I am trying to simulate a single close enclosure with hot wall and cold wall filled with fluid, to simulate natural convection, my Ra is 10^10, I have been trying to simulate it for a while now, and it is not converging. could you please give me some detailed guidlines to help me finish this simulation, and could you please suggest which turbulence model to use. Thanks, Elyyan

please refer guidelines for solving natural convection in fluent 6.0 or 6.1 documentation.. it aint difficult for ur problem, choose proper time step size, if u select boussinesq approx. for density in materials list..u will get an option for bouyancy effects in turbulence models..u select it....ask me for more al the best prasanth

recently some papers has been published regrading the natural convection in poorus media by Dr Tan Ka Kheng. He is using FLUENT for the simulation, may be u can refer to. can search in sciencedirect.

Hi, In an open medium, natural conv. problem is very easy to converge. For the enclosures, it is not. there is an example about natural conv. in an enclosure in the fluent tutorials. However the gravity vector is taken so small that the problem is laminar. if you increase the gravity vector you will see it is not converging, as in your case. The answer i got when i asked this situation to Fluent support people was that, start with very small gravity vector and increase it gradually. let me know if it works. Regards emre

We do a lot of natural convection in closed cavities where I work. Try the following, which have usually been a good starting point for us.

1. Don't use Boussinesq. Define a temperature varying fluid density or, for gases, use ideal gas.

2. Use PRESTO!

3. Start with the following underrelaxations:

a. Pressure = 0.3 b. Density = 0.7 c. Body Force = 0.7 d. Momentum = 0.3 e. Turbulence (all params) = 0.8 f. Energy = 0.95 (increase to near end)

If your mesh isn't the greatest you'll need to modify the multigrid parameters, so make sure you have a good mesh quality.

dear evan, 1. without using boussinesq (which is valid for only certain range of variation in temperature) how can a temperature dependant density can be specified with no prior idea. 2. for multiphase problems with natural convection, is it right to take boussinesq approx. for both fluids. also buoyancy inclusion wont appear in turbulence model panel as appears for single fluid, then what to do? 3. what is significant difference b/n PRESTO! and BODY force weighted schemes as both are recommended for buoyant flows?

thanks and regards prasanth

1) Every material has some known relationship of density versus temperature at a constant pressure. Buoyancy driven problems typically don't have large pressure gradients, so you can generally neglect pressure effects.

2) I'm pretty sure you will never get a bouyancy driven multiphase problem to converge.

3) I reconnend PRESTO! because you have a closed cavity, not because of the buoyancy. It works better than the BODY FORCE scemes in domains with corners.

Thanks Evan, 3. Presto! worked for some time..after that some errors are coming..body force weighted scheme is working well now.

I think that is related to the skewness correction option in PISO (pressure-velocity coupling), as i have deselect it for my problem, because mine is perfect structured mesh. previously i didn't deselected.

If you dont mind can you give your mail ID. i want to discuss with you.

my e-mail id is samala_prasanth@yahoo.com

regards prasanth

Dear Evan, I have used the steps you have provided, I started with Ra 10^7 then tried to increse it to 10^8 (which is the transition to turbulent flow) unfortunately it did not converge, even after 10000 iterations, if you have any suggestions please provide me with some. Appreciate it Elyyan

unfortunately,it did not work, I started with Ra 10^7 and then increased it to 10^8, and it did not converge, I wonder if they have something else. Thanks, Elyyan