open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

Unfortunately I will not be able to answer again in the next two weeks, please state precisely the error and post your latest steering file and your boundary conditions file so that others can help you. Try to understand why you have depth = 0 at the entrance with a constant elevation at 1775.89, is the bottom elevation also at this value ? Look in the results file how is the bottom. You can also choose to initialise with a constant depth, to be sure that you have water everywhere.

With best regards,

Jean-Michel Hervouet

Hey Michel
That is not a good news.
I attached all the input files.
The bottom elevation at entrance is around 1567 m. I will start from the scratch and look for loopholes.
For now if
<i> Q(1) and SL(2), the simulation ends but there is no flow because of
GRACJG (BIEF) : SOLUTION X=0 BECAUSE L2-NORM OF B VERY SMALL: 0.000000
<ii> Q<2> and SL<1>, error appears problem on boundary number 2, give a velocity profile or check water depths.


Thanks

Regards..

T Q(2) SL(1)
s m3/s m
0 690 1578.34
5000 430 1575.67
10000 450 1576.4
15000 720 1579.23
20000 410 1575.899

Hello,

I looked a last time at your files and tried to run the case.

Minor details :

Remove from the steering file :

OPTION FOR LIQUID BOUNDARIES : 2 (this is Thompson conditions, we are not there yet...)
and also remove the name of the steering file (it is not useful and will drive you mad if you change the name).

Bigger detail :

Then I discovered that the problem at the boundary occurs only at iteration number 3 (put first the period for listing printout at 1).

Then I looked at the mesh and realised that it is about a square of side 28 cm !!! You want to enter in a very small area a discharge of 640 m3/s with a time step of 40 s, i.e. 25600 m3 in one time step !!!!!! No wonder that the computation is violently unstable. You probably have a problem of unit in your mesh...

With best regards,

JMH

Hello Aqleema

I think that your mesh is given in latitude-longitude coordinates. You need to tell that to Telemac (which expects , by default, cartesian coordinates).
Please add the following keyword
SPATIAL PROJECTION TYPE=3
You can also add the following keyword in order to take into accound for sphericity of the earth
SPHERICAL COORDINATES=YES
But it seems that your model is not that big.

Another point that could help, you are starting with a cold start (initial eleavation constant everywhere). In this case, if you use large time steps, this could lead to some troubles for the solver. It is recommanded to start with smaller time steps in order to generate physical initial state and then you can increase this latter according to the solver convergence capabilities.

I hope that this helps

with my best regards

Riadh ATA

Hey Riadh

I am using v6p2 version. Too old i guess.
Does the keyword work in this version. Because apparantly software is not recognizing the command.

Regards

Hey Riadh

Can you please tell me what changes should be made to mesh?

Thank you
Regards..

Hello Aqleema

The better is to use the last verison of Telemac, V6P2 is too old and there are a lot of improvements since this version.
Moreover, we can no more assist you if you go on with this old version, the Telemac team is committed to assiting only last release users.

If you do not change Telemac version, you can make the change by yourself in the mesh file. You need to convert latitude-longitude to cartesien x-y coodinates.
With my best regards

Riadh

Hey Riadh
Thank you for your suggestion.

I will upgrade to the latest version and post results.

Thank you
Regards..

Hey Riadh

Thank you for helping out. Seems the miscalculations were because of coordinates as lat long. On upgradation, model worked fine.

Thank You

Regards..