CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   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)

adorean April 22, 2005 04:48

Hi, When I activate turbule
 
Hi,

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

niklas April 22, 2005 05:03

looks like we forgot to change
 
looks 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

adorean April 22, 2005 05:16

Worked for me too. Thanks,
 
Worked for me too.

Thanks, Niklas.

Ervin

adorean April 22, 2005 05:27

Well, now I've got myself a di
 
Well, 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

henry April 22, 2005 06:02

Hi Niklas, Yes this is a bu
 
Hi 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

adorean April 22, 2005 06:39

The above mentioned 'out of te
 
The 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

niklas April 22, 2005 06:55

Hi, the 'out of temperature
 
Hi,

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 05:01.