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

libOpenSMOKE

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

Like Tree128Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2014, 09:47
Default
  #301
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by babakflame View Post
Greetings Tobi

After checking the LES results, It seems that although the flame is captured steadily with piso solver, there are some mistakes in the arrangement of the reacting scalars. I checked my equations and found two errors
1- I should have changed the turbulent Schmidt number (to 0.4)
2- I found an error in my equation for chi_Tilde in ZEqn.H file. I should have used molecular diffusivity instead of turbulent diffusivity.

This is the false code that I have used:
Code:
chi_st=2 * (turbulence->mut()/(rho*sigmat)) * magSqr(fvc::grad(Z));
In the above equation turbulence->mut refers to turbulent viscosity(Mut). In the above formulation, Mut should be replaced with Mu (i.e. laminar viscosity)
If I want to use laminar viscosity(Mu) instead of Mut in the above formula, what should I write to be compatible with the code?

I used mu() for laminar viscosity. I got this error:
Code:
 ZEqn.H:24:16: error: 'mu' was not declared in this scope
then I used turbulence->mu() , this time no error appeared and the code compiled. But this notation is correct for referring to laminar viscosity?

Regards
Bobi

Hi Bobi,

you have three ways to declare mu

Code:
turbulence->mu()          // molecular visco
turbulence->mut()        // turbulent visco
turbulence->muEff()     // molecular + turbulent
To have laminar combustion Z_var = 0 but in the code you will set the cells with Z_var = 0 to Z_var = 0.01 (dont know the correct value). This depend on the area wighted interpolation scheme because if you set Z_var to zero it is not possible to calculate the value of phi due to the fact of the area wighted interpolation.

Therefor you always have an error in your extracted values.
Just as an information.

Regards
Tobi
babakflame likes this.
Tobi is online now   Reply With Quote

Old   January 22, 2014, 15:54
Default Regarding Jet Flame Simulation
  #302
New Member
 
payal
Join Date: Aug 2013
Location: banglore
Posts: 14
Rep Power: 5
payal05 is on a distinguished road
Greeting oll,

After doing the tutorial of sandia flame with flameletSimpleFoam solver i tried to solve the same problem but with the changed domain keeping the rest of the things same as in tutorials, but i encounter the few problems :

Quote:
1. The Mass Fraction of the CO2 is very high as compared with the experiments results .
2. The axial temperature is quite high around 2000 k whereas in experiment results it is less .
3. Other issue is that , i tried to slove this case on 2 computational domains one is 2.5 m and other is 4.5 , the thing is on 2.5 i am getting good appropriate with Exp results but with 4.5 the initial results are quite diffrent to that of the exp results .
So can anybody plz guide me . For more info i can upload files or result graphs ..
Thank You ,
Regards ,
Payal
payal05 is offline   Reply With Quote

Old   January 23, 2014, 07:03
Default
  #303
TBO
Member
 
Join Date: May 2013
Location: Netherlands
Posts: 30
Rep Power: 5
TBO is on a distinguished road
Quote:
Originally Posted by hayhari View Post
It is working well with small CRECK kinetics and GRI Mech.
All,

After some other priorities I restarted with combustion simulations with the use of libOpenSmoke/flameletSimpleFoam. We also made the change from OpenFoam 2.1 to 2.2 in order to use the transient solver as well. I have some questions/issues, hopefully somebody can help me.

So far I am using the PolimiC1C3 kinetics mechanism, however I am also interested in using the more standard GRI Mechanism. I know some people applied this mechanism in the flamelet solver, where can I find the required files to use the GRI mechanism in the Look-Up-Table generation (I know it is possible to generate them with Cantera, however I have no experience with this program, so hopefully somebody can help me out)?

I am modelling a combustor with flameletSimpleFoam (unfortunately I can't share my model/results since I am working for a company). Pressure convergence of this solver is not that good, as already known from other discussions at this forum, so to "overcome" this issue, I used the steady state results to initialize a transient simulation. However this is not working properly. What is basically happening in the transient simulation is that the flame is blowing off and that a new flame starts to develop. So basically the transient solver is more or less neglecting the steady state results that I used for the initialisation. Has anyone encountered a similar problem before or knows how to overcome this problem?

The third and last issue I have is changing the fuel that is used for the simulation, since I am interested in fuel flexibility I would like to change the fuel in the simulation, for example from CO/H2 to CH4. I did this before in turbulentFlameletRhoSimplecFoam in OF 2.1 and that worked. However when I am doing it now in flameletSimpleFoam in OF 2.2 some weird things are happening. I am using the converged solution of the CO/H2 simulation to start the CH4 simulation. The only things I change are the PDF-Library and the mass flow at the fuel inlet (to keep the same thermal power input). In this simulation I get a flame in the dilution zone, while before the flame was in the primary zone, it looks like that something is going wrong with the initialization of the flow field. Does anyone have a good idea how to initialize the flow field somehow without starting from zero when using a new fuel library (since starting from zero takes a lot of simulation time).

Looking forward to some help

Regards
TBO is offline   Reply With Quote

Old   February 11, 2014, 16:56
Default
  #304
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,558
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

I'm a bit out of the loop on this thread, but I believe that the following has not yet been mentioned here on the thread: http://openfoamwiki.net/index.php/Ex...n/flameletFoam

Isn't this one of the source code components that is missing from the libOpenSMOKE and other works? In other words, the missing code for the static binaries that are provided in libOpenSMOKE?

Best regards,
Bruno
babakflame likes this.
__________________
wyldckat is offline   Reply With Quote

Old   February 12, 2014, 02:34
Default
  #305
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 327
Rep Power: 6
babakflame is on a distinguished road
Greetings Bruno

It seems that some other guys are working on the same solver with both RAS and LES approaches. that sounds interesting

I am going to take a look at it. Many thanks for your valuable link.


Regards
Bobi
babakflame is offline   Reply With Quote

Old   February 12, 2014, 15:36
Default
  #306
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno,

cantera is a tool where you can build flamelet like the flameletgenerator by alberto cuoci.

To be sure if its completely the same I had to look into the source code and study it again.

But at the moment I am out of time. Today I was at the university leoben in austria. There I made a presentation about the flamelet model. Maybe I will publish it.
Tobi is online now   Reply With Quote

Old   February 13, 2014, 05:24
Default
  #307
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 327
Rep Power: 6
babakflame is on a distinguished road
Greetings Bruno & Tobi

I made some searches in this new flamelet solver. It seems that it uses RohPimple algorithm. I had problem with prior piosolver in Tobi code (Unstable results). I hope that this transient solver gives stable solutions.

-------------------------------------------
Finally I started installing this solver. I got a problem with installing OpenFoam source i.e. flameletFoam. The earlier steps including cantera and diffusion flame solver compiled successfully.
After adding the mentioned line to .bashrc and executing ./Allwmake I confronted this error including not finding lots of files:

Code:
In file included from turbulenceModel.C:26:0:
turbulenceModel.H:51:25: fatal error: basicThermo.H: No such file or directory
compilation terminated.
make: *** [Make/linux64GccDPOpt/turbulenceModel.o] Error 1


In file included from combustionModel/combustionModel.C:25:0:
combustionModel/combustionModel.H:38:29: fatal error: turbulenceModel.H: No such file or directory
compilation terminated.
make: *** [Make/linux64GccDPOpt/combustionModel.o] Error 1
Did you compile this code successfully? If yes, could you PLZ tell me what is my problem? I did exactly as the instructions in OpenFoam Wiki link.

--------------------------------------------------------
It compiled finally. ./Allclean was needed before ./Allwmake

Regards
Bobi

Last edited by babakflame; February 13, 2014 at 06:50.
babakflame is offline   Reply With Quote

Old   February 14, 2014, 07:22
Default Regarding Bluff Body flame simulation
  #308
Member
 
sonu
Join Date: Jul 2013
Location: delhi
Posts: 91
Rep Power: 5
yash.aesi is on a distinguished road
Greeting all ,
Nwdays i am trying to solve Bluff Body Flame (HM1) using flameletSimpleFoam solver . Just want to asked that did anybody solved the bluff body flame with this solver ??? so that i will get guidance ....



Thanks ,

Regards ,
Sonu
yash.aesi is offline   Reply With Quote

Old   February 17, 2014, 07:39
Default
  #309
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
I think noone did this befor.
But Bobi tryed to investigate more time to this.
Additionally here is a link:

http://web.student.chalmers.se/group...SlidesOFW5.pdf

Regards
yash.aesi likes this.
Tobi is online now   Reply With Quote

Old   February 22, 2014, 02:49
Arrow
  #310
Member
 
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5
vishal_s is on a distinguished road
Hi everyone,
I am trying to solve sydney SM1 swirl flame using turbulentFlameletRhoSimpleFoam solver ....with kinetic mechanism GriMech 3.0 ...but flame is instable...
But I have no idea how to sort out this problem....
Can you give any idea regarding this problem....I am really confused ....

Thanks in advance.....
vishal_s is offline   Reply With Quote

Old   February 22, 2014, 18:48
Default
  #311
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

as mentioned befor here is my presentation.
Its just a very brief description but I think I will translate my thesis in a brief summary letter. This one should give you enough information about the model and how this is working.

Regards Tobi


Presentation: http://www.holzmann-cfd.de/index.php...ffentlichungen (english)
babakflame and yash.aesi like this.
Tobi is online now   Reply With Quote

Old   February 22, 2014, 20:50
Default Some hints to flameletFoam
  #312
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

I had a look into the flameletFoam code from Müller et. al.
Seems very interessting and here some hints or information about the things I realized at the moment:

  • Seems that only adiabatic conditions can be calculated (no enthalpy equation solved)
  • The calculation of Zvar and chi is implemented into the turbulence model RAS and LES
    Therefore in LES Zvar is calculated as followed:
    Code:
        varZ_ = 1.0 * sqr(delta()) * magSqr(fvc::grad(this->thermo().Z()));
  • The scalar dissipation rate in LES is calculated as
    Code:
        chi_ = 2.0 * muEff()/rho_ * magSqr(fvc::grad(this->thermo().Z()));
  • The laminar flamelets are not transfered in a look-up-table befor. It seems that this happens while calculate the flow field (hmmm I am not sure if this is a good option)
  • I have to look at the extraction schedule the next days.


    Regards
    Tobi
babakflame likes this.
Tobi is online now   Reply With Quote

Old   February 23, 2014, 07:02
Default
  #313
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
News to the flameletFoam by Müller et. al.

  • canteraToFoam calculates the extension to turbulent flow fields and derivate the enthalpy hs form the temperature. This is different to the code of Alberto Cuoci et. al.
    Here the temperature is saved and not the enthalpy. Therefore it is possible to be more flexible to the standard libraries that comes with openfoam.

    The question is: if it is possible to simulate non adiabatic simulations...
  • The calculation of temperature in the flow field is derivated form the official thermodynamics of openfoam - all other things are calculated out of the thermodynamics too like:

    - temperature
    - density
    - viscosity
    - . . .
    - . . .

    This is calculated out of the mixture fraction and the enthalpy hs.

    Difference to Alberto Cuocis tool:

    - there you extract all variables out of the flamelets
Tobi is online now   Reply With Quote

Old   February 24, 2014, 02:04
Unhappy
  #314
Member
 
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5
vishal_s is on a distinguished road
Hi all,
I attached the swirl flame images at different time step. As observed, it is becoming unstable with time. Can anyone please suggest how to solve it. I have used turbulent flamelet rho simple foam.

14.05sec.jpg

17.85sec.jpg

20.5sec.jpg
vishal_s is offline   Reply With Quote

Old   February 24, 2014, 04:22
Default
  #315
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 327
Rep Power: 6
babakflame is on a distinguished road
Hi vishal

1- check your courant number. it should be less than 0.4
2- check your grid quality with
Code:
checkMesh
directive.
3- check your outlet B.C. (non-reflecting B.C.)
4- check your flamelet look-up tables.

Could you share your initial velocity file?

Regards
Bobi

Last edited by babakflame; February 24, 2014 at 07:23.
babakflame is offline   Reply With Quote

Old   February 24, 2014, 05:42
Default
  #316
Member
 
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5
vishal_s is on a distinguished road
Hi Bobi,
Using this geometry, simulation for non-reacting swirl flow works well. Detail of geometry and meshing given below.


Mesh stats
points: 1339005
faces: 3963546
internal faces: 3911118
cells: 1312444
faces per cell: 6
boundary patches: 6
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 1312444
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology Bounding box
swirl_inlet 557 697 ok (non-closed singly connected) (-0.03 -0.03 0) (0.03 0.03 0)
bluff_wall 1102 1152 ok (non-closed singly connected) (-0.025 -0.025 0) (0.025 0.025 0)
fuel_inlet 40 51 ok (non-closed singly connected) (-0.0018 -0.0018 0) (0.0018 0.0018 0)
outlet 4934 5015 ok (non-closed singly connected) (-0.065 -0.065 0.15) (0.065 0.065 0.15)
air_inlet 3235 3415 ok (non-closed singly connected) (-0.065 -0.065 0) (0.065 0.065 0)
side_wall 42560 42720 ok (non-closed singly connected) (-0.065 -0.065 0) (0.065 0.065 0.15)

Checking geometry...
Overall domain bounding box (-0.065 -0.065 0) (0.065 0.065 0.15)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (3.0224e-16 2.80494e-16 -2.77309e-16) OK.
Max cell openness = 3.32568e-16 OK.
Max aspect ratio = 8.08259 OK.
Minimum face area = 3.59247e-08. Maximum face area = 1.6634e-05. Face area magnitudes OK.
Min volume = 1.99548e-11. Max volume = 9.38039e-09. Total volume = 0.002535. Cell volumes OK.
Mesh non-orthogonality Max: 43.6981 average: 4.63388
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 1.35829 OK.
Coupled point location match (average 0) OK.
Face tets OK.
Min/max edge length = 0.000133197 0.00493919 OK.
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 0.999907
All face flatness OK.
Cell determinant (wellposedness) : minimum: 0.0443902 average: 4.72887
Cell determinant check OK.
Concave cell check OK.

Mesh OK.


This is the link of my case

https://www.dropbox.com/sh/076o8nsjzg5q5xg/RqLY0m6ThR
vishal_s is offline   Reply With Quote

Old   February 24, 2014, 05:43
Default
  #317
Member
 
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5
vishal_s is on a distinguished road
Hi Bobi,

I am trying to simulate my case using steady-state solver turbulentFlameletRhoSimpleFoam.

Regards
vishal
vishal_s is offline   Reply With Quote

Old   February 24, 2014, 07:29
Default
  #318
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,457
Blog Entries: 5
Rep Power: 25
Tobi will become famous soon enoughTobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Vishal,

I think you have a Problem with your schemes or better ... you should use more under-relaxation.
Additionally I think Zvar is going to -inf and inf. Am I correct?

Furthermore you can set the updateProperties to 1 and varianzEqn to false (then you are using an algebraic Expression for Zvar)

Regards

Last edited by Tobi; February 24, 2014 at 11:54.
Tobi is online now   Reply With Quote

Old   February 24, 2014, 12:23
Default
  #319
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 327
Rep Power: 6
babakflame is on a distinguished road
Hi Vishal

Make your div and grad schemes as follows: It may prohibits the instabilities.

Code:
gradSchemes
{
    default         none;
    
    grad(p)         cellLimited Gauss linear 1;
    grad(U)         cellLimited Gauss linear 1;
    grad(csi)       cellLimited Gauss linear 1;    
    grad(csiv2)     cellLimited Gauss linear 1; 
    grad(H)        cellLimited Gauss linear 1; 
    grad(epsilon)   cellLimited Gauss linear 1;  
    grad(k)        cellLimited Gauss linear 1;      
}

divSchemes
{
    default          none;

    div(phi,U)                  Gauss limitedLinearV 1; //    Gauss limitedLinearV 1;
    div(phiU,p)                 Gauss limitedLinear 1; //    Gauss limitedLinear 1;
    div(phi,epsilon)             Gauss limitedLinear 1;
    div(phi,k)                 Gauss limitedLinear 1;
    div(phi,H)                 Gauss limitedLinear 1;
    div(phi,csi)               Gauss limitedLimitedLinear 1 0 1;
    div(phi,csiv2)              Gauss limitedLimitedLinear 1 0 0.25;
    div((muEff*dev2(T(grad(U)))))       Gauss linear;
}
and lower your solvers tolerance by an order.

I hope this will make you get better results.
babakflame is offline   Reply With Quote

Old   February 24, 2014, 14:23
Default
  #320
Member
 
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5
vishal_s is on a distinguished road
Hi Bobi ,
Thanx for your suggestion... right now I am trying sort it out what is happening after the modification.
Hi Tobi,
Thanx for your suggestion. In my case Zvar is between 0 to 0.1. I also attached the plotting of Z and Zvar after 14.05*1000 iteration. I am in thinking that turbulent intensity should be more as I get very less Zvar with respect to expected Zvar.

pls suggest something....

Plot for Z and Zvar...
https://www.dropbox.com/s/uvcm5zy73i...ilon_14.05.pdf
vishal_s 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



All times are GMT -4. The time now is 02:34.