Fluctuating Pressure Fields (LES-pisoFoam)
 

Hi,

The Case:
I am testing on the pitzDaily ("tutorials/incompressible/pisoFoam/les/pitzDaily") case with time varying velocity inlet conditions. I have extruded the grid to a large 3D case.

A time varying velocity profile is imposed at the inlet (using the timeVaryingMapped type). When the variations are very small, the case converges and the results time series all look good.

The Problem:
When the velocity profiles and the inlet have larger changes in time, the pressure fields fluctuate in time: e.g: from t=0 to t=1 the whole domain has negative pressures. From time t=2 to t=3 the whole domain has positive pressures and so on. Note that the velocity fields look normal and have the expected values.


Do you have any thoughts on this strange behavior?
Thanks.

What numerical scheme are you using for the convective terms in the momentum equations? Sometimes when I get a fluctuating pressure field in LES simulations I have to use the blended scheme (blend of CD and first order upwind) instead of pure central differencing. This adds additional numerical dissipation and you have to be careful not to add to much. However, I have never had the exact problem that you are having, normally when my pressure field is corrupted, then the velocity field is as well. Maybe you have to decrease the time step when you have larger fluctuations since the CFL number in the cells located at the inlet will be higher.

Thanks for your recommendations.
Timestep: i have used extremely small timesteps and also normal timesteps (Courant Number of about 0.5)....but the problem persists...

Discretization Scheme:
divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div(phi,nuTilda) Gauss limitedLinear 1;
div(B) Gauss linear;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
I will try them with 0.5 (blended schemes with more weight for the upwind part...). I hope it works this time!

I'll post here whether it makes any change or not.

Thanks.

Did you acquire any improvements in the simulation? I'm trying to get an LES simulation running using LES as well. However, I don't know if the blended scheme mixes second order Central Differencing scheme with first or second order Upwind Scheme...

Hej,

Have you solved the problem?

I've got the same unphysical pressure functuation. I'm using turbulentInlet BC combined with a velocity profile at the inflow boundary. The velocity field looks normal but the pressure...

Not yet :confused:
But I will post an update when I make it right!

Even the original pitzDaily case has the same problem. I have tried more number of PISO corrections, and also limitedLinear, filteredLinear schemes.
Still no lock :(
As soon as you remove velocity fluctuations at the inlet, the case runs smooth!
Does not matter if you implement the velocity by the "turbulentinlet" or just map them directly......

Any ideas?
You can test it your self and run the pitzDaily tutorial in incompressible/pisoFoam/les/pitzDaily ->check the pressure field instead of U and you will see the fluctuations!

Hi, i've also a pressure issue when using pisoFoam. Although its a completely different case. Im simulating flow around airfoil and using turbulence model k-omega-SST. I've checked all my numerical schemes, tried more loops in fvSolution, set up the Co<0.5. Mesh is good. What i got from Residuals plot is partially not acceptable. Following you can see that all other parameters convergence beside pressure. In addition the pressure run more than the Iterations that i was setting (20000).


what will/are this pressure going to tell us? is anyone actually encounter non fluctuated pressure when using pisoFoam?

Thank You

Hi All,
Well I am stuck with the same problem.
I am simulating an externet cylinder flow. Please bear with me I will go through it thorougly to describe what I have done.

1- My grid is not bad quality. The extents of the domain are 15 times dia meter in x and y direction. I have 1 outlet, 1 inlet, cylinder wall and cylic BC in the normal direction to flow (no high-fi science).
2- I successfully ran the RANS simulation without wall functions (I prepared a grid for LES, with aim to have y+<1). Drag and Strouhal number looked fine. Residuals didn't converge properly. But I thought may be that's because of the unsteadiness in the flow. As we can observe that residuals don't converge very well for PitzDaily as well.
3- I decided to do an LES simulation on the same grid (from previous RANS run) with the same boundary conditions (no turbulentInlet BC, just a fixedValue BC for velocity) and I failed to get the expected behavior of pressure.
4- I created a new grid with more grid points (just to be sure that my grid resolution is not causing problems). But I failed again.
5- I changed the upper and lower Bc of my domain slip wall, (as my boundaries are far enough I thought may be adding slip walls would add to the stability of the case) but this didn't help either.
6- I was using freeStream boundary condition at the outlet which was working very well for me at the outlet, and now I thought about doing what has been done in pitzDaily for outlet and this didn't help either.

I don't know what to do, but I am trying. If something works then the question will arise why did it work?. :p
Anyways I am a bit relieved to know that I am not the only one stuck with this problem. Again I would request everybody to share their experience and the solution if they reach any proper results.

Regards,
Awais

Another info which I forgot is that I am using rhoPimpleFOAM.
Even thought my flow doesn't come under the category of being called compressible flow. But the I will need to study heat transfer in flow as well. That is why I am considering a compressible flow.
Regards,
Awais

The one question is that why the pitzdaily case (pressure field) behave this way. Something is not right. Why OpenFOAM Ltd. is not addressing this issue? People has been facing this for a long time.

Jubayer

Hi Jubayer,
This is not the problem with oneEqEddy SGS model. In fact its the problem with the turbulent inlet BC in the pitzDaily tutorial. Somehow the turbulent inlet BC adds random fluctuations which is not correct.
I have used oneEqEddy model with other cases and it works fine.

Regards,
Awais

Hi Awais,

I don't think its the turbulent inlet BC itself. I have tried to use real time history data from the wind tunnel into the simulation. I am getting the same pressure fluctuations. Seems like anything other than steady inlet is creating pressure fluctuations.

Jubayer

Hi Jubayer,
May be your are right. But I didn't observe any problem with oneEqEddy and Smagorinsky for a simulation of flower over a cylinder.
That is why I thought there is nothing wrong with the oneEqEddy model.
One other thing I could think off is that the pitzDaily is 2D tutorial, may be you should try to extend the same case to 3D. With some perriodic BC in spanwise direction. That might remove your doubts.
LES should be strictly a 3 dimensional simulation. 2D you can't really capture all the flow phenomena associated with large eddies.
Whenever you run a 2D LES, openFOAM always generates a warning that case is 2D.

Regards,
Awais

Hi Awais,

Actually the case that I mentioned is a 3D simulation (Flow inside an empty 3d box, like a wind tunnel)

Jubayer

I have submitted a ticket to OpenFOAM. Let's see what they reply. Issue ID number 0000729

Jubayer

Hi Ali,

glad to hear similar voice on the forum. I am wondering whether you have solved that problem. If yes, can you give me some tipes? That would be helpful. I am trying to do similar simulation but it is a DNS turbulent pipe flow, as I described in the other post:

I am doing DNS of heated pipe flow (one phase) with OF 2.2.2. The solver is buoyantpimplefoam. The pipe diameter is 2mm and length of 30D. I use Inflow Generator as inlet U BC (zeroGradient for p_rgh), convective BC (fixedValue for p_rgh) as outlet U BC. On the wall is fixedValue for U and fixedFluxPressure for p_rgh.

Mesh for pipe is O type. Total mesh number is 16 Mio. (y1 plus 0.15 (y1 under 1e6m)), time step is about 2.5e-5. The simulations is running but I observed that solving implicit pressure equation p_rgh withg PCG solver costs extremly high iterations (about 3000). Even with GAMG, the number of iteration reduce, but the simulation time is not shorter. Can anyone tell me the reason? Thanks.

Hi everybody,

Tanzil said that:
I think that means you are plotting the both initial and final pressure in the same graph. that means you are plotting the pressure residuals in every PISO correction.

I suggest you all to check that which pressure residuals (initial/final) did you plot?

Regards,
Mostafa

Hi Adam,

thank you for your reply. I do not know about his situation. But what I mean is the number of iteration of solving pressure equation every time, as I show in the pasted code. Even in my simple DNS pipe flow (D=2mm, L=5D, Re5400, cyclic BC) using pimpleFoma without heating, the number of iteration of solving pressure equation is still high, between 200 to 500.

1-
that's a part of solution. you should plot the last initial pressure, I think.

at first you determine which field you need. f9 means that you use the 9th field in the row, while you start counting with the comma after "solving for p". e.g:

GAMG: Solving for p, Initial residual = 0.193462, Final residual = 1.37372e-05, No Iterations 8

The 9th field in this example would be the number 1.37e-05. (Fields are seperated by a spare field, this is defined by: "by cut -d' '") Therefore you have to check your logfile and decide which field you want to plot. In the normal case this would be the 9th (-> f9).
The number of "N" you have to write is determined by the number of iterations for p per timestep. In my case GAMG iterated p three times, so I have to ignore two iterations and write two Ns. In your case, p is iterated four times, so you should writes three Ns.

hope this can help you

p.s:
2-
are you solving the channel flow using LES? can you share your results with me? I have some problems when I'm using a finer mesh!

Regards,
Mostafa

Hi Mostafa,

thank you for your reply. I will try your methode. What can we tell through the plot of last initial pressure? Should it be decreasing?

What I am doing is the DNS of turbulent pipe flow with Re5400, I would be glad to share the results with you, which Info do you need?

Regards,
Xu Chu

I think it should be decreasing, but flat residuals is one of LES solution features.
is your approach DNS or you are using a LES model?
I'm trying to simulate Moser's paper for Re_tau=395, but when I refined my grids, the secondary vortexes were dissipated and the U+ vs y+ plot didn't look like the Moser's. although for a coarse grid, the results are approximately the same as Moser's!

My simulation is DNS,not LES. I checked my U+ and y+, it is similar as Eggels and Wu at similar Re. I have about 4 Mio. cells for L=5D, y1+ about 0.15

I plot my initial residual of last pressure correction in every time step, it seems that it swings, and stay in the scale of 1e-1, which is high. Could that be the reason of high number of iteration in the pressure equation?

Hi,

Has anyone else experienced this situation? I'm using the turbulentInlet BC and getting crazy pressure fluctuations all over my domain which is not physical. I need pressure data of my domain and they are getting buried in this unrealistic fluctuations.

Will appreciate any help.

I think what you are talking about is known as 'checkerboarding', a problem occuring on colocated meshes where velocity and pressure become decoupled and pressure field becomes physically unrealistic. There is another thread about it here:
http://www.cfd-online.com/Forums/mai...d-problem.html

I had a problem like this and solved it by making my mesh much finer.

Openfoam uses a Rhie-Chow pressure velocity coupling:
http://www.cfd-online.com/Wiki/Veloc...ssure_coupling
So checkerboard pressure is not the case. The problem is divergence of the velocity (when interpolated or randomly generated) is not zero. The pressure correction step is based on continuity residual and this throws off the pressure at inlet. Usually inlet P BC is zero gradient and outlet is fixedvalue, which makes a nice constant slope gradient of pressure all the way from inlet to outlet.

There's a new BC on foam16 named turbulentDFSEMinlet, but I'm having trouble using it when I scale my problem. Also there's another method called flow rescaling (mentioned in Poletto's paper) that contains the unphysical pressure to inlet rather than the whole domain but I couldn't find much about it.

I noticed that a zeroGradient(not uncommon in LES) velocity outlet does generate this problem. What boundary conditions are you using?
The original pitzDaily with turbulent inlet fluctuations makes use of the inletOutlet for the outlet velocity. I can imagine that a zeroGradient outlet reflects the pressure fluctuations back into the domain, generating these unexpected fluctuations.

Dear Foamer,

I'm stuck in this problem now :confused::confused::confused:. Does anyone of you find a solution for this problem? the problem is this pressure fluctuations affect on the behavior of the velocity fluctuation so I can't get accurate results even for the velocity

Thanks in advance

Mohamed

I recommend st start with small fluctuations and look where the fluctuations arise form. Typical it is a boundary. You may think about the b.c. then.

Dear Uwe,

the problem is the inlet boundary condition is a multi equation B.C and its values differs from t1 to t2 according to the value of this difference the pressure fluctuations make this problem. but still I'm working on it now to apply a time filter to control the value of the velocity fluctuation in each time step.

Thanks

Mohamed

Some commments:

1. If you are simulating turbulent flows, where fluctuations are resolved up to some sgs scale, why you find it strange to get fluctuations in one of the fields (p)? Have you made statistics on the pressure? Plotting the power spectrum of pressure should tell you whether the field is "correct".

2. Using schemes other than CD for "explicit" LES in OF is not correct. Youll be producing "aliasing errors" in the field.

3. Monitoring convergence when doing transient simulations is rather useless. You should consider monitoring mass conservation along with some volume average quantity (tke, helicity) to see "convergence.

4. Using Co = 0.5 is rather high for LES/DNS, specially on an algorithm like PISO which has an inconsistent treatment of the convective term. You want to keep Co ~ 0.1.

My 0.02 cents

Dear Santigo,

Thanks for your comments. I'm using LES with CD scheme (Linear) with the algorithm pimple. In my trials I'm keeping the Co under 0.1 as you said but still the problem is that at some output time steps the pressure at the outlet is higher than that one at the inlet. and this affects the statistics of the velocity such as the decay of the homogeneous turbulence which I'm trying to get the output is not smooth and not identical even after the average in time and space. like the attached curves.

I tried to use Advection outlet B.C for the velocity but still the same.

I forgot what case are you trying to solve. Can you please tell me again with more details? I'd be also nice to have some details about the grid, LES model for sgs fluxes, BCs, and how you are forcing the flow.

One last thing, don't use PIMPLE unless you have a very bad grid and/or complex geometry. Use it as last resort. Go to PISO instead.

Dear Santiago,

I'm using OF-v1612+ and trying to get bypass transition in a rectangular channel. So I'm implementing an inlet B.C which gives isotropic homogeneous turbulence with control of many parameters. I'm using LES pimpleFoam as a solver and pimple algorithm with WALE as a SGS. the mesh is not complex as all of it are hex.

The problem is that at some output time steps it gives pressure at the outlet higher than that of the inlet without any back flow and this affects the turbulence statics during the channel.

I tried many outlet B.Cs fro the velocity and the pressure (it supposed that the normal is zeroGradient for the velocity and fixed value (zero) for the pressure) but the case still exist.

For the schemes I'm using CD schemes. and the Co in most cases not exceed 0.1

Could you please tell me if you need any extra data about the case?

Thanks in advance

Mohamed

Continuity in incompressible LES
 

Dear all,

I also observed the previously described pressure fluctuations in the domain of incompressible LES. After thinking about it and doing some testing, I came to the conclusion that this pressure fluctuation makes sense. Due to the time dependent inlet velocity, the mass inflow is also time dependent. When the mass flow decreases, the fluid has to be decelerated (continiuity in the incompressible case). This is achieved by a positive pressure gradient over the domain. This is why sometimes the outlet pressure is higher than the inlet pressure. The temporal average of the pressure gradient however is still negative.

I hope these thoughts are of some help to future forum visitors.

Dear Aaron,

Thanks for your reply. Actually it's totally true what you mentioned. but in my case the problem was that the mean pressure gradient was also fluctuated between positive and negative.

After many trials, I managed this problem by adding a correction factor for the velocity to keep constant Average mass flow rate (continuity) at the inlet of the channel.

Thanks

Mohamed

@Jublayer:

Hi, what was the outcome of the ticket? There is no information visible when searching for the issue ID ... except that it seems to be no bug ...

Greetings

Thanks for the kind reply. Did you find the reason for high iterations of pressure. Is there any method to cut the cost of running time? Thank you.

Thank you for your comment.
The time step in my DNS case is 3e-6 and I think it is relatively small. However, the max courant number is between 0.3 and 0.4. So should I decrease the time step to keep Co ~ 1? If the Co is not that low, cannot the case reach converged? Thank you.