[rcastilla]

I have been working on capillary flows simulation with interFoam. When I make a simple simulation of the flow between two parallel vertical plates (2D), I got very strange results, due to an inadequate calculation of the contact angle correction (see the thread http://www.cfd-online.com/Forums/ope...tml#post264062 )

In the interfaceProperties library the contact angle correction is performed by modifying the direction of the unitary alpha gradient in the patch. It doesn't modify the alpha distribution itself, but only the vector that describes its gradient direction.

Then, in the interFoam solver, in the pEqn.H file, the contribution of the surface tension force is calculated as

fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1)*mesh.magSf()

The value of sigmaK is correct (it has been corrected by the interface object), but it is pointing in the wrong direction in the boundary cells, since it is calculated with fvc:snGrad(alpha1), which has not been corrected. The effect of that is huge when the flow is dominated by wall adhesion.

I suggest the following expression:

fvc::interpolate(interface.sigmaK()*mag(fvc::grad( alpha1)))*interface.nHatf()

It uses the gradient of alpha for the calculation of the force, but the direction is given by the surfaceScalarField nHatf, which has been corrected in the boundaries by the interface object.

I am testing it, and it seems to work. Simulations are very slow...

Perhaps there is a more elegant way of doing that.

Hope it will be useful.

Robert