[Oscar J]

Originally Posted by ghorrocks

As you are using Fluent, not CFX I can only give general advice.

First of all the general FAQ I previously quoted on accuracy is important. I would not have quoted it otherwise. If you have not done a sensitivity check on your mesh size, convergence and time step size (if transient) then you are just guessing.

Once that is complete you need to consider the key physics. The biggest issue I see here is the Spalart-Allmaras turbulence model. While you say other authors have had good results with SA, this may have been due to luck rather than its inherent qualities. In fact stall prediction is a challenging topic for any turbulence model. I recommend trying a more sophisticated model such as SST, but you may have to advance to DES and SAS family of models to correctly predict this.

Thanks again for the reply. Indeed, i also think that i can improve my simulation approach, e.g. Make a complete grid independence stufy, etc.

Originally Posted by Achilleas

I can not understand a lot from this picture but, as I see, you may have problems with the aspect ratio if you use a y+=1. Furthermore, the skewness of the cells in the leading edge may be problematic. If you also comment about your numerical set-up it would be easier to discuss some things.

I have posted two messages but for some reason only the one with only the mesh picture was uploaded. In the other message i tried to reply with all the info you requested (also attaching pictures), is a long message to be honest. I was waiting to see if it gets uploaded within a couple of minutes but i guess i will have to upload it again...

[Achilleas]

First of all, your results are really satisfactory.

Usually the turbulence length scale is defined as 7-10% of the reference length. So, a value of 0.0125m would be more reliable. I don't believe that your results will change dramatically though.

1) Your numerical set-up seems good to me, including that you considered an incompressible approach. The way that you initialise your solution is also a good one. The convergence check also reveals a good way of handling.

2)3) Your average skewness is too high. It would be good to improve the quality of the corresponding cells, if it is possible. I know that it is also really difficult to improve the aspect ratio at such dense meshes but you can try. However, from my experience, FLUENT can handle many things. So, if you don't have time it shouldn't be a problem for this solver, as you get good results.

Notes:

1) I do not believe that there will be a problem if you change turbulence model and initialise with the results of a previous solution calculated with the use of another turbulence model. I never tried this to be honest.

Additional notes:

*** As I remember, some authors used one rotating domain but I do not remember the accuracy of their results. However, I think that it is better to have 3 different cell zones. From a physical point of view this treatment is the correct one for me. You can just do your rotating domain larger if you want, but I would stay with the 3 separated domains.

*** I think that the results which were posted by me have been calculated with a compressible solver. I don't remember if I had the same separation area when I used the same incompressible solver as you. If I understood correctly your question, I think that the length of your rotor zone shouldn't affect the flow. The boundary conditions should work for ensuring the accurate computations. Unfortunately I am not able to remember my set up but I had posted a picture illustrates my boundary conditions.

*** I remember this note of some authors. For the history, I emailed some of the authors that achieved so good matching of the experimental results, but I never got a reply. So, I would suggest to you to mainly trust the experimental results for your validation.

To conclude, I see that you tried many things and your set-up seems logical to me. My advise is to improve your mesh quality as a first step. I had also tried many things on this problem and my results were similar with yours. Finally, I didn't have enough time and I considered that my results are correct until the first drop of the torque.


Kind regards