CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Wall heat flux drop (http://www.cfd-online.com/Forums/cfx/21218-wall-heat-flux-drop.html)

Rangarajan May 3, 2005 07:54

Wall heat flux drop
 
Hi all,

I am simulating a conjugate heat transfer problem along with radiation. A heater which is placed at a certain distance from the pipe heats it by radiation. The heat is conducted by solid pipe and water flowing through it carries away the heat. I am using CFX 5.7.1 for simulation. I find the heat flux on the solid pipe falling continuously with iteration (even after 1000 iterations) although the surface temperature is steady (not varying). I have tried with solid time scale factor for solid pipe and physical time scale for water.

Kindly suggest me some remidy.

Thanks Ranga

Glenn Horrocks May 3, 2005 18:33

Re: Wall heat flux drop
 
Hi,

Is it a steady state simulation? If so then I don't think your simulation is converged yet.

Regards, Glenn Horrocks

Rangarajan May 4, 2005 05:06

Re: Wall heat flux drop
 
Hi Horrocks

The solution doesnt seem to converge. the residuals fluctuate at 1 e -4 value continuously. This is a steady state simulation. How can i make it converge. Or atleast stop the heat flux dwindling.

Thanks in advance Ranga

Rangarajan May 4, 2005 05:07

Re: Wall heat flux drop
 
Hi Horrocks

The solution doesnt seem to converge. the residuals fluctuate at 1 e -4 value continuously. This is a steady state simulation. How can i make it converge. Or atleast stop the heat flux dwindling.

Thanks in advance Ranga

Glenn Horrocks May 4, 2005 19:21

Re: Wall heat flux drop
 
Hi,

It sounds like you are doing a CHT simulation and usually these require some acceleration in the solid domain by using a solid timescale factor. You can often use a very large acceleration factor in the solid domain of at least 10^1, sometimes up to 10^4 depending on the simulation. This is because the temperature equation in the solid region is a linear equation and so is much less sensitive to large timesteps, and because the fluid timescales are usually much faster than the solid timescales.

I find it useful to use "edit run in progress" with these sort of runs to tweak the parameters as the fly to get the best convergence.

Also, for CHT simulations I recommend using both residuals and imbalances for convergence. The imbalances show clearly when the bulk heat fluxes are approaching convergence. I think you will find the imbalances on your current run are nowhere near converged.

Glenn Horrocks

Rangarajan May 5, 2005 04:46

Re: Wall heat flux drop
 
hi Glenn Horrocks,

thanks for ur suggestions.It exactly CHT simulations.The main problem am facing is that as iteration goes on my temperature reaches steady state say 1000 itern but my heat fluxes goes on decreasing.Temeprature is in steady state even after 1500 itern but flux reduces.

In this Physical time scale factor and solid time scale factor as taken.As now i have given 0.40 sec for Physical time scale and 200 sec for solid time scale .

Water is flowing contionously at velocity 0.125m/sec inside the pipe.

calculation Physical time scale = Diameter/Velocity

=0.0493/0.125

= 0.394

Solid time scale = 500 * Physical time scale

= 200 sec.

Please guide me to set physical and solid time scale , so as to avoid drop in heatflux.

Thanks

Regards

Ranga

Glenn Horrocks May 5, 2005 19:02

Re: Wall heat flux drop
 
Hi,

As I said previously, I suspect your simulation is not converged yet and that is why the heat flux has not found equilibrium. Have a look at the imbalances to see if the heat equations are approaching convergence. Your parameters sound like good values to start with, but adjust it using "edit run in progress" while the run is proceeding to find the best value for your simulation.

CHT simulations are harder to get converged than single domain simulations.

Glenn Horrocks


All times are GMT -4. The time now is 22:25.