[jcoelho5]

Hi,

I am trying to validate the wallHeatTransfCoeff utility in OpenFOAM v9, using rhoPimpleFoam for a forced convection.

My case is a cylindrical pipe with 20mm diameter, 250mm long (to achive L/d > 10).

The fluid used is defined by constant rho, transport properties and cp (it is supposed to simulate Liquid oxygen @74 bar and with T=102K). Here goes the thermophysical properties given as input;

thermoType
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleInternalEnergy;
}

mixture
{
    specie
    {
        molWeight   32;
    }
    
    thermodynamics
    {
        Cp         	1686;
        Cv	    	877;
        Hf             0;
    }
    transport
    {
        mu          160e-06;
        Pr           1.91;
    }
    
    equationOfState
    {
    	rho		1103;
    }
}

The boundary conditions are the following:

U
inlet - volumetricFlowRate (with equivalent value for 7kg/s)
outlet - zeroGradient
wall - zeroGradient

p
inlet - zeroGradient
outlet - fixedValue - 74bar
wall - zeroGradient

T
inlet - fixed Value - 102 K
outlet - zeroGradient
wall - fixed Value - 200 K

k
inlet - turbulentIntensityKineticEnergyInlet (intensity 0.05)
outlet - zeroGradient
wall - kqRWallFunction

epsilon
inlet - turbulentMixingLengthDissipationRateInlet (mixing length 0.005)
outlet - zeroGradient
wall - epsilonWallFunction

nut
inlet - calculated
outlet - calculated
wall - nutkWallFunction

alphat
inlet - calculated
outlet - calculated
wall - compressible::alphatWallFunction

omega
inlet - zeroGradient
outlet - zeroGradient
wall - omegaWallFunction

I tried as turbulence models kEpsilon and kOmega.

Regarding the utility, I added the following to the controlDict

h_coef
    {
        type        wallHeatTransferCoeff;
        libs        ("libfieldFunctionObjects.so");
        model		kappaEff;
        //...
        patches     (".*Wall");
        rho         1103;
        Cp          1686;
        Pr          1.91;
        Prt         0.85;
        executeControl     	timeStep;
        writeControl        writeTime;
    }

and used the kappaEff model since the alternative (ReynoldsAnalogy) is not adequate for liquids.
kappaEff is computed as follow
htc = rho * Cp ( nu/Pr + nu_t/Pr_t)

• htc - heat transf coeff [W/m2/K]
• nu - viscosity
• nu_t - turbulent viscosity
• Pr - fluid laminar Prandtl - input
• Pr_t - fluid turbulent Prandtl "From experimental data, Prt has an average value of 0.85, but ranges from 0.7 to 0.9 depending on the Prandtl number of the fluid in question" - wikipedia

Being so, I have achieved some results that are out of the order of magnitude of the Dittus-Boelter equation (valid for L/D>10, for Re>10000, which is the case). I also tried an approach using the Calculator in paraview, where I use the result output wallHeatFlux (also addded in the controlDict but out of the scope for this post) and divide by the difference of the wall (which is given as input in the boundary condition) and bulk temperatures (which can be approximated to the inlet temperature): h=q / (T_wall - T_bulk)

• OpenFOAM wallHeatTransfCoeff - 10-20 W/m2/K
• Dittus Boelter - ~ 30000 W/m2/K
• OpenFOAM paraview calculator - ~20000 W/m2/K

Why does the option using the simulation wall heat flux differ so much from the automatic computation of the heat transfer coefficient?

Does anyone understand what might be the problem? Has anyone successfully used (and possibly validate) this wallHeatTransfCoeff utility?

[Hr_kules]

Hey, i have a pretty similar problem right now, if not the same. So far i also found that the wallHeatTransferCoefficient is way too inaccurate. I unfortunately have no idea to resolve this. I would stick to manually compute the heat transfer coefficient, since your results at least are of similar magnitude of the results given by the dittus boelter equation.

However may i ask you if you ever had problems with the wall temperatures? In my simulation the temperature difference given by t_wall-t_bulk is way to low to even come close to the temperature difference i can calculate backwards from the dittus boelter equation. However and the temperature difference between in and outlet is correct with regards to the heat given by Q = mdot*cp*(t_outlet - t_inlet).

In conclusion the convection modelling in OpenFoam is quite strange. And the wallHeatTransferCoeffcient also. Did you ever resolve your issue?

[jcoelho5]

No, unfortunately I haven't solve this problem.
Regarding the wall temperature, I forced it to be the 200K specifically for it to have a "significant" temperature difference with the bulk. It was just a (failed) validation case.

[Hr_kules]

Hi, just as a follow up. I solved the problem by switching to k-omega SST for my simulation my results now match dittus boelter, that i used as a reference. The HTC calculation of openFoam still proved to be wrong, however i was able to achieve 1% difference to dittus boelter with just better wall treatment from a k-omega model.

[jcoelho5]

Originally Posted by Hr_kules

Hi, just as a follow up. I solved the problem by switching to k-omega SST for my simulation my results now match dittus boelter, that i used as a reference. The HTC calculation of openFoam still proved to be wrong, however i was able to achieve 1% difference to dittus boelter with just better wall treatment from a k-omega model.

So, the 1% were achieved by the manual computation of q / deltaT? the direct coefficient given by OF is still wrong, right?

[Hr_kules]

Yes, it was done manually. The functionObject still prints out a plain wrong value. Either way i have a better gut feeling regarding the manual computation, since I at least know what is happening there.

Have you made any progress?

[jcoelho5]

Ok, good enough!

No, no progress. Not only I had to focus on other things, but also I did not know what else to do...

Thanks anyways for you input. Still helpful

[Hr_kules]

By the way: I also added an entrance area to the pipe based on correlation that uses the reynolds number (l_entrance = 1.359*Diameter*Re^0.25) and after that a portion that matches L/D = 10. Your case sounds pretty much like mine and the temperature evolution along the pipe wall differs quite much between the entrance and the developed region.

Hope you can solve your problem soon!