Bash functions: `solids4FoamScripts.sh`

Prepared by Ivan Batistić

Section Aims

This document describes the bash functions in the solids4foam/applications/scripts/solids4FoamScripts.sh script;
These bash functions within solids4FoamScripts.sh are used in Allrun and Allclean scripts in solids4foam tutorial cases;
The primary purpose of these functions is to make a case compatible with the current version of OpenFOAM/foam-extend, e.g. convert the case from its foam-extend-4.1 format to its OpenFOAM-v2012 format.

`solids4foam::convertCaseFormat()` and `solids4foam::convertCaseFormatFoamExtend()`

solids4foam::convertCaseFormat() is used to convert a case from foam-extend format to OpenFOAM format, whereas solids4foam::convertCaseFormatFoamExtend() is used to convert any case version to the foam-extend format. No changes are applied if the case format matches the format of the current OpenFOAM/foam-extend version.

Function purpose Converts a case from foam-extend format to OpenFOAM format and vice versa.
Function arguments Path to case directory (most often . is used, referring to the current directory)

Example of usage

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Convert case format to OpenFOAM
solids4Foam::convertCaseFormat .

# Convert case format back to foam-extend
solids4Foam::convertCaseFormatFoamExtend .
  

Changes are performed in different ways:

Relocating files within case structure (see points 1 and 2);
Using sed command to perform insertion, deletion, and substitution (see points 3 and 5);
Having different versions of the same file. The right one is chosen depending on the OpenFOAM version used. The switch between files is performed simply by renaming it (see points 4 or 7).

Note

The following description refers to the function solids4foam::convertCaseFormat().The description of solids4foam::convertCaseFormatFoamExtend() is not providedbecause it performs the same changes only in reverse order.

1. symmetryPlane in foam-extend becomes symmetry in OpenFOAM.

blockMeshDict is located, and every occurrence of symmetryPlane keyword is updated:

patches
(
    symmetryPlane left
    (
        (8 9 20 19)
    )
...
  

is transformed into:

patches
(
    symmetry left
    (
        (8 9 20 19)
    )
...
  

The same is done for the constant/polyMesh/boundary file:

left
{
    type            symmetryPlane;
    inGroups        1(symmetryPlane);
    nFaces          30;
    startFace       1930;
}
  

is transformed into:

left
{
    type            symmetry;
    inGroups        1(symmetry);
    nFaces          30;
    startFace       1930;
}
  

2. If it is found, blockMeshDict is moved to the system/ directory

For solid and fluid simulations, blockMeshDict is found in constant/polyMesh/:

├── 0
├── constant
│   └── polyMesh
│       └── blockMeshDict
└── system
  

and it is moved to the system directory:

├── 0
├── constant
│   └── polyMesh
└── system
 └── blockMeshDict
  

For fluid-solid interaction simulations, there may be two blockMeshDict files, each located in the corresponding solid/ and fluid/ subdirectories:

├── 0
├── constant
│   └── fluid
│   │   └── polyMesh
│   │       └── blockMeshDict
│   └── solid
│       └── polyMesh
│           └── blockMeshDict
└── system
  

These are also relocated to the system directory:

├── 0
├── constant
│   └── fluid
│   │   └── polyMesh
│   └── solid
│       └── polyMesh
└── system
    └── fluid
    │   └── blockMeshDict
    └── solid
        └── blockMeshDict
  

2.1. Rename the functions file

The function file is used to specify the list of function objects and is loaded at the bottom of the controlDict:

#include "./system/functions"
  

In the foam-extend case structure, the functions file is renamed to functions.foam-extend whereas functions.openfoam is renamed to functions:

└── system
    ├── controlDict
    ├── fvSchemes
    ├── fvSolution
    ├── functions
    └── functions.openfoam
  

is transformed into:

└── system
    ├── controlDict
    ├── fvSchemes
    ├── fvSolution
    ├── functions.foam-extend
    └── functions
  

3. Find the turbulenceProperties file and rename the value for the simulationType keyword:

simulationType  RASModel;
  

is renamed to:

simulationType  RAS;
  

Note that in a fluid-solid interaction case, turbulenceProperties file is located in the constant/fluid/ directory, while for fluid simulations, it is in the constant/.

4. If found,boundaryData directory is renamed:

├── 0
├── constant
│   ├── boundaryData
│   ├── boundaryData.openfoam
│   └── polyMesh/
└── system
  

is transformed into:

├── 0
├── constant
│   ├── boundaryData.foamextend
│   ├── boundaryData
│   └── polyMesh/
└── system
  

5. If sample file is found in the system/ directory and if the OpenFOAM.org version is used, uniform is replaced with lineUniform:

sets
(
    lineXX
    {
        type       uniform;
        axis                x;
        nPoints            50;
        start (0.05 1e-6 0.0005);
        end    (0.1 1e-6 0.0005);
    }
...
  

is transformed into:

sets
(
    lineXX
    {
        type   lineUniform;
        axis               x;
        nPoints             50;
        start (0.05 1e-6 0.0005);
        end    (0.1 1e-6 0.0005);
    }
...
  

6. If p file is found, and if the type keyword is set to timeVaryingUniformFixedValue, its value is changed to uniformFixedValue by commenting out the appropriate lines:

inlet
{
    //type          uniformFixedValue;
    type        timeVaryingUniformFixedValue;

    uniformValue  tableFile;
    "file|fileName"     "$FOAM_CASE/0/fluid/time-series";
    outOfBounds         clamp;
}

  

is transformed into:

inlet
{
    type          uniformFixedValue;
    //type        timeVaryingUniformFixedValue;

    uniformValue  tableFile;
    "file|fileName"     "$FOAM_CASE/0/fluid/time-series";
    outOfBounds         clamp;
}

  

7. If found, the version of thechangeDictionaryDict file is updated:

├── 0
├── constant
└── system
    ├── changeDictionaryDict
    ├── changeDictionaryDict.openfoam
    ├── controlDict
    ├── fvSchemes
    └── fvSolution
  

is transformed into:

├── 0
├── constant
└── system
    ├── changeDictionaryDict.foamextend
    ├── changeDictionaryDict
    ├── controlDict
    ├── fvSchemes
    └── fvSolution
  

8. If found, the version of thecreatePatchDict file is updated:

├── 0
├── constant
└── system
    ├── createPatchDict
    ├── createPatchDict.openfoam
    ├── controlDict
    ├── fvSchemes
    └── fvSolution
  

is transformed into:

├── 0
├── constant
└── system
    ├── createPatchDict.foamextend
    ├── createPatchDict
    ├── controlDict
    ├── fvSchemes
    └── fvSolution
  

9. In case the OpenFOAM.com version is used to solve solid mechanics or fluid-solid interaction problems, the leastSquare gradient method in fvSchemes file is replaced with pointCellsLeastSquares to account for boundary non-orthogonal corrections:

gradSchemes
{
    default            leastSquares;
}
  

is transformed into:

gradSchemes
{
    default            pointCellsLeastSquares;
}
  

Note: In fluid-solid interaction cases, this change is performed only on fvSchemes, which refers to solid and is located in system/solid/fvSchemes.

10. In case the force.gnuplot script is found, the path to the force.dat file is changed. force.dat is an output file generated by the forces function object. When foam-extend is used, it is located in the forces/0/ directory; otherwise it is located in postProcessing/fluid/forces/0/:

plot [0.1:] "< sed s/[\\(\\)]//g forces/0/forces.dat" u 1:2 w l
  

is transformed into:

plot [0.1:] "< sed s/[\\(\\)]//g ./postProcessing/fluid/forces/0/force.dat" \
    u 1:2 w l
  

11. In case the plot.gnuplot script is found, the path to the sigma_surface.raw is changed. sigma_surface.raw is an output file generated after using sample utility for post-processing results. When foam-extend is used, it is located in the "postProcessing/surfaces/1/ directory; otherwise, it is located in postProcessing/sampleDict/1/:

path = "postProcessing/surfaces/1/sigma_surface.raw"

is transformed into:

path = "postProcessing/sampleDict.v2012/1/sigma_surface.raw"

Note that the updated path has sampleDict.v2012 in it, and this is because it has the same name in the system/ directory where sampleDict.v2012 is located.

`solids4foam::caseOnlyRunsWithFoamExtend()`

Function purpose This function gives an error if the foam-extend version is not sourced/loaded.
Function arguments None

Example of usage

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

solids4Foam::caseOnlyRunsWithFoamExtend

`solids4foam::caseDoesNotRunWithFoamExtend()`

Function purpose This function gives an error if the OpenFOAM.com or OpenFOAM.org version is not sourced/loaded.
Function arguments None

Example of usage

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

solids4Foam::caseDoesNotRunWithFoamExtend

`solids4foam::removeEmptyDirs()`

Function loops over time directories (whose name is composed of digits or digits and the dot) and removes them if there are no results. Checked resulting fields are U, T, D, pointD, DD, pointDD. The compressed version of these files with .gz extension is also checked. The function also works when the case is decomposed.

Function purpose Remove empty time directories that are inadvertently created when running FSI cases with preCICE.
Function arguments None
Example of usage

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Remove empty time directories created by preCICE
solids4Foam::removeEmptyDirs
  

`solids4foam::err()`

It will construct a message string with the current date time and timezone offset. The message passed as an argument to the err() function will be appended to this message string. The string is written to a file named error.txt and is also displayed on the console as an error output. In case an optional argument (file name) is prescribed, the context of the file name is written to errorCommandLog.txt file.

Function purpose This function is designed to handle and report errors in a script.
Function arguments "error message" - stored to error.txt optional parameter - name of the log file which will be stored to errorCommandLog.txt

Example of usage

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Check if a 0 directory already exists
if [[ -d "postProcessing" ]]
then
 solids4foam::err "The postProcessing directory already exists: run Allclean"
fi
  

In the above example, the error message is stored in the error.txt file and printed in the console as:

ERROR: see error.txt
[2023-09-05T10:19:18+0200]: The postProcessing directory already exists: run Allclean
  

If an optional argument wants to be used, the command should look like this:

#!/bin/bash

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Check if a 0 directory already exists
if [[ -f "postProcessing/data.dat" ]]
then
 solids4foam::err "The data.dat file already exists: run Allclean to delete" postProcessing/data.dat
fi
  

The console output of this will be :

ERROR: see error.txt
[2023-09-05T10:19:18+0200]: The postProcessing directory already exists: run
Allclean to delete postProcessing/data.dat
       see errorCommandLog.txt
  

The context of the data.dat is stored in the errorCommandLog.txt file.

`solids4foam::runApplication()`

Function purpose This function is designed to run OpenFOAM and solids4foam applications with additional logging and error handling.
Function options -a = append (append to an existing log file) -o = overwrite (overwrite existing log file) -s = suffix (adding suffix to the log file) -decomposeParDict <locationOfAlternativeDecomposeParDict> Alternative option for decomposeParDict dictionary location
Function arguments <appName> Name of the executable (command to run)

Note: Parameters which are added after the executable will be passed on to it!
Example of usage

#!/bin/bash

# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Create meshes
solids4Foam::runApplication -s solid blockMesh -region solid
  

In the example above, the word solid is the suffix. blockMesh is the name of the executable with -region solid as an parameter for theblockMesh.

#!/bin/bash

# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions

# Source solids4Foam scripts
source solids4FoamScripts.sh

# Create cellZones for materials
solids4Foam::runApplication setSet -batch batch.setSet
solids4Foam::runApplication setsToZones

# Run the solver
solids4Foam::runApplication solids4Foam
  

In this example, options are not used. setSet is executable with -batch batch.setSet parameter whereas setsToZones and solids4Foam are executables without arguments.

In case the log file already exists and the -a option is not set, it will exit and print that the executable is already running at this location.

Both standard error sterr and standard output stdout are redirected to the log file. If the application returns an error (non-zero exit code), it appears as "ERROR" in the log file. The name of the log file is log.<executable name>. In case the option -s is activated, the name of the log file is log.<executable name>.<suffix>.

`solids4foam::runParallel()`

This function has the same functionalities and options as solids4Foam::runApplication function described previously. The difference is that the executable is run in parallel using MPI.

mpirun -n nProcs executable -parallel >> log.executable

is simply replaced with:

solids4Foam::runParallel executable

decomposeParDict located in the system is automatically checked to get the number of processors nProcs.

In case that $FOAM_MPI is set to msmpi, mpirun is replaced with msmpi.

Bash functions: solids4FoamScripts.sh

Section Aims

solids4foam::convertCaseFormat() and solids4foam::convertCaseFormatFoamExtend()

solids4foam::caseOnlyRunsWithFoamExtend()

solids4foam::caseDoesNotRunWithFoamExtend()

solids4foam::removeEmptyDirs()

solids4foam::err()

solids4foam::runApplication()

solids4foam::runParallel()

Bash functions: `solids4FoamScripts.sh`

`solids4foam::convertCaseFormat()` and `solids4foam::convertCaseFormatFoamExtend()`

`solids4foam::caseOnlyRunsWithFoamExtend()`

`solids4foam::caseDoesNotRunWithFoamExtend()`

`solids4foam::removeEmptyDirs()`

`solids4foam::err()`

`solids4foam::runApplication()`

`solids4foam::runParallel()`