CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Unknown patchField type alphatWallFunction for patch type wall

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 3 Post By fabian_roesler

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 1, 2014, 15:46
Default Unknown patchField type alphatWallFunction for patch type wall
  #1
New Member
 
rana
Join Date: Jul 2014
Posts: 21
Rep Power: 9
ranasa is on a distinguished road
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
ranasa is offline   Reply With Quote

Old   December 12, 2015, 16:35
Default
  #2
New Member
 
Shahabeddin
Join Date: Oct 2015
Location: Iran
Posts: 16
Rep Power: 8
lllshahablll is on a distinguished road
Any Update about this error?
I have the same problem too
lllshahablll is offline   Reply With Quote

Old   December 13, 2015, 08:52
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,965
Blog Entries: 45
Rep Power: 126
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
__________________
wyldckat is offline   Reply With Quote

Old   December 13, 2015, 16:44
Default
  #4
New Member
 
Shahabeddin
Join Date: Oct 2015
Location: Iran
Posts: 16
Rep Power: 8
lllshahablll is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
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
lllshahablll is offline   Reply With Quote

Old   December 14, 2015, 01:27
Default
  #5
Senior Member
 
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 213
Rep Power: 16
fabian_roesler is on a distinguished road
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
wyldckat, adkar and saavedra00 like this.
fabian_roesler is offline   Reply With Quote

Old   December 20, 2015, 17:52
Default
  #6
New Member
 
Shahabeddin
Join Date: Oct 2015
Location: Iran
Posts: 16
Rep Power: 8
lllshahablll is on a distinguished road
Quote:
Originally Posted by fabian_roesler View Post
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:

Code:
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
lllshahablll is offline   Reply With Quote

Old   December 22, 2015, 17:39
Default
  #7
Senior Member
 
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 213
Rep Power: 16
fabian_roesler is on a distinguished road
Well yes. You have to define turbulent Prandtl number for the patches.

Code:
yourPatch
{
    type alphatJayatillekeWallFunction;
    Prt  0.85;
}
Cheers

Fabian
fabian_roesler is offline   Reply With Quote

Old   November 21, 2019, 02:13
Default --> FOAM FATAL IO ERROR: Unknown patchField type alphatJayatillekeWallFunction for p
  #8
New Member
 
Tulirinya John
Join Date: Nov 2019
Posts: 1
Rep Power: 0
Johnnie is on a distinguished road
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
Johnnie is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
boundary conditions for simpleFoam calculation foam_noob OpenFOAM Running, Solving & CFD 8 July 1, 2015 08:07
[GAMBIT] periodic faces not matching Aadhavan ANSYS Meshing & Geometry 6 August 31, 2013 11:25
Floating Point Exception - wrong boundaries or general PC problem? OF 1.6 extend - A.Wendy OpenFOAM 0 February 27, 2013 04:50
[Commercial meshers] Using starToFoam clo OpenFOAM Meshing & Mesh Conversion 33 September 26, 2012 04:04
compressible two phase flow in CFX4.4 youngan CFX 0 July 1, 2003 23:32


All times are GMT -4. The time now is 13:17.