open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone,

I am running a simulation of an experiment using a scale model. The model consists of a single cylindrical pile (D = 0.1m) in a flume (9.9m x 3.96m) with constant velocity of 1 m/s and a water depth of 0.4m. I am trying to recreate the experiment and its results but I am running into a few issues.

The main two things I am looking to recreate are:
- Vortex shedding behind the pile (Von Karman vortex street)
- Horseshoe vortices in front of the pile (This wil only be visible with Telemac-3D)

The Telemac-2D model:

I am using the Smagorinski turbulence model in combination with a very refined mesh around and behind the pile. The refined mesh is necessary to achieve the vortex shedding, with a less refined mesh the vortex shedding does not occur. Because of the small scale of the model, especially the mesh around the pile, I have to use a very small time step (<0.0015s) to keep the Courant number < 1. As the mesh is less refined away from pile, like at the entrance, the Courant number is very small ( down to 0.01 and even lower). This causes an instability starting at the entrance, this can be seen on the picture.

There are 2 parameters that fix this instability.
- OPTION FOR LIQUID BOUNDARIES =2 for the inlet (Thompson method)
- DISCRETIZATIONS IN SPACE = 12;11 (but a lot slower)

The best solution included using VARIABLE TIME STEP and DESIRED COURANT NUMBER but I don’t want to use these as they don’t exist in Telemac-3D.


The Telemac-3D model:

In Telemac-3D DISCRETIZATIONS IN SPACE does not exist and OPTION FOR LIQUID BOUNDARIES = 2 for the inlet results in there being no flow in or out of the model. This is what appears at every iterations:

This means the instability returns in Telemac-3D. The picture shows the moment before Telemac crashes/returns an error. The instability causes an intercrossing of 2 horizontal planes.

What can I do to fix this instability in Telemac-3D and why does OPTION FOR LIQUID BOUNDARIES result in there being no flow into the model?

Any other tips on creating the vortex shedding and horseshoe vortices are also welcome!

Best regards,

Jasper

Hello Jasper,

Which release of TELEMAC-3D are you using?

Your mesh seems very fine close to the cylinder pile (less than 1 cm?).

It should be noticed that there are some hard-coded values in TELEMAC-3D dealing with the mimum volume of prismatic elements, minimum distance between horizontal planes and free surface or bottom, as the main use of TELEMAC is for large areas (# km).
I would suggest you to change in a directory FORTRAN FILE:
- MESH_PROP subroutine: Change the hard-coded value of MINIMUM_VOLUME to 1.D-9 rather than the default one (1.D-6) or less if you have volumes less than that value,
- CALCOT subroutine: change
DISMIN_SUR = 0.2D0
DISMIN_BOT = 0.2D0
to
DISMIN_SUR = 0.001D0
DISMIN_BOT = 0.001D0 for example (maybe you will need another value).

Anyway, I have some comments about your mesh which may improve the results:
- every corner element is overconstrained (3 nodes of the same element on the boundaries, you should have at least one inside the domain), you should change them (e.g. add one or several additional nodes to have more elements or invert one edge),
- you should avoid elements with obtuse angles (angles > 90 degrees), or at least not too bigger than 90 degrees ;
- you should have the z-dimension of your 3D prism elements not bigger than the x and y dimensions. As your mesh is well refined (minimum size in x and y = 1 cm?), you will then have to increase the number of horizontal levels. I know that your CPU times will also increase.

You are right, there are no quasi-bubble elements or quadratic elements for TELEMAC-3D. You have to use linear prisms. If you have spurious oscillations or instabilities, you can try to decrease the keyword FREE SURFACE GRADIENT COMPATIBILITY from 0.9 to even 0. if it helps.


Anyway, have you tried with a coarser mesh?
If not, could you try all my suggestions (changed hard-coded values, increase of the number of planes...) on a coarser mesh and see if the problem with the Thompson conditions still occurs, please?

Hope this helps,

Chi-Tuan

Hi Chi-Tuan,

Are MINIMUM_VOLUME, DISMIN_SUR, and DISMIN_BOT still hard-coded values in v8p5r0? If so, what are these values?

Tracing MINIMUM_VOLUME leads me to lecdon_telemac3d.f, where it's defined as
And similarly, in the same file,
I wondered what MOTREA is...

Thank you!
Jason

Hi
MOTREA is an array for REAL KEYWORDS values
This also means theses values comes from the Telemac dictionary. There is a default value but you could change it in the steering file.

Regards