[ranasa]

Hello,

i want to model a turbulent mixing process in a bend, using the buoyantBoussinesqSimpleFoam;

i want to use alphatWallFunction in alphat file for the wall, but there is a problem that states:


Reading field alphat

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

Valid patchField types are :

104
(
MarshakRadiation
MarshakRadiationFixedTemperature
advective
alphatJayatillekeWallFunction
atmBoundaryLayerInletEpsilon
calculated
codedFixedValue
codedMixed
compressible::thermalBaffle1D<hConstSolidThermoPhy sics>
compressible::thermalBaffle1D<hExponentialSolidThe rmoPhysics>
compressible::turbulentHeatFluxTemperature
compressible::turbulentTemperatureCoupledBaffleMix ed
compressible::turbulentTemperatureRadCoupledMixed
cyclic
cyclicACMI
cyclicAMI
cyclicSlip
directionMixed
empty
energyJump
energyJumpAMI
epsilonLowReWallFunction
epsilonWallFunction
externalCoupled
externalCoupledTemperature
externalWallHeatFluxTemperature
fWallFunction
fan
fanPressure
fixedEnergy
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedJump
fixedJumpAMI
fixedMean
fixedPressureCompressibleDensity
fixedUnburntEnthalpy
fixedValue
freestream
freestreamPressure
gradientEnergy
gradientUnburntEnthalpy
greyDiffusiveRadiation
greyDiffusiveRadiationViewFactor
inletOutlet
inletOutletTotalTemperature
kLowReWallFunction
kqRWallFunction
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
mixedEnergy
mixedUnburntEnthalpy
nonuniformTransformCyclic
nutLowReWallFunction
nutTabulatedWallFunction
nutURoughWallFunction
nutUSpaldingWallFunction
nutUWallFunction
nutkAtmRoughWallFunction
nutkRoughWallFunction
nutkWallFunction
omegaWallFunction
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
phaseHydrostaticPressure
prghPressure
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetry
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalFlowRateAdvectiveDiffusive
totalPressure
totalTemperature
turbulentHeatFluxTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
turbulentMixingLengthDissipationRateInlet
turbulentMixingLengthFrequencyInlet
uniformDensityHydrostaticPressure
uniformFixedGradient
uniformFixedValue
uniformInletOutlet
uniformJump
uniformJumpAMI
uniformTotalPressure
v2WallFunction
variableHeightFlowRate
wallHeatTransfer
waveSurfacePressure
waveTransmissive
wedge
wideBandDiffusiveRadiation
zeroGradient
)


I tried choosing zeroGradient and alphatJayatillekeWallFunction;
this is the error message for both cases;

.
.
.
--> FOAM FATAL ERROR:
Different dimensions for =
dimensions : [1 -1 -1 0 0 0 0] = [0 2 -1 0 0 0 0]

(it means that the alphat and kappat are of the same dimensions)!?!

thanks for any help,
Regards

[lllshahablll]

Any Update about this error?
I have the same problem too

[wyldckat]

Greetings to all!

More details are needed in order to diagnose the problem. Here are a few questions that might help isolate the problem:

1. Which OpenFOAM version is being used?
2. The case you are trying to run, for which OpenFOAM version was it designed to work with?
3. Do you know based on which tutorial the case is derived from?
4. Which solver are you trying to use?

Best regards,
Bruno

[lllshahablll]

Originally Posted by wyldckat

Greetings to all!

More details are needed in order to diagnose the problem. Here are a few questions that might help isolate the problem:

1. Which OpenFOAM version is being used?
2. The case you are trying to run, for which OpenFOAM version was it designed to work with?
3. Do you know based on which tutorial the case is derived from?
4. Which solver are you trying to use?

Best regards,
Bruno

Dear Bruno

Kindly find the answers below for my case:

1.It's OF3.0
2. I tried to reproduce it from a printed book which is tested the case for OF2.1.0
3. But I used a case from tutorials of OF3.0 to make the needed files (hotRoom).
4.the solver is "buoyantBoussinesqSimpleFoam"

Thanks
Shahabeddin

[fabian_roesler]

Hi,

alphatWallFunction is only available in compressible solvers. As you are using a Boussinesq Solver, your fluid is incompressible and only the alphatJayatillekeWallFunction can be used.

Incompressible: http://foam.sourceforge.net/docs/cpp/a10795.html
Compressible: http://foam.sourceforge.net/docs/cpp/a10792.html

Cheers

Fabian

[lllshahablll]

Originally Posted by fabian_roesler

Hi,

alphatWallFunction is only available in compressible solvers. As you are using a Boussinesq Solver, your fluid is incompressible and only the alphatJayatillekeWallFunction can be used.

Incompressible: http://foam.sourceforge.net/docs/cpp/a10795.html
Compressible: http://foam.sourceforge.net/docs/cpp/a10792.html

Cheers

Fabian

Hi Dear Fabian

When I use 'alphatJayatillekeWallFunction' instead the error is like bellow:

buoyantBoussinesqSimpleFoam > log


--> FOAM FATAL IO ERROR: 
keyword Prt is undefined in dictionary "/home/shahabeddin/Desktop/elbow/0/alphat.boundaryField.walll"

file: /home/shahabeddin/Desktop/elbow/0/alphat.boundaryField.walll from line 26 to line 27.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 442.

FOAM exiting

[fabian_roesler]

Well yes. You have to define turbulent Prandtl number for the patches.

yourPatch
{
    type alphatJayatillekeWallFunction;
    Prt  0.85;
}

Cheers

Fabian

[Johnnie]

I have this problem, some help.




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

Valid patchField types are :

112
(
MarshakRadiation
MarshakRadiationFixedTemperature
advective
calculated
codedFixedValue
codedMixed
compressible::alphatJayatillekeWallFunction
compressible::alphatWallFunction
compressible::thermalBaffle1D<hConstSolidThermoPhy sics>
compressible::thermalBaffle1D<hPowerSolidThermoPhy sics>
compressible::turbulentTemperatureCoupledBaffleMix ed
compressible::turbulentTemperatureRadCoupledMixed
convectiveHeatTransfer
cyclic
cyclicACMI
cyclicAMI
cyclicRepeatAMI
cyclicSlip
directionMixed
empty
energyJump
energyJumpAMI
epsilonWallFunction
externalCoupled
externalCoupledTemperature
externalWallHeatFluxTemperature
extrapolatedCalculated
fWallFunction
fanPressure
fanPressureJump
fixedEnergy
fixedFluxExtrapolatedPressure
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedJump
fixedJumpAMI
fixedMean
fixedMeanOutletInlet
fixedPressureCompressibleDensity
fixedProfile
fixedUnburntEnthalpy
fixedValue
freestream
freestreamPressure
gradientEnergy
gradientUnburntEnthalpy
greyDiffusiveRadiation
greyDiffusiveRadiationViewFactor
inletOutlet
inletOutletTotalTemperature
interfaceCompression
kLowReWallFunction
kqRWallFunction
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
mixedEnergy
mixedUnburntEnthalpy
nonuniformTransformCyclic
nutLowReWallFunction
nutTabulatedWallFunction
nutURoughWallFunction
nutUSpaldingWallFunction
nutUWallFunction
nutkRoughWallFunction
nutkWallFunction
omegaWallFunction
outletInlet
outletMappedUniformInlet
partialSlip
phaseHydrostaticPressure
plenumPressure
porousBafflePressure
pressure
prghPressure
prghTotalHydrostaticPressure
prghTotalPressure
prghUniformDensityHydrostaticPressure
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetry
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalFlowRateAdvectiveDiffusive
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
turbulentMixingLengthDissipationRateInlet
turbulentMixingLengthFrequencyInlet
uniformDensityHydrostaticPressure
uniformFixedGradient
uniformFixedValue
uniformInletOutlet
uniformJump
uniformJumpAMI
uniformTotalPressure
v2WallFunction
variableHeightFlowRate
wallHeatTransfer
waveSurfacePressure
waveTransmissive
wedge
wideBandDiffusiveRadiation
zeroGradient
)


file: /home/johnniez/Desktop/openfoamtutorial/cuboidpond/0/alphat.boundaryField.bottom from line 29 to line 31.

From function static Foam::tmp<Foam::fvPatchField<Type> > Foam::fvPatchField<Type>::New(const Foam::fvPatch&, const Foam:imensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
in file /home/ubuntu/OpenFOAM/OpenFOAM-7/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 134.

FOAM exiting