CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Improve simpleFoam convergence (http://www.cfd-online.com/Forums/openfoam-solving/78354-improve-simplefoam-convergence.html)

Daniele111 July 19, 2010 14:08

Improve simpleFoam convergence
 
Hi
How can I improve simpleFoam convergenge? Now time simulation is 30min, can i improve it?

Thanks

matejfor July 20, 2010 02:40

Sure you can. Have a faster computer.
No, well, yes, you can make it run faster but you need to give us more information. Your question could be paraphrased as: "I have a car and it takes 30 minutes to get to work, could it be faster?"

Post here fvSchemes, fvSolution, and screenshot of the residual plot, tell us what is the case (turbulent? what is Re?,backward facing step or swirler or flow around car, plane, building, channel flow), what are the BCs and if the variables (like velocity) are oscillating (e.g. post a plot of a velocity probe).

matej

Daniele111 July 20, 2010 05:25

2 Attachment(s)
:) you're right!! And I like your metaphor! It is a turbulent case (k-epilon model). It is similar to a backward facing step, i have a atmospheric bl with a obstacle on bottom.

top bottom outlet inlet
k symmetry wallFunction zerogradient fixed value
U symmetry 0 zerogradient log profile
p symmetry zerogradient 0 zerogradient
eps symmetry wallfunction zerogradient imposed profile

Thanks

MartinB July 20, 2010 05:59

Hi Daniele,

I would reduce the relaxation factors to:
Code:

relaxationFactors
{
    p              0.3;
    U              0.7;
    k              0.5;
    epsilon        0.5;
    R              0.5;
    nuTilda        0.5;
}

And I would change the solvers to:
Code:

    p
    {
        solver          GAMG;
        tolerance        1e-7;
        relTol          0.001;
        minIter          5;
        maxIter          100;
        smoother        GaussSeidel; // DIC; //DICGaussSeidel; //FDIC;
        nPreSweeps      1;
        nPostSweeps      3;
        nFinestSweeps    3;
        scaleCorrection true;
        directSolveCoarsest false;
        cacheAgglomeration on;
        nCellsInCoarsestLevel 50;    // 500
        agglomerator    faceAreaPair;
        mergeLevels      1;    // 3
    }
   
    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance        1e-6;
        relTol          0.01;
        nSweeps          1;
        maxIter        100;
    };

The solvers for k, epsilon, R and nuTilda the same as for U.

Martin

Daniele111 July 20, 2010 06:44

1 Attachment(s)
Thanks
The execution time is reduced from 2239 sec to 662, but after the obstacle the solution it isn't accurate

Daniele

MartinB July 20, 2010 06:53

Hi Daniele,
your convergence criteria in fvSolution with 1e-3 is rather low...
Restart your simulation from the latest timestep with convergence criteria of 1e-5.
Martin

Daniele111 July 20, 2010 07:03

Thanks
I try it. Uhm In my project the obstacle on the bottom change its position, and then i calculate new solution at new position, this is do in a evolutive algorithm, so the iteration after the first must be very fast less than a minute. can i initialize the new mesh with the last time of previous simulation?

Daniele

MartinB July 20, 2010 07:25

I think, you can use the "mapFields" utility.
With "mapFields -help" you can see the parameters necessary.
In your "system" directory you need a file "mapFieldsDict":

Code:

/*--------------------------------*- C++ -*----------------------------------*\\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.6                                  |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      mapFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// This dictionary is necessary to map fields from another simulation to this
// one. The results from the source will be interpolated to the mesh in this
// case directory.
// Usually patchMap and cuttingPatches will be empty.
// In the case that you want to use the output of one simulation as the
// input for the next one, define patchMap as (inlet outlet).

patchMap        (  );  // usually empty
cuttingPatches  (  );

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

Navigate to your new (!) case directory.

Use the mapFields command like this:
mapFields /home/daniele/workinghere/firstRun -sourceTime 1234

Check the mapped results with paraFoam.

Start the simulation in your new case directory.

Martin

Daniele111 July 20, 2010 09:54

Hi
If I start new simulation with last time of the previous simulation time execution is 93s... I would about 30s 40s; if I use mapfield time execution is 400s. There is a thing that I dont understand: I start a simulation, then I copy last time directory in 0 directory, and restart the same case, and time execution is 30s, but if I start from solution because time is so high?

MartinB July 20, 2010 10:52

It's not necessary to copy last time directory to "0" directory, you can edit the "system/controlDict" to start from your latest time directory:
Code:

startFrom      startTime;              //  firstTime, startTime, latestTime
startTime      0;                      //  set > 0 to continue

Replace "startFrom startTime;" with "startFrom latestTime;" and the simulation continues.
Or replace "startTime 0;" with "startTime 1000;" to start from iteration 1000.

You can use the mapField command with the parameter "-consistent" if your mesh is exactly the same. Otherwise if the meshes are different, the values are interpolated and the solver needs some time steps to adjust the solution again.

May be I didn't understand your questions right... you don't speak german, do you?

Martin

Daniele111 July 20, 2010 11:28

I understand. I try it. Two mesh are very similar, top inlet and outlet are identical, the obstacle position on bottom si traslate of some cm.
I did a simulation, and then I start a new simulation with the same mesh but startTime is latestTime of previous sim, and time execution is 40s, is normal? I don't change nothing, and i start from convergence solution, time execution should not be faster?

p.s i don't speak german, and my english is very bad...you are very kind, and your advice are very useful.

MartinB July 20, 2010 12:23

It's difficult to say if 40s is normal: usually one can observe that the time necessary for a single iteration step (i.e. solving for Ux, Uy, Uz, p ...) is higher in the beginning of the simulation (at least for a steady state simpleFoam simulation). With reaching convergence the time for each single iteration step drops significantly.

Next to the time used for a single iteration step the number of iterations used to reach convergence is important. For my simulations here (simpleFoam without turbulence) I get convergence in a "fresh" simulation after 800 iterations. When using mapFields I can reduce the number of iterations to 400 iterations, although the first few single iteration steps do need the same execution time.

Another important issue in your case is the question: when is your simulation converged good enough? I think a convergence tolerance of 1e-3 is not enough, but may be, 1e-4 is fine and 1e-5 is an overkill? You can save quite a lot of iterations as soon as you know which accuracy you really need...

Some more ideas to speed up your simulations:
Are you running your simulation in parallel mode? If not, and if you have a multicore or multiprocessor machine, use the parallelism!
An important parameter which reduce the number of iterations is the relaxation factor: you can try to increase these factors!
If you are familiar with OpenFOAM's c++ programming language you might try to use an dynamically increasing relaxation factor during runtime. There is at least one thread in this forum where this idea is discussed.

If you can't speed up the simulations time directly you can try to use your hardware more efficiently: create a shell script or a python script that runs dozens of simulations over night. I use this technique quite often... automatic mesh creation with blockMesh is not hard, and with the "sample" utility you can do automatic postprocessing, too.

Hope these ideas are useful

Martin

MartinB July 20, 2010 14:06

Here are some more ideas:
I suppose you are using hexahedra elements. If not, try switching to hexahedra.

Reduce the mesh size, i.e. the number of elements. Run your simulation until convergence. Then use a finer mesh and map the previous results...

Optimize your mesh so it really fits the needs of your case: a fine mesh in the important areas (behind the obstacle for example), a coarser mesh elsewhere.

With the refineMesh utility you can refine the whole mesh immediately. With refineWallLayer you can split the cells next to a patch. If you have hexahedra and you want to refine locally only, I can upload an utility...

Although this is usually done to avoid divergence in complex cases: run simpleFoam without turbulence first, at least for let's say 200 iterations. Then switch on turbulence and continue the simulation.

For my previous suggestion of using mapFields you can try this: just use U and p for the mapping and leave the turbulence fields.

Of course you can combine some of these strategies, too...

Martin

matejfor July 21, 2010 02:50

Daniele,
martin gave you extensive advice to which there's not much to add.
Just a few bits:

a) the precision of the result - using upwind scheme for convection terms will gain you speed, but not precision. The good news is, you may change the scheme on the fly using some utility or script.
Other issue with precision might be the use of k-eps model and consequently wall functions in OpenFOAM.

b) I understand that you have solved solution, then you move the obstacle, map thesolution and run. well your solution is converged, but the flowfield is different as the obstacle is moved so the solution will take a little longer at the beginning. Alternativelly to Martin's suggestion with switching off the turbulence, I would make it bit easier with changing the viscosity which means changing the turbulence level.

You are after two rabbits here. The precision one is going one direction while the speedy one is running slightly other direction. It's hard to get both at the same time.


good luck
matej

Daniele111 July 21, 2010 03:00

Dear Martin

Thanks for everything. You were very patient and kind to me. I try different and valuable advice you gave me.

Daniele

Daniele111 July 22, 2010 07:08

Hi
I refine my mesh only where is necessary and i reduce my domain size. I calculated a first solution with a convergence tolerance of 1e-4, and solution is very good. I try to increase tolerance (1e-3,1e-2) for the following simulation that I inizialized with mapFields, and the time simulation is very good 20s, and 10s, and the solution quality is good. Is it wrong calculate the new solution from a solution more precise,but raising tolerance?

Daniele

MartinB July 22, 2010 07:24

Hi Daniele,
it is not wrong, but you should be aware of the results quality!
Try this: write your results every 50th iteration. You can do this with the following entry in "system/controlDict":
writeInterval 50;

Then check the results in paraview, i.e. have a careful look at how much the results change from let's say timestep 200 to timestep 250, or timestep 200 to 800... it is useful to reduce the number of colors to 10 (in Color Scale Editor, enable "Discrete Colors" with Solution of 10). You can see the amount of change in the fields... then decide for your particular problem, if it is ok or not.

I am doing flow channel shape optimization here, and I can say quite early if the new geometry is better or worse than the latter one. But when reaching the optimum, I must decrease the convergence tolerances more and more.

Martin

matejfor July 22, 2010 07:28

It is completely wrong. You've chosen the wrong rabbit to chase. The tolerance we are talking about is the tolerance with which the solver solves the linearized set of N-S equations. When you release the tolerance, the solver will be faster, but the price....
You can play with a tolerance but when you want reliable solution you should lower it back towards the end of the solution of each of your case.

good luck
matej

Daniele111 July 22, 2010 07:38

Dear Matey
But if i inizialized my simulation with a field very precise, I must not use necessarily a very low tolerance or not?

Daniele111 July 22, 2010 08:02

1 Attachment(s)
Post my solution. The source for mapfields utility is the same for all. I change tolerance convergence.


All times are GMT -4. The time now is 11:09.