FACUtility

FACUtility is an OpenFOAM-based post-processing utility for predicting flow-accelerated corrosion (FAC) wall-thinning rates from a converged CFD solution. The utility combines hydrodynamic quantities derived from the wall region with temperature-dependent chemistry to compute local thinning-related outputs on selected wall patches.

This repository is written for OpenFOAM V2212 and contains:

• FACUtility source code
• required header/source files and build configuration
• four validation / example cases
  • 2D benchmark case (validationCases/2DCase)
  • 3D benchmark case (validationCases/3DCase)
  • 3D elbow pipe case (plant-representative) (validationCases/DN150)
  • Utanohara & Murase compound elbow (validationCases/case4)

The default case settings are configured to reproduce the validation conditions reported in the associated publication.

---

1. Repository Structure

A typical repository layout is shown below. Adjust the paths if your local folder names differ.

├── FACUtility
│   ├── FACUtility.C
│   ├── Make
│   │   ├── files
│   │   └── options
│   ├── createFields.H
│   ├── models
│   │   ├── FACChemistryConstants.C
│   │   ├── FACChemistryConstants.H
│   │   ├── FACChemistryModel.C
│   │   ├── FACChemistryModel.H
│   │   ├── FACErosionModel.C
│   │   ├── FACErosionModel.H
│   │   ├── FACNewtonRaphson.H
│   │   ├── FACThinningModel.C
│   │   └── FACThinningModel.H
│   ├── readFACProperties.H
│   ├── utils
│   │   ├── FACCSV.H
│   │   ├── FACChemistryTable.C
│   │   ├── FACChemistryTable.H
│   │   ├── FACDatWriter.H
│   │   ├── FACInterpolation.C
│   │   ├── FACInterpolation.H
│   │   ├── FACMapping.H
│   │   ├── FACProperties.H
│   │   ├── FACSelection.C
│   │   └── FACSelection.H
│   └── writeOutputs.H
├── LICENSE
├── README.md
└── validationCases
    ├── 2DCase
    │   ├── 0.orig
    │   ├── constant
    │   ├── plots
    │   └── system
    ├── 3DCase
    │   ├── 0.orig
    │   ├── constant
    │   ├── plots
    │   └── system
    ├── case4
    │   ├── 0.orig
    │   ├── constant
    │   ├── plots
    │   └── system
    └── DN150
        ├── 0.orig
        ├── constant
        └── system

---

2. Requirements

• OpenFOAM V2212
• Linux environment or WSL/Linux-compatible shell with OpenFOAM sourced
• C++ compiler supported by the OpenFOAM installation
• wmake available in the environment

Before compiling or running any case, load OpenFOAM V2212:

source /path/to/OpenFOAM-v2212/etc/bashrc

Replace the path above with the correct installation path on your system.

---

3. Compiling FACUtility

FACUtility is a standalone custom OpenFOAM utility and is compiled using wmake.

Step 1: Place the source folder

Copy or link the utility source into your user application area, for example:

mkdir -p $WM_PROJECT_USER_DIR/applications/utilities
cp -r FACUtility $WM_PROJECT_USER_DIR/applications/utilities/

Step 2: Compile

Move into the utility source directory and run wmake:

cd $WM_PROJECT_USER_DIR/applications/utilities/FACUtility
wmake

If compilation is successful, the executable will be created in:

$FOAM_USER_APPBIN/FACUtility

Step 3: Confirm the executable

You can verify that the utility is available using:

which FACUtility

or

ls $FOAM_USER_APPBIN/FACUtility

---

4. License

FACUtility is released under the GNU General Public License v3.0 (GPL-3.0).

FACUtility directly includes OpenFOAM headers and links against OpenFOAM's core libraries (fvMesh, volScalarField, surfaceScalarField, fvc:: operators, etc.). Since OpenFOAM itself is licensed under GPL-3.0, FACUtility is a combined/derivative work under the GPL and inherits the same license. See the LICENSE file for the full text.

5. General Workflow

FACUtility is a decoupled post-processing utility.

The workflow is:

1. Set up and run the CFD case using a suitable OpenFOAM solver.
2. Ensure that the flow and temperature fields are converged.
3. Configure FACProperties and select the target patch.
4. Run FACUtility for the selected time directory.
5. Review the generated post-processing files and ParaView-compatible patch fields.

In summary:

Create mesh -> Run CFD solver -> Run FACUtility -> Post-process outputs

---

6. Input Requirements

Before running FACUtility, the CFD case must already contain the required solution fields. Depending on the selected physical model and case setup, these typically include:

• velocity field U
• pressure field p or p_rgh
• temperature field T
• turbulence quantities required by the parent CFD solver
• mesh and boundary conditions
• FACProperties dictionary

The utility reads the converged OpenFOAM case and computes FAC-related quantities only on the specified wall patch.

---

7. Running the Four Validation Cases

7.1 2D Benchmark Case

# move to the case director
cd validationCases/2DCase 
# copy the original zero folder as "0"
cp -r 0.orig/ 0 
# create mesh
blockMesh 
# run solver
buoyantSimpleFoam # run solver in single core

# Run in parallel
decomposePar # split mesh, adjust the number of cores in "decomposeParDict"
mpirun -np 4 buoyantSimpleFoam -parallel # run solver in parallel 
mpirun -np 4 buoyantSimpleFoam -parallel > log.solver # to log the solver in a file

mv $(foamListTimes -latestTime)/turbulence*muEff $(foamListTimes -latestTime)/muEff # remove the prefix text from muEff under the latest time directory
FACUtility -latestTime # run FACUtility
gnuplot plots/*.xy # run gnuplots to check the results

This case reproduces the 2D validation setup and is intended to demonstrate the local flow acceleration, separation behavior, and resulting FAC-related post-processing.

7.2 3D Benchmark Case

# move to the case director
cd validationCases/3DCase 
# copy the original zero folder as "0"
cp -r 0.orig/ 0 
# create mesh
blockMesh 
# run solver
buoyantSimpleFoam # run solver in single core

# Run in parallel
decomposePar # split mesh, adjust the number of cores in "decomposeParDict"
mpirun -np 4 buoyantSimpleFoam -parallel # run solver in parallel 
mpirun -np 4 buoyantSimpleFoam -parallel > log.solver # to log the solver in a file

mv $(foamListTimes -latestTime)/turbulence*muEff $(foamListTimes -latestTime)/muEff # remove the prefix text from muEff under the latest time directory
FACUtility -latestTime # run FACUtility
gnuplot plots/*.xy # run gnuplots to check the results

This case extends the benchmark workflow to a three-dimensional geometry.

7.3 DN150

# move to the case director
cd validationCases/DN150
# copy the original zero folder as "0"
cp -r 0.orig/ 0 
# create back ground mesh
blockMesh 
# generate *.eMsh for edges
surfaceFeatureExtract
# create mesh
snappyHexMesh -overwrite
# run solver
buoyantSimpleFoam # run solver in single core

# Run in parallel
decomposePar # split mesh, adjust the number of cores in "decomposeParDict"
mpirun -np 4 buoyantSimpleFoam -parallel # run solver in parallel 
mpirun -np 4 buoyantSimpleFoam -parallel > log.solver # to log the solver in a file

mv $(foamListTimes -latestTime)/turbulence*muEff $(foamListTimes -latestTime)/muEff # remove the prefix text from muEff under the latest time directory

FACUtility -latestTime # run FACUtility

Note: The plots are visualized and generated using ParaView

This case reproduces the elbow-pipe validation configuration and is useful for studying circumferential variation in thinning around the bend.

7.4 Case 4 (Utanohara and Murase)

# move to the case director
cd validationCases/case4
# copy the original zero folder as "0"
cp -r 0.orig/ 0 
# create back ground mesh
blockMesh 
# generate *.eMsh for edges
surfaceFeatureExtract
# create mesh
snappyHexMesh -overwrite
# run solver
buoyantSimpleFoam # run solver in single core

# Run in parallel
decomposePar # split mesh, adjust the number of cores in "decomposeParDict"
mpirun -np 4 buoyantSimpleFoam -parallel # run solver in parallel 
mpirun -np 4 buoyantSimpleFoam -parallel > log.solver # to log the solver in a file

mv $(foamListTimes -latestTime)/turbulence*muEff $(foamListTimes -latestTime)/muEff # remove the prefix text from muEff under the latest time directory

FACUtility -latestTime # run FACUtility

Note: The plots are visualized and generated using ParaView