[samiam1000]

Dear all,

reading this tutorial, I have found these lines:

The example shows an explicit volumetric source for a scalar equation, given by a ...ExplicitSource entry. Similarly a constraint can also be applied that sets values in given cells, given by a ...ExplicitSetValue entry. Specialised sources are also available, e.g. actuationDiskSource for wind turbing siting calculations.

It seems that it is possible to set the value of a variable in certain cells, by using the explicitSetValue function.

The point is that I can not understand which is the file that I have to edit.

Could anyone help?

Thanks a lot,

Samuele

[kwardle]

Take a look at constant/sourcesProperties. This is where you set the sources. The easiest way is to use a cellSet as is done in the simpleFoam/turbineSiting tutorial. The cellSets are defined in system/topoSetDict by running topoSet--which will need to be run in parallel after your decomposePar if you are planning to run your solver in parallel.

For an explicit scalar source named s1 on a field T for example, you would have the following in your sourcesProperties:

s1
{
    type            scalarExplicitSource;
    active          true;
    timeStart       0;
    duration        10000;
    selectionMode   cellSet;
    cellSet         s1;

    scalarExplicitSourceCoeffs
    {
        volumeMode      absolute; //specific
        injectionRate
        {
            T              <some scalar value>;
        }
    }
}

Hope that helps.

[samiam1000]

Dear kwardle,

yeah, this helps a lot, thank you very much.

Just a question (I'll google it, but maybe you already know the answer): can I use `explicitSetValue' with buoyantSimpleFoam/buoyantPisoFoam solver, too?

Thanks again,

Samuele

[samiam1000]

Pardon the spam, but I need more help. Let me try to explain what I think I should do:

1. I prepare my case folder
2. I add the constant/sourcesProperties file
3. I give the command topoSet --which (I can not und this point very well. I have a volume patch in my constant/polyMesh/cellZones file.. Isn't it possible to insert in the constant/sourcesProperties the name of that patch instead of running topoSet? I can not und how to use it)
4. I run my simulation.

Is that correct?

If so, I am going to work ok point 3.

Also, in order to embed this functionality in the buoyantSimplFoam folder is it enough to add this line

sources.constrain(UEqn());

in the UEqn.H file, according to this page?


Thanks a lot for your help,

Samuele

[kwardle]

First, no, buoyantSimpleFoam is not currently set up to use sources as you can see in UEqn.H. You are correct in that you need to add the line you mentioned, but you also need to add the source term in the actual equation as:

    tmp<fvVectorMatrix> UEqn
    (
        fvm::div(phi, U)
      + turbulence->divDevRhoReff(U)
      == sources(U)
    );

For example, compare simpleFoam/UEqn.H with the one in buoyantSimpleFoam/UEqn.H and you will see the lines you need to add. But that is NOT everything. There are two additional things to add elsewhere:

1. Add the header to the main solver source file (buoyantSimpleFoam.C) as:

#include "IObasicSourceList.H"

2. Add the line:

 IObasicSourceList sources(mesh);

to the end of createFields.H

Again take a look at the files in simpleFoam as an example. Be sure to recompile your solver and you should be good (unless I have missed something). If there are errors, they are usually helpful it you start at the time and actually take a look at why it is complaining. This will help you add what is missing.
Regards,
Kent

[samiam1000]

Hi Kent and thanks for answering.

I did what you suggested, but I get an error. Here you can find a new post with my problem (I started a new thread since it is a different problem).

If you can have a look, that would be great.
Thanks a lot,

Samuele

PS: now I am trying to run a case using the simpleFoam solver in order to be able to use the explicitSetValue feature. I want to fix the value of a variable (the temperature!) in each cell of a certain patch. That sounds challenging, doesn't it?

[kwardle]

Sorry, I didn't answer item #3 in your post. If you want to apply a uniform source everywhere in your domain (not sure what you mean by 'volume patch') then just create a cellSet as a box bigger than your volume with the following in topoSetDict:

actions
(
    {
        name    bigBox;
        type    cellSet;
        action  new;
     
        source boxToCell;
        sourceInfo
        {
        box (-1 -1 -1) (1 1 1);  //box corner limits
        }
    }
);

[samiam1000]

Sorry: maybe I didn't explain very well what I meant. I don't want to fix the temperature in each cell of my domain, but I want to fix it in each cell that is in a subdomain in the patch called air_infinite.

If you look at my constant/polyMesh/cellZones, you will find:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       regIOobject;
    location    "constant/polyMesh";
    object      cellZones;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

3
(
air_infinite
{
    type cellZone;
cellLabels      List<label> 
1218
(
0
.
.
.
1217
)
;
}

air_internal
{
    type cellZone;
cellLabels      List<label> 
97372
(
1218
.
.
.
98589
)
;
}

air_external
{
    type cellZone;
cellLabels      List<label> 
9492
(
98590
.
.
.
108081
)
;
}
)

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

and what I want to do is to write in the constant/sourcesProperties the name of the patch (i.e. air_internal). Is it possible?

[kwardle]

OK, I misunderstood and thought you were trying to set a source not constrain the value to a set value. Even so, I think the setup is all the same you would just use scalarExplicitSetValue instead in your sourcesProperties as:

s1
{
    type            scalarExplicitSetValue;
    active          true;
    timeStart       0;
    duration        10000;
    selectionMode   cellSet;
    cellSet         bigBox;

    scalarExplicitSetValueCoeffs
    {
        injectionRate
        {
            T              <some scalar value>;
        }
    }
}

As for you question about setting the source on a cellZone. How did you create the cellZone in the first place? You would have had to create a cellSet first and the run setsToZones to create the zone (perhaps there is another way but this is the one I know) or you have converted the mesh from some other format in which case, I think it still makes the set first. Presumably you already have a cellSet named air_internal as well. Take a look in constant/polyMesh/sets/ to see.

[samiam1000]

Originally Posted by kwardle

OK, I misunderstood and thought you were trying to set a source not constrain the value to a set value. Even so, I think the setup is all the same you would just use scalarExplicitSetValue instead in your sourcesProperties as:

s1
{
    type            scalarExplicitSetValue;
    active          true;
    timeStart       0;
    duration        10000;
    selectionMode   cellSet;
    cellSet         bigBox;

    scalarExplicitSetValueCoeffs
    {
        injectionRate
        {
            T              <some scalar value>;
        }
    }
}

Yeah, thanks a lot. That's great.

As for you question about setting the source on a cellZone. How did you create the cellZone in the first place? You would have had to create a cellSet first and the run setsToZones to create the zone (perhaps there is another way but this is the one I know) or you have converted the mesh from some other format in which case, I think it still makes the set first. Presumably you already have a cellSet named air_internal as well. Take a look in constant/polyMesh/sets/ to see.

This is a more challenging question. Well, I convert the mesh from the fluent format and that's why I have those patches in the cellZone file.

Also, I don't have any constant/polyMesh.. How can I create it?
Sorry, but I can not understand your suggestion.
Could you explain the steps?

Thanks again,

Samuele

[kwardle]

Two thoughts.
1. Not sure which converter you used, but fluentMeshToFoam has an option -writeSets which will write your regions as sets. It also has one -writeZones which will just write the zones only. So, you could make a new case and reconvert your mesh with -writeSets and copy those over to the old case..
2. Alternatively, it would be pretty simple to manually create the cellSet file from the cellZone file. The format of the cellSet file would just be:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       cellSet;
    location    "constant/polyMesh/sets";
    object      air_internal;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


97372
(
1218
.
.
.
98589
)

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

That seems easy enough. Just copy and paste the list of cell numbers in you zone and create the file as constant/polyMesh/sets/air_internal.

[samiam1000]

Thanks a lot. I am going to try with this.

Just a question: should I "activate" the sourceProperties file?

I mean, once I save it in the constant folder, how can I `tell' the solver to read it?
Is it automatic?

Thanks again,

Samuele

[kwardle]

If the solver is set up for sources it will look for the file and probably complain if it is not there. If the file sourcesProperties is there and the specific source is set to "active true;" then it should work.

[samiam1000]

I thought about fixing the velocity instead of pressure.
But it doesn't work.

[samiam1000]

That's great.

Everything works, now!

Thanks for the support,

Samuele.

PS: now I have to add this feature into the buoyantSimpleFoam problem. If you want to help me, look at this. Samuele

[samiam1000]

Dear Kent,

could you help me in solving the same problem with buoyanPimpleFoam.

If you want, you can read this thread.

Thanks a lot,

Samuele.

[samiam1000]

Dear Kent,

I would like to embed the explicitSetValue feature (read here) in the chtMultiRegionFoam (see here).

Could you kindly help, please?

Thanks a lot,

Samuele