[Pavolo]

Hello all,

I'm completely new to CFD analysis, so I need some help with the following natural convection problem (due to symmetry, only one half is depicted):



So basically, I have a closed air domain with cylindrical shape (radius 2.5 m and height 18 m). Within the cylinder, a heat source (the parallelepiped) generates 25 kW (which means 625 W/m^2 in the four vertical faces of the parallelepiped). The cylinder is surrounded by water (22ºC). I need to predict the temperature distribution in the whole domain. Rayleigh number >> 1e10.

1) My first question is about the mesh. I have read in Fluent Help about “y+ shouldn’t be greater than 1” and things like that. I guess that is a way of defining the inflation of the layers close to the walls, right? Is that a normalized value?

Regarding the model/solver, I have tried many alternatives so far:

a) Incomp. ideal gas (without specifying reference density) vs Boussinesq (ref. temperature 35ºC): I chose the second one, since it is a closed domain. However, temperature differences are not small (around 25 degrees). Convergence is better with Boussinesq.

b) Realizable k-epsilon with EWT. Options "Thermal Effects" and "Full Buoyancy Effects" activated. I have seen in other posts that, according to some people, this viscous model could be inappropriate for my problem. Any suggestions?

c) Radiation OFF (so far). I have tried using S2S model with low emissivity and I got "unconverged radiosity". But this is another issue...

d) BCs are pretty simple (constant heat flux for the source, steel walls (0.2 m) with convection to 22ºC for the domain limits) and I don't think they are the source of my issues.

e) Coupled pressure-velocity scheme: The only reason is that "simple" didn't converge.

f) Pressure discretization: Body Force Weighted.

g) "Pseudo transient" activated: Again, without this the problem didn't converge. Pseudo time step = 1 s.

Second question would be: 2) Any suggestions about a) – g) ?

With that, I need 1600 iterations to reach convergence (Figure 2). I have read things about performing a transient simulation (decreasing the time step), using relaxation factors, and starting with lower values of g, all to improve convergence. But given that I reach a solution, I didn’t try any of them. 3) Again, any suggestions?



The thing is that I don’t trust my solution. Since I am an electrical engineer, my CFD background is very limited. I am particularly worried about the speed plot (Figure 3):



4) Maximum speed around 1.6 m/s. Isn’t that way too high?

5) Regarding the velocity profile at the walls, I don’t see a typical laminar boundary layer close to the walls (zero velocity that increases, reaches a maximum, and then decreases). Does that mean that my problem is wrong? Is that a meshing issue (the aforementioned y+) or is it a model issue (viscous model)?

Thank you in advance for your time.

PD.: Congratulations to CFD online forums, they are extremely helpful.

[sicfred]

1-You should use one quarter of the geometry (double symmetry).
2-Your geometry is quite simmple, so try to use hexaedral mesh.
3-you should use a thinner inflation layer and check the contours of y+ in the walls. You can estimate the tickness of y+ with the tool of cfd-online
4- I think Boussinesq is a good option.
5-It is true that sometimes could be inappropiate, in my experience this one gave me the best results compare with experimental data, but who knows in other problems. The standard for turbulent models is the SST k-W, and for transition to turbulent boundary layer the "transitional SST" (4 equation).
6-The value of y+ depends of the mesh (inflation layer) and the velocity of the fluid close to the wall. In problems of heat transfer and more in free convection the value of y+ should be less than 1.
7- Try the DO model for radiation.
8- Natural convection problems take a lot of iterations to converge (in my experience more than 3000)

[Pavolo]

Thank you for your answer.

So far, I have improved the mesh (shapes, sizes and especially the inflation layer), and results look more realistic now. However, I still get velocity values over 1.6 m/s at some points, which seems a lot to me. Is this because I am using Boussinesq with large temperature differences?

I am also making attempts regarding radiation, but no luck so far.

Finally, I have taken the next step and included in the model the solid which generates the heat (the parallelepiped). The problem is the same, since now I have a steel solid with a heat generation (W/m3) instead of 5 surfaces with a specified heat flux (W/m2). However, I keep getting "Divergence detected in AMG Solver:TEMPERATURE" no matter what (SIMPLE vs COUPLED, steady vs pseudo transient vs transient, initial small gravity, and so on). Should I change the default relaxation factors, which are the only thing I haven't tried? Any tips regarding this?

[ghost82]

Also, I don't think your solution is converged (continuity residual is quite high); try to monitor some other key values in your domain and see if they remain constant.