[mwaqas]

Hello Everyone,


I am using OF50 for 2D steady state conjugate heat transfer problem (using chtMultiregionSimpleFoam) with heat source. I have 84 disconnected solid region (blue part in image) and fluid passing across solid regions (green part). I have used following fvOptions file for heat source

energySource
{
type scalarSemiImplicitSource;
active true;
selectionMode all;
scalarSemiImplicitSourceCoeffs
{
volumeMode specific;//
selectionMode all;
injectionRateSuSp
{
h (89878 0); // q in [W]; or in [W/m³] if you use specific mode (90570 0)
}
}
}

I have placed this fvOptions file in every system/solid.

The heat source is correct for my setup because same heat source has been used in Ansys and giving physical results.
In my case (OpenFOAM), I used 298K as initial temperature for both solid and fluid regions. Once I start simulation, the temperature keep on increasing for both sold and fluid region (I checked temperature rise up to 500K in 50000 iteration). I am unable to figure out my mistake. Could anyone please tell me the right direction to look for my mistake. I have attached my log file with it (due to size constraints I could not attach my complete log file).





Moreover, I have used same simulation setup for transient case with initial temperature of solid 333K and it was fine with results comparable with ansys as well as experiments.


PS: Unfortunately, I cannot share my entire case here


Regards

[pete20r2]

1.5W each cell shouldn't make temperatures like that!
Can you share fvSchemes and fvSolution for solid and fluid region?
Which version are you on? v1712 introduced sub-looping which is worth checking out.
v1712 Improvements

[mwaqas]

Thank you for your reply. I am using OFv5.0. I didn't try v1712. Here is my fvScheme, fvSolution and thermophysical properties for both fluid and solids. Exactly, this heat should not increase that much temperature.


As I mentioned in my above post, the same heat source with same fluid velocity and physical data has been used in Ansys and results are physical (max temp rise was 303k from 298).
Moreover I did transient simulation using the exactly same physical properties and fluid velocity but that was without heat source (only initial temp of 333k of solid regions).


Regards

[mwaqas]

here is the fvscheme and fvSolution for fluid region. In previous post were for solid regions

[Bloerb]

Your set up seems logical. I would probably remove or reduce the relaxation from the solid domains, since it slows things down, but you are currently adding 89878 W/m³. This a 2D Simulation. Have you thought about the depth of your case? Is that included correctly in that ?

[mwaqas]

Hello Bloreb,


Thank you for your reply. As it is a 2D simulation and top and bottom part have empty patch type. I don't think so the depth will matter (as far as your question, I didn't change depth of my domain). Actually, I had started with 0.6 relaxation factor but it was too slow to converge but still there was continuous increase in temperature.


I was playing around with different parameters, I have noticed one strange thing. I used following function in controlDict to check the density of my fluid (liquid).

functions
{
inletFlux
{
type surfaceFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
log true;
writeFields false;
regionType patch;
region fluid;
name fluid_to_inlet1;
operation average;
fields
( rho );
}

I am using equationofState rhoConst and in this case one has to define density specifically at the end of thermoPhysicalProperties. In my case I have defined density 1660 but the above function always give average value of 2 for rho.

Then I checked for OpenFOAM tutorial where above function calculates air density as 1.18 (Mean above controlDict function is working correctly). But no matter what value of rho I use in my case, it always calculate rho =2.

[pete20r2]

give this a whirl:

in fvOptions:

limitT{
	type	limitTemperature;
	active	yes;

	limitTemperatureCoeffs
	{
		selectionMode	all;
		min		5;
		max		1000;
	}
}

in fvSolution:

solvers
{
    h
    {
        solver          PCG
        preconditioner  DIC;
        tolerance       1e-9;
        relTol          0;
    }
}

relaxationFactors
{
    fields
    {

    }
    equations
    {
        h               1;
    }
}

If this goes nuts, try chucking the limitT fvOption on the fluid too.
You may also need to lower UR of h to .9999 for initial steps, it's very sensitive.

Once you have this running I'd suggest you look again at the accuracy you want. I suspect over your operating range hydro-fluoro ethers will exhibit substantial enough changes in thermophysical properties that it would be worth implementing some of the more advanced equations of state.

I nearly forgot, try using the frozenFlow switch once your fluid field is converged. Since your fluid properties are not dependent on T field at this stage you can solve for T field alone with converged fluid field.
Throw this is the fvSolution for the fluid:

SIMPLE
{
    momentumPredictor yes;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       100000;
    rhoMin          0.2;
    rhoMax          2;
    frozenFlow		true;
}

This is not runtime modifiable as far as I know so you'll have to stop the run, change the switch and continue. It will now only solve for h.

How are you managing 84 solid regions?? I hope you have the folders symlinked!

[pete20r2]

Originally Posted by mwaqas

Then I checked for OpenFOAM tutorial where above function calculates air density as 1.18 (Mean above controlDict function is working correctly). But no matter what value of rho I use in my case, it always calculate rho =2.

You have rhoMax and rhoMin set in fvSolution, you can either make them both the same value as the one given in thermoPhysicalProperties or remove them.

[mwaqas]

Thank you so much Peter for your help. You are life saver for me . I didn't noticed that there is a limit on density in fvSolution. I didn't try yet but I am pretty much sure that the problem was with my value of rho. Because I have checked the value of rho in my transient solition and there it is using correct value of it. I will remove limits on rho and update about my result.