[Outbound]

Greetings,

I'm working on a Master's thesis in which I'm continuing some work meant to validate the use of a porous medium to simulate dense submerged vegetation in compound channel flow.

The first stage is meant to replicate the initial study carried out using ANSYS-CFX in OpenFOAM using porousSimpleFoam. Initially I'm just using a wall with slip condition to simulate the free surface given the porousSimpleFoam doesn't do free surface interaction.

I'm having some trouble setting up the case based on the angleDuctExplicit tutorial.

The mesh contains a symmetry plane and I'm not sure how to define it in the "k" file, i.e., the type for this boundary. I'm just trying the case to run right now, later on I'll have to configure it to use "k-w SST", but so far I haven't been able to properly configure all the "0" folder files and for the following code in the "k" file:

symmetry
    {
        type         symmetryPlane;
       }

I'm getting the following error:

--> FOAM FATAL ERROR:
Invalid wall function specification
Patch type for patch surface must be wall
Current patch type is patch



From function kqRWallFunctionFvPatchField::checkType()
in file derivedFvPatchFields/wallFunctions/kqRWallFunctions/kqRWallFunction/kqRWallFunctionFvPatchField.C at line 45.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::incompressible::kqRWallFunctionFvPatchField< double>::checkType() at ??:?
#3 Foam::fvPatchField<double>::adddictionaryConstruct orToTable<Foam::incompressible::kqRWallFunctionFvP atchField<double> >::New(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#4 Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#5 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::readField( Foam:imensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#6 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields(Foam::dictionary const&) at ??:?
#7 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields() at ??:?
#8 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) at ??:?
#9 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::incompressible::autoCreateWallFunctionField< double, Foam::incompressible::kqRWallFunctionFvPatchField< double> >(Foam::word const&, Foam::fvMesh const&) at ??:?
#10 Foam::incompressible::autoCreateK(Foam::word const&, Foam::fvMesh const&) at ??:?
#11 Foam::incompressible::RASModels::kEpsilon::kEpsilo n(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) at ??:?
#12 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kEp silon>::New(Foam::GeometricField<Foam::Vector<doub le>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) at ??:?
#13 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) at ??:?
#14
at ??:?
#15 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#16
at ??:?
Aborted (core dumped)

For the following code:

symmetry
    {
        type            kqRWallFunction;
        value           uniform 1;
     }

I get the following error message:

--> FOAM FATAL IO ERROR:
inconsistent patch and patchField types for
patch type symmetryPlane and patchField type kqRWallFunction

file: /home/ajevs/OpenFOAM/ajevs-2.3.1/run/porousSimpleFoam/BritoChannelExplicit/0/k.boundaryField.symmetry from line 45 to line 46.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /home/openfoam/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 172.

FOAM exiting

Thank you for any help any of you might provide.

[akidess]

1. A wall function only makes sense on a wall. A symmetry plane is not a wall. Don't use a wall function.

2. Check your boundary file if the patch is set to symmetryPlane. Usage is documented, see 5.2.1.: http://cfd.direct/openfoam/user-guide/boundaries/

[adrieno]

I guess that if you define a patch as a symmetryPlan in your blockMesdDict file, then you'll have to define this patch as a symmetryPlan in all your BC otherwise it doesn't make sense.
Regards,
Adrien

[Outbound]

Well I've define all symmetry planes as such, even the physical patch type which I'm not sure I should be doing, and I've recently changed it back.
I forgot to mention that I used Gmsh to generate the mesh and then used gmshToFoam to create the Polymesh files. This seems to create this Physical Type field.

Also, I'm modifying the case for OpenFOAM 2.3.1

Meanwhile I found what the problem was in boundary file, given that the free surface patch was incorrectly configured, and the the "nut" file in the "0" folder also had problems. The inlet patches were incorrectly configured as wall patches.

Right now the problem is with the porosity settings.

Thanks everyone.