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

- - **DieselFoam error turbulent dispersion**
(*http://www.cfd-online.com/Forums/openfoam-solving/60613-dieselfoam-error-turbulent-dispersion.html*)

Hi,
When I activate turbuleHi,
When I activate turbulent dispersion in an axisymmetric diesel spray simulation, get this error: Create time Create mesh for time = 0 Reading thermophysicalProperties Selecting thermodynamics package hMixtureThermo<reactingmixture> Selecting chemistryReader chemkinReader Reading field U Reading/calculating face flux field phi Creating turbulence model. Selecting turbulence model RNGkEpsilon Creating field DpDt Constructing chemical mechanism Selecting ODE solver SIBS chemistryModel::chemistryModel: Number of species = 5 and reactions = 1 Reading environmentalProperties Reading combustion properties Constructing Spray Selecting injectorType commonRailInjector Selecting atomizationModel off Selecting dragModel standardDragModel Selecting evaporationModel standardEvaporationModel Selecting heatTransferModel RanzMarshall Selecting wallModel reflect Selecting breakupModel ReitzKHRT Selecting collisionModel trajectory Selecting dispersionModel gradientDispersionRAS --> FOAM FATAL ERROR : request for turbulenceModel turbulenceProperties from objectRegistry failed available objects of type turbulenceModel are 0 ( ) Function: objectRegistry::lookupObject<type>(const word&) const in file: /home/ervin/OpenFOAM/OpenFOAM-1.1/src/OpenFOAM/lnInclude/objectRegistryTemplates .C at line: 122. FOAM aborting Can somebody tell me what is this about, and how can this be corrected? Thanks. Ervin |

looks like we forgot to changelooks like we forgot to change this with the new change in runTime/mesh, Henry?
in dispersionRASModel.C change the line sm.runTime().lookupObject<compressible::turbulence model> to sm.mesh().lookupObject<compressible::turbulencemod el> and 'wmake libso' in the dieselSpray-dir. worked for me N |

Worked for me too.
Thanks, Worked for me too.
Thanks, Niklas. Ervin |

Well, now I've got myself a diWell, now I've got myself a different error message:
Time = 0.000585 Evolving Spray Solving chemistry BICCG: Solving for Ux, Initial residual = 0.0893508, Final residual = 3.71189e-08, No Iterations 4 BICCG: Solving for Uy, Initial residual = 0.0470008, Final residual = 8.18107e-07, No Iterations 3 BICCG: Solving for Uz, Initial residual = 0.00210555, Final residual = 4.94314e-08, No Iterations 3 BICCG: Solving for C7H16, Initial residual = 0.00283565, Final residual = 2.4395e-07, No Iterations 2 BICCG: Solving for O2, Initial residual = 0.00264662, Final residual = 8.18177e-07, No Iterations 2 BICCG: Solving for CO2, Initial residual = 0.00283727, Final residual = 2.09632e-07, No Iterations 2 BICCG: Solving for H2O, Initial residual = 0.00283727, Final residual = 2.09632e-07, No Iterations 2 BICCG: Solving for h, Initial residual = 0.00291149, Final residual = 3.13086e-07, No Iterations 2 ICCG: Solving for p, Initial residual = 0.62558, Final residual = 6.53001e-10, No Iterations 28 time step continuity errors : sum local = 3.69438e-12, global = -4.5675e-13, cumulative = -4.31118e-11 ICCG: Solving for p, Initial residual = 0.121549, Final residual = 5.99677e-10, No Iterations 27 time step continuity errors : sum local = 4.06811e-12, global = -8.22919e-13, cumulative = -4.39347e-11 BICCG: Solving for epsilon, Initial residual = 0.00106245, Final residual = 6.1007e-07, No Iterations 2 bounding epsilon, min: -1.59758e+11 max: 9.5401e+11 average: 2.79012e+08 BICCG: Solving for k, Initial residual = 0.4897, Final residual = 4.5726e-07, No Iterations 2 Number of parcels in system | 1101 Injected liquid mass....... | 3.26959 mg Liquid Mass in system...... | 1.13211 mg SMD, Dmax.................. | 13.5651 mu, 145.611 mu Added gas mass = 2.13748 mg Evaporation Continuity Error| 8.76679e-13 mg ExecutionTime = 294.19 s Max Courant Number = 2.12046 Time = 0.00059 Evolving Spray Solving chemistry BICCG: Solving for Ux, Initial residual = 0.0458617, Final residual = 9.53264e-07, No Iterations 3 BICCG: Solving for Uy, Initial residual = 0.158556, Final residual = 6.22212e-07, No Iterations 4 BICCG: Solving for Uz, Initial residual = 0.00461368, Final residual = 5.90762e-08, No Iterations 4 BICCG: Solving for C7H16, Initial residual = 0.00282151, Final residual = 2.05982e-07, No Iterations 3 BICCG: Solving for O2, Initial residual = 0.00261989, Final residual = 3.43801e-07, No Iterations 3 BICCG: Solving for CO2, Initial residual = 0.00304074, Final residual = 5.55743e-07, No Iterations 3 BICCG: Solving for H2O, Initial residual = 0.00304074, Final residual = 5.55743e-07, No Iterations 3 BICCG: Solving for h, Initial residual = 0.00385778, Final residual = 6.85247e-07, No Iterations 3 --> FOAM FATAL ERROR : attempt to use janafThermo<equationofstate> out of temperature range 200 -> 5000; T = 191.289 Function: janafThermo<equationofstate>::checkT(const scalar T) const in file: /home/ervin/OpenFOAM/OpenFOAM-1.1/src/thermophysicalModels/specie/lnInclude/jana fThermoI.H at line: 73. FOAM aborting How can this error be corrected/prevented? Ervin |

Hi Niklas,
Yes this is a buHi Niklas,
Yes this is a bug in 1.1, you also need to make the eqivalent change in dispersionLESModel.C: sm.runTime().lookupObject<compressible::lesmodel> to sm.mesh().lookupObject<compressible::lesmodel> I have fixed this for 1.1.1 H |

The above mentioned 'out of teThe above mentioned 'out of temperature range' error happened because of an ill imposed wall temp. bc (I think). I've changed to fixedValue uniform 293 K and it worked.
Ervin |

Hi,
the 'out of temperatureHi,
the 'out of temperature range' is a secondary effect of a 'crashed' run, look at the courant number 2.1!!! try keeping the courant number low. The problem with spray calculations are that if you have large/sudden variation in injection velocity the added momentum, or energy, can be substantial and you will get this kind of error. N |

All times are GMT -4. The time now is 04:07. |