[juanltm]

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

[wsmith02]

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.

[olivierG]

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

[wsmith02]

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?

[olivierG]

Hello,

Yes, buoyantPimpleFoam already use hThoThermo. It's only buoyantSimpleFoam which should be changed.

About the question How ?:
just use in your thermoPhysicalProperties

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

[Oke'e]

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

[olivierG]

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

[Oke'e]

Thanks so very much Olivier, my work is up and running again.

Howard

[Nikunj.R]

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.

[fabian_roesler]

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

[Zeppo]

Originally Posted by fabian_roesler

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

[praveensrikanth91]

Originally Posted by fabian_roesler

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

Hey Fabian,

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