Mixing combustion of methane and air (2D, local time stepping, with reaction particle function)

OpenFOAM 4.x

Case directory

$FOAM_TUTORIALS/lagrangian/reactingParcelFoam/counterFlowFlame2DLTS

Summary

Methane flows in from the region "fuel" and air (77% nitrogen and 23% oxygen) flows in from the region "air" at a velocity of 0.1 m/s and a temperature of 800 K, respectively. They are combusted in the analysis domain. After combustion, the exhaust gas is discharged from the region "outlet" to the outside of the analysis domain.

Model geometry Model geometry

This is the same analysis as in the reactingFoam tutorial "Mixing combustion of methane and air (2D, local time stepping)", but unlike reactingFoam, there is a file "reactingCloud1Properties" in the directory "constant" for setting the reacting particles. However, this feature is not used in this tutorial.

We use local time stepping (LTS) as a calculation method to calculate the steady state. LTS is a fast method to calculate the steady state by varying the time step for each mesh according to the mesh size. LTS function is enabled by setting "localEuler" as ddtSchemes in the file "fvSchemes" in the directory "system", as shown below.

ddtSchemes
{
    default         localEuler;
}

In the file "fvSolution" in the same directory, parameters such as the maximum width of the time step (maxDeltaT) and the max Courant number (maxCo) are set as follows.

PIMPLE
{
    momentumPredictor no;
    nOuterCorrectors  1;
    nCorrectors     1;
    nNonOrthogonalCorrectors 0;

    maxDeltaT       1e-2;
    maxCo           1;
    alphaTemp       0.05;
    rDeltaTSmoothingCoeff 1;
    rDeltaTDampingCoeff 1;
}

The chemical species and the combustion reactions with methane and oxygen are defined in the file "reactions" in the directory "constant" as follows. The properties of each chemical species are defined in the file "thermo.compressibleGas" in the same directory.

species
(
    O2
    H2O
    CH4
    CO2
    N2
);

reactions
{
    methaneReaction
    {
        type     irreversibleArrheniusReaction;
        reaction "CH4 + 2O2 = CO2 + 2H2O";
        A        5.2e16;
        beta     0;
        Ta       14906;
    }
}

These two file "reactions", "thermo.compressibleGas", are imported in the file "thermophysicalProperties" in the directory "constant" to read the settings.

The meshes are as follows, and the number of mesh is 4000.

Mesh Meshes

The calculation result is as follows.

Temperature at final result Temperature at final result
Flow velocity at final result Flow velocity at final result

Commands

cp -r $FOAM_TUTORIALS/lagrangian/reactingParcelFoam/counterFlowFlame2DLTS counterFlowFlame2DLTS
cd counterFlowFlame2DLTS

blockMesh
reactingParcelFoam

paraFoam

Calculation time

3 minutes 31.41 seconds *Single, Inter(R) Core(TM) i7-2600 CPU @ 3.40GHz 3.40GHz

Reference