
[Sponsors] 
February 13, 2014, 07:51 
[Combustion] Two plane turbulent jets

#1 
New Member
Kevin Preur
Join Date: Feb 2014
Posts: 4
Rep Power: 3 
Hi guys,
I'm working on a project with Fluent on nonpremixed 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.s1. FYI, we usually use hybrid initialisation. We first studied the nonreactive 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 : pressureoutlet, 2 : pressureoutlet, 3 : pressureoutlet, 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 nonpremixed model I think. What do you think ? Thanks a lot for your help and please ask any question if anything is not clear ! 

February 13, 2014, 10:38 

#2 
Senior Member
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8 
Hi,
Here's what works well for my cases of Eddydissipation or nonpremixed 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!  start with small time step and increase gradually  URFs: same as above Other comments:  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 pressureoutlet is what I would try first.  After a quick look at the user guide, I don't think fmg initialization is for your case. 

February 13, 2014, 18:03 

#3 
New Member
Kevin Preur
Join Date: Feb 2014
Posts: 4
Rep Power: 3 
Thanks a lot for your answer this helped a lot !
I worked on this this afternoon and the result is neat. 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 nonpremixed 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 ! 

February 13, 2014, 18:48 

#4 
Senior Member
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 366
Rep Power: 8 
Glad if I helped
Can you pinpoint which modification made the flow symmetric instead of tilting? 

February 14, 2014, 04:38 

#5 
New Member
Kevin Preur
Join Date: Feb 2014
Posts: 4
Rep Power: 3 
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 nonpremixed 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.s1 and methane at 10m.s1, this should be good but I think the problem is the convergence. The static temperature is as follows : The Xvelocity : 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 : 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 ! Last edited by miragef1; February 14, 2014 at 13:03. 

April 12, 2014, 12:14 

#6 
New Member
José Branco
Join Date: Mar 2014
Posts: 4
Rep Power: 3 
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 ke realizeble and DRM19. Some advice? 

April 13, 2014, 05:51 

#7 
New Member
Kevin Preur
Join Date: Feb 2014
Posts: 4
Rep Power: 3 
Hi,
Why are you using EDC instead of nonpremixed 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). 

April 13, 2014, 07:00 

#8 
New Member
José Branco
Join Date: Mar 2014
Posts: 4
Rep Power: 3 
I have to use EDC it is the objective, but i have solve the problem for now. Thank you very much for reply


April 13, 2014, 17:16 

#9 
New Member
Join Date: Apr 2014
Posts: 18
Rep Power: 3 
Hi, I am simulating a high pressure burner combustion. What kind of solver, pressurebased/densitybased are you using? Did you check the mass flow rate balance yet? Thank you.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Problem with Gmsh  nishant_hull  Open Source Meshers: Gmsh, Netgen, CGNS, ...  18  April 22, 2015 08:43 
Problem with divergence  TDK  FLUENT  10  September 8, 2012 01:11 
Turbulent Jets in Water and Air  haze_1986  FLUENT  2  October 3, 2011 21:08 
boundaries with gmshToFoam  ouafa  Open Source Meshers: Gmsh, Netgen, CGNS, ...  7  May 21, 2010 12:43 
Modeling Turbulent Horizontal Buoyant Jets  Jack Travis  Main CFD Forum  2  September 11, 2006 06:36 