[river_fish]

Hi everybody,
I am trying to simulate open channel flow using InterFoam solver and RAS k-epsilon for turbulence modelling. What I know is the flowRate at the inlet and the water level at the outlet. I have tried all kinds of different BC (including splitting the inlet and outlet to air and water) but I always get problems with high velocities in the air phase, which lead to a very small time step and eventually to floating point error. I therefore assume a problem with my initial or boundary conditions:

Initial condition: constant water level at 443 m, zero velocity (0 0 0) everywhere

Inlet BC:
1. U: variableHeightFlowRateInletVelocity
2. p_rgh: zeroGradient
3. alpha_water: variableHeightFlowRate

Outlet BC:
1. U: zeroGradient
2. p_rgh: fixedValue uniform 0
3. alpha.water: zeroGradient

Besides inlet and outlet, I defined two patches, for the atmosphere and the channel bottom with the following BC:

Atmosphere:
1. U: zeroGradient
2. p_rgh: totalPressure
3. alpha.water: inletOutlet

Channel bottom:
1. U: fixedValue uniform (0 0 0)
2. p_rgh: zeroGradient
3. alpha.water: zeroGradient

I'm happy to provide you with more information (i.e. BC for k, epsilon and nut) and would be really grateful if I could get some advice on how to solve this problem. Thanks in advance!

[David*]

In my experience, two things are important to prevent such behavior:

• initialize an absolutely flat water level, preferably within a small cell layer (~10-20 cm) or even at a cell boundary. For this, you need some effort in mesh generation though.

• correct for deviation from z=0, either by using interFoam's href or by shifting the entire mesh, to have the water level in your model close (<10 m) to z=0.

Cheers, David

[river_fish]

Hi David,

Wow, that was very helpful. I did not realize I had to correct for deviation from z=0. Thanks a lot for pointing this out!

Originally Posted by David*

In my experience, two things are important to prevent such behavior:

• initialize an absolutely flat water level, preferably within a small cell layer (~10-20 cm) or even at a cell boundary. For this, you need some effort in mesh generation though.

• correct for deviation from z=0, either by using interFoam's href or by shifting the entire mesh, to have the water level in your model close (<10 m) to z=0.

Cheers, David