CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   InterFoam contact angle (http://www.cfd-online.com/Forums/openfoam-solving/81101-interfoam-contact-angle.html)

JoaoMiranda October 15, 2010 14:28

InterFoam contact angle
 
Usually in a VOF method the contact angle is introduced in the simulation in the calculation of the curvature. The curvature near the boundary is determined based the vector normal to the surface. The vector normal to the surface is calculated from the contact angle.



The vector normal to the surface, n=(nx,ny,nz) is related to the angle by:

ny/SQRT(nx^2+nz^2)=cot(theta)


According to the following paper:


Chen Fang, Carlos Hidrovo, Fu-min Wang, John Eaton, Kenneth Goodson, 3-D numerical simulation of contact angle hysteresis for microscale two phase flow, International Journal of Multiphase Flow, Volume 34, Issue 7, July 2008, Pages 690-705


the calculation of the contact angle becomes complicated in corners, where two angles exist. The calculation of the vector normal do the surface becomes impossible for angles smaller than 45 degrees.


The vector n=(1,ny,nz) is related to the angle by:


ny=cos(theta1)/(1-cos(theta1)^2-cos(theta2)^2)


nz=cos(theta2)/(1-cos(theta1)^2-cos(theta2)^2)


These equation only work for cos(theta1)^2+cos(theta2)^2>1


How are these calculations handled in InterFoam? Specifically, how are contact angles handled in corners?

michielm September 4, 2011 03:06

It's not the calculation that becomes impossible ....
 
I know this question is about a year old, but maybe for the benefit of other openfoam (or CFD) users it is good to know:

The reason that there is no solution to the equations for 45 degrees or less is that it is an unphysical situation to have a contact line in the corner if the CA is below 45 degrees. If this happens, you will get a corner with the low CA fluid completely filling the corners: so called gutter flow.

Check out Concus and Finn or Oron for more details on the math behind this:

* Concus and Finn, On The Behavior Of A Capillary Surface In A Wedge, PNAS, 1969
* Ajaev and Homsy, Modeling Shapes and Dynamics of Confined Bubbles, ARFM, 2006

In some situations, the existence of these `gutters' is essential to describe the physics of two-phase microflows:
* van Steijn et al., Flows Around Confined Bubbles And Their Importance In Triggering Pinch-off, Phys. Rev. Lett., 2009

rajeshchem January 31, 2014 08:40

Conatct angle in multiphaseinterfoam
 
Hi,

Could anyone tell me the implementation of dynamic contact angle in multiphaseInterfoam solver?

There are four contact angle values to be input for multiphaseInterFoam, via.. equlibrium contact angle, Utheta, Advancing contact angle, Receding contact angle.

I found some details , how contact angle is being calculated in multiphaseInterFoam as follows,
θ = (θA − θR ) ∗ tanh(uwall/uθ)

my question is when i use no slip boundary condition, u wall is zero then the theta on left hand side is also becomes zero. Then how the contact angle effect is being imposed in multiphaseinterFoam under no slip BC. First of all, is this solver requires all four contact angle to be defined?

Please help me to understand this contact angle issue.

vigneshTG August 26, 2014 11:29

Contact Angle Correction
 
Hi everyone !

I am trying to understand how contact angle is corrected in interfoam based on theta value given either as input (constant contact angle mode) or calculated dynamically.
I started looking at the function correctcontactangle in interfaceProperties.C and i am confused as to how it corrects the contact angle :confused:. The correctcontactangle function is given below

Code:

void Foam::interfaceProperties::correctContactAngle
(
    surfaceVectorField::GeometricBoundaryField& nHatb,
    surfaceVectorField::GeometricBoundaryField& gradAlphaf
) const
{
    const fvMesh& mesh = alpha1_.mesh();
    const volScalarField::GeometricBoundaryField& abf = alpha1_.boundaryField();

    const fvBoundaryMesh& boundary = mesh.boundary();

    forAll(boundary, patchi)
    {
        if (isA<alphaContactAngleFvPatchScalarField>(abf[patchi]))
        {
            alphaContactAngleFvPatchScalarField& acap =
                const_cast<alphaContactAngleFvPatchScalarField&>
                (
                    refCast<const alphaContactAngleFvPatchScalarField>
                    (
                        abf[patchi]
                    )
                );

            fvsPatchVectorField& nHatp = nHatb[patchi];
            const scalarField theta
            (
                convertToRad*acap.theta(U_.boundaryField()[patchi], nHatp)
            );

            const vectorField nf
            (
                boundary[patchi].nf()
            );

            // Reset nHatp to correspond to the contact angle

            const scalarField a12(nHatp & nf);
            const scalarField b1(cos(theta));

            scalarField b2(nHatp.size());
            forAll(b2, facei)
            {
                b2[facei] = cos(acos(a12[facei]) - theta[facei]);
            }

            const scalarField det(1.0 - a12*a12);

            scalarField a((b1 - a12*b2)/det);
            scalarField b((b2 - a12*b1)/det);

            nHatp = a*nf + b*nHatp;
            nHatp /= (mag(nHatp) + deltaN_.value());

            acap.gradient() = (nf & nHatp)*mag(gradAlphaf[patchi]);
            acap.evaluate();
        }
    }
}



Can anyone point me to some reference where it is explained or Can someone explain how the code !!


Thanks for your time


All times are GMT -4. The time now is 14:34.