wallHeatTransferCoeff + simpleFOAM ( OpenFoam7)

gian93 · September 21, 2020, 05:15

Hi All,
I think open a specific topic is more appropiate.
I want to calculate the heat transfer coefficient (called "virtual htc" as in star ccm +) after a steady state incompressible solver (simpleFoam). The simulation is about water in a cooling pipe.
I don't need energy equation so i decided to use simpleFoam. Infact the flow is steady and the cooling medium is water...
I have verified that wallHeatTransferCoeff function object is available for simpleFoam in openFOAM7.

This is the formula used in wallHeatTransferCoeff.C to calculate the heat transfer coefficient

PHP Code:


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

I have specified this in my controlDict

PHP Code:


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

No errors occours, neither warnings during the simulation..I use KEpsilon model for turbulence, inlet mass flow rate and fixed value for pressure at outlet. Flow velocity is about 3 m/s
Why when I visualize the results in paraview about the wallHeatTransferCoeff I obtain value from 1*10^0 to 6*10^0 and not in the order of 10^4 ?? they seems not to be in w/m^2k ...

Krapf · September 21, 2020, 08:10

Never used it myself, but I think the unit is W/(m*K).

wallHeatTransferCoeff.C

Code:

tmp<volScalarField> twallHeatTransferCoeff
(
    volScalarField::New
    (
        type(),
        mesh_,
        dimensionedScalar
        (
            dimMass/pow3(dimTime)/(dimTemperature/dimLength),
            0
        )
    )
);

$\mathrm{\frac{\frac{kg}{s^3}}{\frac{K}{m}} = \frac{kg}{s^3} \cdot \frac{m}{K} = \frac{kg \cdot m}{s^3 \cdot K} \cdot \frac{m}{m} = \frac{kg \cdot m^2}{s^3 \cdot K \cdot m} = \frac{W}{m \cdot K}}$

gian93 · September 21, 2020, 10:06

yes .. but why I obtain such different results between star CCM + and openfoam? Velocity and pressure gradient is failry the same in the two simulation!

Krapf · September 21, 2020, 17:03

Is the heat transfer coefficient in STAR-CCM+ calculated using the same or a similar equation? Or is it given there in W/(m^2*K)?

gian93 · September 22, 2020, 06:08

you are right... I did not notice that.. so stupid.
Star CCM + reports value in W/m^2K while openFOAM in W/mk
also formulations are quite different.

beside this, I'm much more confused because I' m not familiar with openFOAM local heat transfer formulation..
anyone has developed his localHTC post process utility similar to the Star ccm + one?

Krapf · September 23, 2020, 05:05

Take a look here: Heat Transfer Coefficients from WallHeatFlux
Does this help you?

EDIT: Probably not, because due to simpleFoam you don't have a wall temperature.

gian93 · September 23, 2020, 08:56

Quote:

Originally Posted by Krapf

Take a look here: Heat Transfer Coefficients from WallHeatFlux
Does this help you?

EDIT: Probably not, because due to simpleFoam you don't have a wall temperature.

exactly..simpleFoam does not solve energy.

I have to implement a different local hct calculation similar to the one of star ccm+..

September 21, 2020, 05:15	wallHeatTransferCoeff + simpleFOAM ( OpenFoam7)	#1
gian93 Member giovanni Join Date: Sep 2017 Posts: 50 Rep Power: 8	Hi All, I think open a specific topic is more appropiate. I want to calculate the heat transfer coefficient (called "virtual htc" as in star ccm +) after a steady state incompressible solver (simpleFoam). The simulation is about water in a cooling pipe. I don't need energy equation so i decided to use simpleFoam. Infact the flow is steady and the cooling medium is water... I have verified that wallHeatTransferCoeff function object is available for simpleFoam in openFOAM7. This is the formula used in wallHeatTransferCoeff.C to calculate the heat transfer coefficient PHP Code: `wallHeatTransferCoeffBf[patchi] = rho_Cp_(nuBf[patchi]/Prl_ + nutBf[patchi]/Prt_);` I have specified this in my controlDict PHP Code: `wallHeatTransferCoeff1 { type wallHeatTransferCoeff; libs ("libfieldFunctionObjects.so"); //region fluid; //patches (".Wall"); //default is all walls rho 997; Cp 4215.7; Prl 1.64; Prt 0.9; }` No errors occours, neither warnings during the simulation..I use KEpsilon model for turbulence, inlet mass flow rate and fixed value for pressure at outlet. Flow velocity is about 3 m/s Why when I visualize the results in paraview about the wallHeatTransferCoeff I obtain value from 110^0 to 6*10^0 and not in the order of 10^4 ?? they seems not to be in w/m^2k ...

September 21, 2020, 08:10		#2
Krapf Senior Member Join Date: Oct 2017 Posts: 121 Rep Power: 8	Never used it myself, but I think the unit is W/(mK). wallHeatTransferCoeff.C Code: tmp<volScalarField> twallHeatTransferCoeff ( volScalarField::New ( type(), mesh_, dimensionedScalar ( dimMass/pow3(dimTime)/(dimTemperature/dimLength), 0 ) ) ); $\mathrm{\frac{\frac{kg}{s^3}}{\frac{K}{m}} = \frac{kg}{s^3} \cdot \frac{m}{K} = \frac{kg \cdot m}{s^3 \cdot K} \cdot \frac{m}{m} = \frac{kg \cdot m^2}{s^3 \cdot K \cdot m} = \frac{W}{m \cdot K}}$ Last edited by Krapf; September 21, 2020 at 17:05.*

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
simpleFoam tutorial PitzDaily using Reynolds stress tensor (LRR RASModel)	dlahaye	OpenFOAM Running, Solving & CFD	24	August 4, 2023 14:29
interFoam vs. simpleFoam channel flow comparison	DanM	OpenFOAM Running, Solving & CFD	12	January 31, 2020 15:26
simpleFoam parallel solver & Fluent polyhedral mesh	Zlatko	OpenFOAM Running, Solving & CFD	3	September 26, 2014 06:53
Laminar simpleFoam and inviscid simpleFoam	herenger	OpenFOAM Running, Solving & CFD	7	July 11, 2013 06:27
Trying to run a benchmark case with simpleFoam	spsb	OpenFOAM	3	February 24, 2012 09:07

September 21, 2020, 10:06		#3
gian93 Member giovanni Join Date: Sep 2017 Posts: 50 Rep Power: 8	yes .. but why I obtain such different results between star CCM + and openfoam? Velocity and pressure gradient is failry the same in the two simulation!

September 21, 2020, 17:03		#4
Krapf Senior Member Join Date: Oct 2017 Posts: 121 Rep Power: 8	Is the heat transfer coefficient in STAR-CCM+ calculated using the same or a similar equation? Or is it given there in W/(m^2*K)?

September 22, 2020, 06:08		#5
gian93 Member giovanni Join Date: Sep 2017 Posts: 50 Rep Power: 8	you are right... I did not notice that.. so stupid. Star CCM + reports value in W/m^2K while openFOAM in W/mk also formulations are quite different. beside this, I'm much more confused because I' m not familiar with openFOAM local heat transfer formulation.. anyone has developed his localHTC post process utility similar to the Star ccm + one?

September 23, 2020, 05:05		#6
Krapf Senior Member Join Date: Oct 2017 Posts: 121 Rep Power: 8	Take a look here: Heat Transfer Coefficients from WallHeatFlux Does this help you? EDIT: Probably not, because due to simpleFoam you don't have a wall temperature.