open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I am currently trying to simulate flow downstream of a power plant and I am not able to find a mesh size for which the results (free surface elevation at the upstream boundary) are the same as with the next size up. (The water surface elevation keeps diminuishing when I simulate with a smaller edge lenght, althought it is very small (surface got lower by 4 cm by changing edge lenght from 5 to 3 meters over a model 1 kilometer long)) This worries me as with my previous simulation the free surface elevation didn't really change for a mesh size of 5 vs 10 meters.

My question is : Is this normal ? And what does this means regarding the validity of my simulations ?

Regards,

Martin

P.S. : I must add that I've tried running my case with an edge lenght of 2 meters and my desktop PC didn't manage to return results for some reason ...

Hello,

Usually, mesh convergence is carried out by keeping the Courant Number unchanged and ideally based on the largest time step you can get away with (close to CFL). So when you half your mesh size, you also need to half your time step. With that, convergence should be obtained.

Of course if you change your time step (or leave it big while the mesh size is decreased) the result would look different as larger time step may "smooth" your solution.

I hope this helps,
Sebastien.

Thank you for your answer,

I will try to give it a whirl over the next few days and let you know how it turns out.

Regards,

Martin

Hi, I've finally managed to find a mesh for which convergence is acheved. But, by going to smaller meshes than before, my model has developped instabilities towards the dowstream boundary of my river. I've tried lowering the "COMPATIBILITE DU GRADIENT DE SURFACE LIBRE" from 0.9 to 0.8 and even 0.5 to no apparent results. I've attached a copy of my steering file.

Could anyone provide pointers as to where should I look to reduce those and/or eliminate them.

I must add that I am only interested in steady state, and do not care for unsteady accuracy. Also, I am stuck using v6p0 in scalar mode.

Regards,

Martin

Hello,

You need to take care about the discretization of the bathymetry when splitting your initial mesh elements. The instability in the vicinity of the downstream boundary could be caused by a bad interpolation of the bathymetry which induces unphysical water depths (or at least hard to impose).
You need to keep in mind that, oscillations near a liquid boundary, are very often synonymous of hardness in the imposition of the desired condition (prescribed elevation in your case). The probable causes are the change of the hydraulic regime, a steap gradient of elevation or of bathymetry, partial or complete drying of the boundary etc.

There is solution to dump these oscillations, which I don't recommand, and which consist on increasing the velocity diffusivity (to 10-3 or even 10-2). It is a very efficient technique, but it could hide major problems in the model.

I hope that it was helpful.

Kind regards,

Riadh Ata

Thank you for your answer

But, I've tried running my case with a diffusity of 10-3 and 10-2 and the oscillations didn't really change. I think you are on the right path when you talk about the bathymetry because about 200 meters upstream of my downstream boundary I have an area which has some quite steep slopes with the finest mesh I use. This is where most of the oscillations seem to happen. But, I am quite confident in my bathymetry ...

Anyways, I've joined my files and perhaps it could help you to help me

regards,

Martin

Hello Martin

I tried to run your case as it was, and Telemac was shouting 'Help !!!'
So this are some suggestions:
1-your mesh is really bad with very sudden element size transitions. You need to smooth the mesh in order to get a growing of 1.2 at most.
2- You start with an initial elevation of 128 and you impose an elevation of 117m at the outlet and you want to reach steady state after two physical hours? This is too sudden, too steep and that's why your model makes Telemac suffering. I recommand the use of file for liquid boundary
T SL(1) Q(2) Q(3) Q(4)
s m m3/s m3/s m3/s
0.0 129 100 100 100
100.0 128 200 100 100
500.0 125 400 100 100
1000.0 122 600 100 100
1500.0 120 800 100 100
2000.0 118 800 100 100
2500.0 117 800 100 100
100000.0 117 800 100 100

3-make sure that your bathymetry is correct (1 inlet is at 108 and the two others are at 122 and 128), more over there are two big holes in the middle of the domain.

I run your case with this liquid boundary file for 10000s (4minCPU on 8 procs)and it runs well but steady state is not reached yet.

I hope that this was helpful

Riadh ATA

Hello Riadh,

1. My mesh was already with an edge growth ratio of 1.2. But, I've just created another one with 1.1 and I'll see if it makes any difference.

2. I've also incorporated your suggestion about the liquid boundaries.

3. I know that my bathymetry seems strange but is it some quite recent and precise data, therefore I tend to trust it. The difference between elevations in the inlets is due to the fact that the 2 north west ones are a spill way and it is setup this way in real life.

Lastly, I am considering selling a kidney ! (just kidding ...) so that I could simulate 10000s in 4 minutes. I recon it will take about 2 hours for 7200s... I have a dual core processor but can't install anything myself on this computer and the IT guys told me that there would be a delay of multiple montsh to to get install something so that I could use multiple processors ...

I will simulate my case with your suggestions and let you know how it turns out.

Thanks,

Martin

Hi Martin,

The source of your problem may be the very thin elements along all 3 northern outlets/inlets.

Did you include hard-lines or a series of hard-points just inside the outline when generating your mesh?

I suggest you apply some Laplacian smoothing.
"Edit->T3 Mesh->Auto-adjust Nodes"

Hope this helps... Martin

Hi,

I didn't use any hardlines or points, just density polygons. Is this the best way to proceed ?

Anyway, I will test your suggestion.

Regards,

Martin