# Boundary conditions¶

You need a list of boundary conditions for your problem. For each region of the boundary you first need to tell Ocellaris how to find this region and then the boundary conditions to apply to each of the variables. You must specify BCs for the velocity for a single phase simulation and also for the pressure if you are using a non-algebraic pressure correction method such as IPCS. Coupled methods or algebraic pressure correction methods such as IPCS-A does not use boundary conditions for the pressure at the same location as you give boundary conditions for the velocity. You can of course use a outlet type boundary where the pressure is given but not the velocity. Refer to a textbook about solving the Navier-Stokes equations for details about what types of boundary conditions are reasonable to expect to work.

You can select constant Dirichlet boundary conditions (ConstantValue) or constant Neumann conditions (ConstantGradient). You can also have coded boundary conditions where you give a source code snippet that is executed to calculate the boundary condition value, either in Python (type CodedValue) or in C++ (type CppCodedValue).

How to mark different areas of the boundary is explained below. For the lid driven cavity the boundary conditions are as follows:

boundary_conditions:
-   name: walls
selector: code
inside_code: on_boundary
u:
type: ConstantValue
value: [0, 0]
p:         # <-- only used in non-algebraic pressure correction methods
value: 0
-   name: lid
selector: code
inside_code: on_boundary and x >= 1.0 - 1e-8
u:
type: ConstantValue
value: [1, 0]
p:         # <-- only used in non-algebraic pressure correction methods
value: 0


Note that the - in front of the name: ... lines marks the start of a list item. The boundary conditions should be given as a list of boundary regions. Each region specifies boundary conditions for all variables on the selected boundary.

The boundary conditions for the velocity components can also be broken up and written per component. This allows you to apply different boundary conditions types for each component. In this case it can be written (for the lid):

u0:
type: ConstantValue
value: 1
u1:
type: ConstantValue
value: 0

name

The name of the region. For more helpful error messages etc.

selector

How the region is selected. Supported methods are code and mesh_facet_region.

inside_code

Required when the selector is code: Python code to mark facets as inside the region or not

mesh_facet_regions

Required when the selector is mesh_facet_region: List of identificator numbers of the facet regions from the mesh. See below.

map_code

Required when using periodic boundary conditions: Code for mapping coordinates when using periodic boundary conditions. See below. Since periodic DG function spaces are currently not supported by FEniCS, the support for periodic boundary conditions may have bitrotted. It used to work for CG function spaces, but may not any more.

## Selecting regions by code¶

You can select regions of the boundary by code in the same format as in FEniCS. Ocellaris will run the Python code provided in the inside_code input key in a statement equivalent to:

def boundary(x, on_boundary):
return YOUR_REGION_CODE


if you give a single line expression, or

def boundary(x, on_boundary):
YOUR_REGION_CODE
return inside


if you give a multi line expression. In this case you need to assign a boolean value to the name inside.

How the inside_code works is that any facet where your code evaluates to True will be marked. As you can se above it is possible to mark everything as is done for the walls and then overwrite this mark for parts of the boundary as is done for the lid. The above will have walls everywhere below y=1 and lid on y≥1. The FEniCS / dolfin syntax is used so x is the x-component and x is the y-component.

## Selecting regions from mesh facet regions¶

If you load the mesh along with a facet region file you can select boundary regions by referencing their number given in the facet region file. You can select one or more mesh facet region per Ocellaris boundary region. In the demo calculating flow around the 2D outline of an Ocellaris clownfish the selection of the top and bottom wall is done as follows. Here 2 and 4 are the numbers given to the top and bottom wall respectively in the Gmsh preprocessor using Physical Line(3) =  {...}; Physical Line(5) =  {...};:

boundary_conditions:
-   name: Top and bottom
selector: mesh_facet_region
mesh_facet_regions: [3, 5]
u:
type: FreeSlip


## Common to all boundary conditions¶

The boundary condition for each variable is given in a sub-dictionary that has the following options:

type

What type of BC to apply. Currently the following are available:

• ConstantValue

• ConstantGradient

• CodedValue

• CppCodedValue

• FieldFunction

• FreeSlip

• OpenOutletBoundary, An open outlet zero stress boundary condition

• ConstantRobin

• SlipLength

• InterfaceSlipLength

enforce_zero_flux

For Neumann and Robin boundaries where the value is not prescribed, but you want to ensure that nothing of the variable you are describing flows through the wall. This can be useful when the mesh should be a plane normal to the direction you are describing, but the mesh is not a perfect plane, but has some innacurracies causing the normal to be slightly off

## BC type Constant¶

value

The value to apply when using ConstantXxxx. Either a scalar or a list of scalars.

## BC type Python coded¶

code

Python code to calculate the value

An example of coded boundary conditions can be seen in the the following which applies the Taylor-Green vortex solution as Dirichlet boundary conditions:

boundary_conditions:
-   name: walls
selector: code
inside_code: on_boundary
u:
type: CodedValue
code:
-   value = -sin(pi*x) * cos(pi*x) * exp(-2*pi*pi*nu*t)
-   value =  sin(pi*x) * cos(pi*x) * exp(-2*pi*pi*nu*t)


Notice that there is a list of two code blocks for the velocity. Both are evaluated as scalar fields and must assign to the zeroth component of the value[] array that is provided by FEniCS in order to set the Dirichlet value at the boundary.

Note: If you write the boundary conditions in C++ instead of Python it will normally be significantly faster.

## BC type C++ coded¶

cpp_code

C++ expression to calculate the value

An example of C++ boundary conditions can be seen in the the following which applies the Taylor-Green vortex solution as Dirichlet boundary conditions:

boundary_conditions:
-   name: walls
selector: code
inside_code: on_boundary
u:
type: CppCodedValue
cpp_code:
-   -sin(pi*x) * cos(pi*x) * exp(-2*pi*pi*nu*t)
-    sin(pi*x) * cos(pi*x) * exp(-2*pi*pi*nu*t)


Note that there is no assignment to the value[] array. All math functions from <cmath> are available as well as scalars like the time “t”, the timestep “dt”, time index “it” and number of geometrical dimensions “ndim”. For single phase simulations “nu” and “rho” are also available.

You can use C++ lambda expressions to write multi-line expressions:

# ...
cpp_code: |
// This is the same as 'x <= H ? 1.0 : 0.0'
[&]() {
bool is_above = x > H;
if (is_above) {
return 0.0;
} else {
return 1.0;
}
}()


## BC type known field function¶

Dirichlet BCs given by a known function

function

The name of a known field function

Example from a wave simulation

boundary_conditions:
-   name: Inlet
selector: code
inside_code: 'on_boundary and x < 1e-5'
u0:
type: FieldFunction
function: waves/uhoriz
u1:
type: ConstantValue
value: 0
u2:
type: FieldFunction
function: waves/uvert
c:
type: FieldFunction
function: waves/c


## BC type Constant Robin¶

Robin condition with constant values

d(VAR)/dn = 1/blend (dval - VAR) + nval

blend

A constant blending factor

dval

The Dirichlet value

nval

The Neumann value

## BC type Slip length¶

Wall slip length (Navier) boundary condition with constant value

value

The value to prescribe, default 0

slip_length

The slip length (the distance into the wall where the value is prescribed).

## BC type Interface slip length¶

Wall slip length (Navier) boundary condition where the slip length is multiplied by a slip factor ∈ [0, 1] that varies along the domain boundary depending on the distance to an interface (typically a free surface between two fluids).

value, slip_length

Same as above

slip_factor_function

The function the blends from 0 slip length to full slip length. Typically the name of a FreeSurfaceZone is given.