Dear People,

I am currently working on Fluidised bed, I am able to simulate Cold flow model, but a major problem is faced by me, while considering Fluidised Bed accompanied by Combustion in FLUENT..can any one suggest the best that can be done on FLUENT versions of 6.0 or 6.1

With Regards, krishna..

FLUENT 6.0 and 6.1 don't allows to directly model fluidized bed combustor.

Supposing you're using FLUENT 6.1 because it implements heat balance also for the Eulerian model, you should be able to add the combustion model using UDF, even if this requires quite a long work.

You should find useful information at MFIX site:

http://www.mfix.org

where you can find a free CFD code developed by DOE which implements heat transfer and chemical reaction in granular flow.

Hi

ap

Thanks a lot for the Instant Reply, I will check that out, ap I will get back to u soon

krishna..

Dear ap,

I was able to access the www.mfix.org site, but I am supposed to simulate the Fluidised bed with Combustion only IN Fluent..so only outcome i think is UDF..can u throw some light on it.

If I am modelling Eulerian Granular model with say material sand 1 and if want to include another Granular material like say sand 2 is it possible although I tried, it is showing some like

"Error: divergence detected in AMG solver: pressure correction Error Object: ()"

I donna what is wrong

Plese Help and also Thanks In Advance!!!!

If you have to use FLUENT, you're right: you need UDF to implement combustion reactions.

Divergence of pressure correction equation is a common problem. Try doing as follows:

1. Reduce Pressure under-relaxation factor to 0.2.

2. Reduce Momentum under-relaxation factor to 0.4.

3. Try to do some iteration without secondary phases (you have to disable Volume Fraction equations in Solve->Control->Solution panel). When the solution becomes stable, activate volume fraction equations again and proceed with the calculation.

4. Increase the number of iterations for pressure.

It shouldn't be difficult to implement the model used in MFIX for combustion through UDF, but it requires some work. I don't know what are your doubts, so please post specific questions.

Hi

ap

Dear ap,

Thanks Once more for the Innovative response, I followed the steps told by you(except the step4), and I was able to obtain results...abt the Step 4, you told me to increase the number of Iterations for Pressure..how Do i go abt it..can u plz let me know..

My problem is to simulate combustion in Fluidised Bed using Fluent, as a preliminary Step I am trying out with 2 kinds of Bed materials like one is static, which I accomplish by Patching option, and the second material, I am supposed to Introduce into the domain at constant flow rate ..and therby obtain the Bubbling action of these two bed materials..will this be possible in Fluent, that too with the Eulerian Model.

Thanks in advance,

krishna..

FLUENT uses V-cycle by default for pressure. If you want to increase the number of cycles, you have to go to Solve->Controls->Multigrid, and increase the Max cycles under the Fixed Cycle Parameters group. The default value is 30, but I obtained better results increasing it.

Yes, you can model the bubbling movements of granular materials using the Eulerian Model. Pay attention to the drag correlation you use. Try Gidaspow and Syamlal correlations: they work properly in most case. You can find more information in FLUENT manual and in literature.

I'm interested in your work, if you don't mind, keep me up to date.

Hi

ap

[jimmer]

Originally Posted by ap
;108694

If you have to use FLUENT, you're right: you need UDF to implement combustion reactions.

Divergence of pressure correction equation is a common problem. Try doing as follows:

1. Reduce Pressure under-relaxation factor to 0.2.

2. Reduce Momentum under-relaxation factor to 0.4.

3. Try to do some iteration without secondary phases (you have to disable Volume Fraction equations in Solve->Control->Solution panel). When the solution becomes stable, activate volume fraction equations again and proceed with the calculation.

4. Increase the number of iterations for pressure.

It shouldn't be difficult to implement the model used in MFIX for combustion through UDF, but it requires some work. I don't know what are your doubts, so please post specific questions.

Hi

ap

Hello ap. Is it possible to run MFIX via UDF? Or dou you mean using "modified to suit your case" parts of the fortran code as UDF DLL? Also, is this fine by NETL?

If there is such a possibility would you give me your e-mail or sth to have a more detailed discussion? I try to sim a fluidized bed gasifier. THANKS A LOT

[sircorp]

Dear all.

Is there any mathematical relation between liquid viscosity, fluidising gas density and fluidizing gas velocity.

Either Empirial or Mathematical relation or any fundamental reading.

"I am trying to understand the "Heat transfer behaviour of viscous liquids under fludising gas at various viscosities and gas velocities."