Usage

---

Running a Simulation

CaptureFOAM simulations can be run using any of the included tutorial case as a template. We will demonstrate here using the meaTube tutorial. To begin, source OpenFOAM and copy the case files from the tutorial to a new directory:

1. Prepare the case directory structure using a provided template:

   mkdir -p $FOAM_RUN/capturefoam
   cd $FOAM_RUN/capturefoam
   cp -r $WM_PROJECT_USER_DIR/CaptureFOAM/tutorials/meaTube testCase
   cd testCase
   

2. If desired, modify the input files to reflect the geometry, flow conditions, and chemical processes present in your problem. Important files are described in Case Files.

3. Generate a mesh, perform appropriate pre-processing steps, decompose your case to run in parallel if desired, and then run CaptureFOAM. These steps are illustrated in the Allrun scripts which are present in each tutorial case. For the meaTube case, the Allrun script contains the following:

    #!/bin/sh
    cd ${0%/*} || exit 1    # Run from this directory
       
    . $WM_PROJECT_DIR/bin/tools/RunFunctions
       
    # Create bulk mesh
    runApplication -s fluid blockMesh -region fluid
       
    # Create film mesh
    runApplication extrudeToRegionMesh -region fluid -overwrite
       
    # Change wedge patches to symmetry in film mesh
    sed -i 's/wedge/symmetry/g' constant/film/polyMesh/boundary
       
    # Run case
    runApplication $(getApplication)
       
    # Post-processing
    runApplication reconstructPar -allRegions
   

4. Visualize and post-process the results using ParaView

   paraFoam -builtin
   

CaptureFOAM File Structure

A typical CaptureFOAM case directory is organized as follows:

|-- case-directory/
|   |-- 0/
|   |   |-- film/
|   |   |   |-- U
|   |   |   |-- p
|   |   |   |-- T
|   |   |   |-- delta
|   |   |   |-- species_1
|   |   |   |-- species_2
|   |   |   |-- species_3
|   |   |-- fluid/
|   |   |   |-- U
|   |   |   |-- p
|   |   |   |-- p_rgh
|   |   |   |-- T
|   |   |   |-- species_1
|   |   |   |-- species_2
|   |   |   |-- species_4
|   |
|   |-- constant/
|   |   |-- film/
|   |   |   |-- chemistryProperties
|   |   |   |-- combustionProperties
|   |   |   |-- fvModels
|   |   |   |-- g
|   |   |   |-- momentumTransport
|   |   |   |-- physicalProperties
|   |   |   |-- reactions
|   |   |   |-- speciesThermo
|   |   |-- fluid/
|   |   |   |-- fvModels
|   |   |   |-- g
|   |   |   |-- momentumTransport
|   |   |   |-- physicalProperties
|   |   |   |-- speciesThermo
|   |
|   |
|   |-- system/
|   |   |-- film/
|   |   |   |-- fvSchemes
|   |   |   |-- fvSolution
|   |   |-- fluid/
|   |   |   |-- blockMeshDict
|   |   |   |-- extrudeToRegionMeshDict
|   |   |   |-- fvSchemes
|   |   |   |-- fvSolution
|   |   |-- controlDict
|   |   |-- fvSolution
|   |
|   +-- ..

Case Files

• 0: Directory containing the initial conditions and boundary conditions for each field in each phase. The fields are specified by their file name:
  • phase_type/U: velocity
  • phase_type/p_rgh: reduced pressure
  • fluid/p: thermodynamic pressure (gas phase only)
  • phase_type/T: temperature
  • film/delta: film thickness (film phase only)
  • phase_type/species_i: mass fraction of species \(i\) (each phase may have unique species)

• constant: Directory containing the definitions for thermophysical properties, turbulence modeling, and reactions for each phase, including:

  • film/chemistryProperties: ODE solver settings for the chemical reaction kinetics (film phase only)
  • film/combustionProperties: turbulence modeling type for reaction kinetics (film phase only)

  • film/reactions: description of reaction mechanism following OpenFOAM’s standard format (film phase only)

    Reactions may be enabled in the gas phase by including the appropriate files, but are typically not used for the applications of interest for CaptureFOAM.

  • film/fvModels: Optional fvModels for film phase. Interphase mass transfer is enabled by setting the following in the film/fvModels file:

    filmMassTransfer
    {
        type                filmMassTransfer;
            
        select              all;
            
        specie              CO2;
    }
    

  • fluid/fvModels: Optional fvModels for fluid phase. The bulk of the definitions for interphase mass transfer are contained in this file. An example is taken from the meaTube tutorial case:

    bulkMassTransfer
    {
        type                bulkMassTransfer;
            
        select              all;
            
        transferPatch       film; // Name of patch on which mass transfer occurs
                
        specie              CO2; // Name of specie to transfer
            
        // Mass transfer model type (options: constant, physical)
        interphaseMassTransferModel physical;
            
        // Coefficients for physical mass transfer model
        physicalCoeffs
        {        
            H1                  0.0; // 1st coefficient for Henry volatility constant, Pa-m^3/kmol/K
        
            H2                  2.27e+6; // 2nd coefficient for Henry volatility constant, Pa-m^3/kmol
                
            Dl1                 0.0; // 1st coefficient for Diffusivity of specie in film, m^2/s/K
        
            Dl2                 1.66e-9; // 2nd coefficient for Diffusivity of specie in film, m^2/s 
                
            bulkMassTransferRateModel
            {
                massTransferRateCoefficientModel Higbie;
                    
                HigbieCoeffs
                {            
                    D1              0.0;
                    
                    D2           	1.5e-5;
        
                    inlet           (0.0 0.0 0.0); // Point anywhere along bulk inlet
        
                    direction       (0 0 1); // Bulk flow direction
                }
            }
                
            filmMassTransferRateModel
            {
                massTransferRateCoefficientModel Higbie;
                    
                HigbieCoeffs
                {            
                   D1               $Dl1;
        
                   D2               $Dl2;
                    
                   inlet            (0.0 0.0 1.0); // Point anywhere along film inlet
                
                   direction        (0 0 -1); // Film flow direction
                }
            }
                
            enhancementModel    lowHa; // Enhancement factor model type
                
            tStart              10.0; // When to start chemically enhanced xfer
        }
    }
    

  • phase_type/g: Definition of gravity vector for each phase
  • phase_type/momentumTransport: Sets turbulence model type for each phase
  • phase_type/physicalProperties: Mixture type and energy equation settings for each phase
  • phase_type/speciesThermo: Thermophysical properties for each specie contained in each phase
• system: Contains the discretization and simulation control settings.
  • controlDict: Simulation time settings and input/output options.
  • fvSolution: The base fvSolution file sets the number of outer correctors performed by the multi-region solver
  • phase_type/fvSchemes: Finite volume discretization scheme settings for each phase
  • phase_type/fvSolution: Linear solver and PIMPLE algorithm settings for each phase