Weird hydraulic jump with interFoam [SST k-omega]
I want to simulate free surface flow (or stream flow) around cylinder. Now RAS model SST k-omega is used.
[v=2m/s at +x direction, the water level is set to h=0.6m using groovyBC]
It seems that the results looks reasonable (see Fig above), however, the hydraulic jump at the front of Cylinder looks weird, while the flow is more or less "dynamically stable". Is it because the inlet is too close to the Obstacle - cylinder?
I checked the BCs but could not figure this out, is there some wrong the BCs with inlet?
you are specifying 2 conditions for the flow: level and velocity.
Your level is increasing due to the presence of the obstacle, but GroovyBC does not allow the flow to reach the boundary (see how there is no water above your given level for the cells adjacent to the inlet).
Depending on what was your goal, taking the inlet far away enough from the cylinder may solve your problem, if you want to prescribe both level and velocity.
If what you need to impose is only a discharge (velocity) I guess you should leave alpha1 as zeroGradient and code a BC to calculate the wet area and apply the calculated velocity to such area. In this case you most probably can reach a stable state with your current domain.
thanks for your tips.
the inlet velocity is set quite low while keep the water level, now the result is fine!
Btw, how to set the outlet BCs to achieve the same water level as inlet's?
can i ask BC of your case?
U and p_rgh
I am carrying out the case similar to yours
Were you using interFoam or LTSInterFoam for your case? Which fvSolvers and fvSchemes did you use for the kOmegaSST model? I'm trying to run interFoam with the kOmegaSST turbulence model, but I don't know which solvers and schemes to use, since the tutorial for kOmegaSST is only for the LTSInterFoam.
Thanks for the help!
To answer the question about setting the downstream water level, this can be a bit tricky in OpenFOAM compared to other solvers.
Your current downstream boundary conditions are von neumann (eg. zeroGradient) for pressure, so the boundary isn't influencing upstream pressure in the domain. If you want to influence the upstream water level, you need to set a dirichlet condition using fixedValue or some formula for the hydrostatic pressure at the downstream boundary.
Flow3D accomplishes this with a hydrostatic boundary condition, where an outlet water depth can actually be specified. Within OpenFOAM, I've had success using totalPressure, and setting the value to the water depth * specific weight of the fluid (e.g. 9810 Pa for water). Water depth should match your initial condition for alpha.
The above technique can require some trial and error to prevent sloshing. Also, the above formula only applies to the liquid phase. You will need to apply a neumann boundary or totalPressure of 0 for the air portion of the boundary. Be careful of the phase interface in your implementation.
Once you have it working, I'd be interested to see the results.
Didnt login CFD-Online for a long time since I was working on DEM-CFD couling topic.
I will give a try when i have time.
|All times are GMT -4. The time now is 07:44.|