CFD Online Discussion Forums
Page 2 of 3 1 2 3
Show 40 post(s) from this thread on one page

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Fluctuating Pressure Fields (LES-pisoFoam) (https://www.cfd-online.com/Forums/openfoam-solving/97779-fluctuating-pressure-fields-les-pisofoam.html)

mgg July 13, 2014 08:23
Quote:
Originally Posted by adambarfi (Post 501319)
1-
that's a part of solution. you should plot the last initial pressure, I think.

Code:
cat log | grep 'Solving for p' | cut -d' ' -f9 | sed -n 'p;N;N;N;N' | tr -d ','" title 'p' with lines
or
cat log | grep 'Solving for p' | cut -d' ' -f13 | sed -n 'p;N;N;N;N' | tr -d ','" title 'p' with lines
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

adambarfi July 13, 2014 08:52
Quote:
Originally Posted by mgg (Post 501331)
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!

mgg July 13, 2014 09:15
1 Attachment(s)
Quote:
Originally Posted by adambarfi (Post 501332)
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

mgg July 13, 2014 11:07
1 Attachment(s)
Quote:
Originally Posted by adambarfi (Post 501332)
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!
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?

anishtain4 August 30, 2016 15:08
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.

decah November 3, 2016 16:17
Quote:
Originally Posted by fluentfreak (Post 354245)
Not yet :confused:
But I will post an update when I make it right!
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.

anishtain4 November 16, 2016 11:48
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.

JDS June 7, 2017 08:42
Quote:
Originally Posted by fluentfreak (Post 346179)
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.
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.

crazzy.pirate43 March 14, 2018 05:48
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

piu58 March 14, 2018 06:23
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.

crazzy.pirate43 March 14, 2018 09:58
Quote:
Originally Posted by piu58 (Post 685141)
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

Santiago March 15, 2018 02:28
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

crazzy.pirate43 March 16, 2018 07:05
1 Attachment(s)
Quote:
Originally Posted by Santiago (Post 685260)
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.

Santiago March 16, 2018 07:17
Quote:
Originally Posted by crazzy.pirate43 (Post 685431)
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.

crazzy.pirate43 March 16, 2018 09:24
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

aendres June 19, 2018 07:53
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.

crazzy.pirate43 June 19, 2018 08:27
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

beatlejuice August 14, 2018 08:40
Quote:
Originally Posted by cm_jubayer (Post 404825)
I have submitted a ticket to OpenFOAM. Let's see what they reply. Issue ID number 0000729

Jubayer
@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

calf.Z June 2, 2019 23:27
Quote:
Originally Posted by mgg (Post 501297)
Hi Ali,

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.
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.

calf.Z October 31, 2019 06:53
Quote:
Originally Posted by Santiago (Post 685260)
Some commments:

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
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.


All times are GMT -4. The time now is 09:55.
Page 2 of 3 1 2 3
Show 40 post(s) from this thread on one page