Outflow boundary conditions in ANSYS FLUENT are used to model flow exits where the details of the flow velocity and pressure are not known prior to solving the flow problem. You do not define any conditions at outflow boundaries (unless you are modeling radiative heat transfer, a discrete phase of particles, or split mass flow): ANSYS FLUENT extrapolates the required information from the interior. It is important, however, to understand the limitations of this boundary type.
| Note that outflow boundaries cannot be used in the following cases:
For an overview of flow boundaries, see Section 7.3.1.
ANSYS FLUENT's Treatment at Outflow Boundaries
The boundary conditions used by ANSYS FLUENT at outflow boundaries are as follows:
The zero diffusion flux condition applied at outflow cells means that the conditions of the outflow plane are extrapolated from within the domain and have no impact on the upstream flow. The extrapolation procedure used by ANSYS FLUENT updates the outflow velocity and pressure in a manner that is consistent with a fully-developed flow assumption, as noted below, when there is no area change at the outflow boundary.
The zero diffusion flux condition applied by ANSYS FLUENT at outflow boundaries is approached physically in fully-developed flows. Fully-developed flows are flows in which the flow velocity profile (and/or profiles of other properties such as temperature) is unchanging in the flow direction.
It is important to note that gradients in the cross-stream direction may exist at an outflow boundary. Only the diffusion fluxes in the direction normal to the exit plane are assumed to be zero.
Using Outflow Boundaries
As noted in Section 7.3.11, the outflow boundary condition is obeyed in fully-developed flows where the diffusion flux for all flow variables in the exit direction are zero. However, you may also define outflow boundaries at physical boundaries where the flow is not fully developed--and you can do so with confidence if the assumption of a zero diffusion flux at the exit is expected to have a small impact on your flow solution. The appropriate placement of an outflow boundary is described by example below.
Figure 7.3.11 shows a second ill-posed outflow boundary at location A. Here, the outflow is located where flow is pulled into the ANSYS FLUENT domain through the outflow boundary. In situations like this the ANSYS FLUENT calculation typically does not converge and the results of the calculation have no validity. This is because when flow is pulled into the domain through an outflow, the mass flow rate through the domain is "floating'' or undefined. In addition, when flow enters the domain through an outflow boundary, the scalar properties of the flow are not defined. For example, the temperature of the flow pulled in through the outflow is not defined. ( ANSYS FLUENT chooses the temperature using the temperature of the fluid adjacent to the outflow, inside the domain.) Thus you should view all calculations that involve flow entering the domain through an outflow boundary with skepticism. For such calculations, pressure outlet boundary conditions (see Section 7.3.8) are recommended.
| Note that convergence may be affected if there is recirculation through the outflow boundary at any point during the calculation, even if the final solution is not expected to have any flow reentering the domain. This is particularly true of turbulent flow simulations.
Mass Flow Split Boundary Conditions
In ANSYS FLUENT, it is possible to use multiple outflow boundaries and specify the fractional flow rate through each boundary. In the Outflow dialog box, set the Flow Rate Weighting to indicate what portion of the outflow is through the boundary.
The Flow Rate Weighting is a weighting factor:
By default, the Flow Rate Weighting for all outflow boundaries is set to 1. If the flow is divided equally among all of your outflow boundaries (or if you have just one outflow boundary), you need not change the settings from the default; ANSYS FLUENT will scale the flow rate fractions to obtain equal fractions through all outflow boundaries. Thus, if you have two outflow boundaries and you want half of the flow to exit through each one, no inputs are required from you. If, however, you want 75% of the flow to exit through one, and 25% through the other, you will need to explicitly specify both Flow Rate Weightings, i.e., 0.75 for one boundary and 0.25 for the other.
| If you specify a
Flow Rate Weighting of 0.75 at the first exit and leave the default
Flow Rate Weighting (1.0) at the second exit, then the flow through each boundary will be
|Boundary 1||=||= 0.429 or 42.9%|
|Boundary 2||=||= 0.571 or 57.1%|
Other Inputs at Outflow Boundaries
Radiation Inputs at Outflow Boundaries
In general, there are no boundary conditions for you to set at an outflow boundary. If, however, you are using the P-1 radiation model, the DTRM, the DO model, or the surface-to-surface model, you will set the Internal Emissivity and (optionally) External Black Body Temperature Method in the Outflow dialog box. These parameters are described in Section 13.3.6. The default value for Internal Emissivity is 1 and the default value for Black Body Temperature is 300.
Defining Discrete Phase Boundary Conditions
If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the outflow boundary. See Section 23.4 for details.