CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   [Combustion] Two plane turbulent jets (http://www.cfd-online.com/Forums/fluent/129804-combustion-two-plane-turbulent-jets.html)

 miragef1 February 13, 2014 07:51

[Combustion] Two plane turbulent jets

Hi guys,

I'm working on a project with Fluent on non-premixed combustion in a very simple burner.

We have two turbulent jets (diameter d0 = 6.35 mm) with a spacing of 50 mm between these two. They are flowing either oxygen or methane. The inlet velocities are betwwen [50:100] m.s-1.

FYI, we usually use hybrid initialisation.

We first studied the non-reactive case (flowing only air with both nozzles), so we have a symmetry line between the two nozzles. We used it and the results are pretty neat.

We're now studying the reactive case (air and methane). We do not have the symmetry line any more so we have to model the entire geometry. We first try to have neat results with only air flowing but with the entire geometry. We're having many problems with this because the calculation is not converging well.

Here's a figure of a result :

You can see that the flow is not propagating only in the x direction but also tilting to the left or right. Which should be the case because the inlet velocity is the same for both nozzles.

1) What kind of boundary conditions would pick for the lines (1, 2, 3, 4) ?
FYI we put 1 : pressure-outlet, 2 : pressure-outlet, 3 : pressure-outlet, 4 : wall. We also tried symmetry for 1 and 2 (in the industrial case we have multiple burners) and also wall (but we do not have a confined burner).
2) What solution method would you pick ? The SIMPLE and SIMPLEC are working but the COUPLED is not working at all. What parameter would you tweak to try to stabilise the flow ?
3) Would you try the FMG initialisation ? It doesn't seem to work well in the case we're studying.

The next step is to study the combustion in this geometry. We could use both the species transport model (eddy dissipation) or the non-premixed model I think. What do you think ?

Thanks a lot for your help and please ask any question if anything is not clear !

 macfly February 13, 2014 10:38

Hi,

Here's what works well for my cases of Eddy-dissipation or non-premixed mixture fraction/pdf:

Steady cold flow simulations
- Coupled
- Pressure => PRESTO!
- Pseudo Transient
- URFs: Gradually decrease pressure and momentum URFs if continuity is not converging. Decrease any other URF whose residual is oscillating or not converging.

Transient
- PISO
- PRESTO!
- URFs: same as above

- I always start my combustion simulations from cold flow results, that's the key for convergence for my cases.

- Mesh: did you try with a finer mesh? Is it symmetric about the center plane?

- Discretization: what spatial discretization order are you using? In the end its recommended to use 2nd order.

- I'm not familiar with your type of geometry, can't recommend on boundaries 1 and 2, but pressure-outlet is what I would try first.

- After a quick look at the user guide, I don't think fmg initialization is for your case.

 miragef1 February 13, 2014 18:03

Thanks a lot for your answer this helped a lot !

I worked on this this afternoon and the result is neat.

http://reho.st/preview/self/62ed9e42...20f0881131.png

I still have some problem with the convergence (oscillations) but I'm working on the UFRs.

1) Now that my cold simulation is almost ok, I'll have a look at the non-premixed module.

2) For the mesh, I use some edge sizing modules to stretch the mesh where I'm not interested by the information (aside the flow). The mesh is perfectly symmetric.

3) I'm using 2nd order discretization (I first tried 1st order but 2nd seems better)

4) Pressure outlet is definitely the best, I'm not having problems anymore with it so I'm keeping this boundary condition

5) FMG initilization might converge faster but I'm not sure it's a good idea to go with it as everyone is using the hybrid one.

Thanks again !

 macfly February 13, 2014 18:48

Glad if I helped

Can you pinpoint which modification made the flow symmetric instead of tilting?

 miragef1 February 14, 2014 04:38

Of course.

The residuals are not very stable yet but I'll try to tweak the UFR's a little bit.

So I basically only changed the method :
- Simple to Coupled
- Pressure Standart to PRESTO!
- And I put the pseudo transient on

For the UFRs :
- Pressure : 0.3
- Moment : 0.3
- Density : 0.8
- Body Force : 0.8
- Turbulent kinetic energy : 0.7
- Turbulent dissipation rate : 0.7
- Turbulent viscosity : 0.8

I also tried to use the non-premixed module but I'm not really converging. The flame is way too "long". My cavity is 1.5m long, I'm flowing O2 at 10m.s-1 and methane at 10m.s-1, this should be good but I think the problem is the convergence.

The static temperature is as follows :

http://reho.st/preview/self/1cb32537...60cf5d0646.png

The X-velocity :

http://reho.st/preview/self/9cf6d508...c4f817e6b6.png

We see that it's not symmetric. The upper nozzle is flowing methane the inlet velocities are the same but it's methane and air so I guess that's why it's not symmetric as they are not the same molar mass.

And here are the residuals :

http://reho.st/preview/self/c78dfdbe...d99149e331.png

I definitelly have a problem with the residuals, I'll try to tweak the UFRs a little bit or if you have any ideas ...

Thanks for your help !

 j.eduardo April 12, 2014 12:14

Hey,

Im modeling nom premixed combustion too, but in a slot burner with air/methane mixture with EDC but my combustion blow off.. i dont know what to to. Im using EDC and k-e realizeble and DRM19.

 miragef1 April 13, 2014 05:51

Hi,

Why are you using EDC instead of non-premixed model ? This one worked pretty well for me. You have to use PRESTO! or Second Order pressure discretization with the coupled scheme. And the pseudo transcient option should be used too. Try to lower the relaxation factors A LOT to make your calculation converge (it does take a long time tough).

 j.eduardo April 13, 2014 07:00

I have to use EDC it is the objective, but i have solve the problem for now. Thank you very much for reply

 WJXu April 13, 2014 17:16

Hi, I am simulating a high pressure burner combustion. What kind of solver, pressure-based/density-based are you using? Did you check the mass flow rate balance yet? Thank you.

 All times are GMT -4. The time now is 13:31.