[rap7or]

Hello everyone,

for my Bachelor Thesis I am conducting a CFD Analysis of a combustion process (it's basically a rocket engine -> combustion chamber and laval-nozzle). The programm is Ansys Fluent, and the process has the following parameters in reality:

Mass flow of Fuel-Oxygen-Mixture: 0.02 kg/s
Fuel-Oxygen Ratio: 1:3.4
Fuel: Kerosene
Chamber Pressure: 8 bar
Exit Temperature: 3,000 °C
Exit Velocity: ~ 2500 m/s

In my analysis i use the following settings:
Pressure based solver
Steady-State
Standard k-e
Species: Kerosene-Air Mixture Template
Density: Real-Gas-Peng Robinson
Reactions: Volumetric -> Finite-Rate/Eddy Dissipation

Boundary conditions of the inlet:
150m/s, 0.28 Kerosene, 0.78 Oxygen, 250K, 20% Turbelent Intensity

Methods: Everything on Default, except PRESTO!
Controls: Default


I first run it without reactions, then I patch the interior to ignite the mixture. But everytime after the first step it diverges to a floating point exception.

Do you guys have any recommendations for my analysis with real gas combustion?

[LuckyTran]

Diverging in 1 iteration means you ignition patch is really bad. What variables do you patch? Make sure you patch all the relevant variables to avoid an inconsistent solution (don't forget progress variable).

Try playing around with different ignition strategies, altering the location of the patch, etc. It's not always necessary to ignite with a very high temperature. Just for learning, you can try patching a very low temperature like 250K it won't ignite, but it probably will still blow up.


Try (separately) setting the urf for energy to a ridiculously low value like 0.0001 to see if you can make it past 1 iteration. If this works, then you can probably brute force your way through by slowly ramping the urf.

[JBeilke]

There is probably no need to use real gas when you have only 8 bar pressure and such a high temperature. I would try to get it running with ideal gas at first. When you are able to get some results you can try it with realgas and compare both results.

[rewol]

Few things that comes to my mind:

* 8 bar can be considered as low pressure since fluids are not in super-critical or trans-critical state.
* If you are using steady state, MAKE SURE you also patch a species field for reaction products. Steady-state combustion cases depends highly on initial solution.
* If your geometry is not too complex, i would just patch the entire domain with a spark like, 2000 - 2500 K. But note that this would cause the computation time to be longer.
* I recently completed my study on real-gas combustion and utilized density-based solver which worked very well in my case (RCM1B, benchmark). You can try that too.
* Realizable k-e model is more suitable for jet flows, if my memory serves. But you should keep everything standard at first to see where the problem is.
* Reaction zone must be meshed finer compared to far field to capture combustion physics more accurately. Also try FOU discretization, since RG EOS models will be computationally heavier. Fine meshing in reaction zone could make up for first order accuracy.
* Try Redlich-Kwong at first. It doesnt utilize acentric factor for density computation and can make your simulation take less time.
* I did not start with the cold flow simulation but if you are going to start with CF, make sure you patch product species field.
* You can calculate an initial solution with NON-PREMIXED MODEL and continue with species-transport model later on.

I' ll update if anything else comes to my mind.

Good luck.

[rap7or]

Originally Posted by rewol

Few things that comes to my mind:

* 8 bar can be considered as low pressure since fluids are not in super-critical or trans-critical state.
* If you are using steady state, MAKE SURE you also patch a species field for reaction products. Steady-state combustion cases depends highly on initial solution.
* If your geometry is not too complex, i would just patch the entire domain with a spark like, 2000 - 2500 K. But note that this would cause the computation time to be longer.
* I recently completed my study on real-gas combustion and utilized density-based solver which worked very well in my case (RCM1B, benchmark). You can try that too.
* Realizable k-e model is more suitable for jet flows, if my memory serves. But you should keep everything standard at first to see where the problem is.
* Reaction zone must be meshed finer compared to far field to capture combustion physics more accurately. Also try FOU discretization, since RG EOS models will be computationally heavier. Fine meshing in reaction zone could make up for first order accuracy.
* Try Redlich-Kwong at first. It doesnt utilize acentric factor for density computation and can make your simulation take less time.
* I did not start with the cold flow simulation but if you are going to start with CF, make sure you patch product species field.
* You can calculate an initial solution with NON-PREMIXED MODEL and continue with species-transport model later on.

I' ll update if anything else comes to my mind.

Good luck.

Hey, thanks for your input. I figured most problems out. I used the n-octane template and eddy-dissipation model. The difficulty is, that the combustion educts are fuel and oxygen (o2) and not air. If I use the templates, i get far to high combustion temperatures. I then calculated a chemical formula including other products such as OH, CO etc. and the combustion temperature is now fine.

But it tells me now that at 3,500 K cp errors occur ("invalid cp (-1.173087e+03 J/kgK) for n-octane-vapor at temperature 3441.983280 K"). My cp law is "mixing law". Do you have any ideas how I can fix that?

[rewol]

* If your reactions are 1 or 2 step, over prediction of temperature is normal due to missing intermediate species and radicals that would be produced / consumed. You can implement your own mechanism thru FLUENT though, with appropriate reaction rate constants.

* As for your Cp values, are you using IDEAL GAS or REAL GAS EOS for your simulation ? If your CP values are calculated through polynomials, maybe you should arrange your polynomial constants since they differ with temperature ranges. Make cp constant and try it like that at first.

* If you are utilizing REAL GAS EOS, than all your thermodynamic properties are now function of density, pressure and species concentration along with temperature so make sure they are reasonable as well.

And please explain how you overcome which problem in detail because it may be very helpful to those who are interested, including me : )

I can be of more assistance if you could send me your case file.

Good luck.

[rap7or]

* I use ideal-gas now.

Here are the changes I made:

* Mesh Refinement in crucial areas
* Ideal Gas Law
* Detailed template modification of reaction products and mole fractions in the reaction definition (I added: H, H2, OH, H, CO and 02 (unburnt) to the products and updated all mole fractions, which I calculated from an old NASA Calculator "CEARUN")
* Eddy-Dissipation model (it auto-ignites basically)
* 1-Step reaction
* Decrease of inlet velocity
* Using the density-based solver
* 2D Axisymmetric geometry for testing (less nodes) and finding the right settings faster

[rewol]

For invalid cp issue, check your NASA POLYNOMIAL's.
If you can't fix it, you can just write a simple UDF for specific heat with mixing law as well. It is simply weighted sum of species specific heats.

Polynomial constants can be found from many combustion books or NIST database.

Make sure you investigate other sources for unreasonable cp values in FLUENT FORUM section as well.

Good luck.

[rap7or]

I figured these issues now cpompletely out. I have now a question regarding combustion.

I want to run this simulation now transient, but there are a few problems:

*Fuel: Jet-A, Oxidant: Oxygen (O2) | The templates in Fluent only contain fuel-air mixtures. When I take the kerosene mixture for example and remove nitrogen from the inlet species (0.2 Jet-A, 0.8 Oxygen) I get far too high combustion temperatures.

*I tried my own template where I added CO2, CO, OH, etc. to the combustion products and the combustion temperature was fixed, but the combustion itself got extremely weird (see pictures -> in comnparison with the standard template it immmidiately burns all the fuel and the velocities of the flame is incredible high) and very soon a floating point exception was the result.

*What do I have to do, to run the transient combustion of Jet-A and O2 with the right temperatures and the right reaction mechanism, that the pressure and velocity are right like with the standard mixture templates?

* The species come basically premixed into the combustion chamber (1/3.4 F/O) with a inlet velocity of around 80-100 m/s and burn at 3500K and 9 bar pressure. The exhaust gets accelerated by the laval nozzle. I use the species transport eddy-dissipation model. I need to eject inert gas at an other place, so i cannot use other species models.

[rap7or]

I do have another question regarding transient combustion.

In Fluent, the only mixtures I find are fuel-air mixtures. I use the n-Octane-Air mixture. In my case, the fuel is burnt with an oxidizer (Oxygen O2). They are premixed and get injected into the combustion chamber.

* I use the species transport volumetric reaction model (Eddy-Dissipation) and want to conduct a transient combustion.
* When I set the inlet species without N2 (0.2 Fuel / 0.8 O2) i get far too high combustion temperatures (>5000K)
* I decided to add CO, OH, H2 etc. to the combustion products of the reaction-template and adjusted the chemical equation (mole equilibrium)
* If I then run the simulation, the temperature is correct, but the combustio nis completely screwed (dramatic pressure and velocity increase and the temperature is exactly opposit distributed, PIC2)
* If I run the original n-octane-air template with nitrogen I get correct results (PIC1)

[rewol]

A quick question:
Does your "edited" mechanism include more than 2 reactions ?
If so, EDM would yield incorrect results because it assumes reaction rates for all reactions are equal which is not realistic.

[rap7or]

I just found the combustion problem: I calculated the edited one from an old NASA calculator (CEARUN) which included unburnt oxygen as an product of the combustion. If I exclude O2 from the reaction products (even though the fraction of unburnt O2 is low, the problem disappears).

But appearantly the equilibrium is now not fulfilled. Now my question is, if there is an calculator or a way to calculate a chemical reaction equation of kerosene (c8h18) containing byproducts like co, h2, oh etc. and not an ideal combustion with only h20 and co2 left?

[rewol]

For a single step reaction, you can use the formulation for general hydrocarbons to obtain the reaction with species, such as:

CxHy = a(O2 +3.76N2) -> bCO2 + cCO + dH2O + eH2 + fO2 + 3.76N2

where a, b, c, d, e and f depend on whether the stoicihometry is less or more than 1. You can read Turns book (introduction to combustion) for more details.

Or you can simply look for kerosene oxygen mechanisms from literature.