CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > CONVERGE

No heat release in pfi case

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 12, 2019, 09:38
Default No heat release in pfi case
  #1
New Member
 
Join Date: Nov 2018
Posts: 5
Rep Power: 2
George.Aux. is on a distinguished road
Hello everyone,

I'm working on a pfi model based on si8 case setup. I'm using my own geometry(cylindet head, piston, liner, ports, valves, spark plug etc.). At the engine application I set up the basic parameters: bore, stroke, rod length and the target compression ratio which is around 12.9 cr since this is the maximum when thw solver didnt freeze out(valve hits the piston). At the grid control section i set up an 8mm basic grid, 750k max cell number and im using embeddings only around the injector and spark(not around the cylinder). Im using a spray model with 4 nozzel parametized with the si8 pfi case setup numbers. Im using ic8h18. Any thing else is basicly the same as the si8 pfi example.

My problems: After i run the solver i got around 50J integrated heat release during 1 cycle and the pressure in the cylinder is only 30bar. After ensight post process at the temperature plot i saw that the flame spread is not steady in every direction in the cylinder. What can be the problem?

Thanks in advance!
Attached Images
File Type: jpg received_366591254178322.jpg (54.8 KB, 11 views)
George.Aux. is offline   Reply With Quote

Old   March 12, 2019, 20:11
Default
  #2
New Member
 
Join Date: Nov 2018
Posts: 5
Rep Power: 2
George.Aux. is on a distinguished road
At the following pictures you can see the cylinder equivalence and react ratio(1st), ic8h18 mass in the cylinder(2nd), lambda(3rd), mean temperature in the cylinder(4th) and total cell count(5th).

You can clearly see that the fuel didnt burn during the combustion...I'm using 0,02mJ ignition with starting time from -25ca to -5 ca before TDC at 8000rpm.

U.i. This is just a theoritical investigation and verification process. After it works i would like to validate the model with test bench parameters.
Attached Images
File Type: jpg air-fuel equiv_react_ratio a hengerben(saját).jpg (47.4 KB, 7 views)
File Type: jpg ic8h18 species mass region0.jpg (44.7 KB, 6 views)
File Type: jpg lambda nálam.jpg (46.2 KB, 6 views)
File Type: jpg mean temp hengerben(nekem így néz ki).jpg (43.7 KB, 6 views)
File Type: jpg total cell count.jpg (43.7 KB, 6 views)
George.Aux. is offline   Reply With Quote

Old   March 13, 2019, 08:00
Default
  #3
New Member
 
jetcheve's Avatar
 
John Etcheverry
Join Date: Dec 2018
Posts: 19
Rep Power: 2
jetcheve is on a distinguished road
Quote:
Originally Posted by George.Aux. View Post
At the following pictures you can see the cylinder equivalence and react ratio(1st), ic8h18 mass in the cylinder(2nd), lambda(3rd), mean temperature in the cylinder(4th) and total cell count(5th).

You can clearly see that the fuel didnt burn during the combustion...I'm using 0,02mJ ignition with starting time from -25ca to -5 ca before TDC at 8000rpm.

U.i. This is just a theoritical investigation and verification process. After it works i would like to validate the model with test bench parameters.
Good morning - I see a few issues immediately that you can correct that will be a problem. First - your grid is likely too coarse. An 8 mm base grid is extremely coarse, unless you are using a very large engine, which seems improbable at the engine speed of 8000 RPM.

Second - Are you using AMR? You mention you only mentioned valve and spark embedding. Getting the cell count around the flame kernel and at the flame correct correct will be critical. I would recommend using grid settings similar to the PFI example case you mentioned previously.

Third - Your energy source for ignition seems EXTREMELY low. If you are actually using 0.02 mJ, I don't think you would actually achieve stable combustion. 0.02 J seems more reasonable.

Finally, if you'd post your plot of max temperature vs CAD, we may be able to get a better handle of what's going on.

Thanks!
__________________
John Etcheverry
Research Engineer
CONVERGECFD
jetcheve is offline   Reply With Quote

Old   March 13, 2019, 11:06
Default
  #4
New Member
 
Join Date: Nov 2018
Posts: 5
Rep Power: 2
George.Aux. is on a distinguished road
Thank you for your fast reply!

The recommanded base grid size was 4mm at the example so i should use that, right? And during the validation i can try with 2mm 1mm etc...I guess..

Second- Yes, I'm using AMR at velocity and temperature. Velocity: max. 3 embedding and 1.0 sub grid crit (parcel count exceed is:50), Temperauture: max. 3 embedding,2,5sub grid criteria, start from -40 end at 131 deg. The active regions are the cylinder and intake system 2.

Third- Sorry, It is 0,02J not 0,02mJ.

I attached the max temperature vs cad plot from thermo in the cylinder region.
Attached Images
File Type: jpg max temp vs cad.jpg (42.7 KB, 10 views)
George.Aux. is offline   Reply With Quote

Old   March 13, 2019, 12:10
Default
  #5
New Member
 
jetcheve's Avatar
 
John Etcheverry
Join Date: Dec 2018
Posts: 19
Rep Power: 2
jetcheve is on a distinguished road
Quote:
Originally Posted by George.Aux. View Post
Thank you for your fast reply!

The recommanded base grid size was 4mm at the example so i should use that, right? And during the validation i can try with 2mm 1mm etc...I guess..

Second- Yes, I'm using AMR at velocity and temperature. Velocity: max. 3 embedding and 1.0 sub grid crit (parcel count exceed is:50), Temperauture: max. 3 embedding,2,5sub grid criteria, start from -40 end at 131 deg. The active regions are the cylinder and intake system 2.

Third- Sorry, It is 0,02J not 0,02mJ.

I attached the max temperature vs cad plot from thermo in the cylinder region.
Hi, George. Yes, I would not only use the base grid size from the PFI example, but the rest of the embedding strategy as well (also, in particular, you will want to loosen your maximum cell count in the AMR settings).

I would also recommend taking a look at the rest of the settings in that example. That setup has worked well for similar PFI cases we have used it on. There will probably be some changes you have to make to account for the fact you are using a higher RPM as your engine speed and other things unique to your engine, but it is a good starting point.

The good news is, it seems you are getting combustion (indicated by your maximum temperature after your spark source terminates), the flame is just not propagating out from the kernel the way we would like. This could be corrected with the grid changes I suggested above. Try that and let me know if this helps you out.

Thanks!
__________________
John Etcheverry
Research Engineer
CONVERGECFD
jetcheve is offline   Reply With Quote

Old   March 13, 2019, 17:26
Default
  #6
New Member
 
Join Date: Nov 2018
Posts: 5
Rep Power: 2
George.Aux. is on a distinguished road
I just started the simulation. I hope your advices gonna works for me. Thanks in advance! It's running on an 8 core Xeon workstation with 48gb of ram. So it gonna take some time...

btw. How much hdd space do I need for case setups in engine simulation like this one? 30-40gb is enough without 3d plotting in ensight?

Last edited by George.Aux.; March 14, 2019 at 18:07.
George.Aux. is offline   Reply With Quote

Old   March 18, 2019, 03:42
Default
  #7
Senior Member
 
Tobias
Join Date: May 2016
Location: Germany
Posts: 188
Rep Power: 4
MFGT is on a distinguished road
Hi,
i am using 8 cores only as well and typical full cycle simulation takes around 2-3 days, which of course depends on number of cells etc.

Regarding the overall case size, this depends on output frequency of post files for EnSight (5-10 °CA for example) and writing intervall of textfiles (0.1 °CA for example).

You can compress the post files (and map or restart files) afterwards, so a complete case should be in the size of ca. 8 GB without EnSight postprocessed files.
MFGT is offline   Reply With Quote

Old   March 18, 2019, 09:21
Default
  #8
New Member
 
Join Date: Nov 2018
Posts: 5
Rep Power: 2
George.Aux. is on a distinguished road
Thank you for your reply MFGT!

Saidly i got this error from the solver:
JOB ABORT invoked by rank 7: ERROR: Something is wrong in function get_temp_from_table_massfrac: upper_energy_value must be greater than lower_energy_value!
upper_energy_value is -1.#IND00, and lower_energy_value is -1.#IND00.

Where should i look for the mistake?
George.Aux. is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
partially premixed combustion heat release rate per cell sqek FLUENT 0 May 16, 2017 09:04
heat release rate calculation Karthick .K FLUENT 1 February 27, 2014 20:55
Troubles with heat release rate Xavier Ponticq CFX 4 September 12, 2012 19:49
Heat flux BC in axisymmetric case kevin FLUENT 0 February 7, 2008 19:07
heat release calculation caty Main CFD Forum 1 February 4, 2005 10:28


All times are GMT -4. The time now is 18:40.