Hi to all,

I´m a student and i´m using the fluent to simulate the combustion in a boiler for production of paper. In Gambit, for my mesh i applied the Tgrid option. In Fluent, i choose for turbulency the model K-epsilon standard, i actived the energy equation, the P1 model to radiation, i created the pdf table, i defined the injections and i choose in boundary conditions for the port where the air enters as mass flow inlet and the port for way out of the gases i choose outflow.

The problem is when i ran the program, i can´t make this converge, i tried to change some under-relaxation factors for low values (pressure- 0.2, density- 0.2), i even changed the discretization to all options, but i didn´t see much differences.

But i noted one thing, the residual values during the iterations are going reduce very slowly, but when the program actives injections the residual values raise and the lines of the residuals raise too, then reduce again, next one injection and a new raise and this goes like this way, up and down and never converge. i also try to raise the iterations between the injections, but didn´t work. The fuel is coal. I hope someone can help me.

Sorry for my english, is not the best, but i think you can get the idea of the problem.

Thank you very much Luis Coelho

Hi Luis,

sounds like you are doing the same project as me almost. I am doing a tangentially fired boiler. I too am having convergence problems, similar to your own. I have tried both steady and unsteady state, but no love. Im using the same models as you i think. Can someone suggest some plan for convergence in such a system?

Thanks, Matt

Dear Luis and Matthew,

When simulating coal boilers and furnaces, my best approach is this one:

- fully define your models (turbulence, species transport and reaction, radiation, DPM, etc.), your materials and everything else, but do not start to calculate with all models activated! first deactivate at least radiation equation from the solver controls panel;

- start with first order discretisation for all equations, for pressure use PRESTO and for pressure-velocity coupling use SIMPLEC with 1(for structured mesh) or 2-3 skewness corrections (for unstructured mesh) (this will allow you to use under-relaxation factors like 0.6-0.7 for pressure and momentum, 0.8 for density, and the rest default, DO NOT under-relax energy, not even to 0.9);

- in DPM panel select 20-25 flow iterations per DPM update (DPM iterations are so expensive that it is a total waste of time to update more often, especially when flow field is near convergence, at that moment you could even increase this number to 40-50, for faster convergence)

- converge your 1st order solution to a reasonable level (let's say 3 orders of magnitude), and then activate the radiation equation with a 0.2 under-relaxation, and also change all 1st order discretisations to 2nd order;

- request 50 iterations and then increase under-relaxation for radiation at 0.4, make 50 more iterations, increase to 0.6, and so on up to 1 (if stable, if not stay at 0.8), and then continue to iterate until residuals will settle down (actually residuals will continue to make little jumps when DPM is updated, but the mean value will remain constant).

You were complaining about residuals jumping everytime DPM is updated. I say you should be happy, because this means that your coal is really burning (every update changes temperature field which has a tremendous influence on all other variables). If your coal wouldn't burn, you should not see significant variations in residuals plots (that would be a first indication of non-burning fuel without stopping the iterations to visualize temperature field). With this method I was able to obtain full 2nd order convergence in at most 2000-2500 iterations for 150,000-200,000 elements structured grids within 7 hours on dual Opteron machines.

All the best, Razvan

What do you mean it doesn't converge? The residuals aren't really important - don't you want you want to write a paper about flue gas temperatures, heat fluxes, emissions, unburned carbon or some other interesting things for combustion in a boiler.

So have these parameters started to converge? Use the surface monitor at the outlet to look at things like temperature, O2, unburned gases (like CO) and see if they converge.

Has essentially all of your fuel burned out? Does the energy balance, balance? Do you have the correct mass flow of fuel? Air?

Some boiler configurations will not have a steady-state solution.

My experience with the P1 radiation model is that it can diverge with underrelaxtions higher than about 0.9.

Have some patience - the first CFD boiler models we ran in the 1980's took several months of computer time to converge (well sort of).

Dear Razvan,

Thank you very much for your help, your explaination was simple and objective. I made everything as you said and the solution didn´t converge and unfortunately i didn´t get better results.

With your approach i get residual values between 1 and 2 order of magnitude and with my best approach (pressure-velocity: simple; pressure: standard and the rest in first order upwind) i get values between 2 and 3 order, with 2500 iterations for both cases.

You said i should get convergence for 150,000-200,000 elements structured grids, but I only have 66,000, maybe this can get some influence?

I would like to know if it is possible change the mesh next to the iterations, for example, i made my simulation, but for some reason i concluded that mesh it wasn´t the best, can i change it without make a new case in fluent?

Finally one last question about changing the injection of fuel, i have coal (solid fuel) and if i change for black liquor (liquid fuel), i have to create again the pdf mixture and change the type of fuel injection (off course), but when I define the material type (define - materials) should I choose combustion particle? The burning of a fluid combustible could be considered combustion particle?

All the best, Luis

Dear Luis,

The size of the grid could influence convergence in this way: a denser grid could cause you problems by revealing more phenomenology in the simulated problem and this way generating local unsteadyness, but this is generally not true when using very diffusive turbulence models like standard k-e. A coarse grid will allways provide you with a greater specific rate of convergence, and also more stability. But you could miss some important phenomena in the same time...

Personally, I dont't know any method to build a new grid and "transfer" all settings from an old case without first making a journal file during the setup of that old case. In my opinion you will have to do it all over again this time. All you could profit from the old case is to interpolate that old solution on your new grid.

When burning liquid fuel, you have to define it as "droplets". All other settings could remain the same, if relevant.

All the best, Razvan

Hi Razvan, thanks for the reply. I'm trying your advice.

-Matt

Hi, the injection is also a problem for coal gasification. Sometimes it converges and sometimes not. You should first try to get the gas phase calculation converged, meaning that you deactivate your injection and add the amount of coal to your coal carrying gas (probablely you are using N2). After that has converged you should start replacing your gas-coal slowly to solid coal (you add e.g. 2kg/s of coal to your injection and subtract the same amount from your gas-coal). also you should use very low URF for your DPM such as 0.02. Hope that will help a little bit to get closer to the solution. And residuals are not the only thing to look at as Allan has mentioned it. I usually plot the exit temperature and the velocity as well as the interior temperature to make sure to get a good solution. Plotting species is maybe not such a good idea since it will slow down your calculation. Good luck. Claud

Hi Claud,

i´m going try to do that. It´s one more possibility, but i don´t have a good experience to get the solution by the exit temperature or the velocity. Thank you very much for your help.

All the best. Luis

Dear Razvan

Thank you very much for you help and disponibility.

All the best Luis

[neil_007]

hi. does any one knows how to do the material and energy balance for whole boiler manually?