[artkingjw]

Hi,

I need help with a simulation I'm running on Fluent 2021R1. The problem is a wall bounded flow with boundary conditions pictured in the attachment. The velocity inlet is a simple uniform velocity inlet. The aim at the moment is to get a boundary layer growing at the wall, before I introduce a model into the near wall region at a later stage of the project. As with a usual LES simulation, I've started with a steady state RANS simulation (k-omega SST). The fluid is 'air' set to the compressible 'ideal-gas' density, with Sutherland's law for viscosity. I'm using a pressure based solver



The mesh was generated in Fluent, creating a polyhedral volume mesh. There is an inflation layer growing from the wall at the bottom of the domain.

I'm not sure what I did wrong, but the simulation never seems to work. I've realized that the problem starts with the steady state simulation, which gives a strange solution, even though it does not diverge.

When running the steady state simulation, portions of the 'free stream' region outside the boundary layer accelerate above the inlet velocity specified, while the boundary layer becomes very thin. The steady state simulation also fails to converge after many iterations. The continuity gets close to E-4, but ultimately fluctuates. If I feed this solution into the LES run, the LES will diverge.

If I run the steady simulation for about 1000 iterations or more, the whole domain eventually settles on a similar velocity. I've attached a screenshot to show that it settles to a freestream of ~ 50 m/s, when the inlet was specified at 46 m/s. I'm not sure if feeding this particular solution into LES will cause divergence yet, will find out soon... EDIT: yup it does diverge.



Does anybody have any tips for me? I'm not sure what I've done wrong.

Thanks in advance.

[LoGaL]

What is this “Farfield” you are imposing? Pressure outlet? (That is what I would give there)
And, also, is this a 1 element thick mesh? You won’t run LES with it

[artkingjw]

Originally Posted by LoGaL

What is this “Farfield” you are imposing? Pressure outlet? (That is what I would give there)
And, also, is this a 1 element thick mesh? You won’t run LES with it

Hi thanks for getting back to me.

The 'farfield' BC is the default Fluent Pressure Farfield boundary. I have tried switching it to the 'pressure outlet' BC and it didn't seem to make things better (the steady solution diverged).

The images I've shown are only from the early setup files. I replaced the mesh with something much wider so the spanwise width and element count should not be an issue.

[LoGaL]

Fine.

To be fair, I think it is very difficult to screw the mesh quality with a quadratic domain, so I believe it is not an issue. Would be worthwhile to check it just to be sure.

Only thing It may go wrong with the RANS (which should easily drop to machine level accuracy) is that the periodic BC is somehow screwed. Do you get any warnings about it?

[artkingjw]

Originally Posted by LoGaL

To be fair, I think it is very difficult to screw the mesh quality with a quadratic domain, so I believe it is not an issue. Would be worthwhile to check it just to be sure.

There are a few poor quality mesh elements (Fluent quality of 0.08 or so) within the inflation layer towards the outlet, as the mesh elements start to get bigger and get a little stretched. The problem only starts to appear when I reduce the first element thickness to match y+ within the region of interest.

I've added some attachments to show how I developed the inflation layers on the ground. The ground wall is split into 2, where a uniform inflation (to control 1st element thickness) is set at the upstream portion, and a smooth-transition inflation is used for the downstream portion. Both have the same growth rates. The aim is to increase the size of the elements at the outlet for numerical damping and improved convergence.

Originally Posted by LoGaL

Only thing It may go wrong with the RANS (which should easily drop to machine level accuracy) is that the periodic BC is somehow screwed. Do you get any warnings about it?

Hmm... I didn't get any warnings about the periodic BC. Would Fluent say anything specifically about the periodic BC itself?

I did try using symmetry instead of periodic for the left and right side BC's. They didn't seem to help either.

[artkingjw]

Originally Posted by LoGaL

What is this “Farfield” you are imposing? Pressure outlet? (That is what I would give there)

Just to follow up on this suggestion. I managed to make this BC work to a non-diverging steady state solution. I've attached screenshots to show the result. It is clearly not right, having significant upwash along the domain.

So there are two pressure outlets in this domain, one at the normal outlet location to the right, and one on the top.

It seems the solution converged this time because I used a different velocity inlet. More specifically, I split my velocity inlet into two, with a small inlet above the wall that has a rough boundary layer velocity profile instead of a uniform velocity component. The last time I tried pressure outlet top, the velocity inlet was just a uniform velocity with no boundary layer profile.

[LoGaL]

Okok I have to be honest, I believe you are thinking way too much xD. This RANS should converge like no problem to a nice, steady solution with no garbage and so on.

First thing, fix this mesh and forget about splitting the inflation layer into two (WTF?!?!) for improved convergence and damping ( EHH?). Seriously, who gave you this idea? All it is happening is that where you change from first layer thickness to smooth transition, the height of the first mesh element changes abruptly, and this gives you shitty mesh elements.

Keep things simple, impose a nice first element thickness everywhere. No damping fairy tale, because if you give fluent a good mesh, it will converge even if you smash the workstation. Then put this pressure outlet on the top and run the simulation.

I am afraid to ask you which discretization settings are you using xD? Please, tell me that it is the coupled solver with all second order schemes and that you are not trying to use MUSCLE or QUICK or some exotic things I am not even aware about

[LoGaL]

Originally Posted by artkingjw

It seems the solution converged this time because I used a different velocity inlet. More specifically, I split my velocity inlet into two, with a small inlet above the wall that has a rough boundary layer velocity profile instead of a uniform velocity component. The last time I tried pressure outlet top, the velocity inlet was just a uniform velocity with no boundary layer profile.

Feels to me that it will blow up eventually. The result is completely unphysical

[artkingjw]

Originally Posted by LoGaL

Okok I have to be honest, I believe you are thinking way too much xD. This RANS should converge like no problem to a nice, steady solution with no garbage and so on.

First thing, fix this mesh and forget about splitting the inflation layer into two (WTF?!?!) for improved convergence and damping ( EHH?). Seriously, who gave you this idea? All it is happening is that where you change from first layer thickness to smooth transition, the height of the first mesh element changes abruptly, and this gives you shitty mesh elements.

Keep things simple, impose a nice first element thickness everywhere. No damping fairy tale, because if you give fluent a good mesh, it will converge even if you smash the workstation. Then put this pressure outlet on the top and run the simulation.

Thanks for this. I'll go back to basics.

In the past I have found that this split fixed a divergence issue I was having before with a similar type of wall bounded flow. I read about the 'issue' of having too-small elements at the outlet from an online forum (might be here, or it might have been something like researchgate), and I found out that a colleague of mine also did something similar (but it was a hex mesh instead of polyhedral).

Originally Posted by LoGaL

I am afraid to ask you which discretization settings are you using xD? Please, tell me that it is the coupled solver with all second order schemes and that you are not trying to use MUSCLE or QUICK or some exotic things I am not even aware about

At the moment I am using SIMPLE for P-V Coupling, Least Squares for Gradients, Second order for pressure. As for the other variables, with LES, I use Central Difference, and during steady state, I use Second order upwind. Nothing too exotic, as far as I know this is all pretty standard.

[LoGaL]

Indeed it is pretty standard, I agree. Once you have a simple mesh(plspls make sure it does not complain about mese quality), try running the coupled solver instead of SIMPLE. It is much more stable and converges faster. Then for the LES settings you can go back to SIMPLE or even PISO, but I am not too expert on what to choose there

Also for this problem ( i guess it is subsonic?) you can stick to standard pressure and not use second order. If it is instead a supersonic BL, which I do not think?, then go for second order. Remember also that the job of the steady run is just to get a good starting point for the LES simulation

[artkingjw]

Originally Posted by LoGaL

Indeed it is pretty standard, I agree. Once you have a simple mesh(plspls make sure it does not complain about mese quality), try running the coupled solver instead of SIMPLE. It is much more stable and converges faster. Then for the LES settings you can go back to SIMPLE or even PISO, but I am not too expert on what to choose there

Also for this problem ( i guess it is subsonic?) you can stick to standard pressure and not use second order. If it is instead a supersonic BL, which I do not think?, then go for second order. Remember also that the job of the steady run is just to get a good starting point for the LES simulation

Ok I'm back. Yes this is subsonic.

I've done a few runs (in steady state only so far) to check the choice of BC. First of all to address your concerns: yes this time I've kept it simple with a single uniform inflation layer; minimum quality was > 0.21 from Fluent meshing; I used 1st order for Pressure (unless otherwise stated), 2nd order for everything else, and I used PISO as suggested. Model is k-omega SST.

EDIT: Woops I misread your advice and chose PISO instead of Coupled for the SST steady run. I'll retry it with coupled.

The 4 screenshots attached show the results for:
1) Presusre outlet on top
2) Outlet-vent on top
3) Farfield on top (with a Mach number = same as the inlet velocity and direction)
4) Farfield on top (same as before, but with 2nd order pressure)

You can clearly see that having an 'outlet' of any type on top is incorrect, flow is leaving the domain on both the top and right side. You can see from a pathlines plot (coloured by vertical velocity) that the flow is just moving upwards.

Using a farfield condition on top is clearly better in this regard, however the fluid domain still does not look correct. These results look qualitatively similar to the results I was getting before when my configuration was arguably too complicated. Also, the 2nd order pressure does not seem to 'fix' this issue, nor does it 'break' things.

[LoGaL]

So mesh is okay, settings seem okay. What else are you using? I suppose velocity inlet and pressure outlet?

How are you judging convergence?

How are you setting periodicity? (Even though I think you mentioned that using symmetry gives same shitty results)

[artkingjw]

Originally Posted by LoGaL

So mesh is okay, settings seem okay. What else are you using? I suppose velocity inlet and pressure outlet?

Yup exactly.

Originally Posted by LoGaL

How are you judging convergence?

Just using the residuals at the moment. When the aerodynamic model goes in I will also monitor forces as per usual.

Originally Posted by LoGaL

How are you setting periodicity? (Even though I think you mentioned that using symmetry gives same shitty results)

I'm new to periodicity, my past CFD experience has always used just a free shear wall or symmetry. The periodicity was set in Fluent meshing, using the default 'automatic' mode and using translation (the other option is rotation). As far as I can tell this sets the periodicity based on the correct z-offset, with no x and y offset.

[artkingjw]

This seems promising!

I just ran 2 cases and I've attached the results. Both of these were changed to Coupled PV (my previous results were PISO). I used 2nd order pressure (because I was curious and it works).

1) Farfield BC with matched Mach number on top
2) Free shear wall on top

Case 2 converged quite quickly - it reached E-5 convergence in under 150 iterations. The flow field also looks correct, with the correct 'free stream' velocity. I've used a free shear wall in the past (when I was using PISO or SIMPLE) and it didn't help, giving similar results to using a farfield BC. So the use of a 'wall' by itself is not the whole solution to my problem.

Case 1 is closer to what I want to run eventually. This one didn't converge after 500 iterations (I know it's not the end of the world), settling in around E-2. However, note that the quality of the flow field is significantly better this time, being much more physical.

Thanks for suggesting the Coupled algorithm, it seems to have steered me in the right direction!

[LoGaL]

Yes it is better but I am still not satisfied by the convergence, the boundary layer with RANS should be very smooth, while there you have some weird structures. For such simple flow ( at least as far as RANS is concerned) you can drive fluent to machine level convergence

I was thinking, since we know that the boundary layer is much smaller than the mesh, perhaps it makes sense to impose the free stream velocity in the top layer? Probably you can impose a slip wall there with a prescribed velocity.

Also, can you try reimposing pressure outlet there and stick to the coupled PV? I know it may seem I am obsessed with it, but it should really be the simplest way to go. Consider that yes, it is called pressure outlet, but what it really does is impose static pressure, period. The word outlet is there because it also allows you to specify reverse flow conditions. When you specify it, please also specify sensible reverse flow conditions, i.e. same temperature of your inflow condition, otherwise if you are using ideal gas it may screw up a bit the computation

Oh, also, drive those residuals below E-06 for all the equations before calling it converged

[artkingjw]

Originally Posted by LoGaL

Yes it is better but I am still not satisfied by the convergence, the boundary layer with RANS should be very smooth, while there you have some weird structures. For such simple flow ( at least as far as RANS is concerned) you can drive fluent to machine level convergence

Yes I agree. Could this be due to the "init-turb-vel-fluctuations" command that I used (since this will feed into LES).

Originally Posted by LoGaL

I was thinking, since we know that the boundary layer is much smaller than the mesh, perhaps it makes sense to impose the free stream velocity in the top layer? Probably you can impose a slip wall there with a prescribed velocity.

Also, can you try reimposing pressure outlet there and stick to the coupled PV? I know it may seem I am obsessed with it, but it should really be the simplest way to go. Consider that yes, it is called pressure outlet, but what it really does is impose static pressure, period. The word outlet is there because it also allows you to specify reverse flow conditions. When you specify it, please also specify sensible reverse flow conditions, i.e. same temperature of your inflow condition, otherwise if you are using ideal gas it may screw up a bit the computation.

Gotcha. Yes I understand why you're keen on Pressure Outlet BC, as far as I can understand (and also based on many papers that I've read), it seems that this kind of p=0 BC is common. I'll also give a 'velocity inlet' at the top a try as I think you have suggested.

Yes I am using compressible ideal gas, so a wall of any kind of reflective wall would not be the best as I'm keen on the compressible waves produced.

Originally Posted by LoGaL

Oh, also, drive those residuals below E-06 for all the equations before calling it converged

Ah yes, I was using a more relaxed criteria for an initial solution. That's fair.

[LoGaL]

Yes it definitely could be the fluctuations you imposed , please show me contours before using the command xD

I admit I am really not a big fan of the Farfield BC because I don’t understand exactly what it is doing xD, seems a bit fishy to me. I prefer imposing good old velocities/massflows and pressures.

[artkingjw]

Originally Posted by LoGaL

Yes it definitely could be the fluctuations you imposed , please show me contours before using the command xD

I admit I am really not a big fan of the Farfield BC because I don’t understand exactly what it is doing xD, seems a bit fishy to me. I prefer imposing good old velocities/massflows and pressures.

Yea I've been trying to find more info about the Farfield BC too...

Anyhow, it looks like my problem is solved. I've attached the results from a Pressure Outlet run, both before and after applying fluctuations. I've also shown a zoomed in shot of the BL before applying fluctuations.

So it looks like the problem is solved, and I'll need to see how this behaves in LES next.

[LoGaL]

Yep, it’s definitely fine, I approve it
Good luck with LES, I can’t help you there, I don’t have enough experience

By the way, now that you have something which you know is working, you can also recomplicate the setup, e.g. you can try that inflation layer thing, different schemes and so on. As you have something to compare against, it is very easy to say if a change is good or bad. However, just my tip, if you change the mesh, re-check the quality, because the last thing you want is a bad mesh: if the solver blows up, with a bad mesh you don’t know if it is a solver problem or a mesh problem

[artkingjw]

In an unexpected turn of events, I've run into trouble again, this time still at the steady state portion. I am getting reverse flow that does not die down at the top pressure outlet (>40% of faces). I can confirm that the results look completely wrong afterwards.

The only difference between this time and the last time is I have updated the mesh VERY SLIGHTLY - only slight tweaks to the refinement regions. Using the exact same setup file (using Coupled P-V etc.), the simulation converged well and produced a physical result last time. I'll create a list of meshes to refer to just so this doesn't get confusing

1) Mesh V3.9 - original, confirmed working
2) Mesh V3.10.1 - 'new' mesh with slightly updated sizing regions
3) Mesh V3.10.2 - an attempt to replicate the setup found in V3.9

Unfortunately I didn't backup/save the settings used to create Mesh 3.9. I attempted to recreate that mesh to the best of my memory in Mesh V3.10.2 - but this has not worked. All of these meshes have the same domain size.

I have tried using SIMPLE on V3.10.2 - and it does 'converge' to E-3 only, and the result is unphysical, showing the same 'upwash' effect as mentioned before.

Any ideas on why this is the case?