Post-processing#

This subsection controls the post-processing other than the forces and torque on the boundary conditions. Default values are

subsection post-processing
  set verbosity                        = quiet
  set output frequency                 = 1

  #---------------------------------------------------
  # Fluid dynamic post-processing
  #---------------------------------------------------
  # Kinetic energy calculation
  set calculate kinetic energy         = false
  set kinetic energy name              = kinetic_energy

  # Average velocities calculation
  set calculate average velocities     = false
  set initial time                     = 0.0

  # Pressure drop calculation
  set calculate pressure drop          = false
  set pressure drop name               = pressure_drop
  set inlet boundary id                = 0
  set outlet boundary id               = 1

  # Flow rate at boundaries calculation
  set calculate flow rate              = false
  set flow rate name                   = flow_rate

  # Enstrophy calculation
  set calculate enstrophy              = false
  set enstrophy name                   = enstrophy

  # Viscous dissipation
  set calculate viscous dissipation    = false
  set viscous dissipation name         = viscous_dissipation

  # Pressure power
  set calculate pressure power         = false
  set pressure power name              = pressure_power

  # Others
  set smoothed output fields           = false

  #---------------------------------------------------
  # Physical properties post-processing
  #---------------------------------------------------
  set calculate apparent viscosity     = false
  set apparent viscosity name          = apparent_viscosity

  #---------------------------------------------------
  # Multiphysics post-processing
  #---------------------------------------------------
  # Tracer postprocessing
  set calculate tracer statistics      = false
  set tracer statistics name           = tracer_statistics
  set calculate tracer flow rate       = false
  set tracer flow rate name            = tracer_flow_rate

  # Thermal postprocessing
  set postprocessed fluid              = both
  set calculate temperature statistics = false
  set temperature statistics name      = temperature_statistics
  set calculate heat flux              = false
  set heat flux name                   = heat_flux

  # Multiphase postprocessing
  set calculate barycenter             = false
  set barycenter name                  = barycenter_information
  set calculate mass conservation      = true
  set mass conservation name           = mass_conservation_information

  # Other Cahn-Hilliard postprocessing
  set calculate phase statistics       = false
  set phase statistics name            = phase_statistics
  set calculate phase energy           = false
  set phase energy name                = phase_energy

  #---------------------------------------------------
  # Multiphase post-processing
  #---------------------------------------------------
  # CFD-DEM postprocessing
  set calculate volume phases          = false
  set phase volumes name               = phase_volumes

end

  • verbosity: enables the display of the post-processing values in the terminal. This does not affect the printing of output files. Choices are: quiet (default, no output) or verbose (output at every iteration).

  • output frequency: frequency at which the enabled post-processing is outputted in the respective file. For output frequency = 1 (default value), results are outputted at each iteration.

  • calculate kinetic energy: controls if calculation of kinetic energy is enabled.

    • kinetic energy name: output filename for kinetic energy calculations.

    • The kinetic energy \({E}_k\) is calculated as

    \[{E}_k = \frac{1}{2 \Omega} \int_{\Omega} \mathbf{u} \cdot \mathbf{u} \ \mathrm{d} \Omega\]

    with \(\Omega\) representing the volume of the domain and \(\mathbf{u}\) the velocity.

  • calculate average velocities: controls if calculation of time-averaged velocities is enabled.

    • initial time: initial time used for the average velocities calculations.

  • calculate pressure drop: controls if calculation of the pressure drop from the inlet boundary to the outlet boundary is enabled.

    • inlet boundary id and outlet boundary id: define the IDs for inlet and outlet boundaries, respectively.

    • pressure drop name: output filename for pressure drop calculations.

    • The pressure drop \(\Delta p\) and total pressure drop \(\Delta p_\text{total}\) are calculated as:

    \[\Delta p = \frac{ \int_{\Gamma_\text{inlet}} p \mathrm{d} \Gamma}{\int_{\Gamma_\text{inlet}} 1 \mathrm{d} \Gamma} - \frac{ \int_{\Gamma_\text{outlet}} p \mathrm{d} \Gamma}{\int_{\Gamma_\text{outlet}} 1 \mathrm{d} \Gamma}\]
    \[\Delta p_\text{total} = \frac{ \int_{\Gamma_\text{inlet}} (p + \frac{1}{2} \mathbf{u} \cdot \mathbf{u}) \mathrm{d} \Gamma}{\int_{\Gamma_\text{inlet}} \mathrm{d} \Gamma} - \frac{ \int_{\Gamma_\text{outlet}} (p + \frac{1}{2} \mathbf{u} \cdot \mathbf{u}) \mathrm{d} \Gamma}{\int_{\Gamma_\text{outlet}} \mathrm{d} \Gamma}\]

    with \(\Gamma\) representing the boundary, \(\mathbf{u}\) the velocity and \(p\) the pressure.

  • calculate flow rate: controls if calculation of the volumetric flow rates at every boundary is enabled.

    • flow rate name: output filename for flow rate calculations.

    • The flow rate \(Q\) is calculated as such, with \(\Gamma\) representing the boundary, \(\mathbf{u}\) the velocity and \(\mathbf{n}\) the vector normal to the surface:

\[Q = \int_{\Gamma} \mathbf{n} \cdot \mathbf{u} d \Gamma\]
  • calculate enstrophy: controls if the volume-averaged enstrophy is calculated.

    • enstrophy name: output filename for enstrophy calculations.

    • The enstrophy \(\mathcal{E}\) is calculated as

    \[\mathcal{E} = \frac{1}{2 \Omega} \int_{\Omega} \mathbf{\omega} \cdot \mathbf{\omega} \mathrm{d} \Omega\]

    with \(\Omega\) representing the volume of the domain and \(\mathbf{\omega}\) the vorticity.

  • calculate viscous dissipation: controls if the viscous dissipation is calculated.

    • viscous dissipation name: output filename for the viscous dissipation calculations.

    • The viscous dissipation is calculated as

    \[\frac{1}{\Omega} \int_{\Omega} \mathbf{\tau} : \nabla\mathbf{u} \mathrm{d} \Omega\]

    with \(\Omega\) representing the volume of the domain and \(\mathbf{\tau}\) the deviatoric stress tensor.

  • calculate pressure power: controls if the pressure power is calculated.

    • pressure power name: output filename for the pressure power calculations.

    • The pressure power is calculated as

    \[\frac{1}{\Omega} \int_{\Omega} \nabla p \cdot \mathbf{u} \mathrm{d} \Omega\]

    with \(\Omega\) representing the volume of the domain, \(\mathbf{u}\) the velocity and \(p\) the pressure.

  • smoothed output fields: controls if the Qcriterion field will be smoothed using an L2-projection over the nodes. The same will shortly be applied to the Vorticity.

  • calculate apparent viscosity: controls if parameter calculation of an apparent viscosity is enabled, when using a non Newtonian flow (see section Physical properties - Rheological Models). This is mainly used to define the Reynolds number a posteriori.

    • apparent viscosity name: output filename for apparent viscosity calculations.

  • calculate tracer statistics: controls if calculation of tracer statistics is enabled. Statistics include: minimum, maximum, average and standard-deviation.

    Warning

    Do not forget to set tracer = true in the Multiphysics subsection of the .prm.

    • tracer statistics name: output filename for tracer statistics calculations.

  • postprocessed fluid: fluid domain used for thermal postprocesses. Choices arefluid 0, fluid 1, or both (default).

    • For monophasic simulations (set VOF = false in Multiphysics), both and fluid 0 are equivalent and the temperature statistics are computed over the entire domain.

    • For multiphasic simulations (set VOF = true in Multiphysics), temperature statistics can be computed over the entire domain (both) or inside a given fluid only (fluid 0 or fluid 1), with the fluid IDs defined in Physical properties - Two Phase Simulations.

    Note

    The output files will have a suffix depending on the postprocessed fluid: fluid_0, fluid_1 and all_domain.

  • calculate temperature statistics: controls if calculation of temperature statistics is enabled. Statistics include: minimum, maximum, average and standard-deviation.

    • temperature statistics name: output filename for temperature statistics calculations.

    Example of temperature statistics table:

     time  min    max    average std-dev
0.0000 0.0000 3.9434  0.1515  0.6943
0.2000 2.5183 4.9390  3.3917  0.7229

  • calculate heat flux: controls if calculation of heat flux is enabled. If enabled, these quantities are postprocessed:

    1. the total heat flux \(q_{tot}\) for each Heat Transfer boundary condition. The total heat flux on a boundary \(\Gamma\) is defined as:

    \[q_\text{tot} = \int_\Gamma (\rho C_p \mathbf{u} \mathbf{T} - k \nabla \mathbf{T}) \cdot \mathbf{n}\]

    The output table is appended with one column per Heat Transfer boundary condition, named bc_i where i is the index of the boundary in the parameter file.

    1. the convective heat flux \(q_\text{conv}\) for each Heat Transfer boundary condition. The convective heat flux on a boundary \(\Gamma\) is defined as:

    \[q_\text{conv} = \int_\Gamma h (\mathbf{T}-\mathbf{T}_\infty)\]

    The output table is appended with one column per Heat Transfer boundary condition, named bc_i where i is the index of the boundary in the parameter file.

    1. the thermal energy (\(\mathbf{Q} = m c_p \mathbf{T}\)) over the domain defined by postprocessed fluid.

    2. if there is a Nitsche Immersed Boundary, the total heat fluxes on each solid: \(q_\text{nitsche} = \beta_\text{heat} \left( \mathbf{T}_\text{nitsche} - \mathbf{T} \right)\)

    The output table is appended with one column per solid, named nitsche_solid_i where i is the index of the nitsche solid in the parameter file.

    Warning

    Do not forget to set enable heat boundary condition = true in the Nitsche Immersed Boundary subsection of the .prm.

    • heat flux name: output filename for heat flux calculations.

      Example of heat flux table:

       time  total_flux_bc_0 convective_flux_bc_0 thermal_energy_fluid flux_nitsche_solid_0
0.0000          0.0000               0.0000               0.0000            1000.0000
1.0000         -0.9732               0.0000               1.4856               0.9732

  • calculate barycenter: calculates the barycenter of fluid 1 and its velocity in VOF and Cahn-Hilliard simulations. The barycenter \(\mathbf{x}_b\) and its velocity \(\mathbf{v}_b\) are defined as:

    \[\mathbf{x_b} = \frac{\int_{\Omega} \psi \mathbf{x} \mathrm{d}\Omega }{\int_{\Omega} \psi \mathrm{d}\Omega}\]
    \[\mathbf{v_b} = \frac{\int_{\Omega} \psi \mathbf{u} \mathrm{d}\Omega }{\int_{\Omega} \psi \mathrm{d}\Omega}\]

    where \(\psi \in [0,1]\) is the filtered phase indicator for VOF simulations.

    For Cahn-Hilliard the formula is slightly different since the phase order parameter \(\phi\) belongs to the \([-1,1]\) interval:

    \[\mathbf{x_b} = \frac{\int_{\Omega} 0.5(1-\phi) \mathbf{x} \mathrm{d}\Omega }{\int_{\Omega} 0.5(1-\phi) \mathrm{d}\Omega}\]
    \[\mathbf{v_b} = \frac{\int_{\Omega} 0.5(1-\phi) \mathbf{u} \mathrm{d}\Omega }{\int_{\Omega} 0.5(1-\phi) \mathrm{d}\Omega}\]

    where \(\phi\) is the phase order parameter.

  • barycenter name: name of the output file containing the position and velocity of the barycenter for VOF and Cahn-Hilliard simulations. The default file name is barycenter_information.

  • calculate mass conservation: calculates the mass and momentum of both fluids for VOF simulations.

  • mass conservation name: name of the output file containing the mass of both fluids for VOF simulations. The default file name is mass_conservation_information.

  • calculate phase statistics: outputs Cahn-Hilliard phase statistics, including minimum, maximum, average, integral of the phase order parameter, and the volume of each phase.

    Warning

    calculate phase statistics = true only works with the Cahn-Hilliard solver.

  • phase statistics name: name of the output file containing phase order parameter statistics from Cahn-Hilliard simulations. The default file name is phase_statistics. It is stored in the output folder with in a .dat file.

  • calculate phase energy: outputs Cahn-Hilliard phase energies, including bulk energy, interface energy and total energy. The energies are computed as follow:

    \[E_{bulk} = \int_{\Omega} (1-\phi^2)^2 \mathrm{d}\Omega\]
    \[E_{interface} = \int_{\Omega} 0.5\epsilon^2|\nabla \phi |^2 \mathrm{d}\Omega\]
    \[E_{total} = E_{bulk} + E_{interface}\]

    where \(\epsilon\) is the numerical interface thickness. Note that these energies are not homogeneous to physical energies. Nonetheless, they are a convenient way to track the system’s evolution.

    Warning

    calculate phase energy = true only works with the Cahn-Hilliard solver.

  • phase energy name: name of the output file containing phase energies from Cahn-Hilliard simulations. The default file name is phase_energy.

  • calculate phase volumes: outputs total volume of fluid phase and total volume of solid phase in CFD-DEM simulation. These volumes are computed as follow:

    \[V_{fluid} = \int_{\Omega} \varepsilon_f \mathrm{d}\Omega\]
    \[V_{solid} = \int_{\Omega} (1 - \varepsilon_f) \mathrm{d}\Omega\]

    where \(\varepsilon\) is the void fraction. This is a convenient way to check if the volume of each phase is conserved.

    Warning

    calculate phase volumes = true only works with the lethe-fluid-particle solver.

  • phase volumes name: name of the output file containing phase energies from Cahn-Hilliard simulations. The default file name is phase_volumes.