Appendix: Boundary Conditions

Boundary conditions are specified by using boundary_conditions run control file variable, an example of which is shown below.

run control file boundary condition specification example

boundary_conditions:
<
Inlet=totalPressureInlet(p0=135.0 psi, T=164 R, k=0.05, omega=282.46, incompressible),
IPipe=noslip(adiabatic),
OPipe1=noslip(adiabatic),
OPipe2=noslip(adiabatic),
YPart=noslip(adiabatic),
Outlet1=fixedMassOutlet(mdot=-1027.8 lbm/s),
Outlet2=fixedMassOutlet(mdot=-1027.8 lbm/s)
>

The names of the boundaries specified on the left-hand sides of the declarations above must match those defined in the .vog file for the simulation. In the .vog file, each boundary name is identified with a set of boundary faces on the mesh which comprise the boundary. The corresponding boundary condition specified on the right-hand side of the boundary condition declaration is applied to all faces that comprise the boundary. During the grid generation process, it is important that all faces on the boundary of the domain be assigned to a boundary name. Should any faces not be included in a boundary name group, the code has no way of specifying the boundary conditions for those faces, and will terminate due to an insufficient problem specification. The types of boundary conditions supported in Stream are described in the following sections.

extrapolatedPressureOutlet

This outlet boundary condition is appropriate for compressible flow problems where the flow is supersonic at the outlet. An example of its usage is shown below:

Outlet=extrapolatedPressureOutlet

There are no options required by this boundary condition. Velocity, pressure, temperature, and turbulence quantities are all extrapolated from the center of the cell adjacent to the boundary face to the boundary face center. Density is then computed from the equation-of-state. Due to the use of zeroth-order extrapolation, it is prudent that outlet boundaries using this boundary condition be placed in a location where streamwise gradients are small, as well as to ensure that the grid is highly orthogonal, with the line from any boundary cell center to its respective boundary face center very closely aligned with the boundary normal vector.

fixedMassOutlet

This outlet boundary condition is appropriate for both incompressible and compressible flow problems. Two options are available. Using the mdot option, the total mass flow rate through the boundary can be specified directly, as shown below:

Outlet=fixedMassOutlet(mdot=-10.0 kg/s)

Alternately, using the massFlux option, the mass flow rate per unit area over the boundary can be specified, as follows:

Outlet=fixedMassOutlet(massFlux=-2.0 kg/m/m/s)

Internally, Stream operates using only mass fluxes for the boundary faces. When the boundary mass flow rate is specified using the mdot option, the equivalent massFlux is computed automatically by dividing the specified value by the total boundary area. By convention, a negative value indicates mass flow out of the domain. Positive values for this boundary condition should not be used. One may specify any units that are consistent with the units shown above, and conversion to SI units will be handled internally by the code. For incompressible flows, density, pressure, and turbulence quantities are extrapolated from the center of the cell adjacent to the boundary face to the boundary face center. For compressible flows, pressure, temperature, and turbulence quantities are extrapolated and then density is computed from the equation-of-state. The velocity on any boundary face is then computed directly from the mass flux and the local face density, and is assigned to be in the direction of the local face outward normal vector.

fixedPressureInlet

This inlet boundary condition is appropriate for both incompressible and compressible flow problems, and is designed to hold either a specified pressure or a specified mean pressure over the boundary. The velocity at the boundary faces is obtained via extrapolation from the adjacent cell centers in the interior of the domain. For incompressible simulations, one should specify the value of the pressure or the mean pressure. For compressible simulations, the temperature at the boundary must also be specified using any of the available scalar specification forms detailed here . If the simulation involves turbulent flow, one should also specify the turbulence intensity I, and the turbulent to laminar viscosity ratio muRatio. These two quantities may only be assigned as constant values. Profiles for I and muRatio are not currently available. Inlet values for the primitive turbulence variables variables k, omega, and epsilon are then computed based on the following equations:

\[k = -\frac{3}{2} (\vec{v} \cdot \vec{v}) I, \quad \omega = \frac{\rho k}{\mu_{\text{lam}} \cdot \mu_{\text{ratio}}}, \quad \epsilon = \frac{C_{\mu} \rho k^2}{\mu_{\text{lam}} \cdot \mu_{\text{ratio}}}\]

If the simulation contains multiple species, one should also assign the species mass fraction values using the mixture option. When using the mixture option, one need not list values for which the species mass fraction is zero, as this will be automatically handled by the code.

fixed pressure inlet, incompressible, turbulent

 Inlet=fixedPressureInlet(p=101325.0 Pa, I=0.03, muRatio=100.0)

fixed mean-pressure inlet, compressible, turbulent, multi-species

 Inlet=fixedPressureInlet(pMean=101325.0 Pa, T=300.0K, mixture=[H2=0.5, O2=0.5],
                          I=0.03, muRatio=100.0)

fixedPressureOutlet

This outlet boundary condition is appropriate for both incompressible simulations and compressible simulations where the flow always remains subsonic on the outlet boundary. There are two types of pressure constraints which may be employed for this boundary condition. Since there is no default value, one must explicitly specify either one of the constraints. With the first constraint, a constant pressure is specified and maintained on all boundary faces of the mesh comprising the boundary.

constant pressure

 Outlet=fixedPressureOutlet(p=202650 Pa)

With the second type of constraint, a mean pressure is specified and maintained on the boundary. This is implemented internally within the code by extrapolating the current pressure field from the cells next to the boundary to the boundary faces and then adding the same constant pressure correction value to all boundary faces to achieve the desired mean value.

mean pressure

 Outlet=fixedPressureOutlet(pMean=101320 Pa)

All other solver variables including velocity are extrapolated from the interior of the domain to the boundary. By default, this extrapolation will not allow flow to come into the domain through any face on the boundary. In certain instances, such as the case where one is using this boundary condition to approximate a far-field boundary of nearly constant pressure, one may wish to allow entrainment (flow coming into the domain from outside the domain) to occur.

entrainment

 Outlet=fixedPressureOutlet(p=202650 Pa, entrainment)

The entrainment option can be used with both the p= and pMean= options. In general, one will only want to use this option when there is relatively weak recirculation through the boundary. For internal flow problems, if one finds any recirculation zones in the vicinity of the outlet boundary, it is preferable to re-grid the domain in such a way (by including a part of a downstream component, for example) as to eliminate recirculation at the outlet, which otherwise could be a cause of numerical instability preventing the simulation from achieving convergence.

incompressibleInlet

This boundary condition is used only for incompressible flow simulations. For laminar flow simulations, one need only specify the velocity, either directly via the velocity value (using any the of methods detailed here) or indirectly via the mass flux or mass flow rate through the boundary. The usage of these three methods is shown below:

incompressible, laminar

 Inlet=incompressibleInlet(v=[1.0 m/s, 0.5 m/s, 0.1 m/s])
 Inlet=incompressibleInlet(massFlux=0.5 kg/m/m/s)
 Inlet=incompressibleInlet(mdot=2.7 kg/s)

For turbulent flow simulations, one must also specify the turbulence quantities at the inlet using the k= and omega= options using any of the methods for scalar values detailed here.

For compatibility with Chem, the option prescribed= is also allowed. With this option, one can specify a data file in which the velocity, pressure, temperature, and turbulence quantities are specified at several control points. Values are computed at the centers of the faces on the boundary via a generalized interpolation of the data specified at the control points. For the incompressibleInlet boundary condition, only the velocity and turbulence quantities (for turbulent simulations) are used from the data file, since this is the only required information for incompressible flow.

prescribed BC

 Inlet=incompressibleInlet(prescribed="bc.dat")

Any name may be specified for the boundary condition file. If one specifies no name between the quotes, the default file name bc.dat is used.

noslip

The noslip boundary condition should be used for all solid surfaces in viscous flow simulations. For compressible flow simulations, it is IMPORTANT to note that there is no default method that is automatically selected for heat-transfer at the boundary. Thus, one must explicitly assign either an adiabatic, specified temperature or specified heat flux conditions as an option. The following sections detail all the available options for the no-slip boundary condition.

Wall Functions

The default mode of operation is to compute wall viscous stresses and heat transfer using the standard gradient operations with information in the vicinity of the wall. This is the so-called gridding down to the wall approach, where wall functions are not employed by default. When using this mode, one should ensure that \(y^+ < 3`\) for accurate viscous stresses and heat fluxes. For incompressible flow, because the energy equation is not solved, if one is gridding down to the wall, there are no options required for the no-slip boundary and the boundary condition can be used in either of the following ways:

no-slip, incompressible

 Wall=noslip
 Wall=noslip()

Wall functions can be activated by using the wallFunction option.

wall function

 Wall=noslip(wallFunction)

The only wall function model currently available is that of [NiNe2003]. It is important to note that wall functions are enabled on a patch-by-patch basis. Only boundary patches with the wallFunction option will employ wall functions, while the remaining no-slip surfaces without the wallFunction option will employ the default approach of gridding down to the wall.

Adiabatic Wall

For solid surfaces with no heat flux through any part of the boundary, one should use the adiabatic option. If one is gridding down to the wall, one would specify the boundary condition as follows:

adiabatic wall

 Wall=noslip(adiabatic)

Wall functions can also be enabled for adiabatic boundaries, in which case one need only tack on the wallFunction option.

Specified Temperature at the Wall

For solid surfaces with a fixed temperature distribution, one should use the option T=, with any of the methods specified here to assign the temperature distribution. Wall functions may also be used for boundaries with specified temperature by tacking on the wallFunction option, in a manner like the following:

specified temperature

 Wall=noslip(T=500 K, wallFunction)

For compatibility with Chem, the option Twall= is also supported. This option can also be used to specify a constant scalar wall temperature value like the example above.

Specified Heat Flux at the Wall

For solid surfaces with a fixed heat flux (\(\frac{W}{m^{2}}\)) through the wall, one should use the option qwall= in the following manner (default units shown):

specified heat flux

 Wall=noslip(qwall=1024 W/m/m)

A single constant heat flux value is the only means of specification currently supported. Any units consistent with \(\frac{W}{m^{2}}\) may be used. By convention, the value specified is defined to be the heat flux from the fluid domain to the wall. Thus, one should specify a negative value to have positive heat transfer from the wall to the fluid. At the current time, wall functions cannot be used with the specified heat flux condition, so one must use this option only when gridding down to the wall.

Specified Wall and Reservoir Conditions

If one wants to approximate the condition in which a wall of known effective thermal resistance separates the fluid domain from a reservoir held at constant temperature, one can specify the wall and reservoir conditions in the following manner (default units shown):

specified wall and reservoir conditions

 Wall=noslip(Treservoir=400 K, Rwall=10.0 m*m*K/W)

At the current time, only constant value specifications for both Treservoir and Rwall are supported. With the supplied reservoir temperature and wall effective thermal resistance, the code will perform a 1-D wall heat-transfer balance to compute the wall temperature that balances the flux leaving the fluid domain with that entering the reservoir. At the current time, wall functions cannot be used with this specification, so one must use this option only when gridding down to the wall.

slip

The slip boundary condition should be used for all solid surfaces in inviscid flow simulations. All flow variables are extrapolated to the boundary from the cell values in the interior of the domain. There are no options required for this boundary condition.

slip

 Wall=slip

subsonicInlet

This boundary condition is only used for compressible flow simulations. For numerical stability purposes, the flow should remain subsonic on the boundary during the entire simulation. Pressure on the boundary is obtained by extrapolation from the interior of the domain. Density on the boundary is computed from the equation of state once the temperature at the boundary is known. The velocity on the boundary may be specified either directly via the velocity value (using any the of methods detailed here) or indirectly via the mass flux or mass flow rate through the boundary. The usage of these three methods is shown below:

compressible, subsonic

 Inlet=subsonicInlet(v=[0.5 m/s, 0.1 m/s, 1.0 m/s])
 Inlet=subsonicInlet(massFlux=0.5 kg/m/m/s)
 Inlet=subsonicInlet(mdot=2.7 kg/s)

Note that unlike for incompressibleInlet, the explicit specification of the boundary velocity via the v= option does not result in a fixed-mass inlet because the density at the boundary will evolve during the simulation. The temperature on the boundary must also be specified with the T= option using any the of methods detailed here for scalar specification. For turbulent flow simulations, one must also specify the turbulence quantities at the inlet with the k= and omega= options, again using any of the methods detailed here for scalar specification. If the simulation contains multiple species, one should also assign the species mass fraction values using the mixture= option. When using the mixture= option, one need not list values for which the species mass fraction is zero, as this will be automatically handled by the code.

compressible, turbulent, multi-species, subsonic

 Inlet=subsonicInlet(mdot=2.7 kg/s, T=400 K, k=0.05 m*m/s/s, omega=500.0 1/s,
                     mixture=[H2=0.5, O2=0.5])

For compatibility with Chem, the option prescribed= is allowed. With this option, one can specify a data file in which the velocity, pressure, temperature, mixture species mass fractions and turbulence quantities are specified at several control points. Values are computed at the centers of the faces on the boundary via a generalized interpolation of the data specified at the control points. For the subsonicInlet boundary condition, the only quantity not used from the data file is the pressure because pressure is extrapolated from the interior of the domain.

prescribed BC

 Inlet=subsonicInlet(prescribed="bc.dat")

Any name may be specified for the boundary condition file. If one specifies no name between the quotes, the default file name bc.dat is used.

supersonicInlet

This boundary condition is only used for compressible flow simulations. For numerical stability purposes, the flow should remain supersonic on the boundary during the entire simulation. The velocity on the boundary may be specified either directly via the velocity value (using any the of methods detailed here) or indirectly via the mass flux or mass flow rate through the boundary. The usage of these three methods is shown below:

compressible, supersonic

 Inlet=supersonicInlet(v=[0.5 m/s, 0.1 m/s, 1.0 m/s])
 Inlet=supersonicInlet(massFlux=0.5 kg/m/m/s)
 Inlet=supersonicInlet(mdot=2.7 kg/s)

The temperature and pressure on the boundary must also be specified with the T= and p= options, respectively. Temperature may be specified using any the of methods detailed here for scalar specification, however, at the current time only a single constant value may be specified for pressure. For turbulent flow simulations, one must also specify the turbulence quantities with the k= and omega= options, again using any of the methods detailed here for scalar specification. If the simulation contains multiple species, one should also assign the species mass fraction values using the mixture= option. When using the mixture= option, one need not list values for which the species mass fraction is zero, as this will be automatically handled by the code.

compressible, turbulent, multi-species, supersonic

 Inlet=supersonicInlet(mdot=2.7 kg/s, p=202650 Pa, T=400 K, k=0.05 m*m/s/s,
                     omega=500.0 1/s, mixture=[H2=0.5, O2=0.5])

For compatibility with Chem, the option prescribed= is also allowed. With this option, one can specify a data file in which the velocity, pressure, temperature, mixture species mass fractions and turbulence quantities are specified at several control points. Values are computed at the centers of the faces on the boundary via a generalized interpolation of the data specified at the control points. For the supersonicInlet boundary condition, all entries from the data file are used since no information is extrapolated from the interior to the boundary for supersonic flow. The prescribed= option is used in a manner shown below:

prescribed BC

 Inlet=supersonicInlet(prescribed="bc.dat")

Any name may be specified for the boundary condition file. If one specifies no name between the quotes, the default file name bc.dat is used.

Symmetry

This boundary condition is used where one desires to enforce a zero normal gradient condition at the boundary. This includes symmetry boundaries in 3-D simulations where the flow is symmetric about the boundary. For 2-D simulations, flow variables are only a function of two of the coordinate directions. Grid boundaries with normal vectors parallel to the third coordinate direction should be assigned as symmetry so the flow solution will not vary in this third direction. As there are no options required for this boundary condition, it is generally used as follows:

symmetry

 Boundary=symmetry

totalPressureInlet

This boundary condition can be used for both incompressible and compressible flow and is designed to hold a single fixed value of total pressure at each of the faces on the boundary. The total pressure value is specified using the p0= option. Temperature can be specified either directly with the T= option or indirectly with a total temperature via the T0= option. If temperature is specified, any of the methods detailed here for scalar specification may be used. If total temperature is specified, one may only use a single constant value. For turbulent flow simulations, one must also specify the turbulence quantities with the k= and omega= options, again using any of the methods detailed here for scalar specification. If the simulation contains multiple species, one should also assign the species mass fraction values using the mixture= option. When using the mixture= option, one need not list values for which the species mass fraction is zero, as this will be automatically handled by the code.

compressible, turbulent, multi-species

 Inlet=totalPressureInlet(p0=202650 Pa, T0=400 K, k=0.05 m*m/s/s, omega=500.0 1/s,
                      mixture=[H2=0.5, O2=0.5])

For compressible flows with real fluids, one must also use the option incompressible. This is currently required since the implementation of the total pressure inlet for compressible flow is based on equations which assume an ideal-gas equation of state. Use of the incompressible option instructs the code to revert to the incompressible form of the total pressure relations, which is a suitable approximation for low Mach number inlet flows.

compressible, turbulent, multi-species, real-fluid

 Inlet=totalPressureInlet(p0=202650 Pa, T0=400 K, k=0.05 m*m/s/s, omega=500.0 1/s,
                         mixture=[H2=0.5, O2=0.5], incompressible)

If the simulation involves an incompressible flow, then one should not include the incompressible option, as the incompressible form of the total pressure relation is automatically invoked by the code.

References

[NiNe2003]

1. Nichols and C. C. Nelson, “Application of hybrid rans/les turbulence models,” in Technical Report, 2003.