Hi there,

I'm currently trying to simulate airflow into an air intake, using CFX 5.5, but I have problems with the pressure results I get. I started doing simulations on a bellmouth inlet on which I have extensive experimental data. I find that the pressure losses (both static and total) are predicted way too high with the CFX simulations. The losses are over predicted by anything from two to five times as much. I have tried the k-e and SST turbulence models with progressively finer meshes and boundary inflation, but the answers still remain the same. The boundary conditions are defined as Openings (with the static pressure defined) around the control volume and a single mass flow outlet. Did anyone have similar problems before and, more importantly, does anyone have a solution as to what I can do to improve the CFD results? Any comments or suggestions are welcome.

René

Hi René,

I recommend setting your inlet boundary condition to "Total Pressure", this is the most sensible for such an inlet. If you were to look at the total pressure distribution at your (static pressure) inlet, you would see some variation. This would be physically incorrect, since it is the total pressure which should be constant in the far field.

Also, what advection scheme are you using?

Robin

What sort of convergence levels were you attaining and what do your flow balances look like? The default is 1.0e-4 RMS, you might have to go down to 1.0e-4 MAX to get better results.

The pressure drop will be strongly dependent on the both the inlet turbulence levels and velocity profiles because these strongly influence the boundary layer growth from the inlet. Are you 100% sure about your inlet boundary condition? I think you might want to try a total pressure inlet instead of a static pressure opening as well.

Also, as Robin mentioned, what advection scheme are you using? Upwind is bad. If you are running incompressible flow use a specified blend factor of 1.0. If your running compressible flow, and your flow has shocks in it somewhere then use the high resolution scheme.

Neale

>If you are running incompressible flow use a >specified blend factor of 1.0. If your running >compressible flow, and your flow has shocks in it >somewhere then use the high resolution scheme.

a blend factor a 1.0 is not the same as high resolution?

Hi,
By the way, what means this blend factor?
I always used to work with classical 1st and 2nd order schemes, the classic ones, 1st order: Upwind, Power Law, Hybrid, WUDS, etc.. 2nd: Higher Upwind, Van Leer, etc... But Blend Factor, I never heard about it. Perhaps I should take a look at the manuals.
Sincerely, cfd guy

It a parameter for the NAC scheme in CFX-5 isn't it, to blend between Upwind and NAC?

blend factor=linear scaling factor between upwind and second order scheme

Hi Bart,

A blend factor of 1 sets the discretization scheme to fully second order.

The High Resolution scheme is a bounded second order scheme. This will result in a beta value (blend factor) of 1 throughout most of your domain, but the solver can locally change the value of beta to ensure that there are no "wiggles" in the solution. These "wiggles" develop when the second order correction terms cause unphysical values where sharp discontinuities occur, such as at a free surface or shock. By changing the value of beta, the solution remains physical and offers a sharper solution (hence High Resolution).

If you are curious what value of beta the solver has used, they are written to the results file for each equation set (Velocity U.beta for instance).

Regards, Robin

If this high resolution scheme behaves like a TVD scheme with limiter. At what value of the gradients does this scheme then swith from 2nd to 1st order? I wrote my own TVD code (Euler). What I want to know how a TVD scheme behaves in f.i. the boundary layer (steep gradients in tangential velocity)

Hi Bart,

The High Resolution scheme does not just switch from 2nd to 1st order (ie Beta=0 or 1). Rather, it will set Beta to whatever value it takes to keep the results physical (i.e. eliminating overshoots and undershoots). I'm not sure what what exactly occurs in the boundary layer, but if you are curious, you could set up a simulation and look at the beta values near the wall.

Robin

You said that we can check out these Beta values. So I ask you, these values are in the .res file by default, or must I add any extra expert parameters?


Sincerely, cfd guy

They are in there by default. In Post, the pull-down menu of variables gives you a short list of commonly desired variables, click on the [...] button next to it and you will get the full list.

Of course, the beta values are only there if you ran High Resolution.

Robin