OpenFOAM® User Upgrade Guide

OpenFOAM®  User Upgrade Guide

Note: this is a work-in-progress and will be updated in the near future

This guide is for OpenFOAM users looking for assistance in upgrading their cases to more recent versions of OpenFOAM.

Changes for OpenFOAM v1806

Main system/controlDict
  • writeCompression off (instead of uncompreessed method)

Moving mesh solvers
  • Functionality from many moving mesh solvers promoted to their static mesh equivalents - see v1806 release notes

Meshing

Changes for OpenFOAM v1712

Solver
  • chtMultiRegion solvers: system/fvSolution file is now mandatory

Input dictionaries
  • special treatment for the dictionary include keyword has now been removed after being deprecated many versions ago.

Utilities
  • applyBoundaryLayer: writing the turbulence viscosity field nut is now optional via the option -write-nut
  • noise: power of 2 data samples constraint was removed

Function objects
  • secondaryWrite: option in the system/controlDict superseded by the writeObject function object

Changes for OpenFOAM v1706

Turbulence
  • The omegaWallFunction was updated to replicate v1606+ behaviour via the blended keyword. For more information, see commit ef0361f7

Heat transfer
  • The nMoles entry is no longer required in the thermophysicalProperties dictionary
  • Heat flux field names have been updated to use a lower case ‘q’, e.g. radiative heat flux field name Qr to qr
  • The externalWallHeatFluxTemperature boundary condition now requires a mode entry to state the mode of operation

Function objects
  • ALL: the evaluateControl was renamed executeControl
  • runTimePostProcessing: camera input changed (bug fix to the clipBox entry)

The noise utility inputs in the $FOAM_CASE/noiseDict dictionary were updated:

  • change in syntax for input specification
  • inputFiles entry renamed to files
  • inputFile entry renamed to file
  • for the pointNoise model the csvFileData sub-dictionary was removed
  • See source documentation in $FOAM_SRC/randomProcesses/noise/noiseModels

Changes for OpenFOAM v1612+

General input
  • dictionary keyword entries including the text Name have been shortened, e.g. pName becomes p, phiName becomes phi etc.

Function objects
  • keywords: outputControl renamed writeControl
  • library locations: functionObjectLibs renamed libs
  • faceSource renamed surfaceFieldValue
  • cellSource renamed volFieldValue
  • pressureTools renamed pressure
  • createTurbulenceFields renamed turbulenceFields
  • Peclet renamed PecletNo

Utility updates
  • foamCalc and foamExecFlowFunctionObjects absorbed into the new postProcess utility
  • many utilities converted into function objects
  • the input format for the changeDictionary utility has been simplified. In earlier releases the input followed, e.g.:

    dictionaryReplacement
    {
        U
        {
            internalField   uniform (1 0 0);
        }
    }
    The new syntax removes the outer dictionary level, i.e.

    U
    {
        internalField   uniform (1 0 0);
    }

Deprecated utilities

  • expandDictionary becomes foamDictionary -expand
  • foamDebugSwitches becomes foamDictionary/foamList -debug
  • foamInfoExec becomes foamDictionary
  • secondaryWrite becomes equivalent behaviour using function object time controls
  • execFlowFunctionObjects becomes postProcess utility