/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2017-2018 OpenCFD Ltd.
\\/ M anipulation |
-------------------------------------------------------------------------------
License
This file is part of OpenFOAM.
OpenFOAM is free software: you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by
the Free Software Foundation, either version 3 of the License, or
(at your option) any later version.
OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
for more details.
You should have received a copy of the GNU General Public License
along with OpenFOAM. If not, see .
Class
Foam::functionObjects::vtkWrite
Group
grpUtilitiesFunctionObjects
Description
Writes fields in VTK (xml or legacy) format.
Writes cell-values or point-interpolated values for volFields.
Example of function object specification:
\verbatim
vtkWrite1
{
type vtkWrite;
libs ("libutilityFunctionObjects.so");
writeControl writeTime;
writeInterval 1;
format binary;
legacy false;
decompose false;
...
fields (U p);
selection
{
box
{
action use;
source box;
box (-0.1 -0.01 -0.1) (0.1 0.30 0.1);
}
dome
{
action add;
source sphere;
origin (-0.1 -0.01 -0.1);
radius 0.25;
}
centre
{
action subtract;
source sphere;
origin (-0.1 -0.01 -0.1);
radius 0.1;
}
blob
{
action add;
source surface;
surface triSurfaceMesh;
name blob.stl;
}
}
}
\endverbatim
\heading Basic Usage
\table
Property | Description | Required | Default
type | Type name: vtkWrite | yes |
fields | Fields to output (wordRe list) | yes |
boundary | Convert boundary fields | no | true
internal | Convert internal fields | no | true
single | Combine patches into a single boundary | no | false
interpolate | Interpolate for point values | no | false
\endtable
\heading Output Options
\table
Property | Description | Required | Default
format | ascii or binary format | no | binary
legacy | Legacy VTK output | no | false
precision | Write precision in ascii | no | same as IOstream
directory | The output directory name | no | postProcessing/NAME
width | Padding width for file name | no | 8
decompose | Decompose polyhedral cells | no | false
writeIds | Write cell/patch ids as field | no | false
\endtable
\heading Output Selection
\table
Property | Description | Required | Default
region | Name for a single region | no | region0
regions | List of regions (wordRe list) | no |
patches | Limit to listed patches (wordRe list) | no |
selection | Cell selection (topoSet actions) | no | empty dict
\endtable
Note
The region of interest is defined by the selection dictionary
as a set of actions (use,add,subtract,subset,invert).
Omitting the selection dictionary is the same as specifying the
conversion of all cells (in the selected regions).
Omitting the patches entry is the same as specifying the conversion of all
patches.
See also
Foam::functionObjects::ensightWrite
Foam::functionObjects::fvMeshFunctionObject
Foam::functionObjects::timeControl
SourceFiles
vtkWrite.C
vtkWriteTemplates.C
\*---------------------------------------------------------------------------*/
#ifndef functionObjects_vtkWrite_H
#define functionObjects_vtkWrite_H
#include "functionObject.H"
#include "foamVtkInternalWriter.H"
#include "foamVtkPatchWriter.H"
#include "foamVtkSeriesWriter.H"
#include "fvMeshSubsetProxy.H"
#include "searchableSurfaces.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace functionObjects
{
/*---------------------------------------------------------------------------*\
Class vtkWrite Declaration
\*---------------------------------------------------------------------------*/
class vtkWrite
:
public functionObject
{
// Private Data
//- Reference to the time database
const Time& time_;
//- The output directory
fileName outputDir_;
//- The printf format for zero-padding names
string printf_;
//- VTK output options
vtk::outputOptions writeOpts_;
//- Verbose output
bool verbose_;
//- Convert internal mesh
bool doInternal_;
//- Convert boundary mesh
bool doBoundary_;
//- Combine patches into a single file
bool oneBoundary_;
//- Interpolate cell to point values
bool interpolate_;
//- Decompose polyhedra
bool decompose_;
//- Write cell ids field
bool writeIds_;
//- Track changes in mesh geometry
enum polyMesh::readUpdateState meshState_;
//- Requested names of regions to process
wordRes selectRegions_;
//- Requested names of patches to process
wordRes selectPatches_;
//- Requested names of fields to process
wordRes selectFields_;
//- Dictionary of volume selections
dictionary selection_;
//- Pointers to the requested mesh regions
HashTable meshes_;
//- Subsetting for meshes.
// Access index according to sorted mesh names.
PtrList meshSubsets_;
//- Storage for VTU cells, sizing.
// Access index according to sorted mesh names.
PtrList vtuMappings_;
//- VTK file series
HashTable series_;
// Private Member Functions
//- Update mesh subset according to zones, geometry, bounds
bool updateSubset(fvMeshSubset& subsetter) const;
//- Get patchIds selected in list
labelList getSelectedPatches(const polyBoundaryMesh& patches) const;
//- Read information for selections
bool readSelection(const dictionary& dict);
//- Update meshes, subMeshes etc.
bool update();
// Write
//- Write all volume fields
label writeAllVolFields
(
autoPtr& internalWriter,
UPtrList& patchWriters,
const fvMeshSubset& proxy,
const wordHashSet& acceptField
) const;
//- Write all volume fields with point interpolation
label writeAllVolFields
(
autoPtr& internalWriter,
const autoPtr& pInterp,
UPtrList& patchWriters,
const UPtrList
<
PrimitivePatchInterpolation
>& patchInterps,
const fvMeshSubset& proxy,
const wordHashSet& acceptField
) const;
//- Write selected GeoField fields.
template
label writeVolFields
(
autoPtr& internalWriter,
UPtrList& patchWriters,
const fvMeshSubset& proxy,
const wordHashSet& acceptField
) const;
//- Write selected GeoField fields with point interpolation
template
label writeVolFields
(
autoPtr& internalWriter,
const autoPtr& pInterp,
UPtrList& patchWriters,
const UPtrList
<
PrimitivePatchInterpolation
>& patchInterps,
const fvMeshSubset& proxy,
const wordHashSet& acceptField
) const;
//- No copy construct
vtkWrite(const vtkWrite&) = delete;
//- No copy assignment
void operator=(const vtkWrite&) = delete;
public:
//- Runtime type information
TypeName("vtkWrite");
// Constructors
//- Construct from Time and dictionary
vtkWrite
(
const word& name,
const Time& runTime,
const dictionary& dict
);
//- Destructor
virtual ~vtkWrite() = default;
// Member Functions
//- Read the vtkWrite specification
virtual bool read(const dictionary& dict);
//- Execute - does nothing
virtual bool execute();
//- Write fields
virtual bool write();
//- On end - provide feedback about disconnecting from catatyst.
virtual bool end();
//- Update for changes of mesh
virtual void updateMesh(const mapPolyMesh& mpm);
//- Update for mesh point-motion
virtual void movePoints(const polyMesh& mesh);
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace functionObjects
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#ifdef NoRepository
#include "vtkWriteTemplates.C"
#endif
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //