CFD Online Discussion Forums - Error in turbulentHeatFluxTemperatureFvPatchScalarField v1.6

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Error in turbulentHeatFluxTemperatureFvPatchScalarField v1.6 (https://www.cfd-online.com/Forums/openfoam-solving/68351-error-turbulentheatfluxtemperaturefvpatchscalarfield-v1-6-a.html)

Error in turbulentHeatFluxTemperatureFvPatchScalarField v1.6

I noticed an error in turbulentHeatFluxTemperatureFvPatchScalarField class for temperature gradient calculation:

Code:

00146 void turbulentHeatFluxTemperatureFvPatchScalarField::updateCoeffs()

00147 {

00148     if (updated())

00149     {

00150         return;

00151     }

00152 

00153     const scalarField& alphaEffp =

00154         patch().lookupPatchField<volScalarField, scalar>(alphaEffName_);

00155 

00156     const scalarField& Cpp =

00157         patch().lookupPatchField<volScalarField, scalar>(CpName_);

00158 

 00159     gradient() = q_/(Cpp*alphaEffp);

00160 

00161     fixedGradientFvPatchScalarField::updateCoeffs();

00162 }

From my point of view and based on Fourier's law heat flux q is calculated as:

q = lambda * grad (T) = alpha * rho * Cp * grad (T)

where
lambda - thermal conductivity
alpha - thermal diffusivity
Cp - cpecific heat capacity
rho - density

Thus temperature gradient should be

grad (T) = q / (alpha * rho * Cp)

Please correct me if I'm wrong!

Quote:

Originally Posted by makaveli_lcf (Post 229669)

I noticed an error in turbulentHeatFluxTemperatureFvPatchScalarField class for temperature gradient calculation:
...
Please correct me if I'm wrong!

Are you speaking of the class in the "compressible" or in the "incompressible" namespace?
They are formulated somewhat differently and the incompressible formulation will obviously not have rho in it.

Mark,
I'm speaking about incompressible namespace.
In any case, if not include density in heat flux calculations, left-hand and right-hand dimensions in that relationship will not meet! That is what I mean in details:

Code:

00053 class turbulentHeatFluxTemperatureFvPatchScalarField

00054 :

00055     public fixedGradientFvPatchScalarField

00056 {

00057 // Private data

00058 

00059     //- Heat flux [W/m2]

00060     scalarField q_;

00061 

00062     //- Name of effective thermal diffusivity field

00063     word alphaEffName_;

00064 

00065     //- Name of specific heat capacity field

00066     word CpName_;

00067

[q] = W / m^2 = (J / s) / m^2 = (kg m^2 / s^3) / m^2 = kg / s^3
[lambda] = W / (m K)= (kg m^2 / s^3) / (m K) = kg m / (K s^3)
[alpha = lambda / (rho Cp)] = m^2 / s
[Cp] = J / (kg K) = (kg m^2 / s^2 ) / (kg K) = m^2 / (K s^2)
[grad (T)] = K / m

Thus

q = lambda * grad (T) => [LHS] = W / m^2 equal to [RHS] = W / (m K) * K / m = W / m^2

But if we calculate grad (T) as q / (alpha Cp), then we get

grad (T) = q / (alpha Cp) => [LHS] = K / m not equal to! [RHS] = kg / s^3 / (m^2 / s * m^2 / (K s^2)) = kg K / m^4

So we see that dimensions of the left-hand side (LHS) and the right-hand side (RHS) do not meet unless other than traditional units are used for thermal conductivity, thermal diffusivity, specific heat capacity etc.

It is easy to check, that q = (alpha Cp rho ) grad (T) => grad (T) = q / (alpha Cp rho) gives correct result after dimensions analyzis.

Not sure in incompressible solvers. But in compressible solvers, alphaEff and alpha defined in OF are not the same as the alpha [m^2/s] that we typically refer to.

They actually have already included rho in the definition. Basically in OpenFOAM: alpha = lambda/Cp ( not lambda/Cp/rho)

You might want to check the thermoPhysicalModel to find it out.

Thank you, Yi!
Following your guidance I found in basicThermo_8H_source.html:

Code:

00077             //- Laminar thermal diffusuvity [kg/m/s]

00078             volScalarField alpha_;

That is why there was ambiguity.