[Fluent Inc. Logo] return to home search
next up previous contents index

7.4.1 Inputs at Velocity Inlet Boundaries



Summary


You will enter the following information for a velocity inlet boundary:

All values are entered in the Velocity Inlet panel (Figure  7.4.1), which is opened from the Boundary Conditions panel (as described in Section  7.1.4).

Figure 7.4.1: The Velocity Inlet Panel
figure



Defining the Velocity


You can define the inflow velocity by specifying the velocity magnitude and direction, the velocity components, or the velocity magnitude normal to the boundary. If the cell zone adjacent to the velocity inlet is moving (i.e., if you are using a rotating reference frame, multiple reference frames, or sliding meshes), you can specify either relative or absolute velocities. For axisymmetric problems with swirl in FLUENT, you will also specify the swirl velocity.

The procedure for defining the inflow velocity is as follows:

1.   Choose which method you will use to specify the flow direction by selecting Magnitude and Direction, Components, or Magnitude, Normal to Boundary in the Velocity Specification Method drop-down list.

2.   If the cell zone adjacent to the velocity inlet is moving, you can choose to specify relative or absolute velocities by selecting Relative to Adjacent Cell Zone or Absolute in the Reference Frame drop-down list. If the adjacent cell zone is not moving, Absolute and Relative to Adjacent Cell Zone will be equivalent, so you need not visit the list.

3.   If you are going to set the velocity magnitude and direction or the velocity components, and your geometry is 3D, you will next choose the coordinate system in which you will define the vector or velocity components. Choose Cartesian (X, Y, Z), Cylindrical (Radial, Tangential, Axial), or Local Cylindrical (Radial, Tangential, Axial) in the Coordinate System drop-down list. See Section  7.3.1 for information about Cartesian, cylindrical, and local cylindrical coordinate systems.

4.   Set the appropriate velocity parameters, as described below for each specification method.

Setting the Velocity Magnitude and Direction

If you selected Magnitude and Direction as the Velocity Specification Method in step 1 above, you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity Magnitude) and the direction of the vector:

Figure  7.3.2 shows the vector components for these different coordinate systems.

Setting the Velocity Magnitude Normal to the Boundary

If you selected Magnitude, Normal to Boundary as the Velocity Specification Method in step 1 above, you will enter the magnitude of the velocity vector at the inflow boundary (the Velocity Magnitude). If you are modeling 2D axisymmetric swirl, you will also enter the Tangential-Component of Flow Direction.

Setting the Velocity Components

If you selected Components as the Velocity Specification Method in step 1 above, you will enter the components of the velocity vector at the inflow boundary as follows:

figure   

Remember that positive values for $x$, $y$, and $z$ velocities indicate flow in the positive $x$, $y$, and $z$ directions. If flow enters the domain in the negative $x$ direction, for example, you will need to specify a negative value for the $x$ velocity. The same holds true for the radial, tangential, and axial velocities. Positive radial velocities point radially out from the axis, positive axial velocities are in the direction of the axis vector, and positive tangential velocities are based on the right-hand rule using the positive axis.

Setting the Angular Velocity

If you chose Components as the Velocity Specification Method in step 1 above, and you are modeling axisymmetric swirl, you can specify the inlet Swirl Angular Velocity $\Omega$ in addition to the Swirl-Velocity. Similarly, if you chose Components as the Velocity Specification Method and you chose in step 3 to use a Cylindrical or Local Cylindrical coordinate system, you can specify the inlet Angular Velocity $\Omega$ in addition to the Tangential-Velocity.

If you specify $\Omega$, $v_\theta$ is computed for each cell as $\Omega r$, where $r$ is the radial coordinate in the coordinate system defined by the rotation axis and origin. If you specify both the Swirl-Velocity and the Swirl Angular Velocity, or the Tangential-Velocity and the Angular Velocity, FLUENT will add $v_\theta$ and $\Omega r$ to get the swirl or tangential velocity at each cell.



Defining the Temperature


For calculations in which the energy equation is being solved, you will set the static temperature of the flow at the velocity inlet boundary in the Temperature field.



Defining Outflow Gauge Pressure


If you are using one of the density-based solvers, you can specify an Outflow Gauge Pressure for a velocity inlet boundary. If the flow exits the domain at any face on the boundary, that face will be treated as a pressure outlet with the pressure prescribed in the Outflow Gauge Pressure field.



Defining Turbulence Parameters


For turbulent calculations, there are several ways in which you can define the turbulence parameters. Instructions for deciding which method to use and determining appropriate values for these inputs are provided in Section  7.2.2. Turbulence modeling in general is described in Chapter  12.



Defining Radiation Parameters


If 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) Black Body Temperature. See Section  13.3.15 for details. (The Rosseland radiation model does not require any boundary condition inputs.)



Defining Species Mass Fractions


If you are modeling species transport, you will set the species mass fractions under Species Mass Fractions. For details, see Section  14.1.5.



Defining Non-Premixed Combustion Parameters


If you are using the non-premixed or partially premixed combustion model, you will set the Mean Mixture Fraction and Mixture Fraction Variance (and the Secondary Mean Mixture Fraction and Secondary Mixture Fraction Variance, if you are using two mixture fractions), as described in Section  15.13.



Defining Premixed Combustion Boundary Conditions


If you are using the premixed or partially premixed combustion model, you will set the Progress Variable, as described in Section  16.3.5.



Defining Discrete Phase Boundary Conditions


If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the velocity inlet. See Section  22.13 for details.



Defining Multiphase Boundary Conditions


If you are using the VOF, mixture, or Eulerian model for multiphase flow, you will need to specify volume fractions for secondary phases and (for some models) additional parameters. See Section  23.9.8 for details.


next up previous contents index Previous: 7.4 Velocity Inlet Boundary
Up: 7.4 Velocity Inlet Boundary
Next: 7.4.2 Default Settings at
© Fluent Inc. 2006-09-20