Natural convection on a PCB's heat sink (with CFX)
 

Good morning colleagues,

I want to simulate the natural convection inside a PC case which is using an heat sink to dissipate the heat produced by the CPU. The Pc is fan-less (no air is forced inside the case).

In the picture u can see the model. The CPU is under the heat sink (350000 w/m^2 which is 35 watts for a CPU with an area of 1 cm^2) and the heat sink is inside the case with the bottom and the top opened. Experiments shown that the maximum temperature is about 80 degrees celsius and the air reach a pretty fast speed just because of the natural convection.

I've tried to model it like this. Two domains, one solid and one fluid. The CPU is a wall with heat flow, the heat sink is the interface between the solid and the fluid and the case is suppose to be adiabatic. The PCB, the bottom wall of the solid domain, is also supposed adiabatic because is attached to the board with not real possibility to dissipate.

There's an inlet and an opening. I have good mesh division but the problem give me a fatal error and I can't make it converge.

Can someone help me?
I'm making some mistakes in the interface modeling?
Have I to model the convection in another way?

If I would like to use fluent, what I should do about the interface conditions??

Thanks for your time.

Have you tried the natural convection tutorial that comes with CFX as base start for your own model? If you haven't, do that first, as it will help you with some specifics to modeling natural convection flow.

Anyway, first check if the fluid density will change significantly in your domain. If it doesn't (and it probably doesn't) you can use a fluid with constant properties (Boussinesq approximation). Choose a reference temperature based on the "free stream" temperature, sabe to the one you're using at the bottom inlet.

Set a physical timestep based on sqrt( dL / ( T g) ) (dL: lenght, : thermal expansivity, dT: delta T on dL, g: gravity - search the CFX documentation for "physical time scale", its the first hit), then use a physical timestep of 0.1 times that only for the energy equation.

Using a smaller timestep for the energy equation might be counter intuitive since that is the most stable equation being solved, but keep in mind that big variations in the temperature field strongly affect the velocity field, so by under-relaxating the energy equation you make the velocity field changes smaller (smoother?) and, therefore, the entire problem converges better.

Cheers.

Hi Bruno,

so, I had already used the Boussinesq approximation with a reference temperature the inlet temperature. I've solved the convergence problem, it was about the boundaries conditions, I've changed opening with outlet and inlet from pressure, to total pressure. I've also modified the CPU condition is not an "heat flux" but is a source term!

The fluid is air ideal gas with Boussinesq approximation, it make sense to you?

Now I have convergence but, as usual simulation data are way far from the reality of experiments. First, the temperature field is very very high, like 200 °C more then what we measure, may be I have to re-evaluate some hypothesis, like about the adiabatic walls. Tomorrow I will re-mesh the domains more carefully, I will redesign the heat-sink like the real one and I will use your, gold rule, for the time step. Then I will post again the solution I've found.

I want to start with this simple problem, then I will introduce an heat pipe (another solid in the solid dissipator which have a very high conductivity a sort of heat channel).

Thanks for your time, if you have other advices please tell me.

P.S. I've done the heating coil tutorial, is not that useful!

No, when you use 'Air Ideal Gas' as fluid you automatically activate the full buoyancy model (ie, not Boussinesq). There is no toggle for the Boussinesq approximation; it is activated when you select a constant property fluid (such as 'Air at 25 C') and also enable gravity.

About your results, the high temperature means the flow velocity is not big enough or the air temperature is too hot. Is the region left for fluid flow equivalent to what you have in the real model?

I'm assuming you've already check mesh and turbulence models (and if they're even needed).

Got it, so I can use Air at 25 °C and enable gravity and Boussinesq model.

My results give high temperature i guess because, air in not having a real convection movement. The model is almost what i have in reality, soon I will change boundary conditions, it would be better, then i have to analize also the case and not leave it adiabatic.

The problem is hard, I have to design an heat sink for a 35 watt cpu, with no fan and external temperature of at least 50°C. Is not simple.

Mesh have to be re-done. Sure, I've checked Y+ and turbolence, I have to refine that aspect. Tomorrow I will do it...

Thanks again

If you use 'Air at 25 C', make sure you change its properties (at least density and thermal expansivity) to reflect those from the average temperature you are expecting in your domain.

Can I use a formula for density?

I can easily find it for air right?

If your working fluid is air, just use a constant density.

I am presently modeling a 2D cavity problem in Fluent. I am confused about the boussinesq parameter. I first tried by selecting boussinesq under density of air under materials. I also specified the gravity. I put the density value as 1. It also asks for thermal expansion co-efficient which I put as 1e-5.

Secondly as mentioned by "brunoc" i selected air ideal gas and included gravity. However in the first case I get a convergence in 101st iteration and in the second I don't get convergence even after 500 iterations.

Should I assume that my first results are correct?

Is a density of 1 representative of the average density inside your domain? If it's not, change it to a value that is. As for the thermal expansibility, it will be 1/T_ref (in K).

Your results using an ideal gas model should match those using a Bossinesq approximation, but the simulation with ideal gas is not as stable, so it's expected that it takes more iterations to converge.

Have you refined your mesh around the fluid-solid interface? Because last time when I wasn't doing that I also got a 260 C PCB while in reality it was only 60 C. And maybe try the SST model instead of k-e model. Hope this will help.