Learning Forum

[jfe293]

Hi!

I am running a stormwater retention pond using single phase approach in Fluent. The total height from free surface to the pond bottom is 3.3050m.
My boundary conditions are given below:
Inlet Pipe: Velocity InletOutlet Pipe: Pressure Outlet with gauge pressure 24320 Pa (hydrostatic pressure: 1000* g *Distance of the centroid of the outlet pipe from free surface h = 2.48m)

Free surface: Zero Shear Wall

Other Walls: No slip

My operating pressure is 101325 pa 

refererence pressure location is X=0 Y=0 and Z=0.

My question is how Ansys is calculating the pressure on free surface based on this condition. As it's an open channel flow simulation pressure on free surface should be zero. But I am getting around 26900 pa.

I know that Fluent always calulates the gauge pressure inside the computational domain using the following formula:
Pabs = Patm (Operating Pressure=101325 pa) + Gauge Pressure
In that sense, I am getting the gauge pressure on free surface as 26900 Pa. But according to the physics of open channel flow there should be zero guge pressure on free surface. So, how could I fix it?

[Richie Mathew]

Hello!

You can try the following steps to get better results:

1. Set operating density as 0 kg/m3
2. Create an Expression for Hydrostatic Pressure (Density * g * y). y will depend on where your global coordinates are. For example, if bottom of the domain is 0 and free surface is at 3.305 m, then y = 3.305 - y. Basically, expression should be such that free surface should have gauge pressure as 0.
3. Set the pressure of the outlet pipe with this expression.
4. Use Standard Initialization with gauge pressure as 0.
5. Patch the domain pressure with this expression.
6. Run the simulation.

If the above method does not help, move the reference pressure location to the location of the Free Surface. 

[mpowens]

For a constant  density material the solver pressure solution field satisfies

solver_pressure = physical_pressure - operating_pressure - operating_density*dot(gravity_vector, Position)

There is no option in Fluent to set a relative position.  The pressure reference location is ignored if there are pressure boundaries. But in any case you must set the operating density to zero if you want to see the full gravitational head in the solver pressure solution.