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

why pisoFoam take such a long time to converge?

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

Like Tree6Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 18, 2013, 03:49
Default
  #21
New Member
 
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12
DaSh is on a distinguished road
I understand what you mean Haakon. Of course the Taylor Couette Flow (in my case) will have a steady state solution at some point, e.g. turbulent taylor vortices. I am pretty sure, that it should work with pisoFoam. My time step is actually large. It is 0,05, which should be ok, looking at the courant number (alway < 0,45).
DaSh is offline   Reply With Quote

Old   October 18, 2013, 04:12
Default
  #22
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
DaSh, pisoFoam just does a single iteration each time step (solving momentum and turbulence equation just once). In every unsteady simulation the solution (U, p, k, ...) changes to the next time step so residuals are increased. The piso step will again reduce them and so on.
Now comes a part about how I understand it, so don't take it too serious:
After some reduction of the initial error during the first iterations, there will be an equilibrium of your flow - increasing the residual each time step - and the piso solver - reducing the residual each time step.

If the time step is too large, the introduced error will be large an thus pisoFoam might be not able to handle this: the simulation will diverge or give completely garbage results.
If the time step is small, the introduced error will be small. Then three things can happen:
1) Piso will hit exactly the amount of error and the residual keeps constant from time step to time step.
2) Piso is better. The residual will fall until 1). This will happen, as every iterative procedure gets worse for falling residuals.
3) Piso is worse. The redisuals will go up until 1). Piso gets better - same reason as in 2).

Result:
If you want your residuals to be lower - you need to decrease your time step.
DaSh and allanZHONG like this.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 04:31
Default
  #23
New Member
 
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12
DaSh is on a distinguished road
Thank you for your reply. I understand what you mean and it seems logical. So the point where I am wrong is, that a falling residual does not indicate "where my simulation is". So the flow can change with time going by, although my residual did stop dropping. Because as I get it, it really just gives indication of the error of the current result. So, if I want to reduce the error, I lower the time step. But for my simulation to advance in matters of transition, it will not help?!
DaSh is offline   Reply With Quote

Old   October 18, 2013, 04:36
Default
  #24
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by DaSh View Post
Because as I get it, it really just gives indication of the error of the current result. So, if I want to reduce the error, I lower the time step.
Yes, that's what I think, too.

I don't understand what you mean by your very last sentence (not quoted here).
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 04:47
Default
  #25
New Member
 
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12
DaSh is on a distinguished road
What I mean: As I simulate a transient flow, I should see several stages of flow over the time being. So, a lowering residual is not an indicator for the flow changing its course or appearance.

And thus, my residual, as it is stable/constant, does not indicate, that my flow will not change any further. I just have to wait longer.
DaSh is offline   Reply With Quote

Old   October 18, 2013, 04:53
Default
  #26
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
Ok, but your flow is transient - so it will never stop changing right?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 05:00
Default
  #27
New Member
 
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12
DaSh is on a distinguished road
As I get it, a Taylor Couette Flow should have a steady state solution in turbulent Taylor Voritces. Of course there will be fluctuations in it but it will not change its form again. For the Reynolds number I applied, there should no further instability after turbulent Vortex Flow (e.g. like higher classes of chaos).

Or am I getting something wrong in matters of definition?
DaSh is offline   Reply With Quote

Old   October 18, 2013, 06:04
Default
  #28
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
But if you do LES these fluctuations are resolved and thus keep the residuals to a certain level. I guess, if you do the same thing with any RANS model residuals will keep falling once the large vorticies are there (as some kind of pseudo-transient PISO).
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 06:14
Default
  #29
New Member
 
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12
DaSh is on a distinguished road
Yes, I guess you are right. What matters most for my simulation, is, that although my residual seems to be almost constant, as there are no voritces, it doesn't mean, that they won't come in the future of the simulation.
dickcruz likes this.
DaSh is offline   Reply With Quote

Old   October 18, 2013, 08:46
Default
  #30
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
helloo

I am sorry for late reply..

But finally My solution with simpleFoam converge..

I used a fv schemes and fv solution as below.. and attached is my converged results.. As we can all see its not good at all!...

I nEED HELP BADLY


Quote:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss limitedLinearV 1;
div(phi,k) Gauss limitedLinear 1;
div(phi,epsilon) Gauss limitedLinear 1;
div(phi,R) Gauss limitedLinear 1;
div(R) Gauss linear;
div(phi,nuTilda) Gauss limitedLinear 1;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(U) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p ;
}


// ************************************************** *********************** //

Quote:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{

solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}


U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

epsilon
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}


}

SIMPLE
{
nNonOrthogonalCorrectors 0;

residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega)" 1e-3;
}
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
epsilon 0.7;
}
}

cache
{
grad(U);
}


// ************************************************** *********************** //

Last edited by izna; October 22, 2013 at 10:46.
izna is offline   Reply With Quote

Old   October 18, 2013, 09:08
Default
  #31
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
The log output is still missing.

You really can not expect this to converge. You set everything to linear, gradients have no limiters and so on. You need to get a stable, robust setting and then you can try to make it numerically more accurat. But don't start with this second order low diffusion stuff.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 09:36
Default
  #32
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
look can you please post for me a fv scheme and fv solution fiting for this? ANd i assure you it converged..
izna is offline   Reply With Quote

Old   October 18, 2013, 09:40
Default
  #33
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
log output you mean the graph of iterations?
izna is offline   Reply With Quote

Old   October 18, 2013, 09:41
Default
  #34
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
No, I mean the terminal or log file output that is created during the calculation.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 09:44
Default
  #35
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
but i do not have it with me.. once convegence was acheived.. i check in paraview an then close it all..

can you please give em a good Fv scheme and fv solution?
izna is offline   Reply With Quote

Old   October 18, 2013, 09:46
Default
  #36
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
This doesn't make any sense. I can just guess what might be the reason without the output.
Do you use simple now or still piso?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 09:48
Default
  #37
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
i use simpleFOam...
izna is offline   Reply With Quote

Old   October 18, 2013, 09:51
Default
  #38
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.2.1-57f3c3617a2d
Exec : simpleFoam
Date : Oct 18 2013
Time : 17:49:50
Host : "izna-MS-7592"
PID : 30710
Case : /home/izna/Desktop/me
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 1499

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}

No finite volume options present


SIMPLE: convergence criteria
field p tolerance 0.01
field U tolerance 0.001
field "(k|epsilon)" tolerance 0.001


Starting time loop

Time = 1500

smoothSolver: Solving for Ux, Initial residual = 0.000272676180903, Final residual = 2.21277453827e-05, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.000199629444124, Final residual = 1.62625348368e-05, No Iterations 4
GAMG: Solving for p, Initial residual = 0.00956741607883, Final residual = 0.000397412644069, No Iterations 69
GAMG: Solving for p, Initial residual = 0.000251084793744, Final residual = 1.14590103449e-05, No Iterations 6
GAMG: Solving for p, Initial residual = 2.62606828603e-05, Final residual = 1.25053629257e-06, No Iterations 45
time step continuity errors : sum local = 4.68359960217e-07, global = -4.67471740526e-11, cumulative = -4.67471740526e-11
smoothSolver: Solving for epsilon, Initial residual = 1.66731195606e-05, Final residual = 6.60718162715e-06, No Iterations 1
smoothSolver: Solving for k, Initial residual = 0.000849113107756, Final residual = 6.98826517851e-05, No Iterations 4
ExecutionTime = 46.82 s ClockTime = 47 s


SIMPLE solution converged in 1500 iterations

End


HI i have run it again.. and this is the resutl
izna is offline   Reply With Quote

Old   October 18, 2013, 09:56
Default
  #39
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26
RodriguezFatz will become famous soon enough
Well, I would try:

Code:
ddtSchemes
{
    default steadyState;
}
gradSchemes
{
    default            faceLimited edgeCellsLeastSquares 1; // or faceLimited Gauss linear 1.0;
}
divSchemes
{
default         Gauss upwind phi;
}
//keep the rest from your file
Also use GAMG for pressure:
Code:
p
    {
        solver           GAMG;
        tolerance        1e-6;
        relTol            0.01;
       maxIter         100;    

        smoother         DICGaussSeidel;
    

    
    //simple:
        nPreSweeps       0;
        nPostSweeps      1;
    nFinestSweeps    2;

        cacheAgglomeration true;

        nCellsInCoarsestLevel 50;
        agglomerator     faceAreaPair;
        mergeLevels      1;
    };
Did you think about what hakoon said? Namely that your flow just is transient and thus simple won't converge to steady-state? What is this simulation about?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   October 18, 2013, 09:58
Default
  #40
Senior Member
 
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12
izna is on a distinguished road
hi

i am simulating a 2D case and observing the flow pattern of wind around some rectangular shapes...
izna is offline   Reply With Quote

Reply

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Unstabil Simulation with chtMultiRegionFoam mbay101 OpenFOAM Running, Solving & CFD 13 December 28, 2013 13:12
same geometry,structured and unstructured mesh,different behaviour. sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 22:40
PisoFoam case terminating Solo Sails OpenFOAM Running, Solving & CFD 3 November 29, 2011 07:04
calculation diverge after continue to run zhajingjing OpenFOAM 0 April 28, 2010 04:35


All times are GMT -4. The time now is 09:15.