contact material, contaminant, liquid ﬁlm, etc. The conducting layers are speciﬁed by the wallLayersHeatTransferCoefficient ﬁeld function which includes the thicknessLayers and kappaLayers parameters. An example of a coupledTemperature condition with conducting layers is shown below.

    wall
    {
        type    coupledTemperature;
        h
        {
            type             wallLayersHeatTransferCoefficient;
            thicknessLayers  (0.1 0.2 0.3 0.4);
            kappaLayers      (1 2 3 4);
        }
        value   uniform  400;
    }

The conducting layers are implemented as a ﬁeld function so that they can be extending to cases where the layer thickness is non-uniform. This is demonstrated in the example case in the $FOAM_TUTORIALS/multiRegion/CHT/thermalBending, which uses a specialised displacementGapHeatTransferCoefficient ﬁeld function which models a gap of non-uniform thickness between two regions, due to a displacement of one region due to thermal bending.

OpenFOAM v14 User Guide - 6.6 Thermal boundary conditions

CFD Direct

OpenFOAM v14 User Guide - 6.6 Thermal boundary conditions

How do I apply a wall thermal boundary condition in OpenFOAM?

6.6 Thermal boundary conditions