[guodei]

Hello everyone,

I am confused by how to consider the vertical pressure gradient caused by the gravity in a closed water tunnel in CFX.

I use a simple cuboid model as shown in Fig. 1. The fluid is general water with velocity of 1m/s in the inlet, static pressure in the outlet, and the other boundaries are wall. The mesh is coarse and the convergence criteria is RMS=10^-6.

I have tried two methods to account the effect of gravity: (1) Add a General Momentum Source term in the subdomain with ρ*g in X-axial direction; (2) Use the Buoyancy Model with g in Gravity X Dirn.

About the outlet boundary conditions, I am not sure whether to use ①a static pressure gradient distribution with expression of ρ*g*x or ② a uniform static pressure of 0Pa. I make comparisons among these schemes as (1)①, (1)②, (2)① and (2)②. The contours on the ZX plane are shown in Fig. 2(a-d).

As the CFX-Help states that the pressure in the momentum equation excludes the hydrostatic gradient due to reference density when buoyancy is activated, so I think the schemes of (1)① and (2)② is more suitable.

Maybe the distributions of absolute pressure between the two simulations are similar, but if doing a further research in the tunnel, what effects on the cavitation from the differences in pressure? I am not sure which one is accordant with the actual flow feature.

I am looking forward to discuss with you and thanks in advance!

Fig.1
Fig.2a
Fig.2b
Fig.2c
Fig.2d

[ghorrocks]

First of all, there is no point in modelling the hydrostatic head unless it does something. So if your simulation is constant density then forget about modelling hydrostatic head and just model it with no gravity. If you want to see what the hydrostatic head is you can simply add it in post processing.

It you have to model the hydrostatic head then use the built in gravity model. Read the documentation about hydrostatic head - the definition of pressure is changed such that the hydrostatic component is removed. In this case you model the pressure boundaries with constant pressure.

If you want you can model gravity as a source term. This should be equivalent to the built in model, but possibly a little less accurate and a little less numerically stable as it will suffer greater round off error. You will have to impose the hydrostatic head on the boundary condition in this case.

[guodei]

Originally Posted by ghorrocks

First of all, there is no point in modelling the hydrostatic head unless it does something. .

Thank you for your reply. It makes me have a better understanding about the reasons for the differences between Fig. 2a and Fig. 2d above. So just pay attention to the contours of the absolute pressure in the two figures, does it can be inferred that the source term and buoyancy methods have got the same predictive effect?

Then I simulate a rotor in a tunnel. The rotor is like the wind turbine, just can be used for marine current or tidal turbine. The boundary conditions are similar to the tunnel simulation above and just with a rotating speed for the rotor.

When I use the unsteady simulation using the source term and buoyancy methods to account for the gravity, the results are significantly different. Fig. 3a and Fig. 3b show the streamlines (with variable of Velocity in Stn Frame) through the rotor region. The unsteady simulations have experienced several rotation periods.

I am confused by the differences.
Fig.3a
Fig.3b

[ghorrocks]

I do not understand what you are modelling in the pressure plots you display. Please label the diagrams.

As for your fan simulations:
As I said in my previous post, unless the fluid has density as a function of something then gravity will have no effect. I assume these are incompressible simulations. That means that the simulation which has the distorted fan wake in it is simply poorly converged and/or numerically unstable caused by the introduction of the unnecessary gravity term. That is exactly why I recommend that you do not include it unless you need it. This especially goes for the source term approach as that will cause far more round off error than the built in gravity model.

[guodei]

Originally Posted by ghorrocks

I do not understand what you are modelling in the pressure plots you display. Please label the diagrams.

Thank you for your quickly reply.

Fig. 2(a-d) show the contours on the ZX plane which is the vertical middle section in the domain.

I am interested in the cavitation predictions for the rotor. Considering the pressure distribution will affect the cavitation characteristics, so I want to include the gravity effect to make the calculation closer to the experimental condition.

Is there any way to judge the round off error?

[ghorrocks]

If you want to include hydrostatic effects due to its effect on cavitation then you will want to use the built in gravity model.

It is difficult to quantify round off error. Really all you need to know is whether you have enough round off error to cause a problem. You can tell this by switching between single and double precision (as this directly affects round off error), or by introducing something which has lots of round off error (like a badly chosen reference pressure).

[guodei]

Originally Posted by ghorrocks

If you want to include hydrostatic effects due to its effect on cavitation then you will want to use the built in gravity model.

Thank you very much for your help. I will try it.