open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone, I'm running a simulation on Telemac-3d for a tidal model for my graduating project. when I run the model I can see that it's not moving it's stuck at iteration 3 (I had to decrease the listing to 1 to see why the model is not moving). I'm a beginner to Telemac and I've been trying many solutions but nothing works. i tried to run a different model from my Dr and it works fine but I'm not sure why mine does not work. I hope you guys can help me run this for my graduating project

Hi
More than 8000 iterations at the first steps means probably a problem somewhere.
Huge velocity somewhere, of a shock at boundaries...
Look the result at the first time steps to identify the problem

Regards

i changed from K eps model to Mixing length model and I get iteration lower than 8000 however, the problem is the same I'm not sure why the simulation does not move from this step + I'm unable to identify the problem

You should have very few iterations at the beginning (lower than 100) except if you initial condition is really wrong.
Save all the time step and look carefully to the result at time 1, 2 and 3
Free surface / velocity should show exotic values...

PS: think to update your profile!

I tried to reduce the number of iteration by doing the following:
1- reducing the accuracy of the solvers.
2- changing the solvers and pre-conditioners values to the default values.
3- reducing the maximum number of iteration.
However, the simulation is still stuck and not working.
I also tried to use a boundary conditions of 5.6.6 instead of 5.4.4 which helped also in reducing the iteration but still the simulation is stuck.

Hi,

You seems to be 'stuck' on the 2nd timestep, with an mass error 3x your inflow. Volume increases form 72 to 2753! Seems like you need to look at the initial condition.

Hope that helps,

Patrick

Hello,

Looking at your geometry file, there are several issues to solve before running a computation:
- the extent of the domain is understood to be 2 m times 2 m. If you want to use longitude/latitude, you have to use SPHERICAL COORDINATES = YES + SPATIAL PROJECTION TYPE = 3. But you also have to fill in LONGITUDE OF ORIGIN POINT and LATITUDE OF ORIGIN POINT, but...
- with TELEMAC, it is recommended to use coordinates of plane projection, e.g. UTM, Mercator, Lambert. You should rather convert your geometry file in UMT North e.g. with the relevant number of zone,
- you have many overconstrainted elements, in particular in the river. You should add at least one node of the boundary triangles in the water domain. Using CHECKING THE MESH = YES for 1 time step is enough to have a list of potential errors of your geometry file.

Hope this helps,

Chi-Tuan

Hello again,

Quick additional advice:
- try to use a ratio of size between two elements not too big (a few percent) for numerical reasons,
- try to avoid triangles with obtuse angles,
- upgrade to the latest release v8p3r1 as there have been many fixes solved for the last years, in particular for TELEMAC-3D. Moreover, we cannot assist users with older releases...

Hope this helps,

Chi-Tuan

Hi,
I've noticed that you have chosen TPXO as tidal input. Here are some suggestions that may help you, as I'm also using TPXO and I've met some problems before.
You can try 5 6 6 ... 5 as boundary conditions because the field of velocity is contained in the TPXO binary file.
In many cases, if only the hydrodynamic（T2D/T3D）is considered but there are still many iterations, it may be caused by the divergence of the flow field. Because you're using TPXO, i guess it's the WATER DEPTH in shallow water who causes this divergence, as you've turned off the TIDAL FLATS.
You can try also MINIMUM DEPTH TO COMPUTE TIDAL VELOCITIES INITIAL CONDITIONS & MINIMUM DEPTH TO COMPUTE TIDAL VELOCITIES BOUNDARY CONDITIONS
Hope this helps.
Sorrymaker

Thank you so much everyone. my model works fine :)