Wall
Wall boundary conditions determine how the flow moves along the surface of a solid body.
In the properties panel you can choose whether the Momentum is:
No-slip: This will mean that the flow is stationary along the wall surface. In this case the mesh spacing at the wall must be fine enough to resolve the boundary layer there (i.e., the y+ value must be approximately 1).
Slip: This means the will be treated as being frictionless, allowing the flow to move alongside it at the surface.
Wall Model: This means that a wall function will be used to calculate the wall shear stress.
To define moving walls you can assign the surfaces to a moving frame, see how to define motion.
Energy Equation
In cases where you will be solving the energy equation, such as compressible flow using the ideal gas law, you will also see a dropdown box for Wall Energy with options:
Fixed Heat Flux: Enter a fixed heat flux to calculate the wall temperature.
Fixed Temperature: where a fixed wall temperature is specified and the heat flux is then calculated.
Wall Roughness
In cases where you're working with rough surfaces, you can set the Roughness Height, or equivalent sand grain roughness, in meters. The default value of 0 indicates that any surfaces assigned to the boundary condition are smooth.
Inlet
Inlet boundary conditions allow you to specify incoming flow across a surface, like the opening to an engine or pipe. The parameters you see in the properties panel will vary depending on your simulation settings.
Flow Direction: Choose between Normal to Boundary or Vector, the latter requiring a vector in Cartesian coordinates.
Momentum:
For compressible flows, choose between Total Pressure or Mass Flow.
For incompressible flows, there are additional options:
Velocity Magnitude and Velocity Components, the latter requiring a vector in Cartesian coordinates.
Fan Curve requires you to upload a fan curve CSV file, then specify a value for Total Pressure and Head Loss Coefficient. Your fan curve file must be in CSV format and contain columns for Volume Flow Rate (m3/s) and Pressure Rise (Pa), in that order.
Energy: Currently the only option for this is to specify a Total Temperature.
If you are running turbulent flow simulations (RANS or DES), you will also need to set the Turbulence Specification at the inlet:
For the Spalart-Allmaras model, choose between Turbulent Viscosity Ratio, Turbulent Viscosity, or Prescribed Value.
For the SST model, you must choose between Turbulent Viscosity Ratio and Intensity, Turbulent Viscosity Intensity, or Prescribed Value and then set the model’s two required values at the inlet.
Outlet
Outlet boundary conditions allow you to specify outflow conditions. This is useful for modeling things like the exit nozzle from an engine or water flowing out of a valve.
In the properties panel, choose an Outlet Strategy:
Outlet Pressure requires you to specify:
Pressure Constraint Mode: Choose Local if you'd like the pressure distribution on the outlet to be uniform with a fixed value everywhere (this is the default setting). Choose Average if you'd like the average pressure over the outlet surfaces to be equal to the imposed value. With this option, the distribution is not fixed and can develop naturally.
Static Pressure: Provide a value for static pressure at the outlet. Note this value is specified as relative to the Reference Pressure defined in the Material section of the control panel, and the absolute pressure is the sum of the two.
Target Mass Flow Rate requires you to specify a value for Static Pressure in addition to a value for Outlet Target Mass Flow Rate.
Fan Curve requires you to upload a fan curve CSV file, then specify a value for Static Pressure and Head Loss Coefficient. Your fan curve file must be in CSV format and contain the following columns, in this order:
Volume Flow Rate (m3/s)
Pressure Rise (Pa)
In cases where reverse flow at an outlet is expected, a total pressure and total temperature inlet with a flow direction normal to the boundary is used. This improves stability by discouraging the reverse flow condition because the static pressure is lower than in regions with normal outflow.
Properties like total temperature, turbulence variables, etc. in the reverse flow region are automatically set as the average over the entire outlet. This is based on the assumption that the flow out of the domain mixes fully before re-entering. This strategy is only valid if a majority of the flow at the outlet is moving outwards.
Symmetry
There are no required inputs for symmetry boundaries other than the assigned surfaces. A symmetry boundary ensures that there are no fluxes across the boundary and that all components of flow vectors that are normal to the surface are zero at the surface (the flow is symmetrical on either side).
Far-Field
Far-field boundaries are intended for modeling the outside domains of external flow problems where flow properties such as direction and temperature are known. Unlike inlets, the flow can enter or exit the entire domain through a far-field boundary. A simulation can only have one far-field boundary defined.
In the properties panel, first specify the Static Pressure. Note this value is specified as relative to the Reference Pressure defined in the Material section of the control panel, and the absolute pressure is the sum of the two.
For compressible flow simulations you will also need to set Mach Number and Temperature. For incompressible flow you instead must specify the Velocity Magnitude.
You can define the Far-field Flow Direction Specification using the dropdown menu as either a Direction Vector, adding the components below, or using Far-field Flow Angles, setting the Angle of Attack and Angle of Sideslip. Note that these angles are relative to the body orientation defined in the Body Frame.
If you are running turbulent flow simulations (RANS or DES), you will also need to set the Turbulence Specification at the far field:
For the Spalart-Allmaras model, the dropdown box here will allow you to choose between Turbulent Viscosity Ratio, Turbulent Viscosity, or Prescribed Value, and then you must specify the value below.
For the SST model, you must choose from Turbulent Viscosity Ratio and Intensity, Turbulent Viscosity Intensity, or Prescribed Values, and then set the model’s two required values at the far field.
Interface
Interfaces define the boundaries between two or more volumes in a simulation and connect surfaces that are otherwise disconnected. Interface boundaries allow you to solve across multiple, distinct volumes while treating the union of those volumes as a unified whole. This allows for more advanced physics like Frames & Motion or multiphysics. You can create interfaces between moving and stationary parts, fluid and solid volumes, or two solid volumes.
You can use Automatic Contact Detection to quickly define interfaces in your project.
In the properties panel you must first specify the Method:
Automatic: Fluxes from Side A are directly interpolated onto faces of Side B.
For transient cases, this is called a sliding Interface because the vertices on one side of the interface are moving relative to those on the other side. At each time step, the fluxes are directly transported across the interface.
For steady state cases, the moving parts are kept stationary and assigned different rotational or translational speeds. The flow in each moving volume is solved using a moving reference frame, but the geometry remains fixed in space. This is referred to as the Frozen Rotor technique.
Mixing Plane: A Mixing Plane interface is an interface where solution data is averaged over the azimuthal direction before state information is exchanged across the interface. This is often used for steady state cases to more accurately depict the steady state behavior of the rotating components.
Interfaces may consist of a patchwork of many surfaces from several volumes, so you must specify the side of the interface that a surface belongs to by adding surfaces to Side A and Side B in the properties panel. Click in the box to enter selection mode, then select the desired surfaces from the Geometry panel.
Note: If you have multiple disconnected interfaces in your model, an interface needs to be defined for each one.
Overset
The overset boundary condition allows you to simulate multiple moving objects without the need to deform your mesh. It can also be used in cases with complicated geometry where several parts are meshed independently and overlapping in some areas.
The overset boundary condition will identify which cells in the overlapping regions need to be calculated, inactive, or interpolated, and removes the inactive and interpolated cells from the final solution.
To set up an overset case you will need to upload an overset mesh, or upload a CAD file with overlapping far field boundaries and generate a mesh. After that, specify the surfaces that are overlapping in an Overset boundary condition. Typically this is the outer boundary of the mesh.
Important: Overset meshes must be merged into a single mesh file before uploading to Luminary Cloud.
Note: Whenever possible, make sure that the mesh resolution for each overlapping part is similar. If resolution at the interface is drastically different for each overlapping part, this can impact convergence.
Limitations
This feature is only available for use in compressible flow cases.
Your geometry must already have a far field added before it is imported to use this feature.
Surface to surface mesh overlap is not currently supported.
Periodic Pair
The use of periodic pairs allows you to model flow through a larger domain while running a simulation only on a smaller piece of that domain. This is possible when there is inherent symmetry or periodicity in the domain. Such cases can be either linearly or rotationally periodic.
An example of a rotationally periodic geometry is a six-bladed axial fan with equally spaced blades. In this case, a 60º segment of the fan including a single blade could be used to model the entire fan.
Periodic pairs must have the same shape and mesh topology while being linearly or rotationally displaced from each other. Luminary Cloud couples the corresponding mesh faces on each of the periodic pairs so that they have exactly the same values of the flow variables.
To create a periodic pair:
Click the + symbol next to the Boundary Conditions section.
Select Periodic Pair.
For linearly periodic cases, you must define the vector between the two surfaces in Cartesian coordinates in the Translation input. For rotationally periodic cases, you must define the Origin around which the boundaries are rotated from each other and the Rotation Angles in radians between them, again in Cartesian coordinates.
Click in the Side A box to select surfaces that will be paired. Repeat this step for Side B.
Isothermal
Assign a Fixed Temperature, measured in K, to be applied to the assigned surfaces.
Heat Flux
This boundary condition defines heat flux at wall boundary surfaces in W/m2. If you enter a negative value, temperatures will increase near the boundary condition. Enter a positive value, and temperatures will decrease. Enter 0 for an adiabatic wall.
Integrated Heat Flux
This boundary condition defines total heat flux at wall boundary surfaces in Watts. If you enter a negative value, temperatures will increase. Enter a positive value, and temperatures will decrease. Enter 0 for an adiabatic wall.
Convective Heat Transfer
This boundary condition allows you to model convective heat exchange with an external fluid following Newton's law of cooling. You’ll need to specify:
Heat Transfer Coefficient: Used to compute boundary heat transfer, measured in W/K/m2.
Fixed Temperature: Temperature of the external fluid as specified in Newton's Law of cooling, measured in K.
Tabulated Profiles in Boundary Conditions
For simulations that require a boundary condition to be spatially varying (changes across space) or temporal (changes across time), you can upload a tabulated profile in CSV format and select that data as input for certain parameters.
Make sure your file is formatted as follows:
Spatially Varying | We currently support 1D profiles for Inlet boundary conditions.
|
Temporal | We currently support providing profiles for Heat Flux, Integrated Heat Flux, and Inlet boundary conditions.
|
Select the boundary condition in the control panel.
In the properties panel, toggle the Tabulated Profile option on.
Click Upload File and select your CSV from the file browser.
Click Save.
Select a Profile Type. This specifies the type of 1D spatial variation, either Cartesian or radial, defined in the reference frame associated with the surfaces assigned to the boundary condition. For temporal cases, this will be Time.
For parameters that support tabulated profiles (see complete list below), hover over the input box to select a column from your uploaded CSV.
Set any remaining parameters for your boundary condition.
The following parameters support tabulated profiles as input:
Inlets:
Momentum: Total Pressure and Velocity Magnitude (constant density simulations only).
Temperature: Total Temperature
Turbulence Specification - Spalart Allmaras: Prescribed Value
Turbulence Specification - k-w: Prescribed Value
Heat Flux:
Fixed Heat Flux (W/m2)
Integrated Heat Flux:
Fixed Integrated Heat Flux (W)