how to calculate mean value of lift and drag
 

Hello all....
if i am running unsteady simulation, i will get values of lift and drag that will show time periodic curve when the solution is converged. How can i precisely get the mean value of lift and drag from this converged solution...

one cl curve is attached. this curve is showing time periodic convergence from flow time of 40 and onwards. now how can i calculate mean value from it in FLUENT

hi there,,
this is not a proper way but, anyways, you can do it and you can present it unless you come up with a more elegant way.

You can export the data for the lift coefficient in an excel spreadsheet, isolate the values for which the simulation has "converged" and get an average value...

if you can get Fluent to plot Cl with time or if you can export your data to Matlab, then you can say
mean Cf = (1/t)*integral(Cl*dt)
where t is the total time you want to take into account, i.e. the time for which the periodic behaviour of Cl is fairly steady.

But anyways, beware!! why do you really want the average Cl in an unsteady problem? are you sure it makes sense?? I presume you can always run a steady flow simulation just to get these notional values even though your problem is unsteady essentially.

Hi pano.....
thanks for the reply...... your suggestions regarding the use of excel or matlab seems valid.
but i didn't understand how can i get these values from a steady simulation. i am in search of one specific value so that i can compare it with my experimental data... in my case, if i run the problem for steady case, it doesnt converge to give me a straight line either for Cl or for Cd. so then, how can i find the value through steady simulation....

In the initial time, there may be some transients. Choose some t0 so that for t > t0, the Cd seems periodic. If you have data until time T, then compute an average as



Alternately you can also do a fourier transform and the constant term in the fourier expansion will be the time average value.

Dear Aamer,
so, actually praveen wrote down the formula properly.

Anyways, what I understand is that you would prefer to run a steaty flow time simulation but you haven't managed to get it to converge. There are plenty of reasons for this.

I dont know if you are using a specific turbulence model or if your problem is set in laminar flow. The best check is to set laminar flow or even inviscid (no matter what your problem says) to see what happens. If this doesnt converge under these settings it's very unlikely (but not impossible) that it will converge for tubulent flow.

In the case laminar flow does not converge, go back and check carefully your mesh. There are different aspects that you can assess the quality of you mesh on; equisize skew, aspect ratio, location of max area cell and many more. Try to improve it as much as possible. By improving, I dont mean you make it more dense!!! this usually makes matters worse. Try to get the best quality mesh in the most interesting areas with as much coarse a grid as possible.
You can also check your grid in Fluent, make the reorder and see if the bandwidth gets reduced by a big proportion, then it means that you can further improve the grid. Check for negative volumes, for left-handed cells and make the smooth/swap.
Check your reference values and if that gives you something, then move to turbulence model, choose the one that is going faster, typically the one equation S-A to start with.

I dont know how the geometry is and what the reynolds and mach numbers are like, but convergence is a fairly common issue and you will find a lot of sources to read. In the end you can improve convergence by a grid sensitivity study (i.e. how the quality of your mesh affects the final results). To this end, use the postprocessing tools in Fluent, such as adapting y*

take care, Pano

Dear Pano...
your comments on the subject were very helpful. i am actually validating experimental results of corrugated airfoil at reynolds number of 34000. my case is inherently unsteady and turbulent. but i still started with laminar to check how my simulation goes. the solution was not converging with steady runs. but when i switched to SA model, the solution started to converge for low angles of attack with steady runs, but the solution was not converging for higher angles of attack due to flow separation from the surface. so i had to switch to unsteady calculations. as far as rechecking of mesh is concerned, i am already onto it...... :)

Dear Pano.....
i am getting correct Cd values for almost all angles of attack but i am getting slightly higher Cl than the experimental values . For example at 5 degree angle of attack, experimental Cl is 0.43-0.46 but my computational value is 0.55. What all things to look for, if you are getting correct values of drag Cd but higher values of lift Cl.

Dear friend,,
I am also trying to catch up with the new post of yours on this topic, so I might accidentally be saying more things here at once.

Firstly, as you said the discrepancies in lift coefficient are not terribly big. That said, you may have a biased approach by mistake. Since this is an airfoil, you might want to put more emphasis on the ratio Cl/Cd rather than on the explicit values of each coefficient. That means you can afford to lose some accuracy on the Cd provided that doing so, Cl improves in such a manner that the Cl/Cd ratio improves significantly as this is more important in the end of the day.

Myself, I had the opposite problem, CFD gave me terribly small lift coefficents whereas the drag coefficient was indeed accurate. Because I was dealing with symmetrical foils, I had the luxury of not paying much attention on the lift coefficient varying with AOA as I was only interested in 0 AOA. All this, provided that the error was consistent in all cases examined for verification purposes, i.e. in all foils and conditions examined to simulate the experiment conditions.

Boundaries: I think in the other post, you mentioned 10c tolerances in all directions, that should be more than enough to consider them as symmetry farfields and I think that you'd better define the back boundary as pressure outlet.

Type of grid: My understanding is that to maintain the accuracy of the turbulence model, it is preferable to use C-type block-structured grid which would enable the distinction of the different zones; one zone would embrace the leading edge until roughly the point of transition, then the rest of the foil will be in a fully developed turbulent flow regime. block-structured grid is a pain in the ass to get it nice but it might be worth it.

Near-Wall treatment: I also understand that you have now checked the wall y+ and so on. In addition to that, try alternative ways of dealing with the near-wall treatment using wall functions (instead of near-wall modelling you are probably using right now), these will do better if you have extensive regions where viscosity predominates. With S-A model of course you cant have wall functions, you can only make UDFs which I can't comment on because I havent done it myself. S-A and κ-ω models typically work with near-wall treatment, whereas k-e employs wall functions.

I dont know how long your project is and how much time you have at your disposal, but dont spend your life trying to get the best results, go on with your study unless the extreme precision is itself your ultimate goal. Everybody understands discrepancies (of this magnitude at least) and if you prove you have a consistent error in different cases, then that's a vary formal way of saying, right, I am done with verification, I am moving on. Finally, I know it's the experimental results you're trying to match but how about considering results from algorithms like Xfoil, Aerofoil (if they can actually be applied in your case - I dont know)
Take care, Pano

Just wondering can any one tell me how to do the fourier transform to get the average, amplitude and phase ? Can any one provide me any references?

I will appreciate any help.

Thanks,
Shafi

Dear Pano...
thanks for enlightening me on the subject with very relevant technical details. Most of the things that you have asked me to try have already been done, like , change of boundries (i have tried both outflow and pressure outlet), wall treatment i.e the use of wall functions with K-e model, type of grid (2 different type of grids have been tested, although both were o type) but as i have to proceed to 3D later, so i foresee terrible problems if i go for C-type grid, so i am avoiding that. the values remain the same more or less.
Honestly speaking, i dont have any idea about algos like Xfoils, i will look into that. by the way, my airfoil is not a conventional one, it has corrugations on the surface like that of a dragonfly wing.