<output>

Table 1. Overview of Available Output Options for Section Cut, Volume Data, and Surface Data
	Full Data	Surface	Section Cut	Partial Surface	Partial Volume
pressure	Default	Default	Default	Default	Default
time_avg_pressure	Default	Default	Default	Optional	Optional
window_avg_pressure	Optional	Optional	Optional	Optional	Optional
velocity	Default	Default¹	Default	Optional¹	Default
time_avg_velocity	Default	N.A.	Default	N.A.	Optional
window_avg_velocity	Optional	N.A.	Optional	N.A.	Optional
wall_shear_stress	Default	Default	N.A.	Default	N.A.
time_avg_wall_shear_stress	Default	Default	N.A.	Optional	N.A.
window_avg_wall_shear_stress	Optional	Optional	N.A.	Optional	N.A.
density	Optional	Optional	Optional	Optional	Optional
time_avg_density	Optional	Optional	Optional	Optional	Optional
window_avg_density	Optional	Optional	Optional	Optional	Optional
surface_normal	Default	Default	N.A.	Optional	N.A.
mesh_data	Default	N.A.	N.A.	N.A.	N.A.

<output> - <general>

The <general> category contains the following parameters:

<output_frequency>: Specifies the number of coarsest iterations between consecutive outputs of the volume and the surface data in EnSight Gold format. You can specify fractions of 1 to obtain an output at the desired sub-time step level.
<output_start_iteration>: Specifies after which coarsest iteration the output will start.; Default = 0
<merge_output_files>: Specifies if the output files written in a partitioned way per MPI rank are merged into single files after the simulation is complete. The individual files per MPI rank are not deleted by this operation, so the data size of the output is effectively doubled. H3D or EnSight Gold files will be merged, depending on the file format specified.; Default = false
<delete_unmerged_output_files>: Specifies if the original data written per rank is deleted once a merged file is produced (if requested).; Default= false
<saved_states>: Specifies the number of consecutive output files to be kept, that is, if set to 2, the latest two output time steps are kept while the rest are removed. If set to zero, the feature is deactivated and all output time steps are kept.; Default = 0
<avg_start_coarsest_iteration>: Specifies after which coarsest iteration the continuous averaging of variables and force coefficients starts. The averaging itself also uses information from subiterations on the finer refinement levels.
<file_format>: Option to define whether the output should be in EnSight Gold, H3D, or both formats. <ensight> true/false, <h3d> true/false.; Default = ensight
<avg_window_size>: Specifies the number of consecutive coarsest iterations that will be used for window averaging. This value should be a factor of <output_frequency>.
<output_variables_full>: In this section, you can specify which of the variables listed in Table 1 should or should not be included in the full data output by setting <variable_name> to true or false.
Note: The default case is to export all variables, thus it is not required to explicitly set the variables to “true”; if not mentioned in this section, the variables are still written. To omit a variable from being written, you have to specifically set the corresponding solver deck entry to “false”.
<output_variables_surface>: In this section, you can specify which of the variables listed in Table 1 should be included and which should be excluded in the surface data output by setting <variable_name> to true or false.

Note: The default case is to export all variables, thus it is not required to explicitly set the variables to “true”; if not mentioned in this section, the variables are still written. To omit a variable from being written, you have to specifically set the corresponding solver deck entry to “false”.

<output> - <moment_reference_system>

This category specifies the properties of the moment reference system that is used to calculate the aerodynamic forces in a body-fixed coordinate system and also to calculate the pitch moment to be able to split the lift into front and rear part. The moment reference system is defined according to automotive aerodynamics conventions and needs to be placed in the center of the four support points defined by the wheel positions (in general on the ground plane).

As reference length, you need to indicate the wheel base (the distance between front and rear axle).

It contains the following parameters:

<origin>: The origin of the moment reference system, must be specified via the child parameters <x_pos>, <y_pos> and <z_pos> in $[m]$ .; Default values = 0.0, 0.0, 0.0
<roll_axis>: The roll axis of the moment reference system, must be specified via the child parameters <x_dir>, <y_dir> and <z_dir>.; Default values = 1.0, 0.0, 0.0
<pitch_axis>: The pitch axis of the moment reference system, must be specified via the child parameters <x_dir>, <y_dir> and <z_dir>.; Default values = 0.0, 1.0, 0.0
<yaw_axis>: The yaw axis of the moment reference system, must be specified via the child parameters <x_dir>, <y_dir> and <z_dir>.; Default values = 0.0, 0.0, 1.0

<output> - <aero_coefficients>

This category specifies the properties that are connected to the output of the aerodynamic coefficients.

By default, the instantaneous and averaged aerodynamic coefficients are recorded at every coarsest iteration in the files uFX_coefficients_Inst.txt and uFX_coefficients_Avg.txt in the uFX_coefficientsData folder.

The category contains the following parameters:

<reference_area>: The reference area used to calculate the aerodynamic coefficients (drag, lift, side force) in $[m^{2}]$ .
<reference_area_auto>: Specifies if the value of <reference_area> should be used (false) or if the reference area (the frontal projection area) should be automatically calculated by ultraFluidX itself (true).; Default = true
<reference_length>: The reference length (in $[m]$ ) that is used to calculate the pitch moment to be able to subsequently calculate the front and rear lift coefficients. See <output> - <moment_reference_system>.
<passive_parts>: If certain parts of the geometry should be excluded from the calculation of the aerodynamic coefficients, they can be specified via the child parameter <name> within this category. The specified names must match the respective part names in the STL file.
Note: domain_part_instances defined in the <geometry> tab need to be included here, if applicable.
<coefficients_parts>: Specifies if the aerodynamic coefficients should also be output by part. If set to true (default value), ultraFluidX will create the files uFX_coefficientsPerPart_Inst.txt and uFX_coefficientsPerPart_Avg.txt in the output folder containing the whole list of parts per time step and a subfolder named uFX_coefficientsPerPart, where one individual file per part (uFX_coefficients_#PARTNAME_Inst.txt, uFX_coefficients_#PARTNAME_Avg.txt) will be recorded.
<coefficients_along_axis>: Specifies the number of sections along the x-, y- and z-direction of the object that should be used for the sectional coefficient output.; Has three children: <num_sections_x>, <num_sections_y> and <num_sections_z> that allow you to specify the number of sections per direction.; Creates the files uFX_coefficientsPerSection{X,Y,Z}_Inst.txt and uFX_coefficientsPerSection{X,Y,Z}_Avg.txt for the instantaneous and averaged aerodynamic coefficients per section in x-, y- and z-direction of the object, respectively (output at every coarsest iteration). Set the number of sections to 0 to deactivate the output.
<forces_and_moments_export>: If set to true, the aerodynamic forces and moments will be exported in SI units. For each file uFX_coefficients*.txt, a corresponding file uFX_forcesAndMoments*.txt will be written. This includes the respective files for <coefficients_parts> and <coefficients_along_axis> if they are activated. The default value for <forces_and_moments_export> is false.
<output_start_iteration>: (Optional) Specifies when to start the coefficient output (coarsest iteration). The default value is 0.

<output> - <section_cut>

This category specifies section cuts on which field variables should be output independent from the general variable output. The same conventions apply for the EnSight Gold files and ultraFluidX will create a subfolder named uFX_sectionCuts, where the output of each section cut will be stored in a separate folder.

The category can have an arbitrary number of children named <section_cut_instance>, each with the following parameters:

<name>: Name of the instance, used to create the respective subfolder in uFX_sectionCuts (mandatory).
<axis>: Normal axis of the instance, its direction must be specified via the child parameters <x_dir>, <y_dir> and <z_dir>.
<point>: Point on the instance, its coordinates must be specified via the child parameters <x_pos>, <y_pos> and <z_pos> in $[m]$ .
<bounding_box>: Bounding box of the instance, must be specified via the child parameters <x_min>, <x_max>, <y_min>, <y_max>, <z_min> and <z_max> in $[m]$ .
<output_frequency>: Specifies the number of coarsest iterations between consecutive outputs. Fractions of 1 are allowed to get an output at the desired sub-time step level.
<output_start_iteration>: (Optional) Specifies when to start the section cut output (coarsest iteration) for each section cut instance. Can be used to generate high-frequency output for a specific part of the domain once the initial transient phase is completed. The default value is 0.
<triangulation>: By default, the value is false and all section cuts are exported using “nsided” elements. If set to true, the respective section cut instance is exported using “tria3” elements instead.
<output_variables>: (Optional) In this section, you can specify which variables should be included in the section cut output by setting <variable_name> to true or false. The possible options are listed in Table 1.

<output> - <partial_surface>

This category specifies parts on which surface variables should be output independent from the general variable output. The same conventions apply for the EnSight Gold files and ultraFluidX will create a separate folder in the subfolder named uFX_surfaceData, where the output of each part will be stored.

The category can have an arbitrary number of children named <partial_surface_instance>, each with the following parameters:

<name>: (Optional) Name of the instance.
<parts>: The part(s) on which the surface variables should be output, must be specified with the parameter <name> within the <parts> category. Several parts with the same output behavior can be specified via repeated usage of <name>. The specified names must exactly match the respective part names in the STL file.
<output_frequency>: Specifies the number of coarsest iterations between consecutive outputs. You can specify fractions of 1 to obtain an output at the desired sub-time step level.
<output_start_iteration>: (Optional) Specifies when to start the partial surface output (coarsest iteration) for each partial surface instance. Can be used to generate high-frequency output for a specific part of the domain, once the initial transient phase is completed. The default value is 0.
<output_variables>: In this section, you can specify which variables should be included in the section cut output by setting <variable_name> to true or false. The possible options are listed in Table 1.

<output> - <partial_volume>

This category specifies a volumetric part of the domain in which field variables should be output independent from the general variable output. The same conventions apply for the EnSight Gold files and ultraFluidX will create a separate folder where the output will be stored. The category can have an arbitrary number of children named <partial_volume_instance>, each with the following parameters:

<name>: Name of the instance, used to create the respective folder (mandatory).
<bounding_box>: Bounding box of the instance, must be specified via the child parameters <x_min>, <x_max>, <y_min>, <y_max>, <z_min> and <z_max> in $[m]$ .
<output_frequency>: Specifies the number of coarsest iterations between consecutive outputs. You can specify fractions of 1 to obtain an output at the desired sub-time step level.
<output_start_iteration>: Specifies when to start the partial volume output (coarsest iteration) for each partial volume instance. Can be used to generate high-frequency output for a specific part of the domain, once the initial transient phase is completed. The default value is 0.
<output_variables>: In this section, you can specify which variables should be included in the section cut output by setting <variable_name> to true or false. The possible options are listed in Table 1.
Note: If no variables are chosen explicitly, the full set will be exported; otherwise, only the variables that are indicated in this section are written.

<output> - <single_probe>

This category specifies single probes, where instantaneous surface data or volume data should be output independent from the general variable output. The files are stored in the uFX_probeData folder. Each probe creates one .csv file per output variable, plus an additional file that contains the probe locations (uFX_volumeProbes_***_location.csv and uFX_surfaceProbes_***_location.csv).

The category can have an arbitrary number of children named <single_probe_instance>, each with the following parameters:

<name>: (Mandatory) Name of the instance used to create the respective file or subfolder.
<x_pos>, <y_pos>, <z_pos>: Respective coordinate of the probe in $[m]$ .
<type>: Specifies if data from the nearest voxel (volume) or from the nearest surface triangle (surface) should be output.
<radius>: Specifies the radius [m] of a fictitious sphere whose containing data sources are used to determine the mean value(s) of the requested variable(s).
<output_frequency>: Specifies the number of coarsest iterations between consecutive outputs. Fractions of 1 are allowed to get an output at the desired sub-time step level.
<scientific_notation>: If set to true, the output files are written in scientific notation. If set to false, the output files are written in conventional decimal notation instead.; Default = true
<output_precision>: In combination with scientific notation (default), the output includes eight significant digits. Using this parameter, you can choose an arbitrary value.; Default = 7
<output_variables>: In this section, you can specify which variables should be included in the probe output by setting <variable_name> to true or false. The possible options depend on the probe type:; A default volume probe has five output variables (pressure, velocity (x,y,z) and velocity magnitude). You can optionally request the output of Cp, and time/window averaged pressure, density and velocity.
Note: Volume probes do not have access to wall shear stress.; A surface probe has one default output (Cp). You can optionally request pressure, velocity (x, y, z), velocity magnitude, wall shear stress (tau_wall x, y, z), density and time/window averaged pressure and wall shear stress.
<output_start_iteration>: (Optional) Specifies when to start the output (coarsest iteration) for each single probe instance.; Default = 0

<output> - <probe_file>

This category specifies probe files containing multiple locations where instantaneous surface data or volume data should be output independent from the general variable output.

The files are stored in the uFX_probeData folder. Each probe file instance will create one .csv file per output variable, plus an additional file that contains the probe locations (uFX_volumeProbes_***_location.csv and uFX_surfaceProbes_***_location.csv).

Depending on the type of the probe file, ultraFluidX will either create a single *.csv file containing the transient Cp data (surface probes, uFX_surfaceProbes_#NAME.csv) or multiple *.csv files containing pressure, velocity magnitude and velocity component data (volume probes, uFX_volumeProbes_#NAME_Variable_Name) for recording the data.

The category can have an arbitrary number of children named <probe_file_instance>, each with the following parameters:

<name>

Name of the instance, used to create the respective file(s) or subfolder (mandatory).

<source_file>

Source file containing the probe locations in *.csv format without header, each line defines a probe with the coordinates in

[m]

, which must be separated by semicolons:

x_pos;y_pos;z_pos;Description_A
x_pos;y_pos;z_pos;Description_B

<type>

Specifies if data from the nearest voxel (volume) or from the nearest surface triangle (surface) should be output for each probe location.

<radius>

Specifies the radius [m] of a fictitious sphere whose containing data sources are used to determine the mean value(s) of the requested variable(s).

<output_frequency>

Specifies the number of coarsest iterations between consecutive outputs. Fractions of 1 are allowed to get an output at the desired sub-time step level.

<scientific_notation>

If set to true, the output files are written in scientific notation. If set to false, the output files are written in conventional decimal notation instead.

Default = true

<output_precision>

Using this parameter, you can choose an arbitrary integer value.

Default = 7

<output_variables>

In this section, you can specify which variables should be included in the probe output by setting <variable_name> to true or false. The possible options depend on the probe type:

A default volume probe has five output variables (pressure, velocity (x,y,z) and velocity magnitude). You can optionally request the output of Cp, time/window averaged pressure, time/window averaged velocity and time/window averaged density.

Note: Volume probes do not have access to wall shear stress.

A surface probe has one default output (Cp). You can optionally request pressure, velocity (x, y, z), velocity magnitude, wall shear stress (tau_wall x, y, z), density and time/window averaged pressure and wall shear stress.

<output_start_iteration>

(Optional) Specifies when to start the probe output (coarsest iteration) for each probe file instance. The default value is 0.

<output> - <monitoring_surface>

This category specifies monitoring surfaces, which are arbitrarily shaped, user-defined surfaces for additional post-processing. Monitoring surfaces can be used for the additional visual output of flow field quantities on the respective surface, or for the output of integral values in a summary file.

The files are stored in the uFX_monitoringSurface folder.

The category can have an arbitrary number of children named <monitoring_surface_instance>, each with the following parameters:

<name>

Name of the instance (mandatory).

<parts>

The part(s) which define the monitoring surface. Must be specified with the parameter <name> within the <parts> category. Several parts can be specified via repeated usage of <name>. The specified names must exactly match the respective part names in the STL file.

<visual_output>

<output_frequency>

Specifies the number of coarsest iterations between consecutive outputs. You can specify fractions of 1 to obtain an output at the desired sub-time step level.

<output_start_iteration>

Specifies when to start the visual output (coarsest iteration) for each instance. The default value is 0.

<output_variables>

In this section, you can specify which variables should be included in the visual output by setting <variable_name> to true or false. The possible options include:

pressure
time_avg_pressure
window_avg_pressure
velocity
time_avg_velocity
window_avg_velocity
mass_flow
time_avg_mass_flow
window_avg_mass_flow
normal_velocity
time_avg_normal_velocity
window_avg_normal_velocity
density
time_avg_density
window_avg_density

<summary_output>

<output_frequency>

Specifies the number of coarsest iterations between consecutive outputs. You can specify fractions of 1 to obtain an output at the desired sub-time step level.

<output_start_iteration>

Specifies when to start the summary output (coarsest iteration) for each instance. The default value is 0.

<output_variables>

In this section, you can specify which variables should be included in the summary output by setting <variable_name> to true or false. The possible options include:

pressure
time_avg_pressure
window_avg_pressure
mass_flow
time_avg_mass_flow
window_avg_mass_flow
normal_velocity
time_avg_normal_velocity
window_avg_normal_velocity