Parameters

Parameters#

Every problem will contain parameters that are both specific to the problem, but also general to Oasis. All parameters will be collected in the NS_parameters dictionary, and accessible in every OasisMove hook. You can also adjust the parameters directly though the command line, by passing them as command line arguments.

Overview of parameters#

To get an impression of what parameters you might come accross in the problem files included in OasisMove, we will consider the simplest rigid flow problem as an example: the default DrivenCavity problem. By inspecting the problem file, the parameters are defined in the start of the script:

NS_parameters.update(
    # Mesh parameters
    Nx=50,
    Ny=50,

    # Fluid parameters
    nu=0.001,

    # Simulation parameters
    T=1.0,
    dt=0.005,
    folder="results_driven_cavity",

    # Oasis parameters
    testing=False,
    max_iter=2,
    dynamic_mesh=False,
    save_solution_frequency=5,
    checkpoint=500,
    print_intermediate_info=100,
    velocity_degree=1,
    pressure_degree=1,
    use_krylov_solvers=True
)

In the OasisMove problem files, we distinguish between Mesh, Fluid, Simulation, and Oasis parameters. In addition, some problems have parameters that are specific for the particular problems. The full dictionary of default parameters can be found in the top of the in problems/NSfracStep/__init__.py script.

Mesh parameters#

Mesh parameters are related to the computational mesh, and typically the resolution. In regard to the DrivenCavity problem, the mesh parameters are:

# Mesh parameters
Nx = 50
Ny = 50

By adjusting Nx and Ny we adjust the resolution of the computational domain, which for the DrivenCavity problem is a 2D unit square mesh consisting of triangular elements. The parameters Nx and Ny determine the number of uniform cell intervals in the \(x\) and \(y\) direction, respectively. These parameters can also be used to compute the totan number of triangular cells in 2D: or tetrehedral cells (in 3D) the computational domain consists of:

\[\begin{split} \text{Number of cells (2D) } &= 2 \times N_x \times N_y \\ \text{Number of cells (3D) } &= 6 \times N_x \times N_y \times N_z \end{split}\]

Fluid parameters#

Fluid parameters are related to the fluid properties. In regard to the DrivenCavity problem, the only fluid parameter is the kinematic viscosity (\(\nu\)):

# Fluid parameters
nu = 0.001

Changing the kinematic viscosity will directly influence the Reynolds number, the ratio between inertial and viscous forces defined as:

(1)#\[\begin{align} \text{Re } = \frac{u L}{\nu}, \end{align}\]

where \(u\) is the flow speed and \(L\) is a characteristic linear dimension.

Simulation parameters#

Simulation parameters are related to the computational fluid dynamics simulation. In regard to the DrivenCavity problem, the simulation parameters are:

# Simulation parameters
T = 1.0
dt = 0.005
folder = "results_driven_cavity"

Here, T is the total simulation time, usually in seconds or milliseconds depending on the application and scale of the problem. The number of time steps is controlled by the value of T, and the time step size dt, which are related as follows:

(2)#\[\begin{align} \text{Number of time steps } = \frac{T}{\Delta t}. \end{align}\]

Hence, for the default DrivenCavity problem, the simulation is run for T / dt = 200 time steps. The folder parameter determines where the results are saved for the particular problem, and is intentionally different for every problem to easier distinguish the results. Also, the **NS_namespace parameter newfolder is a derivative of the folder location:

newfolder = folder/data/[RUN NUMBER]/

and is used to determine where the solution files, which are stored to:

newfolder/Solutions

Oasis parameters#

Oasis parameters are miscellaneous parameters related to solver performance, printing simulation info, or parameters inherited from classical Oasis. In regard to the DrivenCavity problem, the Oasis parameters are:

# Oasis parameters
testing = False
max_iter = 2
dynamic_mesh = False
save_solution_frequency = 5
checkpoint = 500
print_intermediate_info = 100
velocity_degree = 1
pressure_degree = 1
use_krylov_solvers = True

The testing flag is there to notify the program where or not it is run as a test. The max_iter parameter is set to 2 for all moving domain simulations in order to ensure convergence of velocity and pressure, based on empirical evidence. By default dynamic_mesh is False, and controlls when the mesh equations are solved followed by mesh coordinate deformation. The save_solution_frequency parameter determines how often the velocity and pressure solution are stored. With the proposed value of 5, the simulation will store the solution every 5th time step. print_intermediate_info determines the frequency of printing simulation info, here set to every 100 time step. Furthermore, the velocity_degree and pressure_degree parameters determine the finite element polynomial approximation order. If use_krylov_solvers is True the solver will use the PETSc Krylov solver, instead of a standard LU solver.

Changing parameters#

Parameters can either be changed directly in the Python problem file, or directly though the command line, by passing them as command line arguments. For instance, if we want to increase the mesh resolution and extend the simulation end time to \(T=20\) for the DrivenCavity problem, you can execute the following command:

$ oasism NSfracStepMove problem=DrivenCavity Nx=100 Ny=100 T=20

Similarly, you can change any of parameters mention here, the ones listed in the problems/NSfracStep/__init__.py script, or that are specified in the Python problem script.

Contents