CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Bluff body stabilized flame - instability

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 28, 2015, 13:59
Post Bluff body stabilized flame - instability
  #1
New Member
 
Kristijan Krapic
Join Date: Apr 2012
Posts: 13
Rep Power: 10
krapic is on a distinguished road
Hi everyone,

I'm simulating a bluff body stabilized flame (test HM1E in Sydney) using the rhoFlameletFoam solver made by Hagen Mueller.

I initialize the simulation with the solution made with rhoSimplecFoam (just air), and I set a field (setField utility) of fuel (methane hydrogen mixture 1:1) in the fuel tube. As you can see from the velocity plot at 0.2s, the flame doesn't stabilize. There were some issues with pressure waves in the fuel tube so the inlet, outlet, coflow and side are set to a waveTransmissive boundary - that solved the pulsating flow at the inlet tube but didn't affect the flame near the coflow.



I experimented with a wide variety of configurations including various mesh densities and BC values but nothing seems to help. Here is the link to the case folder on google drive (due to the size limit on cfd-online). Note - the cantera tables aren't included there. I also included a few videos showing the progress of the simulation.

Does anyone have an idea of what might be causing the instability and have a possible solution to the problem?

Thank you in advanced,
Kristijan
krapic is offline   Reply With Quote

Old   January 28, 2015, 23:16
Default
  #2
New Member
 
Andrew Smith
Join Date: Jan 2015
Location: North Dakota
Posts: 24
Rep Power: 7
Andrew_Sm is on a distinguished road
Quote:
Originally Posted by krapic View Post
Hi everyone,

I'm simulating a bluff body stabilized flame (test HM1E in Sydney) using the rhoFlameletFoam solver made by Hagen Mueller.

I initialize the simulation with the solution made with rhoSimplecFoam (just air), and I set a field (setField utility) of fuel (methane hydrogen mixture 1:1) in the fuel tube. As you can see from the velocity plot at 0.2s, the flame doesn't stabilize. There were some issues with pressure waves in the fuel tube so the inlet, outlet, coflow and side are set to a waveTransmissive boundary - that solved the pulsating flow at the inlet tube but didn't affect the flame near the coflow.



I experimented with a wide variety of configurations including various mesh densities and BC values but nothing seems to help. Here is the link to the case folder on google drive (due to the size limit on cfd-online). Note - the cantera tables aren't included there. I also included a few videos showing the progress of the simulation.

Does anyone have an idea of what might be causing the instability and have a possible solution to the problem?

Thank you in advanced,
Kristijan
Lemme know when you resolve the issue
Thanx for sharing
Andrew_Sm is offline   Reply With Quote

Old   January 29, 2015, 05:17
Default
  #3
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

I downloaded your case and will take a look at it in a few days. I am busy at the moment. I hope to be capable of helping.

Best,
Bobi
babakflame is offline   Reply With Quote

Old   January 31, 2015, 11:50
Default
  #4
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

Normally, You should not experience this instability.

First of all, I think you should reconsider on your grid resolution (Just 13000 points )

In a 3 dimensional simulation with RAS, my recommendation is a grid with at least 1 million points.


Since you are using RAS, my recommendation is a wedge-typed grid with about 150,000 points.

I have done pretty much simulations with this solver, change your grid resolution and check the grid quality.
Afterwards, send me your email, I will send you my 0, constant and system folders (without polyMesh folder).

Your simulation must be stable. Don't worry my friend.

Best,
Bobi
babakflame is offline   Reply With Quote

Old   February 3, 2015, 12:44
Default
  #5
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

I will take a look at your grid tomorrow.

My recommendation is using RAS instead of URAS solvers for quick answers (without any noticeable difference in accuracy) refer to: http://www.cfd-online.com/Forums/ope...nsmoke-22.html

Yes, the proposed tuning for C1 is applicable in bluff-body stabilized flames.

I will email you the files tomorrow.

Best,
Bobi
babakflame is offline   Reply With Quote

Old   February 4, 2015, 07:35
Default
  #6
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

I took a look at your grid. Although I did not visualize it by paraview, the overall structure seems O.K.

I sent u the files via file2send. The files are for a LES simulation. Thereby, you need to change AlphaSgs to Alphat and muSgs to mut. The details of the files are similar. Take a look at what I have used for inlets, outlets and walls c.f. bluff-body.
However, for velocity inlet, use precursor simulation.
I think you have already done it by extending fuel injection to upstream so as to let the fuel stream become fully developed.

Let me know what happens this time

Best,
Bobi
babakflame is offline   Reply With Quote

Old   February 5, 2015, 03:47
Default State of the art
  #7
New Member
 
Kristijan Krapic
Join Date: Apr 2012
Posts: 13
Rep Power: 10
krapic is on a distinguished road
Quote:
Originally Posted by babakflame View Post
Greetings Kristijan

I took a look at your grid. Although I did not visualize it by paraview, the overall structure seems O.K.

I sent u the files via file2send. The files are for a LES simulation. Thereby, you need to change AlphaSgs to Alphat and muSgs to mut. The details of the files are similar. Take a look at what I have used for inlets, outlets and walls c.f. bluff-body.
However, for velocity inlet, use precursor simulation.
I think you have already done it by extending fuel injection to upstream so as to let the fuel stream become fully developed.

Let me know what happens this time

Best,
Bobi
Hi Bobi,

I am running your case right now but since I have access to a computer with only 16 cores, it's going to take a while - 3 days at least.

In the meantime, maybe you could write your thoughts on this kind of burner configuration for everyone in the future to see. These are the possibilities as far as I know as of now - Hagens solver is URAS so it's computationally really expensive, libOpenSmokes steady state solver is fast but cannot capture the highly transient behavior of this type of flow (at least I tried it and cannot achieve a stable solution). LibOpenSmoke's PISO solver is no longer available (at least on OF23x) because of stability issues. Finally, I assume LES is even more computationally demanding then URAS and thus not really appropriate.

So what would you advise people doing this kind of problem to do?

Best regards,
Kristijan
krapic is offline   Reply With Quote

Old   February 7, 2015, 02:49
Default
  #8
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

Providing hints for just a specific configuration is not a correct way of helping people unless the case be very special.
Instead, Tobi is writing a summary detailing solvers employing flamelet approaches based on OpenFOAM. I hope that in this way people would receive comprehensive helps instead of partial hints.

Best,
Bobi
babakflame is offline   Reply With Quote

Old   February 20, 2015, 14:32
Default
  #9
New Member
 
Dmitry
Join Date: Dec 2014
Posts: 8
Rep Power: 7
dimaCFD is on a distinguished road
Hi Kristijan,

You can try my solver: http://www.edcpisofoam.decgroup.org.
with some support from me =)

In general, this application is computationally expensive for the detailed chemistry (etc., the full GRI3.0 mech), however it works fine for one-, two- or three global reactions.

The most stable release is for OF-2.1.x, however if people will be very interested I can provide it for OF-2.3.1 (testing it now).

Thx, Dmitry
dimaCFD is offline   Reply With Quote

Old   February 20, 2015, 15:50
Default
  #10
New Member
 
Kristijan Krapic
Join Date: Apr 2012
Posts: 13
Rep Power: 10
krapic is on a distinguished road
Quote:
Originally Posted by dimaCFD View Post
Hi Kristijan,

You can try my solver: http://www.edcpisofoam.decgroup.org.
with some support from me =)

In general, this application is computationally expensive for the detailed chemistry (etc., the full GRI3.0 mech), however it works fine for one-, two- or three global reactions.

The most stable release is for OF-2.1.x, however if people will be very interested I can provide it for OF-2.3.1 (testing it now).

Thx, Dmitry

Hi Dmitry,

I am aware of your solver, I've read a few reports/papers from people successfully simulating this case with your solver.

Unfortunately, since this is a university project, my supervisor and I agreed to use Hagens solver. Maybe at some point in the future I'll check out yours.

Thanks for the tip though,
Kristijan
krapic is offline   Reply With Quote

Old   February 28, 2015, 04:12
Default Solved
  #11
New Member
 
Kristijan Krapic
Join Date: Apr 2012
Posts: 13
Rep Power: 10
krapic is on a distinguished road
OK guys,

Glad to say the problem is solved.



To my big surprise, the solution was reasonable even with 4.000 cells (image above - comparison between C_e1=1.44 and 1.60). I'm not saying that number of cells is optimal, but it's a good start since simulations run relatively fast on such a coarse mesh.

The key is to use a rather low maximum Courant number, in the range of 0.05 to 0.1 Co. Also, use low under-relaxation factors, even as low as 0.01. Then, as the simulation progresses, you can gradually increase both the maximum Courant number and the relaxation factors. My flame would stabilise around 0.5 seconds so every 0.05-0.1s I would increase those numbers.

Hope this helps,
Kristijan
krapic is offline   Reply With Quote

Old   February 28, 2015, 04:20
Default
  #12
Senior Member
 
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 452
Rep Power: 11
babakflame is on a distinguished road
Greetings Kristijan

Good to hear successful news from you.

I have simulated this flame with Smagorinsky and SpallartAlmaras Sgs models. At the moment, I am testing oneEqEddy on this flame.

Best
babakflame is offline   Reply With Quote

Reply

Tags
bluff body, cantera, flame, flamelet, open foam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ANSYS Meshing] Simple Symmetry Mesh Question - Flow around Bluff Body Matlab69 ANSYS Meshing & Geometry 20 April 23, 2012 09:55
Bluff body used for diffuser testing lemat1 Siemens 0 December 5, 2009 09:11
bluff-body stabilized flame Dmitry Main CFD Forum 0 June 21, 2007 07:30
UDF for lift force on a bluff body sawa FLUENT 2 April 11, 2005 03:06
Bluff Body flame solutions Seckin Gokaltun FLUENT 0 September 19, 2002 17:54


All times are GMT -4. The time now is 23:05.