CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Spray slows then stops

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 30, 2007, 10:51
Default Hi All, Quick problem with
  #1
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
Hi All,

Quick problem with dieselFoam (1.4). I have been using it for some time with various mesh geometries with few problems. However, now I've moved to a slightly more complex 2D mesh and things are acting weird.

I have evolved the surrounding fluid motion (basically a 0.5 mach inlet and the rest is treated as atmosphere) and that works great. Then I try to add spray parcels. Works great for awhile, but then slows down systematically until eventually it simply stops ...

Number of parcels in system | 440
Injected liquid mass....... | 0.0103776 mg
Liquid Mass in system...... | 1.03557e-05 mg
SMD, Dmax.................. | 2.7153 mu, 5.63648 mu
Added gas mass = 0.0103673 mg
Evaporation Continuity Error| 1.36701e-09 mg
ExecutionTime = 3101.49 s ClockTime = 3102 s

Courant Number mean: 0.00151049 max: 0.1
deltaT = 8.33333e-10
Time = 0.000367034

Evolving Spray
Solving chemistry
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for O2, Initial residual = 0.00121118, Final residual = 1.51818e-07, No Iterations 1
DILUPBiCG: Solving for H2O, Initial residual = 0.0012151, Final residual = 4.41561e-11, No Iterations 2
DILUPBiCG: Solving for CH3OH, Initial residual = 0.00121093, Final residual = 4.31205e-11, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.00016995, Final residual = 1.44393e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.000217713, Final residual = 3.62283e-10, No Iterations 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 6.47539e-13, global = 2.01274e-13, cumulative = 5.49663e-11
DICPCG: Solving for p, Initial residual = 9.78815e-07, Final residual = 1.86921e-12, No Iterations 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 3.46536e-15, global = 1.83133e-17, cumulative = 5.49663e-11
DILUPBiCG: Solving for epsilon, Initial residual = 1.59889e-06, Final residual = 1.3528e-10, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 2.62404e-06, Final residual = 5.55037e-10, No Iterations 1

Number of parcels in system | 441
Injected liquid mass....... | 0.0103777 mg
Liquid Mass in system...... | 1.03792e-05 mg
SMD, Dmax.................. | 2.71403 mu, 5.63648 mu
Added gas mass = 0.0103673 mg
Evaporation Continuity Error| 1.37104e-09 mg
ExecutionTime = 3115.53 s ClockTime = 3116 s

Courant Number mean: 0.00151049 max: 0.1
deltaT = 8.33333e-10
Time = 0.000367035

Evolving Spray

... it just randomly stops here. it has occured to me that i am really injecting WAY too many parcels per unit time since my mesh is fairly fine and my time steps are ridiculously small. i have never figured out how to not have the sprayer inject a parcel every time step.

(injected mass is greater because i had the spray mass way down to turn it off while the fluid motion was solved before adding spray parcels)

my injector looks like ...

commonRailInjectorProps
{
position (0.0008 0.000125 0);
direction (1 0 0);
diameter 0.00008;
mass 1.41372e-8;
// mass 1e-20;
injectionPressure 125.0e+05;
temperature 295;
nParcels 1;

X
(
0.5
0.5
);

massFlowRateProfile
(
(0 1)
(5e-4 1)
);

injectionPressureProfile
(
(0 1)
(5e-4 1)
);
}

and my spray properties are pretty standard (no difference between these and the aachembomb case). my droplets are pretty small (3 microns in diameter), but i have simulated 3 micron droplets before in various other 3d meshes using the same basic setup.

i have combustion and chemistry turned off. droplets are comprised of ...

liquidFuelComponents
(
H2O
CH3OH
);

H2O H2O defaultCoeffs;
CH3OH CH3OH defaultCoeffs;

fvSolutions are the same as aachembomb with the exception of having the momemtumpredictor turned off.

any thoughts here would be greatly appreciated.

anthony
coastal593 is offline   Reply With Quote

Old   July 30, 2007, 13:31
Default thinking that perhaps this was
  #2
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
thinking that perhaps this was related to the high density of parcels, i increased the courant limit from 0.1 to 0.5, and found that the simulation stopped moving at a much lower parcel count, this time at 135 (at 0.1 it was in the 400s, as indicated above).

this seems quite strange to me. anyone have any insight? i don't see anything wrong with the simulation until this occurs.
coastal593 is offline   Reply With Quote

Old   July 30, 2007, 15:46
Default after pooring over some of the
  #3
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
after pooring over some of the spray code i've thought that perhaps this could be due fundamentally in my definition of the 2D domain.

in spray.C i see code segments responsible for deciding on whether or not this is a 2D case based on the existence of a wedge or symmetry plane. my case has neither. it is a fairly complex 2D mesh with empty defined for the front and back of the simulation volume.

is this not appropriate for the simulation of sprays? i think because of this it is constructing a 3D injection.

if so, is there a reasonable way to correct this?
coastal593 is offline   Reply With Quote

Old   July 31, 2007, 10:41
Default so far as I can tell the probl
  #4
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
so far as I can tell the problem boils down to "i need to construct a 2D spray in a case with no wedge defined. it seems in spray.C that the only case treated as 2D is when a wedge is defined. anyone have any idea how i might force this? i really can't go to a wedge due to the asymmetry of the case.

ac;
coastal593 is offline   Reply With Quote

Old   July 31, 2007, 14:27
Default i have confirmed that this is
  #5
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
i have confirmed that this is in fact the issue. same configuration and mesh works fine in 3D.

is there really no way to construct a 2d spray injection for nonaxisymmetric domains?

this has been quite the lively discussion so far ... but if anyone has *any* insight i would greatly appreciate it.

thanks!
anthony
coastal593 is offline   Reply With Quote

Old   July 31, 2007, 14:48
Default Dear Anthony, in my persona
  #6
Member
 
Tommaso Lucchini
Join Date: Mar 2009
Posts: 82
Rep Power: 8
lucchini is on a distinguished road
Dear Anthony,

in my personal opinion, the simulation of a 2D non axisymmetric spray is quite unrealistic. Generally 2d simulations are performed for axisysimmetric cases or wedges (see for examples papers by Rolf Reitz, Nordin and the book "Modelling engine spray and combustion processes" by Stiesch).
Should it be possible for you to simulate a wedge instead of a 2d geometry?
You can also post a picture of the grid if you would like some more suggestions.
Furthermore, please study the dieselSpray class in detail. It might be useful for you to better understand the problem you want to simulate.

Regards.

Tommaso
lucchini is offline   Reply With Quote

Old   July 31, 2007, 16:14
Default typically i have done all my p
  #7
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
typically i have done all my previous spray work in 3D and i suppose it will be beneficial in the future for me to return to that.

unfortunately this is really not an axisymmetric geometry that i'm trying to work on so i suppose 3D may be my only option. the reason i was working in 2D was because i was using it as a test bed for a couple of new subroutines i'm writing into the dieselSpray classes before moving back into 3D at significant computational cost.

thanks for your thoughts.
anthony
coastal593 is offline   Reply With Quote

Reply

Thread Tools
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
EFD.V5 stops calculation Martin FloEFD, FloWorks & FloTHERM 2 May 16, 2008 04:40
CFX stops.. Beno CFX 6 January 6, 2004 17:48
Build stops! Michael Bo CFX 3 September 16, 2003 22:02
Why the solution process stops? Julie Polyakh CD-adapco 4 February 20, 2003 09:18
Phoenics stops in the middle of a run ? leon Phoenics 4 August 30, 2001 20:47


All times are GMT -4. The time now is 09:24.