LES evaluation help needed
 

Dear all,

I try to get some experience in LES and need some help.
My setup is a simple straight pipe of 4m length and 1m diameter. Periodic bc with a mass flow rate of 0.044 kg/s is applied, which results (for air) in a velocity of about 0.07 m/s and thereby Re(pipe)=4800. y+=0.9 nearly everywhere, with y=6mm. I have a z and x of about 30mm, thus x+=z+=5.
Attachment 19017

Initialization with RANS, then switched to LES (Smagorinsky-Lilly) with some disturbances from the terminal (as described in the Fluent manual). I set the timestep to something save dt=0.15s, time to cross one cell should be about 0.5s. Also solution methods are set as recommended in the manual. Now, from yesterday to today the simualtion ran and I got some first results.

z-velocity:
Attachment 19020
y-velocity:
Attachment 19019
x-velocity:
Attachment 19018

1) Simulation time is 261s, so the fluid traveled nearly four times through the entire pipe, which is a bit too less, I guess. (?)
2) I would like to let some monitor run during the simulation with some good predictor for convergency. Any ideas? What about a volume integral of vorticity magnitude?
3) Now, I want to check for numerical stability by means of grid size, time step,... What would be good for a judgement of that? Just the velocity profile?
4) Also I was wondering of a Re=4800 pipe is "turbulent enough" to see something in an LES at all.
5) Is there any other good way to see, if my simulation is actually a real LES (and not some VLES with a too large grid), then just do the grid / time step - independence study?

1) compute the volume-averaged kinetic energy and follow its time-evolution. You must reach first a statistically steady state
2) Then, you have to save several samples of your fields, the sampling frequency can be for example any 1 non-dimensional time-unit.
3) For each sample, compute statistics, that is averaged velocity profiles, rms, spectra
4) compute the average of the statistics

then show us the results ... you can find the reference LES solutions in the AGARD report of some years ago

Dear Filippo, thanks for your fast reply.
With "kinetic energy" you mean the kinetic energy of the resolved scales, right? I have to do this with a custom field function "0.5 * v * v * rho"?
All the other points of your post... this is to verify the statistics, correct? Wouldn't it be (nearly) equivalent to show the grid independence?

Yes, compute the resolved kinetic energy and plot versus the time so that you can check for the statistical equilibrium.
Statistics are the only relevant result you can use to validate LES, indeed for implicit filtering such as the approach used in Fluent, you don't have a grid independence as in RANS. Actually by refining the grid your solutions will tend asintotically to the DNS one...

Of course you are right, my bad. But for the time step size I could do that, right?

what do you mean? simply compute first your non-dimensional time step and then save the files each N time-steps, such that N*dt = 1. Save at least 15 samples

Sorry, I ment, I can double / half the time step size to see if any relevant parameter changes.

No.... as in Fluent the filter is only on the spatial scales, you must run your LES case using the time-step as small as possible....

As I understand it, for a given grid, there should be independence of LES statistics for small time step sizes. Thus, when I decrease my time step, hopefully results won't change... Right now I think I am "on the safe site" with dt=0.15s because dz/v = 0.5s.

yes, for a fixed spatial grid and vanishing dt, you reach an independence in the solution, say v(x,t;Delta), but this solution will change when you refine your spatial grid since Delta depends implicitly on the mesh size.
Therefore, the general rule in LES is to use a dt such that you resolve all relevant time scales (a sort of a DNS in time). Otherwise, you implicitly are doing a time-space filtering and your sgs model should take into account also for the unresolved time-scales. But this is a different history ...

Alright, that was what I ment. I wanted to change dt just to see, if it is already small enough!

but you can save computational time ... you can do some estimation of your required dt based non the Kolmogorov time-scale of your problem;)

Is this really the relevant time-scale? I don't think so, because the needed time-scale should depend on the grid size.

the required computational time-step depends on the physics of your problem...

Of course, but for a given grid I get some maximum velocities. Grid-size devided by this velocity gives a time-step estimation. Is this correct? (Courant-number estimation)

are you talking about the cfl condition? first, the numerical stability condition involves also the diffusive scale in a complicate manner that depends on the discretization... then, you must use a dt smaller than that estimated from the convective condition, such that in the computational cell the characteristic diffusive time is of the same order of your computational time-step. This is equivalent to guarantee a DNS resolution in time.

Sorry, but I still don't get your point. :o
Now, there is some time scale needed for DNS. For LES the grid is coarser and the fastes eddies get modeled - so the required time step gets larger. The degree of modeling depends on the size of the grid. That makes the time step of the LES grid size dependent.

> 1) Simulation time is 261s, so the fluid traveled nearly four times through
> the entire pipe, which is a bit too less, I guess. (?)

It depends on the type of flow. For example, accelerating flows tend to settle quickly whereas diffusing flows can take a long time to settle. Given the short length then yes 4 pass throughs will not be enough.

> 2) I would like to let some monitor run during the simulation with some
> good predictor for convergency. Any ideas? What about a volume
> integral of vorticity magnitude?

It isn't clear from your description quite what is fixed and what floats. If the mass flow adjusts to balance the stresses and an imposed pressure drop then the mass flow itself is a simple and reasonable monitor. If the mass flow is fixed and the stresses adjust then you could use those to monitor for equilibrium. The energy in the turbulent motion is also a common measure.

> 3) Now, I want to check for numerical stability by means of grid size,
> time step,... What would be good for a judgement of that? Just the
> velocity profile?

The Peclet and diffusion numbers in the three grid directions and every cell is the usual means of monitoring flow stability and choosing a suitable time step and possibly regridding for more complex flows. During the settling down phase there is often a bit of a bang requiring the time step to be reduced if the convection and/or diffusion is explicitly treated.

> 4) Also I was wondering of a Re=4800 pipe is "turbulent enough" to see
> something in an LES at all.

LES is usually a high Reynolds number model. If you have a low Reynolds number flow then a turbulence model should not be used. Simply perform an unsteady laminar simulation.

> 5) Is there any other good way to see, if my simulation is actually a real
> LES (and not some VLES with a too large grid), then just do the grid /
> time step - independence study?

There is no need to perform a simulation at all. The Reynolds number of the flow tells you.

If you insist on performing a simulation then a "proper" LES needs to resolve all the large scale motion from the largest strongly anisoptropic energy containing scales down to a scale which is reasonably isotropic but still well above the scales dissipating energy directly to heat. Evaluating the work done against the viscous stresses, the LES model stresses and the energy in the resolved motion should indicate if the required assumptions about the turbulent motion are being met.

From a book of Sagaut:

We follow the common interpretation of LES as result of an evolution equation with spatially reduced resolution, and thus we focus on the analysis of errors due to spatial discretizations
and spatial filtering. This implies that the time-step size chosen for time integration is always sufficiently small so that error contributions from temporal discretization and temporal filtering (if applied) are negligible as compared to spatial error contributions. From now on this will will be tacitly assumed.



That means that your dt should be formally at level of the Kolmogorov time-scale to ensure it does not produce filtering effects (or, form a numerical point of view, a time-contribution of the local truncation error)

So it's recommened to take the worst case (=smallest) time step to ensure that it is actually small enough. Ok, but if you double it afterwards and compare the results you can learn for future simulations what might be small enough...

if you use a dt that is suitable from the point of view of the stability constraint but is quite large compared to the characteristic time scales of your turbulent flow, then your solution is somehow implicitly filtered also in time, that is v=v(x,t, Delta_x, Delta_t). However, you do not add an sgs model that would take into account the unresolved time components...

The time varying motion at the Kolmogorov scales is not resolved in an LES but modelled with a turbulence model. If you want negligible numerical errors then you must resolve the motion in time but this will be the grid scale motion and not the viscous dissipation scales. In practice an LES model for the instantaneous sub-grid scale motion tends to be very poor and significantly worse than RANS models for the Reynolds stresses for example. LES works if the sub-grid stresses are small compared to the resolved stresses and if the sub-grid model behaves well in an average sense in transferring energy to/from the sub-grid modelled motion.
In practice there is little need for the grid scale motion to be fully resolved unless you are comparing sub-grid models.

This issue is quite controversial in literature, some authors explicitly consider the time-filtering as present in the simulation and propose some specific sgs model for the unresolved time-scales... however we can be off-topic ;)

From my experience with Fluent and the pipe flow, your Re number might be too low to allow a static Smagorinsky model to work. Otherwise, if you are using a Dynamic version, the problem might be in the convection scheme if it is the bounded central one.

However, some instability is clearly present, and possibly it is just the effect of a bad initialization (the fact that it is suggested by Fluent means nothing)

My experience with this case at Re_D=10k is to use:

dz+ = 30 and (R*dtheta)+=15 with classical wall normal spacings

dt=0.1*nu/u_tau^2 should be always enough (there is no point in going below this value for LES)

I see there are different approaches for the time step setting. Thank you for this insight.

One additional question: Is there any reasonable way to judge if the LES model works in a somewhat proper range? Recently I made an ERCOFTAC workshop about DES and some of the lecturers recommended to check the ratio of resolved to total turbulent kinetic energy for the "LES" part of the DES, which is pretty easy since the RANS model has a modeled "k" anyway.

Is there any way for a real LES to do something like that?

using an eddy viscosity model allow you to compute the averaged radial distribution. Further, you should always do the computation on the same grid and same time-step without using any turbulence model (LES no-model) that give you a clear framework of the action of the sgs model

Radial distribution ok, but that only helps for types of flows where reference values are known. Comparing to DNS results or experiments does only mean you get the correct real results. That does not mean, that your SGS-model works as it is designed for.

Can you give a general rule how to implement your second suggestion?

just set your case to laminar flow, without turbulence model ;)

Well I know how to start a DNS. I ment an advise how to use this information to judge whether the SGS works fine or not...

The Reynolds number tells you this. There is no need to perform a simulation. Your example is for a low Reynolds number flow and so a turbulence model that assumes the Reynolds number is high like a standard LES model is not appropriate. If this is the Reynolds number of your flow of interest then that is good news because you can simply solve the Navier-Stokes equations without any assumptions about turbulence models.

Wanting to solve a steady state flow at low Reynolds number is a fairly common requirement and there are low Reynolds turbulence RANS models although they tend not to be particularly general like the high Reynolds number models.

Wanting to solve an unsteady flow at low Reynolds number and include a turbulence model is odd unless this constraint is coming from something else like being a part of a high Reynolds number flow. Why do you want to do this?

I guess I did not illustrate my thoughts clear enough:
You can run a simulation with LES turbulence model and a bad (too large) grid. Then, the level of modeling of the SGS model will be quite high. These models are pretty imprecise and made to model a relatively small amount of turbulent spectrum. That's what I mean by "That does not mean, that your SGS-model works as it is designed for" in my previous post. The question now is: How can I judge, if the amount of modeling by the SGS model is small enough to give good results.

compare modelled and no-modelled LES by means of statistics (rms, spectra), the effect of the eddy viscosity model is in the damping of the highest resolved wavenumbers

In which case you would seem to be confusing numerical resolution and modelling assumptions plus picking an inappropriate test case. To expand on my answer to your original question:

For an LES simulation good numerical resolution means accurately resolving the large energy containing energy scales. These are the RANS Reynolds stresses which are evaluated from the statistics of the flow. For numerical methods designed for LES these stresses tend to be too anisostropic and too large when under-resolved. This can be seen by grid refinement. For general purpose numerical methods the turbulence may go out or blow up depending on the details.

The sub grid scale stresses can also be evaluated from the statistics (with a modelling assumption for most models) and compared with the Reynolds stresses. In high Reynolds number regions they should be small but they will grow near, for example, walls which usually introduce additional modelling assumptions.

The viscous stresses can also be evaluated from the statistics and compared with the sub-grid stresses and the Reynolds stresses. These are exact terms and so the growth near walls is good rather than a cause of concern.

In addition there are "numerical stresses" which broadly follow from the leading truncation terms in the transport terms. These are usually comparable with the sub grid stresses and in LES orientated numerical schemes their type and behaviour is important and controlled.

The above would be implemented in pretty much all research LES codes but how much is already built into your commercial code I do not know.

I have a further suggestion, that however implies some work...
your Re number is quite low to try a DNS with some effort. Then you can use your DNS solution by applying a volume filter on the velocity components, the width being the same of the volume grid you use for LES. You can then compare all data.
This test is not perfect but can give you further indications about the quality of your LES if coupled with the LES no-model

Hi, in your description, you said "y+=0.9 nearly everywhere, with y=6mm. I have a z and x of about 30mm, thus x+=z+=5". But what if the geometry is complex and you don't really know the size in Z and X direction? What software are you using? can your software plot the X+ and Z+ , just like Y+?

Thank you so much ! I am using StarCCM+ and feeling lost about X+ and Z+...

Aqua

I use Fluent, and here, you need to evaluate x+ and z+ by yourself. "y" is allways the direction of the flow in fluent, even if it isn't actually the "y-direction" of your physical coordinates.

Hi, I know what does Y+ mean, and Y+ actually mean the direction normal to the surface of the model... But did you mean that X+ and Z+ can not be calculated precisely?
Thank you for your kind reply.

I guess what RodriguezFatz was trying to say is that, as those parameters actually depend from your flow direction, there is no obvious way to compute them without knowing in some detail your flow.

And even in that case, your grid might not be aligned with the flow direction, then how would you say what is dx^+ (stream-wise grid spacing in viscous units) and what is dz^+ (span-wise grid spacing in viscous units)?

However, for a given cell near the wall, you usually know the instantaneous y+ or, if you already have your statistics, you can compute the average y+ trough the mean wall shear stress. Then, if you know the grid (in Fluent you have access to several cell-related geometrical parameters) you can compute whatever d+ you want.

I remember doing something like this for a conference, where i had to plot the delta+ in a swirler for different swirl numbers (= different mean flow directions). I did it quite easily in Fluent but there was some hard-coding related to the geometry in order to obtain the correct values.

Hi,

What I do is just calculating

x+ = (y+ / dy) * dx

with dy and dx the real physical coordinates.

Hi, thank you for your reply again. I agree with the equation you mentioned below. But how to get the "real physical coordinate" so that you can get dy and dx? My geometry is complicated and I don't really know what is the size of every cell, which means I don't know exactly what is dx and dy because they varies a lot along the geometry....

Aqua