[dav.dap83]

Hi,


I need to implement a pressureGradient force for spray parcels. I want to simulate gas parcels into a liquid using sprayFoam.

However, pressureGradient force needs a dictionary, and I have not been able to find an example of such a dictionary.
Can anyone provide an example, please?


Thanks

[chegdan]

Voila!

    particleForces
    {
		gravity;
		pressureGradient
		{
			U	U;
		};

    }

Note: This works for 2.1.x

[maysmech]

Originally Posted by chegdan

Voila!

    particleForces
    {
        gravity;
        pressureGradient
        {
            U    U;
        };

    }

Note: This works for 2.1.x

Hi,
It doesn't work with DPMFoam in 2.3.0

[dav.dap83]

Originally Posted by maysmech

Hi,
It doesn't work with DPMFoam in 2.3.0

In DPMFoam the velocity field of the fluid phase is named with Uc rather than U. So you just need to write:

    particleForces
    {
        gravity;
        pressureGradient
        {
            U    Uc;
        };

    }

[maysmech]

Originally Posted by dav.dap83

In DPMFoam the velocity field of the fluid phase is named with Uc rather than U. So you just need to write:

    particleForces
    {
        gravity;
        pressureGradient
        {
            U    Uc;
        };

    }

Thanks, But it leads to this error:

--> FOAM FATAL ERROR: 

    request for volVectorField Uc from objectRegistry region0 failed
    available objects of type volVectorField are
1(U.air)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/aut/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::PressureGradientForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::cacheFields(bool) at ??:?
#4  
 at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  
 at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 at ??:?
Aborted (core dumped)

DPMFoam uses U.air for velocity so using U.air instead of Uc leads to:

--> FOAM FATAL IO ERROR: 
keyword DUcDt is undefined in dictionary "/home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes"

file: /home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes from line 27 to line 29.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 437.

FOAM exiting

[Mojtaba.a]

Originally Posted by maysmech

Thanks, But it leads to this error:

--> FOAM FATAL ERROR: 

    request for volVectorField Uc from objectRegistry region0 failed
    available objects of type volVectorField are
1(U.air)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/aut/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::PressureGradientForce<Foam::KinematicCloud<Foam::Cloud<Foam::CollidingParcel<Foam::KinematicParcel<Foam::particle> > > > >::cacheFields(bool) at ??:?
#4  
 at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  
 at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 at ??:?
Aborted (core dumped)

DPMFoam uses U.air for velocity so using U.air instead of Uc leads to:

--> FOAM FATAL IO ERROR: 
keyword DUcDt is undefined in dictionary "/home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes"

file: /home/user/OpenFOAM/aut-2.3.0/run/tutorials/lagrangian/DPMFoam/testSaffman/constant/kinematicCloudProperties.solution.interpolationSchemes from line 27 to line 29.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 437.

FOAM exiting

Try

    interpolationSchemes
    {
        rho.air             cell;
        U.air               cellPoint;
        mu.air              cell;
        DUcDt            cellPoint;
    }