[MaherEid]

Hello all,

I am running LES simulations for a wind turbine on Fluent with the recommended schemes and settings. At low TSRs my solutions perfectly match the experimental data (Moment coefficient curve Cm vs TSR). At high TSRs or when the expected Cm should be maximum, I keep getting low values for Cm (sometimes as half as it should be).
I tried reducing time step, mesh size, residuals conditions but nothing seems to help.

I would like to know if anybody might have encountered this problem and potentially has a fix for that. Also any idea to try would be great.

Note:
Model: Smagorinski-Lily (dynamic stress)
Y+ does not exceed 0.4

Thanks!

[vinerm]

I am assuming that you are using references values corresponding to high TSR. LES is essentially high-Re number modeling approach and not really good near the walls. With such a fine mesh, which I suppose is maintained at high as well as low TSR, you should use WALE to improve shear stress predictions on the wall. Since is directly related to that, this might improve the result.

[MaherEid]

Originally Posted by vinerm

I am assuming that you are using references values corresponding to high TSR. LES is essentially high-Re number modeling approach and not really good near the walls. With such a fine mesh, which I suppose is maintained at high as well as low TSR, you should use WALE to improve shear stress predictions on the wall. Since is directly related to that, this might improve the result.

Hey
Really appreciate your help,

I tried WALE as you suggested, but the solution did not change (average solution at least). I tried the same case with WMLES and DDES (k-w) but the forces in both cases almost decreased by 50% compared to the previous ones.

I am not really into turbulence modelling (specially LES), but is there anything else I am missing ?

[vinerm]

Do you have a reference or theory that says that a high is expected at high TSR? Is there any critical limit beyond which it might rather reduce, because it is possible.

[MaherEid]

Originally Posted by vinerm

Do you have a reference or theory that says that a high is expected at high TSR? Is there any critical limit beyond which it might rather reduce, because it is possible.

Yes I am comparing my results with experimental data.
I am now considering that the problem is not with the model, but with the solver.

I did the same case in 2 methods:
Blue: Simple Algorithm
Black: Coupled (Courant = 0.8)
(Same model, same initial solution, same time step size ...)

The Simple takes 4-5 iterations per time step while the coupled only 1. The weird thing is that if I reduce the residual criteria in any solver the forces changes suddenly. Can the residual criteria have an impact on this, and is there any value i should consider for the Moment Coefficient residual value?

Thanks

IMG_0589.jpg

[vinerm]

The criterion set for a particular residual can affect the solution only in one manner; by allowing to solver to cut-off or reach a particular depth of residual. E.g., if user sets a criterion as 1e-4, and solver reaches 1e-4 in 5 iterations, then it won't go deeper but if it is set as 1e-6 and the solver takes 10 iterations to reach there, then next iteration will have a slightly better guess. However, the difference is significant only when the convergence is not good. For your case prefer Coupled. Secondly, since coupled and SIMPLE are very different, the solver treats them differently, i.e., the multigrid solver sweeps are different for both. Hence, you will observe difference in the way you reach solution. But once converged, the solutions should be close. However, there has been incidences where SIMPLE never converged, particularly for rotating machines. Coupled, psuedo-transient is the method of choice for rotating machines. Another aspect could be the gradient scheme. Try using Node based instead of default LSQ based.

[MaherEid]

Originally Posted by vinerm

The criterion set for a particular residual can affect the solution only in one manner; by allowing to solver to cut-off or reach a particular depth of residual. E.g., if user sets a criterion as 1e-4, and solver reaches 1e-4 in 5 iterations, then it won't go deeper but if it is set as 1e-6 and the solver takes 10 iterations to reach there, then next iteration will have a slightly better guess. However, the difference is significant only when the convergence is not good. For your case prefer Coupled. Secondly, since coupled and SIMPLE are very different, the solver treats them differently, i.e., the multigrid solver sweeps are different for both. Hence, you will observe difference in the way you reach solution. But once converged, the solutions should be close. However, there has been incidences where SIMPLE never converged, particularly for rotating machines. Coupled, psuedo-transient is the method of choice for rotating machines. Another aspect could be the gradient scheme. Try using Node based instead of default LSQ based.

I am using absolute residuals (1e-3) but the coupled solver reaches as low as 2e-4 in its one iteration per time step. Should I monitor reisduals of Moment coefficient as well, or is the convergence of momentum and continuity enough to ensure the correct values?

And by converged you mean statistically converged (as this is a transient simulation). What's weird to me is that my turbine has 15 blades and the SIMPLE solver (Blue) shows the peaks at every blade, while with the coupled the period is non existent.

[vinerm]

By converged I mean convergence within each time-step. For a transient simulation, fields should converge in each time-step. This is weird that the solve takes only 1 iteration to reach 2e-4. Either your time-step is very very low or there is something wrong with the setup.

[MaherEid]

Originally Posted by vinerm

By converged I mean convergence within each time-step. For a transient simulation, fields should converge in each time-step. This is weird that the solve takes only 1 iteration to reach 2e-4. Either your time-step is very very low or there is something wrong with the setup.

In the coupled it takes only 1. In SIMPLE it is usually 4-5. Well the time step is equivalent to 0.1 degrees. Since this is a LES, I thought I sould decrease the time step size. Is there a way I can know how much to set the time step size?

[vinerm]

Usually, for LES, it is based on frequency. For rotating machine, 0.1 degree is good. Higher would not be preferable.

But, as you mentioned earlier, may be the coefficient has not reached a steady or statistically steady state. Are you monitoring it as the run goes on?

[MaherEid]

Originally Posted by vinerm

Usually, for LES, it is based on frequency. For rotating machine, 0.1 degree is good. Higher would not be preferable.



But, as you mentioned earlier, may be the coefficient has not reached a steady or statistically steady state. Are you monitoring it as the run goes on?

The image I attached earlier(also here), is the moment coefficient. The Blue curve is SIMPLE and Balck curve is coupled. This is around 2 rotations. You can see in the SIMPLE the peaks having the same period (360/15 blades = 24 degrees between each blade). In the coupled there is no period whatsoever.

IMG_0589.jpg

Note that the initial solution for both is the same.

[vinerm]

I'd expect Coupled also to be able to resolve this frequency. It is quite possible that the pressure and velocity for this case are not tightly coupled, though if the system is compressible then this would not be the case. However, if it is not compressible, then prefer using SIMPLE. For flows that do not have a tight coupling between pressure and velocity, SIMPLE or SIMPLEC work better and faster.

[MaherEid]

Originally Posted by vinerm

I'd expect Coupled also to be able to resolve this frequency. It is quite possible that the pressure and velocity for this case are not tightly coupled, though if the system is compressible then this would not be the case. However, if it is not compressible, then prefer using SIMPLE. For flows that do not have a tight coupling between pressure and velocity, SIMPLE or SIMPLEC work better and faster.

What I suspect being the problem is the residuals and when to cut off the time-step. I have been experimenting with it today and I attached 2 pictures here.
In the console image, you can see how the Cm changes within 1 time-step eventhough continuity residuals are already in the e-4 order. If I use the default criteria the time step would have cut off before Cm has converged.
When I reduced the criteria to e-5 for continuity the Cm spiked and the curve has gone in a totally different direction. Do you think that is the problem and do you have any suggestion?

Thank you so much for your help

IMG_0613.jpg
IMG_0612.jpg

[Mutlaq]

Hi Mr.vinerm
I need your Advice in the LES convergence

[vinerm]

What help do you need?

[Mutlaq]

my simulation is LES of flow inside a rectangular tube (water)

I am a beginner in the ِAnsys program. I did 200 simulations to learn about the program
But when I use the LES method the convergence appears like this way, I don’t know if I’m doing it right or not

[vinerm]

I suppose you forgot to attach an image.

[Mutlaq]

https://drive.google.com/file/d/1ysB...J7OgJzG7e/view
this is a picture
No I did not forget but I do not know why did not appear here

[vinerm]

As far as residuals are concerned, those are alright. However, you should monitor some field quantities, such as, velocity, pressure, etc. to confirm convergence.

[Mutlaq]

thank you. Can I ask you at another time if you do not mind?