CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Problem with running chtMultiRegionFoam after using setSet utility (http://www.cfd-online.com/Forums/openfoam/70282-problem-running-chtmultiregionfoam-after-using-setset-utility.html)

Victor November 19, 2009 06:24

Problem with running chtMultiRegionFoam after using setSet utility
 
1 Attachment(s)
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::printStack(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::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#3 Foam::objectRegistry const& Foam::objectRegistry::lookupObject<Foam::objectReg istry>(Foam::word const&) const in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::OutputFilterFunctionObject<Foam::probes>::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::operator++() 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?:confused:
You'll find the packed Case in the attachment

kawuppdich November 19, 2009 07:40

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 November 19, 2009 08:10

no thats not

Victor November 19, 2009 08:22

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 November 19, 2009 08:26

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

kawuppdich November 19, 2009 08:46

all looks fine but same error here

Victor November 19, 2009 09:32

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

Victor November 23, 2009 08:26

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.:confused:
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 June 30, 2010 08:36

Just for information: Victor missed one keyword:
Code:

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, :D

mad

r08n July 1, 2010 07:30

Quote:

Originally Posted by Victor (Post 236880)
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 September 10, 2012 09:30

Quote:

Originally Posted by maddalena (Post 265132)
Just for information: Victor missed one keyword:
Code:

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, :D

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


All times are GMT -4. The time now is 06:36.