CFD Online Discussion Forums - Post processing to tecplot

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - Post processing to tecplot (https://www.cfd-online.com/Forums/openfoam/105777-post-processing-tecplot.html)

Post processing to tecplot

Hi guys,
I am trying to post process my openFoam simulation, by using the istruction

-->foamToTecplot360

The problem is that I encounter the following error message:

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

Valid patchField types are :

52
(
advective
buoyantPressure
calculated
codedFixedValue
codedMixed
cyclic
cyclicAMI
cyclicSlip
directionMixed
empty
fan
fanPressure
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
multiphaseFixedFluxPressure
nonuniformTransformCyclic
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
phaseHydrostaticPressure
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
uniformTotalPressure
waveSurfacePressure
waveTransmissive
wedge
zeroGradient
)

file: /home1/dcappell/OpenFOAM/-2.1.1/run/tutorials/incompressible/simpleFoam/Hump_model_k_epsilon/0/nut::boundaryField::lowerWall from line 41 to line 42.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /u/dcappell/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135.

FOAM exiting
---------------------------------------------------------------------------------------------------------------------------
It seems that Tecplot is not compatible with turbulent wall functions...

Do you know how to fix this problem ?

Thank you very much !

The newest Tecplot versions have a native reader for OpenFOAM data, so there is no need for conversion with this tool.

Thank you for your answer, Bernard,
Could you be more specific, please ?

Which folder / file should I upload ?

Greetings to all!

@daniele: I don't know how exactly you've built your OpenFOAM build, but I've tested with OpenFOAM 2.1.1 a case that used said boundary condition and I had no problems. Nonetheless:

For using foamToTecplot360, try adding to the case's "system/controlDict" this line:

Code:

libs ("libincompressibleRASModels.so");

This should forcefully load the missing BC.
As for using the latest Tecplot, probably you only have to open the folder of the case in Tecplot.
The initial news about this is here: http://www.cfd-online.com/Forums/ope...valuation.html

Best regards,
Bruno

Quote:

Originally Posted by wyldckat (Post 376357)

As for using the latest Tecplot, probably you only have to open the folder of the case in Tecplot.
The initial news about this is here: http://www.cfd-online.com/Forums/ope...valuation.html

It is enough to open the system/controlDict. Only be aware that you can open binary data, but not a binary stored mesh (you can use foamFormatConvert -constant -time :0 -noZero to convert this)

@ Bruno : your command -libs(...) - does not work. I have the following error:

"ill defined primitiveEntry"

@Bernhard: In controlDict you do not have any information about your solution...

Quote:

Originally Posted by danielec87 (Post 376464)

@Bernhard: In controlDict you do not have any information about your solution...

No, but like the .foam file for Paraview, Tepclot will find it from there.

Anyway, could you tell me how to plot the pressure coefficient over a curve wall (for instance an airfoil) in Paraview?
In this case I would avoid to use tecplot !

@daniele: Just in case I wasn't very clear, here is an example of a "system/controlDict":

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.x                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    location    "system";

    object      controlDict;

}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



application     simpleFoam;



startFrom       latestTime;



startTime       0;



stopAt          endTime;



endTime         1000;



deltaT          1;



writeControl    timeStep;



writeInterval   50;



purgeWrite      0;



writeFormat     ascii;



writePrecision  6;



writeCompression off;



timeFormat      general;



timePrecision   6;



runTimeModifiable true;



libs ("libincompressibleRASModels.so");

Notice there is a space between "libs" and "(".

Thank you...it works perfectly now !