[jamestangx]

Dear Foamers,

I am new to OpenFoam and want to add surface tension to the cavitatingFoam solver. Is it possible to add surface tension in cavitatingFoam?

[Background]
I want to add surface tension term in cavitatingFoam solver to calculate collapsing cavitation (need compressible two phase solver). And I tried to implement surface tension according to interFoam solver. The new solver called cavitatingSTFoam is created and major files are attached. (The zip file of the whole solver exceeds the maxfilesize 195.3K, so I just upload the modified major files)

In interFoam.C, the immiscibleIncompressibleTwoPhaseMixture.H is included and the following code is used for surface tension term:

fvc::reconstruct
             (
                (
                    mixture.surfaceTensionForce()
                ) * mesh.magSf()
             )

However, the cavitatingFoam solver uses a different model and include "incompressibleTwoPhaseMixture.H" which dose not have surfaceTensionForce().

I tried to use the same continuum method to model the surface tension and add it in UEqn.H of cavitatingFoam refer to the previous thread Plotting suface tension with interFoam. New problem pops up for "interface","alpha1" and reconstruct function in "UEqn.H".

error message for "interface"

createFields.H: In function ‘int main(int, char**)’:
createFields.H:78:44: error: ‘interface’ was not declared in this scope
         fvc::reconstruct((fvc::interpolate(interface.sigmaK())*fvc::snGrad(alphal))* mesh.magSf())

error message for "alpha1"

cavitatingSTFoam.C:100:55: error: ‘alpha1’ was not declared in this scope
  f = fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1);

error message for "reconstruct"

In file included from cavitatingSTFoam.C:86:0:
UEqn.H:39:14: error: no matching function for call to ‘reconstruct(Foam::tmp<Foam::Field<Foam::Vector<double> > >)’
              )
              ^
UEqn.H:39:14: note: candidates are:
In file included from /opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.H:85:0,
                 from /opt/openfoam240/src/finiteVolume/lnInclude/fvc.H:43,
                 from /opt/openfoam240/src/finiteVolume/lnInclude/fvCFD.H:8,
                 from cavitatingSTFoam.C:35:
/opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.C:53:1: note: template<class Type> Foam::tmp<Foam::GeometricField<typename Foam::outerProduct<Foam::Vector<double>, Type>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::reconstruct(const Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh>&)
 reconstruct
 ^
/opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.C:53:1: note:   template argument deduction/substitution failed:
In file included from cavitatingSTFoam.C:86:0:
UEqn.H:39:14: note:   ‘Foam::tmp<Foam::Field<Foam::Vector<double> > >’ is not derived from ‘const Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh>’
              )
              ^
In file included from /opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.H:85:0,
                 from /opt/openfoam240/src/finiteVolume/lnInclude/fvc.H:43,
                 from /opt/openfoam240/src/finiteVolume/lnInclude/fvCFD.H:8,
                 from cavitatingSTFoam.C:35:
/opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.C:95:1: note: template<class Type> Foam::tmp<Foam::GeometricField<typename Foam::outerProduct<Foam::Vector<double>, Type>::type, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::reconstruct(const Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> >&)
 reconstruct
 ^
/opt/openfoam240/src/finiteVolume/lnInclude/fvcReconstruct.C:95:1: note:   template argument deduction/substitution failed:
In file included from cavitatingSTFoam.C:86:0:
UEqn.H:39:14: note:   mismatched types ‘Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh>’ and ‘Foam::Field<Foam::Vector<double> >’
              )
              ^
UEqn.H:39:14: note:   ‘Foam::tmp<Foam::Field<Foam::Vector<double> > >’ is not derived from ‘const Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> >’

Any ideas?
Thanks for your time，any help and advice is appreciated!

[jamestangx]

I finally added the surface tension term successfully by trial and error. I will share with everyone in case you met the same problem.

error message for "interface"
I included the following header files compared to OpenFoam 2.1 interFoam solver in my solver source code

// imported from interFoam 2.1
#include "interfaceProperties.H"
#include "twoPhaseMixture.H"

error message for "alpha1"
in createFields.H file, there is declarators for alphav, alphal. I don't know why it does not work with alpha1, however, when I change alpha1 ->alphal, the solver can be wmake sucessfully.

    incompressibleTwoPhaseMixture mixture(U, phi);
    volScalarField& alphav(mixture.alpha1());
    alphav.oldTime();
    volScalarField& alphal(mixture.alpha2());

error message for "reconstruct"
Also in "creatFields.H", the following codes should be added. And call the function of interface from "interfaceProperties.H"

// surface tension force is the same to the previous thread plotting surface tension with interFoam
// Construct interface from alphal distribution
    interfaceProperties interface(alphal, U, mixture);
    volVectorField f
    (
        IOobject
        (
            "f",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        fvc::reconstruct((fvc::interpolate(interface.sigmaK())*fvc::snGrad(alphal))* mesh.magSf())
    );

Finally, you can also add f=fvc::reconstruct((fvc::interpolate(interface.sig maK())*fvc::snGrad(alphal))* mesh.magSf()) in the source file for further postprocessing. And the following figure are the final results of surface tension magnitude and tangent vector in the slice view of the cavitation in water using tecplot 360.