[Chrisi1984]

Hi all,

I want to limit the temperature. That mean that every value where T is smaller than 300K, should be set to 300K after every iteration.

I thought something like this:

forAll(fluidRegions[i].cellZones(), zoneI)
{
const cellZone& cz = fluidRegions[i].cellZones()[zoneI];
const labelList& cells = cz;



if (T < 300)
{
forAll(cells, iCells)
{
const label cellId = cells[iCells];
T[cellId]=300;

}
}
}

But this results in errors during compiling.

Can anyone help me?

Best regards Chrisi

[akidess]

Without mentioning your error, you are looking for someone with psychic powers to help you... Anyways, I think the following code fragment would make more sense:

forAll(cells, iCells)
{
    const label cellId = cells[iCells];
    if (T[cellId] < 300) T[cellId]=300;
}

[Chrisi1984]

Hi,

sorry I forgot the error message!

Here it is:

invalid types error: '<unresolved overloaded function type>[const Foam::label]' for array subscript

Regards Chrisi

[Chrisi1984]

My problem is still existing. Any ideas?

[akidess]

Would you share it so that people can learn from this thread?

[Chrisi1984]

Sorry!

I am wrong. I did not solve the problem.


I wanted to write this below an other thread!!

Regards Chrisi

[Chrisi1984]

Hi,

Now I really found a possibility to limit the temperature.

forAll(mesh.cellZones(), zoneI)
{

const cellZone& cz = mesh.cellZones()[zoneI];
const labelList& cells = cz;


forAll(mesh.cellZones(), zoneI)
{

const cellZone& cz = mesh.cellZones()[zoneI];
const labelList& cells = cz;


forAll(cells, iCells)
{
const label cellId = cells[iCells];

if (thermo.T()[cellId] > 1400.0)
{
h[cellId] = 1006*1400;
}

if (thermo.T()[cellId] < 400.0)
{
h[cellId] = 1006*400;
}
}


}


}

Where in 1006 is the value for cp.

I did this because h is approximately cp*T.

Perhabs it helps somebody.

Regardy Chrisi

[akidess]

Why loop through the cellZones within the cellZone loop?

[Chrisi1984]

You are right off course the loop over the cell zones is unnecessary!

Regards Chrisi

[alberto]

Hmm, why not a simple

T.max(300);

P.S. Yes, max, it is not a typo. The max method is equivalent to max(T,300) looped over all cells.

P.P.S. I have no idea why you are doing this, but it might make your energy equation unhappy :-)

[Chrisi1984]

Thank you for your suggestion.

But with T.max(300);

I get this error:

hEqn.H:39: error: ‘Foam::T’ does not have class type

Regards Chrisi

[akidess]

From your previous post I'm guessing you don't have an object T, since you used thermo.T. So you could try using thermo.T.max(300).

[Chrisi1984]

Hi

I tried this too,

but this also results in errors during compiling.

error: ‘thermo->Foam::basicThermo::T’ does not have class type

Regards Chrsi

[alberto]

The correct syntax would be

thermo().T().max(300)

but T is returned only as const, so it cannot be modified at this stage.

You can either define a second method to return T without the const qualifier, or edit the thermo code and introduce the limitation there. Both solutions see quite messy

[Hgholami]

Dear Alberto
I add simple energy equation to icoFluid solver in OF-ext4.0 as:

fvScalarMatrix TEqn
(
fvm::ddt(T_)
+ fvm::div(phi_, T_)
- fvm::laplacian(DT_, T_)
);
TEqn.solve();

and I want to limit temperature. I uses T_.min(300.0) for limitation, but all data will be 300K. Other option,

scalar Lup= 350.0;
scalar Llo= 300.0;

forAll(T_,i)
{
if (T_[i]<Llo){T_.replace(i,Llo);}
if (T_[i]>Lup){T_.replace(i,Lup);}

}

give all data 300K.
I also use

forAll(mesh.cellZones(), zoneI)
{
const cellZone& cz = mesh.cellZones()[zoneI];
const labelList& cells = cz;
Info<< "banana0" << endl;
forAll(cells, iCells)
{
const label cellId = cells[iCells];
Info<< "banana1" << endl;
if (T_[cellId] < 300)
{
Info<< "bananaIf" << endl;
T_[cellId]=300;
}
}
}

It is go to two loops, but not in if. maybe it need other argument instead of [cellId]. So I change the code to

forAll(mesh.cellZones(), zoneI)
{
const cellZone& cz = mesh.cellZones()[zoneI];
const labelList& cells = cz;
Info<< "banana0" << endl;
forAll(cells, patchID)
{
const label cellId = cells[patchID];
Info<< "banana1" << endl;
if (T_[cellId] < 300.0)
{
Info<< "bananaif" << endl;
T_[cellId]=300.0;
}
if (T_[cellId] > 350.0)
{
Info<< "bananaif2" << endl;
T_[cellId]=350.0;
}
}
}
Info<< "Min/max T: after if" << min(T()).value() << ' '
<< max(T()).value() << endl;

Now, the code goes to if but final temperature doesn't change. The other idea was using fvOption, but it doesn't exist in OF-ext4.0. Do you have any idea for this problem? thanks
Also I should note:

const volScalarField& icoFluid::T() const
{
return T_;
}

[Hgholami]

I also test

max(T()).value() = 350.0;
min(T()).value() = 300.0;

but nothing happen.

[Hgholami]

Dear Chrisi1984
Did you solve this problem?

[olivierG]

hello,
Now (2 year old...) you can use energyTransport function object on incompressible flow (see https://www.openfoam.com/releases/op...nd-physics.php) and also from even more years, limit T in fvOption file with "limitTemperature" type.

limitT
    {
        type            limitTemperature;
        active          yes;
        selectionMode   all;
        min             200;
        max             500;
        phase           gas; //optional
    }

regards,
olivier