[Tobi]

Hi Bobi, thanks for trying my libs and solvers.

After you told the problem, I tried to compile it on a other machine and realized that I made a stupid error with the folder names

Delete the folder "flameletModel" and download it again.
I ll make the changes in a few minutes (DONE)

After that everything should work fine and notice that you have to build the libraries first.
For that I added an "Allwmake" script in the libraries folder

If there are other problems, let me know.

Tobi

[Tobi]

Originally Posted by MaximeIST

Hi Tobi

Thanks a lot for sharing your work, I think I will try your flamelet solver in a close future. I will let you know how it is going.

Best Regards,
Maxime

Hi Maxime,

that sounds good.
The problem in that tool is, that its not well tested.
I am looking forward to the update from Alberto that I can resimulate the cases in my thesis in hope to get better quantity results.

For free-stream flames the model gives very nice and good results (like in my thesis shown for CO/H2/N2).
In the presentation of the 5th workshop Alberto gives the results for three or four free-stream flames with very good results.

But for a closed chamber I made no good results. Hence its necessary to get more information about complex chamber simulations.
In seven month its not possible to get familiar with that whole theory and make a lot of simulations.

Especially there should be an URANS solver avaiable for testing and comparing.
I build the turbulentFlameletRhoPimpleFoam but its not stable and the calculation is aborting every time.

I am not sure why that problem occur but I am working on it. I think the next step should be using a transient solver to see if the prediction of the variables Z, Z'', chi and phi_H is changing.

Regards Tobi

Let me know how your experience is.
Tobi

[babakflame]

Dear Tobi
Hi
I have investigated ur sandia3d boundary conditions file in the tutorial folder of flamelet model.we have these lines in it:

internalField uniform 101325;

boundaryField
{
inletfuel
{
type zeroGradient;
}

inletair
{
type zeroGradient;
}

"outlet"
{
type fixedValue;
value $internalField;
}


The world outlet is surrounded by quotation marks. Is it right?
Cause I tried to run this case with my own grid (724000 nodes) and after 452 iterations I got this error:

Time = 452

DILUPBiCG: Solving for Ux, Initial residual = 0.000845421, Final residual = 8.73093e-08, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.000838223, Final residual = 8.46303e-08, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.00037536, Final residual = 8.88454e-08, No Iterations 2
DILUPBiCG: Solving for H, Initial residual = 1.26963e-05, Final residual = 2.0704e-09, No Iterations 2
Correct thermodynamics
DILUPBiCG: Solving for csi, Initial residual = 1.35204e-05, Final residual = 2.20803e-09, No Iterations 2
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5
in "/home/babak/OpenFOAM/babak-2.1.0/platforms/linux64GccDPOpt/bin/rhoSimpleFoamFlamelets_1007"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7
in "/home/babak/OpenFOAM/babak-2.1.0/platforms/linux64GccDPOpt/bin/rhoSimpleFoamFlamelets_1007"
Floating point exception


I have used ur datas for system, constant and 0 folders. Just the grid is mine and I have tested my grid quality in fluent As I had done it in Gambit.Would u plz hint me in this subject?
Also I should note that I have still used the libopenSmoke solver.

Regards
Bobi

[Tobi]

Hi the quotes are not necessary but you can use them if you want to set the same BC for more walls like:

"wallside|wallburner|atmosphere"
{
     type       zeroGradient;
     value     uniform 0;
}

OpenFOAM split that BC into singel BC at the beginning of your simulation. Hence its not an error.


To your problem!
I tested my case again and everything is working fine (see the attachement). I have no experiance with tet meshes. You are probably using a tet mesh, arent you?

Anyway you should check your mesh with the OpenFOAM checking application checkMesh .


Further more you should check the added output while solving your case:

- - - - - - - - - - - - - - - - - - - - - - - - -
rho   min|max:     0.2    1.20256
csi   min|max:     0        1
csiv  min|max:     0        0.0419838
H     min|max:     -998143    -15974.1
- - - - - - - - - - - - - - - - - - - - - - - - -

Especially the fluctuation of the mixture fraction is very instable and the range is limited to [0:0,25]...

If you get over that limit, the solver can handle it but there is something wrong with your BC, mesh or to big relaxation factors.

Write out ever 10th timestep and analyse your variables (if there is an error). Most errors occurs due to csi and csiv2 and bad mesh cells. Analyse the bad regions and think about - how to improve the mesh quality there -.

Further more its very helpful to use pyFoam to have a look at your residual and continuity error. In many cases its gives you the information which variable is not going to converge.


Regard Tobi


PS: thanks for your information. I realized that the 3D tutorial is not working with "Allrun" ... I updated that case now.

[babakflame]

Dear Tobi
Hi
Thanks for ur clues on my problem. I will consruct another grid and will test it very soon.
Also, I tried to use ur solver in the flameletmodel tutorials folder for the case Sandia_CH4H2N2_3D
As I have only 4 processors, I changed mpirun directive in allrun file.
Also I changed number 8 to 4 in decomposepardict file. I don't know whether is there also other files that should I correct or not.
After I executed Allrun and after some preliminary computations I got this error:

Calculating...
[0]
[0]
[0] --> FOAM FATAL ERROR:
[0] number of processor directories = 4 is not equal to the number of processors = 8
[0]
FOAM parallel run exiting
[0]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
--------------------------------------------------------------------------
--------------------------------------------------------------------------
mpirun has exited due to process rank 0 with PID 5771 on
node babak-VPCEA26FG exiting improperly. There are two reasons this could occur:

1. this process did not call "init" before exiting, but others in
the job did. This can cause a job to hang indefinitely while it waits
for all processes to call "init". By rule, if one process calls "init",
then ALL processes must call "init" prior to termination.

2. this process called "init", but exited without calling "finalize".
By rule, all processes that call "init" MUST call "finalize" prior to
exiting or it will be considered an "abnormal termination"

This may have caused other processes in the application to be
terminated by signals sent by mpirun (as reported here).
--------------------------------------------------------------------------
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.x-9234775082d8
Exec : reconstructPar
Date : Dec 07 2012
Time : 14:27:20
Host : "babak-VPCEA26FG"
PID : 5785
Case : /home/babak/OpenFOAM/babak-2.1.x/flameletModel/tutorials/turbulentFlameletRhoSimplecFoam/SANDIA_CH4H2N2_3D
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time



--> FOAM FATAL ERROR:
No times selected

From function reconstructPar
in file reconstructPar.C at line 148.

FOAM exiting

I think there is other places that I should change the number of processors, However I don't know where are they. Would u plz hint me on it?

[Tobi]

Originally Posted by babakflame

Dear Tobi

I think there is other places that I should change the number of processors, However I don't know where are they. Would u plz hint me on it?

Hi,

in the system decomposedParDict you have to change 2 lines.

The first one is your number of processors that you changed already.
Then you have to look at my decompositionMethode -> hierarchical

For that methode you have to change the processors


(4 2 1) = 4 * 2 * 1 = 8

So you can change it to:

(2 2 1) = 2 * 2 * 1 = 4

or so on.

Tobi

[babakflame]

Dear Tobi
Hi
Thanks for all ur helps. I resolved my mistake as u had prescribed. There is also another strange error with this whole thing.
I have compiled & executed ur code successfully on my laptop, however when I tried to compile and install it on my PC for primary CFD runs. I could compile the libraries, But for the turbulentFlameletRhoSimplecFoam solver I got this error:

SOURCE=turbulentFlameletRhoSimplecFoam.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/common/lnInclude -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/flamelets/turbulent/lnInclude -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/pdfThermo/lnInclude -I/opt/openfoam210/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam210/src/turbulenceModels -I/opt/openfoam210/src/turbulenceModels/compressible/RAS/RASModel -I/opt/openfoam210/src/finiteVolume/cfdTools -I/opt/openfoam210/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/turbulentFlameletRhoSimplecFoam.o
turbulentFlameletRhoSimplecFoam.C:34:28: fatal error: basicPdfThermo.H: No such file or directory
compilation terminated.
make: *** [Make/linux64GccDPOpt/turbulentFlameletRhoSimplecFoam.o] Error 1

Also, I should note that I have already installed and compiled gsl & libOpenSMOKE on this PC. I tried to reinstall it Although the efforts were yielded the same result. It seems that it can not identify the basicPdfThermo. H. How does this happens when I have already installed the libraries?


SSSSSSSSSSSOLVED!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! !

I changed the location of flameletmodel folder into the babak-2.1.0 directory. & This mysterious problem solved.

Regards
Bobi

[Tobi]

Originally Posted by babakflame

Dear Tobi
Hi
Thanks for all ur helps. I resolved my mistake as u had prescribed. There is also another strange error with this whole thing.
I have compiled & executed ur code successfully on my laptop, however when I tried to compile and install it on my PC for primary CFD runs. I could compile the libraries, But for the turbulentFlameletRhoSimplecFoam solver I got this error:

SOURCE=turbulentFlameletRhoSimplecFoam.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/common/lnInclude -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/flamelets/turbulent/lnInclude -I/home/babak/OpenFOAM/babak-2.1.0/flameletModel/libraries/pdfThermo/lnInclude -I/opt/openfoam210/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam210/src/turbulenceModels -I/opt/openfoam210/src/turbulenceModels/compressible/RAS/RASModel -I/opt/openfoam210/src/finiteVolume/cfdTools -I/opt/openfoam210/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/turbulentFlameletRhoSimplecFoam.o
turbulentFlameletRhoSimplecFoam.C:34:28: fatal error: basicPdfThermo.H: No such file or directory
compilation terminated.
make: *** [Make/linux64GccDPOpt/turbulentFlameletRhoSimplecFoam.o] Error 1

Also, I should note that I have already installed and compiled gsl & libOpenSMOKE on this PC. I tried to reinstall it Although the efforts were yielded the same result. It seems that it can not identify the basicPdfThermo. H. How does this happens when I have already installed the libraries?


SSSSSSSSSSSOLVED!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! !

I changed the location of flameletmodel folder into the babak-2.1.0 directory. & This mysterious problem solved.

Regards
Bobi

Hi Bobi,

that sounds good.
The problem you had is located in the "Make/options" file. Here the compiler get the information where the files are located (which are needed).

For that I am using a global variable $WM_PROJECT_USER_DIR

EXE_INC = \
    -I$(WM_PROJECT_USER_DIR)/flameletModel/libraries/common/lnInclude \
    -I$(WM_PROJECT_USER_DIR)/flameletModel/libraries/flamelets/turbulent/lnInclude \
    -I$(WM_PROJECT_USER_DIR)/flameletModel/libraries/pdfThermo/lnInclude \

So the compiler searches in that directorys.
If you move the flameletModel folder into a other directory, you have update the paths to the files



But you managed it.
Tobi

[babakflame]

Dear Tobi
Hi
I am executing ur Sandia_CH4N2H2_3D on my PC. It's under execution. During this procedure when I monitor primary parameters in the log file, For instance I get these results or sth like them:

rho min|max: 0.251523 1.20253
csi min|max: 0 1
csiv min|max: -8.24639e+06 6.19117e+15
H min|max: -998143 -15974.1

As u can see mixture fraction variance is not in the desired domain [csiv min|max: 0 0.041983]
Does this influence my final solution and is there any way that I can fix this parameter to the prescribed domain before running the code?

regards
Bobi

[babakflame]

Dear Tobi
Hi

I have executed ur Sandia_CH4H2N2_3D successfully . Although, there are some vague things for me.
First u have chosen the Delta T=1 ,Does this mean that u have marched 1 sec after each iteration?
2- The solution goes for 10000 iterations without any convergance criterion
3- In my results from this simulation, We have a flame after 500 iterations, However after 2000 iterations the flame blowsout. Mysteriously, it comes back after 6500 iterations.

I think that if DeltaT is the real time, it's quantity is too high(1). it can be changed to for instance 0.01 and the maximum iterations can be modified to 1000. Am I right?
Why do we observe blowout?

Best,
Bobi

[Tobi]

Originally Posted by babakflame

Dear Tobi
Hi

I have executed ur Sandia_CH4H2N2_3D successfully . Although, there are some vague things for me.
First u have chosen the Delta T=1 ,Does this mean that u have marched 1 sec after each iteration?
2- The solution goes for 10000 iterations without any convergance criterion
3- In my results from this simulation, We have a flame after 500 iterations, However after 2000 iterations the flame blowsout. Mysteriously, it comes back after 6500 iterations.

I think that if DeltaT is the real time, it's quantity is too high(1). it can be changed to for instance 0.01 and the maximum iterations can be modified to 1000. Am I right?
Why do we observe blowout?

Best,
Bobi

Hi Bobi,

dT does not matter. You are solving a steady state problem and the time derivation dcsi/dt = zero. Its a pseudo-time-step. This belongs to steady state solvers and does not have any references to a time.


To the 3D-case. Its just a test-case that I just created for a sHM tutorial and for having a look at the BC. I never solved that case more than 800 iterations.

If you want results please use the 2D - cases.

You never get a convergence to 1e-6 or something like that. That belongs to the nature of the model. Every 5 iterationsteps you extract the values of phi in each cell and face point. That makes is instabil.

Maybe you can set the relaxation factors to 0.1 to get a better convergence but if you have like an steady fluctuation residual graphic it should be okay.

Write out the last 5 timesteps (after 10 or 20) iterations and have a look at the results with paraview. If there is nothing changing you case is convergenced.


Further more you should know that combustion is mostly instationary so it would be nice if we would have an unsteady solver.

I tried to build one but its not working.


Tobi

[babakflame]

Dear Tobi
Hi
I used the 2D case. Although there are some ambiguities in my mind about the 2D case.
First, why the grid is wedge-shaped? (I had observed this shape in libOpenSMOKE cases too.)
Second, the case converges too soon, However I anticipated further time. Have u compared the results with experimental configuration strictly? ( I will do it very soon by myself).
Third, We see for instance Omega_H2O in the recorded results. Does this refer to H2O mas fraction? (As u know in combustion literature omega refers to production rate however we need mass fractions to compare with experimental results.)

Best,
Bobi

[Tobi]

Originally Posted by babakflame

Dear Tobi
Hi
I used the 2D case. Although there are some ambiguities in my mind about the 2D case.
First, why the grid is wedge-shaped? (I had observed this shape in libOpenSMOKE cases too.)
Second, the case converges too soon, However I anticipated further time. Have u compared the results with experimental configuration strictly? ( I will do it very soon by myself).
Third, We see for instance Omega_H2O in the recorded results. Does this refer to H2O mas fraction? (As u know in combustion literature omega refers to production rate however we need mass fractions to compare with experimental results.)

Best,
Bobi

Hi,

as you can see in the libOpenSMOKE User Guide and the User Guide I made the omega_YY is the mass fraction of the species.

I dont understand your meaning of: "The case is converging too soon"? What do you mean?

And YES I compared the measurements of SANDIA CO/H2/N2 flame with my simulations. very good results.

Like I told befor - have a look at the 5th OpenFOAM Workshop:

Cuoci A., Leoni E., Frassoldati A., Faravelli T., Ranzi E., “Non adiabatic steady laminar flamelet model in OpenFOAM”, Fifth OpenFOAM Workshop, Gothenburg (Sweden), 21-24 June 2010 (http://web.student.chalmers.se/groups/ofw5/Program.htm)


The tutorials have to be wedge shaped. Why not? You are simulating an 2D - circle symmetric problem. Therefor openfoam give the ability to do it with wedge shapes. For more information please read the user guide "Chapter Mesh 5.2.2".

http://www.openfoam.org/docs/user/boundaries.php

Regards
Tobi

[markusrehm]

Hi Tobi,

looks very interesting. Will you thesis be publicly available?

Regards, Markus.

[Tobi]

Originally Posted by markusrehm

Hi Tobi,

looks very interesting. Will you thesis be publicly available?

Regards, Markus.

Hi,

my thesis is not public

[wyldckat]

Greetings to all!

@Tobi:

Originally Posted by Tobi

my thesis is not public

A few quick questions:

• Then is there any way for private entities access it? For example, can anyone go in person to the library of the Institute and request to view the thesis?
• Is it accessible as pay-per-view or via business contract with the Institute?
• In essence: who and how can people legally see your thesis?

Best regards,
Bruno

[Tobi]

Originally Posted by wyldckat

Greetings to all!

@Tobi:

A few quick questions:

• Then is there any way for private entities access it? For example, can anyone go in person to the library of the Institute and request to view the thesis?
• Is it accessible as pay-per-view or via business contract with the Institute?
• In essence: who and how can people legally see your thesis?

Best regards,
Bruno

Hi Bruno,

I have an arrangement of confidentiality. After five years its possible that I can publish it. I ll have a meeting on 18.12. with the company. I will ask them, if its possible for other people to get the thesis in any way.

I ll give you a feedback on 18.12.
Tobi

[babakflame]

Dear Tobi
Hi
In experimental results, we have two sets of datas: Favre and rms . I think that the results that we see in paraview (RAS solutions) are Favre averaged datas. But what about Temperature and mixture fraction rms fluctuations? Can we exploit them from our RAS solution? have u reached a conclusion about this problem?
Best,
Bobi

[Tobi]

Hi Bobi,

everything you see in paraview is Favre-Weighted.
The reason of that is the cacluation of the flamelets.

A favre weighted is much cheaper.

For favre weighted variables you have to replace the density with the reynolds density. This value you are extracting from the look up tables.


RAS and Favre are the same if you are using density weighted calculation.


I always compared favre values

[babakflame]

Dear Tobi
Hi
I see some deviations in my results from experimental results in SANDIA_CH$H2N2 2D case. I want to refine the mesh.( Atleast two times)
I think that in blockMeshDict file, I should modify the following lines:

blocks
( //(h e v )
hex (0 1 2 0 3 4 5 3) (4 1 25) simpleGrading (1 1 0.4)
hex (3 4 5 3 6 7 8 6) (4 1 150) simpleGrading (1 1 15)
hex (9 11 12 10 4 13 14 5) (50 1 25) simpleGrading (7 1 0.4)
hex (4 13 14 5 7 15 16 8) (50 1 150) simpleGrading (7 1 15)

);

I suggest that middle parentheses should be modified like the following:
(8 1 50)
(8 1 300) ......

Am I right? Is there other places that should change?

Best,
Bobi