[miha23]

Dear Foamers!

I'd like to define a volume in my domain where the value of a field variable (e.g. temperature) is constant.
I know that setFields does this, but I need this constant value in that volume to be constant for the whole time.
Can anyone have an idea how to solve this, without hard coding?

Thanks for advance,
Gábor

[alexeym]

Hi,

$FOAM_SRC/fvOptions/constraints/fixedValueConstraint.

Adapting header commentary for temperature:

    fixedTemperature
    {
        type            scalarFixedValueConstraint;
        active          yes;

        selectionMode   cellZone;
        cellZone        zone-with-constant-temperature;
        fieldValues
        {
            T           298.15;
        }
    }

Though, depending on your solver, maybe fixedTemperatureConstraint could be more suitable.

[miha23]

Thank you Alexey. It works fine.

[miha23]

Dear Alexey,

I am using scalarFixedValueConstraint for setting a constant concentration in a volume, but after I define the zone and the needed value in the fvOptions file, and I also add fvOtions(c) to my solver it gives back the following warning messege.

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0639208, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.024972, No Iterations 2
time step continuity errors : sum local = 1.22917e-05, global = 2.26427e-20, cumulative = 2.26427e-20
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 118
    Source fixedConcentration defined for field c but never used
smoothSolver:  Solving for c, Initial residual = 1, Final residual = 0.0451066, No Iterations 3
smoothSolver:  Solving for epsilon, Initial residual = 0.953597, Final residual = 0.0238806, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0701502, No Iterations 1

It only appears once, at the beginning of the simulation.
Have you got any idea, where I could make the mistake?

Thanks,
Gábor

[alexeym]

Hi,

Could you post how do you add fvOptions to your solver? I.e. post relevant code. Otherwise thread will become rather boring game "guess what I did wrong".

[miha23]

My scalar transport eq. in the solver looks like this:
(The -sigma(U &d) is source here, where sigma is just a constant and d is a pointer vector, but I think this part is rather irrelevant in my problem.)

fvScalarMatrix cEqn
	(
		fvm::ddt(c)
		+fvm::div(phi, c)
		-fvm::laplacian(Dt, c)
	==
	   -sigma*(U & d)
	   +fvOptions(c) 

    );

    cEqn.relax();

    fvOptions.constrain(cEqn);

    cEqn.solve();

    fvOptions.correct(c);

And my fvOptions file is this:

fixedConcentration
{
	type 		scalarFixedValueConstraint;
	active 		yes;
	
	scalarFixedValueConstraintCoeffs
	{	
		selectionMode	cellZone;
		cellZone		pollutionSource;
		fieldValues
		{
			c		0;
		}
	}
}

Furthermore, I have checked that

	-I$(LIB_SRC)/fvOptions/lnInclude \
    -lfvOptions \

are included in the Make/options

and my modified simplefoam solver contains the followings also

#include "fvOptions.H"
    #include "createFvOptions.H"

And cEqn is called right after the pEqn:

 // --- Pressure-velocity SIMPLE corrector
        {
            #include "UEqn.H"
            #include "pEqn.H"
	    #include "cEqn.H"

        }

        laminarTransport.correct();
        turbulence->correct();

but I have tried if I put it after the turbulence -> correct(), but in that case the above mentioned warning appears also before "Solving for k" and epsilon

[LuckyTran]

Go into your cellZones dict and make sure you have a cellZone named pollutionSource

If serial case, you need to check constant/polyMesh/cellZones
And make sure they're also present for after you decompose, e.g. in 0/constant/polyMesh/cellZones.

[miha23]

I got the pollution source in the cellZone dict.

Any ideas? Anyone?

[alexeym]

Hi,

The output

Source fixedConcentration defined for field c but never used

is produced by checkApplied method (which in turn calls checkApplied method of concrete finite volume option).

checkApplied method is called (in your case):
- when you do "+fvOptions(c)"
- when you do "fvOptions.constrain(cEqn)"
- and finally when you do "fvOptions.correct(c)"

In your case fvOption(c) does nothing, since you defined only constraining. After first call to constrain method, source marked as used and checkApplied becomes happy.

So, I guess, the message could be ignored.

And finally, does the simulation run smoothly or values of concentration are not constrained?

[Thecomebackkid]

Dear all, I want the variables in specific regions to be constant 0. How is this possible. I have a fvOptions file and headers called in my solver for fvOptions.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 fixedPressureGEARDRV
    {
        type            scalarFixedValueConstraint;
        active          yes;

scalarFixedValueConstraintCoeffs
{
        selectionMode   cellZone;
        cellZone        GEARDRV;
        fieldValues
        {
           p            0;
        }
}
}
 fixedVelocityGEARDRV
    {
        type            vectorFixedValueConstraint;
        active          yes;
vectorFixedValueConstraintCoeffs
{
        selectionMode   cellZone;
        cellZone        GEARDRV;
        fieldValues
        {
            U (0 0 0);
        }
    }
}
  fixedPressureGEARDVN
   {
        type            scalarFixedValueConstraint;
        active          yes;

 scalarFixedValueConstraintCoeffs
{
       selectionMode   cellZone;
        cellZone        GEARDVN;
        fieldValues
        {
            p  0;
        }
    }
}
fixedVelocityGEARDVN
    {
        type            vectorFixedValueConstraint;
        active          yes;

 vectorFixedValueConstraintCoeffs
{
       selectionMode   cellZone;
        cellZone        GEARDVN;
        fieldValues
        {
            U (0 0 0);
        }
    }

}








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

However when running my case none of those regions are zero. Also I have the issue with the checkApplied poping up for pressure not used on first iteration.


Any help is appreciated.

[hhu_lulu]

Have you solved the problem? I have the same issue. The regions where I constraint to 0 by scalarFixedValueConstraint are not zero.

[hhu_lulu]

I think I have figured out another way, in which adding fvOtions(c) to solver is not necessary. The scalarFixedValueConstraint could be placed within functions, i.e. the function scalarTransport in controlDict file.
At least for my case, this adaptation proved to be effective. My model aims to simulate the scalar transport in open channel. The pimpleFoam solver is imposed and the variable s in some regions of computational domain needs to be set to 0.
Previously, I put the scalarFixedValueConstraint in fvOptions file and it didn't work.