[sTeF88]

Hi everybody.
I am really happy that it is a specific CONVERGE section here in cfd-online.
I just have some questions regarding a simulation that I have to run.
I would like to simulate the combustion of premixed air/methane (stoichiometric AFR) in a constant volume chamber. My aim is to check pressure and temperature in such volume at the end of combustion cycle.
By reading some papers and other posts in this forum I have concluded that for my purpose a g-equation model could be the right choice.
So I have realized a simplified model of my physical problem, consisting in a cylindrical volume filled with a stoichiometric mixture of air and methane and a spark plug for source positioning. All surfaces were set as adiabatic wall and I just have a region in which I have inizialized the species and G_EQN (with -0.1 value). Unfortunatly the combustion does not seem to start!!!
I am pretty sure I am making some stuping mistake with my model...but since I am newbie in CONVERGE I cannot fix it.
For this reason I also attach my .cvg +input files, hoping that someone could help me to fix the problem.
Best regards and thanks in advance
sTeF88

[MCoil]

Hi -

Did you ignite the simulation by sourcing "G"?

[sTeF88]

Hi MCoil
At first, thanks for intersting to my topic.

I just followed the configuration of SI8_engine_premix_GEQN tutorial.
The main differences between my case and the former are:
- I have just one volume (the chamber volume) in which there are the methane/air mixture at ambient condition (300 K and 101325 Pa);
- So I have initialized this region with the combustion products in a stoichiometric ratio;
- Then I have modeled a spark plug (even if I think it could not be necessary), to correctly locate the source; all the walls are adiabatic slip wall;
- g-equation parameters are the same as in the tutorial (value 8e+12 1/(m3s) and max passive 0.00025); I have also positioned two fixed embedding around the source (base grid =0.004 mm, fixed1 scale=5 (the nearest to the plug) and fixed2 scale=4);
- the combustion model is the same as the tutorial; the only difference is that as Gulder fuel I have considered Methane; moreover, since I am not interested to a Crank-angle based simulation, I have set as temporal type, PERMANENT.

The simulation time is set to 0.15 ms. In all of my attempts, seem that combustion does not start. At the first time step that I write, the max temperature rise from 300 K to about 330 K, but for the successive time steps the temperature does not vary anymore.. so the combustion could not start..
Regarding your answer, I am not pretty sure what do you mean with "sourcing G". I suppose that I have done this... but maybe, I am missing something.
I hope you could help me...
Thanks in advance
sTeF88

[MCoil]

Hi -

I looked at your case, and in combust.in the combust_temp_cutoff is set to 600K. This is fine for the engine simulation, but in your case, you want to see this at 300K so that combustion runs on the cells you initialized at 300K. I did this, and the case ignited. Give it a try and let me know.

[sTeF88]

Thanks for the quick reply MCoil
That's great..Now combustion starts (obviously)...
If I can, let me ask you one more thing..
In your opinion, is this a right way to extimate the maximum pressure and temperature inside a constant volume chamber, after the combustion of a premixed mixture? Or maybe I am doing something wrong...
Thanks in advance

[egidio.cassone]

Originally Posted by sTeF88

is this a right way to extimate the maximum pressure and temperature inside a constant volume chamber, after the combustion of a premixed mixture? Or maybe I am doing something wrong...
Thanks in advance

It depends on what you want to do. With this setup you will be able to "measure" the mean temperature and pressure in the whole domain trough the "thermo.out" file. There you will find the volume-averaged pressure and the mass-averaged temperature in the your domain (the region0) in the time. you can plot these against time and find the maximum. the "Max_press" and "Max_temp" columns refers to the maximum local value of pressure and temperature.

however, we have employed a similar case to test other things and behaved very well

[shahbazsholapure]

Hi,

I am facing same problem with Ansys Fluent for performing 2D Combustion.

I have all boundary conditions as wall.

Pressure Based Solver, Transient Flow, Spark Plug On, Species Transport (Volumetric).

In Initilization, I have put the initial mass fractions of the fuel and air.

Still nothing works.