CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Fluctuating Pressure Fields (LES-pisoFoam)

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree10Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 13, 2014, 08:23
Default
  #21
mgg
New Member
 
Join Date: Nov 2012
Posts: 27
Rep Power: 11
mgg is on a distinguished road
Quote:
Originally Posted by adambarfi View Post
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
mgg is offline   Reply With Quote

Old   July 13, 2014, 08:52
Default
  #22
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 322
Rep Power: 13
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by mgg View Post
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!
adambarfi is offline   Reply With Quote

Old   July 13, 2014, 09:15
Default
  #23
mgg
New Member
 
Join Date: Nov 2012
Posts: 27
Rep Power: 11
mgg is on a distinguished road
Quote:
Originally Posted by adambarfi View Post
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
Attached Images
File Type: jpg Bild1.jpg (21.3 KB, 80 views)
mgg is offline   Reply With Quote

Old   July 13, 2014, 11:07
Default
  #24
mgg
New Member
 
Join Date: Nov 2012
Posts: 27
Rep Power: 11
mgg is on a distinguished road
Quote:
Originally Posted by adambarfi View Post
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?
Attached Images
File Type: jpg Residual.jpg (58.5 KB, 92 views)
mgg is offline   Reply With Quote

Old   August 30, 2016, 15:08
Default
  #25
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 16
anishtain4 is on a distinguished road
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.
anishtain4 is offline   Reply With Quote

Old   November 3, 2016, 16:17
Default
  #26
Member
 
Declan
Join Date: Oct 2016
Location: Ireland
Posts: 40
Rep Power: 7
decah is on a distinguished road
Quote:
Originally Posted by fluentfreak View Post
Not yet
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.
decah is offline   Reply With Quote

Old   November 16, 2016, 11:48
Default
  #27
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 16
anishtain4 is on a distinguished road
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.
MrBeneS likes this.
anishtain4 is offline   Reply With Quote

Old   June 7, 2017, 08:42
Default
  #28
JDS
New Member
 
Jorden
Join Date: Mar 2016
Posts: 1
Rep Power: 0
JDS is on a distinguished road
Quote:
Originally Posted by fluentfreak View Post
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.
JDS is offline   Reply With Quote

Old   March 14, 2018, 05:48
Default
  #29
Member
 
Mohamed Elghorab
Join Date: May 2016
Location: Coventry, Engalnd
Posts: 41
Rep Power: 8
crazzy.pirate43 is on a distinguished road
Dear Foamer,

I'm stuck in this problem now . 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
crazzy.pirate43 is offline   Reply With Quote

Old   March 14, 2018, 06:23
Default
  #30
Senior Member
 
piu58's Avatar
 
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 727
Rep Power: 13
piu58 is on a distinguished road
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.
__________________
Uwe Pilz
--
Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)
piu58 is offline   Reply With Quote

Old   March 14, 2018, 09:58
Default
  #31
Member
 
Mohamed Elghorab
Join Date: May 2016
Location: Coventry, Engalnd
Posts: 41
Rep Power: 8
crazzy.pirate43 is on a distinguished road
Quote:
Originally Posted by piu58 View Post
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
crazzy.pirate43 is offline   Reply With Quote

Old   March 15, 2018, 02:28
Default
  #32
Senior Member
 
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 351
Rep Power: 13
Santiago is on a distinguished road
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
Santiago is offline   Reply With Quote

Old   March 16, 2018, 07:05
Default
  #33
Member
 
Mohamed Elghorab
Join Date: May 2016
Location: Coventry, Engalnd
Posts: 41
Rep Power: 8
crazzy.pirate43 is on a distinguished road
Quote:
Originally Posted by Santiago View Post
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.
Attached Images
File Type: png 1.png (33.8 KB, 44 views)
crazzy.pirate43 is offline   Reply With Quote

Old   March 16, 2018, 07:17
Default
  #34
Senior Member
 
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 351
Rep Power: 13
Santiago is on a distinguished road
Quote:
Originally Posted by crazzy.pirate43 View Post
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.
Santiago is offline   Reply With Quote

Old   March 16, 2018, 09:24
Default
  #35
Member
 
Mohamed Elghorab
Join Date: May 2016
Location: Coventry, Engalnd
Posts: 41
Rep Power: 8
crazzy.pirate43 is on a distinguished road
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
crazzy.pirate43 is offline   Reply With Quote

Old   June 19, 2018, 07:53
Default Continuity in incompressible LES
  #36
New Member
 
Aaron Endres
Join Date: Jun 2016
Posts: 11
Rep Power: 8
aendres is on a distinguished road
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.
MrBeneS likes this.
aendres is offline   Reply With Quote

Old   June 19, 2018, 08:27
Default
  #37
Member
 
Mohamed Elghorab
Join Date: May 2016
Location: Coventry, Engalnd
Posts: 41
Rep Power: 8
crazzy.pirate43 is on a distinguished road
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
crazzy.pirate43 is offline   Reply With Quote

Old   August 14, 2018, 08:40
Default
  #38
Member
 
Join Date: Nov 2013
Posts: 35
Rep Power: 10
beatlejuice is on a distinguished road
Quote:
Originally Posted by cm_jubayer View Post
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
beatlejuice is offline   Reply With Quote

Old   June 2, 2019, 23:27
Default
  #39
Senior Member
 
Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 6
calf.Z is on a distinguished road
Quote:
Originally Posted by mgg View Post
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 is offline   Reply With Quote

Old   October 31, 2019, 06:53
Default
  #40
Senior Member
 
Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 6
calf.Z is on a distinguished road
Quote:
Originally Posted by Santiago View Post
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.
calf.Z is offline   Reply With Quote

Reply

Tags
fluctuation, les, pisofoam, pressure

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Pressure BC for combustion chamber Giuki FLUENT 1 July 19, 2011 11:35
Fluctuating pressure field vw.cfd OpenFOAM 1 February 8, 2011 06:12
Pressure enigma. Sara Main CFD Forum 22 July 30, 2009 04:46
Hydrostatic pressure in 2-phase flow modeling (long) DS & HB Main CFD Forum 0 January 8, 2000 15:00


All times are GMT -4. The time now is 13:09.