[amuzeshi]

Thank You.
Anyway, I prefered to use y+ function in controlDict so that results are written in postProcessing folder without excess effort.
Friends who have the same problem can copy the following statements into their controlDict at the end.

functions
{
        yPlus
    {
        type            yPlus;
        libs            ("libfieldFunctionObjects.so");
        writeControl    writeTime;
    }

}

[sinvastil]

Hello everyone,


I'm getting a similar error, can somebody help me?


used code: pimpleFoam -postProcess -func yPlus

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: No convergence criteria found


PIMPLE: Operating solver in PISO mode

Time = 0
Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
...
}

No MRF models present

No finite volume options present
yPlus yPlus write:
    writing object yPlus
    patch wall y+ : min = 2.77492, max = 2.79733, average = 2.79134


Time = 0.0377083
Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
...
}

No MRF models present

No finite volume options present


--> 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>]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::functionObjects::yPlus::execute() at ??:?
#4  Foam::functionObjects::timeControl::execute() at ??:?
#5  Foam::functionObjectList::execute() at ??:?
#6  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/pimpleFoam"
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/pimpleFoam"
 Aborted (core dumped)

But if I use in the controlDict the following function:

functions
{
  yPluswall
  {
    type            yPlus;
    libs            ("libfieldFunctionObjects.so");

    executeControl  writeTime;
    writeControl    writeTime;

  }
}

The error doesn't occur during the simulation and I can achieve the yPlus values... I don't understand why?

[wyldckat]

Quick answer: This is a bug and has already been corrected:

• In commit: https://github.com/OpenFOAM/OpenFOAM-6/commit/0f14683c
• Bug report: https://bugs.openfoam.org/view.php?id=3019

To update your installation, it now depends on the installation instructions you've followed.

[sinvastil]

I've followed the Foundation instructions.


Now I've tried the following commands but the problem is not solved:


sudo apt-get update

sudo apt-get install --only-upgrade openfoam6




What I'm doing wrong?

Thanks

[wyldckat]

Greetings Rui,

My apologies, but I didn't test this sooner myself. This issue was reported at https://bugs.openfoam.org/view.php?id=3055 - but I wasn't given a clear indication that the latest Deb package from 20180805 does not solve this issue, but I've confirmed so earlier today.

There are a few possible solutions at the moment:

1. A slow workaround is to run the command one for each time step:
   

   foamListTimes | while read line; do pimpleFoam -postProcess -func yPlus -time $line; done

   Or only run for the latest time:
   

   pimpleFoam -postProcess -func yPlus -latestTime

2. Either you could uninstall that package "openfoam6" and then install from source code, as explained in either of the following pages:
   1. Official instructions: https://openfoam.org/download/source/
   2. Step-by-step instructions written by the community (well, by me at this point in time): https://openfoamwiki.net/index.php/I...nFOAM-6/Ubuntu - make sure you follow the instructions for the version of Ubuntu that you are using.
3. Or you could install the "openfoam5" package and use two terminals from which you use each version of OpenFOAM; then use OpenFOAM 5 only for handling this specific post-processing step.

Best regards,
Bruno

[enricoGuss]

Hi all,

I'm sorry but I was unable to get what to do to correct my case in which the error is very similar:

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 1000

Reading field, p...
Reading field, U...
Creating vorticity field, omega...
Creating second-invariant of strain-rate tensor field, Q...
Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type LESModel
Selecting LES turbulence model oneEqEddyABL
Selecting LES delta type smooth
Selecting LES delta type cubeRootVol
[281] 
[281] 
[281] --> FOAM FATAL ERROR: 
[281] 
    request for volScalarField T from objectRegistry region0 failed
    available objects of type volScalarField are

7
(
nuSgs
Q
nu
delta
p
l
geometricDelta
)
[281] 
[281] 
[281]     From function objectRegistry::lookupObject<Type>(const word&) const
[281]     in file /marconi_work/Pra16_4200/pablo/OpenFOAM//OpenFOAM-2.4.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.
[281] 
FOAM parallel run aborting

The error

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

is similar to the one discussed here but the other problem is that the directory

/marconi_work/Pra16_4200/pablo/OpenFOAM//OpenFOAM-2.4.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C

is wrong but I can't understand who is calling it and so how to modify it (I'm using programs implemented by others). I think it's something related with LESProperties.

Thank you

eg

[wyldckat]

Quick answer @enricoGuss: Please follow the instructions given at How to give enough info to get help - because from your description, if it were a "T" or an alien from outer space, it wouldn't make much difference for anyone reading your post
At the very least, some context of the case you've created would make it a tiny bit easier to understand how you might have configured your case... that and which solver you've used... and which reference tutorial case you based your case on...

Because "T" usually is the temperature field... so I'm guessing it is either being requested by one of the boundary conditions or by a function object... or perhaps you are using some model that is meant to be used with a solver that does have the "T" field...

[enricoGuss]

Originally Posted by wyldckat

Quick answer @enricoGuss: Please follow the instructions given at How to give enough info to get help - because from your description, if it were a "T" or an alien from outer space, it wouldn't make much difference for anyone reading your post
At the very least, some context of the case you've created would make it a tiny bit easier to understand how you might have configured your case... that and which solver you've used... and which reference tutorial case you based your case on...

Because "T" usually is the temperature field... so I'm guessing it is either being requested by one of the boundary conditions or by a function object... or perhaps you are using some model that is meant to be used with a solver that does have the "T" field...

Thank you @wyldckat, I'll try to explain the best I can: I'm using ABLSolver (based on pisoFOAM) to simulate a wind flow. At first I run this solver saving flow distributions at inlet/outlet areas with sliceDataInstantaneous, than I use this data as an input for the next run with a modified version of pisoFoamTurbine. I don't know if there is a reference tutorial for such a case because I'm using an example case build in SOWFA (that uses OpenFOAM).
Quantities that I'm using are
Rwall
T
U
cellDist
k
kappat
nuSgs
p_rgh
qwall

I don't know which file could be useful to show you because I don't understand from where does it comes from. So what I ask you is if you can have an idea of what calls objectRegistry region0.

[wyldckat]

Quick questions/answers:

1. Which example case from SOWFA are you using: https://github.com/NREL/SOWFA/tree/master/exampleCases ?
2. I read one too many custom solvers being mentioned... are you using a solver that is in SOWFA?
   1. And if you are, then are you using the correct solver on the correct case example?
   2. If not, where can I see the source code of that other solver that you are using?
3. "objectRegistry region0" refers to the main mesh domain, usually "region0" is the default name of the mesh, when the mesh was not modified to have multiple regions (e.g. chtMultiRegionFoam uses solid and fluid regions).

[neilk]

I am trying to run a turbulent flow simulation using reactingParcelFilmFoam. But even after defining the turbulent properties and transportProperties, I get the following error

--> FOAM FATAL ERROR: 

    request for dictionary transportProperties from objectRegistry region0 failed
    available objects of type dictionary are

13
(
MRFProperties
radiationProperties
turbulenceProperties
fvSchemes
fvOptions
fvSolution
thermophysicalProperties
data
reactingCloud1Properties
combustionProperties
additionalControls
reactingCloud1OutputProperties
wallFilmRegionOutputProperties
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::IOdictionary]
    in file /usr/local/apps/OpenFOAM/gcc482-v1706/OpenFOAM-v1706/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 239.

FOAM aborting

But I have the transportProperties file defined in my constant folder. The weird twist is that a laminar case of reactingParcelFilmFoam does not require transportProperties file and runs just fine without it.

Does anyone know how to solve this issue?

Thank you

[alexeym]

Hi,

Since there is almost no context, I try to guess: you have used incompressible turbulent heat diffusivity wall function for compressible simulation. I.e. instead of simple alphatJayatillekeWallFunction it should be compressible::alphatJayatillekeWallFunction.

As far as grep shows, alphatJayatillekeWallFunction is the only class, which looks up transportProperties in object registry.

[neilk]

Alexey,

Sorry about the lack of information but your guess was correct. And the simulation is running now.

Thank you!

[neilk]

Alexey,

Is there a way to convert reactingParcelFilmFoam to a steady state solver (something along the lines of simpleReactingParcelFoam)? I tried but I can just get the reactingCloud and the flow field correct.The fields in the wallFilmRegion diverge for the slightest change in the surfaceFilmProperties (although these changes work for the transient solver). Is there a way to go about it?

Thanks

[greel]

Hi guys,

I'm using the MPPICFoam solver in my case. I'm trying to incorporate ke model in order to resolve it. My simulation runs perfectly using laminar model as the tutorial of MPPIC called injection.

But, the same error appear to me related with k.

--> FOAM FATAL ERROR:

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

10
(
alpha.air_0
(1|A(U.air))
nu
mu.air
epsilon.air
p
alpha.air
nut.air
rho.air
k.air
)

I attach my whole folders in order to you could help me.
http://https://drive.google.com/open...goaUpXbQ3wWgUC

Things that I did:
- I incorporated the line in k.air file (k k.air)
- I add the lines folllow all recomedation How to use MPPICFoam with turbulence effects on particle motion?

I hope that you can find the solution as soon as possible.
Thank you in advance

[alexeym]

Hi,

For epsilon inlet you utilise turbulentMixingLengthDissipationRateInlet, which uses k field for calculation (it would be nice to see extended error message to confirm, that error happens in this boundary condition). To configure this BC to use another k field, add "k k.air" in 0/epsilon.air.

[greel]

Thank you alexeym!!
I ran my case with your advice, afterward more errors were showed related with the definition of variables in fvSchemes and fvSolution. And then I put also "U U.air" in k.air and epsilon.air files.
However, I fixed all of them, so I have the turbulent ke case running as well laminar.
Thanks a lot!

[farshadexp]

Hi guys;
I have the same problem, I've read the thread, thanks for instructions.
Using rhoReactingBuoyantFoam to model fire, I've encountered following error:

  --> FOAM FATAL ERROR: 

    request for volScalarField ph_rgh.CH3OH from objectRegistry region0 failed
    available objects of type volScalarField are

65
(
thermo:mu
OH
C2H3
thermo:psi
CH3
C2H5
h
C3H8
C2H6
CO2
HCO
Qdot
H2
(1|A(U))
dpdt
O2_0
C3H7
alphat
CH4_0
p
CH2O
T
CH2
H2O
TabulationResults
AR
N2
nut
K
C2H
CH2CO
K_0
C2H4
rho
CH2OH
C2H2
k
H2O2
HCCOH
h_0
O2
CH2(S)
p_rgh
CH2CHO
HCCO
(thermo:psi*p)
gh
delta
rDeltaT
C
CH4
HO2
CH3CHO
CH3OH
HO2_0
rho_0
CO
O
CH3O
CO_0
H
thermo:rho
EDC<rhoReactionThermo>:kappa
thermo:alpha
CH
)


     From function const Type& Foam::objectRegistry::lookupObject(const  Foam::word&) const [with Type = Foam::GeometricField<double,  Foam::fvPatchField, Foam::volMesh>]
    in file /home/farshad/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2   Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>  const&  Foam::objectRegistry::lookupObject<Foam::GeometricField<double,  Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const  at ??:?
#3  Foam::prghTotalHydrostaticPressureFvPatchScalarField::updateCoeffs() at ??:?
#4   Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double,  Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet  const&) at ??:?
#5  Foam::tmp<Foam::fvMatrix<double>  >  Foam::fv::optionList::operator()<double>(Foam::GeometricField<double,  Foam::fvPatchField, Foam::volMesh> const&,  Foam::GeometricField<double, Foam::fvPatchField,  Foam::volMesh>&, Foam::word const&) at ??:?
#6  ? at ??:?
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  ? at ??:?
Aborted (core dumped)

based on this thread I added some lines to 0/p_rgh but the modeling is still being crashed by the error:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    "(outlet|sides)"
    {
        type            prghTotalHydrostaticPressure;
        p0              $internalField;
    ph_rgh        ph_rgh.CH3OH;
        value           $internalField;
    }

    frontAndBack
    {
        type            prghTotalHydrostaticPressure;
        p0              $internalField;
    ph_rgh        ph_rgh.CH3OH;
        value           $internalField;
    }

    base
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    inlet
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    /*frontAndBack
    {
        type            empty;
    }*/
}

can anyone help me?

[farshadexp]

Thanks to #15 I changed the BC and got rid of the problem.
But still need good explanation. if any.

Immensely appreciated.

[malini1408]

Hi,
I had the similar error except it shows the following:



--> FOAM FATAL ERROR:

request for volScalarField none from objectRegistry region0 failed
available objects of type volScalarField are

28
(
H2O_0
thermo:mu
HMDSO_0
thermosi
nut
N2
K
K_0
CO2_0
h
rho
CO2
k
h_0
Qdot
(1|A(U))
dpdt
Ox_0
Ox
thermosi_0
alphat
HMDSO
rho_0
p
T
H2O
epsilon
thermo:alpha
)

Can someone please tell me what I need to do here?

[wyldckat]

Originally Posted by malini1408

Can someone please tell me what I need to do here?

Quick answer: You need to follow the instructions give here: How to give enough info to get help - so that we get more information about how you got to that error. Otherwise it's just a guessing game...