[cbarring]

Hello.
I am trying to model a water-like liquid as one of the phases in compressibleInterFoam. The equation of state for this liquid would be altered due to impurities. The adiabaticPerfectFluid model would do the job. I put the adiabaticPerfectFluid model code in the thermophysicalProperties.water file. Under OF7, everything works.

When I do exactly the same thing in OF8 and 9 I get:
_____________________________________________

--> FOAM FATAL ERROR:

lookup of thermophysicalProperties.water from objectRegistry region0 successful
but it is not a heRhoThermo<pureMixture<liquid,sensibleInternalEne rgy>>, it is a heRhoThermo<pureMixture<const<eConst<adiabaticPerf ectFluid<specie>>,sensibleInternalEnergy>>>

From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::species::thermo<Foam::ther mophysicalPropertiesSelector<Foam::liquidPropertie s>, Foam::sensibleInternalEnergy> > >]
in file /home/ubuntu/OpenFOAM/OpenFOAM-8/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 178.

FOAM aborting

------------------------------------------------------------------------

It is possible that my implementation adiabaticPerfectFluid is wrong. So I tried using the water properties from Dr. Holzmann's Blog (https://holzmann-cfd.com/community/b...operties-water). Putting this code in thermophysicalProperties.water worked in OF7 but not in OF8. The OF8 error message was:
_____________________________________________

--> FOAM FATAL ERROR:

lookup of thermophysicalProperties.water from objectRegistry region0 successful
but it is not a heRhoThermo<pureMixture<liquid,sensibleInternalEne rgy>>, it is a heRhoThermo<pureMixture<polynomial<hPolynomial<ico Polynomial<specie>>,sensibleEnthalpy>>>

From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::species::thermo<Foam::ther mophysicalPropertiesSelector<Foam::liquidPropertie s>, Foam::sensibleInternalEnergy> > >]
in file /home/ubuntu/OpenFOAM/OpenFOAM-8/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 178.

FOAM aborting

------------------------------------------------------------------------

I suspect that the problem is that the OF8 and 9 versions of compressibleInterFoam require that the mixture in the domain must include a liquid and a gas. This makes sense for VOF to work. However, the choices available for "liquid" are limited to the following fluids (using the Banana Method): Ar, C10H22, .... , CH4N2O, H2O, IC8H18, .... , nC3H8O.

So, to force a new equation of state onto water, I think that I need to customize the H2O file (/opt/openfoam8/src/thermophysicalModels/thermophysicalProperties/liquidProperties/H2O). I would not customize the H2O files that reside in the opt directory. I would customize a copy of this file (on in my home directory) and recompile etc. But this would be a significant effort.

Or, I could just stick with OF7.

Am I missing something here? Does anybody have any ideas on what I can do to easily get OF8 or 9 to work in this situation?

Regards

[cbarring]

Hi. This is an update to this post.

After a lot of trial and error, I found that these fatal errors are result of the following code in the thermophysicalProperties file with relates to the surface tension:
sigma
{
type liquidProperties;
phase water;
}

The fatal error does not occur if I replace the above code with:
sigma 0.07;

The modified thermophysicalProperties file is then exactly the same as the corresponding file for the depthCharge3D tutorial.

So, I think that if one wants to use the liquid model in compressibleInterFoam simulations, one should use:
sigma
{
type liquidProperties;
phase water;
}

For other equations of state, one should use "sigma 0.07; // water". If the fluid is not water, a different value of sigma would be required.

Regards