[ld1305]

I'm considering setting up a simulation involving a turbine working which draws water through it. I'd be wanting to apply a variable speed or torque to the turbine which would spin up and spin down; the speed of the turbine is fast enough to cavitate the water on the blades.

Something I'd be interested in adding would be the ability to have the pump speed respond to the resistance of the water, specifically such that when the turbine speed is sufficient to cavitate the water, the pump could over-speed due to the reduced resistance.

I've not been using CFX long, but have used similar UDFs in Fluent which were able to move a body based on a prescribed external force (like the turbine toque) and the resulting increasing and decreasing pressures on the surfaces in contact with the fluid.

Is this kind of behaviour scriptable in CFX in a similar way? Do you have any recommendations on how to approach the problem?

[ghorrocks]

The hard way of doing this is to use rigid body dynamics to allow the forces on the rotor to change the speed of the rotor. But this is really hard and simulations will take a long time to run.

The easy and recommended way of doing this is to use CFX to generate a map of rotor performance over the speed and flow range you expect to see, and then use that performance map in a simple ODE solver including inertia and any other forces you wish to model. This means the performance map is generated by a series of easy steady state simulations and the dynamic behaviour is modelled by simple dedicated solver (not CFD).

[ld1305]

My concern with using a map is that we'd not be able to predict any over-speed due to cavitation on the blades, which is something we'd like to see happen if possible.

In most use cases we'd use a mapped approach as you suggested, but were really looking to try and capture a specific behaviour using something more complex.

Do you have any tips on the rigid body dynamics approach if we need to take that route?

[ghorrocks]

Before you commit to the very complex transient analysis, are you sure you can't include the overspeed effect in a performance map? Your performance map can go into the overspeed region and if it cavitates there then you can model cavitation to include that effect.

The decision on whether the performance map approach is suitable or not depends on whether the time scales of the fluid flow and rotor accelerations are well separated or not. If the fluid time scale is fast compared to the rotor accelerations then you can use the performance map approach (regardless of how complex the flow is). If the fluid time scale is of a similar time scale to the rotor acceleration then you have to use more sophistocated approaches. An example of this would be blade flutter. (Note CFX has a special model just to model blade flutter)

But to answer your direct question - There has been several posts on the forum of people who have used a rotating frame of reference model with a rotor speed which is defined by a user defined function. Search the forum on how to do this. This approach will be MUCH easier than rigid bodies, if it is suitable. A rigid body analysis of this sort with cavitation would be an epic simulation and not recommended unless you really had to do it.