
[Sponsors] 
February 4, 2017, 02:18 
Fixed Temperature in Porous Zone

#1 
Member
Anirudh Kulkarni
Join Date: May 2016
Posts: 60
Rep Power: 9 
Dear Foamers,
I am trying to simulate flow across a heated porous cylinder. I wish to assign a fixed temperature to the cylinder. If I use toposetDict, it would assign a fixed temperature only for the initial phase, but update it as the simulation runs ahead. Please help me out. Basically, I would like to give a boundary condition to an entire cellzone i.e. fixed temperature. Thanks in advance. 

February 6, 2017, 00:44 
Found it

#2 
Member
Anirudh Kulkarni
Join Date: May 2016
Posts: 60
Rep Power: 9 
We can do this by using fvOptions and
TEqn.H Code:
{ fvScalarMatrix TEqn ( fvm::ddt(T) + (1/porosity)*fvm::div(phi, T)  fvm::laplacian(nu/Pr, T) == fvOptions(T) ); TEqn.relax(); fvOptions.constrain(TEqn); TEqn.solve(); fvOptions.correct(T); rhok = 1.0  beta*(T  TRef); } Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // s1 { type scalarFixedValueConstraint; active true; scalarFixedValueConstraintCoeffs { selectionMode cellZone; cellZone porousZone; fieldValues { T 350; \\the fixed temperature value } } } // ************************************************************************* // 

January 30, 2018, 06:01 
ADDING POROSITY IN TEqn IN OPENFOAM

#3  
Member
Ramana
Join Date: Jul 2017
Location: India
Posts: 58
Rep Power: 8 
Quote:


February 7, 2018, 15:49 

#4 
Senior Member
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 111
Rep Power: 9 
Hello Ramana,
Currently, the only way to implement the flow effects of a porous media in a predefined solver is using the darcy forchheimer model. The coefficients may be determined, depending on the case, using Erguns equation. To use the porosity directly you have to make a usermade solver. A basic approach describing the implementation of a porous medium model in an existing solver is described here: https://www.slideshare.net/Cypiii/op...trainingv51en Regards Lasse 

February 11, 2018, 23:15 

#5  
Member
Ramana
Join Date: Jul 2017
Location: India
Posts: 58
Rep Power: 8 
Quote:
Thank you for your response.I have gone through above link and able to simulate basic flow and heat transfer approach in porous media. Now coming to my simulation ,i want to simulate flow and heat transfer from porous square cylinder to a flowing wind. The computational domain is as appended below cfd.png I have defined the porous cylinder as porous blockage( similar to the one in PisoFaom tutorial) and now i want to modify the governing equation to make a userdefined solver. The governing equations for the above problem are GEqn.png The governing equations for porousmedia in OF are defined as DF Eqn.png In predefined solver for porous media i.e PorousSimplefoam,There is no time derivative (as it is a steady state solver )and there is no entry to read porosity. I have few questions regarding momentum and energy equations 1). How and where to define porosity (1 for fluid region & (0<porosity<1) for porous zone) as i am using single domain approach(single set of governing equations are utilized to solve both fluid and porous zones). 2). what are the modifications required in momentum equation to include porosity effect in it. (similar to the one in fluent solver Eqn. enclosed) fluent Eqn.png Thanks in advance, Reagrds, S.V.Ramana 

February 13, 2018, 06:20 

#6 
Senior Member
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 111
Rep Power: 9 
Hello Ramana,
1) To my understanding the FLUENT porosity will never impact the flow velocity in the medium, its only used in the case of thermal modelling https://www.sharcnet.ca/Software/Ans...ous_media.html. No matter what value you set for porosity, FLUENT predicts that the flow velocity is the superficial velocity in the medium. Some more on that here http://jullio.pe.kr/fluent6.1/help/html/ug/node237.htm Using the DarcyForchheimer equation as described here: http://www.tfd.chalmers.se/~hani/kur...ukurReport.pdf Some other Foamers, have had discussion about this such as Porosity and permeability in PorousInterFoam. 2) If you were to implement the porousity instead of using the DarcyForchheimer, you would need to apply the porousity into the momentum equation similarly to the FLUENT formulation, however, I would not be certain that the correct pressure loss is determined, as I would think you also would have to determine the pressure influence of the porous media using something like the Ergun equation. Hope this makes sense, else please let me know and I will get back to you. Regards Lasse. Last edited by Swagga5aur; February 13, 2018 at 08:18. 

April 27, 2018, 06:48 

#7  
Senior Member
Deep
Join Date: Oct 2017
Posts: 180
Rep Power: 7 
Quote:
Hello Anirudh, I have used this approach in last few months and I've come to a conclusion that this doesn't really "initialise" the porous zone as it should. At least in my simulations I found that the temperature in the porous zone is maintained at the value supplied through fixedTemperatureConstraint throughout the timespan and doesn't change with respect to flow over the consecutive timesteps as it ideally should. I am looking for any alternative. 

Tags 
openfoam 4.1, porous cell zone, temperature bc 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[openSmoke] libOpenSMOKE  Tobi  OpenFOAM Community Contributions  562  January 25, 2023 09:21 
Error in solution using "Grid Interface"  agustinvo  FLUENT  4  January 20, 2015 12:03 
Cluster ID's not contiguous in computenodes domain. ???  Shogan  FLUENT  1  May 28, 2014 15:03 
Fixed mean temperature boundary condition for developing flow  mohsen cheraghi  OpenFOAM  2  July 24, 2011 13:06 
Fluent incident radiation problem  Michael Schwarz  Main CFD Forum  0  October 21, 1999 05:56 