CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

request for volScalarField k from objectRegistry region0 failed+(DPMFoam)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 21, 2017, 01:24
Default request for volScalarField k from objectRegistry region0 failed+(DPMFoam)
  #1
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
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.
abdollahi is offline   Reply With Quote

Old   April 21, 2017, 05:04
Default request for volScalarFiel
  #2
New Member
 
Max
Join Date: Sep 2016
Location: Delft
Posts: 20
Rep Power: 3
WildeCat is on a distinguished road
Hi abdollahi,

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

Quote:
--> FOAM FATAL ERROR:


request for volScalarField k from objectRegistry region0 failed
The next thing openfoam tells you is which fields are available

Quote:
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
WildeCat is offline   Reply With Quote

Old   April 21, 2017, 05:37
Default
  #3
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
thanks
But I have in 0 dictionary U.H2O , k.H2O,Ö. . Fluid in my case is water.
abdollahi is offline   Reply With Quote

Old   April 21, 2017, 05:40
Default More information
  #4
New Member
 
Max
Join Date: Sep 2016
Location: Delft
Posts: 20
Rep Power: 3
WildeCat is on a distinguished road
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?
WildeCat is offline   Reply With Quote

Old   April 21, 2017, 06:34
Default
  #5
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
I sent 0,constant and system dictionary as private message.

thank you very much
abdollahi is offline   Reply With Quote

Old   April 21, 2017, 09:23
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,707
Rep Power: 29
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to 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

Code:
k k.H2O;
so it becomes something like:

Code:
my-lovely-inlet
{
    type turbulentMixingLengthDissipationRateInlet;
    mixingLength 100;
    k k.H2O;
    value uniform 10;
}
alexeym is offline   Reply With Quote

Old   April 21, 2017, 11:43
Default
  #7
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
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 donít understand what do you say? I donít know where I put ď k .H2OĒ in simpleFoam or lagrangian? what dictionary?
thanks
abdollahi is offline   Reply With Quote

Old   April 21, 2017, 13:20
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,707
Rep Power: 29
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to 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.
alexeym is offline   Reply With Quote

Old   April 22, 2017, 00:01
Default
  #9
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
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 is offline   Reply With Quote

Old   April 22, 2017, 00:07
Default
  #10
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
"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
.
.
.
.
abdollahi is offline   Reply With Quote

Old   April 22, 2017, 01:59
Default
  #11
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,707
Rep Power: 29
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
1. In dictionaries, you have posted, find the following sequence of letters:

Code:
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.
alexeym is offline   Reply With Quote

Old   April 23, 2017, 10:07
Default
  #12
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
thanks, I change it, but I have same error.
abdollahi is offline   Reply With Quote

Old   April 23, 2017, 12:59
Default
  #13
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,707
Rep Power: 29
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to 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.
alexeym is offline   Reply With Quote

Old   April 23, 2017, 15:07
Default Answer
  #14
New Member
 
Max
Join Date: Sep 2016
Location: Delft
Posts: 20
Rep Power: 3
WildeCat is on a distinguished road
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 is offline   Reply With Quote

Old   April 24, 2017, 03:55
Default Solution
  #15
New Member
 
Max
Join Date: Sep 2016
Location: Delft
Posts: 20
Rep Power: 3
WildeCat is on a distinguished road
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
WildeCat is offline   Reply With Quote

Old   April 24, 2017, 08:30
Default
  #16
New Member
 
abdollahi
Join Date: Nov 2012
Posts: 14
Rep Power: 6
abdollahi is on a distinguished road
hi
my case is run without error,I really appreciate your help.
abdollahi is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
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


All times are GMT -4. The time now is 18:46.