7.3.18 Fan Boundary Conditions

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 which 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 Section  7.5.

You can find the following information about modeling fans in this section:

Fan Equations

Modeling the Pressure Rise Across the Fan

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

where $\Delta p$ is the pressure jump, $f_n$ are the pressure-jump polynomial coefficients, and $v$ is the magnitude of the local fluid velocity normal to the fan.

The velocity $v$ 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.

Modeling the Fan Swirl Velocity

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.

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:

where $U_\theta$ and $U_r$ are, respectively, the tangential and radial velocities on the fan surface in m/s, $f_n$ and $g_n$ are the tangential and radial velocity polynomial coefficients, and $r$ is the distance to the fan center.

User Inputs for Fans

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  7.3.31), which is opened from the Boundary Conditions task page (as described in Section  7.1.4).

Figure 7.3.31: The Fan Dialog Box

Inputs for a fan are as follows:

1.   Identify the fan zone.

2.   Define the pressure jump across the fan.

3.   Define the discrete phase boundary condition for the fan (for discrete phase calculations).

4.   Define the swirl velocity, if desired (3D only).

Identifying the Fan Zone

Since the fan is considered to be infinitely thin, it must be modeled as the interface between cells, rather than a cell zone. Thus 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, use the Boundary Conditions task page (as described in Section  7.1.3) to change the appropriate interior zone to a fan zone.

Boundary Conditions

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.

Defining the Pressure Jump

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.

Polynomial, Piecewise-Linear, or Piecewise-Polynomial Function

Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the pressure jump:

1.   Check that the Profile Specification of Pressure-Jump option is off in the Fan dialog box.

2.   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 Edit... button to open the dialog box where you will define the function.)

3.   In the dialog box that appears for the definition of the Pressure Jump function (e.g., Figure  7.3.32), 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 Section  8.2 to find out how to use them.

Figure 7.3.32: Polynomial Profile Dialog Box for Pressure Jump Definition

4.   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.

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  7.3-55. 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.

Constant Value

To define a constant pressure jump, follow these steps:

1.   Turn off the Profile Specification of Pressure-Jump option in the Fan dialog box.

2.   Choose constant in the drop-down list to the right of Pressure-Jump.

3.   Enter the value for $\Delta p$ in the Pressure-Jump field.

You can follow the procedure below, if it is more convenient:

1.   Turn on the Profile Specification of Pressure-Jump option.

2.   Select constant in the drop-down list below Pressure Jump Profile, and enter the value for $\Delta p$ in the Pressure Jump Profile field.

User-Defined Function or Profile

For a user-defined pressure-jump function or a function defined in a boundary profile file, you will follow these steps:

1.   Turn on the Profile Specification of Pressure-Jump option.

2.   Choose the appropriate function in the drop-down list below Pressure Jump Profile.

See the separate UDF Manual for information about user-defined functions, and Section  7.6 for details about profile files.

Example: Determining the Pressure Jump Function

This example shows you how to determine the function for the pressure jump. Consider the simple two-dimensional duct flow illustrated in Figure  7.3.33. Air at constant density enters the 2.0 m $\times$ 0.4 m duct with a velocity of 15 m/s. Centered in the duct is a fan.

Figure 7.3.33: A Fan Located In a 2D Duct

Assume that the fan characteristics are as follows when the fan is operating at 2000 rpm:

$Q$ (m $^3$/s)	$\Delta p$ (Pa)
25	0.0
20	175
15	350
10	525
5	700
0	875

where $Q$ is the flow through the fan and $\Delta p$ 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 m $^2$, so that the corresponding velocity values are as follows:

$v$ (m/s)	$\Delta p$ (Pa)
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:

Defining Discrete Phase Boundary Conditions for the Fan

If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the fan. See Section  23.4 for details.

Defining the Fan Swirl Velocity

If you want to set tangential and radial velocity fields on the fan surface to generate swirl in a 3D problem, follow these steps:

1.   Turn on the Swirl-Velocity Specification option in the Fan dialog box.

2.   Specify the fan's axis of rotation by defining the axis origin ( Fan Origin) and direction vector ( Fan Axis).

3.   Set the value for the radius of the fan's hub ( Fan Hub Radius). The default is $1 \times 10^{-6}$ to avoid division by zero in the polynomial.

4.   Set the tangential and radial velocity functions as polynomial functions of radial distance, constant values, or user-defined functions.

You must use SI units for all fan swirl velocity inputs.

Polynomial Function

To define a polynomial function for tangential or radial velocity, follow the steps below:

1.   Check that the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option is off in the Fan dialog box.

2.   Enter the coefficients $f_n$ in Equation  7.3-56 or $g_n$ in Equation  7.3-57 in the Tangential- or Radial-Velocity Polynomial Coefficients field. Enter $f_{-1}$ first, then $f_0$, etc. Separate each coefficient by a blank space. Remember that the first coefficient is for $\frac{1}{r}$.

Constant Value

To define a constant tangential or radial velocity, the steps are as follows:

1.   Turn on the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option in the Fan dialog box.

2.   Select constant in the drop-down list under Tangential or Radial Velocity Profile.

3.   Enter the value for $U_\theta$ or $U_r$ in the Tangential or Radial Velocity Profile field.

You can follow the procedure below, if it is more convenient:

1.   Turn off the Profile Specification of Tangential Velocity or Profile Specification of Radial Velocity option in the Fan dialog box.

2.   Enter the value for $U_\theta$ or $U_r$ in the Tangential- or Radial-Velocity Polynomial Coefficients field.

User-Defined Function or Profile

For a user-defined tangential or radial velocity function or a function contained in a profile file, follow the procedure below:

1.   Turn on the Profile Specification of Tangential or Radial Velocity option.

2.   Choose the appropriate function from the drop-down list under Tangential or Radial Velocity Profile.

See the separate UDF Manual for information about user-defined functions, and Section  7.6 for details about profile files.

Postprocessing for Fans

Reporting the Pressure Rise Through the Fan

You can use the Surface Integrals dialog box to report the pressure rise through the fan, as described in Section  30.6. There are two steps to this procedure:

1.   Create a surface on each side of the fan zone. Use the Transform Surface dialog box (as described in Section  28.10) to translate the fan zone slightly upstream and slightly downstream to create two new surfaces.

2.   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 Plots

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.

Chapter  29 explains how to generate graphical displays of data.

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.)