History and Solution Output

With v7.0 we have introduced a new way of customizing the output on screen, in the history file and in the visualization files. It is now possible to individually define what you want to have in your output.



Let’s define some terminology first.

  • Screen output : The convergence history printed on the console.
  • History output: The convergence history written to a file.
  • Volume output : Everything written to the visualization and restart files.
  • Output field: A single scalar value for screen and history output or a vector of a scalar quantity at every node in the mesh for the volume output.
  • Output group: A collection of output fields.

Note: You can print all available output fields and groups available for the current solver (set with the SOLVER option) by calling SU2_CFD with the -d flag, i.e.

SU2_CFD -d <your_config_file.cfg>

Restart and Visualization Files

SU2 can output the solution in several file formats. You can specify what files you want to have by setting the option OUTPUT_FILES to a list of files. The valid options are described in the following table:

Option value Description
RESTART Native SU2 binary restart format
RESTART_ASCII Native SU2 ASCII CSV restart format
STL_BINARY binary mesh in .stl format
STL_ASCII ASCII mesh in .stl format
MESH Native SU2 mesh in .su2 format
CSV ASCII CSV restart format (identical to RESTART_ASCII)
PARAVIEW_MULTIBLOCK Binary Paraview .vtm format
PARAVIEW Binary Paraview .vtk format
PARAVIEW_ASCII ASCII Paraview .vtk format
TECPLOT Binary Tecplot .szplt format
TECPLOT_ASCII ASCII Tecplot .dat format
SURFACE_CSV Surface values in CSV format (includes all markers set with MARKER_PLOTTING)
SURFACE_PARAVIEW Surface values in binary Paraview .vtk format (includes all markers set with MARKER_PLOTTING)
SURFACE_PARAVIEW_ASCII Surface values in ASCII Paraview .vtk format (includes all markers set with MARKER_PLOTTING)
SURFACE_TECPLOT Surface values in binary Tecplot .szplt format (includes all markers set with MARKER_PLOTTING)
SURFACE_TECPLOT_ASCII Surface values in ASCII Tecplot .dat format (includes all markers set with MARKER_PLOTTING)

The default value of OUTPUT_FILES is (RESTART, PARAVIEW, SURFACE_PARAVIEW). The output frequencies can be set by using the OUTPUT_WRT_FREQ option. OUTPUT_WRT_FREQ accepts a list of integer values for each of the file types in OUTPUT_FILES. If a single value is given, this value will be used as the writing frequency for all output files. If 2 values are used, the first value is used for the first file type in OUTPUT_FILES, and the second value is used for the other file types in the list. For time-dependent problems, the frequency is based on the time iterations, while for steady-state problems it is based on the outer or inner iterations, depending on whether it is a multi-zone or single-zone problem, respectively.

Note: If you run SU2 in parallel you should always use binary output files to get the best performance.

Setting Output Fields

The VOLUME_OUTPUT option can be used to set fields for the restart and visualization files. Here you have the option to specify either single fields and/or groups.

Option value Default value Description Data type
VOLUME_OUTPUT COORDINATES,SOLUTION,PRIMITIVE fields or groups that will be saved to file list of keywords

Example

Groups and fields can be combined, e.g.:

VOLUME_OUTPUT= SOLUTION, PRESSURE, DENSITY

will save all field that are in the SOLUTION group. Pressure is in the PRIMITIVE group for the compressible solver and in the SOLUTION group for the incompressible solver. Density on the other hand is in the SOLUTION group for the compressible solver and in the PRIMITIVE group for the incompressible solver. They can be added individually as in the example above, or by simply adding the entire PRIMITIVE group to the list if file size is no issue. Note that keywords that are not valid for the current setup will simply be ignored.

For the compressible Navier-Stokes solver (i.e. SOLVER=NAVIER_STOKES), a non-exhaustive list of possible fields/groups is the following:

Field Name Description Group Name Remarks
COORD-X x coordinate COORDINATES -
COORD-Y y coordinate COORDINATES -
COORD-Z z coordinate COORDINATES 3D only
DENSITY Density SOLUTION -
MOMENTUM-X Momentum x-component SOLUTION -
MOMENTUM-Y Momentum y-component SOLUTION -
MOMENTUM-Z Momentum z-component SOLUTION 3D only
ENERGY Energy SOLUTION -
PRESSURE Pressure PRIMITIVE -
TEMPERATURE Temperature PRIMITIVE -
MACH Mach Number PRIMITIVE -
PRESSURE_COEFF Pressure Coefficient PRIMITIVE -
LAMINAR_VISCOSITY Laminar viscosity PRIMITIVE -
SKIN_FRICTION-X Skin friction coefficient x-component PRIMITIVE -
SKIN_FRICTION-Y Skin friction coefficient y-component PRIMITIVE -
SKIN_FRICTION-Z Skin friction coefficient z-component PRIMITIVE 3D only
HEAT_FLUX Heat flux PRIMITIVE -
Y_PLUS Y-Plus PRIMITIVE -

Additionally, for every field in the SOLUTION group, the limiters (group name LIMITER) and residuals (group name RESIDUAL) can be saved by adding RES_ or LIMITER_ in front of the field name.

For the incompressible Navier-Stokes solver (i.e. SOLVER=INC_NAVIER_STOKES), the solution group is different:

Field Name Description Group Name Remarks
PRESSURE Pressure SOLUTION -
VELOCITY-X Velocity x-component SOLUTION -
VELOCITY-Y Velocity y-component SOLUTION -
VELOCITY-Z Velocity z-component SOLUTION 3D only
TEMPERATURE Static Temperature SOLUTION INC_ENERGY_EQUATION= YES
DENSITY Density PRIMITIVE -

Turbulence quantities:

Field Name Description Group Name Remarks
NU_TILDE Spalart Allmaras variable SOLUTION SA models
TKE Turbulent kinetic energy k SOLUTION SST models
DISSIPATION Turbulent dissipation rate omega SOLUTION SST models
EDDY_VISCOSITY Turbulent eddy viscosity PRIMITIVE -

To inspect the mesh quality we additionaly have:

Field Name Description Group Name Remarks
ORTHOGONALITY Orthogonality angle MESH_QUALITY -
ASPECT_RATIO CV Aspect ratio MESH_QUALITY -
VOLUME_RATIO CV sub-volume ratio MESH_QUALITY -

For moving grids:

Field Name Description Group Name Remarks
GRID_VELOCITY-X X-component of grid velocity vector GRID_VELOCITY -
GRID_VELOCITY-Y Y-component of grid velocity vector GRID_VELOCITY -
GRID_VELOCITY-Z Z-component of grid velocity vector GRID_VELOCITY 3D only

Customizing the Screen and History Output

Screen Output

You can define the output fields you want to have printed on screen by using the config option SCREEN_OUTPUT.

Option value Default value Description Data type Remark
SCREEN_OUTPUT INNER_ITER, RMS_DENSITY, RMS_MOMENTUM-X,RMS_MOMENTUM-Y, RMS_ENERGY field or group that will be printed to screen list of keywords compressible
SCREEN_OUTPUT INNER_ITER, RMS_PRESSURE, VELOCITY-X,VELOCITY-Y field or group that will be printed to screen list of keywords incompressible

Fields available depend on the solver you are using. Fields available for all solvers are the following:

  • TIME_ITER: Time iteration index
  • OUTER_ITER: Outer (coupling) iteration index (for multi-zone problems only)
  • INNER_ITER: Inner iteration index (pseudo-time iteration)
  • CUR_TIME: Current physical time of your simulation
  • TIME_STEP: Current time step
  • WALL_TIME: Current average wall-clock time for one iteration

If you run a multizone problem, the convergence history of the individual zones (i.e. the convergence of the inner iteration) is disabled by default and only the convergence of the outer iteration is shown. That means SCREEN_OUTPUT in the sub-config files is ignored. You can still print fields from individual zones by using the field name and the zone index. For example in an Fluid-Structure interaction problem the drag in zone 0 and the von-Mises stress in zone 1 can be used as fields by adding DRAG[0] and/or VMS[1] to the screen output in the main config file. It is possible to force the output of the full inner convergence history per zone by setting WRT_ZONE_CONV to YES.

You can also customize the frequency when the convergence history should be written to screen by using SCREEN_WRT_FREQ_INNER, SCREEN_WRT_FREQ_OUTER and SCREEN_WRT_FREQ_TIME.

History Output

The history output can be customized in a similar fashion as the screen output by using the HISTORY_OUTPUT option. In fact, screen and history outputs share all fields which means that everything that can written to screen can be written also to the history file and vice versa.

If you run a multizone problem, in addition to the history files per zone, a file (default: history_multizone.dat) will be created where the convergence history of the outer iteration is stored. Groups for this output can be set by using the HISTORY_OUTPUT option in the main config file.

You can also customize the frequency when the convergence history should be written to the history file by using HISTORY_WRT_FREQ_INNER, HISTORY_WRT_FREQ_OUTER and HISTORY_WRT_FREQ_TIME.

Example

For the compressible Navier-Stokes solver (i.e. SOLVER=NAVIER_STOKES), a non-exhaustive list of possible fields/groups is the following:

Field Name (for screen output) Description Group Name (for history output)
TIME_ITER Time iteration index ITER
OUTER_ITER Outer (coupling) iteration index. ITER
INNER_ITER Inner iteration index (pseudo-time iteration). ITER
CUR_TIME Current physical time of your simulation. TIME_DOMAIN
TIME_STEP Current time step. TIME_DOMAIN
WALL_TIME Current average wall-clock time for one iteration. WALL_TIME
RMS_DENSITY Root-mean square residual of the density. RMS_RES
RMS_MOMENTUM-X Root-mean square residual of the momentum x-component. RMS_RES
RMS_MOMENTUM-Y Root-mean square residual of the momentum y-component. RMS_RES
RMS_MOMENTUM-Z Root-mean square residual of the momentum z-component. RMS_RES
RMS_ENERGY Root-mean square residual of the energy. RMS_RES
DRAG Total Drag coefficient. AERO_COEFF
LIFT Total Lift coefficient AERO_COEFF
SIDEFORCE Total Sideforce coefficient. AERO_COEFF
MOMENT_X Total Moment around the x-axis. AERO_COEFF
MOMENT_Y Total Moment around the y-axis. AERO_COEFF
MOMENT_Z Total Moment around the z-axis. AERO_COEFF
FORCE_X Total Force in x direction. AERO_COEFF
FORCE_Y Total Force in y direction. AERO_COEFF
FORCE_Z Total Force in z direction. AERO_COEFF
EFFICIENCY Total Lift-to-drag ratio. AERO_COEFF


Improve this page