Simulating rotating vane of unknown speed
 

Hi,

I need to simulate a horizontal axis rotating vane but its angular speed unknown and is due to the known freestream velocity. In addition, I want to model the vane rotation as it accelerates from rest until it reaches a steady rotation.

Since the angular speed is unknown that rules out using a rotating domain. Also I don't see an immersed solid working suitably because that does not capture the vane's boundary layer. Finally, there is the rigid body solver, but again it seems that the rotational speed must be defined. I had planned that the rigid body solver could rotate the vane due to the forces on it and cylindrical volume of mesh encapsulating the vane would rotate inside a large stationary mesh via GGI, therefore not needing remeshing. But again I don't see CFX allowing this option.

Does anyone know how to model a rotating body of undefined angular speed?

Thanks

Do you mean you want to model the 3D air flow of the rotor as it accelerates (this sounds like a very long simulation) or do you want to know the angular velocity versus time curve of the rotor (this is very simple to do).

Why? Why not do a range of speeds up to the maximum speed you expect to see and then you have a performance curve of the rotor. Then it is a simple ODE to model the rotor speed versus time and does not require a massive CFD simulation.

For most cases this is correct.

I think the model you are thinking of is the 6DOF solver. This will allow the solid to accelerate. But I say again - this is a very inefficient way of modelling this and will be a massive simulation. A far more efficient way is to do enough frozen rotor simulations over a enough speeds to get the rotor performance curve. Then a simple ODE will give you the speed versus time as the rotor accelerates. This is much more tractable simulation.

Yes, to the first point. I had intended to do a steady-state simulation to 1) model the rotor being locked in position with the freestream flowing past it and 2) initial conditions for the transient simulation. Then do a transient simulation so that the unlocked rotor would spin up to it's maximum angular speed due to the airflow past it. I knew it would be a time consuming simulation but would have expected to be simple to set up.

So it looks like you want a rigid body simulation with the 6DOF solver. Have a look at the tutorial examples for how to set this up - the Buoy model sounds like it is relevant to you.

But I repeat that a more effective way of simulating this is to use a series of simple frozen rotor simulations to get the fan performance curve, then use a simple ODE solver using the performance curve to model the acceleration/deceleration.

Ideally, yes I would have liked to run the simulation with the rigid body solver. But when looking into this I do not see it is possible for the vane to rotate due to the freestream velocity (i.e. not prescribing a vane angular speed) without need to use remeshing. I had broken my geometry upon into a cylindrical volume around the vane, which was inside a larger stationary volume (like the CFX multiphase flow in a mixing vessel tutorial). But I could not see a way of rotating that mesh volume. If this method had been possible then I could simulate the acceleration of the vane from rest to constant speed

Instead I am going to run a series of steady-state simulations, as you mentioned, using the frozen rotor option over a range of vane angular speeds and vane disc position (because fins block the vanes). so I can then plot the vane torque against the vane speed and vane position and when that is the same as the vane's mechanical resistance torque then the vane would in reality be at constant speed. Glenn, is this the method you meant?

If you look at the tutorial example it shows how to make the mesh rotate with the body. As this model only requires rotation this should fully describe the motion with no remeshing.

The method I recommend is to get the performance curve over a range of rotor speeds. This means get the average torque, where the average torque is over the rotation cycle, so including the effects of the upstream obstructions. Once you have the performance curve it is a simple matter of integrating this over time against the inertia of the system, any losses and the power being taken off (or applied) by any external device like a generator; and then you can do a ODE model of the rotor speed against time.

But in the tutorial the angular speed is specified. Where in my case the solver must calculate it due to the freestream airflow.

? I just looked at the tutorial and it does not look specified to me. The rotation of the body is caused by the fluid pushing it around.

What version of CFX are you using?

I am using CFX v17.0. Perhaps we are not talking about the same thing. Tutorial #17, which has the rotating mesh zone at 84 rpm defined. The rigid body tutorial #32 has expression for the buoy walls. I've attached the Guide pages. However, I may have found a way to do this but it needs testing over the weekend.

No, I am not talking about #17. I am talking about #32, the floating buoy. The moving wall you highlight is just to create a wave in the liquid, nothing to do with the rigid body motion. If you look at this example you will see it couples the mesh with the rigid body motion.