[RodriguezFatz]

Dear all,

In my RANS simulations I see that the flow in a completely symmetrical diffuser (with symmetrical inlet and outlet boundary conditions) becomes asymmetric in a certain way, please see the picture.
201509281448.png
The simulation starts to converge to the symmetric solution (left picture) but eventually converges to the unsymmetric right picture, where the flow stics to one side of the wall.

By the way, my simulation is 3d, with pipes at inlet and outlet, k-omega-SST or realizable-k-epsilon model.

Can anyone explain why this happens and if this is physically correct? If not, how can I prevent this?

Thanks for any help,
Philipp.

[FMDenaro]

Originally Posted by RodriguezFatz

Dear all,

In my RANS simulations I see that the flow in a completely symmetrical diffuser (with symmetrical inlet and outlet boundary conditions) becomes asymmetric in a certain way, please see the picture.
Attachment 42376
The simulation starts to converge to the symmetric solution (left picture) but eventually converges to the unsymmetric right picture, where the flow stics to one side of the wall.

By the way, my simulation is 3d, with pipes at inlet and outlet, k-omega-SST or realizable-k-epsilon model.

Can anyone explain why this happens and if this is physically correct? If not, how can I prevent this?

Thanks for any help,
Philipp.

Could you better detail your simulation? If you are using RANS, the solution should converge to the statistically steady state, thereferore what you see is due to the fact that you do not get residuals tend to zero. On the other side, if you want a RANS, the geometry you should use is 2D...
Conversely, an unsteady simulation at high Re nunber, correctly show asymmetric solution, in a sort of K-H instabilities with large structures alternating at upper and lower walls

[RodriguezFatz]

Yes Filippo, you are right. Right now the geometry is actually 2d, but I want to use different inlet boundary conditions, such as single or double bend in the future, so I made this in 3d. Re is about 100,000 in the larger part of the pipe.

This is a picture of the residuals. I don't see anything suspicious here, looks like really good convergence. Unfortunately, if you use Fluent standard settings with 1e-3 convergence you will get the first "symmetrical" solution.
ICM.jpg

This is how the flow velocity looks like.
ICM_2.jpg

Where can I find something about these instabilities you mentioned, specially in pipes? So do you think this might be physical?

[FMDenaro]

In my opinion, at high Re number you cannot get a staedy symmetric vortical ring but a more complex unsteady framework... I am quite sure that performing DNS/LES this is a physical pattern you would get, but using URANS that is quite doubtful.

[FMDenaro]

Originally Posted by RodriguezFatz

Yes Filippo, you are right. Right now the geometry is actually 2d, but I want to use different inlet boundary conditions, such as single or double bend in the future, so I made this in 3d. Re is about 100,000 in the larger part of the pipe.

This is a picture of the residuals. I don't see anything suspicious here, looks like really good convergence. Unfortunately, if you use Fluent standard settings with 1e-3 convergence you will get the first "symmetrical" solution.
Attachment 42398

This is how the flow velocity looks like.
Attachment 42399

Where can I find something about these instabilities you mentioned, specially in pipes? So do you think this might be physical?

the last picture, show a non-symmetric geometry, that's right?

[RodriguezFatz]

No, this case is symmetrical. Flow goes from left to right.
The small (left) section is not a round pipe, but rectangular and expands smoothly to the larger (right) round pipe.

Edit: But it is symmetrical relating to top / bottom, so it seems to be randomly that the flow sticks to the top and not to the bottom.

[RodriguezFatz]

Buongiorno Filippo,
Now I finally managed to reproduce that behavior - even with LES. Unfortunately, I was too lazy to get OpenFoam running, so I did the LES in Fluent. I could only afford wall modeled LES.
Courant number is about 0.6 in the constricted part, pressure differencing is 2nd order. I run some unsteady SIMPLE algorithm, where all residuals are reduced by 2 orders of magnitude within each time step.

If I set the velocity/momentum discretization to "bounded central differencing" I get the symmetrical solution:
bounded_central.jpg
Then, I switched it to "central differencing", I get the asymmetrical one:
central.jpg
Both are pretty stable over a long time.
Switching back to the bounded scheme actually again jumped into the symmetrical solution

1) What do you think about that?
2) I realized that I can increase the under relaxation of SIMPLE to pretty large values, such as 0.8 for pressure and 1 for velocity. They are very stable and give fast decreasing residuals (such as 5 iterations for 0.01 tolerance). Can I expect this behavior for such setups?

Thanks for any help!!!
Philipp.

[FMDenaro]

Hello,
what kind of SGS model do you set in Fluent?
From past experience, the bounding scheme is largely affected by numerical dissipation and you should use central scheme without bounding.
The non-symmetric solution is just a snapshot at some time, do you see the flow oscillating from up and down?

[RodriguezFatz]

Hi,
The model in Fluent is called "Algebraic WMLES S-Omega Model Formulation". Seems to be a Smagorinsky model with some adaptions for the wall modeling.
The non-symmetric solution is stable, i.e. does not jump up and down.

[FMDenaro]

well, in a totally symmetric pipe geometry, same BC.s at wall, homogenoeus inflow, no strong boyancy effect, etc., I cannot imagine any physical reasoning that can drive towards a statistically steady non-symmetric solution...

I would expect an unsteady solution like in the first picture, any different solution seems caused by numerical (or error) effects ...
if you have time, I suggest some further investigation:

1) set central unbounded scheme and dynamic SGS modelling
2) run the same but using laminar model, that means you set no turbulence modelling on an unresolved grid

Of course, I assume you have sufficient grid resolution at walls (at least 2-3 node within y+=1).

As a control of the solution, compute the integral of the kinetic energy over the whole domain and plot it in time to have a monitor of the energy dynamic. I would see how long it takes to disregard the initial numerical transient

[RodriguezFatz]

Filippo, thank you for your ideas! I guess it is "random" whether the solution initially jumps to the top or bottom, because I saw both in my simulations. But once it is there - it remains. The geometry is indeed not cylindrically symmetric, because the constricted part on the left has a rectangular cross section. The geometry is symmetrical w.r.t. the middle plain of the pipe. So the flow goes from pipe to rectangular to pipe. Resulting from that rectangular part in the middle, the solution can only jump to bottom or to top and not to any other direction. Maybe some grid inaccuracies (or random effects from the initialization) let the solution jump more frequently to the top. But again, I already saw both "versions".

When I look at both the RANS and LES results I can see that the "better converged" results are always asymmetric. So for RANS the one with the lower residuals, and for LES the one with less dissipation (i.e. unbounded scheme). This makes me suppose that the asymmetric solution is the physical one. Do you think this is a false conclusion?

I will see if I can (numericaly) afford a wall resolved mesh.

[FMDenaro]

could you post the figures of the geometry in the projection planes?
I mean 3 figures in (x,y), (x,z), (z,y) planes....

Before this problem, have you tried to solve a simplified model like the backward facing step in a cylinder using your BC.s?

[LuckyTran]

It is possible! But you need to be very very careful that it is real and not some mistake on your part.

These are called flow bifurcations and are a type of hydrodynamic instability. They are very physical and happen even in real hardware.

These bifurcations are prone in systems with perfect symmetry or high degree of symmetry. The flow state where the flow sticks to one wall is a lower energy state than a symmetric flow. But because of the symmetry, both branches of the bifurcation can be at similar energies. That is, the flow prefers to stick to one of the walls, both it's equally capable of sticking to either wall. One possible result is an unsteady flow where the flow dynamically switches between the two bifurcation branches, since both of these branches are preferred over the symmetric flow case. Or depending on the initial conditions, the flow may stick to only one wall.

In industrial design of hardware where these flow bifurcations are likely, often the geometry is intentionally made non-symmetric (by offsetting the design) so that one bifurcation branch is preferred. This prevents the dynamic mode switching and makes it easier to predict the flow field since one branch is preferred over the other. Dynamic switching also induces structural vibrations which reduces the life of the hardware. Physically it is very difficult to build perfectly symmetric hardware, but it can closely approximated (which may be intentional or unintentional). The problem then is you don't know which branch you are in, so it is preferred to have an intentionally non-symmetric design to mitigate the uncertainty.

The correct intuition is that in a system with perfect symmetry and ideal boundary conditions, there's no reason for the flow to attain a non-symmetry statistically stationary state. The requirement for everything to be "perfect" is a very strong. With a bit of numerical errors introduce during computational the solution can switch back and forth between two unstable modes. Sometimes it can even be deterministic with DNS, where depending on the initial condition the flow will stick to one side and stay there, and under a different initial condition stick to the other side. Or the flow may dynamically switch back and forth.

You can "prove" that your asymmetric flow is a bifurcation branch by making your geometry non-symmetric and offsetting it in one direction and then verifying that the flow always sticks to one wall. And then offset the geometry in the other direction and verify that the flow now sticks to the other wall.

Sorry for the long post but this is a topic that I am very interested in and have had trouble dealing with experimentally. I spent more than a month debugging a transient TLC heat transfer experiment in a square duct because the heated fluid would tend to stick to two opposite walls rather than be evenly distributed between all four walls. I did all kinds of things, like rotate the rig 90 degrees, 180 degrees, 270 degrees along its axis, even flipped the channel backwards, all sorts of things and eventually found out that my test section was too ideal and symmetric.

[RodriguezFatz]

Wow, great post, thank you for that insight!
Yes, at least for my case this is indeed an industrial hardware. Since these things happen downstream of our device it is not really frightening me, but I found this when trying to simulate the pressure drop of a design.

For the "intentional asymmetry" that you suggest... what do you think is the best? I mean, if I put some small bump on one side, I guess the flow will of course separate there - so what outcome would you expect?

[FMDenaro]

bifurcation in the solution is actually a possiblity (Hopf bifurcation) but that should be studied only within DNS framework. RANS/URAN cannot provide such details and LES is somehow a tool to be used with very care.

The solutions showed in this post seem too affected by numerical issues...
A grid refinement study is required using DNS.
I strongly suggest to use the LES with central unbounded scheme and dynamic model.

Finally, the computational grid MUST be perfectly symmetric to avoid introducing sources of non-symmetric truncation errors

[LuckyTran]

Originally Posted by RodriguezFatz

For the "intentional asymmetry" that you suggest... what do you think is the best? I mean, if I put some small bump on one side, I guess the flow will of course separate there - so what outcome would you expect?

The separation bubble tends to prefer the side with more room. You can force the bubble to one side by making the diffuser start earlier on that side or increasing the width of that side (or maybe slightly larger angle).

Adding a bump... can sometimes kill the bifurcation altogether!

But two things need to be kept in mind. 1) Asymmetrical flow state is a "possible" instability but 2) It is not yet known what is driving the flow into this asymmetric mode

In these simulations it is possible that numerical instabilities are driving the flow to be asymmetrical, which is supported by the fact that you get a symmetrical flow with bounded central differencing but asymmetrical flow with regular central differencing. I am curious to see whether a 1st order upwind scheme (with high numerical diffusion) would result in a symmetric flow but a 2nd order upwind (with less diffusion but more numerically unstable) would result in asymmetric flow.

By the way, did you remember to add perturbations at the inlet to your LES? Otherwise you just ran an unsteady laminar simulation.

So what is the next step? Do you want to study the intended symmetric flow or investigate the asymmetric one?

If you want to study this asymmetric flow in detail, then I also agree that a scheme with very low numerical diffusion is necessary to properly resolve the dynamics and get the proper physics. But as you reduce numerical diffusion, you make the simulation less robust against numerical instabilities.

[FMDenaro]

Originally Posted by LuckyTran

The separation bubble tends to prefer the side with more room. You can force the bubble to one side by making the diffuser start earlier on that side or increasing the width of that side (or maybe slightly larger angle).

Adding a bump... can sometimes kill the bifurcation altogether!

But two things need to be kept in mind. 1) Asymmetrical flow state is a "possible" instability but 2) It is not yet known what is driving the flow into this asymmetric mode

In these simulations it is possible that numerical instabilities are driving the flow to be asymmetrical, which is supported by the fact that you get a symmetrical flow with bounded central differencing but asymmetrical flow with regular central differencing. I am curious to see whether a 1st order upwind scheme (with high numerical diffusion) would result in a symmetric flow but a 2nd order upwind (with less diffusion but more numerically unstable) would result in asymmetric flow.

By the way, did you remember to add perturbations at the inlet to your LES? Otherwise you just ran an unsteady laminar simulation.

So what is the next step? Do you want to study the intended symmetric flow or investigate the asymmetric one?

If you want to study this asymmetric flow in detail, then I also agree that a scheme with very low numerical diffusion is necessary to properly resolve the dynamics and get the proper physics. But as you reduce numerical diffusion, you make the simulation less robust against numerical instabilities.

I am not sure that is fully similar to this case, but a sort of bifurcation in the numerical solution is the case with one inflow and two outflow where the flow can go in a branch or set to both branches

[RodriguezFatz]

Yes, I am running the inlet profile with some of Fluent's perturbations.
I am not quite sure how I can create a WR-LES grid that is perfectly symmetric and also computationally affordable. I don't think my meshing tools are capable of doing this. I just shortened the outlet length strongly and the mesh is incredibely large when I use the wall resolution recommendations of my LES book.

At the end of the day, the "best" solutions I could get (see post #11) show asymmetry. I don't know what the best next step is ...

[RodriguezFatz]

If I set y+=0.5, z+=x+=50 (which is already pretty coarse, I think) and use the smaller outlet path, I get 27 mio cells with Ansys Meshing.
Normally I use ICEM, so I feel like a rookie here... it looks like I can't use hexa mesh + prism layers, so I needed to take the tet mesh. Of course, this blows up the whole mesh. Maybe I give ICEM a try, but the mesh will be unthinkable large anyway...

[FMDenaro]

Originally Posted by RodriguezFatz

If I set y+=0.5, z+=x+=50 (which is already pretty coarse, I think) and use the smaller outlet path, I get 27 mio cells with Ansys Meshing.
Normally I use ICEM, so I feel like a rookie here... it looks like I can't use hexa mesh + prism layers, so I needed to take the tet mesh. Of course, this blows up the whole mesh. Maybe I give ICEM a try, but the mesh will be unthinkable large anyway...

yes, you need some millions of computational nodes... I think you can get symmetric grids if you mesh half domain and copy it...