# Markers and Boundary Conditions

The term *Marker* refers to a named entity in your mesh file. Boundary conditions are defined by assigning names of the markers to the corresponding option. Below you will find a list of the most common boundary conditions along with a short description.

- Euler (Slip) Wall
- Symmetry Wall
- Constant Heatflux (no-slip) Wall
- Isothermal (no-slip) Wall
- Farfield Boundary Condition
- Inlet Boundary Condition
- Outlet Boundary Condition
- Structural Boundary Conditions

## Euler (Slip) Wall

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

An Euler wall for inviscid flow is defined with the `MARKER_EULER`

option. It can also be used as a slip wall in viscous flow. Only the marker name has to be given for this option.

For all Finite Volume (FVM) solvers, i.e. not the `FEM_*`

solvers, its implementation is identical to `MARKER_SYM`

solvers and both options can be used interchangeably.

```
MARKER_EULER = (Euler_Wall1, Euler_Wall2, ...)
```

**Note**: Be aware when switching from an Euler solver to a Navier-Stokes one that most solid walls should become `MARKER_HEATFLUX`

(and vice versa).

## Symmetry Wall

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

A symmetry wall is defined with using the `MARKER_SYM`

option. Only the marker name has to be given for this option.

For all Finite Volume (FVM) solvers, i.e. not the `FEM_*`

solvers, its implementation is identical to `MARKER_SYM`

solvers and both options can be used interchangeably.

```
MARKER_SYM = (Symmetry_Wall1, Symmetry_Wall2, ...)
```

## Constant Heatflux (no-slip) Wall

Solver | Version |
---|---|

`NAVIER_STOKES` , `RANS` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_NAVIER_STOKES` , `HEAT_EQUATION_FVM` |
7.0.0 |

A wall with a prescribed constant heatflux is defined with the `MARKER_HEATFLUX`

option. The option format is the marker name followed by the value of the heatflux (in Watts per square meter `[W/m^2],[J/(s*m^2)]`

), e.g.

```
MARKER_HEATFLUX = (Wall1, 1e05, Wall2, 0.0)
```

**Note**: Typically Navier-Stokes and RANS simulations are setup with adiabatic walls (heatflux = 0).

## Isothermal (no-slip) Wall

Solver | Version |
---|---|

`NAVIER_STOKES` , `RANS` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_NAVIER_STOKES` , `HEAT_EQUATION_FVM` |
7.0.0 |

A wall with a constant temperature is defined with the `MARKER_ISOTHERMAL`

option. The option format is the marker name followed by the value of the temperature (in Kelvin `[K]`

), e.g.

```
MARKER_ISOTHERMAL = (Wall1, 300.0, Wall2, 250.0)
```

## Farfield Boundary Condition

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

A marker can be defined as a Farfield boundary by addings its name to the `MARKER_FAR`

option. No other values are necesseary for that option. The actual values which will be prescribed depend on the solver and other user input settings. More details can be found in the Physical Definition section.

```
MARKER_FAR= (farfield)
```

## Inlet Boundary Condition

Inlet boundary conditions are set using the option `MARKER_INLET`

.

### Total Conditions

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

To describe the **Total Conditions** at the inlet, set the option `INLET_TYPE= TOTAL_CONDITIONS`

(which is the default). The format for `MARKER_INLET`

then is the marker name, followed by the Total Temperature (in Kelvin `[K]`

), the total Pressure (in Pascal `[Pa]`

) and the flow direction unity vector (in meter per second `[m/s]`

). For example:

```
INLET_TYPE= TOTAL_CONDITIONS
MARKER_INLET = (inlet1, 300, 1e6, 1.0, 0.0, 0.0, inlet2, 400, 1e6, 0.0, 1.0, 0.0)
```

### Mass Flow Inlet

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

To describe the **Mass Flow** at the inlet, set the option `INLET_TYPE= MASS_FLOW`

. The format for `MARKER_INLET`

then is the marker name, followed by the Density (in `[kg/m^3`

]), the Velocity magnitude (in meter per second `[m/s]`

) and the flow direction unity vector (in meter per second `[m/s]`

). For example:

```
INLET_TYPE= MASS_FLOW
MARKER_INLET = (inlet1, 1.13 , 20, 1.0, 0.0, 0.0, inlet2, 1.15, 10, 0.0, 1.0, 0.0)
```

**Note**: It is not possible to combine Mass Flow Inlet BCs and Total Condition Inlet BCs yet.

### Velocity Inlet

Solver | Version |
---|---|

`INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` |
7.0.0 |

To describe the **Velocity** at the inlet, set the option `INC_INLET_TYPE= VELOCITY_INLET`

. The format for `MARKER_INLET`

then is the marker name, followed by the Temperature (in Kelvin `[K`

]), the Velocity magnitude (in meter per second `[m/s]`

) and the flow direction unity vector (in meter per second `[m/s]`

).

```
INC_INLET_TYPE= VELOCITY_INLET, VELOCITY_INLET
MARKER_INLET = (inlet1, 300 , 20, 1.0, 0.0, 0.0, inlet2, 200, 10, 0.0, 1.0, 0.0)
```

### Pressure Inlet

Solver | Version |
---|---|

`INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` |
7.0.0 |

To describe the **Total Pressure** at the inlet, set the option `INC_INLET_TYPE= PRESSURE_INLET`

. The format for `MARKER_INLET`

then is the marker name, followed by the Temperature (in Kelvin `[K]`

), the Total Pressure (in Pascal `[Pa]`

) and the flow direction unity vector (in meter per second `[m/s]`

).

```
INC_INLET_TYPE= PRESSURE_INLET, PRESSURE_INLET
MARKER_INLET = (inlet1, 300 , 1e6, 1.0, 0.0, 0.0, inlet2, 200, 1e6, 0.0, 1.0, 0.0)
```

**Note 1**: It is possible to combine Velocity Inlet BCs and Pressure Inlet BCs.

**Note 2**: Updates to the velocity based on the prescribed pressure are damped in order to help with stability/convergence. The damping coefficient can be changed using the `INC_INLET_DAMPING`

option (default is `0.1`

).

## Outlet Boundary Condition

Outlet boundary conditions are set using the `MARKER_OUTLET`

option.

### Pressure Outlet (Compressible)

Solver | Version |
---|---|

`EULER` , `NAVIER_STOKES` , `RANS` , `FEM_EULER` , `FEM_NAVIER_STOKES` |
7.0.0 |

To describe the static thermodynamic pressure at an outlet, the format for `MARKER_OUTLET`

is the marker name, followed by the value of the static pressure (in Pascal `[Pa]`

).

```
MARKER_OUTLET = (outlet, 1e5)
```

### Pressure Outlet (Incompressible)

Solver | Version |
---|---|

`INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` |
7.0.0 |

To describe the pressure at an outlet, set the option `INC_OUTLET_TYPE= PRESSURE_OUTLET`

. The format for `MARKER_OUTLET`

is the marker name, followed by the value of the gauge pressure (in Pascal `[Pa]`

).

```
INC_OUTLET_TYPE= PRESSURE_OUTLET
MARKER_OUTLET = (outlet, 1e1)
```

**Note**: Gauge pressure is zero-referenced against ambient air pressure, so it is equal to absolute pressure minus atmospheric pressure.

### Mass Flow Outlet

Solver | Version |
---|---|

`INC_EULER` , `INC_NAVIER_STOKES` , `INC_RANS` |
7.0.0 |

To describe the mass flow at an outlet, set the option `INC_OUTLET_TYPE= MASS_FLOW_OUTLET`

. The format for `MARKER_OUTLET`

is the marker name, followed by the value of the target mass flow (in kilogramm per second `[kg/s]`

).

```
INC_OUTLET_TYPE= MASS_FLOW_OUTLET
MARKER_OUTLET = (outlet, 1e1)
```

**Note**: Updates to the pressure based on the prescribed mass flow are damped in order to help with stability/convergence. The damping coefficient can be changed using the `INC_OUTLET_DAMPING`

option (default is `0.1`

).

### Periodic Boundary Condition

Solver | Version |
---|---|

`NAVIER_STOKES` , `RANS` , `INC_NAVIER_STOKES` , `INC_RANS` , `FEM_NAVIER_STOKES` |
7.0.0 |

## Structural Boundary Conditions

### Clamped Boundary

Solver | Version |
---|---|

`ELASTICITY` |
7.0.0 |

The format for this boundary condition consists of a list of all clamped surfaces (markers). Structural displacements are set to 0 for the nodes on those surfaces.

```
MARKER_CLAMPED = (surface_1,...,surface_N)
```

**Note**: A well posed structural problem requires at least one surface as `MARKER_CLAMPED`

or `MARKER_DISPLACEMENT`

.

### Displacement Boundary

Solver | Version |
---|---|

`ELASTICITY` |
7.0.0 |

The displacements of the nodes on `surface`

are enforced, the displacement vector is specified by magnitude and direction (the x/y/z components), internally the solver makes the direction unitary, the multiplier (should usually be set to 1) can be used to increase/decrease the magnitude for example after scaling an existing mesh.

```
MARKER_DISPLACEMENT = (surface, multiplier, magnitude `[m]`, x component, y component, z component)
```

**Note**: Be aware of intersecting surfaces with incompatible displacements, there are shared nodes between adjacent surfaces.

### Load Boundary

Solver | Version |
---|---|

`ELASTICITY` |
7.0.0 |

A force-like boundary condition but specified in terms of pressure (units of Pa) which is integrated to obtain nodal forces. The syntax is identical to `MARKER_DISPLACEMENT`

.

```
MARKER_LOAD = (surface, multiplier, magnitude `[Pa]`, x component, y component, z component)
```

**Note**: In the context of nonlinear elasticity, this is not a following force.

### Normal Pressure Boundary

Solver | Version |
---|---|

`ELASTICITY` |
7.0.0 |

Normal pressure boundary condition (positive means into the surface). This is a following force both magnitude and direction depend of the deformation of the structure.

```
MARKER_PRESSURE = (surface, inward pressure `[Pa]`)
```