
[Sponsors] 
April 7, 2009, 06:08 
Thermocapillary free surface flow

#1 
New Member
Zaki Saldi
Join Date: Mar 2009
Posts: 18
Rep Power: 17 
Dear all,
I am interested in the VOF simulation of free surface flow driven by surface tension gradient due to surface temperature variation. To do this, I have tried to add energy equation (temperaturebased) in interFoam, in which the thermal conductivity is weighted by volume fraction, just like density and viscosity. Additionally, at the interface, the smeared surface force has the normal and tangential components of the following form: where Here sigma_0 is surfac tension at reference temperature, sigma_T is dsigma/dT, i.e. the temperature gradient of surface tension, and T_0 is the reference temperature. The first term of the normal force already exists in interFoam, so I need to implement the second term of the surface force and the tangential force. I ended up with the following in UEqn.H : surfaceScalarField muf = twoPhaseProperties.muf(); fvVectorMatrix UEqn ( fvm::ddt(rho, U) + fvm::div(rhoPhi, U)  fvm::laplacian(muf, U)  (fvc::grad(U) & fvc::grad(muf)) // fvc::div(muf*(fvc::interpolate(dev(fvc::grad(U))) & mesh.Sf())) ); if (momentumPredictor) { solve ( UEqn == fvc::reconstruct ( ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(g amma) + fvc::interpolate(dsigmadT*(TT0)*interface.K())*fvc::snGrad(gamma) + fst  ghf*fvc::snGrad(rho)  fvc::snGrad(pd) ) * mesh.magSf() ) ); } and in pEqn.H : phi = phiU + ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(g amma) + fvc::interpolate(dsigmadT*(TT0)*interface.K())*fvc::snGrad(gamma) + fst  ghf*fvc::snGrad(rho) )*rUAf*mesh.magSf(); Here, I have implemented the second term for the normal force (highlighted in blue), but not the whole tangential component of the surface force (in red). This tangential part is a bit confusing, since in UEqn.H, everything in fvc::reconstruct brackets should be of the type surfaceScalarField. I tried to specify fst as follows: volVectorField nhat = gradGamma/(mag(gradGamma) + deltaN); volVectorField fst = dsigmadT*(fvc::grad(T)  nhat*(nhat & fvc::grad(T)))*mag(gradGamma); Here, fst is a volVectorField, which can not be used in UEqn.H and pEqn.H above. Could anyone help me with this problem? Thanks a lot, Zaki 

May 7, 2009, 04:30 

#2 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 17 
Dear Zaki,
Have you had any success in solving your problem? please let me know, Best, Hamed 

May 19, 2009, 07:29 

#3 
New Member
Zaki Saldi
Join Date: Mar 2009
Posts: 18
Rep Power: 17 
Hi Hamed,
I think I have moved one very small step forward in solving the problem with the tangential force. Now I have a modified interFoam to account for this thermocapillary effect. However, after testing the code, I was not satisfied with the result in comparison with the one in literature. Please find the source code and the test case in the attachment. The test case is thermocapillary motion of deformable drops in a vertical temperature gradient (no gravity), which follows the one reported in: www.stanford.edu/group/ctr/Summer/SP08/3_2_Lopez.pdf I tested the first problem in that paper (case of limit of zero marangoni number, page 161162), and comparing my result with figure 1 (page 162). Please kindly have a look at it and I would appreciate it if you could give comments, suggestions, help. regards, zaki 

May 19, 2009, 11:17 
adding Temprature to les/interfoam

#4 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 17 
Dear Zaki,
Thanks for updating the thread, I want to add temperature to les/interFoam? The equation I am trying to add is; (1) rho*Cp*[ddt(gamma*T)+grad(gamma*U*T)]=laplacian(gamma*Landa_eff*T) I know that, a surfaceScalarField should be exist to update thermal conductivity in each time step (2) {Landa_eff = Landa + Cp*nuSgs()}, I have Les Turbulence Model as well. To comply the Eq.2, should I modify a new library for Landa(Thermal conductivity), to call it in TEqn as twoPhaseProperties.landa(), or something else. I also tried with Creatfield and it didn't worked. Please elaborate, Kindly, Hamed hamed.aghajani@gmail.com h.aghajani@kingston.ac.uk 

May 19, 2009, 12:01 

#5 
New Member
Zaki Saldi
Join Date: Mar 2009
Posts: 18
Rep Power: 17 
Hi Hamed,
My questions & remarks: 1. Why do you need gamma in the energy equation (eq. 1) ? 2. Seems to me the terms in eq 2 are dimensionally inconsistent. I think they should be like this: suppose landa = thermal conductivity, and alpha thermal diffusivity. so alpha = landa/(rho*Cp) landa_eff = landa + landa_sgs = landa + rho*Cp*alpha_sgs = landa + rho*Cp*nu_sgs / Pr_t where Pr_t is the turbulent Prandtl number. It is of course elegant to define landa (or its cellface value landaf) in a new library. But I think you can also do it like this:  define landa as volScalarField, also constants landa1 & landa2 for each fluid  after calculating gamma, define landa = landa1*gamma + landa2*(1gamma), also similarly with Cp  before solving energy equation: surfaceScalarField gammaf = fvc::interpolate(gamma); surfaceScalarField landaf = fvc::interpolate(landa); surfaceScalarField landaEff ( "landaEff", landaf + fvc::interpolate(rho*Cp*turbulence>nuSgs()/Pr_t) ); kind regards, zaki 

May 20, 2009, 13:23 
added TEqn to les/interfoam

#6 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 17 
Dear Zaki,
Thanks for your kind reply, I saw the eq.(1) in a paper, Cryogenics 48 (2008) 238–247, and have not understood why the autors chose the energy equation in that form. But I attached part of that paper to this thread. you can find it in eq.8; I couldn't call turbulent Prandt number and the TEqn, as you suggested,I wrote is; surfaceScalarField landaf = fvc::interpolate (landa); surfaceScalarField landaEff ( "landaEff" landaf + fvc::interpolate(rho*Cp*turbulence>nuSgs()) ); fvScalarMatrix TEqn ( rho*Cp* (fvm::ddt(T) + fvm::div(phi, T) )  fvm::laplacian(landaEff, T) ); TEqn.solve(); It is running on a case and I haven't checked the result yet, Kindly, Hamed 

August 24, 2014, 03:24 
thermocapillary

#7 
New Member
Join Date: Aug 2014
Posts: 1
Rep Power: 0 
how can i coding thermocapillary flows in a confined microchannel
with LBM method? 

December 9, 2016, 20:22 

#8 
Member
Kalpana Hanthanan Arachchilage
Join Date: May 2015
Location: Orlando, Florida, USA
Posts: 30
Rep Power: 10 
Dear Dr. Zaki,
I've referred to your PhD dissertation as I'm planning to implement and validate the tangential component of the surface tension force. I've tried to simulate the cavity simulation you used to validate surface tension force. However, i'm not getting the correct result. One thing i noticed is they provided data to obtain the physical properties of liquid. but, it didn't mention anything about the vapor side physical properties. Can you please let me know, what kind of physical properties you used for vapor side. Thank you, Kalpana Hanthanan Arachchilage 

December 12, 2016, 04:59 

#9  
Member
Ricky
Join Date: Jul 2014
Location: Germany
Posts: 78
Rep Power: 11 
Quote:
If I am not wrong, are you trying to validate your case in twophase environment compared to Dr. Saldi's singlephase? If yes, then there are 2 more test cases you could actually use to validate your tangential component of the surface tension force. 1) Is already mentioned here (see post > #3) 2) you could also validate your case with his "TwoPhase Marangoni driven flows" (sec 3.5 of his thesis) > which I am trying to do currently but the results are way off. In my case the surface height at left wall is 0.194 and at the right wall is 0.204. Perhaps you may come up with some better solution. Regards, Ricky Last edited by kera; December 12, 2016 at 08:53. 

December 12, 2016, 10:20 

#10  
Member
Kalpana Hanthanan Arachchilage
Join Date: May 2015
Location: Orlando, Florida, USA
Posts: 30
Rep Power: 10 
Quote:
Thank you for your reply. Actually i was referring to section 3.5. As these nondimensional numbers are only based on liquid properties, you have no idea what kind of properties you should use to the vapor side. I'm using interfoam based solver and i'm also getting similar results that you obtained. However, I assumed liquid and vapor properties to be equal. but, when i used different properties for vapor solution changes and I'm wondering what kind of property i have to use. The other thing is spurious currents. I have tried the droplet simulation as well, but those curved surfaces increase spurious currents and over predicting the results. there is another test case you can simulate. these are the references for that. N.Balcazar et al/ International journal of heat and fluid flow (2016) H.Liu et al/ Journal of computational physics 231 (2012) 44334453 Will let you know if there is any improvement. And please let me know what are the vapor properties you used for the above simulation. Regards, Kalpana 

December 12, 2016, 11:44 

#11 
Member
Ricky
Join Date: Jul 2014
Location: Germany
Posts: 78
Rep Power: 11 
Hello Kalpana,
Well I am using interfoam for the time being. Initially I assumed both the fluids have same properties, I had a solution which was no way to be considered and then I assumed second fluid as air, I had another solution but it's kinda miss leading as the surface height on the left and right walls goes upto 0.182 and 0.216 or something like that. Regards, Ricky Last edited by kera; December 12, 2016 at 12:54. 

Tags 
free surface, interfoam, marangoni, thermocapillary 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
free surface flow past cylinder  vineet  FLUENT  1  February 21, 2011 23:11 
free surface flow in noninertial reference frame  Tiedingg  FLOW3D  1  February 26, 2009 19:51 
Multiphase flow. Dispersed and free surface model  Luis  CFX  8  May 29, 2007 18:13 
Analytical Solution for a Free Surface Flow  Ferreira, VG  Main CFD Forum  0  February 25, 2007 04:56 
CFX4.3 build analysis form  Chie Min  CFX  5  July 12, 2001 23:19 