[shobhit21]

Hello

I have recently started learning openFoam. After a few tutorials I tried to simulate a test case of my own. I am trying to simulate a dam spill way. I was able to generate mesh using gmsh and used it with openFoam interFoam solver using k-Epsilon turbulence model. I have setup 0, constant and system files.

I checked the mesh using "checkMesh" which gave me the output "Mesh OK"

Then i set up the alpha.water to initiate the simulation from a predefined state where the water will be filled behind the spillway using "setFields". Analyzing the flow using paraFoam, I could visualize the alpha.water in the desired zone.

With decomposePar, I was able to divide the work into 4 processors and then execute the simulation using: "mpirun -np 4 interFoam -parallel" and then "reconstructPar" to reconstruct the outputs.

Observations:
1. During simulation, max and min courant No is 0.
2. The simulation ends in few minutes when the deltaT :0.005
3. paraFoam Analysis shows no changes in any parameter with time.

I am attaching the files for reference.
https://drive.google.com/drive/folde...usp=drive_link

[Tobermory]

Looking at your setFields:

regions
(
    boxToCell
    {
        box (-15500 0 0) (15500 25000 45000);
        fieldValues
        (
            volScalarFieldValue alpha.water 1
        );
    }
);

you are setting your initial water column to be 45km tall, and you have an initial time step of 0.02s. The simulation is working just fine - you wouldn't see any effects of gravity at that lengthscale in that time scale.

Go back to your gmsh mesh and rescale it so that the mesh is in metres, and not millimetres, then try run again (after adjusting your setFieldsDict).

Note that in 99.9999% of the cases, you should assume that OpenFOAM can only work in a fixed unit system (kg, m, s etc.)

[shobhit21]

Thanks for pointing that out.
I have scaled the mesh and rerun the simulation but still I could not see any changes in the flow. Now during the run there is a change in Courant number but no velocity or pressure changes or observable flow changes at different time intervals. I believe that I am making some mistake in the boundary conditions. In the image,the flow after 30 seconds of simulations the flow should come out of the spill way due to the initial velocity at the inlet. I would like to understand what mistake I am making here. I am uploading the case after the run for your reference.

https://drive.google.com/drive/folders/1wbkOT2a90v0qmttTw-8WWAVwy8r8ijCB?usp=drive_link
Thanks in advance.

[Tobermory]

A couple of quick observations. Firstly your mesh is awful - for free surface modelling, you want good resolution across the surface, and typically this means using a hex mesh, not tets. This shouldn't prevent you getting a solution, although I have found that OpenFOAM doesn't deal well with tet meshes - it becomes rather unstable. If you want to persist with tets, then google to find more info on the fvSchemes and fvSolution settings that you'll need to use.

Coming back to your boundary conditions, you have set a fixedValue of 1 for alpha on the full height of your inlet plane ... which is not physical. That's why the contour in your attached picture jumps at the inlet plane. You need to use something else - eg variableHeightFlowRate. Check out the interFoam weirOverflow tutorial, which is basically doing the same flow scenario as yours.

Good luck!