[ShinyRiver]

Hi guys,


I would like to model a uniform non-local heat generation or heat source within a solid in openFOAM. In FLUENT that could be explicitly set in defining the solid zone, but in openFOAM I am not sure if it is easily available. Does someone have an idea to do that in openFOAM without having to edit the source code?


Thanks for your support

[Bloerb]

Add an fvOption file to your region folder. Either constant/solid or system/solid depending on your OF version.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  dev                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system/solid";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

options
{
    energySource
    {
        type            scalarSemiImplicitSource;

        selectionMode   all; // or only part of the domain via a cellZone e.g defined with topoSet

        volumeMode      specific; // source term per volume or total
        injectionRateSuSp
        {
            h      (1.5e6 0);   // explicit and implicit part of the source term
        }
    }
}

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

This adds a temperature independent source term in either W or W/m³ depending on the volumeMode. The second number in the injectionRateSuSp(here 0) would be the implicit part and hence the temperature dependent one. Requires a solver which uses fvOption like chtMultiRegion

[Kevin.H]

Hallo,

I try to implement a heat source for a solid as well, but it didn´t worked.
Maybe you can find my Problem.
I use OpenFoam 4.1 and it is a chtMultiRegion case.

heatSource
{
    type            scalarSemiImplicitSource;
    active          true;
 
    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   all; // all, cellSet, cellZone, points
        cellSet         magnet;
        volumeMode      specific; // absolute;
        injectionRateSuSp
        {
           T     (400 0); 
//        h      (1.5e6 0); 
        }
    }
}

Because of the number of Cells I know that OpenFoam set the source into the right Regions:

Creating finite volume options from "system/fvOptions"
Selecting finite volume options model type scalarSemiImplicitSource
    Source: heatSource
    - selecting all cells
    - selected 35200 cell(s) with volume 4.08615e-05

But than I get this result, and nothing happened.
I think wir h it works fine, but when I try to implement a Temperature it doesn´t work.

Solving for solid region magnet
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 118
    Source heatSource defined for field T but never used
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 118
    Source heatSource defined for field T but never used
DICPCG:  Solving for h, Initial residual = 0.812167, Final residual = 0.0564586, No Iterations 14
Min/max T:241.843 293.675
ExecutionTime = 72.39 s  ClockTime = 72 s

Do anyone of u maybe now why it doenst work with T?

Source: http://caefn.com/openfoam/fvoptions-semiimplicitsource

And can maybe anyone explain how I can calculate the HeatFlux (Q(Point)), when I know the h and the A but not the Delta T.

Delta T = internalField Region A - internalField Region B ?

Thank u very much for your help!!

And mabye another Question: In my cases I recocnice that when I change the internalField of a solid to 400K, nothing happend too.
Is this normal?

Best regards

[Kevin.H]

Or I should ask other questions.
If I use the scalarSemiImplicitSource in this way, do I give the CellCet magnet a heat flux of 25Watt?

heatSource
{
    type            scalarSemiImplicitSource;
    active          true;
 
    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   all; // all, cellSet, cellZone, Points
        cellSet         magnet;
        volumeMode      absolute; 
        injectionRateSuSp
        {         h      (25 0); 
        }
    }
}

EDIT: It seems to be right
When I use wallHeatFlux than the result is fine.
Thanks!