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

Introducing polynomial thermophysical properties

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

Like Tree6Likes
  • 1 Post By juanltm
  • 4 Post By olivierG
  • 1 Post By olivierG

Reply
 
LinkBack Thread Tools Display Modes
Old   June 18, 2008, 11:47
Default Im working with metal liquids
  #1
New Member
 
Juan Lopez-Terradas
Join Date: Mar 2009
Posts: 2
Rep Power: 0
juanltm is on a distinguished road
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
mgg likes this.
juanltm is offline   Reply With Quote

Old   August 23, 2011, 12:43
Default find an answer?
  #2
New Member
 
Walter
Join Date: Feb 2011
Posts: 4
Rep Power: 6
wsmith02 is on a distinguished road
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.
wsmith02 is offline   Reply With Quote

Old   April 19, 2012, 11:28
Default
  #3
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
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
olivierG is offline   Reply With Quote

Old   May 18, 2012, 14:01
Default
  #4
New Member
 
Walter
Join Date: Feb 2011
Posts: 4
Rep Power: 6
wsmith02 is on a distinguished road
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?
wsmith02 is offline   Reply With Quote

Old   May 21, 2012, 07:31
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
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 1e-5 0 0 0 0 0 0);
    }
}
... and change value according to your properties.

regards,
olivier
fabian_roesler likes this.

Last edited by olivierG; May 21, 2012 at 07:32. Reason: typo
olivierG is offline   Reply With Quote

Old   August 7, 2012, 11:03
Default
  #6
New Member
 
Howard NJOKU
Join Date: Nov 2010
Location: Nsukka, Nigeria
Posts: 9
Rep Power: 6
Oke'e is on a distinguished road
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
Oke'e is offline   Reply With Quote

Old   August 8, 2012, 03:13
Default
  #7
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
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
olivierG is offline   Reply With Quote

Old   August 28, 2012, 07:55
Default
  #8
New Member
 
Howard NJOKU
Join Date: Nov 2010
Location: Nsukka, Nigeria
Posts: 9
Rep Power: 6
Oke'e is on a distinguished road
Thanks so very much Olivier, my work is up and running again.

Howard
Oke'e is offline   Reply With Quote

Old   November 2, 2012, 11:59
Default
  #9
Member
 
Nikunj Raithatha
Join Date: Jul 2012
Location: Washington DC
Posts: 47
Rep Power: 4
Nikunj.R is on a distinguished road
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.
Nikunj.R is offline   Reply With Quote

Old   May 4, 2013, 07:44
Default inletOutlet or atmosphere BC for U and p_rgh fields
  #10
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 154
Rep Power: 8
fabian_roesler is on a distinguished road
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
fabian_roesler is offline   Reply With Quote

Old   May 4, 2013, 10:44
Default
  #11
Member
 
Join Date: Dec 2009
Posts: 40
Rep Power: 7
Zeppo is on a distinguished road
Quote:
Originally Posted by fabian_roesler View Post
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.
http://eprints.usq.edu.au/1806/1/suslov.pdf
Zeppo is offline   Reply With Quote

Reply

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
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 09:37
thermophysical properties of ham Alex Ivancic Main CFD Forum 1 November 5, 1998 12:09


All times are GMT -4. The time now is 05:15.