View Issue Details

IDProjectCategoryView StatusLast Update
0002048OpenFOAM[All Projects] Bugpublic2016-04-13 12:40
ReporteralsdiaAssigned Tohenry 
PrioritynormalSeveritymajorReproducibilityalways
Status closedResolutionno change required 
PlatformLinuxOSRHELOS Version7
Product Version 
Fixed in Version 
Summary0002048: turbulentHeatFluxTemperature cannot be used anymore with buoyantBoussinesqSimpleFoam
DescriptionIn OpenFOAM 2.4.0 it was possible to use the boundary condition turbulentHeatFluxTemperature with an incompressible solver like buoyantBoussinesqSimpleFoam. But in OpenFOAM 3.0.1 I face the error:

--> FOAM FATAL IO ERROR:
Unknown patchField type turbulentHeatFluxTemperature for patch type wall

why in OF240 the turbulentHeatFluxTemperature is present in incompressible
https://github.com/OpenFOAM/OpenFOAM-2.4.x/blob/2b147f41daf9ca07d0fb4c6b0576dc3d10a435f3/src/turbulenceModels/incompressible/turbulenceModel/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.H

but not in OF301?
https://github.com/OpenFOAM/OpenFOAM-3.0.x/search?utf8=%E2%9C%93&q=turbulentHeatFluxTemperature
Steps To ReproduceTake the hotRoom tutorial:
/opt/openfoam30/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/hotRoom

Change the patch floor in the 0/T.org file to:

floor
{
        type turbulentHeatFluxTemperature;
        gradient uniform 0;
        heatSource power;
        q uniform 64;
        alphaEff alphaEff;
        value uniform 300;
}

Launch the Allrun

SIMPLE: convergence criteria
    field p_rgh tolerance 0.01
    field U tolerance 0.0001
    field T tolerance 0.01
    field "(k|epsilon|omega)" tolerance 0.001

Reading thermophysical properties

Reading field T



--> FOAM FATAL IO ERROR:
Unknown patchField type turbulentHeatFluxTemperature for patch type wall

Valid patchField types are :

104
(
advective
alphatJayatillekeWallFunction
atmBoundaryLayerInletEpsilon
atmBoundaryLayerInletK
calculated
codedFixedValue
codedMixed
compressible::alphatJayatillekeWallFunction
compressible::alphatWallFunction
compressible::thermalBaffle1D<hConstSolidThermoPhysics>
compressible::thermalBaffle1D<hPowerSolidThermoPhysics>
compressible::turbulentHeatFluxTemperature
Additional InformationIf we repeat the same procedure in OF2.4.0 :
tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/hotRoom

1) change the patch floor 0/T.org:

floor
{
        type turbulentHeatFluxTemperature;
        gradient uniform 0;
        heatSource power;
        q uniform 64;
        alphaEff alphaEff;
        value uniform 300;
}

2) add the line rhoCp0 1173; in transportProperties

3) launch the Allrun

SIMPLE: convergence criteria
    field p_rgh tolerance 0.01
    field U tolerance 0.0001
    field T tolerance 0.01
    field "(k|epsilon|omega)" tolerance 0.001


Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 0.0475703, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00653368, No Iterations 7
time step continuity errors : sum local = 5.65209e-09, global = -4.97342e-25, cumulative = -4.97342e-25
DILUPBiCG: Solving for epsilon, Initial residual = 0.0458815, Final residual = 0.00188758, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0721881, No Iterations 1
ExecutionTime = 0.05 s ClockTime = 0 s

Time = 2

DILUPBiCG: Solving for Ux, Initial residual = 0.651198, Final residual = 0.00701648, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.558322, Final residual = 0.00593882, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.651198, Final residual = 0.00701648, No Iterations 1
DILUPBiCG: Solving for T, Initial residual = 0.431799, Final residual = 0.0275141, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.86867, Final residual = 0.00688476, No Iterations 27
time step continuity errors : sum local = 3.05697e-07, global = -6.73656e-24, cumulative = -7.2339e-24
DILUPBiCG: Solving for epsilon, Initial residual = 0.115159, Final residual = 0.00602713, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.624686, Final residual = 0.0490608, No Iterations 1
ExecutionTime = 0.06 s ClockTime = 0 s

OK no error.
TagsNo tags attached.

Activities

alsdia

2016-04-13 08:00

reporter   ~0006107

I used the following workaround to solve the error:
As indicated here http://www.openfoam.org/mantisbt/view.php?id=1856
Use buoyantSimpleFoam instead of buoyantBoussinesqSimpleFoam and set in thermophysicalProperties equationOfState Boussinesq;
then is possible to set

floor
{ type compressible::turbulentHeatFluxTemperature;
      gradient uniform 0;
      heatSource power;
      q uniform 64;
      kappa fluidThermo;
      kappaName none;
}

henry

2016-04-13 09:06

manager   ~0006108

Use buoyantSimpleFoam with

    equationOfState Boussinesq;

This formulation is more general than buoyantBoussinesqSimpleFoam which will probably be removed form future releases usless there is a strong argument to keep it.

Issue History

Date Modified Username Field Change
2016-04-13 02:36 alsdia New Issue
2016-04-13 08:00 alsdia Note Added: 0006107
2016-04-13 09:06 henry Note Added: 0006108
2016-04-13 09:06 henry Status new => closed
2016-04-13 09:06 henry Assigned To => henry
2016-04-13 09:06 henry Resolution open => no change required