Pressure coeff for aerofoils problem
 

Hi all.
I am simulating simple 2D aerofoils (f.e. Joukovsky) with CFX 11 and compare results with JavaFoil, XFoil and others. AOA are very moderate (up to 8deg), Re~250000.
The problem is that results shows constant overestimation of Cp in the region near the leading edge. On the pressure site the Cp reaches up to 1.1, while on the suction site it is approximately -1.6 while other sources shows up to -1.8-2.
My Cp i CFX post is defined:
(pressure-TurbulencePressure)/(0.5*Denisty(inlet)*Velocity(inlet))

I have been trying everything:
- compressible/incompressible,
- mesh,
- turbulence model, conditions,
- AOA, Re
- ......

What else can it be?

Luk

If you are using the other packages incompressible then only run CFX incompressible.

Why are you taking the turbulence pressure off the pressure in the CEL function?

Have you tried a transitional turbulence model? This may affect things in the Re range you are operating in.

I decided to neglect this term because:
- XFoil and others unlikely adds turbulence effects to pressure
- CFX manual states that in case of k-turbulence models this "turbulence pressure" adds to static pressure (however in other place it is stated that to include turbulence in pressure Expert Option must be switched(???)) I dont know what to do with this, however subtraction turbulence helps a little, but not enough.

Unfortunately, transition model changes nothing.

Luk

If the pressure coefficient near the leading edge is wrong then it is unlikely to be a turbulence model problem. I am guessing that the velocity, AOA, material propoerties are wrong, or you have insufficient numerical accuracy (which usually means too coarse mesh).

Can you describe what you did to show mesh does not change things?

Well,
In fact I think, that this is something "inside" calculation itself (no matter what AOA or velocity), because the inconsistency with other sources (like XFoil) comes from sensless effect that static pressure (I mean p in nominator of Cp) seems to be higher than possible.
About the mesh:
- I was using hexa and tetra,
- I was using boundary layer prisms with different y+, and different thickness,
- I was trying different mesh densities along the profile (down to 0.2mm for 200 mm long profile).
- in any of this situation the solution is converged down to 10^-6

The last thing that comes to my mind is to check domain size, however it is quite big now, up to ten times the profile length in every direction.

Lukasz

I have no idea what your first sentence means.

These numbers are meaningless by themselves. You have to establish the accuracy as a % error to make any meaningful error estimates from mesh size. You then design the model to give an allowable level of error for your application. See references like journaltool.asme.org/Content/JFENumAccuracy.pdf for further details.

Talking about some potential error in simulation itself, I mean that no matter what velocity I set sensless Cp occures (By the way what do You mean by "wrong" AOA or velocity? These are boundary conditions and cannot be "wrong" just because some results (like Cp) defined by these conditions occures to be sensless. As I said - this Cp is basicaly SENSLESS and, just after that "wrong" in terms of discrepancy with XFoil. I know that Cp CAN BE higher than unity but not in this case).

About the mesh - in CFX manual there are strictly guidances about mesh preparation for different transition models (if we take transition as a source of the error). The description I put is enough to say that I have checked it all, mabye despite y+ - I checked from 0.1 up to 11.

But anyway - meantime I think that find the source of the error!. It was domain length upstream the foil. The Cp on pressure side drops from 1.1 down to 1.02 just after I stretch it from approximately 7x profile length to ~15x profile length... hmm... If this is a source of error than I am bit shocked...had no idea that size matters that much:))))