Recently, I've modelled a Torrington fan (and scroll), often known as a hamster wheel fan or squirrel cage fan using CFX-Tascflow.

Comparing the pressure rise predicted by CFD to that measured in an experimental test of the fan and scroll, I've found that the model significantly under predicts fan performance. I've found this surprising as usually CFD over predicts performance owing to simplifications not capturing all of the loss mechanisms.

In turbomachinery terms, the aerodynamic conditions associated with the operation of these fans are far from ideal. Large angles of incidence exist at the leading edges of the blades and I'm wondering if this may be a root cause of the problem?

Has anyone, any knowledge of modelling these types of fans and if so, how have your results measured up?

Alan

(1). For single blade row, axial turbine analysis, the predicted loss was not satisfactory with Tascflow, based on my experience. (absolute values are way off the test data) (2).Thin balde, large incidence angle, and possible flow separations are potential loss factors. (3). Here you must use fine mesh and two-layer models at least.(does not mean that you will automatically get the accurate solution.) (4). I don't know the source of problem, but it coud be related to the algorithm and turbulence models used in the code. Pressure is easier to predict, but the loss and efficiency is far more difficult.(not possible unless the method and turbulence model are validated for this problem.)

John's made some good points there.

Are you using a sufficient number of cells in the blade channel? It is very important to accurately capture the loss mechanisms associated with your high angles of incidence.

How well does your model handle convergence? If there are difficulties, it might be due to the transient nature of the flow through these fan.

Phil

What sort of modelling did you use

- steady with mfr or frozen rotor

- transient with sliding mesh

and how much details of the fan did you take into account? Where are your boundaries for inflow and outflow located? Are you convinced that the boundary conditions somehow match the reality?

There is one important point to think about. The flow in a turbomachine is always transient with some sort of rotor-stator interaction.

All the stuff with turbulence modelling and differencing schemes becomes obsolete, if you already over-simplified your modell.

adapco have had a go at this configuration using StarCD. You can see there approach at www.adapco.com

Hi,

john, phil and joern made very good points.

From my experience flow in this kind of blower is often instationnary. in order to expect at least good results you should actually use transient sliding mesh.

Make an accurate mesh regarding blade edges,

best regards

Hi,

what might be a adequate combination of boundary conditions for the inflow and outflow of the fluid domain, if the fan does operate in a room with air at rest ?

Thanks for your opinion,

Marat

Thanks for the suggestions.

I suspect part of the problem could lie with the number of cells I'm using in my impeller. In total, I have 155,000 cells in the impeller, but per blade passage this only amounts to just over 5000. My volute has 30,000.

I'm modelling steady-state with a moving reference frame (frozen rotor interface) and the convergence behaviour is good. I have experienced other fan/volute combinations that exhibit poor convergence due to transient behaviour. These had similar sized meshes & operating conditions which makes me hopeful that I haven't oversimplified any unsteady phenomena in this case.

For the turbulence model, I'm using k-e with scalable wall functions but have also tried k-w without success.

I have now increased my cell count to 14,000 per blade passage and am awaiting the results...

Cheers,

Alan