Hi:

Which is the most powerful in modeling gaseous combustion for FLUENT, STAR-CD, PHOENICS, CFX?

thank you Sincerely, Harry.

None of the above.

Hi, Tsai:

then, which one is reletively powerful?

Sincerely, Harry.

Which of the above is best for you depends on many factors such as what type of combustion application you have etc., support requirements etc....,etc. Basically these things depend on so many factors that a simple one line answer is really not sensible at all.

Having said that, you'll find results for all codes reported in the literature so all have some capability.

This is mainly for gas-phase and gas-solid phase when the solid is modelled as a lagragian stream.

Eulerian-Eulerian combustion (for fluidised or fixed beds) is possible with (to my knowledge) Fluent, CFX and Phoenics but I think in all cases you need to write at least some code - ie its not a standard feature. And its not easy....

So a good starting point is to find some literature on applications like yours and see what code they used. Even better get a demo license from the vendors and see ifyou can solve something with their code. Then choose based on price and support - this last one is very important. Support can vary alot and if you get stuck its pretty impossible to work out what the problem is and even harder to fix it. If you're application is really leading-edge then probably write your own is a painful but perhaps in the long run effective way to go.

Greg

What the heck is that supposed to mean??? Got anything useful to add.

(1). A more practical way to find out which one is better is to visit the website of the code vendor and look for the sample cases. (2). You can also study the history of each company, to see if their researchers are experts in combustion field of interest to you. (3). My suggestion is: (a). define your standard first, as a way to evaluate the code (including the support), (b). develop some standard test cases so that a code can be evaluated, to see how a code performs. (c). check the websites to see whether a vendor has experience in these test cases. If you don't see the sample test cases shown in their website, you can ask for the information.(4). This exercise does not include any real code execution at all. It should be based on the past experience, and your standard of how a good code should perform. (5). You may want to start with the simple laminar diffusion flame first. And checkout which one is easier to use, faster to converge, or more accurate. (6). For me, I would start from PHOENICS, STAR-CD,CFX and then FLUENT.

Hi,Greg:

Thank you for your help.

I saw the archives of CFD-online, and I know that you modeled combustion of methane-air in porous media(I think it is laminar premixed combustion).

Now I'm modeling the same problem with FLUENT5.4.8. I met many difficulties, for example (1)temperature of the flame is too high even if I set Cp as "mixing law" (2)very often, flame is easy to extinct. (3)convergence or stability difficulty even if I adopt points given by FLUENT documentation.

Could you give me some advice? Thank you very much.

Sincerely, Harry.

I've been having some similar difficulties using 5.5.14 recently. In my case I'm using finite rate chemistry and a gas-solid reaction module built from udfs. I'm using laminar flow. In this case I can't get my current model to ignite without diverging to 5000K.

What is your configuration? And what model's are you using??

These combustion problems are, unfortunately, very painful - as I'm all too aware of.

Greg

hi,Greg:

I'm using 5.4.8 now. In my case I'm also using finite rate chemistry and a gaseous premixed reaction (methane/air) in one very small pore. I'm using laminar flow.

After so many failares, I somewhat do not trust the capability of FLUENT to model combustion.

Sincerely, Harry.

Hi, Harry Qiu:

Could you post on your problem in detail.

Hi,Shi:

I'm modeling methane/air combustion in porous media. It is laminar premixed combustion. Can you give me some advice?

Harry.

I am not sure the most commercial CFD codes are mature enough to handle finite rate chemistry. Fluent provides coupled solver, but success is limited to very few cases. A better way to handle this in general is to write your own source term solver (e.g. LSODI) and bypass Fluent's solver. This sounds painful, but in the long run, you will be happy about your decision. Another better code is CFDRC's CFD-ACE. In the past, the code used LSODI to solve the stiff chemical kinetics. Unfortunately, they also migrated to coupled solver for efficiency. However, the code seems more capable of handling stiff kinetics than other codes.

K. Tsai,

Do you have any references for how to do this, details of LSODI solver.

I have implemented a reaction module in fluent which seems to work ok for gas-solid reactions. When I applied it to gaseous finite rate equations everything diverged rapidly. I think I need a better numerical scheme etc etc. etc. to get it to work. So your comments are of much interest. In addition I'm still having problems with Fluent's chemical solver for gaseous finite rate chemistry - its diverging too.....

Regards

Greg

LSODI, LSODE and LSODA are part of a very popular package from Sandia Lab. You should be able to find it on the web, but I am not sure they are still available for free. Other good stiff ODE solver can be used as well. Bypassing Fluent solver can be achieved using UDF. In Fluent UDF guide, there are examples on how to pass a solved solution instead of a source term back to Fluent.

Yeah I downloaded LSODE from Livermore - I think it stands for Livermore Solver for ODE's. Thanks.

I still don't fully understand what 'solution' you are talking about. Do you mean a solution to just the chemical source terms? or to the full species transport equations?

I gather you mean the former. From most equations I've seen the source terms are an algerbraic expression of the current state of the system at a particular control volume. This is what I do, thus I determine the source terms and pass them back to Fluent.

So I don't quite get at what point you need to use a stiff solver unless you want to solve the full set of species transport equations.

Could you explain a bit more in detail and describe the equations you would solve in this manner. If you are going to use the solver for iteration on the source terms could you please provide an example or a reference.

Which udf example in the manual do you refer to?

Thanks Regards

Greg

In Fluent, the source terms are always solved separated from the flow even in coupled solver (called loosely coupled). Thus, the reaction part can always be solved separately. In user-defined scalars, the equations are always solved segregatedly. But it doesn't matter if you use LSODE since you can always force the solution to be the one from LSODE after the reaction step. The idea is to use Fluent's solver for transport and LSODE's solver for reaction. I don't have UDF guide with me right now, but there is an example in the source term section that shows you how to force a solution by giving a very large dS[] term(? not sure). Note that you still need to choose a proper integration time step for LSODE. Usually it can be chosen as (cell volume)/(cell volume flow rate) or k/e, whichever is larger.

How does this reaction solution actually work??

For example say I have a reaction

CO + 0.5 O2 -> CO2

which has a high reaction rate and often causes numerical problems. The molar rate is something like:

R = Aexp(-E/RT)*[CO][O2]

and the source term for each species (kg/m3-s) is something like

Si = ki R where ki = const based on stoichometry and molecular weights etc. for each species.

In this case the source term is an algerbraic function and nothing is solved. This is the approach I understand fluent takes in calculating the source term (at least nothing else is said in the manual)

Would you mind expanding on what you are proposing LSODE would actually solve for?? An equation would be most helpful.

I have noted that many previous 1D models use LSODE, but usually for both the species transport and the reaction. I haven't seen something along the lines you suggest explicitly presented, though implicitly some papers do mention something similar but don't provide any details.

Thanks

Greg

Look at UDF guide 5.4 pp. 79.

Greg,

Look up anything in the literature about timestep splitting or fractional stepping. It's pretty common to use this for solving laminar flames with multi-species reactions.

From the sounds of it, Fluent should be able to solve the hydrodynamics and species equations (with frozen chemistry, i.e., no chemical source terms in the species equaitions, only advection and diffusion), then in a separate step solve the species equations with only the chemical source terms, and no other terms active. In this case the species equations reduce to a set of ODEs:

d(rho*xi)/dt = Pi - Li

where Pi is the rate of production of species xi and Li is the rate of loss of species Li. Pi and Li are given by the reaction rate formula as you stated. That's how these guys can pass off things to the Livermore solver and get updated mass fractions.

Unfortunately this method only works well if the timestep is sufficiently small, so convergence will either be slow or non-existent.

Dan.