- **OpenFOAM Running, Solving & CFD**
(*http://www.cfd-online.com/Forums/openfoam-solving/*)

- - **Spray slows then stops**
(*http://www.cfd-online.com/Forums/openfoam-solving/59534-spray-slows-then-stops.html*)

Hi All,
Quick problem with 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 |

thinking that perhaps this wasthinking 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. |

after pooring over some of theafter 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? |

so far as I can tell the problso 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; |

i have confirmed that this is 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 |

Dear Anthony,
in my personaDear 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 |

typically i have done all my ptypically 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 |

All times are GMT -4. The time now is 22:08. |