[Tobi]

Originally Posted by yash.aesi

greetings oll ,

i have a small doubt that in 0 folder the value of each species (like CH4) in boundary fields is in mole fraction . rite ?? not the mass fraction

correct me if i am wrong




Thank you ,
Regards
sonu

You have no species in the folder 0!
Otherwise you have the MASS FRACTION!

        // 13 - species mass fractions

-> OpenSMOKE_PDF_Flamelet.cpp

Regards
Tobi

[TBO]

I was to quick with answering, I didn't see the reply of Tobi untill I posted my reply

Originally Posted by yash.aesi

greetings oll ,

i have a small doubt that in 0 folder the value of each species (like CH4) in boundary fields is in mole fraction . rite ?? not the mass fraction

correct me if i am wrong




Thank you ,
Regards
sonu

[Tobi]

Hey all,

if anyone is interessted in building a open source calculation flamelet library / program you can send me an message.

Tobi

[payal05]

Greetings Tobi,
actually after doing the given tutorial , i started to solve my case but to have some fair amount of idea i tried to use the PDF-library of the tutorial and rest of the files according to my own problem .

case running well , but i don't have any idea up-to how much time i should run it ? i tried to check the initial and final residual but there is still difference after T=15000 .
so can you plz guide me through this .
Thank You :
Regards ,
Payal

[babakflame]

Hi Payal

but i don't have any idea up-to how much time i should run it ? i tried  to check the initial and final residual but there is still difference  after T=15000 .

Sometimes in numerical simulations the residual traps in a loop and it goes up and down alternatively (fine variations). My suggestion for you is check Temp along centerline ; If noticeable variations did not occur, You have reached your solution.

@ Tobi
Hi buddy
I have found a point in flamelet model 2.2.x look-up table folder.
You have put these lines in runFlameletGeneration.sh file:

kinetics="PolimiC1C3"                                                    #
                                                            #
# aiabate flame                                                        #
fEd[0]=-800                                                        #
                                                            #
# defects

It seems that instead of 0 , you have taken -800 for adiabatic situation. Is it right buddy? I mean although with radiation; we apply non-adiabatic flamelet. But as you might remember; Alberto had suggested to take into account adiabatic flamelet solution (Zero Enthalpy Defect) in his user guide.

Another question buddy:
Have you ever simulated a bluff-body stabilized flame (Sydney Items) with the solver?
If hopefully yes, How was your accuracy?

Regards
Bobi

[payal05]

Thanks Bobi , i wl check that .....

[Tobi]

Hi all,

@Bobi,

1. thanks for your hint to the tutorial with the wrong enthalpy defect for the adiabatic state. I changed that file. I think this mistake was a wrong key pressing in vim but now its corrected.
2. I never simulated a bluff-body stabilized flame. But I think Alberto and his team did it. But I am not sure if I mean the right kind of flames. So I can not give you an advice.
3. At the moment I am configurating my new server and therefor I have no time for cfd anymore. I wanted to calculate a complex gas burner but not now.


@payal,

1. hello and welcome to the libOpenSMOKE thread.
2. for checking if your simulation is converged you have several options:

a) checking the residuals with pyFoam/gnuplot or what ever you want. But keep in mind, that with the SIMPLE algorithm its not possible to get always nice residual graphics (eg. sandia flame tutorial - does not converge after 20.000 iterations; and would not du it)
b) Check the residuals till they have a steady / or periodic fluctuations after that check your last timesteps (maybe everry 50 or 100 iterations; eg. 1500 1550 1600). If you can not realize big changes in your domain (U,T,csi etc.) then your solution should be converged. Problem of that solver is, that combustions always are very instationary and its hard to get a converged solution. There are always fluctuations in your domain - compare the CH4N2H2 flame - there is at the nozzle a field with fluctuation of U, and p so you will never get a convergence till 1e-6 or something like that.
c) Play with schemes and relaxation factors
d) check the transient solver (PISO algorithm). Compared with the steady state solution you will get a very good convergence compared with SIMPLE algorithm in the tutorial case. Negativ aspect - not steady and therefor it take long time for calculation.

3. you have to create new PDF-Libs for your problem


Regards
Tobi

[babakflame]

Hi Tobi

I think I have found my problem with complex flows. In my bluff-body stabilized burner (according to exp data) I should confront negative velocity fields (Due to recirculation zones both for fuel and oxidizer jets), However the achieved numeric data has minimum of zero.
I took a look into fvSchemes file. I found that my scheme for velocity is bounded i.e. can not take negative values.

divSchemes
{
    div(phi,U)          bounded Gauss limitedLinearV 1;
    div(phi,epsilon)     bounded Gauss limitedLinear 1;
    div(phi,k)          bounded Gauss limitedLinear 1;
    div(phiU,p)        bounded Gauss limitedLinear 1;

    div(phi,H)          bounded Gauss limitedLinear 1;
    div(phi,Z)        bounded Gauss limitedLimitedLinear 1 0 1;
    div(phi,Zvar)          bounded Gauss limitedLimitedLinear 1 0 0.25;

    div((muEff*dev2(T(grad(U))))) Gauss linear;
}

My suggestion is changing div(phi,U) and div(phiU,P) from bounded Gauss to Gauss upwind.

Do you have any hint for me that which type should I select to show the negative fields more accurate?

Regards
Bobi

[TBO]

Originally Posted by babakflame

I found that my scheme for velocity is bounded i.e. can not take negative values.

Bobi,

Please correct me if I'm wrong, shouldn't the velocity vector U always be positive (so the size of the velocity), of course the different components (Ux, Uy, Uz) can have negative values (which is the case for e.g. a recirculation zone).

Regards

[Tobi]

Hi all,

for the schemes: the bound keyword is a trick for stabilisation:

bound = Sp(...)

Its not a bounding scheme itselfs like:

Gauss limitedLimitedLinear 0 1 0,4

This scheme limits/bound your variable from 0 to 1 (like alpha1 or csi) with an limiter used of 40% (0,4).

To clear the mind - the following declaration should be correct:

Gauss limitedLinear 0 = Gauss linear

Due to your fact of negative recirculation zones.
TBT is correct - a vector is only positiv - just its components can be negativ.

In the sandia flame you have already recirulation fields.

[yash.aesi]

Greetings Tobi ,

the tutorial with the wrong enthalpy defect for the adiabatic state. I changed that file. I think this mistake was a wrong key pressing in vim but now its corrected.

So, in runFlameletGeneration.sh file:

# aiabate flame                                                        #
fEd[0]=-800

can you plz mention what has to change in the above code ? is it that enthalpy defect (-800) should be changed to zero ?


Thank You ,
sonu

[babakflame]

Hi all

@sonu
Simply, replace -800 with 0 and it's ok.


@Tobi
Thanks buddy for your hints.However, My problem is clearly poor prediction of flow field especially when we leave the near-field region; Do you have any hint for me?

I have exerted some modifications like as: finer mesh, C1 constant change from 1.45 to 1.60
I think may be change the k-epsilon model and use another model.


@TBO
You are of course right, But actually I meant that my calculated data does not predict negative axial velocities and instead zero or near zero values are presented.

Bobi

[Tobi]

Hi Bobi,

a) can you give me more information about your mesh ? maybe the whole case ? A link to that flame?
b) how fine is your mesh in the area you should have recirculation? Can you give some pictures of U, p?

c) Are your BC correct?
d) A other turbulence model can be used ... hmm...
e) SIMPLE or PISO ? did you tested both?

f) 2D or 3D model?


Hi sonu,

as Bobi mentioned - adiabatic flame means that there is no enthalpy defect. So change the value of -800 to 0.

https://github.com/shor-ty/flameletM...f61a406e0bc7f8

Further more you can find the description (in runFlameletGeneration.sh):

# Description:														#
# This script builds non-adiabatic flamelet libraries for OpenFOAM and fluent used by the binaries from Alberto 	#
# Cuoci. The defects has to be defined like below:									#
#															#
# fEd[0]	 	>>> adiabat flame										#
# fEd[1]   -> fEd[x]	>>> positiv enthalpy defects ( 10 20 30 100 200 ...)						#
# fEd[x+1] -> fEd[end]  >>> negativ enthalpy defects (-10 -20 -30 -100 -200 ...)

Regard

[babakflame]

Hi Tobi

Many thanks for your quick reply.

1- This the link to the HM1 flame http://sydney.edu.au/engineering/aer...uids/bluff.htm
I will email you my 2D mesh (wedge-typed)

2- I think my mesh is fine enough. I have attached a pic of my flow field and temperature. Each stream (fuel and oxidizer) has its own recirculation zone in the wake behind the bluff-body. My problem is predicting of RZ not in the right place that has affected all of data.

3- Although other turbulence models like komegaSST might be more accurate but I have seen papers with k-epsilon presenting bluff-body flames.

4- I have tested both Piso and Simple (the poor velocity field in far-field still appears in both), with no noticeable difference.

5- I have tested both 2-D and 3-D; no difference in accuracy.


Regards

Bobi

[yash.aesi]

Thanks Tobi and Bobi for replying ....

[Tobi]

Hi Bobi,

I think I know where the problem could be.
Just let me check your geometry today night. I will have a try on that

Bluff - Body - Flame.

As I understand it right. The fuel is in the inner nozzle and the nozzle has a big thickness so you get air and fuel recirculation areas ?

[payal05]

Greetings all ,
i have a few very basic doubts. someone please clarify. i was just going through the Sandia_CH4H2N2 tutorial and there

PHP Code:

1. In look up table, in data.inp file ,  how that flame position = 0.9 is given . how to decide what should be the value i.e location of the flame ?
2. Again in the input.inp file of look up table , No. of variance = 30 and stretching factor = 1.17 . so how these values are decided ? 


i know it sounds a bit odd to ask these doubts here , but plz don't mind and reply .


Best Regards ,
Payal .

[Tobi]

Originally Posted by payal05

Greetings all ,
i have a few very basic doubts. someone please clarify. i was just going through the Sandia_CH4H2N2 tutorial and there

PHP Code:

1. In look up table, in data.inp file ,  how that flame position = 0.9 is given . how to decide what should be the value i.e location of the flame ?
2. Again in the input.inp file of look up table , No. of variance = 30 and stretching factor = 1.17 . so how these values are decided ? 


i know it sounds a bit odd to ask these doubts here , but plz don't mind and reply .


Best Regards ,
Payal .

Hi,

first question - this variable has no sence to me
I tryed several settings but nothing changed in the files - maybe its "initial" value to be faster in the iterations ? dont know - maybe its not used in the binaries (could be as possible too).

second question - this is the math background. You create flamelets (2D - solutions). This solution describe every pyhsical and chemical variable like - temperature, density, mass fraction, cp ... depend on the mixture fraction Z. This flamelets are steady - state laminar flamelets and could be used for counterflow diffusion flames (like a candle).


For ingenieering issues we always (or in most of the topics) have turbulent flow fields to get a better mixture of air and fuel. For that we have to expand the counterflow flamelets for turbulent flow fields. With the reynolds-average method we will have the average mixture fraction Z and its fluctuation Z''. In re-search it could be found that the best application for that is the favre averaging ... (i stop here).

The thing you should know now it that you expand all variables which depend on the mixture fraction Z are now dependend on the average mixture fraction Z and its fluctuation Z'' (turbulent flow fields).

This expansion are generated with the PDF's (probability distribution functions) for all variables (phi).

Exeption 1: enthalpy-defect = delta dirac function
Exeption 2: scalar dissipation = log normal function (I hope its correct )


Back to the topic for Z and Z''.

In the attachment you find two pictures.
The first one is the 2D graphic - phi depends on Z
The second one is the 3D graphic - phi depends on Z and Z''

How many calculation points you set for Z'' = No. of variance (here = 20 points)
Further more you realize that the gradients are very high between 0 < Z'' < 0.1

So you can set a strech factor so that you can get more lines / points in the area of high gradients.

At least you normalize the variance:

Z is defined as: 0 <= Z <= 1 (0 = oxidator, 1 = fuel)
Z'' is defined as: 0 <= Z'' < 0.25 (that depend on the beta-PDF)

OF solves two equations for Z and Z'' and for that you can interpolate in those graphics.
The trick therefor is to normalize the Z'' lines so that the value is new defined:

Z''_normalized defined as: 0 <= Z''_normalized <= 1


That is shown in picture 3.
If you have that both values Z and Z''_normalized you can calculate all variables (area weighted interpolation).


Hope that are enough information.

regards Tobi

[Tobi]

At all,

I updated the flameletPisoFoam and flameletSimpleFoam tutorial (update of files) ... nothing necessary but for a clean tutorial its helpful.

Regards
Tobi

[payal05]

Thanx Tobi for such a explained answer and clearing my doubts. Also for updated tutorial




Regards,
Payal.