[bolus13]

Hi All,

I am trying to model the flow flow through a siphon using a CFX two phase flow. What I would like to achieve is that the water is driven by the water level difference (pressure) on both sides, but the water level should remain constant. Currently it is driven by an inlet velocity.

Currently the settings are exactly based on CFX tutorial 'free surface flow over a bump'. The model is shown in figure

siphon flow setup.jpg

My inlet is an 'inflow' boundary with normal speed at 1m/s. The fluid values at the boundary I give a VF for air and for water.

My Outlet is a static pressure with the calculated pressure of the air and water column as value.

The top wall is an opening with an Entrainment boundary and 0 relative pressure. Air VF is 1, water VF is zero

Side walls are symmetry. Remainder are no slip walls.

--

During the run I receive warnings that 'A wall has been placed at portion(s) of an OUTLET'. See the attached out file. siphon flow.txt

The run does result ( see attached figure) in a reasonable good velocity field. When I Look at the water velocity field I also see vectors in the air, which is strange. Next to that, high velocity occurs at the boundaries.
siphon spliway water velocity.jpg

If anybody has an idea how to adjust the input, such that the output resembles a real siphon flow, where the flow is driven by the pressure difference and where the water levels remain constant that would be most appreciated

Thanks.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys...f_an_OUTLET.22

In a eularian multiphase flow both phases exist at all locations, so both phases will have velocities at all points. But the almost zero volume fraction in the air region means the water velocity in the air is not important. You could generate a new variable of Water.vf * Wafer.Velocity and that will be effectively zero in the air if you like.

[bolus13]

Thanks for the answer. The explains already part of what I see. The FAQ is also helpful.

Any thoughts on what type of pressure boundary conditions to use to drive this flow whilst keeping the water levels upstream and downstream constant. I do not want to prescribe velocity or mass flow?

[ghorrocks]

For free surface flows you need to be very careful specifying boundary conditions. The flow rate through this device will be dependant on the drop in head from one side to the other. So your boundary conditions need to account for both the correct flow rate and that there will be a drop in head.

The flow over a bump tutorial shows one method, but I find it a little contrived. These sort of boundary conditions are easier when the boundary is only ever a single phase. An example could be if you make the flow well up from under the free surface at the flow rate you require, then the inlet flow is purely water with no air, and it will find its own free surface level and you do not need to define it. This is a much simpler boundary condition to understand exactly what is happening.

[bolus13]

Yes, I agree. It would require first some hand calc to have an idea what the drop in head and flow rate will be. I think this also depends on the type friction and inertia losses encountered. What type of pressure BC and IC would you use for the first situation you describe. Static pressure on both sides equal to the water column pressure as used in de bumb case?

Regarding the welling up. I do like it. So your bottom would be the inlet. In this case what would you use as exit bc

[ghorrocks]

It is all a case of knowing how your flow is controlled. So what is the parameters defining the flow? It could be flow rate, free surface level or pressure. Each of these requires different approaches to definition of the boundary, and you need to consider this at both the inlet and outlet as they are probably different.

[bolus13]

Thanks for the answer.

The flow should be controlled by the free surface level on either side of the siphon. On both sides measurements where done, which I would like to use to drive the flow. Water level upstream is at 6.3m, water level downstream at 5.8m

For this I used opening BC's on the inlet and the outlet using the option 'opening pressure and direction'. The pressure at both inlets is equal to the watercolumn, similar to the flow over a bumb tutorial. Do you think these are the correct BC's to use?

Attached are two images showing the velocity field and the water level (water volume fraction). The mesh is only quads. I use a rough wall in the siphon of 0.001m (concrete)

I get an areaAverage velocity through the sipphon of 2.65 m/s which is higher than the measured values of approximately 2.1 m/s.

Would you have an idea why I get a higher value? Is it the mesh, boundary layer, wrong BC's, or else? What could further improve this result?

[ghorrocks]

It could be any of those of more. See the FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[bolus13]

I understand I have to do those checks.

One thing I am just uncertain about is the use of the boundary conditions for this problem. I know from measurements the still water level (hydrostatic pressure) at either side of the siphon. Can I use that knowledge to define pressure boundary conditions on either side similar to the method and CEL expressions as used in the bumb tutorial.

If I understand correctly, at zero flow speed, the hydrostatic pressure is equal to the total pressure. Now on the inlet I can define a total pressure, but not on the outlet. Here it becomes the static pressure, which I do not know from the start. Any advice on how to best define the BC's?

[ghorrocks]

Yes, if you know the levels you can apply it like the bump tutorial.

The hydrostatic pressure does not equal the total pressure. The hydrostatic pressure is density*g*h, the total pressure is p(static)+1/2 * density *velocity^2. They are very different. Even at zero flow velocity they are different as the hydrostatic head exists at zero flow.

If you know the fluid level then why not just apply the boundaries in the same way as the bump tutorial?

[bolus13]

I did

Are you sure about that. If I measure the static pressure at the seabed it is virtually the same as the water level column (up to where water volume fraction = 0.5), wouldn't that imply that at each location the static pressure equals the hydrostatic pressure.

I did apply the same boundaries as the bumb tutorial. On the inlet I use a 'opening pressure and direction' boundary. Since the flow is moving into the boundary the pressure is taken to be the total pressure (according to the manual). This pressure is then the water column pressure. The water volume fraction at the boundary is determined by the height of the water column.

Now when the water starts flowing the water level will drop, but this change is not reflected in the water volume fraction on the boundary. This is the thing that worries me. The boundary condition will eventually cease to be correct, since the height of the water column at the boundary does not drop when the water starts flowing.

Due to this I think I add more energy into the system then is actually the case. What do you think?

[ghorrocks]

If you read the CFX documentation you will see that when you activate gravity it replaces pressure with a modified pressure with the hydrostatic pressure removed. So please be aware that the variable "pressure" has a modified definition in this case.

Due to this I think I add more energy into the system then is actually the case. What do you think?

Yes, this sounds right.

[bolus13]

Hi Glenn,

Regarding the flow through the siphon in this post.

In real life the flow through a siphon is activated by pumping out air at the top of the siphon. In that way a vacuum is created inside the strucutre and the water can start flowing.

No I want to model this by applying a boundary at the top of my structure that only extracts air, and not the water. Is this possible in CFX?

At the moment I have a boundary modelled as a wall with a source (=sink), but whatever I try, it seems that the air is always extracted together with the water. Is there a correct way of doing this?

[ghorrocks]

I would first use an initial condition which had no air in the siphon. Then you don't need to pull any air out.

But if this is not suitable then put a small outlet with a mass flow rate and monitor the volume fraction of the material leaving. When you start seeing water then you stop the outlet. This is pretty much what I would expect you do for the real device, so it is a good place to start the model from.

[bolus13]

Yes, the first one is logical. I did that. So the simulation starts with the siphon full of water.

Now in real life during the measurements air bubbles entered the siphon at the entrance and had to be pumped out. This is what I try to model.

At the top the siphon I have put a small opening with a wall boundary. Then I have added a boundary source --> air --> continuity and then the option total fluid mass source. The total source is then a negative value proportional to the average air volume fraction at the small opening.

It does work and air is being 'pumped' when it reaches the top of the siphon, but also water and this is not the intention.

I can also select a 'total mass source volume Fraction coefficient', but I am not sure what this is and the documentation is vague about this.

Any idea how to improve this model to only extract air?

[ghorrocks]

Why not just pump everything, water or air? That is what the pump does isn't it?

[bolus13]

It actually works quite fine now. Some water is being pumped out together with the air in the beginning. Eventually most air is out and the pump stops pumping, since the mass flow is related to the air volume fraction at the pump.

Initially I also worked with the homogeneous two phase model. I switched to inhomogeneous, which works much better.

thanks for the help

[bolus13]

Hi Glenn,

The flow through the siphon is working just fine now, but something else came up. Has to do with gravity and rotating domains.

The flow through the siphon is a two phase water-air flow. For this I apply a buoyancy model with gravity included.

Now in the flow I am modelling a tidal turbine with a horizontal axis perpendicular to the flow (a vertical axis turbine flipped sideways). The axis of rotation in not aligned with the gravity vector which does not permit me to run the steady state frozen rotor simulation.

Would you know a solution to this. How can I get the gravity force acting in the correct direction in the rotating domain.

In the meanwhile I am running the problem with only water without gravity and this works fine. Problem is that my power become 'somewhat' higher than with the free surface included.

[ghorrocks]

This restriction is there for a reason - the accelerations due to centripetal and Coriolis effects need to be modified to account for gravity. CFX does not have this model in it so they stop you using this option.

The error message also states that you can use a transient simulation in this configuration. This is one option.

And alternative is you can impose the rotation effects yourself by adding momentum source terms. This will avoid the restriction imposed by the solver but will mean you will suffer from the issue of not properly accounting for the gravitational accelerations - unless you are clever enough to derive the source terms to include gravity, that is.