[anirudh1]

Hello,
I'm simulating early diesel injection with narrow angle injection. I have used DIESEL2 as parcel species. Due to early injection, a fuel film is formed on piston surface, so i have used wall-film model in converge to simulate this and also ticked the film-evaporation. But from the results the film on surface seems to vaporize only a little. I'm attaching the film_mass from film.out, Near-wall avg temperature for piston boundary, and also mean_temp inside cylinder. Piston boundary condition is law of wall and temperature boundary condition is 480K. Mesh size near piston wall is 0.25mm.

Do i need to refine the mesh further near wall?
Is the film model accurate ?
Why only a little of the film is vaporized ?

Kindly help.

Thanks and regards
Anirudh.

filmmass_piston.PNG

Mean_Temperature.PNG
Near_wall_avg_piston.PNG

[ksrivast]

Hello Anirudh,

The mesh sizes you're employing along the piston wall boundary seems suitable for typical diesel engine simulations. But it's always better to conduct a mesh dependence study for your cases, to see if the results improve noticeably when you refine the mesh.

I would say that the piston WALL temperatures play a bigger role and the wall seems on the colder side to me. Are you certain your wall is supposed to be at 480K and not higher temperatures which might improve film evaporation? How certain are you that your film indeed evaporates faster than it currently does in the simulation?

O'Rourke film splash model is our recommendation for ICE cases and has performed well for PFI and GDI case setups. We typically don't employ wall film models for diesel case setups as we don't expect film formation.

Sincerely,

[anirudh1]

Thank you sir for the reply. I took wall temperature as 480K because the early injection creates a HCCI like combustion where the temperatures are on the lower side.

[ksrivast]

Hello Anirudh,

If you have colder wall temperatures we would expect more film and slower film evaporation. You can have a look at your post files to see what your film parcel temperatures are and ascertain if they are still below boiling temperatures. Confirm that the liquid.dat properties are correct and the wall temperatures are in line with your expectations. Do you have a strong reason to expect much less film or its faster evaporation? How are the pressure plots/heat release/emission results matching with experimental data?

CONVERGE does have the ability to modify film heat/mass transfer to improve film evaporation. You can ramp up the values of heat_trans_coeff and mass_trans_coeff (> 1.0), under film > scaling in spray.in (Spray modeling > General > Scaling in STUDIO). But please note that this is an artificial method to improve film evaporation and typically not recommended. If you start playing around with these tuning factors you stray away from predictive CFD and start to curve-fit your CFD results.

Sincerely,

[anirudh1]

Hello sir,
Thanks for the insights.
I have taken liquid.dat file for DIESEL2 from converge example cases.
1)The pressure plot is matching well with the experimental data. The NOx emissions from extended zeldovich mechanism are under predicted.
2) The HC emissions from emissions_region0.out are not matching with the experimental Total Hydrocarbon emissions(THC) measured in lab. There is a large difference. So, i feel the difference might be due to the film evaporation.

[ksrivast]

Hello Anirudh,

Have you run multiple (consecutive) engine cycles for this case? If you're starting with initial conditions (values from initialize.in), the first cycle results might not be too accurate. You should consider evaluating your results from the 2nd or 3rd cycle to see if they match better.

Before any other further recommendations, it would be preferred if we could have a look at your setup to ensure recommended settings are being employed for such cases, and then we could work with you in order to improve your results. Please contact support@convergecfd.com. Please use your official email for all correspondence with Convergent Science. Please mention the issues you are facing, attach your case setup and add the cfd-online thread, as reference.

Sincerely,