[npatricia]

Hello all,

I am having trouble with adding a heat source to my model using fvOptions.
I am trying to model heat transfer in a solar pond, my main source of energy being the sun, which i need to add as a source term in my OpenFoam model.

I am abit confused on how to enable the fvoptions file in my system folder. I am using buoyantBoussinesqSimpleFoam, OpenFoam 5.0.

Thank you for your help
PATRICIA

[omdemircan]

Hi,

Simply placing the fvOptions file in the /system directory was sufficient for my case, OpenFOAM automatically reads the file when executing the selected solver.

Check your log file to see if your solver reads your fvOptions file, if yes, it should write something like the following:

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type limitTemperature
Source: limitTemperature
- selecting all cells
- selected 27300 cell(s) with volume 0.134187

[npatricia]

Thanks Omdemircan,

A quick one, how am I able to check my log file to see if fvOptions is supported? Any command for that. Am really sorry to over ask, but am abit confused in this.
Do I have to add some thing somewhere to effect it in my sytem folder, or what.

Thank you

[omdemircan]

For instance, you can type the following in order to output a log file in real time when using sonicFoam:

sonicFoam > log &

[RobertHB]

Hello Patricia,
the fvOptions file has to be saved unter <your case>\constant\ . Adding a (heat) source to your simulation can be done by using the scalarSemiImplicitSource.

scalarSource
{
    type scalarSemiImplicitSource;
    active true;

    scalarSemiImplicitSourceCoeffs
    {
        volumeMode    specific;         
        selectionMode cellSet;
        cellSet c1;
         
        injectionRateSuSp
        {
            T (1 0);
        }
    }
}

Alternatively you can define your source using points

        selectionMode points;
        points
        (
            (1.1 -1.01 -0.1)
            (1.1 -1.01 0)
        );

[npatricia]

Thanks alot for your replies,
@RobertHB, saving the fvOptions file in my case is exactly my challenge.
I have read some information in this line, and according to my understanding, my buoyantBoussinesqSimpleFoam in OpenFoam 5.0 fully supports this functionality. I just need to have this file either in my constant or system dictionary for my case to be able to add my source terms, which am failing to figure out how to do.

Kindly through more light on how to save this file.
Thank you once again.

[RobertHB]

Originally Posted by npatricia

[...] my buoyantBoussinesqSimpleFoam in OpenFoam 5.0 fully supports this functionality. [...]

Yes, it does, take a look at the TEqn.H:

    fvScalarMatrix TEqn
    (
        fvm::div(phi, T)
      - fvm::laplacian(alphaEff, T)
     ==
        radiation->ST(rhoCpRef, T)
      + fvOptions(T)
    );

And it definitely hast to go in .../constant/. I acutally dont understand which problem you are facing. ??
Here is a pretty detailed tutorial about implementing source terms: https://foamingtime2.wordpress.com/s...th-generation/

[npatricia]

My problem is where to save this file, and how. because neither does my constant/system dictionaries have the fvOptions file detected.

[Eko]

Originally Posted by RobertHB

And it definitely hast to go in .../constant/. I acutally dont understand which problem you are facing. ??

Is this always the case? For any kind of source term?
I would have put the fvOptions into the system folder.
I know (at least I think so) that for multiregion solvers it has to be in constant.

Originally Posted by npatricia

My problem is where to save this file, and how. because neither does my constant/system dictionaries have the fvOptions file detected.

Can you post your fvOptions file here? Full file with header please.

[RobertHB]

Originally Posted by Eko

Is this always the case? For any kind of source term?

I had another look at it and apparently (at least back in 2015, LINK) the fvOptions Dict could be placed in either constant or system.

Why can the fvOptions dictionary be stored in eithersystem or constant case sub-directory?
Check the constructor of the fv::IOoptionList c lass.

But i didnt follow through on checking the constructor.

//edit: But the question of constant vs. system is easy to check, right? Place it in either, does it run? > No? > Try the other. Does it run? > No? You probably messed up or your solver doesn't support fvOptions.

[Eko]

Originally Posted by RobertHB

//edit: But the question of constant vs. system is easy to check, right? Place it in either, does it run? > No? > Try the other. Does it run? > No? You probably messed up or your solver doesn't support fvOptions.

That's true. That's how I am doing it


But I have another question regarding injectionRateSuSp.

      injectionRateSuSp
        {
            variable_name     (Sc Sp);
        }

What does Sc and Sp stand for? Does it have to do with the explicit and linearised contributions?
I always see Sp=0 and Sc with a value.
What would happen if I set Sc=0 and Sp gets the value.
I am going to try it but wanted to ask you guys as well

[RobertHB]

Originally Posted by Eko

What does Sc and Sp stand for? Does it have to do with the explicit and linearised contributions?

Yes it does. Sc is constant part of your injection rate. I did a few test on what Sc does, but i could figure out a relationship.

I always see Sp=0 and Sc with a value.
What would happen if I set Sc=0 and Sp gets the value.
I am going to try it but wanted to ask you guys as well

I'd guess it will only work if you have a scalar field before starting the calculation as Sp works on the field value. Anyhow, Sc = 0 should equal to no injection.

[npatricia]

Greetings all,

I succeeded in creating an fvOption file for a test case I am trying out, however I am getting this error when I try to run the case
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-dcea1e13ff76
Exec : buoyantBoussinesqSimpleFoam
Date : Feb 22 2018
Time : 18:50:41
Host : "tflows-PowerEdge-R410"
PID : 5969
Case : /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


Reading g
Reading thermophysical properties

Reading field T

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Creating turbulence model

Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}

Reading field alphat

Calculating field g.h

Creating finite volume options from "constant/fvOptions"

Selecting finite volume options model type scalarCodedSource


--> FOAM FATAL IO ERROR:
keyword selectionMode is undefined in dictionary "/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation"

file: /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation from line 21 to line 96.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 442.

FOAM exiting

Kindly advise on how I can do away with this error
Thank you

[npatricia]

The fvOption file is as follows
radiation
{
type scalarCodedSource;
active yes;
name radiativeHeatExchange;

scalarCodedSourceCoeffs
{
selectionMode all;
fields (T);

codeInclude
#{
// Need this for Stefan-Boltzmann constant
#include "constants.H"
#};

codeCorrect
#{
#};

codeAddSup
#{
using constant:hysicoChemical::sigma;

if (not isActive())
return;

// Looking up model parameters
scalar Qsm = coeffs().lookupOrDefault<scalar>("Qsm", 164.0);
scalar rhow = coeffs().lookupOrDefault<scalar>("rho", 1000);
scalar Cp = coeffs().lookuoOrDefault<scalar>("Cp", 4200);
scalar Rt = coeffs().lookupOrDefault<scalar>("Rt", 0.03);
scalar ew = coeffs().lookupOrDefault<scalar>("ew", 0.97);

// Getting source vector from equation matrix
scalarField& src = eqn.source();
const volScalarField& T = eqn.psi();

// Iterating through patch
word top_patch_name = coeffs().lookupOrDefault<word>("patch", "top");
const fvPatch& pp = mesh().boundary()[top_patch_name];
forAll(pp, i) {
label cell_i = pp.faceCells()[i];
scalar Ai = pp.magSf()[i];
scalar Ts = T[cell_i];

// Heating
src[cell_i] -= Qsm*(1-Rt)*Ai/rhow/Cp;

// Cooling
src[cell_i] -= -sigma.value()*ew*paw4(Ts)*Ai/rhow/Cp;
}
#};

codeSetValue
#{
#};

code
#{
$codeInclude;
$codeCorrect;
$codeAddSup;
$codeSetValue;
#};
}

radiativeHeatExchangeCoeffs
{
selectionMode all;

patch top; // Name of the top patch
Qsm 163.0; // Solar radiative heat flux
Rt 0.03; // Reflectivity of water
ew 0.97; // Emissivity of water
rho 1000.0;
Cp 4200.0;
}
}

// fvOption to describe evaporation heat losses
evaporation
{
type scalarCodedSource;
active yes;
name evaporationHeatLosses;

scalarCodedSourceCoeffs
{
selectionMode all;
fields (T);

codeInclude
#{
#};

codeCorrect
#{
#};

codeAddSup
#{
if (not isActive())
return;

// Looking up model parameters
scalar A = coeffs().lookupOrDefault<scalar>("A", 2.7);
scalar rhow = coeffs().lookupOrDefault<scalar>("rho", 1000);
scalar Cp = coeffs().lookupOrDefault<scalar>("Cp", 4200);
scalar Ta = coeffs().lookupOrDefault<scalar>("Ta", 25);
scalar e2 = coeffs().lookupOrDefault<scalar>("e2", 31.69);
scalar b0 = coeffs().lookupOrDefault<scalar>("b0", 3.2);
scalar u2 = coeffs().lookupOrDefault<scalar>("u2", 0);

// Getting source vector from equation matrix
scalarField& src = eqn.source();
const volScalarField& T = eqn.psi();

// Iterating through patch
word top_patch_name = coeffs().lookupOrDefault<word>("patch", "top");
const fvPatch& pp = mesh().boundary()[top_patch_name];
forAll(pp, i) {
label cell_i = pp.faceCells()[i];
scalar Ai = pp.magSf()[i];
scalar Ts = T[cell_i] - 273.15;

// Buck equation
scalar es = 0.61121*exp((18.678 - Ts/234.5)*(Ts/(257.15 + Ts)));
// Converting into mbar
es *= 10;
scalar Qe = -(A*cbrt(Ts - Ta) + b0*u2)*(es - e2);

src[cell_i] -= Qe*Ai/rhow/Cp;
}

#};

codeSetValue
#{
#};

code
#{
$codeInclude;
$codeCorrect;
$codeAddSup;
$codeSetValue;
#};
}

evaporationHeatLossesCoeffs
{
selectionMode all;

patch top; // Name of the top patch
A 2.7; // Empiric constant
e2 31.69; // Assuming 25 C 2 meters above the surface
b0 3.2; // Another empiric constant
u2 0.0; // Wind velocity 2 meters above the surface
Ta 25; // Ambient temperature in C
rho 1000;
Cp 4200;
}
}

// vi: set ft=foam et sw=2 ts=2 sts=2;

[Eko]

Originally Posted by npatricia

Greetings all,

I succeeded in creating an fvOption file for a test case I am trying out, however I am getting this error when I try to run the case
[...]
Creating finite volume options from "constant/fvOptions"

Selecting finite volume options model type scalarCodedSource


--> FOAM FATAL IO ERROR:
keyword selectionMode is undefined in dictionary "/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation"

file: /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation from line 21 to line 96.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 442.

FOAM exiting

Kindly advise on how I can do away with this error
Thank you

Please post your fvOptions file here. The mistake is in it.
It seems like you're missing selectionMode.

[npatricia]

@ Eko, I have as well posted the fvOptions file.
Thank you

[RobertHB]

--> FOAM FATAL IO ERROR:
keyword selectionMode is undefined in dictionary "/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation"

Try placing the selectionMode and the corresponding field not in the coeffs section but one further upward after name radiativeHeatExchange;

If i remember correctly if it wants it placed in scalarCodedSourceCoeffs it'll tell you

[npatricia]

Thank you so much RobertHB,
I was able to rectify that, though have a new error arising now
Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00990741, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00990413, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.0179848, Final residual = 0.0001954, No Iterations 1
Using dynamicCode for fvOption:: radiation at line 28 in "/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs"
Creating new library in "dynamicCode/sourceTime/platforms/linux64GccDPOpt/lib/libsourceTime_2d9782ba70b4b08459f487659c5cba04e3b4 27ff.so"
Invoking "wmake -s libso /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/dynamicCode/sourceTime"
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file codedFvOptionTemplate.C
/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs: In member function ‘virtual void Foam::fv::sourceTimeFvOptionscalarSource::addSup(F oam::fvMatrix<double>&, Foam::label)’:
/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs:71:51: error: ‘paw4’ was not declared in this scope
/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs: In member function ‘virtual void Foam::fv::sourceTimeFvOptionscalarSource::addSup(c onst volScalarField&, Foam::fvMatrix<double>&, Foam::label)’:
/home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs:71:51: error: ‘paw4’ was not declared in this scope
codedFvOptionTemplate.dep:580: recipe for target 'Make/linux64GccDPOpt/codedFvOptionTemplate.o' failed
make: *** [Make/linux64GccDPOpt/codedFvOptionTemplate.o] Error 1


--> FOAM FATAL IO ERROR:
Failed wmake "dynamicCode/sourceTime/platforms/linux64GccDPOpt/lib/libsourceTime_2d9782ba70b4b08459f487659c5cba04e3b4 27ff.so"


file: /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.scalarCodedSourceCoeffs from line 28 to line 80.

From function codedBase::createLibrary(..)
in file db/dynamicLibrary/codedBase/codedBase.C at line 213.

FOAM exiting

Kindly advise please.
Thank you

[alexeym]

Hi,

This

// Cooling
src[cell_i] -= -sigma.value()*ew*paw4(Ts)*Ai/rhow/Cp;

should be

// Cooling
src[cell_i] -= -sigma.value()*ew*pow4(Ts)*Ai/rhow/Cp;

[npatricia]

Thanks a lot @Alexeym for that correction, had sliiped off in typing. having a new error though which am failing to understand what it means

--> FOAM FATAL ERROR:
Attempt to return primitive entry ITstream : /home/tflows/OpenFOAM/OpenFOAM-2.4.0/tutorials/heatTransfer/buoyantBoussinesqSimpleFoam/solarPond_1/constant/fvOptions.radiation.sourceTimeCoeffs, line 89, IOstream: Version 2.0, format ASCII, line 0, OPENED, GOOD
primitiveEntry 'sourceTimeCoeffs' comprises
on line 89 the verbatim string "\
"
as a sub-dictionary

From function const dictionary& primitiveEntry::dict() const
in file db/dictionary/primitiveEntry/primitiveEntry.C at line 191.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam:rimitiveEntry::dict() const at primitiveEntry.C:?
#3 Foam::fv:ption:ption(Foam::word const&, Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&, bool) at ??:?
#4 Foam::fv::sourceTimeFvOptionscalarSource::sourceTi meFvOptionscalarSource(Foam::word const&, Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at constant/fvOptions.radiation.scalarCodedSourceCoeffs:106
#5 Foam::fv:ption::addRemovabledictionaryConstructo rToTable<Foam::fv::sourceTimeFvOptionscalarSource> ::New(Foam::word const&, Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ~/OpenFOAM/OpenFOAM-2.4.0/src/OpenFOAM/lnInclude/autoPtrI.H:34
#6 Foam::fv:ption::New(Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ??:?
#7 Foam::fv::CodedSource<double>::redirectFvOption() const at ??:?
#8 Foam::fv::CodedSource<double>::addSup(Foam::fvMatr ix<double>&, int) at ??:?
#9 ? at ??:?
#10 ? at ??:?
#11 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12 ? at ??:?
Aborted (core dumped)