open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

a colleague did a tutorial of another cfd solver in which he produced very nice Karman vortex streets downstream of a pier. (On Youtube one can find a lot of such vortex street simulations).

It aroused our interest to compare the solvers and so I simulated the case with Telemac-2D based on the mesh from my colleague and almost the same hydraulic boundary conditions. Enclosed the mesh file if someone is interested. Please change the extension *.geo to *.slf. Hydraulic boundary condition is 0.1 m/s inlet velocity.
I did some parameter tests: viscosity, type of advection, treatment of the linear system, FE and FV, and I never got the Karman vortex street but steady flow fields.

Why no eddies in Telemac-2D? Does the numerical diffusion dampen out the eddies?

I would be glad for an answer and hints!

Best regards,
Clemens

Dear Clemens,

Unfortunately we are not able to simulate this problem, at least, until tuesday, we are moving to new offices and our computers are not working for a while.
Actually, the case of a flow around bridge piers is one of the validation cases of Telemac2d. We are able to observe nice vortices behind the pier. I invite you to look at this case and compare it with your model. You can for example use the same numerical parameters and the same boundary conditions and identify the minimum Reynolds number that generates the Karman instabilities. This way permits you to quantify the numerical diffusivity and dispersion of each code and compare fairly their effeciency.

Finally, can you send us all necessary files (not only the geometry) in order to simulate your case and assess the obtained results.

With my best regards

Riadh

Hello,

To give a complement to what said Riadh, we have also here a student that is currently cheking Telemac-2D against experimental results and it is OK. You must have a Reynolds number large enough, and then you find the correct period of oscillations, linked to the Strouhal number. One thing is that the k-epsilon model is not convenient for that, because it is a RANS model that may find a turbulent viscosity that puts the Reynolds number under the threshold value, so the k-epsilon model, in some sense, gives you the averaged result.

You must also be cautious that you are not plagued by numerical diffusion of advection, depending on the scheme it is around U*DX/2, and depending on your mesh size, it could induce a low Reynolds number.

Well these are some hints...

JMH

Hello,

thank you both for your valuable hints!

For those who are interested, Enclosed there is a working steering file and the boundary condition files.
In my previous simulations I used a too low time step. By doubling the time step the vortex streets appear. However the max Courant number with the lower time steps were around 1.4 and the lowest values around 0.2.
As in the validation case now I used a liquid boundary file with an inflow hydrograph to steady state boundary conditions, otherwise I get a steady flow field. Interesting and strange? Using the k-e model gives a steady flow field as Jean-Michel Hervouet said in the previous post. In FE the type of advection plays a role. With Finite volume schemes I have also steady flow fields.
So I think it is quite hard to find good settings for such cases beginning with the choice of time step, type of advection to other key words as in the validation case example.

Best regards,
Clemens

Hello again,

Yes, very small time steps will introduce too much numerical diffusion, and it is so for finite volumes. Actually the validation case has a symmetric mesh and symmetric data, so the oscillations can only appear if symmetry is broken somewhere, and it happens in truncation errors. Then the first eddy will go to the right or to the left, at random, and it results that this case is very sensitive, and you will find enormous differences only by changing the compiler. The liquid boundary file starts with no discharge, so it gives a different behaviour. I think the best results are obtained with the method of characteristics for the advection of velocities (so TYPE OF ADVECTION : 1;5). In version 6.2 it will be very spectacular with quasi-bubble element or even quadratic element (the method of characteristics has been improved in this case and we get very nice von Karman eddies).

With best regards,

Jean-Michel Hervouet

Hello,

thank you for the explanations, very interesting topic.
So if I understand you correctly, for example by using higher order schemes in space and time, truncation errors should decrease and the oscillations possibly vanish?
In this context I think on symmetric expansion flow for which a numerical model gives also an asymmetric flow field but not due to small external imperfections which occur naturally in a physical model or in nature (but due to truncation errors?) And so it is very difficult, to compare for such cases a numerical model with a physical model.

Nice article in Hydrolink!
Best regards,
Clemens

Hello,

We had also a student working on sudden expansions, for sediment settling basins, and we do find the assymmetry.

JMH

Dear Konsonaut,
recently we wrote a short communication for SimHydro conference in which we compared numerical simulations versus experimental results (by Kantoush et al.) for a number of configurations. In some cases, the influence of the Coanda effect, resulting from a perturbation of the flow field
that pushes the main flow towards one side of the channel while increasing the velocity magnitude near the
wall, can be important.
Please find attached the article.

All the best,
Pablo