[rsoni451]

Hello Everyone,

I have setup a simulation with motored conditions in a single cylinder engine.

LES simulation is running from 300 CADs to 750 CADs with mass flow rate as the inlet boundary condition. It is running very slow(107 CADs in 60 hrs). The base mesh size is 16 mm and embedding level up to 4. So the minimum cell size is 0.5 mm.

Can anybody tell me how can I speed up the simulation. I am running it on 30 cores on a HPC.

Thanks in advance!

Bests,
Rajat

[MFGT]

Hi,

what does CONVERGE report as time step limiter? Whats your cell count during simulation? Are all your cores "real" ones, so Hyperthreadding is off?
What are your CFL settings? You can set them differently for certain more unimportant regions (exhaust port).

Regarding the cell size. I wouldnt go to 16mm base mesh, as this can affect your cell distribution in a bad manner. Can you check cell_count_ranks.out for load ballancing?

Either stick to 4mm base (1mm in cylinder, 0.5mm AMR and fixed embedding and down to 0.125mm at Spark) or 2mm base with same embedding sizes. This wont make a big difference.

But this is recommendation for RANS, LES is usually a step finer.

[rsoni451]

Hello MFGT ,

1. Where can I find the details about time step limiter?
2. Cell count is from 20k to 800k(Do you think it is less, keeping in mind that I am running LES?).
3. The cores are all real ones.

And the load balancing per core looks fine ....its almost equally divided.
4. Default CFL settings are being used i.e. vel=1, viscosity=0.5, Mach=50.

Do you have any suggestions?

And I will surely change the mesh settings as 16 mm base mesh size appears to be very big, although I am using 4 level embedding.

Thanks in advance!

Kind Regards,
Rajat

[SamWijey]

Hi Rajat,

The time step limiter information that Tobias was talking about can be found in time.out. There are many strategies to speed up a simulation but they depend on the nature of the problem analysed. Can you compare your case setup to a relevant example case? In v2.4 Studio gives you access to a wide variety of example cases so that you can start with our recommended settings.

What is the cells/processor you get ? We have seen 20000 to 30000 cells per core gives you the best speed up for engine simulations. But there are a lot of other parameters that contribute to speed up

If you think you have incorporated all recommended settings and your simulation is still slow, send your case to support@convergecfd.com

Thanks,

[rsoni451]

Hello Tobias and Sameera,

I have reduced the base mesh size to 4 mm with corresponding changes in embedding scaling. The minimum grid size being 0.5 mm.

The simulation is running now a little bit faster now . Load balancing seems to be fine. Around 175k cells on spreaded out on 15 CPUs.

The time step limiter is the convective CFL number.
Minimum time step is e-10.

But still one Crank angle is taking around 30 mins with total no. of cells 2.65 million(2.2 million intake and 0.4 million in cylinder).

Is it normal?
Is there any possibility to make it faster?

Kind Regards,
Rajat

[SamWijey]

What is the minimum time step, set at in inputs.in? I would limit that to 1e-8 for ICE cases without VOF. If your time step is reaching 1e-10, then there's something wrong with the case. Can you send your case files (*.in and *.dat files) to support@convergecfd.com? Please use your official email for all correspondence with Convergent Science.

Thanks,

[rsoni451]

Hi Tobias and Sameera,

I have increased the time step to e-8 and the simulation is running much faster now.
Thanks for the help.
Cheers

Regards,
Rajat

[hosseinamir71]

Hello everyone,
I am trying to simulate a premature air and fuel in a cylinder. Most often, during the simulation, I faced the time-step limiter of dt_cflk.
I found not much information regarding this time-step in the manual. It is mentioned that it is based on MAX_CFL_U. However, I have not yet found how it is based on. Does anyone know what this time-step is and how I can manage to control this limiter which greatly reduces my simulation time.
Thanks

[ksrivast]

Hello Amir,

The time step limit dt_cflk is set by the Conduction CFL number, which is based on the value of max_cfl_nu (Maximum Diffusion CFL limit). You can specify the value of max_cfl_nu in inputs.in. A smaller value might be more stable, but takes longer to converge. You can try increasing this value to get larger values for dt_cflk. However, if your case is similar to any of our example cases, we strongly recommend you use the value provided there.

Information on different time step limiters and how to control them can be found in Chapter 23 of our v2.4 manual.

Sincerely,

Srivastava

[hosseinamir71]

Originally Posted by ksrivast

Hello Amir,

The time step limit dt_cflk is set by the Conduction CFL number, which is based on the value of max_cfl_nu (Maximum Diffusion CFL limit). You can specify the value of max_cfl_nu in inputs.in. A smaller value might be more stable, but takes longer to converge. You can try increasing this value to get larger values for dt_cflk. However, if your case is similar to any of our example cases, we strongly recommend you use the value provided there.

Information on different time step limiters and how to control them can be found in Chapter 23 of our v2.4 manual.

Sincerely,

Srivastava

Hi
Thanks for your reply. Actually, I am simulating a flame in a cylinder using SAGE. As you said I find a similar example in the cases, which was SAGE premix case and I used the number for limiters as they are, which was 1 for CFL_U and 2 for CFL_NU. However, i again faced that it takes a lot of cycles. I mean, for just 1ms around 50,000 cycles. On 8 core CPU, it takes a week or more for me. I don't think it is normal. I hope I find some keys that I would be able to manage to make the run time fast.
Thanks

[ksrivast]

Hello Amir,

I cannot give you an idea of normal run times without looking at your case setup. However, I do offer the following suggestions to make sure you have optimal run times:

1. If your time limiter is dt_cfl/dt_cflk/dt_cfld like you mentioned before, please increase the values of the maximum cfl limits gradually. But be wary, as this might make the simulation less stable.

2. Please check if you are having too many recoveries that are bringing down your time steps. If so, you have a bad case setup with you and it needs improvement.

3. Please check your metis_map.out file and make sure you have good load balancing.

Sincerely,

Srivastava