The fan model is a lumped parameter model that can be used to determine the impact of a fan with known characteristics upon some larger flow field. The fan boundary type allows you to input an empirical fan curve that governs the relationship between head (pressure rise) and flow rate (velocity) across a fan element. You can also specify radial and tangential components of the fan swirl velocity. The fan model does not provide an accurate description of the detailed flow through the fan blades. Instead, it predicts the amount of flow through the fan. Fans may be used in conjunction with other flow sources, or as the sole source of flow in a simulation. In the latter case, the system flow rate is determined by the balance between losses in the system and the fan curve.
ANSYS Fluent also provides a connection for a special user-defined fan model that updates the pressure jump function during the calculation. This feature is described in User-Defined Fan Model.
A fan is considered to be infinitely thin, and the discontinuous pressure rise across it is specified as a function of the velocity through the fan. The relationship may be a constant, a polynomial, piecewise-linear, or piecewise-polynomial function, or a user-defined function.
In the case of a polynomial, the relationship is of the form
(6–123) |
where is the pressure jump,
are the pressure-jump
polynomial coefficients, and
is the magnitude of the local
fluid velocity normal to the fan.
Important: The velocity can be either positive or negative.
You must be careful to model the fan so that a pressure rise occurs
for forward flow through the fan.
You can, optionally, use the mass-averaged velocity normal to the fan to determine a single pressure-jump value for all faces in the fan zone.
For three-dimensional problems, the values of the convected tangential and radial velocity fields can be imposed on the fan surface to generate swirl. These velocities can be specified as functions of the radial distance from the fan center. The relationships may be constant or polynomial functions, or user-defined functions.
Important: You must use SI units for all fan swirl velocity inputs.
For the case of polynomial functions, the tangential and radial velocity components can be specified by the following equations:
(6–124) |
(6–125) |
where and
are, respectively,
the tangential and radial velocities on the fan surface in m/s,
and
are the tangential
and radial velocity polynomial coefficients, and
is the distance to the fan
center.
Once the fan zone has been identified (in the Boundary Conditions task page), you will set all modeling inputs for the fan in the Fan Dialog Box (Figure 6.55: The Fan Dialog Box), which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions).
Inputs for a fan are as follows:
Identify the fan zone.
Define the pressure jump across the fan.
Define the discrete phase boundary condition for the fan (for discrete phase calculations).
Define the swirl velocity, if desired (3D only).
Since the fan is considered to be infinitely thin, it must be modeled as the interface between cells, rather than a cell zone. Therefore the fan zone is a type of internal face zone (where the faces are line segments in 2D or triangles/quadrilaterals in 3D). If, when you read your mesh into ANSYS Fluent, the fan zone is identified as an interior zone, right-click the zone in the tree and use the Type sub-menu to change it to a fan zone (for more details, see Changing Cell and Boundary Zone Types).
Once the interior zone has been changed to a fan zone, you can open the Fan dialog box and specify the pressure jump and, optionally, the swirl velocity.
To define the pressure jump, you will specify a polynomial, piecewise-linear, or piecewise-polynomial function of velocity, a user-defined function, or a constant value. You should also check the Zone Average Direction vector to be sure that a pressure rise occurs for forward flow through the fan. The Zone Average Direction, calculated by the solver, is the face-averaged direction vector for the fan zone. If this vector is pointing in the direction you want the fan to blow, do not select Reverse Fan Direction; if it is pointing in the opposite direction, select Reverse Fan Direction.
Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the pressure jump:
Check that the Profile Specification of Pressure-Jump option is off in the Fan Dialog Box.
Choose polynomial, piecewise-linear, or piecewise-polynomial in the drop-down list to the right of Pressure-Jump. (If the function type you want is already selected, you can click the button to open the dialog box where you will define the function.)
In the dialog box that appears for the definition of the Pressure Jump function (for example, Figure 6.56: Polynomial Profile Dialog Box for Pressure Jump Definition), enter the appropriate values. These profile input dialog boxes are used the same way as the profile input dialog boxes for temperature-dependent properties. See Defining Properties Using Temperature-Dependent Functions to find out how to use them.
Set any of the optional parameters described below. (optional)
When you define the pressure jump using any of these types of functions, you can choose to limit the minimum and maximum velocity magnitudes used to calculate the pressure jump. Enabling the Limit Polynomial Velocity Range option limits the pressure jump when a Min Velocity Magnitude and a Max Velocity Magnitude are specified.
Important: The values corresponding to the Min Velocity Magnitude and the Max Velocity Magnitude do not limit the flow field velocity to this range. However, this range does limit the value of the pressure jump, which is a polynomial and a function of velocity, as seen in Equation 6–123. If the calculated normal velocity magnitude exceeds the Max Velocity Magnitude that has been specified, then the pressure jump at the Max Velocity Magnitude value will be used. Similarly, if the calculated velocity is less than the specified Min Velocity Magnitude, the pressure jump at the Min Velocity Magnitude will be substituted for the pressure jump corresponding to the calculated velocity.
You also have the option to use the mass-averaged velocity normal to the fan to determine a single pressure-jump value for all faces in the fan zone. Turning on Calculate Pressure-Jump from Average Conditions enables this option.
To define a constant pressure jump, follow these steps:
Turn off the Profile Specification of Pressure-Jump option in the Fan Dialog Box.
Choose constant in the drop-down list to the right of Pressure-Jump.
Enter the value for in the Pressure-Jump field.
You can follow the procedure below, if it is more convenient:
Turn on the Profile Specification of Pressure-Jump option.
Select constant in the drop-down
list below Pressure Jump Profile, and enter
the value for in the Pressure Jump
Profile field.
For a user-defined pressure-jump function or a function defined in a boundary profile file, you will follow these steps:
Turn on the Profile Specification of Pressure-Jump option.
Choose the appropriate function in the drop-down list below Pressure Jump Profile.
See the Fluent Customization Manual for information about user-defined functions, and Profiles for details about profile files.
This example shows you how to determine the function for the
pressure jump. Consider the simple two-dimensional duct flow illustrated
in Figure 6.57: A Fan Located In a 2D Duct. Air at constant density
enters the 2.0 m 0.4 m duct with a velocity of 15 m/s. Centered in the duct
is a fan.
Assume that the fan characteristics are as follows when the fan is operating at 2000 rpm:
| | |
| 25 | 0.0 |
| 20 | 175 |
| 15 | 350 |
| 10 | 525 |
| 5 | 700 |
| 0 | 875 |
where is the flow through the fan and
is the
pressure rise across the fan. The fan characteristics in this example
follow a simple linear relationship between pressure rise and flow
rate. To convert this into a relationship between pressure rise and
velocity, the cross-sectional area of the fan must be known. In this
example, assuming that the duct is 1.0 m deep, this area is 0.4 m2, so that the corresponding velocity values are as
follows:
| | |
| 62.5 | 0.0 |
| 50.0 | 175 |
| 37.5 | 350 |
| 25.0 | 525 |
| 12.5 | 700 |
| 0 | 875 |
The polynomial form of this relationship is the following equation for a line:
(6–126) |
If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the fan. See Setting Boundary Conditions for the Discrete Phase for details.
If you want to set tangential and radial velocity fields on the fan surface to generate swirl in a 3D problem, follow these steps:
Turn on the Swirl-Velocity Specification option in the Fan Dialog Box.
Specify the fan’s axis of rotation by defining the axis origin (Fan Origin) and direction vector (Fan Axis).
Set the value for the radius of the fan’s hub
(Fan Hub Radius). The default is to avoid division by zero in the polynomial.
Set the tangential and radial velocity functions as polynomial functions of radial distance, constant values, or user-defined functions.
Important: You must use SI units for all fan swirl velocity inputs.
To define a polynomial function for tangential or radial velocity, follow the steps below:
Check that the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option is off in the Fan Dialog Box.
Enter the coefficients in Equation 6–124 or
in Equation 6–125 in the Tangential- or Radial-Velocity
Polynomial Coefficients field. Enter
first, then
, and so on. Separate each coefficient by a blank
space. Remember that the first coefficient is for
.
To define a constant tangential or radial velocity, the steps are as follows:
Turn on the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option in the Fan Dialog Box.
Select constant in the drop-down list under Tangential or Radial Velocity Profile.
Enter the value for or
in the Tangential or Radial Velocity Profile field.
You can follow the procedure below, if it is more convenient:
Turn off the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option in the Fan Dialog Box.
Enter the value for or
in the Tangential- or Radial-Velocity Polynomial Coefficients field.
For a user-defined tangential or radial velocity function or a function contained in a profile file, follow the procedure below:
Turn on the Profile Specification of Tangential or Radial Velocity option.
Choose the appropriate function from the drop-down list under Tangential or Radial Velocity Profile.
See the Fluent Customization Manual for information about user-defined functions, and Profiles for details about profile files.
You can use the Surface Integrals Dialog Box to report the pressure rise through the fan, as described in Surface Integration. There are two steps to this procedure:
Create a surface on each side of the fan zone. Use the Transform Surface Dialog Box (as described in Transforming Surfaces) to translate the fan zone slightly upstream and slightly downstream to create two new surfaces.
In the Surface Integrals dialog box, report the average Static Pressure just upstream and just downstream of the fan. You can then calculate the pressure rise through the fan.
Graphical reports of interest with fans are as follows:
Contours or profiles of Static Pressure and Static Temperature.
XY plots of Static Pressure and Static Temperature vs position.
Displaying Graphics explains how to generate graphical displays of data.
Important: When generating these plots, be sure to turn off the display of node values so that you can see the different values on each side of the fan. (If you display node values, the cell values on either side of the fan will be averaged to obtain a node value, and you will not see, for example, the pressure jump across the fan.)