
[Sponsors] 
Introducing polynomial thermophysical properties 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 18, 2008, 11:47 
Im working with metal liquids

#1 
New Member
Juan LopezTerradas
Join Date: Mar 2009
Posts: 2
Rep Power: 0 
Im working with metal liquids and booyantsimpleFoam. The idea is simulate heat transfer with low Reynolds in low Peclet liquids.
Ive got the thermophysical properties of the liquid that i am using (density, viscosity, heat conductivity and cp) as a polynomial which does not fit with any thermophysical model, because all of them use the perfectGas model and so on. How can I introduce the polynomial model? Maybe with the NSRDS functions? But, how I use it with the OF? Maybe the question is a bit stupid but ive been working a lot on it and i dont find any solution. Im sure that there is an easy way to solve it. Thank you very much 

August 23, 2011, 12:43 
find an answer?

#2 
New Member
Walter
Join Date: Feb 2011
Posts: 8
Rep Power: 12 
Hi, I realize that this is an old thread, but did you ever find an answer to your question? I am struggling with this exact issue now.
Thanks, w. 

April 19, 2012, 11:28 

#3 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14 
hello,
I know this is an old thread, but if someone still doesn't succeed to use liquid polynomial properies with buoyantSimpleFoam / buoyantPimpleFoam, there is an easy way. For buoyantPimpleFoam, juste use the thermo type: thermoType hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>; For buoyantSimpleFoam, in the 2.0 and 2.1 version at least, you can't use hRhoThermo directely (hPsi used instead), so you just need to copy the solver to a new one like "rhoBuoyantSimpleFoam", and : * change name + modify Make/file * modify all call to basicPsiThermo to basicRhoThermo in createFields * modify the include in the new rhoBuoyantSimpleFoam, change #include basicPsiThermo.H by basicRhoThermo.H * compile the new solver: wclean & wmake * ... and now you can use icoPoly8ThermoPhysics with your new solver. regards, olivier 

May 18, 2012, 14:01 

#4 
New Member
Walter
Join Date: Feb 2011
Posts: 8
Rep Power: 12 
Thanks for the info Oliver.
It has been a while since I looked at this problem (dealing with other issues), but I will have to come back to it eventually. I am looking at buoyantPimpleFoam as you suggested. It looks like in 2.1.0 the calls already all reference basicRhoThermo and not basicPsiThermo, is that consistent with what you have? Does that mean with the stock buoyantPimpleFoam (2.1.0) I can use icoPoly? My next question then is... how? This is really my first venture into a heat transfer problem, and then again with variable props. What is the format for specifying : rho, mu, K, h, T, alpha as a poly function? is there a simple way to modify one of the Thermo classes so that these can be interpolated from a table of arbitrary size (such as h vs P) rather than a poly? 

May 21, 2012, 07:31 

#5 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14 
Hello,
Yes, buoyantPimpleFoam already use hThoThermo. It's only buoyantSimpleFoam which should be changed. About the question How ?: just use in your thermoPhysicalProperties Code:
thermoType hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>; mixture { specie { nMoles 1; molWeight 1; } equationOfState { rhoCoeffs<8> ( 2000 0 0 0 0 0 0 0); } thermodynamics { Hf 0; Sf 0; CpCoeffs<8> ( 1000 0 0 0 0 0 0 0); } transport { muCoeffs<8> (0.3 0.0008 0.0000007 0.0000000001 0 0 0 0); kappaCoeffs<8> ( 1 1e5 0 0 0 0 0 0); } } regards, olivier Last edited by olivierG; May 21, 2012 at 07:32. Reason: typo 

August 7, 2012, 11:03 

#6 
New Member
Howard NJOKU
Join Date: Nov 2010
Location: Nsukka, Nigeria
Posts: 9
Rep Power: 12 
Hi,
Pls I want to use 'hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>' under the 'bouyantPimpleFoam' solver but I am not sure where to obtain the coefficients to use in rhoCoeffs<8>, CpCoeffs<8>, muCoeffs<8> and kappaCoeffs<8> for water. If I use zeros as in your example, wont that amount to constant properties? That's what I am trying very hard to avoid. Any assistance will be very well appreciated. Oke'e 

August 8, 2012, 03:13 

#7 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14 
hello,
The coefficients hoCoeffs<8>, CpCoeffs<8>, muCoeffs<8, ... are polynome, with F= a0 + a1*T + a2*T^2 + ... so you just need to set your polynomial function. In my previous exemple, all coefficients where constant, but it is up to you to set your fluid properties. regards, olivier 

August 28, 2012, 07:55 

#8 
New Member
Howard NJOKU
Join Date: Nov 2010
Location: Nsukka, Nigeria
Posts: 9
Rep Power: 12 
Thanks so very much Olivier, my work is up and running again.
Howard 

November 2, 2012, 10:59 

#9 
Member
Nikunj Raithatha
Join Date: Jul 2012
Location: Washington DC
Posts: 47
Rep Power: 10 
Hello!
I am following these steps and not getting any error when the properties are constant (entering just A0) for all the properties. However, when i set a linear dependence for rho (by enetering A0 and A1), the solution fails to converge. Can anyone point the possible issue with this? Thanks! Nikunj. 

May 4, 2013, 07:44 
inletOutlet or atmosphere BC for U and p_rgh fields

#10 
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 213
Rep Power: 15 
Hi
This thread has grown old again but your problem could be your boundary conditions. With temperature depending density your solver case needs an inletOutlet or atmosphere BC for U and p_rgh fields. Otherwise continuity cannot be conserved. Regards Fabian 

May 4, 2013, 10:44 

#11  
Senior Member
Sergei
Join Date: Dec 2009
Posts: 255
Rep Power: 18 
Quote:


September 22, 2016, 12:54 

#12  
New Member
Praveen Srikanth
Join Date: Jul 2012
Location: West Lafayette, IN
Posts: 23
Rep Power: 10 
Quote:
This is quite an old post but I am running into similar issues with convergence in chtMultiRegionFoam with the icoPolynomial EOS model. I do have a closed liquid domain with no inlet or outlet boundaries. Is there a way to deal with such domains to account for property variations? Thank you so much Praveen 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to use thermophysical data  lasb  OpenFOAM Running, Solving & CFD  1  September 23, 2010 09:36 
Problem with the thermophysical  ivanyao  OpenFOAM Running, Solving & CFD  1  July 14, 2009 09:45 
How to implement thermophysical properties in a solver  dominik_christ  OpenFOAM Running, Solving & CFD  0  June 17, 2008 11:29 
Thermophysical properties in a cylinder  guilherme  OpenFOAM Running, Solving & CFD  1  December 3, 2006 08:37 
thermophysical properties of ham  Alex Ivancic  Main CFD Forum  1  November 5, 1998 11:09 