[uygar]

Hello everyone,

I am currently working on a laminar, time-dependent, compressible case with inlets, outlets, and solid regions that cool down over time. Even though I defined the objects as solids in the regionProperties file, OpenFOAM still asks for p_rgh and p files for the solid regions. From what I understand, pressure files shouldn’t be necessary for solids.

I even tried adding the files it asked for — it worked for the p file, but not for the p_rgh file.

What might I be missing?

[dlahaye]

Not sure.

How do you specify the thermodynamics on the solid domain?

[powabna]

Hey,
For what I know it should be working with only T for solids.. an here's a proof: link

Have you checked the log file for splitMeshRegions?
Maybe for some reason geometry haven't been splitted as you intended?


Edit: p for solids is needed if you model more mechanical cases (deformation, thermal expansion etc.)

[uygar]

Originally Posted by dlahaye

Not sure.

How do you specify the thermodynamics on the solid domain?

Thank you for your response,

I hope I didn't misunderstand. Here is my solid's thermoPhysicalProperties file:


thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

[uygar]

Originally Posted by powabna

Hey,
For what I know it should be working with only T for solids.. an here's a proof: link

Have you checked the log file for splitMeshRegions?
Maybe for some reason geometry haven't been splitted as you intended?


Edit: p for solids is needed if you model more mechanical cases (deformation, thermal expansion etc.)

Thank you for your response,

Yes, I think the problem is not about my mesh. Because when I run checkMesh -allTopology -allGeometry here is the response:

CellZone Cells Points Volume
fluid 128182 34535 498.82439
pat3 11587 2882 73.728
evap 20072 6861 3.0592566
pat5 10280 2668 73.728
pat6 10542 2715 73.728
pat4 10305 2673 73.728
pat1 11788 2914 73.728
pat2 11825 2923 73.728

I actually dont want my solids to expand or anything I only want them to cool down over time.

[dlahaye]

thermo looks fine. Do not have other clues immediately. Sorry.

[Lorenzo210]

Hi,


I think that heSolidThermo needs a "p" field for its member functions to be called.

In particular, I am referring to "calculate" in line 40 of the following:
https://www.openfoam.com/documentati...8C_source.html


So, I guess pressure is needed, but not necessarily used in the computations, and that's the reason why the pressure field needs to be defined in the 0 folder.


I looked at some tutorials in v2406 and all the solid regions I found have both T and p in the 0 folder.



I am not really aware of the calculations happening for what concerns the thermophysical properties... in order to be completely sure of what's happening, you might try to set different values/conditions for pressure in the solid and see if something changes!



Cheers,
Lorenzo

[dlahaye]

Correct.

The solver solves for sensible enthalpy in the solid domain. To recover temperature from enthalpy, a value for pressure including the boundary is required. Hence the need for 0/solid/p .

[uygar]

Originally Posted by Lorenzo210

Hi,


I think that heSolidThermo needs a "p" field for its member functions to be called.

In particular, I am referring to "calculate" in line 40 of the following:
https://www.openfoam.com/documentati...8C_source.html


So, I guess pressure is needed, but not necessarily used in the computations, and that's the reason why the pressure field needs to be defined in the 0 folder.


I looked at some tutorials in v2406 and all the solid regions I found have both T and p in the 0 folder.



I am not really aware of the calculations happening for what concerns the thermophysical properties... in order to be completely sure of what's happening, you might try to set different values/conditions for pressure in the solid and see if something changes!



Cheers,
Lorenzo

Thank you for your response,

I tried creating a file for p, but after that, it asked for a p_rgh file. I also created a file for that, but it still didn't work. I just keep getting this error:

--> FOAM FATAL ERROR: (openfoam-2212 patch=230612)

failed lookup of p_rgh (objectRegistry evap)
available objects of type volScalarField:

11
(
interRegionHeatTransferModel:htc
htcConst
thermo:mu
betavSolid
thermosi
h
p
T
AoV
thermo:rho
thermo:alpha
)



From const Type& Foam:bjectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
in file ./src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 571.

FOAM exiting

[Yann]

Hello,

Could you post the full log so we can see what is going on when you get this error?

Do you have any function objects in controlDict which might try to access p_rgh in the solids?

[uygar]

Originally Posted by Yann

Hello,

Could you post the full log so we can see what is going on when you get this error?

Do you have any function objects in controlDict which might try to access p_rgh in the solids?

Thank you for your response,

But I managed to solve the problem. Apparently, it was about the 0/fluid/p and p_rgh files. It was like this:

fluid_to_pat
{
type fixedValue;
value uniform 101325;
}

I changed it to type zeroGradient
and it proceeded.

[Yann]

Hello,

In a CHT case, you should have boundary conditions on p set to calculated, and use fixedFluxPressure rather than zeroGradient on walls for p_rgh.
(Have a look at the tutorials to see how boundary conditions are defined on p and p_rgh)

Cheers,
Yann