[karam]

Hi Foamers~

I want to simulate coal combustion simulation in a furnace.

So, I decided to use coalChemistryFoam.
Before I simulate real furnace, I tested some cases.
coalChemistryFoam tutorial just contains closed chamber case.

My combustion furnace has 1 inlet & 1 outlet. (Simple geometry - cylinder)
I made furnace mesh file by star-CD ver.4

There are 2-type of mesh.
1. tetrahedral ~ 30,000 cells
2. polyhedral ~ 10,000 cells

However, OpenFOAM(coalChemistryFoam) does not work for this mesh!!
(I mean "janaf-thermo error")

checkMesh utility says "mesh is ok"

my boundary conditions like this ( Attachment )


For Hexahedral mesh, coalChemistryFoam is always OK.........

HOW CAN I USE coalChemistryFoam in tetrahedral or polyhedral mesh......

[kalle]

I've never used coalChemistryFoam, but you should maybe have a look at your pressure boundary conditions. Typically you can start with putting a fixed pressure at the outlet and zero gradient on walls and inlets.

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

internalField   uniform 100000;

boundaryField

{
    wall_1
    {
        type            zeroGradient;
    }
    inle_2
    {
        type            zeroGradient;
    }
    outl_3
    {
        type            fixedValue;
        value           uniform 100000;
    }
}

Your velocity data file is named 'Untitled', usually you would name it 'U'

Good luck,
Kalle

[yingkun]

Hi,karam
I am using coalChemistryFoam too,and I have two inlets/one outlet,and I met the problem of "attempt to use janafThermo<equationOfState> out of temperature range...",have you ever encounter with it?

[schmidt_d]

Foamers,
Usually, this error occurs when low temperatures (below room temperature) occur in the solver. The solver can't look up properties and throws an error.
-DPS

[amin_jalalian]

Hi Foamers
I am working with coalChemistryFoam with an IFRF furnace with 2 inlet and 1 outlet. I disabled limestonParcels because I dont have it in my case. In "coalCloud1Properties" in folder "constant" which is main file in adjustment of coal injection, I chose patchFlowRateInjection for injectionModels, but I didn't find any tutorial that use this injectionModel. In this model we have some cases:

type patchFlowRateInjection;
massTotal 10;//added
parcelBasisType number;//mass;
SOI 0;//added
patchName in_1;
duration 100; // NOTE: set to 1 for steady state
concentration 0.0005077;//0.08198;;0.01
parcelConcentration 1e3;

Is this cases sufficient for patchFlowRateInjection?
Why particles didn't come in?

Cloud: coalCloud1
Current number of parcels = 0
Current mass in system = 0
Linear momentum = (0 0 0)
|Linear momentum| = 0
Linear kinetic energy = 0
model1:
number of parcels added = 0
mass introduced = 0

JANAFTHERMO errors without entering any particle occurs,why? I have changed kinetic, deltaT but yet there is janafThermo error and no entrance of particles.

[openfoammaofnepo]

Dear Amin,

I also use coalChemistryFOAm for the IFRF furnace (non-swirling B1 flame). Below is my setting for the injection model:

    injectionModels
    {
        model1
        {
            type            patchInjection;
            massTotal       2;               // total mass, [kg]
            SOI             0;                 // start-time of the injection
            parcelBasisType mass;
            patchName       INLET_035;
            duration        1000;              // [s]
            parcelsPerSecond 25e4;              // [parcel/s]
            U0              (40.7 0 0);        // [m/s]
            flowRateProfile constant 0.0589;   // [kg/s]
//            massFlowRate constant 0.0589;
            sizeDistribution
            {
//              type        fixedValue;        // monodispersed coal particles
//              fixedValueDistribution
//              {
//                  value   63e-6;
//              }
                type        RosinRammler;      // polydispersed coal particles
                RosinRammlerDistribution
                {
                    minValue        5e-06;
                    maxValue        200e-6;
                    d               63e-06;
                    n               1.5;
                }
            }
        }
    }

I think patchInjection should also work. How about your choice?

Originally Posted by amin_jalalian

Hi Foamers
I am working with coalChemistryFoam with an IFRF furnace with 2 inlet and 1 outlet. I disabled limestonParcels because I dont have it in my case. In "coalCloud1Properties" in folder "constant" which is main file in adjustment of coal injection, I chose patchFlowRateInjection for injectionModels, but I didn't find any tutorial that use this injectionModel. In this model we have some cases:

type patchFlowRateInjection;
massTotal 10;//added
parcelBasisType number;//mass;
SOI 0;//added
patchName in_1;
duration 100; // NOTE: set to 1 for steady state
concentration 0.0005077;//0.08198;;0.01
parcelConcentration 1e3;

Is this cases sufficient for patchFlowRateInjection?
Why particles didn't come in?

Cloud: coalCloud1
Current number of parcels = 0
Current mass in system = 0
Linear momentum = (0 0 0)
|Linear momentum| = 0
Linear kinetic energy = 0
model1:
number of parcels added = 0
mass introduced = 0

JANAFTHERMO errors without entering any particle occurs,why? I have changed kinetic, deltaT but yet there is janafThermo error and no entrance of particles.

[amin_jalalian]

Hi Dear openfoammaofnepo,

At last I couldn't use patchFlowRateInjection and I used patchInjection too.

I saw your code settings. I have some questions Can I ask you?

1-What is difference between flowRateProfile and massFlowRate? I used both of them. I think flowRateProfile is only the shape of profile, and massFlowRate is the flow rate. Is it true?

2-What is difference between massTotal and multiply of duration and massFlowrate (or flowRateProfile what you have used)= duration*massFlowRate? I think they must be equal. I set magnitude of mass total =20*0.004583333=0.09167
Is it true?

3- Why you have used parcelsPerSecond=25e4? Is this number a guess or not? If not what is its basic?

4-When you stop the code and run again do you set SOI to last result time which you have? I test it one time and I put SOI zero, I saw that code inject all parcels that must be injected from zero to reRun time.

Thank you because of your reply.

This is my code settings

type patchInjection;
massTotal 0.09167; //added
parcelBasisType mass; //;number
SOI 7.23; //0;//added
patchName in_1;
duration 20; // NOTE: set to 1 for steady state
U0 (26 0 0);
massFlowRate 0.004583333;//kg/s
parcelsPerSecond 1e5;
flowRateProfile constant 1;

[openfoammaofnepo]

Dear Admin,

1- flowRateProfile can allow us to specify the time evolution of the flow rate.

2- Yes, I think so.

3- I use that to control the number of the parcel, This is initially a guess and I adjusted it based on the accuracy and cost.

4- I am not sure for this.

In the IFRF furnace, how did you ignite the pulverized coal flame? It seems very difficult to ignite it. My case is flame B1 from IFRF furnace No. 1. I first inject the coal particle, and also the hot air streams. Then set "topoSet" to set a pocket with high temperature (say 1800K or 2000K). However, the flame is always not ignited. Did you meet the same problems?

Originally Posted by amin_jalalian

Hi Dear openfoammaofnepo,

At last I couldn't use patchFlowRateInjection and I used patchInjection too.

I saw your code settings. I have some questions Can I ask you?

1-What is difference between flowRateProfile and massFlowRate? I used both of them. I think flowRateProfile is only the shape of profile, and massFlowRate is the flow rate. Is it true?

2-What is difference between massTotal and multiply of duration and massFlowrate (or flowRateProfile what you have used)= duration*massFlowRate? I think they must be equal. I set magnitude of mass total =20*0.004583333=0.09167
Is it true?

3- Why you have used parcelsPerSecond=25e4? Is this number a guess or not? If not what is its basic?

4-When you stop the code and run again do you set SOI to last result time which you have? I test it one time and I put SOI zero, I saw that code inject all parcels that must be injected from zero to reRun time.

Thank you because of your reply.

This is my code settings

[amin_jalalian]

hi openfoammaofnepo,

Thanks. I put initial temp of domain 1800 K. No problem in ignition.

[anna_93]

Hey everybody, I know it´s an old topic but maybe someone can help me. I changed the injectionModels of the tutorial following your examples. If I wanna run the Simulation I always got this error:

--> FOAM FATAL ERROR:
Unknown carrier component f. Valid carrier components are:

N2
O2
CH4
H2
CO2
H2O

From function Foam::label Foam::SLGThermo::carrierId(const Foam::word&, bool) const in file SLGThermo/SLGThermo.C at line 163.


Are there any other changes I have to do?

Thanks a lot!

[Pooria]

Originally Posted by amin_jalalian

Hi Foamers
I am working with coalChemistryFoam with an IFRF furnace with 2 inlet and 1 outlet. I disabled limestonParcels because I dont have it in my case. In "coalCloud1Properties" in folder "constant" which is main file in adjustment of coal injection, I chose patchFlowRateInjection for injectionModels, but I didn't find any tutorial that use this injectionModel. In this model we have some cases:

type patchFlowRateInjection;
massTotal 10;//added
parcelBasisType number;//mass;
SOI 0;//added
patchName in_1;
duration 100; // NOTE: set to 1 for steady state
concentration 0.0005077;//0.08198;;0.01
parcelConcentration 1e3;

Is this cases sufficient for patchFlowRateInjection?
Why particles didn't come in?

Cloud: coalCloud1
Current number of parcels = 0
Current mass in system = 0
Linear momentum = (0 0 0)
|Linear momentum| = 0
Linear kinetic energy = 0
model1:
number of parcels added = 0
mass introduced = 0

JANAFTHERMO errors without entering any particle occurs,why? I have changed kinetic, deltaT but yet there is janafThermo error and no entrance of particles.

Hello Amin,

I am just wondering if you have any material describing coalChemistryFoam tutorials. My field is continuous casting but now I am supposed to work with this model for a blast furnace race way with 3 inlets and 1 outlet. However, first I need to understand the tutorial which I am struggling.

Thanks for your help.