
[Sponsors] 
compressibleInterFoam : biphasic, compressible, equation of state 

LinkBack  Thread Tools  Display Modes 
March 11, 2013, 05:04 
compressibleInterFoam : biphasic, compressible, equation of state

#1 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Hi everyone,
I am a new user on OpenFoam. I would like to run a compressible and biphasic case. It seems that, it is possible using compressibleInterFoam. However, I also want to change the two fluids' equation of state. Do I have to modify the C code of the solver, or there is a simpler way ? Thanks Best regards Clément Last edited by clementolivier; March 11, 2013 at 07:46. 

March 11, 2013, 12:41 

#2 
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,147
Blog Entries: 1
Rep Power: 15 
you should change source code, there is no easier task
__________________
Training Course on OpenFOAM at (http://www.isme.ir/) My Weblog (http://openfoam.blogfa.com/) 

March 12, 2013, 04:33 

#3 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Thank you for your answer, I will get back to work !


March 12, 2013, 05:36 

#4 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 241
Rep Power: 9 
hello,
This is already possible to change the fluid equation of state. Take a look in the depthCharge tutorial, in TransportProperties : would can choose constant, linear, perfectFluid, ... Regards, olivier 

March 12, 2013, 06:04 

#5 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Thank you for your answer olivierG.
I can see how to change the constants of the model (nu,rho,rho0,psi), but I do not quite see how to change the formula of the equation of state. Do you mean that the argument of transportModel specifies it ? If it is the case, is there any exhaustive list of all allowed arguments ? 

March 12, 2013, 06:18 

#6 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 241
Rep Power: 9 
hello,
First what the state equation you would use ? And which version of openfoam do you use ? To get the list of state equation, put "dummy" instead of perfectFluid : you will get a list. To find more info, you should take a look at the source code. this part was in the solver for the 2.1.x version, but has moved with the 2.2.x regards, olivier 

March 12, 2013, 06:39 

#7 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Thank you again for your help
I want to use the equation of state called the Stifeffened Gas Equation of State for the liquid, and the Perfect Gas Equation of State for the gas. I am currently usig OpenFoam v2.1.1. I am sorry but I have done a grep rin "perfectFluid" * in the directory tutorials/multiphase/compressibleInterFoam, and it is nowhere written. Can you explain more precisely where whould I type "dummy". I am right now reading the C++ code in order to fix my problem. 

March 12, 2013, 06:46 

#8 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 241
Rep Power: 9 
hello,
1) in your tuto case, set "dummy" (or anythink), then launch the solver: you will get an error message, which will say dummy is not a equation of state, and will list the possible one. 2) For the 2.1.1, the definition is in the solver source, never in the tutorial. take a look at applications/solvers/multiphase/compressibleInterFoam/phaseEquationsOfState/ in your installation directories. regards, olivier 

March 12, 2013, 07:10 

#9 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Thanks,
I still do not see where should I set "dummy" (or anything). Moreover the directory applications/solvers/multiphase/compressibleInterFoam/phaseEquationsOfState/ does not exist in my version. I will get I last version and it will be easier for me to communicate. regards, Clément 

March 12, 2013, 07:22 

#10 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 241
Rep Power: 9 
hello,
Sorry, i wasn't clear. copy the tuto (depthCharge3D). Open depthCharge3D/constant/transportProperties You have 2 phase, air and water. In the definition of water, you should have: Code:
equationOfState { type perfectFluid; rho0 1000; R 3000; } regards, olivier 

March 12, 2013, 07:36 

#11 
New Member
Clement Olivier
Join Date: Mar 2013
Posts: 7
Rep Power: 4 
Thank you very much,
Indeed in the last version, I can see everything you are talking about. I think,this will fix my problem. Thank you again Regards, Clément 

August 13, 2013, 13:10 
equationOfState  R

#12  
Senior Member
Join Date: Nov 2012
Location: Bavaria
Posts: 145
Rep Power: 5 
Hallo Olivier,
I am not clear about equationOfState models. What meanding has R? Quote:
Aylalisa 

August 22, 2013, 04:15 

#13 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 241
Rep Power: 9 
hello,
R is the specific gaz constant = R/M (M=molar mass). R is used to calculate the compressibility psi = 1/RT. For liquid, you still need to set compressibility and use the same law (you can guess this from the name "perfectLiquid"). But R is really bigger, to act as a very low compressible media. regards, olivier 

August 25, 2013, 11:30 
help

#14 
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 5 
hi
In compressible liquid/gas flows, the pEqn reads : ( fvm::ddt(psi,p)+fvc::div(phi)+fvm::div(phid,p,".." )fvm::laplacian(..,p) ) Can someone tell me what is the form of the differential equation? 

Tags 
compressibleinterfoam, eos, equation of state, multiphase 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Calculation of the Governing Equations  Mihail  CFX  7  September 7, 2014 06:27 
Solver for compressible NavierStokes equation  treima  OpenFOAM Running, Solving & CFD  3  May 30, 2012 05:25 
problem about adding another equation of state  yhaomin2007  OpenFOAM  4  May 16, 2012 04:36 
equation of state imbalance  Ramya  CDadapco  0  November 23, 2006 00:48 
equation of state imbalance(engine simulation)  hennie  CDadapco  1  July 4, 2002 03:21 