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

Problems with temperature jump at the boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 24, 2005, 17:47
Default Hi. I am doing LES for a free,
  #1
New Member
 
Bei
Join Date: Mar 2009
Posts: 21
Rep Power: 8
tsjb00 is on a distinguished road
Hi. I am doing LES for a free, non-reactive jet, where cold fuel jet flows into quiescent hot air. hCombustionThermo is used for species mixing and compressible LES model is used for the flow. When the temperature difference between the jet and the surroundings is huge, the code collapses after a few time steps. The temperature in some cells goes wildly high and exceeds the temperature limits for janafThermo. I do turn off the chemical reaction and no chemical source term is included in h equation. I also try using TVD scheme for interpolation. However, it still doesn't work for big temperature difference. Please tell me how to solve this problem. Many thanks!

Bei
tsjb00 is offline   Reply With Quote

Old   August 24, 2005, 19:13
Default Sounds like a numerics problem
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Sounds like a numerics problem to me. What is your mesh like: orthogonality, skewness, near the boundaries? Do you get any useful info from checkMesh?

I would try switching the convection schemes to upwind and using limited laplacian schemes, e.g.

laplacian(muEff,U) Gauss linear limited 0.5;

(between 0.5 and 1, depending on how bad the mesh is).


If that does not help, have a careful look at your setup and boundary conditions - there must be something not quite right, e.g. inflow through pressure boundary or similar. Also, have a look at the solution to see where the problem appears - that may tell you a good deal. Of course, there's no point looking at it when it has blown up - dump the results often and try to find out what has gone wrong first.

Keep us posted :-)

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 25, 2005, 02:14
Default Hi, Are you using the multi
  #3
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
Hi,

Are you using the multivariate scheme?
If not there will be a numerical difference in how
enthalpy and species are transported which will result in an artificial change in temperature.

N
niklas is offline   Reply With Quote

Old   August 25, 2005, 12:26
Default Hi! I check the mesh and the s
  #4
New Member
 
Bei
Join Date: Mar 2009
Posts: 21
Rep Power: 8
tsjb00 is on a distinguished road
Hi! I check the mesh and the schemes. The mesh seems ok, but changing the convection schemes does work. I am still running the program to get the fully developed flow.Hope it will work well this time. Thank you all for your kindly help!

Best regards,

Bei
tsjb00 is offline   Reply With Quote

Old   August 25, 2005, 13:33
Default One more quick question. If I
  #5
New Member
 
Bei
Join Date: Mar 2009
Posts: 21
Rep Power: 8
tsjb00 is on a distinguished road
One more quick question. If I want to use the non-reactive solution as the initial condition for modeling reactive flow, should I just set the start time to the one corresponding to the directory of non-reactive solution? Or should I just use the directory of previous solution as 0? I assume the solver will load in the solution from the directory of start time and resume calculation, is that so? Thanks again!

Bei
tsjb00 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Cyclic jump boundary condition hjasak OpenFOAM Running, Solving & CFD 10 April 16, 2010 15:35
porous jump boundary jump thread not handled hari FLUENT 0 March 4, 2006 03:24
how to do a temperature jump for wall bc???? tieri FLUENT 0 January 13, 2006 13:42
porous-jump boundary condition in CFX? Ted CFX 0 April 24, 2005 01:30
porous jump boundary condition koh FLUENT 1 March 23, 2005 08:02


All times are GMT -4. The time now is 09:24.