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

DieselFoam error turbulent dispersion

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 22, 2005, 04:48
Default Hi, When I activate turbule
  #1
Member
 
Ervin Adorean
Join Date: Mar 2009
Posts: 68
Rep Power: 8
adorean is on a distinguished road
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
adorean is offline   Reply With Quote

Old   April 22, 2005, 05:03
Default looks like we forgot to change
  #2
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
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
niklas is offline   Reply With Quote

Old   April 22, 2005, 05:16
Default Worked for me too. Thanks,
  #3
Member
 
Ervin Adorean
Join Date: Mar 2009
Posts: 68
Rep Power: 8
adorean is on a distinguished road
Worked for me too.

Thanks, Niklas.

Ervin
adorean is offline   Reply With Quote

Old   April 22, 2005, 05:27
Default Well, now I've got myself a di
  #4
Member
 
Ervin Adorean
Join Date: Mar 2009
Posts: 68
Rep Power: 8
adorean is on a distinguished road
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
adorean is offline   Reply With Quote

Old   April 22, 2005, 06:02
Default Hi Niklas, Yes this is a bu
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
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
henry is offline   Reply With Quote

Old   April 22, 2005, 06:39
Default The above mentioned 'out of te
  #6
Member
 
Ervin Adorean
Join Date: Mar 2009
Posts: 68
Rep Power: 8
adorean is on a distinguished road
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
adorean is offline   Reply With Quote

Old   April 22, 2005, 06:55
Default Hi, the 'out of temperature
  #7
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
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
niklas 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
Running dieselFoam error adorean OpenFOAM Running, Solving & CFD 118 March 12, 2009 15:37
DPM turbulent dispersion Springbok Main CFD Forum 0 July 15, 2008 04:14
Turbulent Dispersion in Particle Tracking ariel CFX 2 April 22, 2008 22:02
Turbulent dispersion Julie Polyakh CD-adapco 0 May 15, 2003 07:14
turbulent dispersion of particles! danney CFX 0 April 2, 2003 09:17


All times are GMT -4. The time now is 13:32.