|
[Sponsors] |
solved: contact angle correction in interFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 25, 2010, 04:14 |
solved: contact angle correction in interFoam
|
#1 |
Senior Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 109
Rep Power: 17 |
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Dynamic contact angle | rmousavibt | Fluent UDF and Scheme Programming | 12 | October 31, 2021 22:38 |
Slug Flow, interFoam, problems with Contact Angle | PrzemekPL | OpenFOAM Running, Solving & CFD | 13 | February 18, 2014 22:10 |
[Netgen] Import netgen mesh to OpenFOAM | hsieh | OpenFOAM Meshing & Mesh Conversion | 32 | September 13, 2011 05:50 |
Implemening Slip bc and Dynamic contact angle in interFoam | asaha | OpenFOAM Running, Solving & CFD | 2 | July 29, 2010 15:49 |
Theoretical background of formula for dynamic contact angle in interfoam | sebastian_vogl | OpenFOAM Running, Solving & CFD | 3 | June 22, 2009 12:25 |