
[Sponsors] 
help adding the energy equation to porousinterfoam using the enthalpy formulation 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 9, 2013, 15:26 
help adding the energy equation to porousinterfoam using the enthalpy formulation

#1 
Member
nadine moussa
Join Date: Mar 2012
Posts: 30
Rep Power: 13 
Hello All,
I am adding the enrgy equation to porousinterfoam using the enthalpy formulation. So for my conductivity calculation, i need to multiply each material conductivity with the cell porosity. I search around to find out how to use the cell porosity but I didn't have any luck, so please can anyone lead me with his or her suggestions? Thank you all, Nadine 

May 13, 2013, 05:30 

#2 
Member
Join Date: Feb 2013
Posts: 30
Rep Power: 12 
Hi!
I'm afraid I cannot help you with your original question but I wonder whether you tried some simple cases with porousInterFoam? for example, if a socalled "rectilinear flow" is considered which is basically a 1D flow (imagine a rectangle where you have the inlet on the left hand side and the outlet on the right) there is an analytical solution to the flow front progression, xf = sqrt(2*K*P0*t/(mu*eps)) where xf denotes the flow front progression, K the permeability of the porous medium, P0 the injection pressure, mu the viscosity in Pa*s and eps the porosity. Now, as far as I have gleaned, the porosity eps is not taken into account when using the porousInterFoam solver but even if I assume eps=1, the solver does not yield correct results. Have you /has anyone experienced this problem? There have been some discussions last year to that topic and I also found a debugged version of the porousInterFoam solver (http://sourceforge.net/apps/mantisbt...iew.php?id=129) which should repair the problem of not taking the porosity into account. I'm trying to compile this debugged version and I will let you know whether this fixes the problem I described above, but still, I'm curious of your experiences with porousInterFoam. Greetings, Natalie 

May 13, 2013, 07:47 

#3  
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 17 
Quote:
Dear Natalie and Nadine, I would like to add some lights about porousInterFoam. Actually, porousInterFoam does not simulate two phase flow in porous media, expect in some very special cases (as the HeleShaw cells). This solver is not consistent with the twophase flow physic in porous media. You have to keep in mind that porous media laws are in fact averaged equations. That means that in one cell of the mesh, you have both fluid and solid, even if this latter is not physically represented. In twophase flow through porous material, we use the concept of saturation S, which is the rate of liquid over the void space volume of the cell. Basically, S varyies on the range [0,1]. The problem with porousInterFoam, is that this solver is just a VOF solver with additionnal resistance source terms. With that solver, the saturation does not exist and the phase indicator is either equal to 0 or 1. You can't have value in between (for exemple, S=0.4 means that the void space of a cell is filled by 40% liquid and 60% gas). So, in my opinion, this solver has absolutely no meanings. I think the right solution is to program a solver based on IMPES method (see a presentation I made at OFW7 for additionnal details). Best regards, Cyp Last edited by Cyp; May 13, 2013 at 13:14. 

May 13, 2013, 15:51 

#4 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,895
Rep Power: 36 
Hi Cyp,
Please allow me to disagree, since I exactly know the debugged version that Natalie referred to, as I myself posted that particular report. The debugged version corrects for the previous error that computational cells with a solid present did not fill faster than cells without a solid. The solution to this error was straight forward, because MULES was actually prepared to this type of flows, though the interface was not utilised in porousInterFoam. We had a master student, who tested the solver and he obtained good results in comparison with experimental data for coastal engineering size problems (dimensions of many meters in each direction). Kind regards, Niels P.S. There has not been a response to the bug report, since the error is still present in version 2.2.0. 

May 13, 2013, 15:56 

#5  
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 17 
Quote:
Yes, but with porousInterFoam, even with the debugged version, you can't have gas AND liquid in the same cell, can you ? 

May 13, 2013, 16:07 

#6 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,895
Rep Power: 36 
Hi Cyp,
I have just gone through your presentation, and I now understand what you mean. For your problems, where the saturation is of importance, then porousInterFoam will not work, because the two fluids are considered as immiscible. For coastal engineering problems, however, where there is a pretty clear interface between air and water, capillary effects can largely be neglected in man made structure and grain sizes are say 10 cm or larger, porousInterFoam does a pretty good job. I have tried reading the posts by Nadine and Natalie, however, it is a bit unclear to me, which effects are of importance to them. All the best, Niels 

May 14, 2013, 03:07 

#7 
Member
Join Date: Feb 2013
Posts: 30
Rep Power: 12 
Hi!
Thank you all for your replies! @Cyp: I'm afraid I cannot find the presentation you referred to, could you post a link? Although I think, I know the concept of introducing the saturation S as an independent variable. However, in my case, I can assume that the interface is sharp without taking capillary effects into account, so it sounds to me as if the debugged version of the porousInterFoam solver would solve my problem :) @Niels: Great to "meet" you in person! I have tried to compile your debugged version of the porousInterFoam solver, but I'm running into some problems. It is to say I am quite new to OpenFoam and thats the first additional piece of code I'm trying to compile. However, here is what I do and get: I'm using OpenFoam version 2.1.1 on Ubuntu 12.04. I have downloaded your file and put the entire directory "debuggedPorousInterFoam" into $FOAM_INST_DIR/applications/multiphase/interFoam and added the line wmake debuggedPorousInterFoam to the file Allwmake in $FOAM_INST_DIR/applications/multiphase/interFoam . Running Allwmake, I get the following errors when it comes to compiling the debuggedPorousInterFoam solver: + wmake debuggedPorousInterFoam In file included from /home/openfoam/TryoutOF/openfoam211/applications/solvers/multiphase/interFoam/createFields.H:96:0, from debuggedPorousInterFoam.C:60: /home/openfoam/TryoutOF/openfoam211/src/finiteVolume/lnInclude/readGravitationalAcceleration.H: In function ‘int main(int, char**)’: /home/openfoam/TryoutOF/openfoam211/src/finiteVolume/lnInclude/readGravitationalAcceleration.H:5:9: error: redeclaration of ‘Foam::uniformDimensionedVectorField g’ /home/openfoam/TryoutOF/openfoam211/src/finiteVolume/lnInclude/readGravitationalAcceleration.H:2:35: error: ‘Foam::uniformDimensionedVectorField g’ previously declared here In file included from debuggedPorousInterFoam.C:61:0: createPorousZones.H:21:45: error: ‘class Foam:orousZone’ has no member named ‘zoneId’ In file included from debuggedPorousInterFoam.C:63:0: /home/openfoam/TryoutOF/openfoam211/applications/solvers/multiphase/interFoam/correctPhi.H:37:12: error: ‘pimple’ was not declared in this scope In file included from debuggedPorousInterFoam.C:76:0: /home/openfoam/TryoutOF/openfoam211/applications/solvers/multiphase/interFoam/setDeltaT.H:37:36: error: ‘maxAlphaCo’ was not declared in this scope /home/openfoam/TryoutOF/openfoam211/applications/solvers/multiphase/interFoam/setDeltaT.H:37:48: error: ‘alphaCoNum’ was not declared in this scope In file included from debuggedPorousInterFoam.C:84:0: alphaEqnSubCycle.H:3:15: error: ‘piso’ was not declared in this scope In file included from alphaEqnSubCycle.H:22:0, from debuggedPorousInterFoam.C:84: alphaEqn.H:20:45: error: ‘class Foam:orousZone’ has no member named ‘zoneId’ In file included from alphaEqnSubCycle.H:30:0, from debuggedPorousInterFoam.C:84: alphaEqn.H:20:45: error: ‘class Foam:orousZone’ has no member named ‘zoneId’ .. and so on. Did I put the code at the wrong place in the source or do I need to (re)compile something else before? I would also be very interested in this master's thesis you mentioned, is it online available? Kind regards, Natalie 

May 14, 2013, 03:51 

#8 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,895
Rep Power: 36 
Good morning Natalie,
Unfortunately, the version you have downloaded is meant for version 1.6ext, and there are always small differences between the versions. Therefore: 1. Compare the debugged and your versions of porousInterFoam. 2. Transfer the differences into your 2.1.1. version of porousInterFoam, however, please note that some interfaces in the classes could have changes since 1.6ext. 3. Compile. A very pronounced difference is the call to Code:
MULES::explicitSolve(); Kind regards Niels P.S. As far as I know the thesis is not available online, and since I am no longer at University, I cannot help you in that regard. 

May 14, 2013, 08:35 

#9 
Member
Pierre HORGUE
Join Date: May 2009
Posts: 33
Rep Power: 16 
I totally agree with Cyp.
The VOF model is defined at the miscroscopic scale (or porescale) while the darcytype penalization term in the momentum equation is defined at the macroscopic scale where the computation cell is composed about thousand pores. The capillary force term depending on the local interface curvature : Code:
fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1) In your case, considering really strong simplifications : 1) capillary effect are negligible in the porous media. 2) your interface is always sharp in the porous media whatever the flow properties you can use the model but it remains in my opinion an illdefined model. In all cases, i think that is necessary to remove the capillary term in the porous medium (even if it has probably no effect, it is a physical non sense to keep it) and change the name of the solver because it misleads some people. Regards, Pierre 

May 16, 2013, 11:09 

#10 
Senior Member
Cyprien
Join Date: Feb 2010
Location: Stanford University
Posts: 299
Rep Power: 17 
dear all,
If you are looking for some good references regarding multiphase flow in porous media, have a look at : Petroleum reservoir simulation  Khalid Aziz, Antonín Settari it's the bible ! A more recent book is : Computational Methods for Multiphase Flows in Porous Media (Computational Science and Engineering)  Zhangxin Chen, Guanren Huan, Yuanle Ma All concepts and equations are detailed! Moreover, I am curious about the derivation of your analytical solution. Can you provide a reference ? Best, Cyp 

May 23, 2013, 02:40 

#11 
Member
Join Date: Feb 2013
Posts: 30
Rep Power: 12 
Hi Cyp,
have a look at this paper: http://www.scielo.br/scielo.php?pid=...pt=sci_arttext Here the RTM process (resin flow through fibrous preform) is modelled. Although the analytic solution stems from the reduction of the NavierStokes equations to Darcy's law, a simulation in that regime should give similar results, I believe. Best, Natalie 

September 20, 2013, 15:14 

#12  
Member
Mohammad Bahreini
Join Date: Dec 2012
Posts: 36
Rep Power: 12 
Quote:
can you guide me for this subject? Regards, 

June 8, 2014, 18:06 

#13 
New Member
David
Join Date: May 2012
Location: Canada
Posts: 12
Rep Power: 13 
Hi Nadine ,
Did you figure out a solution to your problem ?? Thanks 

June 9, 2014, 02:44 

#14 
Member
santhosh
Join Date: Apr 2009
Location: India
Posts: 70
Rep Power: 16 
Hi,
I am also looking for a solution where porousInterFOAM takes into account of porosity of computation cell. I thought by modifying the temporal term wherein, you have the porosity term in the equation, will solve the problem. Good to see the debuggedInterFoam here. Thanks. I will look into it now to see if I can modify work with 2.2.0 version. 

June 9, 2014, 04:30 

#15 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,895
Rep Power: 36 
Good day,
A lot of other things was also done to have (large scale) porosiy effects included, so take e.g. a look at the solver porousWaveFoam in the waves2Foam toolbox. Kind regards, Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

June 17, 2014, 08:14 

#16 
Member
nadine moussa
Join Date: Mar 2012
Posts: 30
Rep Power: 13 
Hello David,
well I sort of did but without using porousinterFoam! I changed the interFoam code where I added the energy equation and modified the momentum equation to account for the porosity. sorry not much help!!! 

June 17, 2014, 08:21 

#17 
New Member
David
Join Date: May 2012
Location: Canada
Posts: 12
Rep Power: 13 
Hi Nadine,
Were you able to add the effect of porosity [ the thermal conductivity of the porous material] in the energy equation? From my knowledge OpenFOAM doesn't take into account this effect and the only thermal model available for porous media is Fixed temperature !! I will appreciate any guidance in this point Thanks 

June 17, 2014, 08:25 

#18 
Member
nadine moussa
Join Date: Mar 2012
Posts: 30
Rep Power: 13 
David,
In my case I used the porosity approach in order to get two different regions (solid and fluid) so the porosity is either 1 or 0 no intermediate values. I wrote the thermophysical properties as function of the porosity and added a source term to the momentum equation as function of the porosity as well. hope this will help Nadine 

June 17, 2014, 08:39 

#19 
New Member
David
Join Date: May 2012
Location: Canada
Posts: 12
Rep Power: 13 
Thanks Nadine ,
I will try this and see how it goes David 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Adding viscous dissipation term to energy equation  newbee  OpenFOAM Running, Solving & CFD  6  March 3, 2021 10:37 
error message  cuteapathy  CFX  14  March 20, 2012 06:45 
energy equation in rhoCentralFoam  nakul  OpenFOAM  0  October 10, 2010 15:07 
ke turbulence model and energy equation  Blob  Main CFD Forum  0  May 29, 2009 08:35 
Why FVM for highRe flows?  Zhong Lei  Main CFD Forum  23  May 14, 1999 13:22 