solution "converged" but I doubt it.
 

Hi!

I'm quite new to Fluent and i'm working on a simple 2D airfoil to get familiar with fluent.

for small angles of attack everything goes fine, and the results look good. The problem is that for larger angles of attack the drag becomes too large.

Also after 600 iterations Fluent said the solution was converged however i thought there still were quite large osscilations in the drag coefficient. So i'm not convinced it really is converged.
These are the last couple lines from the log: (i'm very sorry i did not manage to align the labels and the values corectly, but the second to last collumn is the drag which interests me the most.)
iter continuity x-velocity y-velocity k omega Cm-1 Cl-1 Cd-1 time/iter
604 1.0310e-03 2.1044e-06 2.5835e-07 2.7216e-04 6.7361e-06 -1.5131e-02 1.3867e+00 4.0607e-02 1:13:07 4417
605 1.0290e-03 2.1021e-06 2.5775e-07 2.7146e-04 6.7220e-06 -1.5194e-02 1.3865e+00 4.0575e-02 1:13:12 4416
606 1.0246e-03 2.0994e-06 2.5785e-07 2.7075e-04 6.6806e-06 -1.5258e-02 1.3863e+00 4.0543e-02 1:13:16 4415
607 1.0246e-03 2.0986e-06 2.5755e-07 2.7006e-04 6.6923e-06 -1.5323e-02 1.3861e+00 4.0510e-02 1:13:19 4414
608 1.0138e-03 2.0973e-06 2.5774e-07 2.6937e-04 6.6589e-06 -1.5389e-02 1.3859e+00 4.0476e-02 1:13:21 4413
609 1.0080e-03 2.0966e-06 2.5761e-07 2.6869e-04 6.6472e-06 -1.5454e-02 1.3857e+00 4.0442e-02 1:13:22 4412
610 1.0122e-03 2.0951e-06 2.5802e-07 2.6801e-04 6.6054e-06 -1.5520e-02 1.3855e+00 4.0409e-02 1:13:23 4411
611 1.0120e-03 2.0942e-06 2.5796e-07 2.6734e-04 6.6152e-06 -1.5587e-02 1.3853e+00 4.0375e-02 1:13:24 4410
612 1.0052e-03 2.0921e-06 2.5820e-07 2.6667e-04 6.5827e-06 -1.5654e-02 1.3851e+00 4.0341e-02 1:13:24 4409
613 1.0003e-03 2.0908e-06 2.5807e-07 2.6600e-04 6.5734e-06 -1.5721e-02 1.3849e+00 4.0307e-02 1:13:24 4408
! 614 solution is converged
614 9.9645e-04 2.0887e-06 2.5834e-07 2.6534e-04 6.5328e-06 -1.5789e-02 1.3847e+00 4.0272e-02 1:13:24 4407

Furthermore i'm using the k-omega SST model (which you might have seen from the log) and as solver is just use the SIMPLE one.

The Cd of 4.0272e-2 that is calculated is at least twice as large as i expect it to be (around 2e-2).

If someone can help me out with this i will be very grateful!
and if you have any questions which could help you to better understand my problem dont hesitate to ask!

Kind regards,
Jasper

Did you read the text on judging convergence in the FLUENT manual, or the guidelines that should be somewhere on this forum as a sticky?

The main message is, be careful when using residuals to judge convergence, as amount the residuals can decrease very much depends on your initial guesses and problem. In fact, I'd say to never judge convergence based on residuals. Always base convergence on whether or not the quantities of interest - such as drag here - reach a steady value (say, fluctuate less than 1% or so). It seems this is not the case, so tighten your convergence criteria, for example by setting the desired residuals to 10^-5 or decoupling convergence from residuals completely by setting different convergence monitors in the monitor tab.

Furthermore, convergence does not mean correctness. Even if the solution converges it may still be wrong - maybe the turbulence model is not applicable for the situation, maybe the mesh is too crude. I'm not an aerodynamics guy so I am not very up to date on the best practice guidelines for wing modeling.

Anyway, make sure that all your discretizations are at least second order accurate. Furthermore, I can imagine that resolving the flow around the foil accurately is important to get a good value of the drag on an airfoil, and as far as I know the SST model switches to accurate resolution of the boundary layers if y+ < 1, so make sure your mesh close to the foil is fine enough to meet that criterion.

Under Solution -> Monitors -> Residuals (click Edit) -> Convergence Criterion (right corner) put "none" instead of absolute or you can untick some options or decrease their value for convergence (continuity, xyz velocities, k, epsilon etc.. depending on your model).

What I usually do is put none, then create Cd, Cl or some other monitors, volumetric flow through a known surface, velocity or pressure at some point behind/in front of an object etc.. the more convergence monitors the better. Then just keep staring at those until you see realistic convergence of those values. Once I've determined that let's say x number of iterations is enough, then I usually iterate to that number for meshes/cases of similar quality or properties.

As you can see even for the latest 10 iterations the residuals are still changing in a quite large amount. So it is definitely not converged to a good amount. what you can do is go to monitors and in residuals and uncheck absolute convergence box. So the residuals can go down as much as it need to and manually you observe when the residuals stop to change at all. at that point the convergence is achieved to a suitable level.

Further issues with Cd value comes from meshing method used, mesh amount, Y+ , amount of boundary layers used and flow conditions.

Allright, thanks for the responses and it sounds like some good advice!
However i'm not near the computer i run fluent on so i will try it tomorrow...
Furthermore I am certain that I need to use a turbulence model and a professor advised k-omega SST and my y+ value is also correct, so that will not be the issue I think. But changing the convergence criterion sound like the solution I need!

thanks again, and I will try tomorrow!