CFD Online Discussion Forums - OpenFoam 2.2 fvOptions temperature limits

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - OpenFoam 2.2 fvOptions temperature limits (https://www.cfd-online.com/Forums/openfoam-solving/117348-openfoam-2-2-fvoptions-temperature-limits.html)

OpenFoam 2.2 fvOptions temperature limits

Dear all,
As some of you know, OF 2.2 introduce a new system of "fvOptions" files where we can set the porosity and so on...
There is another interesting command that is "temperatureLimitsConstraint". As its name says, it is used to constraint the temperature to a minimum and maximum value.

Because I didn't find any example online, here is my file:
You have to put it into the "fvOptions" file located in system

Code:

source1

{

    type            temperatureLimitsConstraint;

    selectionMode   all;

    active          true;



        temperatureLimitsConstraintCoeffs

        {

            Tmin     220;

            Tmax     270;

        }

}

This command will bound the temperature between 220K and 270K in all the domain. It is useful in some cases if your compressible solver can't catch the value temperature value during the first iterations.

Edit: the page description come from here: http://www.openfoam.org/version2.2.0/fvOptions.php

Thanks for the tip!

Does this work for all compressible solvers? I tried adding this to sonicFoam and it seems to get ignored.

As I remember, sonic foam is mostly hard coded so it might not work.
To check, find the thermo equation in the source code and check if you can find a line with "+ fvoptions" or something similar.

Hi Fredo,
Thanks for your tip. May i know whether there exists similar options to control turbulent kinetic energy k and epsilon?
ksv

For k, omega et epsilon, you can add a simple code such as:

Code:

        k= max(k, kMin);

        k= min(k, kMax);

where kMin and kMax can be defined in the code or by a dimensionedScalar and a IOdictionary.

We must use fOption for T because T is not a variable used by OpenFoam. The function "fOption" actually modify the thermo equation (enthalpy) to correct the temperature.

Hi all,

sorry for re-opening this thread but I'm using the temperatureLimitsConstraint in conjunction with chtMultiRegionFoam (OF-2.2.x, latest available update) and it actually doesn't seem to me it's working as it is supposed to. The fvOptions dict appears to be read properly, but when the enthalpy equation is solved the temperature violates the imposed bounds, even if all the discretization schemes should be bounded/limited. Here there are my fvSchemes and fvOptions dictionaries (there is only one fluid region at this stage), together with an extract of runtime output log.

fvSchemes:

Code:

ddtSchemes

{

    default         Euler;

}



gradSchemes

{

    default         cellMDLimited Gauss linear 1;

    grad(U)         cellMDLimited Gauss linear 0.5;

    //grad(h)         faceLimited Gauss linear 1;

    

}



divSchemes

{

    default        none;

    div(phi,U)      bounded Gauss linearUpwindV grad(U);

    div(phi,K)      bounded Gauss linear;

    div(phi,h)      bounded Gauss limitedGamma 1 264157 294289; 

    div(phi,k)      bounded Gauss upwind;

    div(phi,epsilon) bounded Gauss upwind;

    div(R)          Gauss linear;

    div((muEff*dev2(T(grad(U))))) Gauss linear;

}



laplacianSchemes

{

    default         none;

    laplacian(muEff,U) Gauss linear limited 0.333;

    laplacian(Dp,p_rgh) Gauss linear limited 0.333;

    laplacian(alphaEff,h) Gauss linear limited 0.333;

    laplacian(DkEff,k) Gauss linear limited 0.333;

    laplacian(DepsilonEff,epsilon) Gauss linear limited 0.333;

}



interpolationSchemes

{

    default         linear;

}



snGradSchemes

{

    default         limited 0.333;

}



fluxRequired

{

    default         no;

    p_rgh;

}

fvOptions:

Code:

temperature_constraints

{

    type          temperatureLimitsConstraint;

    active        yes;

    selectionMode cellZone;

    cellZone      fluid;

    

        temperatureLimitsConstraintCoeffs

        {

            Tmin     263;

            Tmax     293;

        }

        

}

log:

Code:

Region: fluid Courant Number mean: 1.4132369e-05 max: 0.98128545

deltaT = 2.381967e-05

Time = 0.000100306





Solving for fluid region fluid

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

DILUPBiCG:  Solving for Ux, Initial residual = 0.00081227894, Final residual = 1.6049071e-07, No Iterations 1

DILUPBiCG:  Solving for Uy, Initial residual = 0.07792845, Final residual = 1.8250737e-05, No Iterations 1

DILUPBiCG:  Solving for Uz, Initial residual = 0.0014009406, Final residual = 3.9984243e-07, No Iterations 1

DILUPBiCG:  Solving for h, Initial residual = 0.000399081, Final residual = 8.990734e-08, No Iterations 1

Min/max T:262.29196 299.81974

Min/max rho:1.1716795 1.347332

GAMG:  Solving for p_rgh, Initial residual = 0.0007644805, Final residual = 1.345729e-05, No Iterations 3

GAMG:  Solving for p_rgh, Initial residual = 6.2938682e-05, Final residual = 1.757067e-06, No Iterations 2

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (fluid): sum local = 3.6194871e-09, global = -1.1723455e-09, cumulative = 9.1079573e-09

Min/max rho:1.1709893 1.3499513

GAMG:  Solving for p_rgh, Initial residual = 1.1436979e-05, Final residual = 3.3044886e-07, No Iterations 2

GAMG:  Solving for p_rgh, Initial residual = 2.5426255e-06, Final residual = 4.4810886e-08, No Iterations 2

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0

time step continuity errors (fluid): sum local = 9.2017652e-11, global = -1.1644798e-11, cumulative = 9.0963125e-09

DILUPBiCG:  Solving for epsilon, Initial residual = 4.9736441e-05, Final residual = 2.2259148e-08, No Iterations 1

DILUPBiCG:  Solving for k, Initial residual = 8.5244714e-13, Final residual = 1.2977543e-16, No Iterations 1

bounding k, min: 4.9998752e-16 max: 1.15 average: 0.0022126182

Any comments about this?

V.

Typically in a CHT analysis, the system directory will have subdirectories for each region. Did you put the fvOptions file in the relevant subdirectory? Also, at the top of the log file, OpenFOAM will tell you what it has read from the fvOptions file.

*UPDATE*
Same behavior here. Doesn't seem to limit the temperature at all.

Quote:

Originally Posted by crmccreary (Post 501622)

Did you put the fvOptions file in the relevant subdirectory?

Yes.

Quote:

Originally Posted by crmccreary (Post 501622)

*UPDATE*
Same behavior here. Doesn't seem to limit the temperature at all.

Well, in my case the wrong max/min temperatures in the domain appeared to be related to the externalWallHeatFluxTemperature boundary condition, which is evidently affected by some bad implementation issue in the OF-2.2.x branch and goes always unstable unless an EXTREMELY fine near wall grid is arranged (I've checked this behavior for a simple 2D buoyancy driven cavity flow, see this tread for further details: http://www.cfd-online.com/Forums/ope...tml#post496092 ). Regarding the fvOptions temperature constraint, I haven't investigated it any further so I cannot add more useful information about it.

Best

V.

I was using the 2.3.x branch. Temperature in the solid blows up, not obeying the fvOptions limit. I suspect that, for some reason, diffusion at the boundary becomes zero thus zero heat flux at the boundary and the applied heat flux (fixed gradient on the solid) yields a near infinite temperature on the solid. Just a guess.

THis does work in chtMultiRegionSimpleFoam in V2.3.1

in conjunction with scalarSemiImplicitSource
to construct a heat source limited by temperature

the comment in header file gives the wrong names for the coeffs it is Tmin and Tmax
not maximum and minimum.

Code:

   Temperaturelimit1

         {

        type            temperatureLimitsConstraint;

        active          true;

        selectionMode   all;

        

     temperatureLimitsConstraintCoeffs

        {

            Tmin     200;

            Tmax     340;

        }    

        

     }    

    energySource1

    {

        type            scalarSemiImplicitSource;

        active          true;

        

        selectionMode   all;

    

       

        scalarSemiImplicitSourceCoeffs

        {

            volumeMode      specific;

            injectionRateSuSp

            {

                h           (  20000 0 ); // 2e4 = 20w/litre

            }

        }

    }

Adding a fvOptions file in system folder with :

Code:

temperatureLimit

{

    type limitTemperature;

    active true;



    limitTemperatureCoeffs

    {

        selectionMode all;

        min <Tmin>;

        max <Tmax>;

    }

}

seems to resolve the issue.

Hi everyone

My simulation in OF v1806 using rhoSimpleFoam crashed after very few iterations due to divergence in temperature. After limiting the temperature the solver runs very well.
Now the same simulation has a very similar behaviour in foam-extend 4.0 when using dbnsTurbFoam. When I tried to apply limits I realised that fvOptions is not available in the foam-extend version. Does anyone know a work around or how I can apply limits?
Many thanks.

Limit temperature within the inner loop?

Is there a way to limit temperature within the inner loop?

My temparature blows up within a loop?

I am also interested in limiting the temperature for another variable interface temperature Tf? Anybody having any ideas?
I am using interfacecomposition model in reactingTwoPhaseEulerFoam?

Thanks
Stanley