[jvinuales]

Hi everyone,

I am trying to set up a case using simpleFoam and k-omega SST. I have low y+ (<1). So I followed the recommendations on this post:

Why Menter's SST model low-Re issue has not been seriously investigated?

0/k

    walls
    {
	type fixedValue;
	value uniform 0.000000000001;
    }

0/nut

    walls
    {
	type calculated;
	value uniform 0;
    }

0/omega

    walls
    {
        type            omegaWallFunction;
        value           $internalField;
    }

When I run the case, I got the following error:

--> FOAM FATAL ERROR:
Attempt to cast type calculated to type nutWallFunction at index 0

I ran the case with wall functions and it runs without error (but no convergence).

Please, any idea why I am getting this error?

log

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.063120202, No Iterations 5
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.097361982, No Iterations 4
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.064783265, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.99353884, Final residual = 0.0071047527, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.17426867, Final residual = 0.0010439839, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.02697205, Final residual = 0.0002594569, No Iterations 4
time step continuity errors : sum local = 0.017789744, global = 0.0025942697, cumulative = 0.0025942697


--> FOAM FATAL ERROR:
Attempt to cast type calculated to type nutWallFunction at index 0

    From function To& Foam::refCast(From&, Foam::label) [with To = const Foam::nutWallFunctionFvPatchScalarField; From = const Foam::fvPatchField<double>; Foam::label = int]
    in file /home/pawan/OpenFOAM/OpenFOAM-v1912/src/OpenFOAM/lnInclude/typeInfo.H at line 162.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::nutWallFunctionFvPatchScalarField::nutw(Foam::turbulenceModel const&, int) at ??:?
#3  Foam::omegaWallFunctionFvPatchScalarField::calculate(Foam::turbulenceModel const&, Foam::List<double> const&, Foam::fvPatch const&, Foam::Field<double>&, Foam::Field<double>&) at ??:?
#4  Foam::omegaWallFunctionFvPatchScalarField::calculateTurbulenceFields(Foam::turbulenceModel const&, Foam::Field<double>&, Foam::Field<double>&) at ??:?
#5  Foam::omegaWallFunctionFvPatchScalarField::updateCoeffs() at ??:?
#6  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
#7  Foam::kOmegaSSTBase<Foam::eddyViscosity<Foam::RASModel<Foam::IncompressibleTurbulenceModel<Foam::transportModel> > > >::correct() at ??:?
#8  ? at ??:?
#9  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#10  ? at ??:?
Aborted (core dumped)

[jvinuales]

Originally Posted by jvinuales

I am trying to set up a case using simpleFoam and k-omega SST. I have low y+ (<1).

I forgot to mention. I am using OpenFoam v1912

[HPE]

Can you share your nut file, please?

As far as I understand, this problem comes from a recent .org integration which changed the hierarchy of wallFuncs. There must a nutWallFunction be defined now among nut boundary conditions if you use some wall function somewhere else, like omegaWallFunction.

I think this bug will be fixed in the next release.

[jvinuales]

Thanks for your answer.

0/nut

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    x1
    {type		cyclicAMI;}

    x2
    {type		cyclicAMI;}
	
    y1
    {type		cyclicAMI;}
	
	y2
    {type		cyclicAMI;}
	
	z1
    {type		cyclicAMI;}
	
    z2
    {type		cyclicAMI;}	

    walls
    {
	type calculated;
	value uniform 0;
    }
}

It may look strange but the flow is maintained through a fixedJumpAMI in p.

[jvinuales]

Originally Posted by HPE

There must a nutWallFunction be defined now among nut boundary conditions if you use some wall function somewhere else, like omegaWallFunction.

I think this bug will be fixed in the next release.

Is there an alternative set up that I can use for my case (k-omega SST with resolved b.layer i.e. y+<1) that does not result in an error?

[jvinuales]

Hi everyone,

Is there no fix for this? I do not want to have to run my simulations with another turbulence model because a bug... cannot anyone recommend a fix or an alternative set up with meaningful physics for k-omega SST with resolved boundary layer?

[requou]

Hello jvinuales,


I don't know if you still need help on that but my way of fixing this bug it to use a fixed value for omega instead of a wall function. In fact, it is my understanding that using OmegaWallFunction on the wall only calculate the BC at the wall and therefore can be used even we are not using a wall function but it is not mandatory and directly giving the value also works.



See: https://curiosityfluids.com/2019/02/...ry-conditions/ to know what value to choose.

[HPE]

Hi,

- requou is right.
- you can use `omegaWallFunction` for low-Re type meshes. For the viscous sublayer mesh, it will correctly return the y+<5 value. Also it is preferable for numerical stability reasons.
- please do also consider `blended on` keyword in omegaWallFunction.

Hope this helps.

[AlxB]

Hello requou,
thanks for the link to the formula for omega at the wall.



but:

what is Δywall ?
is it the distance of the first node from the wall ?

what is nu ?
is the fluid kinematic viscosity or the turbulent kinematic viscosity ?

I am not sure of these and would be happy to get a clarification.

[Markus Kolano]

Maybe this helps someone: In my understanding, for the LowRe-setup, you need to use the nutLowReWallFunction (https://www.openfoam.com/documentati...lFunction.html) if you want to use the omegaWallFunction (and not fixedValue as also correctly suggested above). It is supposed to be a dummy BC which sets nut to zero but allows to calculate y+.



Also see the following post:



Wall function usage

[farzadmech]

Dear jvinuales
Did you find an answer for your question? I have the same problem, I can runs using Laminar model, but when I want to use kOmegaSST it gives me error.


Thanks,
Farzad

Originally Posted by jvinuales

Hi everyone,

I am trying to set up a case using simpleFoam and k-omega SST. I have low y+ (<1). So I followed the recommendations on this post:

Why Menter's SST model low-Re issue has not been seriously investigated?

0/k

    walls
    {
	type fixedValue;
	value uniform 0.000000000001;
    }

0/nut

    walls
    {
	type calculated;
	value uniform 0;
    }

0/omega

    walls
    {
        type            omegaWallFunction;
        value           $internalField;
    }

When I run the case, I got the following error:

--> FOAM FATAL ERROR:
Attempt to cast type calculated to type nutWallFunction at index 0

I ran the case with wall functions and it runs without error (but no convergence).

Please, any idea why I am getting this error?

log

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.063120202, No Iterations 5
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.097361982, No Iterations 4
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.064783265, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.99353884, Final residual = 0.0071047527, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.17426867, Final residual = 0.0010439839, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.02697205, Final residual = 0.0002594569, No Iterations 4
time step continuity errors : sum local = 0.017789744, global = 0.0025942697, cumulative = 0.0025942697


--> FOAM FATAL ERROR:
Attempt to cast type calculated to type nutWallFunction at index 0

    From function To& Foam::refCast(From&, Foam::label) [with To = const Foam::nutWallFunctionFvPatchScalarField; From = const Foam::fvPatchField<double>; Foam::label = int]
    in file /home/pawan/OpenFOAM/OpenFOAM-v1912/src/OpenFOAM/lnInclude/typeInfo.H at line 162.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::nutWallFunctionFvPatchScalarField::nutw(Foam::turbulenceModel const&, int) at ??:?
#3  Foam::omegaWallFunctionFvPatchScalarField::calculate(Foam::turbulenceModel const&, Foam::List<double> const&, Foam::fvPatch const&, Foam::Field<double>&, Foam::Field<double>&) at ??:?
#4  Foam::omegaWallFunctionFvPatchScalarField::calculateTurbulenceFields(Foam::turbulenceModel const&, Foam::Field<double>&, Foam::Field<double>&) at ??:?
#5  Foam::omegaWallFunctionFvPatchScalarField::updateCoeffs() at ??:?
#6  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
#7  Foam::kOmegaSSTBase<Foam::eddyViscosity<Foam::RASModel<Foam::IncompressibleTurbulenceModel<Foam::transportModel> > > >::correct() at ??:?
#8  ? at ??:?
#9  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#10  ? at ??:?
Aborted (core dumped)