Setting Up Outflow Boundaries

You specify outflow conditions on boundaries where the fluid leaves the simulation domain.

NoteFor solution stability and accuracy, you are advised to use outlet boundaries far downstream of strong recirculation areas, where it is reasonable to expect outflow everywhere on the boundary.
For each outflow boundary:
  1. Select the Regions > [region] > Boundaries > [boundary] node and set Type to one of the following:
    • Pressure Outlet—set this boundary type when you know the working pressure at the boundary. The boundary pressure can be considered as the static pressure of the environment into which the fluid enters. In normal outflow conditions, the boundary face values of all other variables, such as velocity, are extrapolated from the interior of the solution domain. If recirculation, that is, backflow occurs through the pressure boundary, various methods are available to control the backflow direction and pressure.
    • Outlet—this boundary type represents an outflow condition where no backflow occurs. You set the outlet boundary at locations where the flow is directed outwards only and where the flow profile is fully developed. The outflow conditions are not prescribed, but they are determined by the flow upstream of the outlet boundary. To determine the mass flow at the outlet boundary, you can either set the fraction of the total outflow leaving at the boundary or you can explicitly set the mass flow rate or the corrected mass flow rate. You can place more than one outlet boundary in your computational domain. However, you can not mix the split ratio option with mass flow rate or corrected mass flow rate outlet boundaries in one simulation. Except for the corrected mass flow rate option used with the coupled solver, the outlet boundary is not valid for transonic, supersonic, or hypersonic flows.

    For more information, see the specific topics in the Theory Guide under Boundary Conditions.

    When you combine different boundary types in your simulation, be aware of the following limitations:

    • Do not use the outlet boundary with specified split ratio in combination with a pressure outlet or a stagnation inlet boundary condition. Otherwise, the flow is indeterminate.
    • Combine an outlet boundary with specified mass flux with at least one other pressure-type boundary such as pressure outlet or stagnation inlet.
    • For a pressure outlet boundary combined with an outlet boundary with specified mass flux, in cases where the pressure outlet acts as an inlet, be careful when specifying the pressure condition. In the event of reversed flow, the dynamic head is taken out of the specified pressure, which can cause an incorrect pressure profile at the pressure outlet.
  2. Expand the [boundary] node and, depending on the selected boundary type, follow the appropriate steps:
    Boundary Type Steps
    Pressure Outlet
    1. Select the Physics Values node and set Pressure to the working pressure at the boundary.

      You can use a field function or a table to describe a dependence on space, iteration, or time step.

    2. If you want to set up a turbomachinery simulation, select the Physics Values > Pressure node and select Radial Equilibrium.

      The radial equilibrium pressure boundary condition is suitable for strong rotational flows where the centrifugal forces due to rotation are balanced by the radial pressure gradient force. The Radial Equilibrium method is compatible with all pressure outlet options except Average Pressure.

    3. Set the method by which Simcenter STAR-CCM+ computes the direction of any backflow that enters the simulation through the outflow boundary:
      1. Select the Physics Conditions > Backflow Specification node.
      2. Set Direction to one of the following options:
        1. Boundary-Normal—with this option, the inflow direction is normal to each boundary face.
        2. Extrapolated—select this option to extrapolate the inflow direction from the interior of the domain. In most situations, this is less stable than the Boundary Normal option. However, it is recommended for situations where the flow is known to be parallel to the pressure boundary, such as a co-flowing jet.
        3. Components—select this option to specify the inflow direction as individual angle components using the Physcs Values > Flow Direction node.
        4. Angles—select this option to set the inflow direction angles directly using the Physcs Values > Flow Angles node.
      3. By default, Simcenter STAR-CCM+ subtracts the dynamic head at the pressure outlet boundary in the case of inflow. If you do not want to use the dynamic head but maintain the pressure at the specified pressure value, set Pressure to Static.
    4. For compressible and non-isothermal flows, to prevent spurious numerical reflection of the solution into the solution domain:
      1. Select the Physics Conditions > Pressure Outlet Option node and set Option to Non-Reflecting or Unsteady Non-Reflecting for steady or unsteady simulations, respectively. Note that these options are only available when you use the Coupled Flow model.
      2. Select the Physics Values > Non-Reflection Mode Specification and set the Number of modes to retain. Specify a number of modes that is less than the number of cells in the circumferential direction.

    For more information, see Flow Boundaries Reference—Pressure Outlet.
    Outlet Depending on the available flow data at the outlet or the objective of the simulation, do one of the following:
    • If you know the fraction of the total outflow leaving at the boundary:
      1. Select the Physics Conditions > Mass Flow Specification node and set Mass Flow Specification to Split Ratio.
      2. Select the Physics Values > Split Ratio node and set a value from 0 to 1.

        When there are multiple outlet boundaries on one continuum, the fractions of the mass flow passing through each of the boundaries must sum up to 1.

    • If you know the mass flow at the boundary:
      1. Select the Physics Conditions > Mass Flow Specification node and set Mass Flow Specification to Mass Flow Rate.
      2. Select the Physics Values > Mass Flow Rate node and set the total corrected mass per unit time (kg/s) for the whole boundary.

        You can use a field function or a table to describe a dependence on iteration or time step, but the mass flow rate or the corrected mass flow rate cannot vary spatially across the boundary. The total mass flow is distributed over the faces of the boundary as described in Mass Flow Inlet in the Theory Guide.

    • For turbomachinery applications, if you want to simulate the full compressor speedline from choke to surge or, if you know the corrected mass flow that is delivered from a compressor to a gas turbine engine:
      1. Select an energy model in the physics continuum.
      2. Select the Physics Conditions > Mass Flow Specification node and set Mass Flow Specification to Corrected Mass Flow Rate.
      3. Select the Physics Values > Corrected Mass Flow Rate node and set the total corrected mass per unit time (kg/s) for the whole boundary.

        You can use a field function or a table to describe a dependence on iteration or time step, but the corrected mass flow rate cannot vary spatially across the boundary. The total corrected mass flow is distributed over the faces of the boundary as described in Mass Flow Inlet in the Theory Guide.

    For more information, see Flow Boundaries Reference—Outlet.