[Divyanshu01]

Hello all !
I have been trying to simulate Sandia D flame using LES, but an error message always shows up, which is,


--> FOAM Warning :
From function Foam::scalar Foam::janafThermo<EquationOfState>::limit(Foam::sc alar) const [with EquationOfState = Foam::perfectGas<Foam::specie>; Foam::scalar = double]
in file /home/ubuntu/OpenFOAM/OpenFOAM-5.x/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 117
attempt to use janafThermo<EquationOfState> out of temperature range 250 -> 3000; T = -184.276


and a series of such messages with different values of T. I can see that T is diverging but I can not figure out the cause.


The program then terminates with the message,


#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::combustionModels::EDC<Foam::combustionModels ::psiChemistryCombustion>::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Floating point exception (core dumped)




Please help me understand the cause of divergence and meaning of this last message.


Thanks.

[arvindpj]

Originally Posted by Divyanshu01

Hello all !
I have been trying to simulate Sandia D flame using LES, but an error message always shows up, which is,


--> FOAM Warning :
From function Foam::scalar Foam::janafThermo<EquationOfState>::limit(Foam::sc alar) const [with EquationOfState = Foam:erfectGas<Foam::specie>; Foam::scalar = double]
in file /home/ubuntu/OpenFOAM/OpenFOAM-5.x/src/thermophysicalModels/specie/lnInclude/janafThermoI.H at line 117
attempt to use janafThermo<EquationOfState> out of temperature range 250 -> 3000; T = -184.276


and a series of such messages with different values of T. I can see that T is diverging but I can not figure out the cause.


The program then terminates with the message,


#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::combustionModels::EDC<Foam::combustionModels :siChemistryCombustion>::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Floating point exception (core dumped)




Please help me understand the cause of divergence and meaning of this last message.


Thanks.

Use a temperature limiter in fvObjects to constrain the temperature between Tmin and Tmax. But this is usually a fix, the main cause may be due to large time step or some of the reaction ODE settings.

Cheers,
Jay

[Zhiheng Wang]

Originally Posted by arvindpj

Use a temperature limiter in fvObjects to constrain the temperature between Tmin and Tmax. But this is usually a fix, the main cause may be due to large time step or some of the reaction ODE settings.

Cheers,
Jay

Hello,
Please give a brief about combustion model, constant/reaction file , chemistryProperties file( in case of Arrehinius rate) and boundary condition.
it seems your temperature is going down compared to the minimum temperature in thermo.gasproperties may be you are using wrong combustion parameters.

[Sandeep lamba]

Hi all,

I am trying to simulate Sandia Flame D with FGMFoam, I have already done RANS of the same and got desired results. Now as I am trying to simulate it with LES I have done some fixes such as Turbulent inlet conditions for Velocity and changing turbulent model to LES (kEqn and Smagorinsky ). Also I have worked on the mesh refinement. But, still I am not getting acceptable results infact getting very poor results. (some contours are attached ). The simulation starts very well but only up to a small time (0.045 Sec). But later on the dissipation stops as can be seen in the contours attached.


Someone please comment on the problem.

Thanks in advance.


Kind regards
T_nut_Ch4_0.4.jpg

T_nut_Ch4_0.03.jpg

T_nut_Ch4_0.05.jpg

T_nut_Ch4_0.06png.jpg

[STHX]

Hi Sandeep,

I tried similar LES this weekend. It seems that LES results are not correct for following reasons.
1) Grid is not refined for LES (in case you are using similar grid size as RANS tutorial)
2) LES is strictly for 3D simulations.

Because of second reason, 2D LES will be wrong irrespective of how refined your grid is.

Hope it helps. I have not tried 3D LES yet, for it takes more computation resources.

[Sandeep lamba]

Thanks for the reply and suggestion. Now I am moving to 3D and first trying RANS. I have made 45 Degree segment of Sandia flame (mesh pic link https://drive.google.com/file/d/1Z_o...ew?usp=sharing). Now I am confused which type of boundary condition should be given for the symmetric cut sections. I have used CyclicAMI but when simulation run new error of ''No MRF model persent'' appears. Any hint regarding this please.

[Sandeep lamba]

I did some fixes with my mesh and now using 3D geometry. I am getting some improved results. But, there seems some problems with Pressure fields (pressure wave are visible in domain). the boundary conditions for U is fixed value at inlet and inletoutlet at outlet. For pressure it is zerogradient at inlet and totalPressure at outlet.
The combustion model is FGM and LES model is kEqn.
Anyone please comment.
the link for contours is here:

https://drive.google.com/drive/folde...0y?usp=sharing

kind regards


Sandeep Lamba

[piu58]

The inletoutlet b.c. may be problematic. I recommend at least make a few experiments with zero gradient first.

LES is very demanding in all of the model: Mesh, boundary conditions, schemes. So I recommend further starting with conservative schemes firs.

It is always a good idea of using relaxation factors.

You need first stabilize the simulation. At the next step you should get the results in the expected range of values. In your case, this is near the inlet.

If you managed this you may start to get reliable results for the more problematic regions of your simulation.

[Sandeep lamba]

Thank you Uwe Pilz for quick reply. I used zeroGradient at outlet and also relaxation factor as you told and it worked. There are no more pressure wave, other fields are also improved.
Again thanks a lot.


kind regards

Sandeep Lamba

[Amirreza_pro]

Hi guys, I'm new to openFoam and I have a question about simulation of Sandia Flame D.
I have already simulated Sandia_D with RAS in openFoam.
Now I'm going to simulate Sandia_D with LES.
But I don't know how to change the set up to get the results for LES.
Should I change the setting for the RAS model or there is alreay a test case in toturial folders.
I would be appreciated if someone can help me by this case.

[kont87]

Originally Posted by Sandeep lamba

Hi all,

I am trying to simulate Sandia Flame D with FGMFoam, I have already done RANS of the same and got desired results. Now as I am trying to simulate it with LES I have done some fixes such as Turbulent inlet conditions for Velocity and changing turbulent model to LES (kEqn and Smagorinsky ). Also I have worked on the mesh refinement. But, still I am not getting acceptable results infact getting very poor results. (some contours are attached ). The simulation starts very well but only up to a small time (0.045 Sec). But later on the dissipation stops as can be seen in the contours attached.


Someone please comment on the problem.

Thanks in advance.


Kind regards
Attachment 82469

Attachment 82470

Attachment 82471

Attachment 82472

LES implementation in OF is 3D, due to filter size implementation I believe.
In the literature, there are different mesh sizes used for that specific case, some people had very good results as low as 500000-1M cells.

[saeed jamshidi]

Originally Posted by piu58

The inletoutlet b.c. may be problematic. I recommend at least make a few experiments with zero gradient first.

LES is very demanding in all of the model: Mesh, boundary conditions, schemes. So I recommend further starting with conservative schemes firs.

It is always a good idea of using relaxation factors.

You need first stabilize the simulation. At the next step you should get the results in the expected range of values. In your case, this is near the inlet.

If you managed this you may start to get reliable results for the more problematic regions of your simulation.

Hi piu58,

Thank you for your usefull comments.

I accidentally red this thread and saw your responce. I fully understand the importance of BC, discretization and even Mesh refinement. But, I have heared that it is not usual to use relaxation factors when we are using Piso or Pimple algorithm! we just consider all of the factor as following:

relaxationFactors
{
   
    equations
    {
        ".*"        1;
    }
}

Would you please explain a little bit about this matter.
Thank you.

[piu58]

In transient simulation, relaxation leads to slower changes than in reality. But it dampens all kind of oscillations which occur very often, especially at critical regions of your simulations. Starting from this oscillations, your simulation may blow off.

If you need the transient phase, you should reduce relaxations in the last steps: After your simulation works well.