open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,
I just computed my study area the first time. I choosed the constant viscosity as turbulence model and a Velocity Diffusivity of 1.0.
When I now look at my results there are no eddies at all which is not realistic. So I guess I have to change this parameter.

But what is the right value for my mesh?
There are different edge sizes (from 0.1 m to 45 m) in the study area. But the mesh size in that areas where eddies are expected is between 3 m and 15 m.

Or are there other parameters I have to change?

I attached my geometry file and my cas-file and hope anybody can help me.

Cheers

Sarah

Hello,

You can try 0.0001 to see if it is the problem, but I see many other things :

ADVECTION : .false.

You should remove this, you will have no eddies if you remove advection...

You should remove all keywords removing physical terms :

ADVECTION OF TRACERS : .false.
DIFFUSION OF TRACERS : .false.

Remove also STEERING FILE= ... (it is useless and can only drive you mad if you change the name and forget changing it inside...).

With you option it is also better to have :

SOLVER = 1 / this is conjugate gradient, OK if the TREATMENT OF THE LINEAR SYSTEM is 2 (wave equation) because the linear system is thus symmetric.

Ask for the information on solver, and look how many iterations it does, up to 20-30 iterations or even more you can try to have a larger time step than 0.1 s. Then you can also look at the advection scheme for velocities (first number of keyword TYPE OF ADVECTION), try characteristics to start with (1).

Regards,

Jean-Michel Hervouet

Hi Jean-Michel.
first I want to thank you again. After changing the parameters as you adviced results came up as expected.
Now I have some questions to better understand in which way the parameters affect the results.

1. I thought the Advection is a parameter which only has to be activated if the distribution of a tracer or sediment transport shall be simulated. What is the impact of this parameter to the turbulence?

2. You recommended to use Solver number 1. In the manual I didn't found a definition what's the difference between the solvers provided and in what kind of solver is useful in which situation?

3. How many iterations are acceptable to get satisfying results or is it justa question of CPU-time?

4. When I want to simulate the same study area with the k-Epsilon turbulence model to compare the influence of those models and their results. Can I just change the TURBULENCE MODEL to 3 and VELOCITY DIFFUSIVITY to 1E-06. Or are there other parameters depending on the k-Epsilon model I have to change?

Cheers
Sarah

Hello,

Here are the answers :

1 : removing advection is very artificial, even without tracer you have also the advection of velocities.

2 : there is a course on iterative solvers on this website. 1 is conjugate gradient, for symmetric systems. 7 is GMRES, rather for difficult and non symmetric systems, now in Telemac mainly for pressure equation and SUPG.

3 : number of iterations acceptable : very difficult to answer. One option consists of looking at the time step that gives the minimum of computer time, but it may lead to very large CFL numbers. Let's say between 1 and 60 iterations is OK.

4 : it will work like this, unless you want to add a given turbulence on open boundaries, in which case you would have to look at routines like kepscl.f

With best regards,

Jean-Michel Hervouet

Thank you for the quick answers!
Unfortunately I can't find the course on iterative solver. Could you give me a hint where I can find it or a link.

You said Solver 1 (conjugate gradient) is for symmetric systems. What is meant with systems? The geometry or a numerical system?

Hello,

bottom of home page --> manuals

or the link : www.opentelemac.org/index.php/component/...ar-systems?Itemid=56

by system I mean a linear system.

Regards,

Jean-Michel Hervouet

Thank you Jean-Michel,
that's very kind of you!!!

Cheers
Sarah