[Victor]

Hi at all,

as a Open-FOAM-beginner, i tried to use chtMultiregionFoam-solver as it is used in the HeatTransfer Tutorial Case. In my case,there is a part in the middle of the body that is cut out by the setSet utility in order to simulate a solid. After running blockMesh, setSet, setsToTones, splitMeshRegions without any errors the case allways stops,when running the chtMultiRegionFoam solver:

/OpenFOAM-1.6/bin/tools/RunFunctions: line 38: 615 Aborted $APP_RUN $* > log.$APP_NAME 2>&1

the log-file:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-f802ff2d6c5a
Exec : chtMultiRegionFoam
Date : Nov 19 2009
Time : 10:34:59
Host : pag
PID : 615
Case : /nfs/home/fleischer/OpenFOAM/fleischer-1.6/run/Tube1/Test2_4
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create fluid mesh for region Fluid for time = 0.0001

Create solid mesh for region Stack for time = 0.0001

*** Reading fluid mesh thermophysical properties for region Fluid

Adding to thermoFluid

Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Adding to rhoFluid

Adding to KFluid

Adding to UFluid

Adding to phiFluid

Adding to gFluid

Adding to turbulence

Selecting turbulence model type laminar
Adding to DpDtFluid

*** Reading solid mesh thermophysical properties for region Stack

Adding to rhos

Adding to cps

Adding to Ks

Adding to Ts

Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006
Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006



request for objectRegistry region0 from objectRegistry Test2_4 failed
available objects of type objectRegistry are

2
(
Stack
Fluid
)
#0 Foam::error:rintStack(Foam::Ostream&) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#3 Foam:bjectRegistry const& Foam:bjectRegistry::lookupObject<Foam:bjectReg istry>(Foam::word const&) const in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::OutputFilterFunctionObject<Foam:robes>::st art() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libsampling.so"
#5 Foam::functionObjectList::read() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::Time:perator++() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 main in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116


From function objectRegistry::lookupObject<Type>(const word&) const
in file db/objectRegistry/objectRegistryTemplates.C at line 140.

FOAM aborting


Does anybody know where this problem comes from?
You'll find the packed Case in the attachment

[kawuppdich]

Hi Victor
I havent looked in your case but I would say there is something wrong with your coupled regions.
Did you customize them? (for example in 0.001/T)

[kawuppdich]

no thats not

[Victor]

Hi kawuppdich,

i have already looked at the boundary conditions for several times and cannot find any problem. And all log-files don't show any errors. So I don't know why there is a message "request for objectRegistry region0" in the chtMultiRegionFoam!?
I searched for similar problems, but there are only problems like "request for uniformDimensionedVectorField g from objectRegistry region0 failed"!?

[kawuppdich]

the problem is there is no region0. normaly it should be fluid or Stack. I don´t know where it comes from. I had the same error and my problem was that i´ve forgot to customize the boundary

[kawuppdich]

all looks fine but same error here

[Victor]

hmm, i don't find it either....
But thanks a lot for your helpkawuppdich!!

[Victor]

I have an idea where the problem could come from. After setting up a similar case with setSet, setsToZones,splitMeshRegions for the chtMultiregionFoam everything worked fine.
But when i tried to use the probes() function the problem we discussed above ocurred again.
Does anybody know if this could be the reason?
Or does anybody know an alternative for the probes() function without saving the whole data accumulated during the simulation?

here the additional part of the controlDict-File:


functions
{
probesTest
{
// Type of functionObject
type probes;

// Where to load it from (if not already in solver)
functionObjectLibs ("libsampling.so");
outputControl timeStep;
outputInterval 1;

// Locations to be probed. runTime modifiable!
probeLocations
(
( -0.05 0 0)
( -0.04 0 0)
( -0.03 0 0)
( -0.02 0 0)
( -0.01 0 0)
( 0.00 0 0)
( 0.01 0 0)
( 0.02 0 0)
( 0.03 0 0)
( 0.04 0 0)
( 0.05 0 0)
);

// Fields to be probed. runTime modifiable!
fields
(
rho
p
U
T
);
}
};

[maddalena]

Just for information: Victor missed one keyword:

functions
{ 
  probesTest
    {
    // Type of functionObject
        type probes;

        // Where to load it from (if not already in solver)
        functionObjectLibs ("libsampling.so");
        outputControl   timeStep;                                              
        outputInterval  1;                                                     

        region heater;

        // Locations to be probed. runTime modifiable!
        probeLocations
        (
       ( -0.05 0 0)
       ( -0.04 0 0)    
       ( -0.03 0 0)    
       ( -0.02 0 0)    
       ( -0.01 0 0)    
       ( 0.00 0 0)    
       ( 0.01 0 0)    
       ( 0.02 0 0)    
       ( 0.03 0 0)
       ( 0.04 0 0)
       ( 0.05 0 0)    
    );

        // Fields to be probed. runTime modifiable!
        fields
        (
        rho
        p
        U
        T
    );
     }
};

This entry is not compulsory, as soon as there is only one region in the case. chtMultiRegionFoam, as the name says, is able to manage different regions, thus probes function needs the region name!
Hope this help someone,

mad

[r08n]

Originally Posted by Victor

request for objectRegistry region0 from objectRegistry Test2_4 failed
available objects of type objectRegistry are
2
(
Stack
Fluid
)

Before running the simulation (after `splitMeshRegions`), edit the files 0.001/Stack/polyMesh/boundary: there must be an entry like:

Stack_to_Fluid
{
...
sampleRegion region0;
samplePatch ...
...
}

Change these entries to be

Stack_to_Fluid
{
...
sampleRegion Fluid;
samplePatch Fluid_to_Stack;
...
}

Analogously, in 0.001/Fluid/polyMesh/boundary, there must be this entry:

Fluid_to_Stack
{
...
sampleRegion Stack;
samplePatch Stack_to_Fluid;
...
}

i.e., 'polyMesh/boundary' files of each region contain entries for neighbouring regions
and neighbouring patches.

[Linse]

Originally Posted by maddalena

Just for information: Victor missed one keyword:

functions
{ 
  probesTest
    {
    // Type of functionObject
        type probes;

        // Where to load it from (if not already in solver)
        functionObjectLibs ("libsampling.so");
        outputControl   timeStep;                                              
        outputInterval  1;                                                     

        region heater;

        // Locations to be probed. runTime modifiable!
        probeLocations
        (
       ( -0.05 0 0)
       ( -0.04 0 0)    
       ( -0.03 0 0)    
       ( -0.02 0 0)    
       ( -0.01 0 0)    
       ( 0.00 0 0)    
       ( 0.01 0 0)    
       ( 0.02 0 0)    
       ( 0.03 0 0)
       ( 0.04 0 0)
       ( 0.05 0 0)    
    );

        // Fields to be probed. runTime modifiable!
        fields
        (
        rho
        p
        U
        T
    );
     }
};

This entry is not compulsory, as soon as there is only one region in the case. chtMultiRegionFoam, as the name says, is able to manage different regions, thus probes function needs the region name!
Hope this help someone,

mad

Thanks, Maddalena!

I had the very same problem and it seems to be solved by now!
(Testing the tool, but looking good!)

Cheers,
Bernhard

[dasith0001]

Hi,

I am running into the same problem but trying to calculate 'wallHeatFlux' from the 'topSolid' region in the patch called ' maxZ'.

OpenFOAM version is 10.

my 'wallHeatFlux' function looks like

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  10
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "system";
    object      sample;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

type            surfaces; //sets; //surfaces
functionObjectLibs           ("libsampling.so");

region           topSolid; 

//libs            ("fieldFunctionObjects");
//region           topSolid;

writeControl         writeTime;
interpolationScheme  cellPointFace;
setFormat            raw; //vtk

fields          ( wallHeatFlux ); //U p

surfaces
(
    surfaces1
    {
        type         plane;
        patchName    maxZ;
    }

);

and I am getting the error of

PHP Code:

[0] --> FOAM FATAL ERROR:
[0]
    request for objectRegistry region0 from objectRegistry V07processor0 failed
    available objects of type objectRegistry are

10
(
midAir
seal
bottomSolid
thermalB
topSolid
heater
wallSolid
heaterZ2
stand
wallSolid2
) 


Would you guys be able to direct me in the right way, relatively new, specially to OF10. help is hugely appreciated.

Thanks,
Dasith

[dasith0001]

found the answer at

https://www.cfd-online.com/Forums/openfoam-solving/248597-wallheatflux-openfoam-version-10-a.html