2D airfoil flow problem
 

Hi guys,
i'm working on my thesis which consist in study the flow past a pitching airfoil NACA 0015 at Re 1.5e6 focusing on the transition and vortex shedding. Before i do that i run some steady and then transient simulations for the AoA between 1 and 23 to validate my mesh. The cord length is of 0.5459m, i'm using a duoble O-mesh with the external circumference of 40m radius while is the internal of 2m. I'm interested in study the transition so i use 1600 point on the airfoil which are thickened on the leading edge and the trailing edge and an inflation of 32 level with first cells height of 8*10e-6 and a growth rate of 1.1. The external mesh is structured while the internal is unstructured and the circumference are divided with 280 points. I check my quality and seems to be good, my teacher thinks is good too.


Steady:

In fluent i set pressure-far-field for the external vicumference as b.c., SST Transition (4 eq) as viscous model and SIMPLE + second order discretization. I run over 30000 iteration for every AoA.



The problem is:

my Cl and Cd are good, in agreement with other simulation and the experimental data, contours are good too, but if i look at pathlines there are some vortices in the pressure side for the AoA 5:11 and we don't know the reason!

I try to modify the mesh but it doesn't work, so i change the scheme and with SIMPLEC is the same while with PISO they disappear. The problem with PISO is that the lift coefficient is too small. So i use again SIMPLEC and i set adaptive mesh based on iso-values of vorticity, FLUENT create a mesh with over 1 milions cells and of course it take too much time.
At that point i switch to the transient one thinking that it was a problem of the stady state simulation.



Transient:
time step size of 0.001s and over 7000 time step. I use PISO and second order implicit for time discretization. I run at 11 AoA and the problem is now in on the suction side because there are zones in which velocity became of 0.5 Mach. I don't know if it is right so i try to switch to SIMPLEC and set the time step to 1e-5 for try. The vortices are disappeared, the pathlines and the contours are good so as the lift coef. but the time step is too small and i have to simulate about 8s.

Reading on the forum i discovered that Coupled scheme is better when the time step is large and so i do. He provide the same results of SIMPLEC.
When i switch to 9 AoA the Coupled scheme doesn't work anymore and now i run one with SIMPLEC and time step of 0.0001. Tomorrow i'm going to check what happen.


My questions are:
1. Why there are vortices on the pressure side?
2. Why the flow field is deeply influenced by the scheme and give me different solution?
3. Do you have any suggest to improve my simulations?



I made geometry and mesh in workbench.
Sorry for my english guys, i hope you will undestand the problem. Any suggest and tip will be appreciated.


Thanks for your attention.

Time-step is important
 

Hi Mike

Time-step is important. 1 ms appears to be large to me. I am not sure what velocity you have. But you have to ensure that cell Courant number is limited to 1. Schemes are not important as long as you get convergence, however, they do affect the number of iterations. Coupled is alright as long as pressure and velocity are tightly coupled, which is the case for compressible flows. But even SIMPLEC is alright if it converges. And for flows that have no multiphase or reactions, SIMPLEC is good. You have to keep time-step small enough so as to ensure that the convergence is achieved within every time-step. It does not mean you can use 100 iterations per time-step. That will deliver unexpected outcome. And prefer bounded second-order for temporal discretization.

SST transition model is meant to be used if objective is to predict the point of onset of turbulence. If that is not the objective you may use SST k-.

If you wish to run it as steady-state, then use either of the schemes but ensure that you achieve a deep convergence. Most of the the times, this can be achieved by running with first-order schemes for first 500 iterations to develop a better initial field and then switching to higher-order schemes. To develop better initial field, FMG initialization also helps. If FMG initialization fails, then there is something wrong with your setup. So, it is actually a good test of setup.

Hi Vinerm,
thanks for the answer.


Yes, my object is to study the transition of the boundary layer and i hae to use SST transition.
For steady-state simulation, today i found that the problem of the recirculation zones on the pressure side dissapear if i use for the moment equation a first-order spatial discretization. The lift and drag curves are bettere and more stable. As soon i switch to the second order, some vortices appear in the pressure side.



Do you think it's a grid problem?



My freestream velocity is 41.511m/s.

Mesh appears to be alright
 

I do not think that mesh is the problem, provided you have enough cell along the length. First-order appears to be stable because it has very high numerical diffusion. This diffuses the vortices over the space. It is quite possible that vortices are real and are supposed to be there. However, if that is the case, then case has to be run transient.

Furthermore, check the y+ for the mesh on airfoil boundary as well as cell Courant number.

My y+ was good even if i had that pathlines. I don't know if that vortices are real because if i use different scheme, pathlines change. Also, for what i know about flows over arifoils, the recirculation zone appears on the suction side because pressure increase in the flow direction. The question is that i have this "problem" only for AoA between 5 and 11, for AoA of 12 the recirculation zone is on the s.s. and the flow on the pressure side is laminar.

Turbulence model
 

Then, quite possibly, issue is with the turbulence model. I would doubt that it is due to the the model not being Galilean invariant, however, I would suggest trying the Intermittency Transition model, at least for the cases where you see the vortices on the pressure side.

Do you think it could be due to the boundary condition for turbulence? i set:
intermittecny = 0
turbulent intensity = 0.1
turbulent viscosity ratio = 0.1


ForIntermittency transition model you mean SST Transition right?

It's different
 

SST-Transition model is a 4-equation model. Intermittency transition model is different and uses only 3-equations. You have to choose k- and then choose transition model under options. Boundary conditions look alright. In case you do not observe any transition to turbulence, try with a slightly increased intensity and viscosity ratio at the inlet.