[gmingardo]

Hi everybody!
I am trying to match the spanwise distribution of total pressure losses from my CFD results with some experimental results that I've been provided with.
You can see from the figure that the two curves differ both in trend and in values. In general, it seems that the CFD is over-estimating the pressure losses.


The plot shows the comparison between CFD and Experimental results. In the y-axis you can see the difference between inlet total pressure and local total pressure, normalized w.r.t. the former. In the x-axis, there is the distance from the endwall, normalized w.r.t. the blade span. These values are the pitch-wise averages of the losses at each distance from the endwall

Those results have been obtained with:
Mesh: structured, 3.5 million elements (chosen by mesh size convergence analysis), y+ between 0 and 4.
Solver: CFX, SST as turbulence model with all default characteristics, Tu = 10% (as this gave the most similar trend, even if the wind tunnel has Tu = 1%), velocity profile as inlet boundary conditions, average static pressure at the outlet.
The Reynolds number is around 70000, the convergence is fast and smand the simulation is stopped at RMS=1E-6.
I am playing with many parameters in order to solve this problem, for now with not much success. I tried other turbulence models, in particular some Reynolds Stress Models because I read that the isotropic assumption of the Reynolds Stress Tensor could not hold for the secondary flow, but the result didn't change. I also tried transitional models, both Gamma and Gamma Theta, but nothing. I changed the mesh to have y+< 1 everywhere, but again no improvement. Also, I changed the value of the beta* parameter, the A1, the alpha and beta of the omega transport equation.
I read in "Secondary Flow Loss Reduction in a Turbine Cascade with
a Linearly Varied Height Streamwise Endwall Fence", Krishna Nandan Kumar and M. Govardhan, that none successfully modeled the pressure losses with the secondary flow, but it was 2011.
My question:
Do you have any suggestion? Do you know what would be an appropriate turbulence model to capture the total pressure losses when there are large regions of secondary flow?

Thank you a lot and please tell me if any more information on the simulation should be provided

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Also, I have no idea what your graph shows. Labelling the axes would help.

[gmingardo]

Thank you for your response and for the feedback! I tried to make the whole question clearer.
Anyway, I read the thread you linked me, and I've found particularly interesting the part about the discretization error, so I'm going to go deeper on it. However, I already performed a mesh convergence analysis (keeping fixed the size of the first boundary layer element) and I am already sure that the total pressure loss is constant for increasing mesh size. Also, I already tried to refine the boundary layer, making y+<1 everywhere, but this didn't change the result.
The other suggestions are useful, but I think I have already taken them into account.
I am quite convinced that the problem lays in the turbulence model. Do you think that it would be clever to change some model parameters?

[ghorrocks]

Don't forget boundary proximity checks and convergence tolerance. They are important too. Your comment about not matching the experimental turbulence intensity is concerning, I would look into this more closely - note that you need to define 2 turbulence parameters in a 2 equation turbulence model. Turbulence intensity is one, but a second will be a length scale, dissipation or something like that. So do not forget the second turbulence parameter.

Assuming you have done the normal accuracy and error checks described in the FAQ....

Your airfoil is at Re=70000. This is quite a low Re and most airfoils at this Re are laminar for a good proportion of the foil (and could be mostly laminar if it is a laminar flow airfoil). This means turbulence transition effects are likely to be important. So I would look at the turbulence transition model again, that is a likely candidate.

Providing this airfoil is running at an angle of attack which results in attached flows then SST + turb transition model would be the model I would consider. Anisotropy should be small so RSM is not required.

I strongly recommend against tweaking the model to get it to fit your data. Unless you REALLY know what you are doing (ie are a turbulence modelling expert) you are just going to make it worse. The models provided with CFX are very general in nature, so if the turbulence model is not working then you have probably chosen the wrong turbulence model.

[gmingardo]

The flow I'm analyzing regards a linear turbine cascade, actually, not an airfoil. It's an internal flow, sorry for not specifying.

For the boundary proximity, I am using the inlet velocity distribution at the distance from the inlet at which it has been experimentally measured, namely one blade pitch upstream. The outlet instead is positioned 3.5 blade pitches away from the outlet, while measurements are taken 80% of a pitch downstream the outlet. What do you think?

An overall total pressure loss coefficient ((Pt_inlet-Pt_outlet)/Pt_inlet) is plotted as user parameter during the convergence, and I saw that it reaches a steady value before the end of the convergence, which is set to stop at RMS = 1E-6.
I thought it can be a good indicator, assuming that if the total pressure is converged at inlet and outlet, and the maximum residual for the pressure is in the order of 1E-6, it means that the pressure field is converged. Do you think it is a valid criterion to assess a proper convergence?

For the length scale, I always let the solver autocompute it. Should I set it on my own?

Transition models already gave me an improvement but it was still far from matching with the experiments.

For what regards separation, my flow has a strong secondary flow that actually causes a separation from the suction side caused by the interaction with the vortex. That's why I though that anisotropy could have been a problem, but the Omega-based Reynolds Stress Model did not change the result.

I followed a course on CFD and I further studied in these days the SST model, so I have an idea of how the coefficients influence the transport equations. However, I'm far from being an expert in turbulence modeling.

Thank you for all the suggestions and help!

[ghorrocks]

Boundary proximity: Do a simulation where you double the distance to the inlet and/or outlet. If it makes no difference then boundary proximity is OK. If it changes then you need to be aware your results are sensitive to the boundary location.

Convergence: Same as for the boundary proximity - make the tolerance much looser or tighter (eg RMS=1e-5) and see if it makes a difference.

Length scale: If you have experimental results then you need to make sure you specify both turbulence parameters so you have the turbulence intensity and dissipation correct. I would not trust auto-compute.

Transition Model: OK, a step in the right direction but it sounds like you have not checked several other factors (boundary proximity, convergence tolerance) so do not write it off yet.

Separation: If you have a large separation then that changes things a lot. SST might not be suitable. I would consider DES or SAS approaches, or possibly LES if you are brave and have access to some powerful computers.

Tuning SST: Based on this post it may be possible that SST is an inappropriate model. You won't fix that by fiddling with the model constants, it is an inherent limitation of the model.

[gmingardo]

Alright, I will check all these things and then I'll let you know if there will be any change. I have very limited computational power so I really hope to fix everything with the other factors.
Thanks a lot for the help