[sourav90]

Dear FOAMers,

Sometimes I feel the need to change the writeInterval from prior knowledge & in stead of modifying the controlDict every time, I wonder if it's possible to do like this:

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application         particleFoam;

startFrom           startTime;
startTime           0;
stopAt               endTime;
endTime            1000;

deltaT                1e-1;
writeControl        runTime;
// writeInterval       10;

// my wish :) 
writeInterval      table
(
    (0           1) // start with interval of 1
    (10       10) // from T=10, writeInterval 10
    (1000   50) // use 50 from T=10 until the end
);


purgeWrite          0;
writeFormat         binary;
writePrecision      6;
writeCompression    off;

timeFormat          general;
timePrecision       6;
runTimeModifiable   yes;

functions{
... 


I find two similar examples, but applicable for other objects

1. HIstorically, page 9 of this example shows such implimentation: https://www.dhcae-tools.com/images/d...rcelSolver.pdf
2. Time-varied boundary condition table: This is presently available as options in current OpenFOAM distribution: 2nd or 3rd example in section 5.2.3.4 of https://cfd.direct/openfoam/user-gui...25-1790005.2.2
   
   

   inlet 
   { 
       type         uniformFixedValue; 
       uniformValue table ((0 0) (10 2)); 
   }

Anyone knows if it's possible, or how to implement? thanks.

[sourav90]

Thanks to MartinB, who provided this working example of using functionObject in controlDict.

PHP Code:

/*--------------------------------*- C++ -*----------------------------------*\
  | =========                 |                                                 |
  | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
  |  \\    /   O peration     | Version:  v2006                                 |
  |   \\  /    A nd           | Website:  www.openfoam.com                      |
  |    \\/     M anipulation  |                                                 |
  \*---------------------------------------------------------------------------*/
  FoamFile
  {
      version     2.0;
      format      ascii;
      class       dictionary;
      location    "system";
      object      controlDict;
  }
  // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

  application     simpleFoam;

  startFrom       startTime;

  startTime       0;

  stopAt          endTime;

  endTime         2000;

  deltaT          1;

  writeControl    timeStep;

  writeInterval   100000; // <------ big number

  purgeWrite      0;

  writeFormat     ascii;

  writePrecision  6;

  writeCompression off;

  timeFormat      general;

  timePrecision   6;

  runTimeModifiable true;

  functions
  {
      userWriteInterval
      {
          type coded;
          libs            ("libutilityFunctionObjects.so");
          name writeInterval;

          code
          #{
          #};

          codeExecute
          #{
              const Time& runTime = mesh().time();
              scalar myWriteInterval(1);

              // better logic here:
              // for example with a function1
              if (runTime.value() > 10)
              {
                  myWriteInterval = 10;
              }
              if (runTime.value() > 50)
              {
                  myWriteInterval = 50;
              }

              if (!(runTime.timeIndex() % label(myWriteInterval)))
              {
                  const_cast<Time&>(runTime).writeNow();
              }
          #};
      }

  }

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


The `$FOAM_INST_DIR/OpenFOAM-x/applications/test/Function1` can be referred if someone understands the C++ code well enough

[AtoHM]

Thanks for providing the solution here.

Just one question, as I am not very skilled at understanding c++: it seems from my test, that the writeInterval set here does act on the iteration number and not the physical time.
How can I make sure, that output is written at fixed physical time intervals? Example: with the current setting lets say I provided writeInterval of 100. The solver dt varies between 0.0012 and 0.0018. This causes output in the physical interval of 0.12 - 0.18 s depending on the intermediate time steps.
What do I have to change, that the provided writeInterval is interpreted as the physical interval?

[courant_numero_uno]

You could change "writeInterval" to "runTime" in the code above, and adjust the if statement switches as you wish.
writeControl can write based on several criteria, see below for 2112.
https://www.openfoam.com/documentati...n-objects.html