# InterFoam contact angle

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 15, 2010, 14:28 InterFoam contact angle #1 New Member   Joao Miranda Join Date: Oct 2010 Posts: 1 Rep Power: 0 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?

 September 4, 2011, 03:06 It's not the calculation that becomes impossible .... #2 Member   Michiel Join Date: Oct 2010 Location: Delft, Netherlands Posts: 97 Rep Power: 15 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 v_scientist likes this. Last edited by michielm; September 4, 2011 at 10:44. Reason: Wrong reference

 January 31, 2014, 07:40 Conatct angle in multiphaseinterfoam #3 New Member   Rajesh Join Date: Jul 2012 Location: New Delhi Posts: 8 Rep Power: 13 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.

 August 26, 2014, 11:29 Contact Angle Correction #4 Member   Vignesh Join Date: Oct 2012 Location: Darmstadt, Germany Posts: 66 Rep Power: 13 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 . 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(abf[patchi])) { alphaContactAngleFvPatchScalarField& acap = const_cast ( refCast ( 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 kmou likes this. __________________ Thanks and Regards Vignesh

October 19, 2016, 12:08
#5
Member

Camille Bilger
Join Date: Jul 2013
Posts: 43
Rep Power: 12
Quote:
 Originally Posted by vigneshTG 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 . The correctcontactangle function is given below Thanks for your time
Hi Vignesh, Did you understand how the variable theta is being passed correctly to the function correctContactAngle from the boundary condition implementation that calculates theta ?
Thank you

October 19, 2016, 14:13
#6
Member

Vignesh
Join Date: Oct 2012
Posts: 66
Rep Power: 13
Quote:
 Originally Posted by kmou Hi Vignesh, Did you understand how the variable theta is being passed correctly to the function correctContactAngle from the boundary condition implementation that calculates theta ? Thank you
Hi kmou,

Check kunkelman's thesis in the link, section 3.2.4

Please read it and let me know if you don't understand !!
__________________
Thanks and Regards

Vignesh

October 20, 2016, 06:05
#7
Member

Camille Bilger
Join Date: Jul 2013
Posts: 43
Rep Power: 12
Quote:
 Originally Posted by vigneshTG Hi kmou, Check kunkelman's thesis in the link, section 3.2.4 Please read it and let me know if you don't understand !!
That helps a lot thank you! Although I am still wondering how is theta passed from the dynamicContactAngle imposed boundary condition.
I'm guessing the answer lies in here:

if (isA<gammaContactAngleFvPatchScalarField>(gbf[patchi]))
{
const gammaContactAngleFvPatchScalarField& gcap =
refCast<const gammaContactAngleFvPatchScalarField>
(gbf[patchi]);

October 20, 2016, 06:27
#8
Member

Vignesh
Join Date: Oct 2012
Posts: 66
Rep Power: 13
Quote:
 Originally Posted by kmou That helps a lot thank you! Although I am still wondering how is theta passed from the dynamicContactAngle imposed boundary condition. I'm guessing the answer lies in here: if (isA(gbf[patchi])) { const gammaContactAngleFvPatchScalarField& gcap = refCast (gbf[patchi]);

Yes you are right !!
__________________
Thanks and Regards

Vignesh

 Tags contact angle, corner, interfoam

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post rmousavibt Fluent UDF and Scheme Programming 12 October 31, 2021 22:38 rcastilla OpenFOAM Bugs 24 March 2, 2016 13:43 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 sebastian_vogl OpenFOAM Running, Solving & CFD 3 June 22, 2009 12:25

All times are GMT -4. The time now is 07:25.

 Contact Us - CFD Online - Privacy Statement - Top