|
[Sponsors] |
request for volScalarField k from objectRegistry region0 failed+(DPMFoam) |
![]() |
|
LinkBack | Thread Tools | Display Modes |
![]() |
![]() |
#1 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
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: ![]() #1 Foam::error::abort() at ??:? #2 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam: ![]() #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. |
|
![]() |
![]() |
![]() |
![]() |
#2 | ||
New Member
Max
Join Date: Sep 2016
Location: Delft
Posts: 21
Rep Power: 3 ![]() |
Hi abdollahi,
the error message you get tells you the solution. You are using "DPMFFoam" as a solver and a field called "k". Quote:
Quote:
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 |
|||
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
thanks
But I have in 0 dictionary U.H2O , k.H2O,…. . Fluid in my case is water. |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Max
Join Date: Sep 2016
Location: Delft
Posts: 21
Rep Power: 3 ![]() |
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? |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
I sent 0,constant and system dictionary as private message.
thank you very much |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
|
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 Code:
k k.H2O; Code:
my-lovely-inlet { type turbulentMixingLengthDissipationRateInlet; mixingLength 100; k k.H2O; value uniform 10; } |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
|
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.
|
|
![]() |
![]() |
![]() |
![]() |
#9 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
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 . . . . |
|
![]() |
![]() |
![]() |
![]() |
#10 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
"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 . . . . |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
|
1. In dictionaries, you have posted, find the following sequence of letters:
Code:
turbulentMixingLengthDissipationRateInlet 3. Make corresponding corrections in the case, which halts with error. |
|
![]() |
![]() |
![]() |
![]() |
#12 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
thanks, I change it, but I have same error.
|
|
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
|
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. |
|
![]() |
![]() |
![]() |
![]() |
#14 |
New Member
Max
Join Date: Sep 2016
Location: Delft
Posts: 21
Rep Power: 3 ![]() |
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
|
|
![]() |
![]() |
![]() |
![]() |
#15 |
New Member
Max
Join Date: Sep 2016
Location: Delft
Posts: 21
Rep Power: 3 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#16 |
New Member
abdollahi
Join Date: Nov 2012
Posts: 16
Rep Power: 7 ![]() |
hi
my case is run without error,I really appreciate your help. |
|
![]() |
![]() |
![]() |
Thread Tools | |
Display Modes | |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel | U.Golling | OpenFOAM | 34 | May 24, 2016 12:30 |
Initial conditions for uniform flow | andreas | OpenFOAM | 5 | November 16, 2012 16:00 |
ParaView/Parafoam error when making animation | Disco_Caine | OpenFOAM Paraview & paraFoam | 6 | September 28, 2010 09:54 |
user subroutine error | CFDUSER | CFX | 2 | December 9, 2006 07:31 |
user defined function | cfduser | CFX | 0 | April 29, 2006 10:58 |