Learning Forum

[ozankekul]

Hello, 

I am trying to model non premixed nh3/h2 combustion via EDC (eddy dissipation concept) model. Actually, i am not sure if i achieved to start combustion. I tried several method such as patching, using a different model for the initialization. Sometimes, i observe that the residuals relating to the radicals change during the simulation. I infer that when these residuals change, i achieved to start combustion. In this situation, the iterations take a lot of time and dont proceed. Could you help me about how can i use EDC for my simulation. How should i proceed ? By the way, i am using a reduced kinetic mechanism for the modelling.  

On the other hand, i also used steady diffusion flamelet approach but as far as i know,  i have to correct the NOx emission with unsteady laminar flamelet approach. However, when i used unsteady laminar flamelet approach after the solution was obtained from the first approach, i observe that NOx emissions dont change. Everything is same. 

Consequently, i want to model the combustion of a non-premixed nh3/h2 flame and predict the no emissions. Which way should i follow. 

if anybody helps , i apprecite a lot. 

Thanks. 

[Ren]

Using the EDC model typically takes two steps:

1. Obtain a reasonably converged solution using an "easier" combustion model such as "Eddy-Dissipation" (EDM) or EDM + "Relax to Chemical Equilibrium" (RTCE). RTCE can be selected from "Chemistry Solver" dropdown menu in the Species Model dialog box. This soluton will provide a good flow field and temperature field as a starting point for EDC.

2. Switch to EDC and continue the calculation

 

[ozankekul]

Dear Ren, 

Thanks for your suggestion. I suppose, i will not import the reaction mechanism before the "Eddy-Dissipation" (EDM) model. After i had obtained a first solution with this model, i will import the reaction mechanism and switch to EDC (Eddy Dissipation Consept) model. Is this the correct way, isn't it ? 

Thanks. 

Ozan  

[Ren]

Hi, Ozan,

Yes, you can do it as you described, i.e., EDM with some simple global reactions first, then import the detailed mechanism and EDC, 

For your information, Fluent allows to have multiple mixture materials stored in the same case and you can select/switch the mixture material to use in the "Species Model" dialog box, depending on the requirement. Please note, however, that only one mixture material can be in use at any time.

 

[ozankekul]

Hello Ren, 

I tried the methods you mentioned but for both EDM and EDM+Relax to Chemical Equilibrium, i could not get the results. From EDM to EDC, fluent closed without any reason after some iterations or solution diverged. From EDM+Relax to Chemical Equilibrium to EDC, the temperature in the combustor gradually decreased and the i think the flame extinguished. Can you share your suggestion for these situations. 

Or, can i use finite-rate/eddy dissipation model for my case? can i use a detailed reaction mechanism with this model? if yes, is the modelling easier with this model than EDC. 

Thanks, with my best regards. 

 

 

[Ren]

Hello, Ozan,

After switching to the EDC model, please double check the species boundary conditions in the inlets to make sure that Fluent has correctly mapped the species boundary conditions.

What do you mean by "From EDM to EDC, fluent closed without any reason after some iterations"? 

After switching to the EDC model from either EDM or EDM+RTCE, please try the following:

1. Solving only the species equations for, say, 50 iterations, by disabling the solution of all other equations (Solution->controls->Equations...)
2. Enabling the solution of all equations and continue the calculation.

The Finite-Rate/Eddy-Dissipation model is not suitable for a detailed chemical mechanism.

 

[ozankekul]

 

 

Hello Ren, 

Thanks for your support. I meant by “From EDM to EDC, fluent closed without any reason after some iterations”? , fluent shuts down after few iterations. Anyway, i will try the method you have mentioned. 

Moreover, which chemistry solver should i use? Stiff or Chemkin CFD solver ? And should i change the ISAT parameters? 

Thanks again. 

Ozan 

 

 

 

[Ren]

Hello, Ozan,

For larger mechanisms Chemkin-CFD solver tends to be faster. 

Usually you do not change anything for ISAT except the ISAT error tolerance. You should keep the default value of 0.001 initially and reduce the error tolerance only after a reasonably converged solution has been obtained. After reducing the ISAT error tolerance, re-converge the calculation. This process should be repeated until changes in quantities of interest are acceptable.