Customizing the output of the simulation

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.

Customizing the screen and history output

Screen output

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

History output

The history output can be customized in a similar fashion to 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. However, instead of specifying single output fields, for the history output it is only possible to specify output groups by using the group name.

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.

Example

For the compressible Navier-Stokes solver (i.e. PHYSICAL_PROBLEM=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

Customizing the volume Output

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.

Example

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

Field Name Description Group Name
COORD-X x coordinate COORDINATES
COORD-Y y coordinate COORDINATES
COORD-Z z coordinate COORDINATES
DENSITY Density SOLUTION
MOMENTUM-X Momentum x-component SOLUTION
MOMENTUM-Y Momentum y-component SOLUTION
MOMENTUM-Z Momentum z-component SOLUTION
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
HEAT_FLUX Heat flux PRIMITIVE
Y_PLUS Y-Plus PRIMITIVE


Improve this page