[fnohpat]

I am solving a classic heat transfer problem in the ceiling wall, considering heat conduction and heat loss through convection. For simplicity, I am using a one-dimensional model. I have employed the solvers "laplacianFoam" and "chtMultiregionFoam." Both the upper and lower surfaces experience heat transfer through convection.

Inside the wall, there is a fixed ambient temperature and a constant coefficient "h" for convection. On the outer surface, the external air temperature and "h" (depending on wind speed) are measured every 10 minutes. The boundary condition on the external surface, using the "codedMixed" type, is as follows:

{
type codedMixed;

refValue uniform 0;
refGradient uniform 0;
valueFraction uniform 1;
value $internalField;
name robin; // name of generated BC

code
#{
scalar Tinf = 293; // ambient temperature (k)
scalar hc = 12; // heat transfer coefficient (w/m^2k)
scalar k = 1.5; // thermal conductivity (w/mk)

forAll((*this), i)
{
scalar delta =this->patch().deltaCoeffs()[i];
this->refValue() = Tinf;
this->valueFraction() = 1.0/(1+k*delta/hc);
}
#};


}


Could someone please advise me on how to conduct a simulation for an entire day? The ambient temperature and "h" values need to be read every 600 seconds from a CSV table in the format "Time, Tinf, hc". Due to the small simulation time step, linear interpolation of values for intermediate times is necessary.

Thank you in advance for your assistance.

Best regards, Felipe Noh.

[LongGe]

Hello Noh

How about using the Function1 class?

The following is a simple usage of Function 1.

1. test-code using OpenFOAM-v2306 via OpenCFD

#include "argList.H"
#include "IOstreams.H"
#include "Function1.H"
#include "IOdictionary.H"

using namespace Foam;

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
argList::noParallel();

const word dictName("yourDict"); <- NOTEs::yourDict" must always be "function1Properties".

#include "setRootCase.H"
#include "createTime.H"
#include "setConstantRunTimeDictionaryIO.H"

#if (OPENFOAM > 2212)
dictionary propsDict(IOdictionary::readContents(dictIO));
#else
dictionary propsDict(static_cast<dictionary&&>(IOdictionary(d ictIO)));
#endif

auto Ta = Function1<scalar>::New("Ta", propsDict);
Ta().writeData(Info);

auto ha = Function1<scalar>::New("ha", propsDict);
ha().writeData(Info);

//for time = 10
Info << "Ta(10)=" << Ta().value(10) << endl;
Info << "ha(10)=" << ha().value(10) << endl;

return 0;
}

2. input tables
2-a yourDict in constant/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object function1Properties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Ta
{
type table;
file "<constant>/your-Ta";
}

ha
{
type table;
file "<constant>/your-ha";
}

// ************************************************** *********************** //

2-b your-Ta in constant
// time[sec] Ta[K]
(
(0 273.15)
(60 283.15)
(120 293.15)
);

// ************************************************** *********************** //

2-c your-ha in constant
// time[sec] ha[W/m2/K]
(
(0 15)
(60 16)
(120 17)
);

// ************************************************** *********************** //


3. Execution Result for this test-code
$ Test-code
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2306 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v2306 OPENFOAM=2306 version=v2306
Arch : "LSB;label=32;scalar=64"
Exec : Test-code
Date : Aug 17 2023
Time : 13:29:14
Host : gauss
PID : 5783
I/O : uncollated
Case :
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Ta table;
TaCoeffs
{
file "<constant>/your-Ta";
}
ha table;
haCoeffs
{
file "<constant>/your-ha";
}
Ta(10)=274.817
ha(10)=15.1667

[fnohpat]

Dear Tatsuya Shimizu

Thank you for your prompt response.

On the other hand, I am new to OpenFOAM and don't have experience with programming. I am using OpenFOAM 9. Should I include the code you suggest within the codedMixed code in my boundart condition?

Thank you in advance for your assistance.

[LongGe]

Hello Noh

For inputs where the physical quantity is time-varying, it is best implemented using the Function1 class. Also, Function1 can easily read an external Table, which would match your application.

[olesen]

Originally Posted by fnohpat

Dear Tatsuya Shimizu

Thank you for your prompt response.

On the other hand, I am new to OpenFOAM and don't have experience with programming. I am using OpenFOAM 9. Should I include the code you suggest within the codedMixed code in my boundart condition?

Thank you in advance for your assistance.

The advice is to leverage existing boundary condition types whenever possible and avoid doing coding. The Function1 and PatchFunction1 provide a fairly general way to hook in different types of input (table, function, code, expressions, ...) and are supported by a number of different regular boundary conditions. You might, for example, start with an "externalWallHeatFluxTemperature" boundary condition and then specify "Ta" and "h" as different types of Function1 or PatchFunction1.