[zhangxiaolin]

Hi.I am using CONVERGE to simulate the combustion in cylinder. The maximum number of the cell is set below 600k and the simulation time is very long (a few days)with 16CPUs. The time-step is mostly limited by dt_spray or piso at around dt=2e-007. Sometime "dt= 1.515837606e-007,time-step limited by 2*max_piso reached, recovering ......"

(1)I try to reduce the maximum number of the cell in AMR to 400k but the simulation time didn't change.I don't know why.
(2)I try to enlarge the "mult_dt_spray" and the simulation time also didn't change.The time step is mostly limited by dt_grow or dt_piso. There are many lines in the detailed run.log such as
"Line 547206: time-step limit =dt_piso
Line 547207: time-step limit =dt_grow
Line 547208: time-step limit =dt_spray
Line 547209: time-step limit =dt_grow
Line 547210: time-step limit =dt_grow
Line 547211: time-step limit =dt_piso
Line 547212: time-step limit =dt_grow"
I doubt if this will result in the long running time.
(3) I try to enlarge the Maximum number of PISO iterations to avoid the time-step limit =dt_piso, but the simulation time is still the same and there are many lines in run.log such as "
ncyc= 8001,dt= 3.969803126e-007, time-step limit =dt_grow

ncyc= 8002,dt= 4.962253908e-007, time-step limit =dt_grow

ncyc= 8003,dt= 6.202817385e-007, time-step limit =dt_grow

ncyc= 8004,dt= 3.876760865e-007, time-step limit =dt_grow"
I doubt if this will result in the long running time.
Thank you for your attention!

[Blanco]

Your simulation time looks normal to me if for "few days" you are considering 2 days and you are simulating the whole engine cycle... In any case "dtgrow" means that the time step is increasing, therefore there was something limiting the time step in previous steps and that's where you should look. Dtpiso as you intented is obtained when Piso scheme reached its iteration limit which is 9 by default, you can try to increase it a little bit but this doesn't guarantee that your simulation time will be less...the time step will be higher but will also tale longer to solve because an higher number of piso iterarion will be required, in "critical" condition.

In any case 600k cells for in cylinder combustion is a low Cell count in my opinion, even for a RANS simulation. What is your application? What are your engine dimensions?

Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

[Blanco]

I would add that probably the Cell distribution is not optimal because 600k cells is your maximum cell count but you have 16 cores...what is your base grid size, AMR settings and base grid cell count?

Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

[MFGT]

Originally Posted by Blanco

In any case 600k cells for in cylinder combustion is a low Cell count in my opinion, even for a RANS simulation. What is your application? What are your engine dimensions?

Well, i am below 600k cells between -70°CA and +70°CA for a peak power single cylinder simulation of engines with conventional size. So i would consider this as normal.

During inflow and injection the cell count is higher of course. But other than that, i also stay below 1 million.

However, time step sizes of x.xxe-7 usually occur only at valve closing events, injection or ignition.

[zhangxiaolin]

It is a 3D single cylinder diesel engine and the simulation is a sector which is only 1/8 of the cylinder (bore=0.1m,stroke=0.12m).The base grid size is 2mm, minimum size is 0.125mm.
Now,the simulation time is about a week , I think it is too long but I have no way to reduce the simulation time.
Thank you for your help.

[zhangxiaolin]

Originally Posted by Blanco

I would add that probably the Cell distribution is not optimal because 600k cells is your maximum cell count but you have 16 cores...what is your base grid size, AMR settings and base grid cell count?

Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

It is a 3D single cylinder diesel engine and the simulation is a sector which is only 1/8 of the cylinder (bore=0.1m,stroke=0.12m).The base grid size is 2mm, minimum size is 0.125mm.
Now,the simulation time is about a week , I think it is too long but I have no way to reduce the simulation time.
Thank you for your help.

[zhangxiaolin]

Originally Posted by MFGT

Well, i am below 600k cells between -70°CA and +70°CA for a peak power single cylinder simulation of engines with conventional size. So i would consider this as normal.

During inflow and injection the cell count is higher of course. But other than that, i also stay below 1 million.

However, time step sizes of x.xxe-7 usually occur only at valve closing events, injection or ignition.

The spray duration in my simulation is long. Is there any solution to reduce the simulation time(I do not know why reduce the maximum cell number doesn't work)?
Thank you!

[Blanco]

Originally Posted by MFGT

Well, i am below 600k cells between -70°CA and +70°CA for a peak power single cylinder simulation of engines with conventional size. So i would consider this as normal.

During inflow and injection the cell count is higher of course. But other than that, i also stay below 1 million.

However, time step sizes of x.xxe-7 usually occur only at valve closing events, injection or ignition.

During combustion phase I usually start with low cell count but I rapidly get more than 600k cells after ignition and start of combustion (spark ignition) or just after injection (compressione ignition). For a spark ignition engine, I get more than 600k cells before reaching +45° actually.

In intake stroke simulation, with injection for a pfi engine, I easily reach 1.5-1.6e6 cells

All this, however, is for a partial load case and low rpm.

Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

[Blanco]

Originally Posted by zhangxiaolin

It is a 3D single cylinder diesel engine and the simulation is a sector which is only 1/8 of the cylinder (bore=0.1m,stroke=0.12m).The base grid size is 2mm, minimum size is 0.125mm.
Now,the simulation time is about a week , I think it is too long but I have no way to reduce the simulation time.
Thank you for your help.

OK so that's not a complete cylinder case. I agree that One week it's too long for a sector analysis...I would suggest to decrease base grid size to 1 mm and lower AMR level to 3 (keeping 0.125 mm min cell size), this should help load balancing. You can also try base size 0.5 mm and AMR level =2. But even if you do that I doubt that simulation time will drop considerably...I think there is something other that increase your computational effort. how many species are you considering in you mech.DAT?

Sent from my HUAWEI TAG-L01 using CFD Online Forum mobile app

[SamWijey]

Send your case files to support@convergecfd.com and we will review the files and make some suggestions to run faster. Please use your official email address for all communications with Convergent Science.

Thanks,