open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello and happy new year!
I am new here and I started to work with the k-e turbulence model on telemac3D, to modelize an experimental open channel.
I have some difficulties with convergence, and maybe someone can help me, because I haven't found test cases using k-e model on Telemac3D on both horizontal and vertical directions.
The computation crashes at approximately 24s in my case.

The open channel modeled is in a lab and has very small dimensions, that might be a source of the problem? (5meters by 0.8meter with 0.12m depth).

This modelization is part of my PHD project wich aims to modelize a tidal turbine with source terms in Telemac3D. Our first objective is to get a correct boundary layer for the bottom of a rough channel, using k-e model of turbulence in all directions (to compare with literature results).


Here are details of the simulation:

• I used different cell sizes to take into account the boundary layer: Here I used a cell size of 8mm at the bottom, corresponding approximately to y+=20 at 1/tenth of the cell, where the velocity is calculated with the logarithmic law (as told in the manual if I am correct). Then the cell size slightly increases until the free surface (the plane heights are coded on condim.f source file).
  I first saw that the planes are not modelled properly, and there seems to be a minimum vertical cell size required. Where could I find this limit in the code?
• I also used a Nikuradse roughness of 1.21mm on the bottom and the walls, corresponding to the experiment. I use negative altitude: free surface is at z=0 and bottom at z= -0.12meters.
• The flow is progressively establishing in the channel, thanks to a temporal boundary condition function (canal-temporal-BC.qsl).
• I used Telemac3d v7.1.0 ; parallel computation

My interrogations are especially by choosing the correct simulation parameters in the canal.cas file: which schemes for diffusion and advection? implicitation for velocities?...


I would really thank you if you have other k-e cases to share with me or tips.

Vincent

Hello Vincent,

If you have just started with TELEMAC, you can swith to the new version of the TELEMAC-MASCARET system 7.2 available since a few days.

In the subroutine CALCOT, you have two hard coded values DISMIN_BOT and DISMIN_SUR that may be changed, in particular if you have small water depths.

You have several test cases of TELEMAC-3D using the k-epsilon model in the subdirectory examples/telemac3d and which can help you to choose good parameters for your steering file.

Hope this helps,

Chi-Tuan

Hello,
Indeed it helps a lot, thank you.
I checked in details the files on the SVN repository and I finally found 3 tests cases with k-e model:erosion_flume ; tetra ; and Viollet (I had missed them the first time).

For the new Telemac version, we have the v7p1 installed on our cluster so I think I will keep using this version, but it is nice to know that.

And I will change the values of DISMIN_BOT and DISMIN_SUR, and do computations step by step (no roughness first, then roughness,...) in order to see when the problem appears.

I let you know when I'll have more results.

Vincent

Hello,
I managed to run my simulations after viewing that similar case:
Convergence problems with v7p1r1

The main point to achieve convergence was to use the MURD SCHEME ( Explicit N):
I didn't try the different schemes but I know that the characteristics scheme couldnt converge for my simulation.
I also had to modify DISMIN_BOT and DISMIN_SUR in CALCOT.F, ACCURACY FOR DIFFUSION OF K-EPSILON and MAXIMUM NUMBER OF ITERATIONS FOR DIFFUSION OF K-EPSILON (dico variables); and THRESHOLD DEPTH FOR WIND =0.001 (dico variable because I imposed wind on the free surface).


Doing my simulations I realized that the bottom boundary conditions for K
and Epsilon are calculated with variables for U* at the altitude of the top of the first cell and not at 1/10th. But a parameter FICT (delta in the reference book) is used to compute Epsilon only, and its default value is 2 (without any explanation). Was this arbitrary chosen to achieve better results with K-epsilon scheme?
Otherwise results seem to be in good agreements but I realized that the reference I chose is finally not detailed enough to have reliable quantified results.

Best regards,
Vincent

Hello,
I advanced a bit and could get results in agreement with experiments.
But my next step is to model a tidal turbine in the channel which needs really small cells.

I get a problem then, which is specific for small cells. I know that Telemac is an oceanic code and is not designed for those sizes, but I'm really interested in knowing more about that.
I still have no turbine in my simulation.

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.

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


Has someone any idea of what to look for in my case?
If not I think i will respect similitude laws to do run another simulation.

Thank you,

Vincent

I also attach my simulation files. I hope the compilation will succeed because I created new subroutines and added a lot of files to the fortran file (addprofile.f).