[Dan1788]

Dear all,

I am simulating a piloted premixed flame using reactingFoam (OpenFoam 2.2.0). Below shown is the grid.

https://www.dropbox.com/s/hcb7tqhylz...itled.jpg?dl=0

Also attached is the 0, constant and system folder inputs.

As shown, the mesh consists of bluff body walls with a coflow and a high temperature hydrogen pilot near the premixed inlet that consists of CH4+O2.

I am using the PaSR model of reactingFoam and k-epsilon turbulence model for my simulations.

The problem I face is that when I run the simulation with chemistry and reactions on and 1500 K given as boundary condition to the inlet of the pilot, the premixed mixture does not react. When I look at the contour plot, the entire domain is 300 K

Is there any artificial technique by which I can model ignition, using a spark or setting a high temperature patch in the computational domain??

Please help me out of this impasse I am facing. Thanks!

[Howard]

Hi man, I a new user of OpenFoam. I'm now also trying to use reactingFOAM for simulation of premixed combustion. I tried your case but failed. Could give me some suggestion about how to use reactingfoam to simulated premixed combustion? I will appreciate it very much if you could give me help.

[remir]

Hi,

couldn't open the dropbox link, I wanted to check your reaction file.

Anyways, if you want to artificially ignite, you can use a fvOptions file in the /system dir.
You could also set a flame front using a setField (try swak4foam if you havn't already).

If the reaction is not too complex, you can try another chemistry ODE solver than SIBS.

To answer Howard as well, here is a typical methane-air premixed case I work on, using the PitzDaily tut as a base and a simple chemistry.

Hope it helps,

Remi

[Howard]

Originally Posted by remir

Hi,

couldn't open the dropbox link, I wanted to check your reaction file.

Anyways, if you want to artificially ignite, you can use a fvOptions file in the /system dir.
You could also set a flame front using a setField (try swak4foam if you havn't already).

If the reaction is not too complex, you can try another chemistry ODE solver than SIBS.

To answer Howard as well, here is a typical methane-air premixed case I work on, using the PitzDaily tut as a base and a simple chemistry.

Hope it helps,

Remi

Thank you very much! I would like to ask if I want to use multistep reaction mechanism, how to choose the solver, or where could I learn about the information related to solvers. You are really a GAOSHOU in this area, could you give me some suggestion about how to learn these detail things of reactingFOAM and OpenFoam? I just started reading the userguide but found lots of parameters in reactingFOAM don't understand.

[remir]

Well, for multistep reactions with premixed-combustion, I think reactingFoam is really the one you want to go with.

For more detailed information, you should be able to find most of them already written in this forum, or on links like this one http://www.openfoam.org/version2.3.0/numerics.php (information about ODE solvers, important when dealing with detailed chem).

Good luck !

[Howard]

Thank you very much for your case.

[Howard]

Originally Posted by remir

Well, for multistep reactions with premixed-combustion, I think reactingFoam is really the one you want to go with.

For more detailed information, you should be able to find most of them already written in this forum, or on links like this one http://www.openfoam.org/version2.3.0/numerics.php (information about ODE solvers, important when dealing with detailed chem).

Good luck !

Thank you very much for your case. I tried it, but I have a question, the terminal often shows the' time step continuity errors' though the programme continues to operate. What's more, I was wondering since it's a premixed combustion, how to set the equivalence ratio as the XiFoam has this parameter, but I haven't seen in your file.

[remir]

Hi,

about the time step continuity error, is this something that appears only at the begining of the simulation? During the ignition, the temperature may become very high, leading to some unphysical behaviours. You could try and change the value of "h" in /system/fvOptions.

Also, my best practise for combustion with more detailed chemistry is to always ignite with a one-step chemistry, much easier and stable. Then a switch to a more complex set of equations.

Regarding the equivalence ratio now:

In XiFoam, the parameter you change in CombustionProperties does not affect the thermodynamics of your mixture. You can check it by changing the ER from 1 to 0.5, the temperature field should remain approximately the same. The parameter is used for transport properties I think.

In reactingFoam, the user must manually calculate the corresponding mass fractions of methane, O2 and N2 and write the values in /0/CH4(O2,N2). You could create a simple program to do it for you, check the theory online.
In the file I gave you, the ER should be around 0.8.

Good luck,

Remi

[Howard]

Originally Posted by remir

Hi,

about the time step continuity error, is this something that appears only at the begining of the simulation? During the ignition, the temperature may become very high, leading to some unphysical behaviours. You could try and change the value of "h" in /system/fvOptions.

Also, my best practise for combustion with more detailed chemistry is to always ignite with a one-step chemistry, much easier and stable. Then a switch to a more complex set of equations.

Regarding the equivalence ratio now:

In XiFoam, the parameter you change in CombustionProperties does not affect the thermodynamics of your mixture. You can check it by changing the ER from 1 to 0.5, the temperature field should remain approximately the same. The parameter is used for transport properties I think.

In reactingFoam, the user must manually calculate the corresponding mass fractions of methane, O2 and N2 and write the values in /0/CH4(O2,N2). You could create a simple program to do it for you, check the theory online.
In the file I gave you, the ER should be around 0.8.

Good luck,

Remi

Hi, man thank you very much for your case, it could work! now I'm considering to use multi-step mechanism. I read this forum and some mentioned just like below, but it seems not work. What I have try is to write two fuels reaction equations as below, both fuels have more than one reaction steps. Is there something wrong?
reactions
{
Reaction1
{
.....
}
Reaction2
{
......
}
}

What's more, your case uses PaSR combustion model, do you kow if I want to change to other like flamelet model, how to manage this? Thank you!

[remir]

Hi,

for your reactions, you'll have to be a little more specific
Maybe there is just a unit problem in your coefficients ? Can you post the detailed equations as well as the link to where you found them?

There are two ways to write your reactions in OpenFOAM:
writing them in chemkin format in chemkin/chem.inp
writing them in constant/reaction using OpenFOAM format.

To switch from chemkin to OpenFOAM format, you can use: chemkinToFoam chem.inp therm.dat reactions thermo.compresibleGas (note that all files have to be in the same file before you run the program).
This will convert your chemkin files (chem.inp and therm.dat) and write the results in reactions and thermo.compressibleGas.

Now, about the combustion model, you might want to check this thread: http://www.cfd-online.com/Forums/ope...meletfoam.html

[Howard]

Originally Posted by remir

Hi,

for your reactions, you'll have to be a little more specific
Maybe there is just a unit problem in your coefficients ? Can you post the detailed equations as well as the link to where you found them?

There are two ways to write your reactions in OpenFOAM:
writing them in chemkin format in chemkin/chem.inp
writing them in constant/reaction using OpenFOAM format.

To switch from chemkin to OpenFOAM format, you can use: chemkinToFoam chem.inp therm.dat reactions thermo.compresibleGas (note that all files have to be in the same file before you run the program).
This will convert your chemkin files (chem.inp and therm.dat) and write the results in reactions and thermo.compressibleGas.

Now, about the combustion model, you might want to check this thread: http://www.cfd-online.com/Forums/ope...meletfoam.html

Thank you so much for your reply! Really beneficial. I will have a try of what you told.
Now I operate the reactingFoam and XiFoam, but the result seems not the same. I am considering the 'combustion properties' maybe the reason, for your reactingFoam case, the combustionMoel is PaSR_ but XiFoam not. So do you know is there any other combustionMoel available in reactionFoam? or where to find this information.
The other thing is in XiFoam 'combustionProperties' has some paramerters like ignitionthickness,ignitionSphereFraction which your reactingFoam case doesn't have. Do you think the sentences of ignition can be added to reactingFoam?

[remir]

Hi,

I don't think reactingFoam has a completely different combustion model available. You could use rhoReactingFoam, but it won't change that much your simulation.
For XiFoam's properties in combustionProperties, they are indeed a little tricky to set. I think you could set ignition to off and use the same fvOptions as in reactingFoam to ignite. I don't know if this works, but you can have a try !

I have also read sa while ago that ignition in reactingFoam could be realized in the same fashion as for XiFoam, but I can't put my hands on this thread anymore, sorry.

Anyways, best of luck for this, it's not easy to ignite, with both solvers !

[Howard]

Originally Posted by remir

Hi,

I don't think reactingFoam has a completely different combustion model available. You could use rhoReactingFoam, but it won't change that much your simulation.
For XiFoam's properties in combustionProperties, they are indeed a little tricky to set. I think you could set ignition to off and use the same fvOptions as in reactingFoam to ignite. I don't know if this works, but you can have a try !

I have also read sa while ago that ignition in reactingFoam could be realized in the same fashion as for XiFoam, but I can't put my hands on this thread anymore, sorry.

Anyways, best of luck for this, it's not easy to ignite, with both solvers !

Hi remir, thanks a lot for your answers. Now I generally understand the reactingFoam. However, there are still some questions: In the 'reactions' document, is the 'Ta' activation energy? Because in CHEMKIN this position should be Ea(activation energy). What's more, in 'Chemstry Properties', I read some tutorial and cases that there is a 'turbulent Reaction' on selection but in your case not. Finally, I read your document ' fundySetfieldDict' but I don't know what's that meaning.

[remir]

Hi,

OpenFOAM uses activation temperature in K, while chemkin uses activation energy in cal/mol. Hence the need for a converter (chemkinToFoam).

FunkySetField is an OpenFOAM application I installed a while ago, that enables the setting of "strange" initial conditions. You don't have to use it.

About Turbulent Reaction, I also have little clues about what it does. My guess is that it controls the PaSR model to some extent. I disabled it to test its impact on the simulation, and forgot to put it back on when I created the test case.

Good luck !

[Howard]

Originally Posted by remir

Hi,

OpenFOAM uses activation temperature in K, while chemkin uses activation energy in cal/mol. Hence the need for a converter (chemkinToFoam).

FunkySetField is an OpenFOAM application I installed a while ago, that enables the setting of "strange" initial conditions. You don't have to use it.

About Turbulent Reaction, I also have little clues about what it does. My guess is that it controls the PaSR model to some extent. I disabled it to test its impact on the simulation, and forgot to put it back on when I created the test case.

Good luck !

Hi, remir. So appreciate your answer! I tried the multistep mechanism and it works. Now I try to use some other multistep mechanism but the problem is what I find is like the attachment is GRIMech, do you know how to use it in openfoam or translate to CHEMKIN format? Another question is in the ignition part what's the meaning of 'h', do you have some opinion of how to set the number? And finally, I would like to ask that if the CH4 and other reactants in the '0' folder the percentage number is massfraction? or maybe molfraction? Thank you!

[remir]

Hi,

I am also stuck at trying to figure out how to use these kinds of mechanism directly in OpenFOAM. I think it has not been done yet, or at least not reported in this forum.

Regarding the value of h, unfortunately, this is mainly trial and error. From my experience, it can range from 1 to 100, depending on your mesh, flow conditions and mechanism.

Finally, OpenFOAM only uses mass fraction !

Let me know if you find how to use this mechanism

[Howard]

Originally Posted by remir

Hi,

I am also stuck at trying to figure out how to use these kinds of mechanism directly in OpenFOAM. I think it has not been done yet, or at least not reported in this forum.

Regarding the value of h, unfortunately, this is mainly trial and error. From my experience, it can range from 1 to 100, depending on your mesh, flow conditions and mechanism.

Finally, OpenFOAM only uses mass fraction !

Let me know if you find how to use this mechanism

Hi, remir. About the detailed mechanism data, I think that could be built by yourself according to some literature. And the data source could be found from some websites like http://www.reactiondesign.com/suppor...chanisms-data/ .Good luck.

[Howard]

Originally Posted by remir

Hi,

I am also stuck at trying to figure out how to use these kinds of mechanism directly in OpenFOAM. I think it has not been done yet, or at least not reported in this forum.

Regarding the value of h, unfortunately, this is mainly trial and error. From my experience, it can range from 1 to 100, depending on your mesh, flow conditions and mechanism.

Finally, OpenFOAM only uses mass fraction !

Let me know if you find how to use this mechanism

Hi, remir. When I try to use the chemkinToFoam, the terminal shows HOCO not found in table. valid entries:
53
(
OH
CN
C2H3
.
.
.

does this mean OpenFoam can't deal with these species like HOCO? what can do then?

[remir]

Hello,

I think it just means that you forgot to specify the thermodynamic data for this species in particular !
Or maybe the name changed a little after the conversion and you have to find it manually in thermo properties.

Hope this solves your problem.


ps: thanks for the previous link you mentioned, I'll have a look

[Howard]

Originally Posted by remir

Hello,

I think it just means that you forgot to specify the thermodynamic data for this species in particular !
Or maybe the name changed a little after the conversion and you have to find it manually in thermo properties.

Hope this solves your problem.


ps: thanks for the previous link you mentioned, I'll have a look

Thank you! I already realized the problem. But during the process of establish the thermodata, there are still some species I cannot find, like H2NN,NCCN,OCHCHO, etc. Do you have good suggestion?