foamToVTK(1)

www.openfoam.com, OpenFOAM-v2112

foamToVTK [OPTIONS]

Description

General OpenFOAM to VTK file writer

Options

  • -allRegions
    Use all regions in regionProperties
  • -ascii
    Write in ASCII format instead of binary
  • -case dir
    Specify case directory to use (instead of cwd)
  • -constant
    Include the 'constant/' dir in the times list
  • -fields wordRes
    Specify single or multiple fields to write (all by default) Eg, 'T' or '(p T U "alpha.*")'
  • -latestTime
    Select the latest time
  • -name subdir
    Directory name for VTK output (default: 'VTK')
  • -no-boundary
    Suppress output for boundary patches
  • -no-internal
    Suppress output for internal volume mesh
  • -no-lagrangian
    Suppress writing lagrangian positions and fields
  • -no-point-data
    Suppress conversion of pointFields. No interpolated PointData.
  • -noZero
    Exclude the '0/' dir from the times list
  • -one-boundary
    Combine all patches into a single file
  • -overwrite
    Remove any existing VTK output directory
  • -parallel
    Run in parallel [Parallel option]
  • -patches wordRes
    Specify single patch or multiple patches to write Eg, 'top' or '( front ".*back" )'
  • -region name
    Use specified mesh region. Eg, -region gas
  • -regions wordRes
    Use specified mesh region. Eg, -regions gas Or from regionProperties. Eg, -regions '(gas "solid.*")'
  • -time ranges
    List of ranges. Eg, ':10,20 40:70 1000:', 'none', etc
  • -doc
    Display documentation in browser
  • -help
    Display short help and exit
  • -help-full
    Display full help and exit

ADVANCED OPTIONS

  • -cellSet name
    Convert mesh subset corresponding to specified cellSet
  • -cellZone name
    Convert mesh subset corresponding to specified cellZone
  • -debug-switch name=val
    Specify the value of a registered debug switch. Default is 1 if the value is omitted. (Can be used multiple times)
  • -decomposeParDict file
    Use specified file for decomposePar dictionary
  • -excludePatches wordRes
    Exclude single or multiple patches from writing Eg, 'outlet' or '( inlet ".*Wall" )'
  • -faceSet name
    Convert specified faceSet only
  • -faceZones wordRes
    Specify single or multiple faceZones to write Eg, 'cells' or '( slice "mfp-.*" )'.
  • -fileHandler handler
    Override the file handler type
  • -finite-area
    Write finite area fields
  • -hostRoots *((host1 dir1) .. (hostN dirN))*
    Per-subprocess root directories for distributed running. The host specification can be a regex. [Parallel option]
  • -info-switch name=val
    Specify the value of a registered info switch. Default is 1 if the value is omitted. (Can be used multiple times)
  • -legacy
    Write legacy format instead of xml
  • -lib name
    Additional library or library list to load (can be used multiple times)
  • -nearCellValue
    Use cell value on patches instead of patch value itself
  • -noFunctionObjects
    Do not execute function objects
  • -opt-switch name=val
    Specify the value of a registered optimisation switch. Default is 1 if the value is omitted. (Can be used multiple times)
  • -pointSet name
    Convert specified pointSet only
  • -poly-decomp
    Decompose polyhedral cells into tets/pyramids
  • -processor-fields
    Write field values on processor boundaries only
  • -roots *(dir1 .. dirN)*
    Subprocess root directories for distributed running [Parallel option]
  • -surfaceFields
    Write surfaceScalarFields (eg, phi)
  • -with-ids
    Additional mesh id fields (cellID, procID, patchID)
  • -with-point-ids
    Additional pointID field for internal mesh
  • -world name
    Name of the local world for parallel communication [Parallel option]
  • -doc-source
    Display source code in browser
  • -help-compat
    Display compatibility options and exit
  • -help-man
    Display full help (manpage format) and exit
  • -help-notes
    Display help notes (description) and exit

COMPATIBILITY OPTIONS

  • -allPatches (now -one-boundary)
    The option was last used in 1806.
  • -finiteAreaFields (now -finite-area)
    The option was last used in 2012.
  • -noLagrangian (now -no-lagrangian)
    The option was last used in 1806.
  • -noPointValues (now -no-point-data)
    The option was last used in 1806.
  • -noFaceZones
    This option is ignored after 1806.
  • -noLinks
    This option is ignored after 1806.
  • -poly
    This option is ignored after 1806.
  • -useTimeName
    This option is ignored after 1806.
  • -xml
    This option is ignored after 1806.

See Also

Online documentation https://www.openfoam.com/documentation/

Copyright

Copyright © 2018-2021 OpenCFD Ltd.