Hi everyone! I want to simulate a hydraulic turbine (Francis). CFX resolves rho*g*z term in N. S. Equation automatically when I use water as material or do I need to set buoyancy? Why does CFX ask me to set a reference coordinates for buoyancy? I'm confuse. Can you explain me about buoyancy?

Thanks a lot!

You choose where is the direction of your gravity!

Thanks but I don't understand if I need to use buoyancy or not. I have two simulation with the same bc one is with buoyancy and other without. I don't find any real differences in pressure and total pressure. In buoyancy case I have an absolute pressure different from pressure because there is the rho*g term. Then what's the differences in two cases? If I don't use buoyancy does CFX solve correctly my flow? Thanks

when u consider buoyancy , you will perform a simulation more near from experimental!

Ok Thank you very much! But how do I have to set the reference coordinates in buoyancy? Can I set it in automatic? Can reference coordinates modify the solution? I know it modifies the absolute pressure but are pressure and total pressure correct (near to experimental)independently the reference coordinates I choose? If I use buoyancy and I want to calculate energy between Inlet and Outlet, can I write

Energy=(massflowAve(Total Pressure in Stn Frame)@Inlet-massflowAve(Total Pressure in Stn Frame)@Outlet)/rho ? Or I need to consider

Energy=(massflowAve(Total Pressure in Stn Frame)@Inlet-massflowAve(Total Pressure in Stn Frame)@Outlet)/rho+g*(massflowAve(z)@Inlet-massflow(z)@Outlet) ?

Thanks

Hi, In the case of a Francis turbine, your fluid density is constant and therefore there is no buoyancy effect. The confusion comes from the fact that, in the real power plant, the turbine converts the energy available from the head difference between head water and tail water levels. But, think about the model test, the pressure difference is provided by pumps and not by the geodetic head difference. The turbine is converting the energy difference between inlet and outlet, no matter what causes it. In a CFD simulation, when you set the inlet boundary conditions as prescribed velocity components and turbulent quantities, and the outlet boundary condition as a constant reference pressure, the code will solve for a pressure field, which is compatible with the boundary conditions (with the inlet flow among them), geometry and guide vane opening. Whether in reality a portion of your pressure field is produced by the water level difference or not, it is not relevant for the solver and it cannot recognize it, in this case. In other words, in the case of a Francis turbine, with such boundary conditions, what you will get from the solver is: (p+rho*g*z) instead of only (p). If you are interested in analysing net head, head losses per component and efficiency, be careful then, not to compute the geodetic difference once again. With this set of boundary conditions, your calculated net head may present slight deviations from model test, reflecting in the turbine efficiency. However, for a proper simulation model and turbulence model, in a stable operating point, these deviations should not be significant. There is also the alternative of specifying the pressure at inlet and outlet as boundary conditions, but, then, it is very likely to get the deviations at the volume flow, with the disadvantage that this set of boundary conditions, for hydraulic turbines, can produce convergence difficulties and worse accuracy.

Dear Magnoli thank you very much for your walk-through.

[mohammadfatheh@gmail.com]

how can i get the details of francis turbine , i want to do cfd analysis of francis turbine