CFD Online Discussion Forums - [mesh manipulation] objectRegistry error with Postprocessing Function Objects

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)

- - [mesh manipulation] objectRegistry error with Postprocessing Function Objects (https://www.cfd-online.com/Forums/openfoam-meshing/130703-objectregistry-error-postprocessing-function-objects.html)

objectRegistry error with Postprocessing Function Objects

Hello,

I am a new OpenFoam user and I am simulating a valve with icoFoam solver.
The cylindrical housing is modelled with blockMesh followed by a double call to MirrorMesh, then the plate geometry is imported through .stl file and SnappyHexMesh.
The meshing process and the simulation worked fine.

Since I need to calculate the forces on the plate, I used the PostProcessing function Objects "forces", adding the corresponding entries in controlDict. With the introduction of these mirrorMesh reports an error:

Code:

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.3.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 2.3.0-f5222ca19ce6

Exec   : mirrorMesh

Date   : Mar 03 2014

Time   : 11:10:47

Host   : "eugenio-desktop"

PID    : 7743

Case   : /home/eugenio/OpenFOAM/eugenio-2.3.0/run/tutorials/incompressible/icoFoam/checkValve_cylinderSnappy

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time







--> FOAM FATAL ERROR: 



    request for objectRegistry region0 from objectRegistry checkValve_cylinderSnappy failed

    available objects of type objectRegistry are

0()



    From function objectRegistry::lookupObject<Type>(const word&) const

    in file db/objectRegistry/objectRegistryTemplates.C at line 198.



FOAM aborting



#0  Foam::error::printStack(Foam::Ostream&) at ??:?

#1  Foam::error::abort() at ??:?

#2  Foam::objectRegistry const& Foam::objectRegistry::lookupObject<Foam::objectRegistry>(Foam::word const&) const at ??:?

#3  Foam::OutputFilterFunctionObject<Foam::forces>::allocateFilter() at ??:?

#4  Foam::OutputFilterFunctionObject<Foam::forces>::start() at ??:?

#5  Foam::functionObjectList::read() at ??:?

#6  Foam::functionObjectList::timeSet() at ??:?

#7  Foam::Time::operator++() at Time.C:?

#8  Foam::Time::operator++(int) at ??:?

#9  

 at ??:?

#10  __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"

#11  

 at ??:?

Aborted (core dumped)

It seems to complain about "regions", but I haven't done any partitioning in my mesh domain. When excluding the entry "functions {..}" from controlDict and reintroducing it after the meshing process, the problem arises with the icoFoam solver.

Does anyone experienced a similar problem?

Thank you!

solved!

Code:

mirrorMesh -noFunctionObjects

Has anyone managed to get this working properly? I see the same error when I try to use this function object to calculate field averages in cellZones in a parallel case with a single region:

Quote:

functions
{
bufferVolume
{
type cellSource;
functionObjectLibs ("libfieldFunctionObjects.so");
enabled true;
outputControl timeStep;
outputInterval 1;
log true; // log to screen?
valueOutput true; // Write values at run-time output times?
source cellZone; // cellZone or all
sourceName bufferVolume;
operation volAverage;
fields
(
p
);
}
}

I get the same error except for the case name. Does the solver need any special code to support function objects?

Quote:

request for objectRegistry region0 from objectRegistry checkValve_cylinderSnappy failed available objects of type objectRegistry are 0()

Edit: If I add this to controlDict when the solver is already running it works for me.

[volIntegrate] Unable to integrate over cellZone

Hello everyone,

I stumbled upon the exact same problem, just wanted to ask again, maybe someone will be able to help in 2021 :)

I am using interFoam to simulate wave breaking on coastal structures. To measure how much water has crossed a particular structure, I would like to calculate $\int \alpha dV$ "downstream" of the structure, using the volFieldValue and the volIntegrate operation.

Because I only want to measure the volume of water in a type of sink downstream of the structure, I followed the documentation and added a new cellZone using topoSetDict :

Code:

    {

         name    bacCellSet;

        type    cellSet;

        action  new;

        source  boxToCell;

        box     (21.6 -2 -2) (22.0 2 2); // Overall domain bounding box (-4 -0.01 0) (22 0.99 2)

    }



    {

        name    bac;   //This is the cellZone I will be using

        type    cellZoneSet;

        action  new;

        source  setToCellZone;

        set     bacCellSet;

    }

I then specified that cellZone into the volFieldValue function objet in system/controlDict:

Code:

     waterVolume

     {

        type            volFieldValue;

        libs            ("libfieldFunctionObjects.so");

        log             true;



        enabled         true;



        writeControl    timeStep;

        writeInterval   1;



        writeFields     true;



        regionType      cellZone;

        region          bac;



        operation       volIntegrate;

        fields

        (

            alpha.water

        );

    }

However, when running the simulation, I get the following warning:

Code:

--> FOAM Warning :



    request for objectRegistry bac from objectRegistry isoADVECTOR_irreguliere_Tp9.5s_Hs2.8m_gamma1.0_N70_RAFFINE1processor0 failed

    available objects of type objectRegistry are

1(region0)

The highlighted part of the error message is my case directory name, but I found it weird that "processor0" was added right after it, instead of "/processor0", which would make it look more like a path.

I get the same error message when running in sequential (not in parallel).

I have no idea where this could come from, as I have never encountered the "objectRegistry" word before.

Cheers,

Victor

I think, you problem is this line

Code:

region bac;

Regions are used in the chtMultiRegionFoam solver. I think you want "name" or something else.

See e.g. https://github.com/OpenFOAM/OpenFOAM...oneAverage#L21

Thanks Joachim, using "name" worked perfectly.

I just checked the documentation (https://www.openfoam.com/documentati...ieldValue.html), it turns out "name" was the correct entry to use. I don't know how I came up with "region"...

Would not have been mad if I had received a RTFM... :)