[mwaqas]

Hello Everyone,

In chtMultiRegionFoam, I want to calculate heat transfer coefficient. OpenFOAM has introduced "wallHeatTransferCoeff" function object in OF6 to calculate heat transfer coefficient directly. Here is the link

https://github.com/OpenFOAM/OpenFOAM...ransferCoeff.H

I am trying to test this function. Hence, I have only included following function in controlDict to calculate the wall heat transfer coefficient.

functions
{
wallHeatTransferCoeff1
{
type wallHeatTransferCoeff;
libs ("libfieldFunctionObjects.so");
region bottomWater;
rho 1.225;
Cp 1005;
Prl 0.707;
Prt 0.9;
}
}

But I am getting following error

[0] --> FOAM FATAL ERROR:
[0] Unable to find incompressible turbulence model in the database[1]
[1]
[1] --> FOAM FATAL ERROR:
[1] Unable to find incompressible turbulence model in the database
[1]
[1] From function virtual bool Foam::functionObjects::wallHeatTransferCoeff::exec ute()
[1] in file wallHeatTransferCoeff/wallHeatTransferCoeff.C at line 227.

It seems like wallHeatTransferCoeff has not been for chtMultiRegionFoam, but realease note of OF6 specially mentions that it could be used to calculate heat transfer coefficient in multi-regio simulation.

https://openfoam.org/release/6/

Did anyone try this function? Am I missing something or making a mistake?
I took OF6 multiRegionHeater tutorial, I didn't change anything in tutorial at all

Thank you

Regards

[Bloerb]

This was made for incompressible solvers. Hence your error message. While chtMultiRegion can calculate incompressible flow it is still a compressible solver (which allows the user to set a constant density). If you follow the link you gave to the commit you can read

wallHeatTransferCoeff: New functionObject to calculate the wall heat …

…transfer coefficient

for incompressible flow simulated using simpleFoam, pimpleFoam or pisoFoam.

Now these solvers can be used with a -region option, but are not conjugate solvers.

This function object calculates this in the following fashion:

            wallHeatTransferCoeffBf[patchi] =
                rho_*Cp_*(nuBf[patchi]/Prl_ + nutBf[patchi]/Prt_);

It should be easy to calculate this in ParaView or via your own (coded) function object for compressible flow

[mwaqas]

Hi Bloerb,

Thank you for your reply.

wallHeatTransferCoeff: New functionObject to calculate the wall heat transfer coefficientfor incompressible flow

You are absolutely right, it is mentioned over there that it is for incompressible flow but I couldn't find that it is only for flow using using simple. pimple or pisoFoam.
What I could find is:

Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ];

It is meant for multiRegion (off course incompressible) and as per my understanding from this link, there is only one solver for multiregion in OF-6 i.e. chtMulriRegionFoam (they have combined both chtMulriRegionSimpleFoam and chtMulriRegionFoam in one solver i.e chtMulriRegionFoam) and chtMulriRegionFoam is by default for compressible fluid.

Solvers: chtMultiRegionFoam conjugate heat transfer (CHT) solver runs both steady-state and transient solutions (deprecating chtMultiRegionSimpleFoam) [ commit 283f8b ]; added option for reactions and combustion to chtMultiRegionFoam [ commit 7c237a ].

Then how could we use wallHeatTransferCoeff for multi-region?

Regards

[Bloerb]

As I said, you can't use it with this solver without programming your own utility

[gian93]

Originally Posted by Bloerb

This was made for incompressible solvers. Hence your error message. While chtMultiRegion can calculate incompressible flow it is still a compressible solver (which allows the user to set a constant density). If you follow the link you gave to the commit you can read

wallHeatTransferCoeff: New functionObject to calculate the wall heat …

…transfer coefficient

for incompressible flow simulated using simpleFoam, pimpleFoam or pisoFoam.

Now these solvers can be used with a -region option, but are not conjugate solvers.

This function object calculates this in the following fashion:

            wallHeatTransferCoeffBf[patchi] =
                rho_*Cp_*(nuBf[patchi]/Prl_ + nutBf[patchi]/Prt_);

It should be easy to calculate this in ParaView or via your own (coded) function object for compressible flow

Could someone explain the formula used for heat transfer coefficient mentioned above? I want to use it for an incompressioble simulation with water trough pipes . Water is at 100C and the solver used is simpleFoam. I want to visualize the "virtual" heat transfer coefficient at walls . I think that I have set correctly the function object in the controlDict :

wallHeatTransferCoeff1
    {
        type        wallHeatTransferCoeff;
        libs        ("libfieldFunctionObjects.so");
        //region      fluid;
        //patches     (".*Wall");
        rho         997;
        Cp          4215.7;
        Prl         1.64;
        Prt         0.9;
    }

the problem is that paraFoam shows me very small heat transfer coefficient... (it should be on the order of 3*10^4 but mine are on the order of 5*10^0)..

what I have missed? thanks