Default
value

averaging_interval_pr

Averaging interval for output of vertical profiles to local file DATA_1D_PR_NETCDF and/or  PLOT1D_DATA (in s). 

If this parameter is given a non-zero value, temporally averaged vertical profile data are output. By default, profile data data are not subject to temporal averaging. The interval length is limited by the parameter dt_dopr. In any case averaging_interval_pr <= dt_dopr must hold.

If an averaging interval can not be completed at the end of a run, it will be finished at the beginning of the next restart run. Thus for restart runs, averaging intervals do not necessarily begin at the beginning of the run.

cfl_factor

0.1, 0.8 or 0.9
(see right)

Time step limiting factor. 

In the model, the maximum allowed time step according to CFL and diffusion-criterion dt_max is reduced by dt = dt_max * cfl_factor in order to avoid stability problems which may arise in the vicinity of the maximum allowed timestep. The condition 0.0 < cfl_factor < 1.0 applies.

The default value of cfl_factor depends on the timestep_scheme used:

For the third order Runge-Kutta scheme it is cfl_factor = 0.9.

In case of the leapfrog scheme a quite restrictive value of cfl_factor = 0.1 is used because for larger values the velocity divergence significantly effects the accuracy of the model results. Possibly larger values may be used with the leapfrog scheme but these are to be determined by appropriate test runs.

create_disturbances

Switch to impose random perturbations to the horizontal velocity field. 

With create_disturbances = .T., random perturbations can be imposed to the horizontal velocity field at certain times e.g. in order to trigger off the onset of convection, etc..

The temporal interval between these times can be steered with dt_disturb, the vertical range of the perturbations with disturbance_level_b and disturbance_level_t, and the perturbation amplitude with disturbance_amplitude. In case of non-cyclic lateral boundary conditions (see bc_lr and bc_ns), the horizontal range of the perturbations is determined by inflow_disturbance_begin and inflow_disturbance_end. A perturbation is added to each grid point with its individual value determined by multiplying the disturbance amplitude with a uniformly distributed random number. After this, the arrays of u and v are smoothed by applying a Shuman-filter twice and made divergence-free by applying the pressure solver.

The random number generator to be used can be chosen with random_generator.

As soon as the desired flow features have developed (e.g.  convection has started), further imposing of perturbations is not necessary and can be omitted (this does not hold for non-cyclic lateral boundaries!). This can be steered by assigning an upper limit value for the perturbation energy (the perturbation energy is defined by the deviation of the velocity from the mean flow) using the parameter disturbance_energy_limit. As soon as the perturbation energy has exceeded this energy limit, no more random perturbations are assigned
. 
Timesteps where a random perturbation has been imposed are marked in the local file RUN_CONTROL by the character "D" appended to the values of the maximum horizontal velocities.

cross_normalized_x

Type of normalization applied to the x-coordinate of vertical profiles to be plotted with profil.

This parameter only applies for  data_output_format = 'profil'.

If vertical profiles are plotted with the plot software profil (data on local file PLOT1D_DATA, parameters on local file PLOT1D_PAR) the x-values of the data points can be normalized with respect to certain quantities (e.g. the near-surface heat flux) in order to ensure a better comparability. This type of normalization then applies to all profiles of one coordinate system (panel). The normalization quantities are re-calculated for each output time of each individual profile. If temporally averaged profiles are output (see averaging_interval_pr), then the normalization quantities are also temporally averaged accordingly. If the value of a normalization quantity becomes zero, then normalization for the total respective coordinate system (panel) is switched off automatically (also for the y-axis).

By default, the normalization quantities are calculated as the horizontal mean of the total model domain and and these values are also used for the normalization of profiles from subdomains (see statistic_regions). Instead of this, they can be calculated from the data of a certain subdomain by using the parameter normalizing_region (however, they are used again for all subdomains and even for the total domain). 

The user can choose between the following normalization quantities:

For each coordinate system (panel) to be drawn (see cross_profiles) an individual normalization quantity can be assigned. For example: if cross_normalized_x = 'ws2','ws3', then the x-values in the 1st coordinate system are normalized with respect to w_*² and in the 2nd system with respect to w_*³. Data of the further coordinate systems (if any are to be drawn) are not normalized. 

Using a normalization leaves all vertical profile data on local file PLOT1D_DATA unaffected, it only affects the visualization. Within profil, the normalization is steered by parameter normx which may be changed subsequently by the user in the parameter file (local file PLOT1D_PAR).
 
The assigned normalization quantity is noted in the axes labels of the respective coordinate systems (see cross_xtext).

cross_normalized_y

Type of normalization applied to the y-coordinate of vertical profiles to be plotted with profil. 

This parameter only applies for  data_output_format = 'profil'.

If vertical profiles are plotted with the plot software profil (data on local file PLOT1D_DATA, parameter on local file PLOT1D_PAR) the y-values of the data points can be normalized with respect to certain quantities (at present only the normalization with respect to the boundary layer height is possible) in order to ensure a better comparability.

The user can choose between the following normalization quantities:

For further explanations see cross_normalized_x.

cross_profiles

Determines which vertical profiles are to be presented in which coordinate system if the plot software profil is used.  

This parameter only applies for  data_output_format = 'profil'.

The default assignment is: 

cross_profiles = 

' u v ',
' pt ', 
' w"pt" w*pt* w*pt*BC wpt wptBC ', 
' w"u" w*u* wu w"v"w*v* wv ', 
' km kh ',
' l ' ,
14 * ' '

If plot output of vertical profiles is produced (see data_output_pr), the appropriate data are written to the local file PLOT1D_DATA. Simultaneously, the model produces a parameter file (local name PLOT1D_PAR) which describes the layout for a plot to be generated with the plot program profil. The parameter cross_profiles determines how many coordinate systems (panels) the plot contains and which profiles are supposed to be drawn into which panel. cross_profiles expects a character string (up to 100 characters long) for each coordinate system, which consists of the names of the profiles to be drawn into this system (all available profiles and their respective names are described at parameter data_output_pr). The single names have to be separated by one blank (' ') and a blank must be spent also at the beginning and at the end of the string. 

Example: 

cross_profiles = ' u v ', ' pt '

In this case the plot consists of two coordinate systems (panels) with the first panel containing the profiles of the horizontal velocity components ('u' and 'v') of all output times (see dt_dopr) and the second one containing the profiles of the potential temperature ('pt').

Whether the coordinate systems are actually drawn, depends on whether data of the appropriate profiles were output during the run (profiles to be output have to be selected with the parameter data_output_pr). For example if data_output_pr = 'u', 'v' was assigned, then the plot only consists of one panel, since no profiles of the potential temperature were output. On the other hand, if profiles were assigned to data_output_pr whose names do not appear in cross_profiles, then the respective profile data are output (PLOT1D_DATA) but they are not drawn in the plot.

cross_xtext

x-axis labels of vertical profile coordinate systems to be plotted with profil. 

This parameter only applies for  data_output_format = 'profil'.

The default assignment is: 

cross_xtext = 

'wind speed in ms>->1', 
'pot. temperature in K', 
'heat flux in K ms>->1', 
'momentum flux in m>2s>2', 
'eddy diffusivity in m>2s>->1', 
'mixing length in m', 
14 * ' '

This parameter can be used to assign x-axis labels to vertical profiles to be plotted with the plot software profil (for output of vertical profile data see data_output_pr).
The labels are assigned to those coordinate systems (panels) defined by cross_profiles according to their respective order (compare the default values of cross_xtext and cross_profiles).

Umlauts are possible (write “ in front of, similar to TeX), as well as super- and subscripts (use ">" or "<" in front of each character), special characters etc. (see UNIRAS manuals) when using the plot software profil.

cycle_mg

Type of cycle to be used with the multi-grid method. 

This parameter determines which type of cycle is applied in the multi-grid method used for solving the Poisson equation for perturbation pressure (see psolver). It defines in which way it is switched between the fine and coarse grids. So-called v- and w-cycles are realized (i.e. cycle_mg may be assigned the values 'v' or 'w'). The computational cost of w-cycles is much higher than that of v-cycles, however, w-cycles give a much better convergence.

data_output

With the parameter nz_do3d  the output can be limited in the vertical direction up to a certain grid point.

Output on parallel machines:

By default, with parallel runs, processors output only data of their respective subdomains into seperate local files (file names are constructed by appending the four digit processor ID, e.g. <filename>_0000, <filename>_0001, etc.). After PALM has finished, the contents of these individual files are sampled into one final file using the program combine_plot_fields.x (to be started e.g. by a suitable OUTPUT command in the mrun configuration file).

Alternatively, PALM is able to collect all grid points of a cross section on PE0 before output is done. In this case only one  output file (DATA_2D_XY_NETCDF, etc.) is created and combine_plot_fields.x does not have to be called. In case of very large numbers of horizontal gridpoints, sufficient memory is required on PE0.  This method can be used by assigning data_output_2d_on_each_pe = .F..

3d volume data output is always handled seperately by each processor so that combine_plot_fields.x has to be called anyway after PALM has been finished.

Old formats:

Beside the NetCDF format, 2d cross section data and 3d volume data can also be output, for historical reasons, in a different (binary) format using parameter data_output_format.

By assigning data_output_format = 'avs', the 3d volume data is output to the local file PLOT3D_DATA. Output is in FORTRAN binary format readable by the plot software AVS.  The order of data on the file follows the order used in the assignment for data_output (e.g. data_output = 'p', 'v',...  means that the file starts with the pressure data, followed by the v-component of the velocity, etc.). Both instantaneous and time averaged data are written on this file! Additional to this file, PALM creates a second binary file (local name PLOT3D_COOR) with coordinate information needed by AVS. As third and fourth file two ASCII files are created (AVS-FLD-format, local name PLOT3D_FLD and PLOT3D_FLD_COOR), which describe the contents of the data file and/or coordinate file and are used by AVS. However, AVS expects the content description in one file. This needs the local file PLOT3D_FLD_COOR to be appended to the file PLOT3D_FLD (by suitable OUTPUT command in the mrun configuration file: “cat PLOT3D_FLD_COOR >> PLOT3D_FLD”) after PALM has finished. To reduce the amount of data, output to this file can be done in compressed form (see do3d_compress). Further details about plotting 3d volume data with AVS can be found in chapter 4.5.5.

data_output_pr

Quantities for which vertical profiles (horizontally averaged) are to be output. 

By default vertical profile data is output to the local file DATA_1D_PR_NETCDF. The file's format is NetCDF.  Further details about processing NetCDF data are given in chapter 4.5.1.

For historical reasons, data can also be output in ASCII-format on local file PLOT1D_DATA which is readable by the graphic software profil. See parameter data_output_format for defining the format in which data shall be output.

For horizontally averaged vertical profiles always all vertical grid points (0 <= k <= nz+1) are output to file. Vertical profile data refers to the total domain but profiles for subdomains can also be output (see statistic_regions). 

The temporal interval of the output times of profiles is assigned via the parameter dt_dopr. Within the file PLOT1D_DATA, the profiles are ordered with respect to their output times.

Profiles can also be temporally averaged (see averaging_interval_pr). 

The following list shows the values which can be assigned to data_output_pr. The profile data is either defined on u-v-levels (variables marked in red) or on w-levels (green). According to this, the z-coordinates of the individual profiles vary. Beyond that, with a Prandtl layer switched on (prandtl_layer) the lowest output level is z = zu(1) instead of z = zw(0) for profiles w'' u'',w''v", wu and wv . 

#u, #v, #pt, #km, #kh, #l

These initial profiles have been either set by the user or have been calculated by a 1d-model prerun.

data_output_2d_on
_each_pe

In runs with several processors, by default, each processor outputs cross section data of its subdomain into an individual file. After PALM has finished, the contents of these files have to be sampled into one file using the program combine_plot_fields.x. 

Alternatively, by assigning data_output_2d_on_each_pe = .F., the respective data is gathered on PE0 and output is done directly into one file, so combine_plot_fields.x does not have to be called. However, in case of very large numbers of horizontal gridpoints, sufficient memory is required on PE0.

disturbance
_amplitude

Maximum perturbation amplitude of the random perturbations imposed to the horizontal velocity field (in m/s). 

The parameter create_disturbances describes how to impose random perturbations to the horizontal velocity field. Since the perturbation procedure includes two filter operations, the amplitude assigned by disturbance_amplitude is only an approximate value of the real magnitude of the perturbation.

disturbance_energy
_limit

Upper limit value of the perturbation energy of the velocity field used as a criterion for imposing random perturbations (in m²/s²). 

The parameter create_disturbances describes how to impose random perturbations to the horizontal velocity field. The perturbation energy is defined as the volume average (over the total model domain) of the squares of the deviations of the velocity components from the mean flow (horizontal average). If the perturbation energy exceeds the assigned value, random perturbations to the fields of horizontal velocities are imposed no more. The value of this parameter usually must be determined by trial and error (it depends e.g. on the total number of grid points).

disturbance_level_b

Lower limit of the vertical range for which random perturbations are to be imposed on the horizontal wind field (in m). 

This parameter must hold the condition zu(3) <= disturbance_level_b <= zu(nz-1). Additionally, disturbance_level_b <= disturbance_level_t must also hold.

The parameter create_disturbances describes how to impose random perturbations to the horizontal velocity field.

disturbance_level_t

Upper limit of the vertical range for which random perturbations are to be imposed on the horizontal wind field (in m). 

This parameter must hold the condition disturbance_level_t <= zu(nz-1). Additionally, disturbance_level_b <= disturbance_level_t must also hold.

The parameter create_disturbances describes how to impose random perturbations to the horizontal velocity field.

do2d_at_begin

Output of 2d cross section data at the beginning of a run. 

The temporal intervals of output times of 2d cross section data (see data_output) are usually determined with parameters dt_do2d_xy, dt_do2d_xz and dt_do2d_yz. By assigning do2d_at_begin = .T. an additional output will be made at the beginning of a run (thus at the time t = 0 or at the respective starting times of restart runs).

do3d_at_begin

do3d_compress

Output of data for 3d plots in compressed form. 

This parameter only applies for  data_output_format = 'avs'.

Output of 3d volume data may need huge amounts of disc storage (up to several Terabytes ore more). Data compression can serve to reduce this requirement. PALM is able to output 3d data in compressed form using 32-bit integers, if do3d_compress = .T. is assigned. This yields a loss of accuracy, but the file size is clearly reduced. The parameter do3d_precision can be used to separately define the number of significant digits for each quantity.

So far compressed data output is only possible for Cray-T3E machines. Additional information for handling compressed data is given in chapter 4.5.6.

do3d_precision

Significant digits in case of compressed data output. 

This parameter only applies for  data_output_format = 'avs'.

In case that data compression is used for output of 3d data (see do3d_compress), this parameter determines the number of significant digits which are to be output.

Fewer digits clearly reduce the amount of data. Assignments have to be given separately for each individual quantity via a character string of the form '<quantity name><number of significant digits>', e.g. 'pt2'. Only those quantities listed in data_output are admitted. Up to 9 significant digits are allowed (but large values are not very reasonable because they do not effect a significant compression).

The default assignment is do3d_precision = 'u2', 'v2', 'w2', 'p5', 'pt2'.

dt

Time step to be used by the 3d-model (in s). 

This parameter is described in detail with the initialization parameters (see dt). Additionally, it may be used as a run parameter and then applies to all restart runs (until it is changed again). A switch from a constant time step to a variable time step can be achieved with dt = -1.0.

dt_averaging_input_pr

Temporal interval of data which are subject to temporal averaging of vertical profiles and/or spectra (in s). 

By default, data from each timestep within the interval defined by averaging_interval_pr, and averaging_interval_sp are used for calculating the temporal average. By choosing dt_averaging_input_pr > dt, the number of time levels entering the average can be minimized. This reduces the CPU-time of a run but may worsen the quality of the average's statistics.

For more explanations see parameter dt_averaging_input.

Temporal interval at which data (3d volume data (instantaneous or time averaged), cross sections (instantaneous or time averaged), vertical profiles, spectra) shall be output (in s). 

Temporal interval at which time averaged 3d volume data and/or 2d cross section data shall be output (in s). 

dt_disturb

Temporal interval at which random perturbations are to be imposed on the horizontal velocity field (in s). 

The parameter create_disturbances describes how to impose random perturbations to the horizontal velocity field.

dt_dopr

Temporal interval at which data of vertical profiles shall be output (to local file DATA_1D_PR_NETCDF or/and PLOT1D_DATA) (in s). 

If output of horizontally averaged vertical profiles is switched on (see data_output_pr), this parameter can be used to assign the temporal interval at which profile data shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_dopr, which has zero value by default. Reference time is the beginning of the simulation, thus t = 0, i.e. output takes place at times t = skip_time_dopr + dt_dopr, skip_time_dopr + 2*dt_dopr, skip_time_dopr + 3*dt_dopr, etc. Since profiles can not be calculated for times lying within a time step interval, the output times can deviate from these theoretical values. If a time step ranges from t = 1799.8 to t = 1800.2, then in the example above the output would take place at t = 1800.2. In general, the output always lie between t = 1800.0 and t = 1800.0 + dt. If the model uses a variable time step, these deviations from the theoretical output times will of course be different for each output time.

In order to guarantee an output of profile data at the end of a simulation (see end_time) in any way,  end_time should be equal or a little bit larger than the respective theoretical output time. For example, if dt_dopr = 900.0 and 3600.0 seconds are to be simulated, then end_time >= 3600.0 should be chosen. 

A selection of profiles to be output can be done via parameter data_output_pr. 

Temporal interval at which data of vertical profiles shall be output (output for printouts, local file LIST_PROFIL) (in s). 

This parameter can be used to assign the temporal interval at which profile data shall be output. Reference time is the beginning of the simulation, thus t = 0. For example if dt_dopr_listing = 1800.0, then output takes place at t = 1800.0, 3600.0, 5400.0, etc. Since profiles can not be calculated for times lying within a time step interval, the output times can deviate from these theoretical values. If a time step ranges from t = 1799.8 to t = 1800.2, then in the example above the output would take place at t = 1800.2. In general, the output always lie between t = 1800.0 and t = 1800.0 + dt (numbers are related to the example above). If the model uses a variable time step, these deviations from the theoretical output times will of course be different for each output time.

In order to guarantee an output of profile data at the end of a simulation (see end_time) in any way,  end_time should be a little bit larger than the respective theoretical output time. For example, if dt_dopr_listing = 900.0 and 3600.0 seconds are to be simulated, then it should be at least  end_time > 3600.0 + dt. If variable time steps are used (which is the default), dt should be properly estimated. 

Data and output format of the file LIST_PROFIL is internally fixed. In this file the profiles of the most important model variables are arranged in adjacent columns.

dt_dots

Temporal interval at which time series data shall be output (in s). 

The default interval for the output of timeseries is calculated as shown below (this tries to minimize the number of calls of flow_statistics)

       IF ( averaging_interval_pr == 0.0 )  THEN
          dt_dots = MIN( dt_run_control, dt_dopr )
       ELSE
          dt_dots = MIN( dt_run_control, dt_averaging_input_pr )
       ENDIF

This parameter can be used to assign the temporal interval at which data points shall be output. Reference time is the beginning of  the simulation, i.e. output takes place at times t = dt_dots, 2*dt_dots, 3*dt_dots, etc. The actual output times can deviate from these theoretical values (see dt_dopr).  Is dt_dots < dt, then data of the time series are written after each time step (if this is requested it should be dt_dots = 0).

The default value of dt_dots is calculated as follows:

By default time series data is output to the local file DATA_1D_TS_NETCDF. Because of the default settings of dt_dots, it will generally be created for each model run. The file's format is NetCDF.  Further details about processing NetCDF data are given in chapter 4.5.1.

dt_do2d_xy

Temporal interval at which horizontal cross section data shall be output (in s). 

If output of horizontal cross sections is switched on (see data_output and section_xy), this parameter can be used to assign the temporal interval at which cross section data shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_do2d_xy, which has zero value by default. Reference time is the beginning of the simulation, i.e. output takes place at times t = skip_time_do2d_xy + dt_do2d_xy, skip_time_do2d_xy + 2*dt_do2d_xy, skip_time_do2d_xy + 3*dt_do2d_xy, etc. The actual output times can deviate from these theoretical values (see dt_dopr).

Parameter do2d_at_begin has to be used if an additional output is wanted at the start of a run (thus at the time t = 0 or at the respective starting times of restart runs).

dt_do2d_xz

Temporal interval at which vertical cross sections data (xz) shall be output (in s). 

If output of horizontal cross sections is switched on (see data_output and section_xz), this parameter can be used to assign the temporal interval at which cross section data shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_do2d_xz, which has zero value by default. Reference time is the beginning of the simulation, i.e. output takes place at times t = skip_time_do2d_xz + dt_do2d_xz, skip_time_do2d_xz + 2*dt_do2d_xz, skip_time_do2d_xz + 3*dt_do2d_xz, etc. The actual output times can deviate from these theoretical values (see dt_dopr).

Parameter do2d_at_begin has to be used if an additional output is wanted at the start of a run (thus at the time t = 0 or at the respective starting times of restart runs).

dt_do2d_yz

Temporal interval at which vertical cross section data (yz) shall be output (in s). 

If output of horizontal cross sections is switched on (see data_output and section_yz), this parameter can be used to assign the temporal interval at which cross section data shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_do2d_yz, which has zero value by default. Reference time is the beginning of the simulation, i.e. output takes place at times t = skip_time_do2d_yz + dt_do2d_yz, skip_time_do2d_yz + 2*dt_do2d_yz, skip_time_do2d_yz + 3*dt_do2d_yz, etc. The actual output times can deviate from these theoretical values (see dt_dopr).

Parameter do2d_at_begin has to be used if an additional output is wanted at the start of a run (thus at the time t = 0 or at the respective starting times of restart runs).

dt_do3d

Temporal interval at which 3d volume data shall be output (in s). 

If output of 3d-volume data is switched on (see data_output), this parameter can be used to assign the temporal interval at which 3d-data shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_do3d, which has zero value by default. Reference time is the beginning of the simulation, i.e. output takes place at times t = skip_time_do3d + dt_do3d, skip_time_do3d + 2*dt_do3d, skip_time_do3d + 3*dt_do3d, etc. The actual output times can deviate from these theoretical values (see dt_dopr).

Parameter do3d_at_begin has to be used if an additional output is wanted at the start of a run (thus at the time t = 0 or at the respective starting times of restart runs).

dt_restart

Temporal interval at which a new restart run is to be carried out (in s).

For a description how to assign restart times manually see run time parameter restart_time. dt_restart does not show any effect, if restart_time has not been set.

dt_run_control

Temporal interval at which run control output is to be made (in s). 

Run control information is output to the local ASCII-file RUN_CONTROL. At each output time, one line with information about the size of the time step, maximum speeds, total kinetic energy etc. is written to this file. Reference time is the beginning of the simulation, i.e. output takes place at times t = dt_run_control, 2*dt_run_control, 3*dt_run_control, etc., and always at the beginning of a model run (thus at the time t = 0 or at the respective starting times of restart runs). The actual output times can deviate from these theoretical values (see dt_dopr).

Run control information is output after each time step can be achieved via dt_run_control = 0.0.

end_time

Simulation time of the 3D model (in s). 

The simulation time is starting from the beginning of the initialization run (t = 0), not starting from the beginning of the respective restart run.

force_print_header

Steering of header output to the local file RUN_CONTROL. 

By default, informations about the model parameters in use are output to the beginning of file RUN_CONTROL for initial runs only (these informations are identical to that which are output to the local file HEADER). With force_print_header = .T., these informations are also output to RUN_CONTROL at restart runs.

mg_cycles

Number of cycles to be used with the multi-grid scheme.

This parameter determines the number of cycles to be carried out in the multi-grid method used for solving the Poisson equation for perturbation pressure (see psolver). The type of the cycles can be set with cycle_mg.

ngsrb

normalizing_region

Determines the subdomain from which the normalization quantities are calculated. 

If output data of the horizontally averaged vertical profiles (see data_output_pr) is to be normalized (see cross_normalized_x, cross_normalized_y), the respective normalization quantities are by default calculated from the averaged data of the total model domain (normalizing_region = 0) and are thus representative for the total domain. Instead of that, normalization quantities can also be calculated for a subdomain. The wanted subdomain can be given with the parameter normalizing_region, where 1 <= normalizing_region <= 9 must hold. These quantities are then used for normalizing of all profiles (even for that of the total domain).

nsor

Number of iterations to be used with the SOR-scheme. 

This parameter is only effective if the SOR-scheme is selected as pressure solver (psolver = 'sor'). The number of iterations necessary for a sufficient convergence of the scheme depends on the grid point numbers and is to be determined by appropriate test runs (the default value will not at all be sufficient for larger grid point numbers). The number of iterations used for the first call of the SOR-scheme (t = 0) is determined via the parameter nsor_ini.

nz_do3d

omega_sor

Convergence factor to be used with the the SOR-scheme. 

If the SOR-scheme is selected (psolver = 'sor'), this parameter determines the value of the convergence factor, where 1.0 <= omega_sor < 2.0 . The optimum value of omega_sor depends on the number of grid points along the different directions in space. For non-equidistant grids it can only be determined by appropriate test runs.

prandtl_number

Ratio of the eddy diffusivities for momentum and heat (K_m/K_h). 

For runs with constant eddy diffusivity (see km_constant), this parameter can be used to assign the Prandtl number (ratio K_m / K_h).

profile_columns

Number of coordinate systems to be plotted in one row by profil. 

This parameter only applies for  data_output_format = 'profil'.

It determines the layout of plots of horizontally averaged profiles (data_output_pr) when plotted with the plot software profil. Generally, the number and sequence of coordinate systems (panels) to be plotted on one page are determined by cross_profiles. profile_columns determines how many panels are to be arranged next to each other in one row (number of columns). The respective number of rows on a page is assigned by profile_rows. According to their order given by data_output_pr, the panels are arranged beginning in the top row from left to right and then continued in the following row. If the number of panels cranz > profile_columns * profile_rows, the remaining panels are drawn on an additional page. If cranz < profile_columns, then profile_columns = cranz is automatically set. If row  contains any panel, then the value of profile_rows is reduced automatically.

profile_rows

Number of rows of coordinate systems to be plotted on one page by profil. 

This parameter only applies for  data_output_format = 'profil'.

It determines the layout of plots of horizontally averaged profiles. See profile_columns.

psolver

Scheme to be used to solve the Poisson equation for the perturbation pressure. 

rayleigh_damping
_factor

Factor for Rayleigh damping. 

A so-called Rayleigh damping is applied to all prognostic variables if a non-zero value is assigned to rayleigh_damping_factor.  If switched on, variables are forced towards the value of their respective basic states (e.g. the geostrophic wind). The intensity of damping is controlled by the value the rayleigh_damping_factor is assigned to. The damping starts weakly at a height defined by rayleigh_damping_height and rises according to a sin²-function to its maximum value at the top boundary.

This method effectively damps gravity waves, caused by boundary layer convection, which may spread out vertically in the inversion layer and which are reflected  at the top boundary. This particularly happens with the upstream-spline scheme switched on (see momentum_advec or scalar_advec). Therefore, with this scheme the Rayleigh damping is switched on (rayleigh_damping_factor = 0.01) by default. Otherwise it remains switched off. 

The Rayleigh damping factor must hold the condition 0.0 <= rayleigh_damping_factor <= 1.0. Large values (close to 1.0) can cause numerical instabilities.

rayleigh_damping
_height

2/3 *
zu(nz)

Height where the Rayleigh damping starts (in m). 

With Rayleigh damping switched on (see rayleigh_damping_factor), this parameter determines the range where damping is applied. By default, Rayleigh damping will be applied in the upper third of the model domain.

residual_limit

Largest residual permitted for the multi-grid scheme (in s^-2m^-3). 

This is a parameter to steer the accuracy of the multi-grid scheme (see psolver). The assigned cycle (v- or w-cycle, see mg_cycles) is passed through until the residual falls below the limit given by residual_limit. If this is not the case after 1000 cycles, the PALM aborts with a corresponding error message.

The reciprocal value of this parameter can be interpreted as a factor by the divergence of the provisional velocity field is approximately reduced after the multi-grid scheme has been applied (thus the default value causes a reduction of the divergence by approx. 6 orders of magnitude). 

restart_time

Simulated time after which a restart run is to be carried out (in s).

The simulated time refers to the beginning of the initial run (t = 0), not to the beginning of the respective restart run. Restart runs can additionally be forced to be carried out in regular intervals using the run time parameter dt_restart.

Note:
A successful operation of this parameter requires additional modifications in the mrun-call for the respective run (see chapter 3.3).

The choice of restart_time or dt_restart does not override the automatic start of restart runs in case that the job runs out of CPU time.

section_xy

Position of cross section(s) for output of 2d horizontal cross sections (grid point index k). 

If output of horizontal cross sections is selected (see data_output), this parameter can be used to define the position(s) of the cross section(s). Up to 100 positions of cross sections can be selected by assigning section_xy the corresponding vertical grid point index/indices k of the requested cross section(s). The exact location (height level) of the cross section depends on the variable for which the output is made: zu(k) for scalars and horizontal velocities, zw(k) for the vertical velocity. Information about the exact location of the cross section is contained in the NetCDF output file (if the default NetCDF output is switched on; see data_output_format).

Assigning section_xy = -1 creates the output of horizontal cross sections averaged along z. In the NetCDF output file these (averaged) cross sections are given the z-coordinate -1.0.

Assignments to section_xy does not effect the output of horizontal cross sections of variable u_* and theta_* and the liquid water path lwp*. For these quantities always only one cross section (for z=zu(1)) is output.

section_xz

Position of cross section(s) for output of 2d (xz) vertical cross sections (grid point index j). 

section_yz

Position of cross section(s) for output of 2d (yz) vertical cross sections (grid point index i). 

termination_time
_needed

CPU time needed for terminal actions at the end of a run in batch mode (in s).

If the environment variable write_binary is set true (see chapter 3.3), PALM checks the remaining CPU time of the job after each timestep. Time integration must not consume the CPU time completely, since several actions still have to be carried out after time integration has finished (e.g. writing of binary data for the restart run, carrying out output commands, copying of local files to their permanent destinations, etc.) which also takes some time. The maximum possible time needed for these activities plus a reserve is to be given with the parameter termination_time_needed. Among other things, it depends on the number of grid points used. If its value is selected too small, then the respective job will be prematurely aborted by the queuing system, which may result in a data loss and will possibly interrupt the job chain.

An abort happens in any way, if the environment variable write_binary is not set to true and if moreover the job has been assigned an insufficient CPU time by mrun option -t.

Note:
On the IBM computers of the HLRN the time used by the job before the start of PALM have also to be accounted for (e.g. for compilation and copying of input files).

use_prior_plot1d
_parameters

Additional plot of vertical profile data with profil from preceding runs of the job chain. 

This parameter only applies for  data_output_format = 'profil'.

By default, plots of horizontally averaged vertical profiles (see data_output_pr) only contain profiles of data produced by the model run. If profiles of prior times (i.e. data of preceding jobs of a job chain) shall be plotted additionally (e.g. for comparison purposes), use_prior_plot1d_parameters = .T. must be set.

For further explanation see chapter 4.5.2.

z_max_do1d

Height level up to which horizontally averaged profiles are to be plotted with profil (in m). 

This parameter only applies for  data_output_format = 'profil'.

It affects plots of horizontally averaged profiles (data_output_pr) when plotted with the plot software profil. By default, profiles are plotted up to the top boundary. The height level up to which profiles are plotted can be decreased by assigning z_max_do1d a smaller value. Nevertheless, all vertical grid points (0 <= k <= nz+1) are still output to file PLOT1D_DATA.

If a normalization for the vertical axis was selected (see cross_normalized_y), z_max_do1d has no effect. Instead, z_max_do1d_normalized must be used.

z_max_do1d
_normalized

Normalized height level up to which horizontally averaged profiles are to be plotted with profil. 

This parameter only applies for  data_output_format = 'profil'.

It affects plots of horizontally averaged profiles (data_output_pr) when plotted with the plot software profil, if a normalization for the vertical axis is selected (see cross_normalized_y). If e.g. the boundary layer height is used for normalization, then z_max_do1d_normalized = 1.5 means that all profiles up to the height level of z = 1.5* z_i are plotted.

z_max_do2d

Height level up to which 2d cross sections are to be plotted with iso2d (in m). 

This parameter only applies for  data_output_format = 'iso2d'.

It affects plots of  2d vertical cross sections (data_output) when plotted with iso2d. By default, vertical sections are plotted up to the top boundary. In contrast, with z_max_do2d the visualization within the plot can be limited to a certain height level (0 <= z <= z_max_do2d). Nevertheless, all grid points of the complete cross section are still output to the local files PLOT2D_XZ or PLOT2D_YZ. The level up to which the section is visualized can later be changed by manually editing the file PLOT2D_XZ_GLOBAL or PLOT2D_YZ_GLOBAL (the respective iso2d-parameter is yright).

Default
value

Explanation

dt_prel

Temporal interval at which particles are to be released from a particle source (in s). 

By default particles are released only at the beginning of a simulation (t_init=0). The time of the first release (t_init) can be changed with package parameter particle_advection_start. The time of the last release can be set with the package parameter end_time_prel. If dt_prel has been set, additional releases will be at t = t_init+dt_prel, t_init+2*dt_prel, t_init+3*dt_prel, etc.. Actual release times may slightly deviate from thesel values (see e.g. dt_dopr).

The domain of the particle source as well as the distance of  released particles within this source are determined via package parameters pst, psl, psr, pss, psn, psb, pdx, pdy and pdz. By default, one particle is released at all points defined by these parameters. The package parameter particles_per_point can be used to start more than one particle per point.

Up to 10 different groups of particles can be released at the same time (see number_of_particle_groups) where each group may have a different source. All particles belonging to one group have the same density ratio and the same radius. All other particle features (e.g. location of the source) are identical for all groups of particles.

By default, particles are weightless and transported passively with the resolved scale flow. Particles can be given a mass and thus an inertia by assigning the package parameter density_ratio a non-zero value (it defines the ratio of the density of the fluid and the density of the particles). In these cases their radius must also be defined, which affects their flow resistance.

Boundary conditions for the particle transport can be defined with package parameters bc_par_t, bc_par_lr, bc_par_ns and bc_par_b.

For analysis, additional output of particle information in equidistant temporal intervals can be carried out using dt_write_particle_data (file PARTICLE_DATA).

Statistical informations (e.g. the total number of particles used, the number of particles exchanged between the PEs, etc.) are output to the local file PARTICLE_INFOS, if switched on by the parameter write_particle_statistics.

If a job chain is to be carried out, particle informations for the restart run (e.g. current location of all particles at the end of the run) is output to the local file PARTICLE_RESTART_DATA_OUT, which must be saved at the end of the run and given as an input file to the restart run under local file name PARTICLE_RESTART_DATA_IN using respective file connection statements in the mrun configuration file.

The output of particles for visualization with the graphic software dvrp is steered by the package parameter dt_dvrp. For visualization purposes particles can be given a diameter by the parameter dvrp_psize (this diameter only affects the visualization). All particles have the same size. Alternatively, particles can be given an individual size and a color by modifying the user-interface (subroutine user_init_particles). Particles can pull a “tail” behind themselves to improve their visualization. This is steered via the parameter use_particle_tails.

So far, the particle transport realized in PALM does only work duly in case of a constant vertical grid spacing!

bc_par_b

Bottom boundary condition for particle transport.

By default, particles are reflected at the bottom boundary. Alternatively, a particle absorption can set by bc_par_b = ´absorb´.

bc_par_lr

Lateral boundary condition (x-direction) for particle transport.

By default, cyclic boundary conditions are used along x. Alternatively, reflection (bc_par_lr = ´reflect´) or absorption (bc_par_lr = ´absorb´) can be set.

This lateral boundary conditions should correspond to the lateral boundary condition used for the flow (see bc_lr).

bc_par_ns

Lateral boundary condition (y-direction) for particle transport.

By default, cyclic boundary conditions are used along y. Alternatively, reflection (bc_par_ns = ´reflect´) or absorption (bc_par_ns = ´absorb´) can be set.

bc_par_t

Top boundary condition for particle transport.

By default, particles are absorbed at the top boundary. Alternatively, a reflection condition can be set by bc_par_t = ´reflect´.

density_ratio

0.0, 9 *
9999999.9

Ratio of the density of the fluid and the density of the particles.

With the default value the particles are weightless and transported passively with the resolved scale flow. In case of density_ratio /= 0.0 particles have a mass and hence inertia so that their velocity deviates more or less from the velocity of the surrounding flow. Particle velocity is calculated analytically and depends on (besides the density ratio and the current velocity difference between particles and surrounding fluid) the particle radius which is determined via radius as well as on the molecular viscosity (assumed as 1.461E-5 m²/s).

If density_ratio = 1.0, the particle density corresponds to the density of the surrounding fluid and the particles do not feel any buoyancy. Otherwise, particles will be accelerated upwards (density_ratio > 1.0) or downwards (density_ratio < 1.0).

With several groups of particles (see number_of_particle_groups), each group can be assigned a different value. If the number of values given for density_ratio is less than the number of groups defined by number_of_particle_groups, then the last assigned value is used for all remaining groups. This means that by default the particle density ratio for all groups will be 0.0.

Temporal interval at which time series data of particle quantities shall be output (in s). 

dt_write_particle_ data

Temporal interval for output of particle data (in s).

This parameter can be used to assign the temporal interval at which particle data shall be output. Data are output to the local file PARTICLE_DATA. See the file description for more details about its format.

By default, no particle data are output.

dvrp_psize

Diameter that the particles is given in visualizations with the dvrp software (in m). 

In case that particles are visualized with the dvrp software (see chapter 4.5.7), their size can be set by parameter dvrp_psize. All particles are displayed with this same size.

Alternatively, the particle diameters can be set with the user-interface in routine user_init_particles (at the beginning of the simulation) and/or can be redefined after each timestep in routine user_particle_attributes (both routines can be found in file user_interface.f90). 

Note: This parameter determines exclusively the size under which particles appear in the dvrp visualization. The flow relevant particle radius is determined via the particle package parameter radius!

maximum_number_of_
particles

Maximum number of particles (on a PE). 

This parameter allows to set the number of particles for which memory must be allocated at the beginning of the run. If this memory becomes insufficient during the run, due to the release of further particles (see dt_prel), then more memory is automatically allocated.

maximum_number_of_
tailpoints

Maximum number of tailpoints that a particle tail can have. 

 maximum_number_of_tailpoints sets the number of descrete points the tail consists of. A new point is added to the particle tails after each time step. If the maximum number of tail points is reached after the corresponding number of timesteps, the oldest respective tail points is deleted within the following timestep. 

All particle tails have the same number of points. The maximum length of these tails is determined by the value of maximum_number_of_tailpoints and by the minimum distance between each of the adjoining tailpoints,  which can be set by minimum_tailpoint_distance. Additionally, it can be determined that the temporal displacement between the current position of the particle and the oldest point of the tail may become not larger than a value to be assigned by maximum_tailpoint_age.

maximum_tailpoint_
age

Maximum age that the end point of a particle tail is allowed to have (in s). 

If the temporal displacement between the oldest point of a particle tail and the current position of the particle becomes larger than the value given by maximum_tailpoint_age, this oldest point (which defines the end of the tail) is removed. If this time is so small that the number of points defining the particle tail do not exceed the value given by maximum_number_of_tailpoints, then the length the particle tails is a measure for the distance the particle travelled along during the time interval defined via maximum_tailpoint_age, i.e. for the particle velocity. Fast particles will have long tails, slow particles shorter ones (note: this will not neccessarily hold if minimum_tailpoint_distance = 0.0).

minimum_tailpoint_distance

Minimum distance allowed between two adjacent points of a particle tail (in m). 

In case of minimum_tailpoint_distance > 0.0 the particle tail is extended by a new point only if the distance between its current position and the most recent tail point exceed the distance given via minimum_tailpoint_distance.

If the length of the particle tails shall be proportional to the respective particle velocity, the parameter maximum_tailpoint_age must also be set appropriately.

particle_advection_
start

Time of the first release of particles (in s).

If particles are not to be released at the beginning of the run, the release time can be set via particle_advection_start.
If particle transport is switched on in a restart run, then read_particles_from_restartfile = .F. is also required.

See also end_time_prel.

particle_maximum_age

Maximum allowed age of particles (in s). 

If the age of a particle exceeds the time set by particle_maximum_age, the particle as well as its tail is deleted.

pdx

Distance along x between particles within a particle source (in m). 

If the particle source shall be confined to one grid point, the distances given by pdx, pdy and pdz must be set larger than the respective domain size or psl = psr has to be set alternatively.

pdx can be assigned a different value for each particle group (see number_of_particle_groups).

pdy

pdz

psb

psl

psn

psr

pss

pst

radius

random_start_position

Initial position of the particles is varied randomly within certain limits. 

By default, the initial positions of particles within the source excatly correspond with the positions given by psl, psr, psn, pss, psb, pst, pdx, pdy, and pdz. With random_start_position = .T. the initial positions of the particles are allowed to randomly vary from these positions within certain limits. 

Very important:
In case of random_start_position = .T., the random-number generators on the individual PEs no longer  run synchronously. If random disturbances are applied to the velocity field (see create_disturbances), then as consequence for parallel runs the realizations of the turbulent flow fields will deviate between runs which used different numbers of PEs!

read_particles_from_
restartfile

Read particle data from the previous run. 

By default, with restart runs particle data is read from file PARTICLE_RESTART_DATA_IN, which is created by the preceding run. If this is not requested or if in a restart run particle transport is switched on for the first time (see particle_advection_start), then read_particles_from_restartfile = .F. is required.

vertical_particle_
advection

Switch on/off vertical particle transport.

By default, particles are transported along all three directions in space. With vertical_particle_advection = .F., the particles will only be transported horizontally.

write_particle_
statistics

Switch on/off output of particle informations.

For write_particle_statistics = .T. statistical informations (e.g. the total number of particles used, the number of particles exchanged between the PEs, etc.) which may be used for debugging are output to the local file PARTICLE_INFOS. 

Note: For parallel runs files may become very large and performance of PALM may decrease.

Default
value

dt_dvrp

Temporal interval of scenes to be displayed with the dvrp software (in s). 

Isosurfaces, cross sections and particles can be displayed simultaneous. The display of particles requires that the particle transport is switched on (see dt_prel). Objects to be displayed have to be determined with mode_dvrp.

If output of scenes created by dvrp software is switched on (see mode_dvrp), this parameter can be used to assign the temporal interval at which scenes are to be created (and the respective  graphical data is to be output to the streaming server). Reference time is the beginning of  the simulation, i.e. output takes place at times t = dt_dvrp, 2*dt_dvrp, 3*dt_dvrp, etc. The actual output times can deviate from these theoretical values (see dt_dopr).  Is dt_dvrp < dt, then scenes are created and output after each time step (if this is requested it should be dt_dvrp = 0).

dvrp_directory

Name of the directory into which data created by the dvrp software shall be saved. 

By default, the directory name is generated from the user name (see package parameter dvrp_username) and the base file name (given as the argument of mrun option -d) as '<user name>/<base file name>'.

dvrp_file

Name of the file into which data created by the dvrp software shall be output. 

This parameter can be given a value only in case of dvrp_output = 'local' which determines that the data created by dvrp is output to a local file (on the machine where PALM is executed). Apart from the default, it is only allowed to assign '/dev/null' (which means that no output is really stored). This can be used for special runtime measurements of the dvrp software.

dvrp_host

'origin.rvs.
uni- hanover.de'

Name of the computer to which data created by the dvrp software shall be transferred. 

In case of dvrp_output = 'rtsp' only the default value is allowed (streaming server of the RRZN). For dvrp_output = 'local' the assigned value is ignored.

dvrp_output

Output mode for the dvrp software.

dvrp_password

Password for the computer to which data created by the dvrp software is to be transferred. 

Assigning a password is only necessary in case of dvrp_output = 'ftp'. For dvrp_output = 'rtsp' the default value must not be changed!

dvrp_username

User name of a valid account on the computer to which data created by the dvrp software is to be transferred. 

Assigning a value to this parameter is required in case of dvrp_output = 'rtsp' or 'ftp'.

mode_dvrp

Graphical objects (isosurfaces, slicers, particles) which are to be created by the dvrp software. 

Several different objects can be assigned simultaneously and will be displayed in the same scene. Allowed values for mode_dvrp are 'isosurface#' (isosurface), 'slicer#' (cross sections), and 'particles'. Within the strings the hash character ("#") has to be replaced by a digit ≤9. Up to 10 objects can be assigned at the same time, e.g. : 

mode_dvrp = 'isosurface2', 'slicer1', 'particles', 'slicer2'

In this case one isosurface, two cross sections, and particles will be created. The quantities for which an isosurface are to be created have to be selected with the parameter data_output, those for cross sections with data_output (data_output also determines the orientation of the cross section, thus xy, xz, or yz). Since for data_output and data_output lists of variables may be assigned, the digit at the end of the mode_dvrp-string selects the quantity, which is given at the respective position in the respective list (e.g. 'isosurface2' selects the quantity given in the second position of data_output). If e.g. data_output and data_output are assigned as data_output = 'u_xy', 'w_xz', 'v_yz' and data_output = 'pt', 'u', 'w' are indicated, then - assuming the above assignment of mode_dvrp - an isosurface of u, a horizontal cross section of u and a vertical cross section (xz) of w is created. For locations of the cross sections see data_output. The theshold value for which the isosurface is to be created can be defined with parameter threshold.

The vertical extension of the displayed domain is given by nz_do3d.

The vertical extension of the displayed domain is given by nz_do3d.

Assignments of mode_dvrp must correspond to those of data_output and data_output! If e.g. data_output = 'pt_xy' and data_output = 'w' was set, then only the digit "1" is allowed for mode_dvrp, thus 'isosurface1' and/or 'slicer1'. 

Further details about using the dvrp software are given in chapter 4.5.7.

superelevation

Superelevation factor for the vertical coordinate. 

For domains with unfavorable ratio between the vertical and the horizontal size (the vertical size is determined by nz_do3d) a superelevation /= 1.0 may be used. If e.g. the horizontal size is substantially larger than the vertical size, a superelevation much larger than 1.0 should be used, since otherwise the domain appears as a "flat disk" in the visualization and thus the vertical direction is only very poorly resolved.

superelevation_x

Superelevation factor for the horizontal (x) coordinate. 

This parameter can be used to stretch the displayed domain along the x-direction. See also superelevation.

superelevation_y

This parameter can be used to stretch the displayed domain along the y-direction. See also superelevation.

threshold

Threshold value for which an isosurface is to be created by the dvrp software. 

If the creation of isosurfaces is switched on via parameter mode_dvrp, then the respective threshold value for which the isosurface is to be created can be assigned via threshold. If several isosurfaces are given by mode_dvrp, then an individual threshold value for each isosurface can be assigned. The order of the threshold values refers to the order of the isosurfaces given by mode_dvrp.

Default
value

averaging_interval_sp

Averaging interval for spectra output to local file DATA_1D_SP_NETCDF and/or  PLOTSP_X_DATA /    PLOTSP_Y_DATA (in s). 

If this parameter is given a non-zero value, temporally averaged spectra data are output. By default, spectra data data are not subject to temporal averaging. The interval length is limited by the parameter dt_dosp. In any case averaging_interval_sp <= dt_dosp must hold.

If an averaging interval can not be completed at the end of a run, it will be finished at the beginning of the next restart run. Thus for restart runs, averaging intervals do not necessarily begin at the beginning of the run.

Vertical level for which horizontal spectra are to be calculated and output (gridpoints).

data_output_sp

Quantities for which horizontal spectra are to be calculated and output.

Allowed values are:  data_output_sp = 'u', 'v', 'w', 'pt', 'q'.

Spectra are calculated using the FFT-method defined by fft_method.

By default spectra data are output to the local file DATA_1D_SP_NETCDF. The file's format is NetCDF.  Further details about processing NetCDF data are given in chapter 4.5.1.

The temporal interval of the output times of profiles is assigned via the parameter dt_dosp. 

The vertical levels for which spectra are to be computed and output must be given by parameter comp_spectra_level.

dt_dosp

Temporal interval at which spectra data shall be output (in s). 

If output of horizontal spectra is switched on (see data_output_sp), this parameter can be used to assign the temporal interval at which spectral data  shall be output. Output can be skipped at the beginning of a simulation using parameter skip_time_dosp, which has zero value by default. Reference time is the beginning of  the simulation, i.e. output takes place at times t = skip_time_dosp + dt_dosp, skip_time_dosp + 2*dt_dosp, skip_time_dosp + 3*dt_dosp, etc. The actual output times can deviate from these theoretical values (see dt_dopr).  If dt_dosp < dt, then spectral data are output after each time step (if this is requested it should be dt_dosp = 0).

plot_spectra_level

Vertical level(s) for which horizontal spectra are to be plotted (in gridpoints). 

This parameter only affects the display of spectra in plots created with profil. The spectral data created and output to file are exclusively determined via comp_spectra_level.

spectra_direction

Direction(s) along which spectra are to be calculated. 

Allowed values are 'x', 'y' and 'xy'. For every quantity given by data_output_sp a corresponding direction must be assigned.

Calculation of spectra requires cyclic boundary conditions along the respective directions (see bc_lr and bc_ns).