[CFD_SG_01]

Hello everybody,

I face some difficulties to set a compressible steady case using rhoSimpleFoam.
Before showing detailed BC and the output issue I'd like to add the case is perfectly running with the incompressible solver Simple either with a kOmegaSST or kEpsilon turbulence model. The reason why I need to switch to a compressible solver is solve some density fluctuation in the system.

Here is the output error the terminal shows :

PHP Code:

nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.01
    field U      tolerance 0.0001
    field e      tolerance 0.001
    field "(k|epsilon)"  tolerance 0.001

Reading thermophysical properties

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

[stack trace]
=============
#1  Foam::sigFpe::sigHandler(int) in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#2  ? in /lib/x86_64-linux-gnu/libc.so.6
#3  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#4  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#5  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#6  Foam::fluidThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#7  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#8  Foam::fluidThermo::New(Foam::fvMesh const&, Foam::word const&) in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/lib/libfluidThermophysicalModels.so
#9  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/bin/rhoSimpleFoam
#10  ? in /lib/x86_64-linux-gnu/libc.so.6
#11  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#12  ? in /usr/lib/openfoam/openfoam2312/platforms/linux64GccDPInt32Opt/bin/rhoSimpleFoam
=============
Floating point exception 


The thermophysicalProperties :

PHP Code:

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

mixture // air at room temperature (313.15 K)
{
    specie
    {
        molWeight   28.9664;
    }
    thermodynamics
    {
        Cp          1003.62;
        Hf          0;
    }
    transport
    {
        mu          1.82e-05;
        Pr          0.9;
    }
} 


And here are the BC I set :
Velocity U:

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2312                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    
//Inlet
    AMI2
    {
                      
    type            fixedValue;
        value           uniform (0 0 0.5);
        
        
    }

//Outlet
    AMI3
    {
        type             inletOutlet;
    phi           phi;
    inletValue       $internalField;
        value           $internalField;
    }


//Walls
"(AMI5|AMI7|manifold|refined_surfaces|Pstat_out.*|Pstat_in)"
    
    {
      type            noSlip;
    }

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


T

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2312                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions      [0 0 0 1 0 0 0];

internalField   uniform 313;

boundaryField
{
//Inlet
    AMI2
    {
        type            fixedValue;
        value           $internalField;                
                        
    }

//Outlet
    AMI3
    {
        type            zeroGradient;
    }


//Walls
"(AMI5|AMI7|manifold|refined_surfaces|Pstat_out.*|Pstat_in)"
    
    {
        type            zeroGradient;
    }

}


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


Alpha_t

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2312                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
//Inlet
    AMI2
    {
        type            calculated;
        value           uniform 0;
                         
    }

//Outlet
    AMI3
    {
        type            calculated;
        value           uniform 0;
    }


//Walls
"(AMI5|AMI7|manifold|refined_surfaces|Pstat_out.*|Pstat_in)"
    
    {
        type            compressible::alphatWallFunction;
        value           uniform 0;
    }

   
}


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


and Pressure :

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2312                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
//Outlet
    AMI3
    {
        type            fixedValue;
        value           uniform 0;
    }
    
//Walls
"(AMI5|AMI7|manifold|refined_surfaces|Pstat_out.*|Pstat_in)"
    {
        type            zeroGradient;
    }
    
//Inlet
    AMI2
    {
        type            zeroGradient;
    }

    "proc.*"
    {
        type            processor;
    }

}


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


N.B.: The checkMesh is fine

Do you have any suggestion that could help to figure out this issue ?

Thank you in advance for your help

[Yann]

Hello,

The error message mentions libraries related to the thermophysicalProperties but your file seems to be fine. (it runs properly on a tutorial)

This is the usual output from rhoSimpleFoam when starting:

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

Reading field U

Reading/calculating face flux field phi

In your case it seems to crash when trying to read the U field, so I would expect the problem would be somehow related to U.

I am a bit puzzled by your patches named AMI. Is it supposed to be AMI interfaces or is it wall/patches? How is it defined in your polyMesh/boundary file?
If these are AMI interfaces it should be defined as cyclicAMI boundary conditions.

Since the crash occurs while the solver is starting up, the problem is most likely related to some conflicts in your case setup.

Regards,
Yann

[CFD_SG_01]

Originally Posted by Yann

I am a bit puzzled by your patches named AMI. Is it supposed to be AMI interfaces or is it wall/patches? How is it defined in your polyMesh/boundary file?
If these are AMI interfaces it should be defined as cyclicAMI boundary conditions.

Since the crash occurs while the solver is starting up, the problem is most likely related to some conflicts in your case setup.

Hello,
Thank you for your reply.
In fact the AMI designation, in this case, doesn't refer to AMI interface but are only used to set inlet and outlet. The reason why I set AMI names is in case of adding additionnal parts to the initial geometry.

I've checked the set up and I still can't find my mistake.

[CFD_SG_01]

This problem is solved. The mistake came from an error in the initial p file.
It is necessary to use absolute pressure value instead of relative pressure value.
In my case I change uniform 0 to uniform 101325