CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

coalChemistryFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 6, 2009, 21:50
Default coalChemistryFoam
  #1
New Member
 
trackeras
Join Date: Apr 2009
Posts: 4
Rep Power: 9
karam is on a distinguished road
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......
Attached Files
File Type: gz BCs.tar.gz (1.4 KB, 46 views)
karam is offline   Reply With Quote

Old   November 6, 2009, 23:48
Default
  #2
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 272
Rep Power: 13
kalle is on a distinguished road
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.

Code:
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
kalle is offline   Reply With Quote

Old   June 13, 2011, 22:59
Default
  #3
Member
 
桂莹
Join Date: Apr 2011
Posts: 36
Rep Power: 7
yingkun is on a distinguished road
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?
yingkun is offline   Reply With Quote

Old   December 4, 2012, 09:58
Default Janaf
  #4
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 71
Rep Power: 9
schmidt_d is on a distinguished road
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
schmidt_d is offline   Reply With Quote

Old   July 17, 2016, 11:02
Question Injection In coalChemistryFoam
  #5
New Member
 
amin jalalian
Join Date: Mar 2014
Posts: 29
Rep Power: 4
amin_jalalian is on a distinguished road
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 is offline   Reply With Quote

Old   October 22, 2016, 19:46
Default
  #6
Senior Member
 
Join Date: Jan 2013
Posts: 310
Rep Power: 6
openfoammaofnepo is on a distinguished road
Dear Amin,

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

Code:
    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?

Quote:
Originally Posted by amin_jalalian View Post
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 is offline   Reply With Quote

Old   October 23, 2016, 09:31
Default
  #7
New Member
 
amin jalalian
Join Date: Mar 2014
Posts: 29
Rep Power: 4
amin_jalalian is on a distinguished road
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

Quote:
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;
amin_jalalian is offline   Reply With Quote

Old   October 23, 2016, 19:25
Default
  #8
Senior Member
 
Join Date: Jan 2013
Posts: 310
Rep Power: 6
openfoammaofnepo is on a distinguished road
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?


Quote:
Originally Posted by amin_jalalian View Post
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
openfoammaofnepo is offline   Reply With Quote

Reply

Tags
coal, coalchemistryfoam, poly, tetra

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
coalChemistryFoam: Where can I find more information about the models? mighelone OpenFOAM Running, Solving & CFD 4 December 5, 2015 03:36


All times are GMT -4. The time now is 14:30.