[mexicalense]

Hi,



I was wondering if someone could guide me regarding an issue I had for the past days.

I'm relatively new to CFD/openFOAM. I need to simulate the filling process of a hydrogen tank and see how the temperature and pressure field develops.
I'm using OF5 for this, and attached are my case files in case they're needed.
(I generated my mesh in Gmsh, so my .msh file is attached too and needs to be converted with (gmshToFoam")



The issue is that the simulation appears to run without any problem, but the temperature and pressure rise inside the tank is very small (almost nothing) regardless if I use a low or high mass flow rate inlet.

After studying, searching and debugging for a few weeks I could make the case run without crashing, still my temp and pressure do not appear to rise as expected for a hydrogen tank filling process


I try to validate my set up by replicating other papers for the same tank filling scenario where CFD was used, but without success yet. I think this might be an issue with my boundary conditions, especially p and U. But I've try several types and combinations and still my problem remains.


I would really appreciate if someone with more experience could guide me a little bit here.

Thanks.

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e6;

boundaryField
{
    inlet
    {
    type        zeroGradient;
        
    }
    
    upperWall
    {
        type            zeroGradient;
    }

    lowerWall
    {
        type            zeroGradient;
    }
 
    rightWall
    {
        type            zeroGradient;
    }
   
    leftWall
    {
        type            zeroGradient;
    }
 
    defaultFaces
    {
        type            empty;
    }


}

\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    
    
    inlet
    {

        type            flowRateInletVelocity;
        massFlowRate    0.1;       
       //rho             rho;
       //rhoInlet        0.0887;
        value           uniform (0 0 0);
  
     
    }

    upperWall
    {
        type            noSlip;
    }

    lowerWall
    {
        type            noSlip;
    }

    rightWall
    {
        type            noSlip;
    }

    leftWall
    {
        type            noSlip;
    }
 
    defaultFaces
    {
        type            empty;
    }


}

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 298.15;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform  273.15;
    }
    
    upperWall
    {
        //type            zeroGradient;

         type            externalWallHeatFluxTemperature;  
         mode            coefficient;
         Ta              uniform 298.15;
         thicknessLayers (0.005 0.02);
         kappaLayers     (0.4 0.53);
         kappaMethod     fluidThermo;
         h               uniform 10;
         value           $internalField;  //initial temperature
         kappaMethod     fluidThermo;
      
         
        
    }

    lowerWall
    {
         //type            zeroGradient;

         type            externalWallHeatFluxTemperature;  
         mode            coefficient;
         Ta              uniform 298.15;
         thicknessLayers (0.005 0.02);
         kappaLayers     (0.4 0.53);
         kappaMethod     fluidThermo;
         h               uniform 10;
         value           $internalField;  //initial temperature
         kappaMethod     fluidThermo;
        
    }

    rightWall
    {
         //type            zeroGradient;

         type            externalWallHeatFluxTemperature;  
         mode            coefficient;
         Ta              uniform 298.15;
         thicknessLayers (0.005 0.02);
         kappaLayers     (0.4 0.53);
         kappaMethod     fluidThermo;
         h               uniform 10;
         value           $internalField;  //initial temperature
         kappaMethod     fluidThermo;
       
    }

    leftWall
    {
         //type            zeroGradient;

         type            externalWallHeatFluxTemperature;  
         mode            coefficient;
         Ta              uniform 298.15;
         thicknessLayers (0.005 0.02);
         kappaLayers     (0.4 0.53);
         kappaMethod     fluidThermo;
         h               uniform 10;
         value           $internalField;  //initial temperature
         kappaMethod     fluidThermo;
         
    }
    
    defaultFaces
    {
        type            empty;
    }

  }

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       polynomial;
    thermo          hPolynomial;
    equationOfState PengRobinsonGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

mixture
{
    equationOfState
    {
        Tc        32.994;
        Vc        65.5e-3;
        Pc        1293920.25;
        Zc        0.309;
        omega        -0.220;
    }
    specie
    {
        molWeight       2.016;
    }
    thermodynamics
    {
        
        Hf  0;
        Sf  0;
        CpCoeffs<8> (6436.5105 63.161307 -0.1685728 1.5229265e-04 0 0 0 0);
   
    }
    transport
    {

        muCoeffs<8>     ( -0.135666 6.84115878e-02 -3.928747e-04 1.8996e-06 -5.23104e-09 7.4490972e-12 -4.250937e-15 0 );
        kappaCoeffs<8>  ( 2.009705e-02 3.234622e-04 2.1637249e-06 -6.49151204e-09 5.52407932e-12 0 0 0 );

             
    }
}


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

[mexicalense]

A little update and background.
My inlet mass flow rates can range from constant 0.01 to 0.1 Kg/s.
Tank dimensions are:

L = 6.6 m
Dia. = 0.7 m
Volume = 2.5933 m^3
inlet dia. = 0.005 m

The tank is designed to hold 40 Kg of hydrogen at 20 MPa (ideal gas).
Using Peng Robinson EOS I calculated the real gas mass at full condition is around 34.4 Kg @ 20MPa and 333.15 K (max temp limit for tank liner)

Assuming a mass flow rate of 0.1 kg/s, the filling time should be around 343 seconds. That's how long I set my simulation time.
But as you can see in the picture, at the end time although the temperature rise seem appropriate, the pressure only increases by 1.2 MPa from the tank initial pressure condition of 1 MPa and 298.15 K

[sapujapu]

You're using local time stepping to calculate you solution and you're just calculating 343 iterations. LTS is just another technique to obtain a steady-state solution, its not transient. If you want to calculate the transient filling process, change it from localEuler to Euler.

[Tobermory]

... or try Crank Nicholson if you want a more accurate picture of the transient behaviour. CN tends towards 2nd order (depending on how much blending you add, for stability), whilst Euler is 1st order and more "diffusive" (in time). As Sapujapu correctly points out, LTS is a pseudo-transient scheme, so the intermediate solutions before steady state are typically not physical.

[mexicalense]

Hi again
Thank you so much for your suggestions.

It fixed my issue, my bad.
Now the simulation looks good!


I'm was searching here in the forum and other websites about how to implement gravity for the rhoCentralFoam solver. Does anyone can provide guidance about how to do that??

It seems it's not as straight forward as with BuoyantBoussinesqPimpleFoam and the other buoyancy solvers.


Thanks in advanced.

[sadeghsalehi]

Hi All,
That would be great if the issue was resolved, a brief explanation is given here such that we know how the problem was solved.
Thanks