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

full mechanism don't combust in openfoam

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

Like Tree1Likes
  • 1 Post By sushant

Reply
 
LinkBack Thread Tools Display Modes
Old   January 24, 2013, 23:33
Default full mechanism don't combust in openfoam
  #1
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi everyone, I am doing LES combustion spray in openfoam. I tried one global reaction for combustion, which works OK. But when I try full mechanism reactions, it nearly doesn't burn or burn very slow(the highest T is like only 1200K). I tried heptane and dodecane, both meet this problem. The mechanism of heptane is from the openfoam wiki tutorial case. I attached one heat release rate plot for dodecane case. I wonder is there any other extra set for using full mechanism? Because when I run one global reaction, it burns normally. Any hinit about this problem? Or you can tell me how to check the mechanism that is read by openFoam.

Another problem I got is how to simulate like use dodecane for calculating liquid properties while use heptane for reaction mechanism. I know this can be done in Kiva, so I guess it also can be done in openfoam.

Thanks!

Case setup : T = 900[k], p = 5.92[MPa], Ignition Delay = 0.44[ms], O2 = 15.00; N2 = 75.15; CO2 = 6.22; H2O = 3.62, fuel: dodecane;
Attached Images
File Type: jpg dQdt.jpg (86.0 KB, 52 views)
conceptone is offline   Reply With Quote

Old   February 10, 2013, 10:17
Default
  #2
Member
 
Likun
Join Date: Feb 2013
Posts: 48
Rep Power: 4
Likun is on a distinguished road
Send a message via Skype™ to Likun
Hi conceptone, hope you have solved your problem. I also would like to do some LES simulation on spray combustion using OpenFoam. But I totally have no idea, if OpenFoam can be readily used to simulate spray combustion or not? Do I need to develop my own code?

Thanks!
Likun is offline   Reply With Quote

Old   February 10, 2013, 15:19
Default
  #3
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi, I don't solve this problem yet...But we can keep sharing if any progress
conceptone is offline   Reply With Quote

Old   February 11, 2013, 12:06
Default chemFoam
  #4
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 8
sushant is on a distinguished road
I am seeing the same behaviour with n-heptane combustion using the 44-species Pitsch et al. mechanism [1] in that the temperature never exceeds 1200 K. For the same case if I switch to a 159-species mechanism [2] a temperature in the right range is predicted, as is the case with the 544-species mechanism that comes with the OpenFOAM tutorial.

By the way you can quickly test various mechanisms using the chemFoam solver instead of doing it on a mesh.

An attached plot shows the temperature evolution in time, using a one-step reaction mechanism and the three other mechanisms referred to above. Additionally I also threw in the curve for chemFoam's 544-species mechanism evaluated by SENKIN, this data of course comes from the chemFoam/nc7h16/validation folder. Check this solver and the corresponding tutorial.

Does anyone have ideas on what is going wrong or how to diagnose this behaviour?

Thanks,
Sushant

--
[1] Comb. Flame 137, pp. 320-339, 2004;
files at http://www.stanford.edu/group/pitsch/Downloads.htm
(the therm.dat file in the URL above is missing an END at the end)

[2] Proceedings of the Combustion Institute 28, p. 2029-2037, 2000;
files at https://www-pls.llnl.gov/?url=scienc...uced_mechanism
Attached Images
File Type: jpg Screen Shot 2013-02-11 at 5.03.27 PM.jpg (53.5 KB, 37 views)
File Type: jpg Screen Shot 2013-02-11 at 5.04.56 PM.jpg (43.3 KB, 24 views)
francescomarra likes this.
sushant is offline   Reply With Quote

Old   February 12, 2013, 16:45
Default
  #5
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi sushant,
Thanks for discussing. I wanna share one plot run by chemFoam, compared with the result by chemkin software. The result matches good, which may demonstrate the chemisty part in openfoam is good.

One thing I wanna make sure is that for the first plot you post, what solver do you use? Is it chemFoam or sprayFoam?
And what version of openfoam are you using?
Attached Images
File Type: jpg chemkin.jpg (22.1 KB, 23 views)
File Type: jpg chemfoam.jpg (83.5 KB, 24 views)
conceptone is offline   Reply With Quote

Old   February 13, 2013, 10:06
Default
  #6
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 8
sushant is on a distinguished road
Hi, it's all chemFoam on 2.1.x so far.
sushant is offline   Reply With Quote

Old   February 14, 2013, 05:45
Default
  #7
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 8
sushant is on a distinguished road
Hello,

In case of the H2 tutorial (chemFoam 2.1.x) the predicted temperature is much lower than SENKIN data. Has anyone been able to get it working correctly?

Last edited by sushant; February 14, 2013 at 06:41.
sushant is offline   Reply With Quote

Old   February 14, 2013, 14:06
Default
  #8
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi sushant, one thing important here I found is you got to set the Tcommon the same, you can try this.
And you can refer to the post
sprayFoam aachenBomb FATAL ERROR when running combustion
conceptone is offline   Reply With Quote

Old   February 14, 2013, 14:30
Default
  #9
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 8
sushant is on a distinguished road
Hi,

The Tcommon value is the same for all species in the 44-specie mechanism I am using (or rather would like to use).

In the 159-species mechanism Tcommon is vastly different for many species. Even Tmin and Tmax are different for some species. This mechanism works flawlessly and the results are also good for the first few ms of the sandia bomb, but I simply cannot afford the computational time it requires.
sushant is offline   Reply With Quote

Old   February 23, 2013, 12:00
Thumbs up
  #10
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 8
sushant is on a distinguished road
This problem is fixed by modifying the file src/thermophysicalModels/specie/thermo/specieThermo/specieThermoI.H, and replacing the definition of K(T) with

Code:
template<class Thermo>
inline Foam::scalar Foam::specieThermo<Thermo>::K(const scalar T) const
{
    scalar arg = -this->nMoles()*this->g(T)/(this->RR*T);

    if (arg < 600.0)
    {
        return ::exp(arg);
    }
    else
    {
        return VGREAT;
    }
}
(Recompile libspecie; on OS X I need to wclean first, YMMV)

For more info see: http://www.openfoam.org/mantisbt/view.php?id=657.

This results from using a 2.1.x from before 01.11.2012 which hasn't been updated thereafter. Doing a
Code:
git pull
and recompiling will fix this without the need for the above manual step.

Thanks to: Tommaso Lucchini
sushant is offline   Reply With Quote

Old   February 23, 2013, 13:46
Default
  #11
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Good detection,buddy!
Also, I found if you meet any crashing problem like
[3] #3 Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >:mega(Foam::Reaction<Foam::sutherlandTransport< Foam::specieThermo<Foam::janafThermo<Foam:erfect Gas> > > > const&, Foam::Field<double> const&, double, double, double&, double&, int&, double&, double&, int&) const at sigaction.c:0
[0] #3 Foam::ODEChemistryModel<Foam:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >:mega(Foam::Reaction<Foam::sutherlandTransport< Foam::specieThermo<Foam::janafThermo<Foam:erfect Gas> > > > const&, Foam::Field<double> const&, double, double, double&, double&, int&, double&, double&, int&) const in in "/usr"/usr/er/erc/people/lc/people/liaoiao23/OpenFOAM/li23/OpenFOao23-2.1.1AM/liao23-2./platforms1.1/platform/linux64Gcc44DPOpts/lin/lib/libcheux64GccmistryModel44DPOpt.so"/lib/
(basically the omega function in chemistryModel class)
you can adjust the "eps" parameter in chemistyProperties dict to a smaller value,this would solve the problem.
conceptone is offline   Reply With Quote

Old   February 25, 2013, 14:13
Default
  #12
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi sushant, I am not sure why the nmoles is a problem mentioned in the post, though when the nmoles can be a very small number, the exp(-small) still approaches 1(essentially 1) as the exp is continous function.
conceptone is offline   Reply With Quote

Old   September 9, 2013, 01:12
Default
  #13
New Member
 
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 4
RJ87 is on a distinguished road
Hi Foamer,

May I know how do you guys set boundary condition for liquid n-heptane. Did you guys kept it to density of 1000 and specific heat of 4187? Or you guys have change it according to the respective n-heptane density of approx 684 and specific heat of 2465?

Because the spray behaviour with new parameters does not look correct to me. =(
RJ87 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
using reduced mechanisms in openFOAM Alish1984 OpenFOAM Running, Solving & CFD 4 August 17, 2012 06:26
Official OpenFOAM Training Courses early 2013 (and 2012 update) opencfd OpenFOAM Announcements from ESI-OpenCFD 0 July 18, 2012 07:30
Cross-compiling OpenFOAM 1.6 on Linux for Windows 32 and 64bits with Mingw-w64 wyldckat OpenFOAM Announcements from Other Sources 7 January 19, 2010 16:39
2009 OpenFOAM Summer School in Zagreb, Croatia hjasak OpenFOAM Announcements from Other Sources 0 March 27, 2009 13:08
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25


All times are GMT -4. The time now is 06:57.