Skip to content

Markers-and-BC.md

Latest commit

 

History

History
executable file
·
285 lines (198 loc) · 12.7 KB

Markers-and-BC.md

File metadata and controls

executable file
·
285 lines (198 loc) · 12.7 KB
title Markers and Boundary Conditions
permalink /docs_v7/Markers-and-BC/

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

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, ...)

The negative Sapalart-Allmaras model implements the same boundary conditions as for the standard/standalone version.

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 viscous 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).

Heat Transfer or Convection (no-slip) Wall

Solver Version
NAVIER_STOKES, RANS, INC_NAVIER_STOKES, INC_RANS 7.0.0

A wall with a prescribed locally variable heatflux via a heat transfer coefficient and and a Temperature at infinity (or reservoir Temperature) is defined with the MARKER_HEATTRANSFER option. The heatflux q computes to q = h(T_inf - T_wall), where T_wall is the local wall temperature and therefore no user input. The option format is the marker name followed by the value of the heat-transfer coefficient (in Watts per square meter and Kelvin [W/(m^2*K)],[J/(s*m^2*K)]) and the value of the Temperature at infinity (in Kelvin [K]), e.g.

MARKER_HEATTRANSFER = (Wall1, 10.0, 350.0, Wall2, 5.0, 330.0, ...)

Note: The Heat Transfer Wall degenerates to an adiabatic wall when the heat transfer coefficient is zero. On the other extreme (a very high heat transfer coefficient) the Heat Transfer Wall degenerates to an isothermal wall with Temperature at infinity being the wall temperature.

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. The implementation is based on the Riemann invariants of the Euler system calculated from the user input config file. 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. These are prescribed by computing the Riemann invariants.

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

For two given periodic surfaces periodic marker and donor marker SU2 defines periodicity by

MARKER_PERIODIC= ( periodic marker, donor marker, rotation_center_x, rotation_center_y, rotation_center_z, rotation_angle_x-axis, rotation_angle_y-axis, rotation_angle_z-axis, translation_x, translation_y, translation_z, ... )

The same number of points on both surfaces is assumed. Their orientation is specified by the additional set of parameters. Whereby rotation_center_ specifies the coordinates of the center of rotation for the specified axis, rotation_angle_ defines the rotation angle [in radians] between periodic marker and donor marker about the specified axis and translation_ specifies the translation in space between periodic marker and donor marker about the specified axis.

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]`)