## Wind tunnel modelling, BCs and convergence issues

Questions and remarks about code_saturne usage
Forum rules
Please read the forum usage recommendations before posting.
Emonet_L
Posts: 7
Joined: Fri Mar 01, 2019 10:58 am

### Wind tunnel modelling, BCs and convergence issues

Hello,

I am working on a wind tunnel for which I set some Inlet, Outlet, Wall and Symmetry BCs. To avoid modelling the fan, I would like to assign an Inlet BC with a negative volumic flow rate to my outlet (I am not sure it is the more relevant solution).
Besides, I have assigned the same value of volumic flow rate at the inlet because my real system is closed, it seems to me a good way to preserve continuity.

After starting steady calculation, I have an error that I can't figure out.

I don't know if the problem comes from the BC definition or something else so I tried another modelling where I changed the geometry to have both Inlet and Outlet almost at the same location (Outer annular duct, see attached for more info). That way allows me to assign the same velocity (less physically representative of the fan but better than nothing) to each BC (from 1 to 10 m/s).

This solution worked and seems to converge after thousands of iterations but the residuals are way too high !

For the two calculations, I followed the advice from Antech:
viewtopic.php?f=2&t=2445&p=13435&hilit= ... nce#p13435
- SIMPLEC algorithm
- Least squares method over partial extended cell neighbourhood
- Reference time-step = 1e-3 or 1e-4 s; Max CFL = 5; Max Fourier = 10;
Min time-step factor = 1e-3; Max time-step factor = 100; time-step variation = 0.1
- First computation with Upwind convective scheme for all variables, Restart SOLU with 0.8
blend for Velocity and Upwind for other variables, Restart SOLU for Velocity and Upwind for
other variables

1st questions: Can you please tell me what is wrong with my first modelling? Is this a BC problem or something else?

2nd questions: Is there any way to obtain lower values of residuals? Maybe a thinner mesh (combined with a Low Reynolds model?)? Can you give me (if a general definition exists) a limit range not to exceed to be sure that the solution is accurate enough?

For now I use Code_Saturne 5.0.9 on Windows10 x64, only with the GUI.
The final purpose will be to add an obstacle of more or less complex geometry.

I hope I am clear enough, please find attached details of the two computations (listing, mesh, xml, etc...). Please tell me if you need other file/data/information to understand my issue.

Thank you.

Best regards,

Luc
Attachments
Wind_tunnel.zip

Emonet_L
Posts: 7
Joined: Fri Mar 01, 2019 10:58 am

### Re: Wind tunnel modelling, BCs and convergence issues

My bad ! I made a mistake when I modified the mesh from a previous one for the Vflow BC modelling !

I deleted a surface and now the computation is running ! (see attached for the new mesh that is still very coarse)

Forget about the previous "1st questions", but if it is not bothering you can you give me your advice anyway?

I still need to know more about "2nd questions" related to convergence, residuals and SIMPLE-like solvers.

Sorry for the mistake and thank you in advance.

Best regards,

Luc
Attachments
Sans_solide_BC_Vflow.cgns

Luciano Garelli
Posts: 240
Joined: Fri Dec 04, 2015 1:42 pm

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

Looking at you mesh, I think that you should try with a finner mesh, because in the outer annulus you only have 2 cell in the radial direction. Also, you can to try to created a mesh of hexa, this will help to reduce the residual and the convergence.

Regards,

Luciano

Antech
Posts: 126
Joined: Wed Jun 10, 2015 10:02 am

### Re: Wind tunnel modelling, BCs and convergence issues

Emonet_L
Hello.
In our practice (aerodynamics), we usually don't get residuals as low as 10^-4 or so. They may oscillate around 10^-3 asympote or even be higher. The other thing is that residuals may lay already oscillate around their asymptotes and be not too high while solution is not actually converged. From these observations I derived that residual monitoring is not the way to go in real life. I don't even say about cases with shedding vortexes past the obstacles etc. when they are solved in static. So I use another approach. First, I look at the number of iterations (for example, in Saturne, I do at least ~300 iterations for most cases and 1000...3000 iterations when there are swirling flows and RSM). Second, I check the flow (velocity/pressure fields) in Catalyst in ParaView. In CFX (that is my primary tool at work now), I set some monitors, for example, for the inlet average pressure, maximum velocity, average pressure/velocity/temperature at some characteristic location e.t.c. (it's easy in CFX with it's GUI and mesh analysing/access features, but it has no Catalyst in our versions, newer ones are very expensive for the company). There are monitors in Saturne but I don't know if it can monitor quantities averaged over surfaces or volumes via GUI. These averaged and maximum values-of-interest monitoring is very important for solution convergence estimation, IMHO.

Regarding the mesh. It all depends on what you want to get from the simulation. If you only need the outer annular region to pass the air through it, you may stay with these just 2 cell in radial direction or even exclude this region. In the mein volume, there will be the geometry of the thing being tested so the mesh will be different anyway.

Regarding BCs. I would just set the inlet velocity and pressure outlet with zero static pressure. You don't need to set the outlet flow rate, it will follow the continuity. But, if the velocity/pressure field at the tunnel inlet is sufficiently irregular, the best way is to introduce the blower (I don't know if the rotor/stator setting is difficult in Saturn). If you just set the inlet velocity profile, you will be unable to set the pressure profile at the same BC (in any code), that may easily lead in non-physical flow field at the inlet. You will need the blower or some emulation of it to obtain an acceptable inlet flow field. (In CFX you just need to set the rotating domain and one option at the interface + use dynamic approach [time step for such velocities may be as high as 0.01 s] but, in Saturne, I'm not sure that it will be stable in dynamics with large timesteps).

Yvan Fournier
Posts: 3078
Joined: Mon Feb 20, 2012 3:25 pm

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

To add to the previous post, yes, monitors in Code_Saturne are usable for time averages of volume fields, including from the GUI. Surface monitors are available also but not yet from the GUI.

For convergence, a rule of thumb which was quoted quite some years ago for unsteady computations was to run enought time steps for 2 full passages through the domain. But in some geometries, this is probably overkill, so I concur that placing monitors at various points (near the inlets, outlets, and at a few other locations) and checking that all seem stabilized (or exhibit small fluctuations with a stable mean) remains the most efficient and reliable method.

Best regards,

Yvan

Emonet_L
Posts: 7
Joined: Fri Mar 01, 2019 10:58 am

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

First, thank you very much for all your clear answers.

As you advised me I will explore these trails:
- Thinner mesh with hexa parts where it is possible, tetra otherwise.
- Definition of a fan beyond the outlet, I need to get informations about how to do it with the GUI (I guess in C_S documentations) because it is still unclear for me but seems to be more "realistic".
Otherwise, I hope simple BCs like Velocity Inlet and Static Pressure Outlet will be sufficient.

I think I am now aware of convergence quality criterions thanks to your recommendations.

Best regards,

Luc

Emonet_L
Posts: 7
Joined: Fri Mar 01, 2019 10:58 am

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

I have a few more questions about the fan subpanel in Code_Saturne 5.0, I would be glad if someone aware of it could help me.

First, I wonder if I have to define another cell-zone just for the fan? Because when I add a fan definition the "zone id" is automatically "0" and I am not sure if I need to change this value or if it is a nomal default value.

Then, I am not sure of the values I have to write in "Inlet axis" and "Outlet axis" options, it says that the vector does not need to be normalized. So I do not care about the values? I just have to define the orientation with random numbers?

Finally, Do you know if the fan modelling can have an influence on the stability and/or the accuracy of the results? Because I want to be more realistic but I am not sure it is worth.

Thank you in advance.

Best regards,

Luc

Yvan Fournier
Posts: 3078
Joined: Mon Feb 20, 2012 3:25 pm

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

No, you do not need to define another cell zone. The fan definition array label should be "Fan id" and not "Zone id" (I'lll fix it in version 6.0.

I do not remember about the normalization, but if in doubt, check with 2 different vector lengths.

The fan modeling will behave as an explicit velocity/pressure source term if I am correct (It would be safe to check), so its influence on the stability will be as such.

Best regards,

Yvan

Emonet_L
Posts: 7
Joined: Fri Mar 01, 2019 10:58 am

### Re: Wind tunnel modelling, BCs and convergence issues

Hello Yvan,

Thank you very much for your help and explanations, it should be clear to me now !
I checked and the coordinates seems to correspond to the location of the axis' origin.

If I am write, it is only possible to define one Outlet axis, isn't it? Because for my study, the air enters the fan axialy and leaves radialy all around of it, I do not know how to deal with it through the GUI.

Do you know if it would be possible to model this kind of blower? Maybe in a future version?

Best regards,

Luc

Yvan Fournier
Posts: 3078
Joined: Mon Feb 20, 2012 3:25 pm

### Re: Wind tunnel modelling, BCs and convergence issues

Hello,

Yes, the fan model you can define with the GUI only includes "axial" fans (it was initially written for fans forcing convection in cooling towers).

If your fan model is more complex, you would need to check if you can simulate it using an appropriate source term (probably, but I assume you also need a boundary/wall on one side).

The main examples I know of with flow entering axially and leaving radially are some pump designs, which we usually simulate using the turbomachinery rotor/stator feature (but this leads to a much more detailed mesh and costly computation, not a simplified source-term based model).

Regards,

Yvan