Hi all

I have to simulate a buoyancy driven flow inside spherical vessel. My task is to calculate heat transfer through walls of closed spherical vessel. The wall temperature are at 300 K and the fluid is filled at 310 K at operating pressure 5bar. There are no pressure, velocity boundary conditions.

Kindly let me know

1. Can I use Boussinesq approx to calculate heat transfer from wall in closed system? (We have neglected radiation and conduction. .

2. If unsteady state analysis of this problem is possible? I tried the unsteady analysis but its taking lot of time about 17 hrs and still could not reproduce the experimental results.

Thanks in advance

The accuracy of Boussinesq is a function of the material. Yes, it should work. From a numerical stability standpoint, convergence is often better using one of the ideal gas models for gases or an explicitly defined rho vs. T material property.

Sounds like an unsteady solution to me. Transient buoyance problems take a long time to run. Get more processors and run parallel, if you aren't already.

Thanks Evan

Yes you are right my analysis is transient one and its taking hell lot of time, specially at higher pressure like 10 bars or so, it took 16 hrs to simulate 1 sec of flow time even though I am running on 2 parallel processors.

But If I am not mistaken, somedays before in one of your reply to a previous post, you had advised not to use boussinesq approximation in closed one.

Kindly clarify me the reasoning behind this. Does it affects my simulation because my system is also a closed one.

Also please let me know if the computational time can be decreased by improving the smoothness or skewness of the grid or any other approach through which the computational time can be reduced for further simulations.

Thanks in advance

Regards Nitesh.

Nitesh,

Our observation has been that using Boussinesq makes the convergence more difficult, and that we get better solver performance using ideal gas or a defined rho vs temperature relationship. I don't know why this is, but we see it. Also, make sure to use PRESTO! for closed cavities, it does better in corners.

As for mesh, the key is to have a structured mesh. We have found that a structured mesh gives better performance in buoyancy-dominated problems if one mesh axis is aligned with the gravity vector.

Will any of this reduce a 16 hours simulation to 2 hours? No way. But every little bit helps.

Hi Evan

Thanks a lot for the information.

Please confirm me if I have adopted the right procedure for defining the operating density in case of "density as function of temperature".

1. First we will define density as function of temperature in material panel.

2. Specify operating pressure and operating temperature in operating panel.

3. Operating density in the operating panel needs to be specified on basis of density as function of temperature specified in the operating panel.

Thanks a lot about the information on the grid structure, I have modified it to make it more structured.

Nitesh.

Your procedure looks correct.

Thanks Evans

please specify me some estimation (example) of density temperature relation as an alternative for Boussinesq approximation

what should be the degree of polynomial that may help in easy convergence of convection problem.

Nitesh.

The order of the polynomial will depend on the fluid. Usually, we just use density versus temperature data points (piecewise linear).

Thanks again

In high pressure range 10-50 bars, I have observed more than one circulation center, which is clear reference of transition to turbulent flow.

At such high pressure, the rayleigh number becomes more than 10^9. so it may become important to include the turbulence model along with bouyancy driven flow and that may probably help in the convergence problem at high pressure or so....

Kindly correct me if there is any mistake in my observation and please let me know about the turbulence parameter specification or any special care to be taken while simulating this flow...

Thanks in advance

Nitesh.

Turbulence will complicate things a bit. We have observed that the different turbulence models can give significantly different results. Avoid using wall functions. The enhanced wall treatment works better. We like k-w.

[thermal energy]

hi friends,

ı simulate melting problem inside annulor geometry. ı use paraffin (melting range 56-58oC) as a phase change material. first, ı have boussinesq approximation. and also my material properties depends on temperature like Cp (spesific heat) and k (thermal conductivity). my problem here is that,

if ı use piecewisepolynomial for k and Cp (solid value and liquid value), ı have a convergence problem (figure attached). but if ı use constant value for Cp and k, ı have no problem and it is still converging (iteration going on)

what's the reason of this. what's wrong. thanks for help

[beer]

Your residuals are down to 1e-4, these are not really convergence problems I think. I can only assume what happens due to your picture. You have probably a convergence criteria of 1e-3 or 1e-4 for your transient simulation. Now when the transient simulation produces a solution with a residual of let's say approx. 5e-5 and than decides to go to the next time step it can sometimes happen that the solution does not "change enough" to bring up the residuals over your criteria. Than the solver stops the current time step and starts a new time step. It is some time ago that I used Fluent, but there should be something like a minimum of iterations each time step, give it a solid number (at least 2, but should be more)
Alternatively: smaller residual criteria.

That is like I said only a problem I saw sometime ago in one of my simulations but I could be also totally wrong in this case.

Cheers