Domain

In the domain section, the global definitions for the simulation are set, such as the number of dimensions and the numerical reference parameters.

Commands

domain
{
     ndim                              3
     min_domain                        "0.0 0.0 0.0"
     max_domain                        "1.0 3.0 0.0"
     BC_min                            "OUTLET PERIODIC SIMPLEOUTLET"
     BC_max                            "OUTLET PERIODIC SIMPLEOUTLET"

     outlet_vel                        "0.05 0.0 0.0" 
     outlet_bodyforce_on               true

     ref_rho                           1000.
     ref_length                        0.1
     ref_vel                           1.0
     ref_curv                          1.0
     ref_visc                          1.0

     bodyforce                         "0. 0. 0."
     t_damp_bodyforce_start            0.
     t_damp_bodyforce_end              0.
     bodyforcefile                     inputFileName.txt 
		
     inputfile                         initialparticlepositions.txt
     inputfileReadMode                 AUTO                         
     inputfile_factor                  0.001
}

Definitions

Command	Contents	SI Unit Example
`ndim`	The dimensionality of the problem. 1 Options 1 2 3
`min_domain`	Minimum bounds of the computational box (vector defining a point location). Note: If both `min_domain` and `max_domain` are not specified in the configuration file, the variables will be determined by the code automatically. 1
`max_domain`	Maximum bounds of the computational box (vector defining a point location). Note: If both `min_domain` and `max_domain` are not specified in the configuration file, the variables will be determined by the code automatically. 1
`BC_min`	Boundary condition at the minimum boundary. For an illustration of domain boundaries, refer to Comment 2. Options OPEN PERIODIC SIMPLEOUTLET (Default) - Deletes all particles that cross it. OUTLET - Differs from a SIMPLEOUTLET in the following ways: By default, it has an associated zero-gradient velocity condition. Outlet velocity can be specified (`outlet_vel`) and the influence of the gravitational force on the outgoing fluid (`outlet_bodyforce_on`) can be added. There can be multiple OUTLET boundaries specified in the domain. Related Commands `outlet_vel` `outlet_bodyforce_on`
`BC_max`	Boundary condition at the maximum boundary. For an illustration of domain boundaries, refer to Comment 2. Options OPEN PERIODIC SIMPLEOUTLET (Default) - Deletes all particles that cross it. OUTLET - Differs from a SIMPLEOUTLET in the following ways: By default, it has an associated zero-gradient velocity condition. Outlet velocity can be specified (`outlet_vel`) and the influence of the gravitational force on the outgoing fluid (`outlet_bodyforce_on`) can be added. There can be multiple OUTLET boundaries specified in the domain. Related Commands `outlet_vel` `outlet_bodyforce_on`
`outlet_vel`	Specifies the velocity of the OUTLET boundary. Note: If this command is not specified, the OUTLET option applies zero-gradient velocity at the boundary. If there are multiple outlets, all of them will use the same outlet velocity value.
`outlet_bodyforce_on`	If this flag is switched on, the outlet particles will experience the prescribed body force. This is useful in cases where the outlet plane is perpendicular to the body force (gravity) direction. In this case, the zero gradient velocity at the outlet no longer applies. Options false (Default) true
`ref_rho`	Reference density. This should be the lowest fluid density in the domain.

Reference values have been automated. They can be set manually, as is recommended. Depending on the case definition, the code will automatically pick up the reference values, provided that the max_dist command is defined in the motion definition.

For density, the lowest fluid density will be picked up as the reference. For length, the code will analyze the size of the domain in the direction of the body force applied and choose that length as the reference length. This means that if variable body force is being used, the reference length is specified manually.

For velocity, if there is defined motion in the configuration file, the code will automatically calculate maximal velocity of the motion, multiply it by a ref_vel_factor (the default value is 1.5) for conservative purposes, and set that value as the reference velocity. If there is no motion defined, or if the motion is rigid body or position file, the reference velocity must be defined manually. For reference curvature, the default curvature will be set as 1/(5*dx). In order to resolve droplets accurately, there needs to be a droplet radius of at least five particles.

ref_rho

Reference density

Should be the lowest fluid density in the domain.

Default: If not specified, the code will automatically detect it.

ref_length

Reference length: A typical length scale defining the relevant physics.

Examples:

Diameter in case of a channel flow
Fluid height (depth) for hydrostatic problems, for example gearboxes and tanks.

Default: The code will automatically try to find a relevant length for a hydrostatic problem.

It is recommended that you specify this reference value, as it can be difficult for the code to identify the correct value in certain cases.

ref_vel

Reference velocity

Should be highest expected velocity in the domain.

Default: If the motion is defined in the .cfg file, the code will automatically calculate the maximum velocity and multiply it by the ref_vel_factor value in order to assure stable running of the simulation.

ref_curv

Reference curvature (needed only if surften_model is set to ADAMI or SINGLE_PHASE).

Should be the curvature of the smallest droplet that needs to be resolved (1/radius of the droplet).

Default: If not specified, the value will be set to 1/(5*dx)

Related Options/Commands: surften_model

ref_visc

Reference viscosity (needed only if viscTempCoupling is set to true).

Should be the highest expected viscosity in the domain.

Related Options/Commands: viscTempCoupling, Viscosity-temperature dependence models

bodyforce

Gravitational acceleration

Body force vector must be specified (if using variable body force file, the latter bodyforcefile command will overwrite it).

t_damp_bodyforce_start

Before this time the body force is zero. Starting from this time, a gravitational acceleration is added to the system.

Note: Ramping up to the given value is defined with t_damp_bodyforce_start and t_damp_bodyforce_end commands.

Defaults: 0

t_damp_bodyforce_end

This time must not be smaller than t_damp_bodyforce_start. Within the time interval between t_damp_bodyforce_start and t_damp_bodyforce_end the gravitational acceleration is ramped up to reach the full body force at t_damp_bodyforce_end. At later times the full body force is applied.

Defaults: 0

bodyforcefile

Name of the file that contains the body force vector as a function of time, allowing simulations of sloshing tanks.

This is simultaneously a switch for the code. If you have this command present, it will use the specified input file and ignore the previous bodyforce input.

Related options/commands: Varying body force (acceleration)

inputfile

This file is the geometry input file (textfile) and needs to be present in the folder where the simulation is launched together with the config-file.

inputfile_factor

This factor can be used to scale the input file content.

Note: nanoFluidX uses SI-units. Therefore, this factor is useful if a model is created in SimLab in millimeter-units and needs to be converted to meters while reading in.

Example:

Model in mm → convert to meters: 0.001
Model in km → convert to meters: 1000

Default: 1.0

inputfileReadMode

Describes the data format that is to be read in.

Options:

INPTFL_AUTO: Reads all of the lines that are provided in the file.
INPTFL_PXYZ: Reads four columns: Phase ID, x, y and z coordinate
INPTFL_PXYZUVW: Reads seven columns: Phase ID, x, y and z coordinates and u, v and w components of the initial velocity

Default: INPTFL_AUTO

Comments

If both min_domain and max_domain are not specified in the configuration file, the code will automatically detect the minimum and maximum dimensions of the case and create a bounding box automatically. This is useful when operating with closed geometry, such as a gearbox. To simulate a sloshing/splashing case where the fluid is not constrained within solid walls, or if there are periodic or inlet boundary conditions associated with the domain, it is necessary to manually prescribe the size of the domain (bounding box). [ndim, min_domain, max_domain]
Each of the six bounding planes is marked in a separate color, with the colored arrow showing the surface normal of the boundary. The direction of these surface normals in the sketch has no influence on the code execution, they are provided to help visualize the domain. The two red dots at the opposite corners of the domain are minimum and maximum extent of the domain.

Figure 1. Sketch of nanoFluidX domain boundaries

[#reference_zg2_xms_k2b__domain_ref_r_varname_pdk_sms_p5b, #reference_zg2_xms_k2b__domain_ref_r_varname_wz4_sms_p5b]