7.3.19 Radiator Boundary Conditions

A lumped-parameter model for a heat exchange element (for example, a radiator or condenser), is available in ANSYS FLUENT. The radiator boundary type allows you to specify both the pressure drop and heat transfer coefficient as functions of the velocity normal to the radiator.

A more detailed heat exchanger model is also available in ANSYS FLUENT. See Section  14 for details.

Radiator Equations

Modeling the Pressure Loss Through a Radiator

A radiator is considered to be infinitely thin, and the pressure drop through the radiator is assumed to be proportional to the dynamic head of the fluid, with an empirically determined loss coefficient which you supply. That is, the pressure drop, $\Delta p$, varies with the normal component of velocity through the radiator, $v$, as follows:

where $\rho$ is the fluid density, and $k_L$ is the non-dimensional loss coefficient, which can be specified as a constant or as a polynomial, piecewise-linear, or piecewise-polynomial function.

In the case of a polynomial, the relationship is of the form

where $r_n$ are polynomial coefficients and $v$ is the magnitude of the local fluid velocity normal to the radiator.

Modeling the Heat Transfer Through a Radiator

The heat flux from the radiator to the surrounding fluid is given as

where $q$ is the heat flux, $T_{{\rm air},d}$ is the temperature downstream of the heat exchanger (radiator), and $T_{\rm ext}$ is the reference temperature for the liquid. The convective heat transfer coefficient, $h$, can be specified as a constant or as a polynomial, piecewise-linear, or piecewise-polynomial function.

For a polynomial, the relationship is of the form

where $h_n$ are polynomial coefficients and $v$ is the magnitude of the local fluid velocity normal to the radiator in m/s.

Either the actual heat flux $(q)$ or the heat transfer coefficient and radiator temperature $(h, T_{\rm ext})$ may be specified. $q$ (either the entered value or the value calculated using Equation  7.3-61) is integrated over the radiator surface area.

Calculating the Heat Transfer Coefficient

To model the thermal behavior of the radiator, you must supply an expression for the heat transfer coefficient, $h$, as a function of the fluid velocity through the radiator, $v$. To obtain this expression, consider the heat balance equation:

where

$q$	=	heat flux (W/m $^2$)
$\dot{m}$	=	fluid mass flow rate (kg/s)
$c_p$	=	specific heat capacity of fluid (J/kg-K)
$h$	=	empirical heat transfer coefficient (W/m $^2$-K)
$T_{\rm ext}$	=	external temperature (reference temperature for the liquid) (K)
$T_{{\rm air}, d}$	=	temperature downstream from the heat exchanger (K)
$A$	=	heat exchanger frontal area (m $^2$)

Equation  7.3-63 can be rewritten as

where $T_{{\rm air},u}$ is the upstream air temperature. The heat transfer coefficient, $h$, can therefore be computed as

or, in terms of the fluid velocity,

User Inputs for Radiators

Once the radiator zone has been identified (in the Boundary Conditions task page), you will set all modeling inputs for the radiator in the Radiator dialog box (Figure  7.3.34), which is opened from the Boundary Conditions task page (as described in Section  7.1.4).

Figure 7.3.34: The Radiator Dialog Box

The inputs for a radiator are as follows:

1.   Identify the radiator zone.

2.   Define the pressure loss coefficient.

3.   Define either the heat flux or the heat transfer coefficient and radiator temperature.

4.   Define the discrete phase boundary condition for the radiator (for discrete phase calculations).

Identifying the Radiator Zone

Since the radiator is considered to be infinitely thin, it must be modeled as the interface between cells, rather than a cell zone. Thus the radiator 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 radiator 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 radiator zone.

Boundary Conditions

Once the interior zone has been changed to a radiator zone, you can open the Radiator dialog box and specify the loss coefficient and heat flux information.

Defining the Pressure Loss Coefficient Function

To define the pressure loss coefficient $k_L$ you can specify a polynomial, piecewise-linear, or piecewise-polynomial function of velocity, or a constant value.

Polynomial, Piecewise-Linear, or Piecewise-Polynomial Function

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

1.   Choose polynomial, piecewise-linear, or piecewise-polynomial in the drop-down list to the right of Loss Coefficient. (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.)

2.   In the dialog box that appears for the definition of the Loss Coefficient function (e.g., Figure  7.3.35), 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 7.3.35: Polynomial Profile Dialog Box for Loss Coefficient Definition

Constant Value

To define a constant loss coefficient, follow these steps:

1.   Choose constant in the Loss Coefficient drop-down list.

2.   Enter the value for $k_L$ in the Loss Coefficient field.

Example: Calculating the Loss Coefficient

This example shows you how to determine the loss coefficient function. Consider the simple two-dimensional duct flow of air through a water-cooled radiator, shown in Figure  7.3.36.

Figure 7.3.36: A Simple Duct with a Radiator

The radiator characteristics must be known empirically. For this case, assume that the radiator to be modeled yields the test data shown in Table  7.3.1, which was taken with a waterside flow rate of 7 kg/min and an inlet water temperature of 400.0 K. To compute the loss coefficient, it is helpful to construct a table with values of the dynamic head, $\frac{1}{2}\rho v^2$, as a function of pressure drop, $\Delta p$, and the ratio of these two values, $k_L$ (from Equation  7.3-59). (The air density, defined in Figure  7.3.36, is 1.0 kg/m $^3$.) The reduced data are shown in Table  7.3.2.

Table 7.3.1: Airside Radiator Data

Velocity (m/s)	Upstream Temp (K)	Downstream Temp (K)	Pressure Drop (Pa)
5.0	300.0	330.0	75.0
10.0	300.0	322.5	250.0
15.0	300.0	320.0	450.0

Table 7.3.2: Reduced Radiator Data

v (m/s)	$\frac{1}{2}\rho v^2$ (Pa)	$\Delta p$ (Pa)	$k_L$
5.0	12.5	75.0	6.0
10.0	50.0	250.0	5.0
15.0	112.5	450.0	4.0

The loss coefficient is a linear function of the velocity, decreasing as the velocity increases. The form of this relationship is

where $v$ is now the absolute value of the velocity through the radiator.

Defining the Heat Flux Parameters

As mentioned in Section  7.3.19, you can either define the actual heat flux $(q)$ in the Heat Flux field, or set the heat transfer coefficient and radiator temperature $(h, T_{\rm ext})$. All inputs are in the Radiator dialog box.

To define the actual heat flux, specify a Temperature of 0, and set the constant Heat Flux value.

To define the radiator temperature, enter the value for $T_{\rm ext}$ in the Temperature field. To define the heat transfer coefficient, you can specify a polynomial, piecewise-linear, or piecewise-polynomial function of velocity, or a constant value.

Polynomial, Piecewise-Linear, or Piecewise-Polynomial Function

Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the heat transfer coefficient:

1.   Choose polynomial, piecewise-linear, or piecewise-polynomial in the drop-down list to the right of Heat-Transfer-Coefficient. (If the function type you want is already selected, you can click on the Edit... button to open the dialog box where you will define the function.)

2.   In the dialog box that appears for the definition of the Heat-Transfer-Coefficient function, 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.

Constant Value

To define a constant heat transfer coefficient, follow these steps:

1.   Choose constant in the Heat-Transfer-Coefficient drop-down list.

2.   Enter the value for $h$ in the Heat-Transfer-Coefficient field.

Example: Determining the Heat Transfer Coefficient Function

This example shows you how to determine the function for the heat transfer coefficient. Consider the simple two-dimensional duct flow of air through a water-cooled radiator, shown in Figure  7.3.36.

The data supplied in Table  7.3.1 along with values for the air density (1.0 kg/m $^3$) and specific heat (1000 J/kg-K) can be used to obtain the following values for the heat transfer coefficient  $h$:

Velocity (m/s)	$h$ (W/m $^{2}$-K)
5.0	2142.9
10.0	2903.2
15.0	3750.0

The heat transfer coefficient obeys a second-order polynomial relationship (fit to the points in the table above) with the velocity, which is of the form

Note that the velocity $v$ is assumed to be the absolute value of the velocity passing through the radiator.

Defining Discrete Phase Boundary Conditions for the Radiator

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

Postprocessing for Radiators

Reporting the Radiator Pressure Drop

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

1.   Create a surface on each side of the radiator zone. Use the Transform Surface dialog box (as described in Section  28.10) to translate the radiator 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 radiator. You can then calculate the pressure drop across the radiator.

To check this value against the expected value based on Equation  7.3-59, you can use the Surface Integrals dialog box to report the average normal velocity through the radiator. (If the radiator is not aligned with the $x$, $y$, or $z$ axis, you will need to use the Custom Field Function Calculator dialog box to generate a function for the velocity normal to the radiator.) Once you have the average normal velocity, you can use Equation  7.3-60 to determine the loss coefficient and then Equation  7.3-59 to calculate the expected pressure loss.

Reporting Heat Transfer in the Radiator

To determine the temperature rise across the radiator, follow the procedure outlined above for the pressure drop to generate surfaces upstream and downstream of the radiator. Then use the Surface Integrals dialog box (as for the pressure drop report) to report the average Static Temperature on each surface. You can then calculate the temperature rise across the radiator.

Graphical Plots

Graphical reports of interest with radiators 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 radiator. (If you display node values, the cell values on either side of the radiator will be averaged to obtain a node value, and you will not see, for example, the pressure loss across the radiator.)