- Generated on Thu Nov 21 2024 03:41:30 for Neko by
1.9.1
|
Neko
0.9.99
A portable framework for high-order spectral element flow simulations
|
The case file defines all the parameters of a simulation. The format of the file is JSON, making it easy to read and write case files using the majority of the popular programming languages. JSON is heirarchical and, and consists of parameter blocks enclosed in curly braces. These blocks are referred to as objects. The case file makes use objects to separate the configuration of different parts of the solver. We refer the reader to the examples shipped with the code to get a good idea of how a case file looks. The table below provides a complete reference for all possible configuration choices.
The current high-level structure of the case file is shown below.
The version keywords is reserved to track changes in the format of the file. The the subsections below we list all the configuration options for each of the high-level objects. Some parameters will have default values, and are therefore optional.
A common scheme for controlling the output frequency is applied for various outputs. It is described already now in order to clarify the meaning of several parameters found in the tables below.
The frequency is controlled by two paramters, ending with _control and _value, respectively. The latter name is perhaps not ideal, but it is somewhat difficult to come up with a good one, suggestions are welcome.
The _value parameter is a number, that defines the output frequency, but the interpretation of that number depends on the choice of _control. The three following options are possible.
simulationtime, then _value is the time interval between the outputs.tsteps, then _value is the number of time steps between the outputs.nsamples, then _value is the total number of outputs that will be performed in the course of the simulation.never, then _value is ignored and output is never performed.This object is mostly used as a high-level container for all the other objects, but also defines several parameters that pertain to the simulation as a whole.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
mesh_file | The name of the mesh file. | Strings ending with .nmsh | - |
output_boundary | Whether to write a bdry0.f0000 file with boundary labels. Can be used to check boundary conditions. | true or false | false |
output_directory | Folder for redirecting solver output. Note that the folder has to exist! | Path to an existing directory | . |
output_precision | Whether to output snapshots in single or double precision | single or double | single |
load_balancing | Whether to apply load balancing. | true or false | false |
output_partitions | Whether to write a partitions.vtk file with domain partitioning. | true or false | false |
output_checkpoints | Whether to output checkpoints, i.e. restart files. | true or false | false |
checkpoint_control | Defines the interpretation of checkpoint_value to define the frequency of writing checkpoint files. | nsamples, simulationtime, tsteps, never | - |
checkpoint_value | The frequency of sampling in terms of checkpoint_control. | Positive real or integer | - |
checkpoint_format | The file format of checkpoints | chkp or hdf5 | chkp |
restart_file | checkpoint to use for a restart from previous data | Strings ending with .chkp | - |
restart_mesh_file | If the restart file is on a different mesh, specifiy the .nmsh file used to generate it here | Strings enging with .nmsh | - |
mesh2mesh_tolerance | Tolerance for the restart when restarting from another mesh | Postive reals | 1e-6 |
timestep | Time-step size | Positive reals | - |
variable_timestep | Whether to use variable dt | true or false | false |
max_timestep | Maximum time-step size when variable time step is activated | Positive reals | - |
target_cfl | The desired CFL number | Positive real | 0.4 |
cfl_max_update_frequency | The minimum interval between two time-step-updating steps in terms of time steps | Integer | 0 |
cfl_running_avg_coeff | The running average coefficient a where cfl_avg_new = a * cfl_new + (1-a) * cfl_avg_old | Positive real between 0 and 1 | 0.5 |
max_dt_increase_factor | The maximum scaling factor to increase time step | Positive real greater than 1 | 1.2 |
min_dt_decrease_factor | The minimum scaling factor to decrease time step | Positive real less than 1 | 0.5 |
cfl_deviation_tolerance | The tolerance of the deviation from the target CFL number | Positive real less than 1 | 0.2 |
end_time | Final time at which the simulation is stopped. | Positive reals | - |
job_timelimit | The maximum wall clock duration of the simulation. | String formatted as HH:MM:SS | No limit |
output_boundary field When the output_boundary setting is set to true, and additional .fld file will be stored in the beginning of the simulation, where the recognized boundaries will be marked with an integer number. This is a good way to debug the simulation setup. The value of the number depends on the type of the boundary as follows:
w label.v label.o label.sym label.on label.Note that the boundary conditions can be both prescribed via the labels in the case file or built into the mesh via conversion from a .re2 file. Both types will be picked up and marked in the field produced by output_boundary.
Used to define the properties of the numerical discretization.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
polynomial_order | The oder of the polynomial basis. | Integers, typically 5 to 9 | - |
time_order | The order of the time integration scheme. Refer to the time_scheme_controller type documention for details. | 1,2, 3 | - |
dealias | Whether to apply dealiasing to advection terms. | true or false | false |
dealiased_polynomial order | The polynomial order in the higher-order space used in the dealising. | Integer | 3/2(polynomial_order + 1) - 1 |
The configuration of the fluid solver and the flow problem. Contains multiple subobjects for various parts of the setup.
As per the governing equations, Neko requires the value of the density and dynamic viscosity to define the flow problem. These can be provided as rho and mu in the case file.
Alternatively, one may opt to provide the Reynolds number, Re, which corresponds to a non-dimensional formulation of the Navier-Stokes equations. This formulation can effectively be obtained by setting \( \rho = 1 \) and \( \mu = 1/Re \). This is exactly what Neko does under the hood, when Re is provided in the case file.
Note that if both Re and any of the dimensional material properties are provided, the simulation will issue an error.
As an alternative to providing material properties in the case file, it is possible to do that in a special routine in the user file. This is demonstrated in the rayleigh-benard-cylinder example. Ultimately, both rho and mu have to be set in the subroutine, but it can be based on arbitrary computations and arbitrary parameters read from the case file. Additionally, this allows to change the material properties in time.
The optional boundary_types keyword can be used to specify boundary conditions. The reason for it being optional, is that some conditions can be specified directly inside the mesh file. In particular, this happens when Nek5000 .re2 files are converted to .nmsh. Periodic boundary conditions are always defined inside the mesh file.
The value of the keyword is an array of strings, with the following possible values:
w, a no-slip wall.v, a velocity Dirichlet boundary.sym, a symmetry boundary.o, outlet boundary.on, Dirichlet for the boundary-parallel velocity and homogeneous Neumann for the wall-normal. The wall-parallel velocity is defined by the initial condition.sh, Non-penetration condition combined with a set shear stress vector. Only works with axis-aligned boundaries. See below for how to set the stress vector.d_vel_u, d_vel_v, d_vel_w (or a combination of them, separated by a "/"), a Dirichlet boundary for more complex velocity profiles. This boundary condition uses a more advanced user interface.d_pres, a boundary for specified non-uniform pressure profiles, similar in essence to d_vel_u,d_vel_v and d_vel_w. Can be combined with other complex Dirichlet conditions by specifying e.g.: "d_vel_u/d_vel_v/d_pres".o+dong, outlet boundary using the Dong condition.on+dong, an on boundary using the Dong condition, ensuring that the wall-normal velocity is directed outwards.wm, Non-penetration condition combined with a wall model that sets the shear stress vector. Only works with axis-aligned boundaries.In some cases, only some boundary types have to be provided. For example, when one has periodic boundaries, like in the channel flow example. In this case, to put the specification of the boundary at the right index, preceding boundary types can be marked with an empty string. For example, if boundaries with index 1 and 2 are periodic, and the third one is a wall, we can set.
Some boundary types require extra input to make sense, e.g. for v, the velocity value to be set has to be specified. This is controlled by separate JSON objects inside the fluid, as specified below.
The object inflow_condition is used to specify velocity values at a Dirichlet boundary. This does not necessarily have to be an inflow boundary, so the name is not so good, and will most likely be changed along with type changes in the code. Since not all cases have Dirichlet boundaries (note, the special case of a no-slip boundary is treated separately in the configuration), this object is not obligatory. The means of prescribing the values are controlled via the type keyword:
user, the values are set inside the compiled user file.uniform, the value is a constant vector, looked up under the value keyword.blasius, a Blasius profile is prescribed. Its properties are looked up in the case.fluid.blasius object, see below.The object shear_stress is used to specify the shear stress vector used at the sh boundaries. The only keyword to specify is value, which should be a real vector with three components, corresponding to the three coordinate axes. It is the responsibility of the user to set the vector in the direction parallel to the boundary.
The object wall_modelling is used to specify the wall model configuration for wm boundaries. The following wall models are currently available, selectable via the type keyword:
rough_log_law. Implements the logarithmic law for rough walls. Additional parameters are kappa, B, and z0. The latter is the roughness length-scale normalizing the wall-normal coordinate, and the former two are the standard log-law constants. The value of kappa defaults to 0.41.spalding. Implements the Spalding profile. Additional parameters are kappa and B, which are the standard log-law constants. The default values are 0.41 and 5.2, respectively.For all wall models, the distance to the sampling point has to be specified based on the off-wall index in the wall-normal direction. Thus, the sampling is currently from a GLL node and arbitrary distances are not yet supported. The index is set by the h_index keyword, with 1 being the minimal value, and the polynomial order + 1 being the maximum.
A 3D field with the name tau will be registered in the field registry. At wm boundaries it will store the magnitude of the predicted stress. This can be used to post-process the predictions. Additionally, the sampling points are marked with values -1 in this field, for verification purposes.
The object initial_condition is used to provide initial conditions. It is mandatory. Note that this currently pertains to both the fluid, but also scalars. The means of prescribing the values are controlled via the type keyword:
user, the values are set inside the compiled user file. as explained in the user defined initial condition section of the user file documentation.uniform, the value is a constant vector, looked up under the value keyword.blasius, a Blasius profile is prescribed. Its properties are looked up in the case.fluid.blasius object, see below.point_zone, the values are set to a constant base value, supplied under the base_value keyword, and then assigned a zone value inside a point zone. The point zone is specified by the name keyword, and should be defined in the case.point_zones object. See more about point zones point-zones.md.field, where the initial condition is retrieved from a field file. The following keywords can be used:| Name | Description | Admissible values | Default value |
|---|---|---|---|
file_name | Name of the field file to use (e.g. myfield0.f00034). | Strings ending with f***** | - |
interpolate | Whether to interpolate the velocity and pressure fields from the field file onto the current mesh. | true or false | false |
tolerance | Tolerance for the point search. | Positive real. | 1e-6 |
mesh_file_name | If interpolation is enabled, the name of the field file that contains the mesh coordinates. | Strings ending with f***** | file_name |
fld files that were written in double precision. To check if your fld file was written in double precision, run the command: #std 4 ... indicates single precision, whereas #std 8 ... indicates double precision. Neko write single precision fld files by default. To write your files in double precision, set case.output_precision to "double"."interpolate" is set to true even if the field file matches with the current simulation.The blasius object is used to specify the Blasius profile that can be used for the initial and inflow condition. The boundary cannot be tilted with respect to the coordinate axes. It requires the following parameters:
delta, the thickness of the boundary layer.freestream_velocity, the velocity value in the free stream.approximation, the numerical approximation to the Blasius profile.linear, linear approximation.quadratic, quadratic approximation.cubic, cubic approximation.quartic, quartic approximation.sin, sine function approximation.The source_terms object should be used to specify the source terms in the momentum equation. The object is not mandatory, by default no forcing term is present. Each source term, is itself a JSON object, so source_terms is just an array of them. Note that with respect to the governing equations, the source terms define \( f^u \), meaning that the values are then multiplied by the density.
For each source, the type keyword defines the kind of forcing that will be introduced. Furthermore, the start_time and end_time keywords can be used to set a time frame for when the source term is active. Note, however, that these keywords have no effect on the user-defined source terms, but their execution can, of course, be directly controlled in the user code. By default, all source terms are active during the entire simulation.
The following types are currently implemented.
constant, constant forcing. Strength defined by the values array with 3 reals corresponding to the 3 components of the forcing.boussinesq, a source term introducing boyancy based on the Boussinesq approximation, \( \rho \beta (T - T_{ref}) \cdot \mathbf{g} \). Here, \( \rho \) is density, \( \beta \) the thermal expansion coefficient, \( \mathbf{g} \) the gravity vector, and \( T_{ref} \) a reference value of the scalar, typically temperature.
Reads the following entries:
scalar_field: The name of the scalar that drives the source term, defaults to "s".reference_value: The reference value of the scalar.g: The gravity vector.beta: The thermal expansion coefficient, defaults to the inverse of ref_value.coriolis, a source term introducing a Coriolis force, defined as \( -2 \Omega \times (u - U_g) \). Here, \( \Omega \) is the rotation vector and \( u \) is the velocity vector, and \( U_g \) is the geostrophic wind. Several ways of setting \( \Omega \) are provided via the following keywords.
rotation_vector: Array with 3 values. Directly assigns \( \Omega \) to the provided vector.omega and phi: Both scalars. The latitude phi should be provided in degrees. Sets \( \Omega = [0, \omega \cos \phi, \omega \sin \phi ] \). Common notation when modelling the atmosphere. This assumes that the \( z \) axis is normal to the ground.f: Scalar, referred to as the Coriolis parameter, \( f = 2 \omega \sin \phi \). Sets \( \Omega = [0, 0, 0.5f ] \). This assumes both that \( z \) axis is normal to the ground and that the ground-normal component of the Coriolis force is negligible.The geostrophic wind is set to 0 for all components by default. Other values are set via the geostrophic_wind keyword.
user_pointwise, the values are set inside the compiled user file, using the pointwise user file subroutine. Only works on CPUs!user_vector, the values are set inside the compiled user file, using the non-pointwise user file subroutine. Should be used when running on the GPU.brinkman, Brinkman permeability forcing inside a pre-defined region.The Brinkman source term introduces regions of resistance in the fluid domain. The volume force \( f_i \) applied in the selected regions are proportional to the fluid velocity component \( u_i \).
\begin{eqnarray*} f_i(x) &=& - B(x) u_i(x), \\ B(x) &=& \kappa_0 + (\kappa_1 - \kappa_0) \xi(x) \frac{q + 1}{q + \xi(x)}, \end{eqnarray*}
where, \( x \) is the current location in the domain, \( \xi: x \mapsto [0,1] \) represent an indicator function for the resistance where \( \xi(x) = 0 \) is a free flow. \( \kappa_i \) describes the limits for the force application at \( \xi(x)=0 \) and \( \xi(x)=1 \). A penalty parameter \( q \) help us to reduce numerical problems.
The indicator function will be defined based on the object type. The following types are currently implemented.
boundary_mesh, the indicator function for a boundary mesh is computed in two steps. First, the signed distance function is computed for the boundary mesh. Then, the indicator function is computed using the distance transform function specified in the case file.point_zone, the indicator function is defined as 1 inside the point zone and 0 outside.Each object are added to a common indicator field by means of a point-wise max operator. This means that the indicator field will be the union of all the regions defined by the objects.
To assist correct placement and scaling of objects from external sources, the meshes can be transformed using the mesh_transform object. The object can be used to apply a transformation to the boundary mesh. The following types are currently implemented.
none, no transformation is applied.bounding_box, the boundary mesh is transformed to fit inside a box defined by box_min and box_max. The box is defined by two vectors of 3 reals each. The keep_aspect_ratio keyword can be used to keep the aspect ratio of the boundary mesh.After the indicator field is computed, it is filtered using a filter type specified in the case file. The filter is used to smooth the indicator field before computing the Brinkman force. The following types are currently implemented.
none, no filtering is applied.The filtering can be defined for each object separately. Additionally, the filter can be specified for the entire source term, in which case it will be applied to the final indicator field, after all sources have been added.
Additional keywords are available to modify the Brinkman force term.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
brinkman.limits | Brinkman factor at free-flow ( \( \kappa_0 \)) and solid domain ( \( \kappa_1 \)). | Vector of 2 reals. | - |
brinkman.penalty | Penalty parameter \( q \) when estimating Brinkman factor. | Real | \( 1.0 \) |
objects | Array of JSON objects, defining the objects to be immersed. | Each object must specify a type | - |
distance_transform.type | How to map from distance field to indicator field. | step, smooth_step | - |
distance_transform.value | Values used to define the distance transform, such as cut-off distance for the step function. | Real | - |
filter.type | Type of filtering applied to the indicator field either globally or for the current object. | none | none |
mesh_transform.type | Apply a transformation to the boundary mesh. | bounding_box, none | none |
mesh_transform.box_min | Lower left front corner of the box to fit inside. | Vector of 3 reals | - |
mesh_transform.box_max | Upper right back corner of the box to fit inside. | Vector of 3 reals | - |
mesh_transform.keep_aspect_ratio | Keep the aspect ratio of the boundary mesh. | true or false | true |
Example of a Brinkman source term where a boundary mesh and a point zone are combined to define the resistance in the fluid domain. The indicator field for the boundary mesh is computed using a step function with a cut-off distance of \( 0.1 \). The indicator field for the point zone is not filtered.
The optional gradient_jump_penalty object can be used to perform gradient jump penalty as an continuous interior penalty option. The penalty term is performed on the weak form equation of quantity \( T \) (could either be velocity or scalar) as a right hand side term
\( - < \tau |u \cdot n| h^2_{\Omega ^e} G(T) \phi_{t1} \phi_{t2} \frac{\partial \phi_{n}}{\partial n}>\),
where \( <> \) refers to the integral over all facets of the element, \( \tau \) is the penalty parameter, \( |u \cdot n| \) is the absolute velocity flux over the facet, \( h^2_{\Omega ^e} \) is the mesh size, \( G(T) \) is the gradient jump over the facet, \( \phi_{t1} \phi_{t2} \) are the polynomial on the tangential direction of the facet, and finally \( \frac{\partial \phi_{n}}{\partial n} \) is the gradient of the normal polynomial on the facet.
Here in our Neko context where hexahedral mesh is adopted, \( h^2_{\Omega ^e} \) is measured by the average distance from the vertices of the facet to the facet on the opposite side. And the distance of a vertex to another facet is defined by the average distance from the vertex to the plane constituted by 3 vertices from the other facet.
The penalty parameter \( \tau \) could be expressed as the form \( \tau = a * (P + 1) ^ {-b}\), for \( P > 1 \) where \( P \) is the polynomial order while \( a \) and \( b \) are user-defined parameters. The configuration uses the following parameters:
enable, the boolean to turn on and off the gradient jump penalty option, default to be false.tau, the penalty parameter that can be only used for \( P = 1 \), default to be 0.02.scaling_factor, the scaling parameter \( a \) for \( P > 1 \), default to be 0.8.scaling_exponent, the scaling parameter \( b \) for \( P > 1 \), default to be 4.0.The mandatory velocity_solver and pressure_solver objects are used to configure the solvers for the momentum and pressure-Poisson equation. The following keywords are used, with the corresponding options.
type, solver type.cg, a conjugate gradient solver.pipecg, a pipelined conjugate gradient solver.bicgstab, a bi-conjugate gradient stabilized solver.cacg, a communication-avoiding conjugate gradient solver.cpldcg, a coupled conjugate gradient solver.gmres, a GMRES solver. Typically used for pressure.fusedcg, a conjugate gradient solver optimised for accelerators using kernel fusion.fcpldcg, a coupled conjugate gradient solver optimised for accelerators using kernel fusion.preconditioner, preconditioner type.jacobi, a Jacobi preconditioner. Typically used for velocity.hsmg, a hybrid-Schwarz multigrid preconditioner. Typically used for pressure.ident, an identity matrix (no preconditioner).absolute_tolerance, tolerance criterion for convergence.max_iterations, maximum number of iterations before giving up.projection_space_size, size of the vector space used for accelerating the solution procedure. If 0, then the projection space is not used. More important for the pressure equation.projection_hold_steps, steps for which the simulation does not use projection after starting or time step changes. E.g. if 5, then the projection space will start to update at the 6th time step and the space will be utilized at the 7th time step.monitor, monitoring of residuals. If set to true, the residuals will be printed for each iteration.The optional flow_rate_force object can be used to force a particular flow rate through the domain. Useful for channel and pipe flows. The configuration uses the following parameters:
direction, the direction of the flow, defined as 0, 1, or 2, corresponding to x, y or z, respectively.value, the desired flow rate.use_averaged_flow, whether value specifies the domain-averaged (bulk) velocity or the volume flow rate.All the parameters are summarized in the table below. This includes all the subobjects discussed above, as well as keyword parameters that can be described concisely directly in the table.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
scheme | The fluid solve type. | pnpn | - |
Re | The Reynolds number. | Positive real | - |
rho | The density of the fluid. | Positive real | - |
mu | The dynamic viscosity of the fluid. | Positive real | - |
output_control | Defines the interpretation of output_value to define the frequency of writing checkpoint files. | nsamples, simulationtime, tsteps, never | - |
output_value | The frequency of sampling in terms of output_control. | Positive real or integer | - |
inflow_condition.type | Velocity inflow condition type. | user, uniform, blasius | - |
inflow_condition.value | Value of the inflow velocity. | Vector of 3 reals | - |
initial_condition.type | Initial condition type. | user, uniform, blasius, field | - |
initial_condition.value | Value of the velocity initial condition. | Vector of 3 reals | - |
initial_condition.file_name | If "type" = "field", the path to the field file to read from. | String ending with .fld, .chkp, .nek5000 or f*****. | - |
initial_condition.sample_index | If "type" = "field", and file type is fld or nek5000, the index of the file to sampled. | Positive integer. | -1 |
initial_condition.previous_mesh | If "type" = "field", and file type is chkp, the previous mesh from which to interpolate. | String ending with .nmsh. | - |
initial_condition.tolerance | If "type" = "field", and file type is chkp, tolerance to use for mesh interpolation. | Positive real. | 1e-6 |
blasius.delta | Boundary layer thickness in the Blasius profile. | Positive real | - |
blasius.freestream_velocity | Free-stream velocity in the Blasius profile. | Vector of 3 reals | - |
blasius.approximation | Numerical approximation of the Blasius profile. | linear, quadratic, cubic, quartic, sin | - |
shear_stress.value | The shear stress vector value for sh boundaries | Vector of 3 reals | [0, 0, 0] |
wall_modelling.type | The wall model type for wm boundaries. See documentation for additional config parameters. | rough_log_law, spalding | - |
source_terms | Array of JSON objects, defining additional source terms. | See list of source terms above | - |
gradient_jump_penalty | Array of JSON objects, defining additional gradient jump penalty. | See list of gradient jump penalty above | - |
boundary_types | Boundary types/conditions labels. | Array of strings | - |
velocity_solver.type | Linear solver for the momentum equation. | cg, pipecg, bicgstab, cacg, gmres | - |
velocity_solver.preconditioner | Linear solver preconditioner for the momentum equation. | ident, hsmg, jacobi | - |
velocity_solver.absolute_tolerance | Linear solver convergence criterion for the momentum equation. | Positive real | - |
velocity_solver.maxiter | Linear solver max iteration count for the momentum equation. | Positive real | 800 |
velocity_solver.projection_space_size | Projection space size for the momentum equation. | Positive integer | 20 |
velocity_solver.projection_hold_steps | Holding steps of the projection for the momentum equation. | Positive integer | 5 |
velocity_solver.monitor | Monitor residuals in the linear solver for the momentum equation. | true or false | false |
pressure_solver.type | Linear solver for the pressure equation. | cg, pipecg, bicgstab, cacg, gmres | - |
pressure_solver.preconditioner | Linear solver preconditioner for the pressure equation. | ident, hsmg, jacobi | - |
pressure_solver.absolute_tolerance | Linear solver convergence criterion for the pressure equation. | Positive real | - |
pressure_solver.maxiter | Linear solver max iteration count for the pressure equation. | Positive real | 800 |
pressure_solver.projection_space_size | Projection space size for the pressure equation. | Positive integer | 20 |
pressure_solver.projection_hold_steps | Holding steps of the projection for the pressure equation. | Positive integer | 5 |
pressure_solver.monitor | Monitor residuals in the linear solver for the pressure equation. | true or false | false |
flow_rate_force.direction | Direction of the forced flow. | 0, 1, 2 | - |
flow_rate_force.value | Bulk velocity or volumetric flow rate. | Positive real | - |
flow_rate_force.use_averaged_flow | Whether bulk velocity or volumetric flow rate is given by the value parameter. | true or false | - |
freeze | Whether to fix the velocity field at initial conditions. | true or false | false |
advection | Whether to compute the advetion term. | true or false | true |
The scalar object allows to add a scalar transport equation to the solution. The solution variable is called s, but saved as temperature in the fld files. Some properties of the object are inherited from fluid: the properties of the linear solver, the value of the density, and the output control.
The scalar equation requires defining additional material properties: the specific heat capacity and thermal conductivity. These are provided as cp and lambda. Similarly to the fluid, one can provide the Peclet number, Pe, as an alternative. In this case, cp is set to 1 and lambda to the inverse of Pe.
As for the fluid, turbulence modelling is enabled by setting the nut_field to the name matching that set for the simulation component with the LES model. Additionally, the turbulent Prandtl number, Pr_t should be set. The eddy viscosity values will be divided by it to produce eddy diffusivity.
The boundary conditions for the scalar are specified through the boundary_types keyword.
The value of the keyword is an array of strings, with the following possible values:
d=x, sets a uniform Dirichlet boundary of value x (e.g. d=1 to set s to 1 on the boundary, see the Rayleigh-Benard example case).d_s, a Dirichlet boundary condition for more complex, non-uniform and/or time-dependent profiles. This boundary condition uses a more advanced user interface.The object initial_condition is used to provide initial conditions. It is mandatory. The means of prescribing the values are controlled via the type keyword:
user, the values are set inside the compiled user file as explained in the user defined initial condition section of the user file documentation.uniform, the value is a constant scalar, looked up under the value keyword.point_zone, the values are set to a constant base value, supplied under the base_value keyword, and then assigned a zone value inside a point zone. The point zone is specified by the name keyword, and should be defined in the case.point_zones object. See more about point zones point-zones.md.field, where the initial condition is retrieved from a field file. Works in the same way as for the fluid. See the fluid section for detailed explanations.The configuration of source terms is the same as for the fluid. A demonstration of using source terms for the scalar can be found in the scalar_mms example.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
enabled | Whether to enable the scalar computation. | true or false | true |
Pe | The Peclet number. | Positive real | - |
cp | Specific heat cpacity. | Positive real | - |
lambda | Thermal conductivity. | Positive real | - |
nut_field | Name of the turbulent kinematic viscosity field. | String | Empty string |
Pr_t | Turbulent Prandtl number | Positive real | - |
boundary_types | Boundary types/conditions labels. | Array of strings | - |
initial_condition.type | Initial condition type. | user, uniform, point_zone | - |
initial_condition.value | Value of the velocity initial condition. | Real | - |
source_terms | Array of JSON objects, defining additional source terms. | See list of source terms above | - |
gradient_jump_penalty | Array of JSON objects, defining additional gradient jump penalty. | See list of gradient jump penalty above | - |
advection | Whether to compute the advetion term. | true or false | true |
This object adds the collection of statistics for the fluid fields. For additional details on the workflow, see the corresponding page in the user manual.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
enabled | Whether to enable the statistics computation. | true or false | true |
start_time | Time at which to start gathering statistics. | Positive real | 0 |
sampling_interval | Interval, in timesteps, for sampling the flow fields for statistics. | Positive integer | 10 |
Simulation components enable the user to perform various additional operations, which are not strictly necessary to run the solver. An example could be computing and output of additional fields, e.g. vorticity.
A more detailed description as well as a full list of available components and their setup is provided in a separate page of the manual.
Point zones enable the user to select GLL points in the computational domain according to some geometric criterion. Two predefined geometric shapes are selectable from the case file, boxes and spheres.
A point zone object defined in the case file can be retrieved from the point zone registry, neko_point_zone_registry, and can be used to perform any zone-specific operations (e.g. localized source term, probing...). User-specific point zones can also be added manually to the point zone registry from the user file.
A more detailed description as well as a full list of available components and their setup is provided in a separate page of the manual.
This object adds the collection of runtime statistics (timings) for identified profiling regions. A region is defined as all functions between a call to profiler_start_region(name, id) and profiler_end_region(name, id). Neko currently supports 50 regions, with id 1..25 being reserved for internal use.
| Name | Description | Admissible values | Default value |
|---|---|---|---|
enabled | Whether to enable gathering of runtime statistics | true or false | false |
output_profile | Wheter to output all gathered profiling data as a CSV file | true or false | false |
1.9.1