[yousefaz]

Hello,

I am trying to simulate a homogeneous atmospheric boundary layer in FLUENT using steady state RANS. I am using a Standard k-e model with inlet UDF functions for velocity, k, and epsilon as specified by Richards and Hoxey (1993).

For the most part, I seem to have set up the model correctly. Here is a comparison of the inlet and outlet profiles (which would collapse for a perfectly homogeneous ABL):



However, there seems to be a divergence issue at the bottom corner of the domain near the outlet (right hand side), which particularly affects the kinetic energy throughout the entire domain. It seems to occur in the boundary layer. The solution is fully converged with residual values dropping to 10E-7.

Here is the velocity contour (note the blue (=0 velocity) on the bottom right):



There is a concentration of negative pressure at that corner. Interestingly, no warnings of reverse flow appeared:



The turbulent kinetic energy contour shows values blowing up near that corner:




Zoomed pics with mesh shown:

Pressure:



TKE:



Epsilon:




Any ideas on how to resolve this issue would be greatly appreciated.
Thanks in advance.

[sariug]

hey man.

I have the same problem.

Have you figured it out ?

[yousefaz]

Hi Sariug,

It turns out the problem is due to the standard wall function (SWF) in ANSYS Fluent, which is ideal for mechanical applications, not so much for atmospheric boundary flow.

The roughness value specified for the SWF in ANSYS Fluent is based on the equivalent sand grain roughness (Ks), whereas the log-law ABL equation is based on the aerodynamic roughness height (y0). The relationship between the two has been derived in the literature for the ANSYS Fluent code as follows:

Ks = 9.793*y0/Cs (default value of roughness constant: Cs = 0.5).

The problem here is that in urban flows (y0 = 0.5 - 2m) the resulting Ks value is very large (9.8 - 39.2 m). Fluent requires the centroid height of the near-ground cell (yp) to be at least equal to the equivalent sand grain roughness (yp>Ks). This means that your total first cell height would be unreasonably large (20-80m) and would not allow you to achieve high mesh refinement near the ground surface.

Ignoring the condition (yp>Ks) results in the problem described in this post, where there is an imbalance between the equations for the inlet profile, the turbulence model, and the SWF. This manifests as an initial acceleration of the flow near the ground surface, and a spike in the turbulent kinetic energy. However, as the flow travels across the domain, it adapts to the SWF, and the spike in TKE disappears. But you end up with a different Vel, tke, and epsilon profiles than what you specified at the inlet (i.e. an inhomogenous ABL).

PS: I noticed that in the posted images, the inlet is at the right hand side (flow is in the +ve x direction). So the issues described occur at the inlet, not the outlet.

This 2007 paper by Bert Blocken: (http://dx.doi.org/10.1016/j.atmosenv.2006.08.019) discusses the problem in more detail and suggests remedial measures to reduce this error.
There is no easy fix to this problem, but a few thing you can try:

1. Select ABL profiles with smaller roughness values (y0)
2. The inflation layer near the ground needs to transition smoothly to the far field (unlike the images attached in this post). This often requires increasing the number of inflation cells.
3. In FLUENT, you can maximize the value of Cs (and hence minimize Ks). The maximum value allowed in the input window is 1, however, you can specify a larger value using this UDF:
   
   //Define roughness constant Cs
   DEFINE_PROFILE(roughness_constant_Cs,t,i)
   {
   real x[ND_ND];
   real z;
   face_t f;
   
   begin_f_loop(f,t)
   {
   F_CENTROID(x,f,t);
   z = x[2];
   F_PROFILE(f,t,i) = **; //replace ** with Cs value
   }
   end_f_loop(f,t)
   }
   

Note that these measures will not fully resolve the problem. The only way to do that is to develop a new wall function based on y0 instead of Ks.

Good luck
Y.A.Z