open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,
I post this message here because it might be interesting for some particular usages of Telemac3D with very small cells.

I am using Telemac3D with K-epsilon model to model a small free surface channel (1.4m broad with only 0.3m depth).
I am doing a grid convergence study, but for very small cells the results become wrong. The size limit is at about 5mm.

When the mesh becomes too small (5mm), the values for K and Epsilon sink to their minimal values imposed by the code, even if I had added inlet turbulence intensity of about 5% by a hand-coded function. The inlet profiles are respected but then the values sink in just a few cells. There seems to be a computation error for K and Epsilon for small cells, that is not easy to look at in the code equations. It also creates wrong velocity values. I am running an hydrostatic simulation.

The y+ size is correct, as K and Epsilon are correctly calculated at the boundary, but the terms are wrong in the free stream. I also checked different grid (regularly spaced with 5mm; or refined in the figure below) and the problem seems to come from the horizontal grid and not the vertical refinement.

Especially the simulation with very smooth mesh refinement shows that problem (images attached).


Has someone already experimented it and has some clue?


Thank you,

Vincent

Hello,

could you share you steering file?

Maybe this helps since we had also problems when using the k-e model in lab scale: since the cell size is related to the cell volume, you can try to lower the minimum values for the volume which are hard coded in the corresponding subroutines for the advection scheme. For example EPS in the subroutine murd3d.f. Another hint is to lower the ACCURACY FOR DIFFUSION OF K-EPSILON.

Once we did some tests - geometric dimensions were similar to your case - about the needed inflow length for k-e in order to get rid of the somewhat imposed empirical upper boundary conditions. It can be amazingly long as you can see in the picture which shows k at around mid water depth along the center axis of the flume. Interestingly the needed length could not be shortened that much by giving a more reasonable boundary condition for k and e compared to the minimum values (default option).


Best regards,
Clemens

Hello Clemens,
Thank you a lot for your answer. The default EPS=1e-6 is indeed reached during the iterations in murd3d.f, and I will investigate it.
Here are my simulation files. I hope the compilation will work for you.

Your tests are very interesting and I have one question. How did you deal with the turbulence decay due to the presence of imposed dissipation (epsilon) at the inlet? In my case I want to specify the decay in the channel by imposing epsilon, to simulate the flow behind a turbulence grid.
I checked the turbulence evolution at x=2meters and its profile has evolved in a good way, even if its profile is still not totally established (a discontinuity that existed near the bottom in my inlet-condition is still visible). I still have to ameliorate my interpolation at this point.

Have a nice day,
Vincent

Hi,

I tested the semi-empirical formulas for k and epsilon from the Nezu and Nakagawa book (1993). For both the quantities the formulas describe a exponential decay from the bottom to the free surface, as typically measured in river flows (no stress at the surface). In contrast, the OPTION FOR THE BOUNDARY CONDITIONS OF K-EPSILON = 2 (available in the newer version in Telemac-3D = "HANS AND BURCHARD FORMULA") simply assumes a linear decrease from the imposed bottom conditions for k and epsilon to the free surface. However, as the figure shows, both the approaches (TEL3D_TurbOn_Rodi and TEL3D_TurbOn_NezuandNakagawa) result in a very similar behaviour downstream of the inlet.

I didn't have time to have a closer look at your case but in the inletprofile.ivp you specify TKE=0 at the bottom where normally it should have the highest value. And are you sure that you have smooth hydraulic conditons?
Second, I think your time step is too big. For geometries in lab scale usually we had to use much smaller time steps (e.g. 0.01), but of course this depends also on the appearing flow velocities in your case.

Best regards,
Clemens

Hello,
Your work is indeed very interesting for river flows, especially to know which length is necessary to have a stabilized TKE value.

In my case the code reads the vertical profile for U, K and Epsilon except at the bottom. At the bottom, the value for Ubottom is imposed (hard-coded for the moment but I will change it). Then U*, K and Epsilon are deduced with the boundary law (I have to be very precise on the Ubottom value in order to have correct results, and I launched different simulations in order to set Ubottom).

For the time step, I just recently realized that the MURD scheme was explicit, and that I might have to lower it. But if I understood well, subiterations are done for the time step. I am currently playing on EPS and the time step but settings are delicate. Do you have clues on it?

Thank you a lot,
Vincent