[murilommen]

Dear Foamers,

I have been trying to simulate a non-premixed combustion on the attached geometry. The fuel enters through the small centered pipe whereas the air, through the two others on the upper and lower side.
When I was working with FLUENT, all I needed to do was specify the initial conditions, run a steady state and use it as an initial condition for the transient simulation.
Now with OpenFOAM5.0 what happens is that even though I manage to get a stabilized flow, I can't seem to find a way to ignite the reaction.
The case I have based myself to follow was reactingFoam/RAS/SandiaD_LTS

I have looked through the forum, tried (unsucessfully) to install swak4foam to ignite it artificially, but I can't seem to get it done. Am I missing something here?

Thanks!

BC's
Fuel: CH4, 301K, 3m/s
Air: 343K, 10m/s (both holes)

[murilommen]

By looking further in the forum, I have (unsucessfully) tried to ignite it by inserting an Energy Source through the fvOptions file, but I still can't seem to get it done. Next step is to try activating the energySource after the flow is stabilized.

Thoughts?

energySource1
{
    type            scalarSemiImplicitSource;
    active          true;
    timeStart       0;
    duration        0.01;

    scalarSemiImplicitSourceCoeffs
    {
	selectionMode	all;
        volumeMode      specific;
        injectionRateSuSp
        {
            T           (1700 0);
        }
    }
}

[clapointe]

Getting (stable) ignition for reacting flows can be tricky. However, there are various tutorials that use an energy source for ignition at some point (in time). Here's one example of an fvOptions file : https://github.com/OpenFOAM/OpenFOAM.../gas/fvOptions. A quick scan of yours -- use h instead of T (enthalpy). Other parameters can be taken from the file I've linked. If you're doing non-premixed combustion you might want to run without ignition for a bit to let the flow develop and mix before igniting -- this may help with stability.

Caelan

[murilommen]

Thank you for your answer Caelan!

I was trying for the past few days enabling the heat source by applying to all domain a high Temperature value after 5 seconds (and then switched to enthalpy, as you suggested). But the program will not work that way, making a combustion occur where only air gets in, even before the fluid is stabilized.

When trying to create a box cellSet using topoSetDict, I get the following error:

Create time

Create polyMesh for time = 0

Reading topoSetDict

Time = 0
    mesh not changed.
Created cellSet ignitionCellSet
    Applying source boxToCell
    Adding cells with center within boxes 1((-0.0630417 0.0240592 0.00619917) (0.000372681 -0.0200989 0.00619917))
    cellSet ignitionCellSet now size 0
Created cellZoneSet ignition
    Applying source setToCellZone
    Adding all cells from cellSet ignitionCellSet ...
    cellZoneSet ignition now size 0
End

I checked the nodes I want to create my box from and my topoSetdict file looks like this:

actions
(
    {
        name    ignitionCellSet;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-0.0630417 0.0240592 0.00619917)(0.000372681 -0.0200989 0.00619917);
        }
    }
    {
        name    ignition;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
	    set ignitionCellSet;
        }
    }

);

What else could possibly be going wrong here? Is it such a big deal to have the high enthalpy applied to all domain for a short period of time?

Thanks again!

Edit: I am using a mesh converted from the ANSYS Fluent mesher.

[clapointe]

Applying a large amount of energy to the whole domain sounds unnecessary and a good way to cause instability. The problem now looks to be that your cellSet is empty. topoSet should select cells with cell centers inside of the box for boxToCell. Make sure that you specify the bottom left and then the top right. You'll also need different z coordinates, even for a 2d mesh.

Caelan