[Eko]

Hey guys I have started working with OpenFOAM 3weeks ago and need some tips for setting up my case.

I am looking at a building with a heat source (in kW) and want to simulate the heating of the room. I just want to see the air temperature nothing else.

I would like to set a start temperature (for example 293K) and want to see the temperature 1, 2 or 3 hours later.

I already checked some tutorials but didn't find one which has a heat source given in W or J. The hotRoom tutorial seems to work with temperature and doesn't really help me.

So my questions are:

1. How do I set up a start Temperature and where? (T-file?)
2. How and where do I define the heat source?
3. How do I calculate the temperature at 1,2 or 3 hours? (by using calculated
BC in T-file or is there another way?)
4. I would use buoyantBoussinesqPimpleFoam solver. Or should I try
chtMultiRegionFoam?


If you need more information or think that I've forgot something just let me know.
Thank you in advance and happy new year everyone.

[piu58]

I used buoyantBoussinesqPimpleFoam with some success. I did not find a boundary condition that you indent to use. I recommend to use the temperature b.c. and calculate the heat production form the result. In a few steps you should have found a temperature which fulfills the heat production.

[Bloerb]

buoyantBoussinesqPimpleFoam and chtMultiRegionFoam are essentially identical in recent OF versions since you can choose the Boussinesq assumtion in the thermoPhysicalProperties file. If you need different regions coupled cht is the way to go. E.g If you want to include conduction through the walls and can't treat them as boundary condtions. To answer your questions:

The initial temperature is set in the 0/T file. You can set a uniform value to the entire volume or use the setFields utility to vary it in space.

You can add a volumetric heat source via fvOption

/*--------------------------------*- 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    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

options
{
    energySource
    {
        type            scalarSemiImplicitSource;

        selectionMode   all;

        volumeMode      specific;
        injectionRateSuSp
        {
            h      (1.5e6 0);   
        }
    }
}


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

This will add a heat source of 1.5e6 W/m³ to everything. In your case you probably need to define a cellZone and specify selectionMode to that cellZone. You can also change the volumeMode so that your heat source is in W. You can however also specify a heat source as a boundary condtion.

    heat
    {
        type            externalWallHeatFluxTemperature;
        kappaMethod     fluidThermo;
        mode         flux; // flux for W/m² or power for W
         q        uniform 100; // 100 W/m²
         Q        uniform 100; // 100 W
        value           $internalField; // initial temperature
    }

You can calculate the temperature after 3 hours by simply checking it in paraview. Or you can use a functionObject to calculate it for a specifc patch or the volume etc.

[Eko]

Thanks a lot guys
I will try to setup the case within the next days and will tell you if it worked out or if I need more help.

[Eko]

Originally Posted by Bloerb

You can however also specify a heat source as a boundary condtion.

    heat
    {
        type            externalWallHeatFluxTemperature;
        kappaMethod     fluidThermo;
        mode         flux; // flux for W/m² or power for W
         q        uniform 100; // 100 W/m²
         Q        uniform 100; // 100 W
        value           $internalField; // initial temperature
    }

You can calculate the temperature after 3 hours by simply checking it in paraview. Or you can use a functionObject to calculate it for a specifc patch or the volume etc.

Does this even work with the Boussinesq approximation? It seems like it's implemented for compressible cases and the Boussinesq solver is incompressible.

I am still trying to figure out how to add a heat source. I am trying to add one to the floor of the hot room tutorial case, just to understand it.


Another question: Is it possible to set up a heat source in W/m² by using fvOptions?


Edit: is there any tutorial case with a heat source given in W or W/m²? checked all heatTransfer tutorials but didn't find what I was looking for

[Eko]

One more question. If I put a solid, for example a cube into the room as heat source. So the air in the room is heaten up by this cube. Does this already count as multiregion? Do I have to use chtMultiRegionFoam in this case or can buoyantBoussinesqPimpleFoam solve this?

[piu58]

May be you can find boundary conditions which are suitable for what happens with the cube. If you want to know the temperature distribution in the cube I see two ways
- multi region

or

if the heat capacity of the room is mauch larger than the one of the cube

- Define the cube as wall and read the temperature distribution of the wall. Make a different simulation with only the cube and set this temperature as b.c.

[Eko]

Originally Posted by piu58

May be you can find boundary conditions which are suitable for what happens with the cube. If you want to know the temperature distribution in the cube I see two ways
- multi region

or

if the heat capacity of the room is mauch larger than the one of the cube

- Define the cube as wall and read the temperature distribution of the wall. Make a different simulation with only the cube and set this temperature as b.c.

I don't really need to know what happens with the cube. I just want to see how the temperature in the room changes. I looked at buoyant and cht cases and the cht ones seem to be easier (at least I understand more ). I still have no clue how I can add a heatsource in W or W/m² while using buoyant solvers (bc didn't work out and I don't know how to properly use fvOptions).

I'm currently setting up a more difficult case with chtMultiRegionFoam and till now it's going well. Just a lot more work to do with the CAD, meshing, setting up files compared to buoyant tasks.