[abdollahi]

Hi Everyone,

I have a problem with my case solving by lagrangian(DPMFoam), which, I am presenting you in the following feedback information:




--> FOAM FATAL ERROR:


request for volScalarField k from objectRegistry region0 failed
available objects of type volScalarField are


12
(
nut.H2O
k.H2O
(1|A(U.H2O))
kEpsilon:G
alpha.H2O_0
nu
div(phi.H2O)
p
rho.H2O
mu.H2O
alpha.H2O
epsilon.H2O
)




From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/a/OpenFOAM/OpenFOAM-2.4.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.


FOAM aborting


#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3 Foam::turbulentMixingLengthDissipationRateInletFvP atchScalarField::updateCoeffs() at ??:?
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoef fs() at ??:?
#5 Foam::RASModels::kEpsilon<Foam::PhaseIncompressibl eTurbulenceModel<Foam::singlePhaseTransportModel> >::correct() at ??:?
#6 ? at ??:?
#7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8 ? at ??:?
Aborted (core dumped)




Did anyone have the same problem before ? I mean, how to deal with error type : "request for volScalarField k from objectRegistry region0 failed" ?

I will be appreciate for any advice.

[WildeCat]

Hi abdollahi,

the error message you get tells you the solution. You are using "DPMFFoam" as a solver and a field called "k".

--> FOAM FATAL ERROR:


request for volScalarField k from objectRegistry region0 failed

The next thing openfoam tells you is which fields are available

available objects of type volScalarField are


12
(
nut.H2O
k.H2O
(1|A(U.H2O))
kEpsilon:G
alpha.H2O_0
nu
div(phi.H2O)
p
rho.H2O
mu.H2O
alpha.H2O
epsilon.H2O
)

I imagine you have a field "k" in the "0" directory. This field should based on your error message be specified per species, so in your case "k.H2O".

You can check out the openfoam tutorial (I put the link for openfoam301) here
https://github.com/OpenFOAM/OpenFOAM.../Goldschmidt/0

where the velocity "U" is specified as "U.air".

Hope I was of help

[abdollahi]

thanks
But I have in 0 dictionary U.H2O , k.H2O,…. . Fluid in my case is water.

[WildeCat]

Hi abdollahi

For me to help you more I need more information.

Would it be possible for you to upload a simplified version of your test case with the 0, constant and system directory?

[abdollahi]

I sent 0,constant and system dictionary as private message.

thank you very much

[alexeym]

Hi all,

@abdollahi

Error is caused by turbulentMixingLengthDissipationRateInletFvPatchSc alarField. It uses TKE to calculate dissipation rate and by default in OpenFOAM TKE field is called k.

In you case it is called k.H2O, so in turbulentMixingLengthDissipationRateInlet description you have to add

k k.H2O;

so it becomes something like:

my-lovely-inlet
{
    type turbulentMixingLengthDissipationRateInlet;
    mixingLength 100;
    k k.H2O;
    value uniform 10;
}

[abdollahi]

Hi alexeym
I solve this case by simpleFoam as steady state, after it is converged, I replace the latest time in 0 dictionary in lagrangian (DPMFoam). I don’t understand what do you say? I don’t know where I put “ k .H2O” in simpleFoam or lagrangian? what dictionary?
thanks

[alexeym]

Since the error happens during DPMFoam run, you have to add the line to 0 folder in DPMFoam case. And since turbulentMixingLengthDissipationRateInlet is BC for epsilon, you have to add the line to epsilon.H2O file. But since it you, who run simulations, you should know better.

[abdollahi]

hi,
"k" in 0 dictionary in simpleFoam:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 1;

boundaryField
{
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.045;

value $internalField;
}
outlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.06;
U U;

value $internalField;
}
walls
{
type kqRWallFunction;
value uniform 0;
}
bottom
{
type kqRWallFunction;
value uniform 0;
}
back
{
type wedge;
}
front
{
type wedge;
}
stl
{
type kqRWallFunction;
value uniform 0;
}
}


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





"k.H2O" in 0 dictionary in DPMFoam:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "1228";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField nonuniform List<scalar>
25179
(
3.15091e-06
2.56557e-06
2.0005e-06
1.37121e-06
7.18191e-07
4.0741e-07
.
.
.
.

[abdollahi]

"epsilon" in 0 dictionary in simpleFoam:



/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -3 0 0 0 0];

internalField uniform 200;

boundaryField
{
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.15;

value $internalField;
}
outlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.0025;

value $internalField;
}
walls
{

type epsilonWallFunction;
value $internalField;
}
bottom
{

type epsilonWallFunction;
value $internalField;
}
back
{
type wedge;
}
front
{
type wedge;
}
stl
{

type epsilonWallFunction;
value $internalField;
}
}


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


"epsilon.H2O" in 0 dictionary in DPMFoam:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "1228";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -3 0 0 0 0];

internalField nonuniform List<scalar>
25179
(
7.08276e-08
5.18813e-08
3.57445e-08
2.02775e-08
7.64593e-09
.
.
.
.

[alexeym]

1. In dictionaries, you have posted, find the following sequence of letters:

turbulentMixingLengthDissipationRateInlet

2. Compare what you have around and what I have posted in post #6 (request for volScalarField k from objectRegistry region0 failed+(DPMFoam)).

3. Make corresponding corrections in the case, which halts with error.

[abdollahi]

thanks, I change it, but I have same error.

[alexeym]

What changes did you made? Error is EXACTLY the same? It looks like WE have problems running the case, not you.

Any way, the only person in the thread, who saw you case files is WildeCat, let's wait for his answer.

[WildeCat]

Hi all, I saw parts of the file and I agree, that the error is most likely from what you mention Alex. I send this as a pm to abdollahi. But I got the case as messages and couldnt run it myself. Could you upload the case on a fileshare? It would make things a hell of a lot easier for us to help you. Cheers

[WildeCat]

I have received the full case and indeed Alex, what you suggested is the right solution. After correcting this error, also 2 others show up which have to be corrected in the same way.

For everybody having a similar problem I refer them to post #6 and

https://www.cfd-online.com/Forums/op...onditions.html

which presents how to restart a simulation with a different boundary condition

Best regards

[abdollahi]

hi
my case is run without error,I really appreciate your help.

[amuzeshi]

Hello Alex
my error is relatively the same; but mine is about yPlus. I'm using simpleFoam -postProcess -func yPlus. yPlus is generated only in 0 time but not in the next steps (case dir/postProcessing/yPlus). What's the problem? The error is as the following:

--> FOAM FATAL ERROR: 

    request for volScalarField yPlus from objectRegistry region0 failed
    available objects of type volScalarField are

5
(
nut
k
nu
p
epsilon
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]

.
.
.
#3  Foam::functionObjects::yPlus::execute() at ??:?
.
.
.

[alexeym]

Hi,

Creating single postProcessing/yPlus/0/yPlus.dat file is normal yPlus function object behaviour. In this file data for all time steps are stored.

Describe your case in more details. yPlus function object runs on pitzDaily tutorial case quite OK: creates yPlus field for every available saves and collects statistics in postProcessing folder.

[amuzeshi]

This is a backward Facing Step case using k-w. Pls check if you could get yPlus using the method mentioned.

[alexeym]

Everything was identical to pitzDaily tutorial. You case converged in 1198 iterations. simpleFoam -postProcess -func yPlus calculated y+ values without any problems.