open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear Friends,

I tried to simulate a simple open channel flow case with constant discharge. But the result is very unreasonable. The error message says, ill-posed problem entering free velocity. I tried to modify different parameters but didn't work.

How can this be corrected?

Thank you.

This is related to your boundary setup. Here are a couple things to check:
- do you start your simulation with depth zero everywhere? You need to have at least some water at the inflow boundary.
- do you have large slope at the inflow boundary potentially causing supercritical flow? You may need to move the boundary to somewhere flatter so the inflow is not supercritical.
Otherwise you may want to post your model for us to check.
Hailiang

I tired with different initial boundary conditions but it didn't work.

Please check the attached files. If you can find what is the problem.

Thank you.

Regards

Karki, it may be a better way to start with an example model distributed with the program and see how the case file was setup, including the keywords and values.

Here are a few issues:
- the mesh geometry is a major issue. At the river left boundary, there are a few very thin cells. Thin cells are often killer of model stability and should be deleted. After the deletion, you also need to update the corresponding boundary condition file.

- your geometry file (.slf) already includes the elevation of every mesh node, there is no need to provide BOTTOM TOPOGRAPHY FILE anymore. So you can comment the line with /

- are you trying to model wind impact on hydrodynamic? If not, you can comment line AIR PRESSURE = true. If yes, you can consult telemac2d manual for details how to include the wind effect.

- you do not have to include ADVECTION OF TRACERS = false. By default it is false. Without specifying a keyword the program will automatically use the default value.
- try VELOCITY PROFILES = 4;1.

- comment line STEERING FILE. It is not wrong to specify that but it is not needed by the program anymore.

- specify keywords LISTING PRINTOUT PERIOD, GRAPHIC PRINTOUT PERIOD and VARIABLES FOR GRAPHIC PRINTOUTS

- your time step 10 seconds is too large comparing with your cell size. Try to reduce it to 0.1 seconds. After editing your time step, your GRAPHIC PRINTOUT PERIOD should also be adjusted according to your desired output frequency. eg if you want to output results every 1 second, you need GRAPHIC PRINTOUT PERIOD = 10.

After these edits please report back whether the ill posed problem persists.

Hope this helps,

Hailiang

Also the order of the two boundaries do not match between the boundary conditions file and the case file. To match your boundary conditions file, you need to update your case file

PRESCRIBED FLOWRATES =0;0.001
PRESCRIBED ELEVATIONS =0.17;0
VELOCITY PROFILES =1;4

If you used Fudda to create the boundary conditions file and the case file, you should get the correct boundary order.

Good luck!

Hailiang

Thank you Hailiang for your suggestions.

I followed your suggestions as well as made some other modifications as follows.

1. I remade the mesh from the beginning where those thin cells are not present now.
2. I gave the proper order of the boundary where Boundary 1 = outflow and Boundary 2= Inflow.
3. I removed air pressure option.
4. I changed time step=0.1 seconds
5. I set the Velocity profile option as per your comment.
6. I set the initial condition=constant depth=0.04
7. I also changed some numerical parameters.

Simulations results improved quite well. However the ill posed problem occurred. The velocity at the outflow boundary seems very high. At other places inside the channel, the results seems good.

But the volume balance is not correct. The amount of volume entering the domain and coming out don not match. Hence If I run the simulation for longer time, the inflow volume becomes negative. It looks like the volume going out is greater than the volume coming inside the domain. Is it also related to the boundary condition?

My confusion now is,

1. What does the initial condition=constant depth/constant elevation/zero depth mean? Does it mean the condition at the start of the simulation. for example initial depth=0.04, means, water with a constant depth of 0.04m is already present inside the whole channel?

2. Can we set the inflow/outflow boundary location at slightly different location from the main domain boundary? For example, if our domain of simulation is x=0 to x=100, the can we set inflow boundary at x=10 and outlet boundary at x=90? but the simulation will occur from x=0 to x=100 see the attached figure mesh1.jpg.

3. What can be other possible solution of the ill posed problem? or is it the boundary condition is yet not defined properly by me for the model to give appropriate solution?

Please check the attached files.

Once again Thank you.

Regards,
Saroj karki

1 Yes constant depth 0.4 m means water is 0.4 m everywhere in the domain at time zero. You could also verify it by viewing the water depth output at time zero. For river flooding study you may want to set the water depth to zero in floodplain and some depth inside the stream/river. To achieve this you could create an initial depth geometry and feed it as a previous computation file. This initial depth is related to the negative flow out of the domain. It will take longer time for the model to achieve water balance (ie inflow = outflow) with higher water depth than it should be at steady state. So to reduce the discrepancy between inflow and outflow, you can run the model for longer duration.

2 No. Boundary conditions are to be defined at *physical* boundaries. To achieve what you would like to do, you can use sources to inject into (positive flow) or extract (negative flow) water from the model domain.

3 The ill posed problem has been discussed at post www.opentelemac.org/index.php/assistance...48-ill-posed-problem.

Hailiang