thermalSolid

This page documents the heat-conduction-only solid model. The runtime type is:

thermalSolid

The model solves the transient heat equation for temperature T in a solid region. It does not solve a momentum equation, and the displacement field stays at its initial value. It exists to provide the solid side of conjugate heat transfer, where a fluid model exchanges temperature and heat flux with a rigid solid.

User Guide

What this model solves

thermalSolid:

• solves rhoC*ddt(T) == laplacian(k, T), with no source terms;
• takes C and k from a thermalModel, configured in constant/thermalProperties;
• implements the setTemperatureAndHeatFlux(), setEqInterHeatTransferCoeff(), faceZoneTemperature(), faceZoneHeatFlux() and faceZoneHeatTransferCoeff() interface used by the thermal fluid-solid interfaces;
• returns a zero surface-normal gradient from tractionBoundarySnGrad(), so traction boundary conditions have no effect.

Supported solution algorithms

This model implements a single, segregated implicit loop for the heat equation. It does not read solutionAlgorithm.

Model options

absoluteTemperatureTolerance is an absolute change in degrees: once the temperature stops moving by more than this between outer iterations, the thermal loop is considered converged.

The relevant inherited solidModel entries are:

The mechanical options inherited from solidModel are read but have no effect, since no momentum equation is assembled.

Required input files

• T and D in the time directory;
• constant/solidProperties;
• constant/thermalProperties, providing the thermal sub-dictionary;
• constant/mechanicalProperties, which is still needed because the density is taken from the mechanical law when forming rhoC;
• constant/g.

T is MUST_READ, so a case that omits it will fail at construction.

Example constant/thermalProperties:

thermal
{
    type            constant;
    C               C [0 2 -2 -1 0 0 0] 434;
    k               k [1 1 -3 -1 0 0 0] 250;
}

Recommended dictionary setup

Minimal example for constant/solidProperties, as used on the solid side of a conjugate heat transfer case:

solidModel        thermalSolid;

thermalSolidCoeffs
{
    nCorrectors                  10000;
    solutionTolerance            1e-06;
    alternativeTolerance         1e-07;
    absoluteTemperatureTolerance 1e-06;
    infoFrequency                100;
}

fvSchemes must provide a laplacian(k,T) entry, and fvSolution must provide a solver for T.

Boundary conditions

Temperature boundaries use the usual OpenFOAM scalar patch types, plus:

• thermalRobin, which carries both a temperature and a heat flux and is the type required on a thermal fluid-solid interface. Calling setTemperatureAndHeatFlux() on any other patch type is a fatal error.
• thermalConvection, for a convective heat-transfer boundary.

Displacement boundary conditions may be present but are not solved for.

Field glossary

• T: temperature; the only field this model solves for.
• grad(T): temperature gradient, used to report the heat flux.
• heatFlux: -k*grad(T), constructed and written by writeFields().
• rhoC: product of density and specific heat capacity.

Each write also prints the maximum and minimum temperature and the maximum magnitude of the heat flux.

Developer Notes

Class role

thermalSolid inherits directly from solidModel and adds a thermalModel member. It is the minimal solid model: it satisfies the solidModel interface but leaves the mechanical part inert.

• nonLinGeom() returns LINEAR_GEOMETRY;
• solutionD() returns D(), but D is never solved for;
• tractionBoundarySnGrad() returns a zero field of patch size.

The header's Description block, inherited from thermalLinGeomSolid, still mentions a strongly coupled momentum equation; the implementation solves the heat equation only.

Construction

The constructor calls the base solidModel constructor, constructs the thermalModel from the mesh, builds rhoC_ as thermal.C()*mechanical().rho() and k_ from thermal.k(), reads T (MUST_READ), creates grad(T), reads absoluteTemperatureTolerance, and forces creation of T.oldTime().

Note that DisRequired() is not called, consistent with the absence of a momentum solve.

evolve()

A single loop on the heat equation: store T, relax and solve rhoC*ddt(T) - laplacian(k, T), relax T, update grad(T). On OpenFOAM.com builds the solver-performance dictionary is cleared each iteration, to avoid an expensive copy of the residual history when many correctors run. The loop exits through the private converged() overload or when iCorr reaches nCorrectors. evolve() always returns true.

Conjugate heat transfer interface

setTemperatureAndHeatFlux() and setEqInterHeatTransferCoeff() write into a thermalRobin patch field; faceZoneTemperature(), faceZoneHeatFlux() and faceZoneHeatTransferCoeff() read the corresponding quantities back out on a global face zone. These are the hooks the thermal fluid-solid interfaces call each coupling iteration.

Extension points

• evolve() if the heat equation needs source terms;
• the private converged() overload for a different convergence criterion.

If a mechanical solve is ever wanted here, prefer thermalLinGeomSolid instead of extending this class.

Tutorials

Cases that select thermalSolid:

• thermoFluidSolidInteraction/flowOverHeatedPlate
• thermoFluidSolidInteraction/thermalCavity

In both, thermalSolid is the solid region of a conjugate heat transfer simulation, and the solid does not deform.