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

Modeling Turbulent Reactive Flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 9, 2009, 04:08
Default Modeling Turbulent Reactive Flow
  #1
New Member
 
Sanjib Das Sharma
Join Date: May 2009
Posts: 22
Rep Power: 8
sanjibdsharma is on a distinguished road
Hi I am trying to model a multi-species, turbulent reactive flow. From the examples, I understand I need to create a chemkin type format for the reacting species and a thermophysical data file. However, are there any models similar to the Eddy-break-up model in OpenFoam ? If so, where do I find it and how do I change the mixing parameters for this model ?

Thanks in advance.

Sanjib
sanjibdsharma is offline   Reply With Quote

Old   June 13, 2009, 08:04
Default
  #2
Member
 
Ville Tossavainen
Join Date: Mar 2009
Location: Helsinki, Finland
Posts: 60
Rep Power: 8
villet is on a distinguished road
Hello Sanjib,

search the forum with keyword "reactingFoam" which is a general reacting flow solver in OpenFOAM. You can find a tutorial case here:

http://openfoamwiki.net/index.php/Tu..._firstTutorial

The mixing parameter "Cmix" can be found in "constant/chemistryProperties" dictionary. As you mentioned, the chemical properties are read in ChemKin format.

The chemisty is solved in a separate library and called in "reactingFoam" solver, so the solver code is quite compact. You can find the source code file for turbulence-chemistry interaction "chemistry.H" in "reactingFoam" solver directory. You can find similarities with the Chalmers PaSR model to other eddy-break up models.

Hope this helps,
Ville
villet is offline   Reply With Quote

Old   June 19, 2009, 00:01
Default
  #3
Member
 
edison
Join Date: May 2009
Location: Australia
Posts: 33
Rep Power: 8
Edison_Ge is on a distinguished road
hi, I'm working on the similar area. Are there more advanced combustion method like flamelet or even PDF in OpenFOAM?
Thanks a lot!
Edison_Ge is offline   Reply With Quote

Old   June 22, 2009, 17:02
Default
  #4
Member
 
Ville Tossavainen
Join Date: Mar 2009
Location: Helsinki, Finland
Posts: 60
Rep Power: 8
villet is on a distinguished road
Quote:
Originally Posted by Edison_Ge View Post
hi, I'm working on the similar area. Are there more advanced combustion method like flamelet or even PDF in OpenFOAM?
I haven't seen transported PDF model in OpenFOAM. Someone else can correct me if I'm wrong.

Are you interested in non-premixed or premixed flamelet models? Hannes Kroger at University of Rostock has worked on premixed combustion. He has a SVN repository for all of his stuff (search the forum "hannes repository).

Hannes' work has helped me on my ever-lasting project which is more about non-premixed combustion and deals with flamelet/progress-variable model.

About the more sophisticated models in OpenFOAM, you should check this thread:

Where to find the theory for weller flamet combustion model

Hope this helped,
Ville
villet is offline   Reply With Quote

Old   June 24, 2009, 00:35
Default
  #5
Member
 
edison
Join Date: May 2009
Location: Australia
Posts: 33
Rep Power: 8
Edison_Ge is on a distinguished road
thanks ville!

I found hannes repository and his work is very helpful to my research.

I'm working on non-premixed combustion with PDF transport model. My supervisor and me are working on a new mixing model and considering implement it in openFOAM. But the previous problem is that no much OPENFOAM usage in my school, university of Queesland, AU.

If that's possible I'd like to know more of your work with OpenFOAM. My email is yipeng.ge@uqconnect.edu.au

Cheers

Last edited by Edison_Ge; July 15, 2009 at 22:04.
Edison_Ge is offline   Reply With Quote

Old   June 24, 2009, 03:46
Default premixed combustion
  #6
New Member
 
Chris
Join Date: May 2009
Posts: 6
Rep Power: 8
Burn is on a distinguished road
Hi,

I am working in premixed flame modelling and I have searched for the repository of Hannes Kroger but without success.
Could someone explain what exactly to search for in order to find it or post a link to it?

Thanks
Burn is offline   Reply With Quote

Old   July 9, 2009, 08:06
Default
  #7
Member
 
Ville Tossavainen
Join Date: Mar 2009
Location: Helsinki, Finland
Posts: 60
Rep Power: 8
villet is on a distinguished road
Quote:
Originally Posted by Burn View Post
Hi,

Could someone explain what exactly to search for in order to find it or post a link to it?

Thanks
Here's the link for the post:
http://www.cfd-online.com/Forums/ope...tml#post198279
villet is offline   Reply With Quote

Old   July 9, 2009, 08:10
Default
  #8
New Member
 
Chris
Join Date: May 2009
Posts: 6
Rep Power: 8
Burn is on a distinguished road
Thank you for the link
Burn is offline   Reply With Quote

Old   December 6, 2009, 10:49
Default
  #9
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
Hello Vill, hello Sanjib, hello everyone

I am trying to impliment a turbulent reacting flow. my idea was to use the reactingFoam solver.

My case:
i have zylinder with a fuel (CH4) inlet, an air inlet and a coflow inlet. at the other of the zylinder is an outlet.

first of all i impliment a simpleFoam case just with velocity field (without the reaction). that works fine. so, now i am trying to add the reaction.

i was trying to run the reactingFoam tutorial (http://openfoamwiki.net/index.php/Tu..._firstTutorial). i updated the path of the "chem.inp" and "therm.dat" files as describe and run the case. after the there was a error message.

"keyword psiChemistryModel is undefined in dictionary"

so, i added the keyword as in the dieselFoam tutorial.

"psiChemistryModel ODEChemistryModel<gasThermoPhysics>;"

another error message came up.

Reading chemistry properties


Reading g

Reading thermophysicalProperties
Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics>
Selecting thermodynamics package hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
Selecting chemistryReader chemkinReader
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam:imensionedField<double, Foam::volMesh>:perator/=(Foam:imensionedField<double, Foam::volMesh> const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>:
perator/=(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#5 Foam::multiComponentMixture<Foam::sutherlandTransp ort<Foam::specieThermo<Foam::janafThermo<Foam:er fectGas> > > >::correctMassFractions() in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#6 Foam::multiComponentMixture<Foam::sutherlandTransp ort<Foam::specieThermo<Foam::janafThermo<Foam:er fectGas> > > >::multiComponentMixture(Foam::dictionary const&, Foam::List<Foam::word> const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam: :specieThermo<Foam::janafThermo<Foam:erfectGas> > >, Foam::word, Foam::string::hash> const&, Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#7 Foam::reactingMixture<Foam::sutherlandTransport<Fo am::specieThermo<Foam::janafThermo<Foam:erfectGa s> > > >::reactingMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#8 Foam::hPsiMixtureThermo<Foam::reactingMixture<Foam ::sutherlandTransport<Foam::specieThermo<Foam::jan afThermo<Foam:erfectGas> > > > >::hPsiMixtureThermo(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#9 Foam::hCombustionThermo::addfvMeshConstructorToTab le<Foam::hPsiMixtureThermo<Foam::reactingMixture<F oam::sutherlandTransport<Foam::specieThermo<Foam:: janafThermo<Foam:erfectGas> > > > > >::New(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#10 Foam::hCombustionThermo::NewType(Foam::fvMesh const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libreactionThermophysicalModels.so"
#11 Foam:siChemistryModel:siChemistryModel(Foam::fvMes h const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#12 Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >::ODEChemistryModel(Foam::fvMesh const&, Foam::word const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#13 Foam:siChemistryModel::addfvMeshConstructorToTable <Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:
erfectGas> > > > >::New(Foam::fvMesh const&, Foam::word const&, Foam::word const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#14 Foam:siChemistryModel::New(Foam::fvMesh const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libchemistryModel.so"
#15 main in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#16 __libc_start_main in "/lib/libc.so.6"
#17 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122
Gleitkomma-Ausnahme

so, i don't know what's mean. has anyone an helpfull advice for me how to fix my problem.

Thanks in advance.

regarts,

Ilja
hamburgFoam is offline   Reply With Quote

Old   December 7, 2009, 09:53
Default
  #10
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 8
dhuckaby is on a distinguished road
IIja,

I was able to reproduce a similar error when I either set all the initial mass fractions to 0 or
all the mass fractions were set to 0 at any boundary.

Dave

Last edited by dhuckaby; December 7, 2009 at 09:53. Reason: typo
dhuckaby is offline   Reply With Quote

Old   December 7, 2009, 13:26
Default
  #11
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
Hey Dave,

thank you for your advice. i played a bit with the mass fraction and set it like below.

BC T CH4 O2 N2
inlet one 293 0.5 0 0
inlet two 293 0.5 0 0
inlet three 293 0 0.2 0.8
Internal field 293 0 0.2 0.8

the mass fraction in the Ydefault-file are set to all to 0.

but i have still the same error!

the mass fraction is the fraction of one substance with there mass to the total mixture mass. where i have to set the total mixture mass of a species?


Regards, Ilja
hamburgFoam is offline   Reply With Quote

Old   December 7, 2009, 16:58
Default
  #12
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 8
dhuckaby is on a distinguished road
IIja,

Could you post the text for the "thermophysicalProperties" and "chem.inp" for the case
described above ?

You could also try running with all the inlet mass fractions set to the the mass fractions of the initial condition.

Dave
dhuckaby is offline   Reply With Quote

Old   December 7, 2009, 19:01
Default
  #13
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>;

CHEMKINFile "$FOAM_CASE/chemkin/chem.inp";

CHEMKINThermoFile "~OpenFOAM/thermoData/therm.dat";

inertSpecie N2;

liquidComponents ( CH4 );

liquidProperties
{
CH4 CH4 defaultCoeffs;
}


// ************************************************** *********************** //

and the cham.inp file...

ELEMENTS
H O C N
END
SPECIE
CH4 O2 N2 CO2 H2O
END
REACTIONS
CH4 + 2O2 => CO2 + 2H2O 6.70091E+12 0.0 4.84149E+04! 1
FORD / CH4 0.2 /
FORD / O2 1.3 /
END
hamburgFoam is offline   Reply With Quote

Old   December 8, 2009, 10:00
Default
  #14
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 8
dhuckaby is on a distinguished road
IIja,

I ran the tutorial case with the settings described in the previous posts I was only able to reproduce the error when the sum of the species mass fractions was equal to zero. The code ran OK when the mass fractions did not sum to unity.

I think the location in code where the error occurs is the divide in:
thermophysicalModels/reactionThermo/lnInclude/multiComponentMixture.C
void Foam::multiComponentMixture<ThermoType>::correctMa ssFractions()

Dave
dhuckaby is offline   Reply With Quote

Old   December 8, 2009, 13:57
Default
  #15
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
Hey Dave,

thank you for your help. your advice fixed THAT problem.

the problem was: the names of my species-files were ch4, o2 and n2 (instead of CH4, O2 and N2) and the mass fraction in the Ydefault file was set to zero. so FOAM couldn't read the files and set all mass fractions like in the Ydefault to zero.

i ran the case and another error came up...

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading chemistry properties


Reading g

Reading thermophysicalProperties
Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics>
Selecting thermodynamics package hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
Selecting chemistryReader chemkinReader
Selecting chemistrySolver ode
Selecting ODE solver SIBS
ODEChemistryModel: Number of species = 5 and reactions = 1
Reading field U

Reading/calculating face flux field phi

Creating turbulence model.

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon


Different dimensions for =
dimensions : [1 -1 -1 0 0 0 0] = [0 2 -1 0 0 0 0]
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::dimensionSet:perator=(Foam::dimensionSet const&) const in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>:perator=(Foam::tmp<Foam::Geometri cField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#4 Foam::compressible::RASModels::kEpsilon::kEpsilon( Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#5 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kEpsilo n>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#6 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#7 Foam::compressible::turbulenceModel::addturbulence ModelConstructorToTable<Foam::compressible::RASMod el>::NewturbulenceModel(Foam::GeometricField<doubl e, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#8 Foam::compressible::turbulenceModel::New(Foam::Geo metricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libcompressibleTurbulenceModel.so"
#9 main in "/home/openfoam/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/reactingFoam"
#10 __libc_start_main in "/lib/libc.so.6"
#11 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122


From function dimensionSet:perator=(const dimensionSet& ds) const
in file dimensionSet/dimensionSet.C at line 143.

FOAM aborting


Dave, do you have an idea what dimensions are meant?
hamburgFoam is offline   Reply With Quote

Old   December 8, 2009, 15:34
Default
  #16
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
fixed it so far!
thx Dave
hamburgFoam is offline   Reply With Quote

Old   December 15, 2009, 12:47
Default
  #17
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
Hello everyone,

i am modelling a reactingFoam case for a CH4-air combustion. i ran the case and it was fine. the problem is, that flame-temperatur was very much lower than expected.

my properties for the pre exponential factor A, temperature exponent b and the activation energy are as below:

ELEMENTS
H O C N
END
SPECIE
CH4 O2 N2 CO2 H2O
END
REACTIONS
CH4 + 2O2 => CO2 + 2H2O 6.70091E+12 0.0 4.84149E+04! 1
FORD / CH4 0.2 /
FORD / O2 1.3 /
END

do anyone has an idea what i could have done wrong and how to increase the flame-temperature?

regards,

Ilja
hamburgFoam is offline   Reply With Quote

Old   December 16, 2009, 10:11
Default
  #18
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 8
dhuckaby is on a distinguished road
Ilja,

A number of things may effect the flame temperature (and shape):
- turbulence model
- ode solver and settings
- kinetic model
- mesh resolution

The following paper, among other topics, has comparisons between experimental data and OF flame simulations:
http://www.opensourcecfd.com/confere...haiderRehm.pdf

Dave
dhuckaby is offline   Reply With Quote

Old   December 17, 2009, 11:01
Default
  #19
New Member
 
Ilja Sabelfeld
Join Date: Nov 2009
Posts: 22
Rep Power: 7
hamburgFoam is on a distinguished road
Hey Dave,

thanks, you halped me again.

But I have problems to ignite my flame. I would like to simulate a flame with specific bc's so I can compare the flame with the measured one.

My temperature BC's are:

fuel inlet: 291 K
pilot: 1880 K
coflow: 294 K

in addition I chose for the internelField 293 K.

If I run the case with this settings the reaction couldn't start. I was thinking that the fuel-inlet-temperature was to low to ignite. the autoignition temperature of CH4 is 823 K. so, I raised the fuel-inlet-temperature to 900 K to proof, if it would ignite. it did. I ve got a flame temperature of 2500 K. I was expecting 2300 K with the fuel-inlet-temperature of 291 K.

is there another possibility for ignition? maybe to configurate a temperature profile at the fuel-inlet, that the flow would have a temperature of 900 K at the first iteration-steps and change after this to 291 K?

best regards,

Ilja
hamburgFoam is offline   Reply With Quote

Old   December 18, 2009, 15:34
Default
  #20
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 8
dhuckaby is on a distinguished road
Ilja,

There is a "timeVaryingFixedValue" boundary condition which would allow you to decrease the inlet temperature over time. Did you try igniting by increase the pilot temperature ? There is also an ignition model on the wiki as well as one use in coalChemistryFoam (1.6.x). Also, "funkySetFields" would alllow you to build a numerical "spark" as an initial condition.

Dave
dhuckaby 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
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 20:28
Laminar flow or Turbulent flow mech FLUENT 0 January 27, 2007 19:51
laminar and turbulent flow in one simulation msna FLUENT 0 January 27, 2007 18:35
Reynolds and Turbulent Flow Frederic Dubinski Main CFD Forum 2 October 20, 2004 13:57
PhD in turbulence Hans Main CFD Forum 14 October 8, 2001 03:03


All times are GMT -4. The time now is 08:01.