Natural Convection in Enclosures
 

Dear all,

I'm trying to model a fully immersed electronic cooling module in steady state. I have tried 3D but have reverted back to 2D due to difficulties. However I am still struggling to get a solution that converges. The left hand wall of the 'electronic component' has been given constant heat flux of 2000 W/m^2 (equating to a TDP of 100W) and the cold plate (right wall) has a constant temperature of 298 K. The top and bottom walls are adiabatic. The fluid being considered is a dieletric with the following properties (at 298 K):

Density - 1660 kg/m^3
Specific heat capacity - 1140 J/kg.K
Thermal expansion - 1.15E-3 K^-1
Dynamic viscosity - 1.12E-3 Pa.s
Thermal conductivity - 6.9E-2 W/m.K

The Rayleigh number of the flow is calculated to be 6.91E7 therefore the flow is turbulent (ANSYS suggests flow is laminar below E8 but I have come across papers saying the transition to turbulence occurs at E7). I have tried numerous variations of the turbulent models k-epsilon and k-omega and both pressure and density solvers but I am unable to get a converged result. I am using the Boussinesq approximation for the fluid density. I have specified the fluids operating temperature as 298 K. The operating temperature T0 is used as the reference temperature for the Bousinesq approximation.

Solution Method:
I am using the SIMPLE scheme with PRESTO! for the pressure based solver as this has been recommended before.

Solution Controls (laminar):
Pressure:1
Density:1
Body Forces:1
Momentum:0.1
Energy:1

Solution Controls (k-epsilon):
Density:1
Body Forces:1
Momentum:0.1
Turbulent kinetic energy:0.8
Turbulent dissipation rate:0.8
Turbulent viscosity:0.8
Energy:1

If I solve the problem with Laminar flow my solution converges nicely, see figures. However with a Rayleigh number of 6.91E7 and assuming a turbulent flow the the continuity residual settles at 1E4 although the component temperature does converge (to the same temperature as with laminar flow). Can anyone recommend how I could reduce the continuity residual?



Regards,

Chuck7

I believe its recommended to set the operating temperature = the max temp in the domain. And you actually shouldn't specify any operating density when using the boussinesq. in your case since you have heat flux boundary at the hot wall its not so clear what the max temp will be but i think higher then 298 K since the lowest temp is 303 K. when you adjust the temp you would also need to adjust the other properties for the new reference temp. You could also to try to solve just the energy equation first then turn on the flow equations once he temperature based on conduction only through the fluid is solved

Hi edoan,

You're right about no needing to set an operating density however an initial density is needed for the Bousinesq approximation. I guess I could find the operating temperature by running an initial simulation and then use the final average fluid temperature in a subsequent simulation.

Okay. How would I got about solving the energy and flow equations separately?

Thanks

Solution>Solution Controls>Equations

Thanks nvarma. Still cannot get it to converge :/ Looks like I might have to stick with a 2D laminar problem!

at an Ra of 1.65E9 , your solution would be significantly different(wrong?) without a turbulence model.

Just to make sure, are you running a steady or transient case?

If you so badly want a steady state solution, try running an implicit transient scheme with high time-steps and once you reach a near-steady state reduce the time step and obtain an accurate result.

Alternatively, try coupled scheme with pseudo transient.



Also,

1. I wouldn't use a Bousinesq for that Delta T.
2. Did you use a k-w sst model? You'd need that to predict transition.
3. Mesh. Make sure you used the right mesh for k-e with wall function and k-w with no wall function.

Good luck.

I've edited my case such that my Rayleigh number is now much lower. Okay I could try that. The reason I want a steady case is purely to reduce computational time.

Why can't I use Bousinesq? Is the temperature difference too large?
I have just used a standard fine mesh. Is that not appropriate?
I will try what you suggested.

Thanks

the Boussinesq approximation is valid when B(T-T0)<<1
From your contour plot, Delta T~10^2, B=10^-3.
B(T-T0) is in the order of 0.1.

However full compressible solution can be time consuming and evern harder to converge, so I would suggest you get a converged solution with boussinesq approx. first and see if the temp gradients are that high.



Make sure you resolve the boundary layers. For example look at the images here http://www.computationalfluiddynamic...oundary-layer/

You just have to be fine enough to resolve those scales.

Hi nvarma,

Thanks for your help. I have now made some progress and updated my problem. My temperature difference is 15K so I think the Boussinesq approximation is now acceptable.

Hi Chuck7,

I using Fluent 14.0, and I modelling natural convection in the nuclear spent fuel pool, my suggestion is: opent fluent -> help -> Tutorial Guide and find topic "Modelling radiation and natural convection" (in fluent 14.0v 307 page, in the 15.0 version could be another page number). So, try this model without radiation model (for me it works very well).

Regards,
Audrius