open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi everyone,

I need some help here.

I'm trying to do simple simulation by reaching a steady state using Q-H boundary cond. However, I'm having the following problem :

1. Inflow at outlet location and/or strange recirculation (as shown on following pic)



2. I can't seem to have a constant flow throughout the reservoir and outlet boundary (and water level in power canal too) can't stop oscillating.

3. Negative water depths and velocity magnitude on land surface (see last jpeg).

From what I read in previous posts :

I tried lowering free surface comp. to 0.9 without success.

I played with Implicitation factors (i used 0.5, 0.55 and 1) but none of them seems to work.

I tried using mass lumping H and velocity profiles 5 too...

So right now i'm beginning to scratch my head and being confused...


I'm attaching cas file , geo and bound cond.

Any help, solutions or problem causes will be appreciated.

Thank you for your time

Mathieu

Hi

My first Idea will be to set an initial elevation equal to the boundary condition in elevation to avoid an initial shock...

The second one is to use a constant time step.

Hope this helps

Hi Cristophe,

Thanks for reply.

I'm currently testing your suggestions. I'll post back results soon.

Hi again,

I've ran a simulation of 15 days to try to reach steady state (INFLOW = OUTFLOW)

I've rearranged outlet boundary conditions as on the following


At the end of the simulation, level seems to stop varying at elevation 345.74m which is close to what I prescribed (345.73 m)



However, outflow never really stabilize. It never stop oscillating even if level is constant. see green curve below.




I don't think that if I go further it's gonna stabilize.

I simulating a relatively large domain of around 650 km² with about only 40 000 mesh nodes. Would it be possible that my mesh is too coarse and causing outflow oscillations ???

Any other suggestions to solve this ???

Mathieu

Hello,

It could be that the period of oscillations is related to the time it takes for a long wave to travel across the domain. Anyway the amplitude is small (7 mm). At the last Telemac User Club, a user reported such oscillations that were observed also in the physics (a case with several parallel channels), the domain behaves like a musical instrument and a resonance frequency is observed. Maybe increasing the diffusion coefficient, or choosing implicitation coefficients closer to 1 would help cancelling this.

The fact that we impose a constant discharge upstream is perhaps also a reason. When a wave goes upstream the domain and reaches the entrance, the discharge is certainly momentarily decreased, discarding this fact may trigger the phenomenon.

With best regards,

Jean-Michel Hervouet

Hello Mathieu

Hereafter some remarks and suggestions about your model.
In addition to the reasons cited in the previous posts, the outflow is oscilating probably also to the poor quality of your mesh. I've made a glance on the mesh and immediately I saw the huge gradients in the bathymetry and hence on the water depths. The code is suffering because in many locations in the model, the bathymetry is decreasing of 20 m in a SINGLE element of about 40 m length.
In many location also (and close to the outlet), there are many elements with one node having about 10m of water depth and the 2 remaining nodes which are completely dry !!
Your application, at these conditions, is in the limit of the Saint-Venant assumptions. Moreover, the severe wet/dry passages present in the model deteriorate more and more the quality of the solution and amplify, for sure, the instabilities.

I hope that this is helpful.
With my best regards

Riadh

Thanks to all for great suggestions and comments

I will try to increase overall mesh density and see what it looks like.



Mathieu

Hi

Before increasing mesh where i have strong bathymetric gradient, I tried what suggested Jean-Michel by increasing velocity diffusivity. Increasing mesh of a domain that size would give me too many nodes for my personal computer.

I found that the more I increase velocity diffusivity, the more stable the simulation. I finally reached a steady state where inflow = stable outflow by using 0.1 which is a lot over default value.

My question is :

Does using a much higher value than default for this parameter will affect the scaling of wind drag coefficient value???

My ultimate goal is to simulate unsteady winds over the reservoir.

Thanks again for precious help

Mathieu

Hello,

A diffusion of 0.1 m2/s is what I advise when you have no clue, it is a normal turbulent diffusion. The default value is 1.E-4 but this should even be changed into 1.E-6 because it should be the molecular diffusivity when the k-epsilon model is used. We'll probably do it for the next version.

Regards,

JMH