[gmingardo]

Hi all,
I am trying to simulate a water cooling system to assess how much heat I can get rid of. This cooling system is a rather tight and long channel, inside an aluminium support. So, given the heat entering the aluminium support from one of the wall, I need to calculate the conduction in the support first, and the convection with the fluid after. For this simulations I used the System coupling between Steady Thermal Model and CFX, 7 as max iteratons and 0.05 as a residual target.

I know that the low Reynolds (around 12000) number could have given problems with the turbulence model; I used the SST with no modifications, but I followed the suggestions on the boundary layer meshing given in: http://www.computationalfluiddynamic...oundary-layer/

My boundary conditions are:
CFX: mass flow at inlet and outlet, temperature at the inlet
Thermal: 1kW entering heat, 373 K of temperature at the support boundary

The simulations keep giving unreasonable results, with extracted heat around 7 kW (despite the incoming heat is 1kW) and wall heat transfer coefficients of 125000 W/(m^2K)

Do you have any idea? Let me know if you need any further information.
Thank you in advance for your help

[bparrelli]

3 questions:

1. can you show me a plot of the convergence behavior? (Residuals and imbalance)
2. Is it possible for you specify total pressure at the inlet, and mass flow at the outlet.
3. What fluid properties and EOS are you using? (density, specific heat, viscosity, and thermal conductivity) I have found in the past that not carefully checking these values are in agreement with your thermal BCs can lead to unrealistic heat transfer coefficients.

[gmingardo]

Thank you for answering. So:
1)The residual plot is the one of CFX and the imbalance comes form the system coupling I suppose, right?


in the residual one, there are a lot of other previous simulations before in which I was trying different turbulence approaches, but the simulation with the coupling is just the last part (I didn't know how to cut off the others)

2)I can try this, yes, how would it make it a difference?
3) Since it's water, I didn't even look at them and I relied on the Ansys material library. should I take a look?

[bparrelli]

My answers in red below.

Originally Posted by gmingardo

Thank you for answering. So:
1)The residual plot is the one of CFX and the imbalance comes form the system coupling I suppose, right?


in the residual one, there are a lot of other previous simulations before in which I was trying different turbulence approaches, but the simulation with the coupling is just the last part (I didn't know how to cut off the others) This is fine. No apparent issues here.

2)I can try this, yes, how would it make it a difference? It might not, but having a system pressure is important to establish the density and pressure gradients correctly.

3) Since it's water, I didn't even look at them and I relied on the Ansys material library. should I take a look? I would check. The transport properties are very dependent on temperature. For CHT problems, I always recommend using your own custom materials.

[bparrelli]

Can you send a picture of the model so I can see how you are applying the thermal BCs? If the items from the previous post are not the issue, then the thermal BCs could be.

[gmingardo]

Hi, sorry but it took time to me to try your suggestions as I have not much computational power
I changed the flow constants on the material part of CFX. I took some values from the web, sites like http://www.engineeringtoolbox.com/.
The simulation gives now a much better result: indeed the heat extracted is in the range that I expected. However, the wall heat transfer coefficient is still of an insane order of magnitude, like 10^5. Could I say that the simulation is reliable but that the coefficient has not been calculated correctly? So, can I trust this result, despite the value of the coefficient?

BTW, pictures of the model are here below. The project overview shows lighting bolts with red crosses because my computer had a problem during the calculation and has been interrupted badly, but no problem with the model itself.




The flow enters at 52 C and exits at 55 C.
Other problem: the Heat Flux and the Wall Heat Flux integrals at the surface are not the same value. What is the difference? Is it normal?
Thank you a lot, you have already been very kind and useful!

[bparrelli]

How are you calculating the heat transfer coefficient? CFX estimates it by using a localized bulk temperature which can vary by a lot across the domain. There is an expert parameter that you can activate in CFX-Pre where you can specify a constant bulk temperature. This should fix the problem. Based on the picture of the model you provided, the heat transfer coefficient should be in the ballpark of a 1D calculation using the Dittus-Boelter relationship, or something similar.

[bparrelli]

To activate this expert parameter, in your CFX-Pre model, select Insert>Solver>Expert Parameter. Next, select the "Physical Models" tab and under "Miscellaneous", activate the "tbulk for htc" parameter, and specify the bulk temperature for the heat transfer coefficient. This should resolve your issue.

[evcelica]

Why are you using system coupling for thermal only model? You can solve all of this directly in CFX.

[gmingardo]

because I want to take into account the non uniformity of temperature and heat flux distribution on the wall. I think it makes the difference in the thin walls separing the channels

[evcelica]

Right, but you can do the solid heat transfer in CFX as well. It can do more than just fluids.

[gmingardo]

oh, this I didn't know. So I should input another body, set it as solid and mesh it? and there I could do the analysis?

[evcelica]

Correct. Set interfaces between the domains as well.