CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Equilibrium thru Interface

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes
  • 1 Post By akidess
  • 1 Post By Cyp
  • 5 Post By Cyp

Reply
 
LinkBack Thread Tools Display Modes
Old   November 19, 2012, 03:23
Question Equilibrium thru Interface
  #1
Member
 
Hanniel Freitas
Join Date: Jan 2012
Location: Natal, Brazil
Posts: 34
Rep Power: 6
hfsf is on a distinguished road
Hi Foamers!
I'm having a little bit of trouble trying to remake the work done at the work of Waheed et al (2002) (http://www.sciencedirect.com/science...17931002001242), where some axissymetric wedge section of a drop inside a cilinder is taken, this drop containing solute, and the outer phase is solute-free. So, essencially I want to computate the solute transfer.

The main problem is that i need to establish a equilibrium of the solute concentration inside and outside the drop, what I believe I could do by phisically stablishing a interface boundary in my domain and using groovyBC to ser the dragient expression. So, essencially, my domain would consist of 2 regions: the drop and the outer phase. By now, the mesh construction is OK, and I could stablish this phisical boundary and the paraFoam recognizes it.

But running my case in my own implementation of interfoam (interfoam + solute transport), i noticed that the interface bondary (so called defaultFaces) is not needed. In fact, I can remove it from the boundary listed in the 0 directory with no problem! That's not right, my solver just ignores my equilibrium condition. What should I do? My master depends on this series of simulation

I'm attaching my case files. Thanks in advance, I hope someone out there could help me.

PS: In order to save space, after download and extraction please run blockMesh.
Attached Files
File Type: zip Drop.zip (14.6 KB, 23 views)
hfsf is offline   Reply With Quote

Old   November 19, 2012, 04:28
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,164
Rep Power: 20
akidess will become famous soon enough
I think you need two domains with non-identical vertices, which you then couple using some sort of a baffle boundary condition. Have a look at the tutorials for chtMultiRegionFoam, where this is done for the temperature equation.

- Anton
hfsf likes this.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2
akidess is offline   Reply With Quote

Old   November 19, 2012, 06:51
Default
  #3
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 251
Rep Power: 10
Cyp is on a distinguished road
Do you have a partitioning relationship between the concentration in both side of the interface ?

Something like :

C_{g} = H C_{l} \texttt{   at   } \mathcal{A}_{gl}

If it is the case, you can add a transport equation in interFoam solver using the theory of distributions (see Haroun (2012) for exemple)). The concentration jump will be considered as an additional term in your transport equation.

Best,
Cyp
hfsf likes this.

Last edited by Cyp; November 19, 2012 at 09:27.
Cyp is offline   Reply With Quote

Old   November 19, 2012, 07:07
Default
  #4
Member
 
Hanniel Freitas
Join Date: Jan 2012
Location: Natal, Brazil
Posts: 34
Rep Power: 6
hfsf is on a distinguished road
Dear Cyp and Anton,

Thanks for the fast reply. I will check your suggetions, thanks in advance.

And yes Cyp, i have a partitioning condition like the one you showed. But how could I implement this on the solver to consider this jump only thru the interface boundary? I will check the reference you suggested.
hfsf is offline   Reply With Quote

Old   November 19, 2012, 08:27
Default
  #5
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 251
Rep Power: 10
Cyp is on a distinguished road
I can explain it to you through a simple example. Consider only the diffusion between two phases (beta and gamma for instance) :

In the beta-phase you have
\nabla \cdot  D_{\beta}\nabla C_{\beta} = 0,

and in the gamma-phase
\nabla \cdot  D_{\gamma} \nabla C_{\gamma} = 0.

Both phases are connected through a flux continuity at the interface
\textbf{n}_{\beta\gamma} \cdot D_{\beta} \nabla C_{\beta} = 
\textbf{n}_{\beta\gamma} \cdot D_{\gamma} \nabla C_{\gamma} \texttt{  at  } \mathcal{A}_{\beta \gamma},

and the thermodynamic equilibrium condition reads:
C_{\beta}=H C_{\gamma} \texttt{  at  } \mathcal{A}_{\beta \gamma}


What you look for is an partial differential equation that govern
C = \alpha C_{\beta} + (1-\alpha) C_{\gamma}
where \alpha is the phase indicator provided from the VOF solution. With such a formulation, C is defined on the whole domain. In the same manner, you can defined a diffusion field as
D = \alpha D_{\beta} + (1-\alpha) D_{\gamma}

Now you express the derivative of C :
\nabla C = \alpha \nabla C_{\beta} + (1-\alpha) \nabla C_{\gamma} + (C_{\beta} - C_{\gamma})\nabla \alpha

multiplying this relation by D and applying the divergence operator, you get :

\nabla \cdot D \nabla C = \alpha \nabla \cdot D_{\beta}\nabla C_{\beta} + (1-\alpha) \nabla \cdot D_{\gamma} \nabla C_{\gamma}
+ (D_{\beta}\nabla C_{\beta}-D_{\gamma} \nabla C_{\gamma})\nabla \alpha + \nabla \cdot D (C_{\beta} - C_{\gamma})\nabla \alpha

Just keep in mind that according to the distribution theory you have : \textbf{n}_{\beta\gamma} = -\nabla \alpha. Consequently, the previous equation reduces to:

\nabla\cdot D \nabla C = \nabla \cdot D (C_{\beta} - C_{\gamma})\nabla \alpha,

This additional term represents the interfacial jump condition. If there is a continuity, you can get rid of it. However, if you have a partitioning relation, you have to consider it.

At the interface, we have C_{\beta}=H C_{\gamma}.

Consequently, C_{\beta} - C_{\gamma}= (1-H)C_{\gamma}

more over, C = \alpha C_{\beta} + (1-\alpha) C_{\gamma} = (\alpha H + (1-\alpha))C_{\gamma}

So C_{\beta} - C_{\gamma}= \frac{(1-H)}{\alpha H + (1-\alpha)} C

So your diffusion equation becomes :
\nabla\cdot D \nabla C = \nabla \cdot D \frac{(1-H)}{\alpha H + (1-\alpha)} C \nabla \alpha,

With such a formulation, you will automaticly have a jump condition at the interface between beta and gamma.

You can also optimised the solution with D = \frac{D_{\beta} D_{\gamma}}{\alpha D_{\gamma} + (1-\alpha)D_{\beta}}

I let you adapt this exemple to the advection-diffusion equation.

Best regards,
Cyp

Last edited by Cyp; November 19, 2012 at 09:26.
Cyp is offline   Reply With Quote

Old   June 28, 2013, 02:55
Default
  #6
Member
 
Luca Giannelli
Join Date: Jun 2010
Location: Kobe, Japan
Posts: 58
Rep Power: 8
voingiappone is on a distinguished road
Quote:
Originally Posted by Cyp View Post
So your diffusion equation becomes :
\nabla\cdot D \nabla C = \nabla \cdot D \frac{(1-H)}{\alpha H + (1-\alpha)} C \nabla \alpha,

With such a formulation, you will automaticly have a jump condition at the interface between beta and gamma.

You can also optimised the solution with D = \frac{D_{\beta} D_{\gamma}}{\alpha D_{\gamma} + (1-\alpha)D_{\beta}}

I let you adapt this exemple to the advection-diffusion equation.

Best regards,
Cyp
Cyp,

I don't actually know if you are still following this tread but I have a couple of questions.
It came for me too the time to implement the phase jump condition so I came back to this useful thread. In my previous case (a non-volatile tracer) I just had the Laplacian of a bunch of constants and alpha1: no problem in the solution if you insert the explicit laplacian (alpha1 already calculated). But in this case it is different because we have C an alpha1 simultaneously in the laplacian.

For what I can see in the other terms OpenFOAM always expects in the laplacian a dimensionedScalar and a volScalarField. So, I gathered all the constant terms in the fraction and calculated them before the C equation:

H =  D \frac{(1-H)}{\alpha H + (1-\alpha)}

Being this a function of alpha1 I had to define it in the Createfields.H as another volScalarField. Again, no problem. What I actually cannot understand is: how do I formulate this in C++??

\nabla\cdot D \nabla C = \nabla \cdot H \cdot C \nabla \alpha,

should become

Code:
fvm::laplacian(DC, C)
But if I code it this way, my solver won't compile. For what I see, the compiled does not like the fact that C is in the Laplacian.
Moreover my low C++ knowledge prevents me for finding an alternative formulation.
Do you have any hint?

Thanks!
voingiappone is offline   Reply With Quote

Old   March 11, 2016, 10:53
Default
  #7
New Member
 
Rimsha
Join Date: Jan 2016
Posts: 25
Rep Power: 2
block is on a distinguished road
Quote:
Originally Posted by voingiappone View Post
Cyp,

I don't actually know if you are still following this tread but I have a couple of questions.
It came for me too the time to implement the phase jump condition so I came back to this useful thread. In my previous case (a non-volatile tracer) I just had the Laplacian of a bunch of constants and alpha1: no problem in the solution if you insert the explicit laplacian (alpha1 already calculated). But in this case it is different because we have C an alpha1 simultaneously in the laplacian.

For what I can see in the other terms OpenFOAM always expects in the laplacian a dimensionedScalar and a volScalarField. So, I gathered all the constant terms in the fraction and calculated them before the C equation:

H =  D \frac{(1-H)}{\alpha H + (1-\alpha)}

Being this a function of alpha1 I had to define it in the Createfields.H as another volScalarField. Again, no problem. What I actually cannot understand is: how do I formulate this in C++??

\nabla\cdot D \nabla C = \nabla \cdot H \cdot C \nabla \alpha,

should become

Code:
fvm::laplacian(DC, C)
But if I code it this way, my solver won't compile. For what I see, the compiled does not like the fact that C is in the Laplacian.
Moreover my low C++ knowledge prevents me for finding an alternative formulation.
Do you have any hint?

Thanks!
Hi CyprienThank you very much for the explanation, can i please have a reference for these equation? I would really like to get in depth to understand the equations better.

Kind Regards

Rimsha
block is offline   Reply With Quote

Old   March 11, 2016, 13:57
Default
  #8
Cyp
Senior Member
 
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 251
Rep Power: 10
Cyp is on a distinguished road
@Article{Haroun2010,
Title = {Volume of fluid method for interfacial reactive mass transfer: Application to stable liquid film },
Author = {Y. Haroun and D. Legendre and L. Raynal},
Journal = {Chemical Engineering Science },
Year = {2010},
Number = {10},
Pages = {2896 - 2909},
Volume = {65},
Abstract = {A volume of fluid method is developed in order to simulate reactive mass transfer in two-phase flows and is applied to study reactive laminar liquid film. The thermodynamic equilibrium of chemical species at the interface is considered using Henry's law. The chemical species concentration equation is solved using primitive variables and local fluxes are locally directly calculated at the interface. The present treatment of jump discontinuity of chemical concentration is consistent with a volume of fluid approach and the difficulty to calculate accurate local mass flux across interface is overcome. For plane interface, the precision of the numerical simulation is found to be very satisfactory while for curved interface a special procedure has been developed to reduce the development of spurious fluxes at the interface. The algorithm is validated for different cases by comparison with available solutions. The method is then applied to study non-reactive and reactive mass transfer in a falling liquid film. The results show that the liquid side mass transfer is well predicted by the Higbie (1935) theory when the transfer is controlled by the film advection provided that adequate parameters are considered, i.e. the actual velocity at interface and not the average liquid film velocity. For situations controlled by diffusion, the Sherwood number tends to a constant value characteristic of purely diffusive situations. For the reactive mass transfer, first and second order irreversible chemical reactions in the liquid phase are considered. The numerical results are compared respectively, with Danckwerts (1970) and Brian et al. (1961) solutions and good agreement is observed. The proposed Volume of Fluid method is shown to be well adapted to deal with interfacial reactive mass transfer problems. },
DOI = {http://dx.doi.org/10.1016/j.ces.2010.01.012},
File = {Haroun2010.pdf:ARTICLES/Haroun2010.pdf:PDF},
ISSN = {0009-2509},
Keywords = {\{CFD\}},
URL = {http://www.sciencedirect.com/science/article/pii/S0009250910000291}
}

Cheers,
Cyp is offline   Reply With Quote

Old   March 11, 2016, 14:01
Default
  #9
New Member
 
Rimsha
Join Date: Jan 2016
Posts: 25
Rep Power: 2
block is on a distinguished road
Quote:
Originally Posted by Cyp View Post
@Article{Haroun2010,
Title = {Volume of fluid method for interfacial reactive mass transfer: Application to stable liquid film },
Author = {Y. Haroun and D. Legendre and L. Raynal},
Journal = {Chemical Engineering Science },
Year = {2010},
Number = {10},
Pages = {2896 - 2909},
Volume = {65},
Abstract = {A volume of fluid method is developed in order to simulate reactive mass transfer in two-phase flows and is applied to study reactive laminar liquid film. The thermodynamic equilibrium of chemical species at the interface is considered using Henry's law. The chemical species concentration equation is solved using primitive variables and local fluxes are locally directly calculated at the interface. The present treatment of jump discontinuity of chemical concentration is consistent with a volume of fluid approach and the difficulty to calculate accurate local mass flux across interface is overcome. For plane interface, the precision of the numerical simulation is found to be very satisfactory while for curved interface a special procedure has been developed to reduce the development of spurious fluxes at the interface. The algorithm is validated for different cases by comparison with available solutions. The method is then applied to study non-reactive and reactive mass transfer in a falling liquid film. The results show that the liquid side mass transfer is well predicted by the Higbie (1935) theory when the transfer is controlled by the film advection provided that adequate parameters are considered, i.e. the actual velocity at interface and not the average liquid film velocity. For situations controlled by diffusion, the Sherwood number tends to a constant value characteristic of purely diffusive situations. For the reactive mass transfer, first and second order irreversible chemical reactions in the liquid phase are considered. The numerical results are compared respectively, with Danckwerts (1970) and Brian et al. (1961) solutions and good agreement is observed. The proposed Volume of Fluid method is shown to be well adapted to deal with interfacial reactive mass transfer problems. },
DOI = {http://dx.doi.org/10.1016/j.ces.2010.01.012},
File = {Haroun2010.pdf:ARTICLES/Haroun2010.pdf:PDF},
ISSN = {0009-2509},
Keywords = {\{CFD\}},
URL = {http://www.sciencedirect.com/science/article/pii/S0009250910000291}
}

Cheers,
Brilliant, thank you very Cyprien, highly appreciated

Rimsha
block is offline   Reply With Quote

Old   May 24, 2016, 04:54
Default
  #10
Member
 
Timm Severin
Join Date: Mar 2014
Location: Munich
Posts: 60
Rep Power: 4
Astrodan is on a distinguished road
Note that although it was ages ago there is a mistake in the derivation done by Cyp:
Quote:
Originally Posted by Cyp View Post
At the interface, we have C_{\beta}=H C_{\gamma}.

Consequently, C_{\beta} - C_{\gamma}= (1-H)C_{\gamma}
is wrong, it should be C_{\beta} - C_{\gamma}= (H-1)C_{\gamma}

leading to the result of

\nabla\cdot D \nabla C = \nabla \cdot D \frac{(H-1)}{\alpha H + (1-\alpha)} C \nabla \alpha,

which, by the way, describes the view from "the other phase" compared to Haroun, who ends up at
\nabla\cdot D \nabla C = \nabla \cdot D \frac{(1-H)}{\alpha + H (1-\alpha)} C \nabla \alpha,
which would be equal to assuming C_\gamma = H C_\beta (which in fact is just H_1 = \frac{1}{H_2}).
Note that Cyps answer was a mixup of both solutions of nominator and denominator.

Edit: Thanks anyway Cyp, this was generally a great help.
And while at it, has anyone here managed to reproduce the calculations in the paper with OpenFOAM? I kind of struggle with different Henry coefficients (some work, some produce an exception).
Astrodan is offline   Reply With Quote

Old   June 14, 2016, 10:14
Default
  #11
Member
 
Timm Severin
Join Date: Mar 2014
Location: Munich
Posts: 60
Rep Power: 4
Astrodan is on a distinguished road
Finally my solver works now the way it was supposed to be. For anyone who cares I will attach my modified solver as well as two testcases. All modifications were made by made, but based on the publication by Haroun et al (2010), cited above, as well as Nieves-Remacha et al (2015):
OpenFOAM Computational Fluid Dynamic Simulations of Two-Phase Flow and Mass Transfer in an Advanced-Flow Reactor

María José Nieves-Remacha, Lu Yang, and Klavs F. Jensen
Industrial & Engineering Chemistry Research 2015 54 (26), 6649-6659
DOI: 10.1021/acs.iecr.5b00480
The Attachements:

interHarounFoam:
This is the solver. it is a modified version of interFoam, implementing both Equations found in Nieves-Remacha (2015), Supplemental. This means it implements as well the Haroun approach, as an approach by Marshall et al. (2012). It is merely for testing purpose, the diffusion coefficients are fixed to 1e^{-5} m^2 s^{-1} in the createFields.H, and the fields used are named H (for Haroun) and M (for Marshall).

NievesRemacha2015:
This is a sample case for the first example in the supplemental by Nieves-Remacha et al. It contains all relevant data to run interHarounFoam and generate one set of the results.

Haroun2010:
A sample case to reproduce the example shown in Figure 1 a/b of Haroun et al. (2010). This case can be run as it is, too.

A couple of further notes:
  • Both sample cases contain a visual.pvsm, which can be loaded in paraview (either using File > Load State) or starting paraview with the parameter --state=visual.pvsm.
    You will have to fix the path to your case, though.
  • Since diffusion coefficients and Herny coefficient are fixed in the solver, you will need to modify the createFields.H and re-compile the solver every time you want to try other values. Sorry about that. I am working on a library, which does the same thing, only better, which I intend to "publish" here soon.
  • In the fvSchemes make sure to use a Gauss linear scheme (or Gauss cubic, for what it matters) to solve div(phi,C). Most other schemes will fail, somewhere between extremely wrong results to crashing the solver.
  • Nieves-Remacha implement both equations as balances using the cellSurface (surfaceScalarField phiC), calculating first phiC ~ snGrad(alpha) and then div(phiC). Mathematically, the same could be achieved by having a laplacian(c, alpha) (something like that). Here OF allows to use a volScalarField c, which can also be created based on Harouns equation. However, this doesn't work either. I couldn't be bothered with the numerics or maybe even a simpler, mathematical reason for this, but you might care about this if you ever want to implement it on your own. Took me some days..
I hope this helps someone, I worked on this for quite a while.


May the foam be with you,
Timm
Attached Files
File Type: zip Haroun2010.zip (38.0 KB, 11 views)
File Type: zip interHarounFoam.zip (9.5 KB, 10 views)
File Type: zip NievesRemacha2015.zip (27.6 KB, 8 views)
Astrodan is offline   Reply With Quote

Reply

Tags
drop, interface position, interfoam, openfoam

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 45 February 8, 2016 05:42
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 21:09


All times are GMT -4. The time now is 03:50.