This section describes the general information on setting up your testcases with Ateles.
The input file written in Lua provides all simulation
parameter like geometry, initional condition, scheme, etc. for the Ateles
solver. Lua syntax is fairly easy to follow and we go on describing all the
features we use in detail.
Hint: "--" specifies a comment.
It is also good to know that Lua is case sensitive.
Additional, Lua executes the file in linear fashion,
thus everything you want to use (like functions for initial condition)
need to be defined before use.
The general overall structure of the Lua input file for Ateles
can be seen in the file ateles.lua present in the repository root
which we assume you already checked out.
This also is the default name for the input file,
however different names can be used in case you want to use
and keep multiple scripts.
You would just need to pass those input file as a command line argument.
If no input file is specified,
the code checks and runs for the default input file if present.
Every simulation should have a name,
which is specified by a variable called simulation_name.
If you would like for example to set up a testcase for flow through a cube,
it could be called 'flow_cube'.
simulation_name = 'flow_cube'
You can use just anything as a simulation name, just make it clear and descriptive, as it will help you to identify produced results from the simulation. The simulation name will appear in all output files, so if you use good and unique names, you always know where a particular output came from.
The variable sim_control is used to define the stopping criteria or the time
when you would like the simulation to finish.
Currently there are three possible options:
Running simulation for certain specific steps in simulation time:
sim_control = {
time_control = {
min = 0,
max = {sim = 5.0}
}
}
Here max denotes the 'final simulation time'
(amount of time we want to simulate in seconds).
In this case it will end after 5 seconds.
Running simulation for certain maximum iterations:
sim_control = {
time_control = {
min = 0,
max = {iter = 1000}
}
}
Here max denotes the 'maximum number of iterations'
after which the simulation stops.
In this case the simulation will end after 1000 iterations.
Running simulation for a specific amount of computation time:
sim_control = {
time_control = {
min = 0,
max = {clock = 3600}
}
}
Here max denotes the 'maximum computation time' in seconds.
In this case it is 1 hour (3600s).
Note that if max is not defined as a table, e.g. max = 1.0,
it refers to the simulation time.
You can also specify the frequency at which information about the current time
is printed to the screen.
For that you have to define a table called interval in time_control.
Like max (and also min) this is a time setting
and can be provided in terms of the prescribed definitions.
Complicated geometries are created by Seeder, a preprocessing tool with which you can get familiar with by visiting its documentation. For the moment, we will consider a simple pre-defined geometry (in our case a cube with periodic boundries and no obstacles).
mesh = {
predefined = 'cube',
origin = {
-1.0,
-1.0,
-1.0
},
length = 2,
refinementLevel = 4
}
We can specify the length and position (origin) of that cube.
The position of the mesh is only relevant
if you specify positions of other objects, too,
such as initial conditions or trackers.
Next, the refinementLevel tells Ateles how fine the space is discretized.
A refinement level of 4 means that the space is cut into 2^4 portions
in each dimension.
The scheme definitions can be given through the variable scheme.
It further contains the variables spatial and temporal.
It is possible to use predefined names such as 'modg'
(for modal discontinuous Galerking scheme) in the spatial variable.
The maximal polynomial degree for each spatial direction is given
as input through the variable m.
The temporal variable can also take predefined names as an input.
Next we define the equation system and the related parameters. The possible equations that are implemented in Ateles can be used following the below mentioned syntax.
Euler Equations:
equation = {
name = 'euler', -- we solve euler equations
numflux = 'lax_friedrich', -- numerical flux to use
-- possible are 'lax_friedrich', 'godunov' or 'hll'
isen_coef = 1.4, -- isentropic coefficient
r = 1.0, -- ideal gas constant
material = {
characteristic = 'global_euler3D_characteristic',
relax_velocity = 'global_euler3D_relax_velocity',
relax_temperature = 'global_euler3D_relax_temperature'
}
}
-- cv heat capacity
equation["cv"] = equation["r"] / (equation["isen_coef"] - 1.0)
Navier Stokes Equations:
equation = {
name = 'navier_stokes', -- we solve navier stokes equations
mu = 1.831e-05, -- viscosity (default = 2.121996-314)
therm_cond = 2.55e-02, -- thermal conductivity (default = 6.953195-310)
isen_coef = 1.4, -- isentropic coefficient
r = 296.0, -- ideal gas constant
material = {
characteristic = 'global_euler3D_characteristic',
relax_velocity = 'global_euler3D_relax_velocity',
relax_temperature = 'global_euler3D_relax_temperature'
}
}
--(cv) heat capacity and (r) ideal gas constant
equation["cv"] = equation["r"] / (equation["isen_coef"] - 1.0)
Maxwells Equations:
equation = {
name = 'maxwell',-- we solve maxwell’s equations
material = {
permeability = 'global_maxwell_permeability',
permittivity = 'global_maxwell_permittivity',
conductivity = 'global_maxwell_conductivity'
}
}
Filtered Navier Stokes Equations:
equation = {
name = 'filtered_navier_stokes', -- we solve filtered navier stokes equations
mu = 1.831e-05, -- viscosity
therm_cond = 2.55e-02, -- thermal conductivity
isen_coef = 1.4, -- isentropic coefficient
r = 296.0, -- ideal gas constant
nvar = 5,
-- Turbulence parameter for Smagorinsky model
turbulence_model = 'smagorinsky',
-- Germano-Lilli model
--turbulence_model = 'germano'
Cs = 0.04, -- suggested value between 0.1 and 0.2
Ci = 0.005, -- Value for Yoshizawa model
prandtl_sgs = 0.6, -- suggested value
material = {
characteristic = 'global_euler3D_characteristic',
relax_velocity = 'global_euler3D_relax_velocity',
relax_temperature = 'global_euler3D_relax_temperature'
}
}
Maxwell Equations with divergence correction:
equation = {
name = 'maxwellDivCorrection', -- we solve maxwell’s equations with divergence correction
mu = perma, -- the magnetic permeability of vacuum
epsi = permit, -- the electric permitivity of vacuum
chi = 1.0, -- parameter for electric divergence cleaning
gam = 1.0, -- parameter for magnetic divergence cleaning
material = {
permeability = 'global_maxwell_permeability',
permittivity = 'global_maxwell_permittivity',
conductivity = 'global_maxwell_conductivity'
}
}
Some of the configuration is equation specific, as different equation systems consist of different terms and variables and therefore need different configuration settings. Thus we are not going into detail about each and every setting here.
All of these settings can be defined by constant values, functions in the Lua configuration file, or as predefined functions implemented in the solver. It is important to know that constants defined in the configuration file are stored in the 'solver environment' while initializing the simulation, whereas Lua functions need to be evaluated at every timestep. Taking this into consideration, constants or predefined values are handled within the solver, but Lua functions imply the change of the 'evaluation environment', i.e. we need to run Lua code, which is inherently slow.
Initial conditions can be specified using the initial_condition variable.
Through this all the initial condition
for the state variables can be specified.
These might be predefined functions, Lua functions or just constants.
Material denotes parameters bound to specific reagions of the domain. With material, you can e.g. specify a sphere inside your flow domain with a given porosity. Material is also defined by either constants, Lua functions or predefined functions.
Todo
Describe source terms in short words
Restart files are the main method for writing data during the simulation
and can also used for post-processing e.g. visualization.
For writing, the name of the restart folder
needs to be specified in the variable write.
The temporal definitions of the restart files
can be given through the variable time.
In the time_control table one can specify
min,max,min and max with the variable interval.Again min, max and interval are time settings
and can be defined in the same way as described in
General Simulation Settings.
As the name implies, restart files can also be used to restart a simulation
with the state stored in it. To read a restart file, the variable read is
used. It defines the file to read and restart the simulation from.
restart = {
---- file to restart from
--read = './restart/simulation_header_1.892E-03.lua',
-- folder to write restart data to
write = './restart/',
-- temporal definition of restart write
time_control = {
min = 0,
max = {clock = 3600},
interval = {iter = 10}
}
}
In the above example the generation of the restart files
starts when the simulation begins
and ends at least after 3600 seconds (one hour) of computation time.
In this timeframe every 10th iteration a restart file is being created.
The variable read is commented out for this example.
Note
You should make sure that you create the directory for storing the restart files in advance. This needs to be done manually.