[Tobi]

Originally Posted by babakflame

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:

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:

 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

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

[payal05]

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 :

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

[TBO]

Originally Posted by hayhari

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

[wyldckat]

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]

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

[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.

[babakflame]

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:

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

[yash.aesi]

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

[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

[vishal_s]

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.....

[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)

[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:

      varZ_ = 1.0 * sqr(delta()) * magSqr(fvc::grad(this->thermo().Z()));

• The scalar dissipation rate in LES is calculated as

      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

[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

[vishal_s]

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

[babakflame]

Hi vishal

1- check your courant number. it should be less than 0.4
2- check your grid quality with

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

[vishal_s]

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]

Hi Bobi,

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

Regards
vishal

[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

[babakflame]

Hi Vishal

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

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.

[vishal_s]

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