# Natural Convection in Enclosures

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

March 28, 2015, 08:33
Natural Convection in Enclosures
#1
New Member

Charlie Howard
Join Date: Mar 2015
Posts: 6
Rep Power: 3
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
Attached Images
 Static Temperature Contours. Ra=6.19E7, laminar flow assumed.jpg (37.4 KB, 20 views) Velocity Contours. Ra=6.19E7, laminar flow assumed.jpg (38.1 KB, 16 views) Residuals. Ra=6.19E7, standard k-epsilon.jpg (39.6 KB, 24 views) Component Temperature Convergence. Ra=6.19E7, standard k-epsilon.jpg (36.0 KB, 18 views) Residuals. Ra=6.19E7, laminar flow assumed.jpg (34.4 KB, 16 views)

Last edited by Chuck7; April 7, 2015 at 06:16. Reason: Updated Problem

 March 30, 2015, 14:27 #2 Member     Ethan Doan Join Date: Oct 2012 Location: Canada Posts: 90 Rep Power: 6 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 nima_nz likes this.

 April 1, 2015, 05:57 #3 New Member   Charlie Howard Join Date: Mar 2015 Posts: 6 Rep Power: 3 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

 April 1, 2015, 11:09 #4 Member   nm Join Date: Mar 2013 Posts: 78 Rep Power: 5 Solution>Solution Controls>Equations

 April 2, 2015, 03:14 #5 New Member   Charlie Howard Join Date: Mar 2015 Posts: 6 Rep Power: 3 Thanks nvarma. Still cannot get it to converge :/ Looks like I might have to stick with a 2D laminar problem!

 April 2, 2015, 08:51 #6 Member   nm Join Date: Mar 2013 Posts: 78 Rep Power: 5 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.

 April 2, 2015, 10:10 #7 New Member   Charlie Howard Join Date: Mar 2015 Posts: 6 Rep Power: 3 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

April 2, 2015, 10:52
#8
Member

nm
Join Date: Mar 2013
Posts: 78
Rep Power: 5
Quote:
 Why can't I use Bousinesq? Is the temperature difference too large?
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.

Quote:
 I have just used a standard fine mesh. Is that not appropriate?
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.

 April 7, 2015, 06:08 #9 New Member   Charlie Howard Join Date: Mar 2015 Posts: 6 Rep Power: 3 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.

 April 7, 2015, 08:54 #10 New Member   Audrius Join Date: Apr 2015 Location: Kaunas Posts: 7 Rep Power: 3 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

 Tags electronic cooling, enclosure, natural convection, rayleigh number

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post salvo-K61IC OpenFOAM 4 January 16, 2015 14:27 Czarulla FLUENT 1 November 19, 2014 08:18 Ciefdi OpenFOAM Running, Solving & CFD 0 November 7, 2013 12:44 jorien CFX 0 October 14, 2011 09:26 Alex CD-adapco 5 December 12, 2007 05:58

All times are GMT -4. The time now is 23:25.