Why different Y+ values using different Turbulent Models with same Mesh
 

Dear all,

I am modelling a 3D model of a compressor blade cascade. (7 blades in a row).

I experimented on 3 Turbulent models; Spalart-Allmaras, k-epsilon, and k-omega

The y+ values on the surface of the blades are of prime importance. So I checked the results using contour plot of a y+ on the blade surfaces. The findings are as follows;

SA: max y+ is around 8
k-e and k-w : y+ stay between 0-2

My question is why? The mesh and all other settings are unchanged, I only switched between different 3 turbulent models. How could the y+ values be different? From my understanding there is only one equation for y+ which relates the velocity, the distance from the wall to the adjacent cell, etc.

Could you please suggest?

May I ask a second question;

Since I want to stick with the Spalart-Allmaras turbulence model, which requires y+ less than 1 or over 30

I have tried to coarsen the mesh so that I would achieve y+ > 30, but I obtained loads of poor quality elements as an exchange. So, I decided to stick with the y+ = 1 approach.

However, I could only go down to 8 instead of y+ = 1 to 5, keeping number of elements, aspect ratio at a manageable level.

My question is, by saying y+ = 1 is the requirement, if I could only achieve y+ of 8, would this mean my solution is completely wrong?

or the farther you go from y+ = 1, the less accurate your solution gets?

If I could only get y+ = 8, will this be acceptable? Not being able to achieve y+ =1, what would this affect the accuracy of the solution? in what aspects?

The velocity in the y+ is unknown until you solve the problem. That is, y+ is not known a priori.

With different turbulence models that predict different flows you should expect a different y+.

Ahhh..... this clears things up for me.

Please correct me if i'm wrong...

So, the velocity, as a solution, is the reason why the calculated y+ has different values using different turbulence model? Even though the original mesh is untouched.

Could you please suggest whether or not my calculated y+ of 8 (ideally it should be 1-5 as required by the SA turbulence model) is sufficient?

y+ is a non-dimensional wall-normal coordinate scaled based on the friction velocity. It is not limited to only the 1st wall adjacent cell and you don't need a mesh to calculate y+.

You already know from superior turbulence models (k-e and k-w) that the wall y+ is more like 2. The fact that SA predicts something much bigger should be interpreted as a failure of the turbulence model and/or the wall functions, not your mesh.

As an impropable example, let's say you know the actual y+ (from say DNS or measurements) is already 0.001. You can refine the grid forever and maybe never get this number because your model always wants to predict something else. Again, this is not the fault of your grid but the flow that each model spits out. On the other hand let's say the actual y+ is 100. So relative to the true y+, all your models have already over-resolved this region but yet you somehow still get the wrong y+.

The more important question is whether your result is even sensitive to the wall y+? Otherwise who cares? If you are worried about y+ sensitivity, then you should do a y+ sensitivity by running several meshes (which you should always do anyway).

y+ is not of prime important. What is your sought-after-parameter? Are you doing CFD for the sake of calculating y+? Or are you doing CFD for the sake of getting an actual result? These are the problems you should focus your effort into solving.

Thank you very much,

This is getting deeper and deeper and requires time to understand your answer.

In a meanwhile, I will give an answer to your question, I am running a blade (axial compressor blade of a gas turbine) cascade model (comprises of 7 blade in a row), I will need the static pressure distribution at the blade surface so that I can compare them with the experiment (low-speed wind tunnel).

So, the most important parameter I am seeking for is the static pressure distribution on the blade surface (both suction side and pressure side). Due to the very high angle of attack (36 - 45 degrees, blade is highly twisted from root to tip), the flow at the suction side sees no separation, on the other hand the flow from the pressure side sees separation and large re-circulation area in the stream-wise direction.

So, should I be worried about the y+ value? I am very new to turbulence/turbomachine modelling? A y+ value of 8 is okay?

Here is the computational domain