Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Counter flow diffusion flame simulation using Fluent

  1. Jul 10, 2016 #1
    Hi,
    I am trying to model a counter flow diffusion flame using ansys fluent with fuel/oxidiser as methane/air.
    The problem is that the flame temperature(800 K) is much lower than what it should be(>1600 K).
    I am using Non premixed combustion module with steady diffusion flamelet and adiabatic energy treatment since combustion is instantaneous process. I am using a standard 30 species chemkin reaction mechanism from standard mechanisms library.
    My PDF table seems OK as The plots show a max temperature of 1800 K at a mean mixture fraction value of 0.1. The geometry is a simple cylinder with two inlets in the axial direction and outlet in radial direction(image).
    The Dia of two inlets is 60mm and the gap=10mm.
    Can any body explain why am I not getting the desired temperature? I would be happy to provide any further information if required. 2.png
     
  2. jcsd
  3. Jul 11, 2016 #2

    Nidum

    User Avatar
    Science Advisor
    Gold Member

    You need to think about the validity of those assumptions .
     
    Last edited: Jul 11, 2016
  4. Jul 11, 2016 #3
    If the lookup table is OK, can you check what the values of the mixture fraction are in your domain? Can you show a contour plot of Z at the symmetry plane? Can you also visualize the mesh in that same plane? Can you show a picture of the lookup table?
    Is it a laminar diffusion flame, or do you have a turbulence model activated?

    My combustion simulations are almost always non-adiabatic. Do you know when a flame is non-adiabatic?
     
  5. Jul 14, 2016 #4
    Hi Bigfooted,
    Thanks for the reply. By look up tables, if you mean the thermodynamic table, I am using the one from the standard fluent database. My Chemkin mechanism is a 30 species one with CH4 and O2 as the boundary species. After generating the flamelets, I plot the PDF tables and I get the temperature maxima at a mean mixture fraction of around 0.1(the temperature being around 1800).
    Then I go for the boundary conditions. I give a inlet flow velocity of 0.1m/s at both the inlets. I set a MMF of 1 for fuel and 0 for oxidizer.
    It is a standard counterflow diffusion flame for non premixed condition. But fluent suggests that we cannot use the non premixed combustion module without keeping turbulence on. So it makes the setup turbulent. But fluent also suggests that a turbulent flame is solved as a composition of luminary local flamelets. The geometry I have shown above is just to make the problem more clear. Actually I am using an axis-symmetric equivalent of the same. I do not sure if I'm right but I am considering it adiabatic because combustion is a spontaneous process. I would have loved to share some pictures of the results but I am not sure which ones you asked for above.

    Thank you
     
  6. Jul 14, 2016 #5
    OK, if you simulate a 2D axially symmetric case, can you show your mesh and a contour plot of the mixture fraction?

    Can you explain to me what adiabatic means? It is very important to know and I think you do not fully understand it.
     
  7. Jul 15, 2016 #6
    These are the images you asked for.
    I suppose adiabatic is a condition where we do not have heat exchange between system and surroundings.The mesh has two inlets on left and right, an outlet at the top and axis a the bottom. There are no walls which eventually means I have no place to define heat transfer coefficients.
    8.jpg 9.jpg
     
  8. Jul 15, 2016 #7
    OK, that is clear. Let's go to the next step in the analysis. Let's compare the values from the lookup table with the values from the simulation.
    Can you make a graph of the temperature as a function of the mixture fraction from your pdf lookup table (for mixture fraction variance 0)?
    Can you also make a graph of the temperature and the mixture fraction as a function of x from your simulation results (for y=0)? Can you make another graph with 2 lines: mixture fraction as function of temperature from the pdf table and mixture fraction as function of temperature from the simulation data on the x-axis?

    I hope this comparison will show you what is wrong with your simulation.

    Indeed, in an adiabatic system there is no change in heat, do you see that adiabatic has nothing to do with if the process is instantaneous or not? An adiabatic flame is simply a flame where the total enthalpy of the gas is not changing. If there is radiation, or if there is a solid (a wall) that takes heat away from the flame, then the combustion is not adiabatic.
     
  9. Jul 15, 2016 #8
    The PDF plot is a 2D plot (with constant Variance=0) on a 3D surface(with constant scalar dissipation=0).Maximum of Mean Temperature(K) is 2.240994e+03 and occurs at Mean Mixture Fraction = 5.683755e-02.
    10.jpg


    Below are the images from simulation results as functions of x.
    11.jpg
    12.jpg


    Should I activate the energy equation and the radiation models? Also I could not plot the last Image with two curves as I don't know how to.
     
  10. Jul 16, 2016 #9
    Well, it is clear that this lookup table is not the one that is being accessed to obtain the temperature. Does your pdf table contain laminar flamelets for different mixture fraction variances? Can you visualize the mixture fraction variance in your domain?
     
  11. Jul 17, 2016 #10
    Hi Bigfooted,
    Thank you for your continuous help.
    Yes, my pdf table contains flamelets for different mixture fraction variances. Below is an image of the PDF table. I hope it would help.


    pdf table.png

    Scalar dissipation varies from 0-26 and the scaled variance varies from 0-0.25 .


    Following is a curve for the mixture fraction variance in the domain.


    mixture fraction variance.jpg
    Following is an image of scalar dissipation in the domain.
    scalar dissipation.jpg

    From the above data, I conclude that my domain has a max deviation of 0.15 and a max scalar dissipation of 4 and both of them peak near the zone where I am getting max temperature(850K). So I decided to make another temperature plot from PDF table keeping the value of dissipation=4 and variance =0.15.
    Following is what I get.

    pdf temperature.jpg
    The above graph peaks around 850K(approximately around my flame temperature).
    I hope this information is useful. I am certainly doing something wrong. I just cannot realize to where the problem exists.
     
    Last edited: Jul 17, 2016
  12. Jul 17, 2016 #11
    Your variance and scalar dissipation rate in your simulation are very high and this causes the temperature to drop. fluctuations increase due to turbulence, so you should try to lower the turbulence levels in your simulation. You could do the following:
    - Lower the velocity of the streams to reduce the Reynolds number of your setup.
    - Check what turbulence boundary conditions you are using. you could set them at constant k and epsilon and give a very low value for k (k=0.001) and a value for epsilon e=1. From your plots I gather that your mixture fraction variance is already set to zero at the boundaries?
     
  13. Jul 17, 2016 #12
    Hi,
    Thank you very much. That exactly was the problem. I used the values suggested by you.
    K=0.0001, e=1, T(flame)=1450 K
    K=0.0001,e=2, T(flame)=1650 K
    K=0.0001, e=5, T(flame)=1780 K
    K=0.0001, e=10, T(flame)=1847 K
    K=0.0001, e=15, T(flame)=1893. K
    There were no significant changes further increasing e or decreasing K.
    Is the approach OK?
     
  14. Jul 17, 2016 #13
    Very good! The higher values for turbulence dissipation keep the turbulent kinetic energy from growing again. You can also refine your mesh to see if the solution is truly mesh independent (your mesh is quite coarse, but for this diffusion dominated flame it is probably sufficient). If you can find detailed measurements of a counterflow diffusion flame, you could use them to really fine-tune your simulation.
     
  15. Jul 18, 2016 #14
    Hi,
    Thank you once again. I will test my case with different mesh refinements and post it in the thread if I find something fruitful.
    It would be very kind of you if you could suggest with any such appropriate text which would contain the detailed measurements for my case.

    Regards
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook

Have something to add?
Draft saved Draft deleted



Similar Discussions: Counter flow diffusion flame simulation using Fluent
  1. Help in fluent (Replies: 1)

Loading...