[linyx]

Hi Everybody, I have a problem in Fluent and I hope you guys can help me out

When i was calculating the maximim lift of wings in fluent, I find that the maximum lift depend on the initial condition. When the initial condtion is the inlet velocity boundary condtion,then after iteration, the lift of a certain angle, for example, 20, is very low, and the flow shows that the wing is stalled.

However, when the initial condition is the last time calcution result, for example, 18 degree of attack,where the flow is attached, then the iteration result of 20 degrees shows that the flow is still attached.

what's more, if initial conditon is changed, for example the result of 15 degree of attack, the 20 degrees result is diffrent from the former one.

What i am interested is the maximun lift and drag at critical angle, so these changeable results really make me puzzled, which result should i trust?


Ps: I know there is a Hysteresis phenomenon in wing aerodynamic around critical angles, but my simulation is not dynamic nor unsteady, I just change the boundary condtion or rotate the mesh to change the angle, I think it won't be the explanation to my problem.

[Aeronautics El. K.]

What are the convergence criteria that you are using?

[linyx]

Originally Posted by Aeronautics El. K.

What are the convergence criteria that you are using?

I use the steady solver, so the convergent criteria is the lift coefficient never changed with iteration, and the residual goes flat

[Aeronautics El. K.]

Originally Posted by linyx

I use the steady solver, so the convergent criteria is the lift coefficient never changed with iteration, and the residual goes flat

Very precise...

When the wing is stalled, do you expect the pressure distribution to be same over time?
If you consider what is happening at stall, you'll understand why the residuals will never "go flat".
What I would expect would be some periodicity in the manner the residuals will be fluctuating.

[linyx]

Originally Posted by Aeronautics El. K.

Very precise...

When the wing is stalled, do you expect the pressure distribution to be same over time?
If you consider what is happening at stall, you'll understand why the residuals will never "go flat".
What I would expect would be some periodicity in the manner the residuals will be fluctuating.

You are right, the stall always envolves some periodic or unsteady motion,.

When I was simutating the 2d airfoils at high angles of attack, it was flunctuating with residual and lift.

This time I am simulating the 3d rectangular wings with aspect ratio of 1.25, using SA turbulence model, the lift goes surprisingly convergence to a value and residuals do not fluntuate even at stalling anlge.

My point is, why at high angles of attack, lift value is not the same under differnt initial conditions, it really makes me hard to decide, since I am intersted in maximum lift. Does it have anything to do with Hysteresis phenomenon near the stalling angles?

[Aeronautics El. K.]

For entertaining and educational reasons I tried a similar problem myself! lol
I attach a picture with the residuals and another one with the streamlines. This is a 2D case however, a NACA 4415 @ 50 degrees. I initialised the flowfield from the inlet.

What I am thinking about your problem is that it hasn't fully converged. How many iterations do you perform?

[linyx]

Originally Posted by Aeronautics El. K.

For entertaining and educational reasons I tried a similar problem myself! lol
I attach a picture with the residuals and another one with the streamlines. This is a 2D case however, a NACA 4415 @ 50 degrees. I initialised the flowfield from the inlet.

What I am thinking about your problem is that it hasn't fully converged. How many iterations do you perform?

I iterated about several thoudsand times, at critical angle of attack, just above or below the stalling angle,the result is not the same depend on the initial conditons even in 2d flows.

Actually my case is a 3d multi-element wings, so it is kind of complicated about the flow. the boundary condtion is velocity inlet and pressure outlet, I wanna know which one should i trust in these various initial conditons.

The attachment is the residual plot and lift plot,the former one is plot of 28 degree initiated on the result of 20 degree, and later one is plot of 28 degree initiated on the result of 25 degree. You can see that the flow is completely different at the same angle of attack

[linyx]

The latter case plot attachment is here

[Aeronautics El. K.]

hmm, if I were you, I'd let them perform the same number of iterations, say 20000.
maybe you should also try a different turbulence model like the sst k-w

[linyx]

You can see the lift coefficient change so little with iterations, So, it would be same no matter how many iterations it has.

the actual model is very large, Sst requires stringent near wall mesh, which is not affordable in 3d in this work station.

[Aeronautics El. K.]

In the second case Cl is changing considerably...
Anyway, it's your project, you decide...

[oj.bulmer]

Looking at your velocity contours, why do I get a feeling that your mesh is coarse? Have you done mesh independence study?

Lefteris is right, the Cl in second case is fluctuating a lot, it is not converged. Also, try using realizable turbulence model and second order discretization scheme. These should reduce the numerical diffusion.

OJ

[Aeronautics El. K.]

I re-run the test case, again for entertaining reasons! :P
This time instead of turbulence intensity 1% and turbulence viscosity ratio of 10 at the inlet, I use a value of 1 for k and w (sst k-w again)... the results are different and (much) better I dare say...

[linyx]

if you carefully observe the cl flunctuation limit, you can see that the cl flunctute between 2.7275~2.7279, which is small enough.

Acutally I have done other simulations through many iterations, the result of 28 degrees from 20 degrees and 25 degrees is converged and different.

I havn't done the mesh indepence study, to be honest. however I think my mesh is fine to resolve the flow, the attachment is my mesh in 2d. Anyway, I would do some independance study to see if this happans again.

Let me make my problem clear, my problem is to calculate the maximum lift of multi-element wings at low speed. I use the SAmodel, pressure based solver, second order in momentum discretinization. If I initiated my case with inlet boundary, the stall angle is 25 degrees. However, if I changed boundary condtions to 28 at the result of 25 degrees, the fluent shows it can still maintain attached flow, however, if I initiated at the inlet of 28 degrees or from the result of 20 degrees, the result then shows the flow is stalled. Further, if I change the boundary condtions from the result of 28 degrees, it seems can get a higher stalling angle.

These problem really makes me puzzled to determine the maximun lift. Does it have sth to do with the Hysteresis phenomenon in wing aerodynamic around stalling angles.

[Aeronautics El. K.]

Whatever your problem is, the real problem is that you insist you are right and you don't take under consideration what other people suggest in order to help you out. It seems as if you just want confirmation that what you do is correct.
Well then... good luck

[linyx]

No, I do not mean it, I just want to make my problem clear to you, so you can detect which one I am making wrong. I do not insisted I am right, I just don't know which step I am taking carelessly.

Well, thank you for your suggestions for recent days, since I am really trapped by this problem recently and get annoyed somehow, sorry if you feel unpleased.

[oj.bulmer]

if you carefully observe the cl flunctuation limit, you can see that the cl flunctute between 2.7275~2.7279, which is small enough.

Yes you are right. I couldn't notice the values on X and Y axis to be honest, and assumed the monitors are for all the run. But they seem to be only for 35 iterations. It is always recommended to show the monitors of all the iterations (or at least last 30% iterations) to make sure they are not changing with iterations. 35 iterations are too small to conclude that

It is strange that your results are too sensitive to the initial conditions. But then I again reiterate the point, if you haven't done mesh independence test, then your results are not credible. I insist you do a mesh independence study and make sure your problems are not related to mesh. You see, the wake of your wings have significant gradients but in that region your mesh is quite coarse. Unless you know it is small enough to capture the flow physics, you can't continue with this mesh.

Spalart Alamaras is a one equation model and only solves Euler equations. You may consider kw SST, which is better for wall bounded flows.

OJ

[Aeronautics El. K.]

Linyx,
I'm neither pleased nor the opposite. I just told you my opinion before that in the second series of photos you posted, the Cl convergence history shows that Cl is still changing which enhances my opinion that the solution has not yet converged.
I don't claim to be an expert here but oj.bulmer told you the same thing as I did so I think you should at least try to let fluent perform more iterations. It would be just a few hours work done by the computer while you'd be enjoying your coffee and no harm done if we're wrong about it...

[linyx]

Hey, I have read some articles and asked some specialist on the forum, It indeed has something to do with Hysteresis phenomenon around the stalling angles, that is, around the stalling angles, the wing has two solutions, by increasing and decreasing angles. the attachment is some pic briefly show the trend.

that somehow explains why i can get two different answers at the same angle of attack, but there is still some bugs in here, and I am gonna dig it out.

[Aeronautics El. K.]

Is the wing pitching up-down and/or plunging?