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 Modeling Heat Exchangers for details.
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
that you supply. That is, the pressure drop, , varies with
the normal component of velocity through the radiator,
, as
follows:
(6–127) |
where is the fluid density, and
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
(6–128) |
where are polynomial coefficients
and
is the magnitude of the local
fluid velocity normal to the radiator.
The heat flux from the radiator to the surrounding fluid is given as
(6–129) |
where is the heat flux,
is
the temperature downstream of the heat exchanger (radiator), and
is the radiator temperature. The convective heat
transfer coefficient,
, 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
(6–130) |
where are polynomial coefficients
and
is the magnitude of the local
fluid velocity normal to the radiator in m/s.
To define the actual heat flux , specify a Temperature of absolute zero (0 K, 0 °R, –273.15 °C, –459.67 °F),
and set the constant Heat Flux value.
To define the radiator temperature, enter the value for 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.
(either the entered value or the value calculated
using Equation 6–129) is integrated over
the radiator surface area.
Fluent does not allow you to specify a value less than absolute zero for the radiator temperature.
To model the thermal behavior of the radiator, you must supply
an expression for the heat transfer coefficient, , as a function of the fluid
velocity through the radiator,
. To obtain this expression, consider
the heat balance equation:
(6–131) |
| where | |
| | |
| | |
| | |
| | |
| | |
| | |
| |
Equation 6–131 can be rewritten as
(6–132) |
where is the upstream air
temperature. The heat transfer coefficient,
, can therefore be computed as
(6–133) |
or, in terms of the fluid velocity,
(6–134) |
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 6.58: The Radiator Dialog Box), which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions).
The inputs for a radiator are as follows:
Identify the radiator zone.
Define the pressure loss coefficient.
Define either the heat flux or the heat transfer coefficient and radiator temperature.
If defining the heat flux, specify the Temperature as absolute zero.
Define the discrete phase boundary condition for the radiator (for discrete phase calculations).
Since the radiator is considered to be infinitely thin, it must be modeled as the interface between cells, rather than a cell zone. Therefore 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, right-click the zone in the tree and use the Type sub-menu to change it to a radiator zone (for more details, see Changing Cell and Boundary Zone Types).
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.
To define the pressure loss coefficient you can specify
a polynomial, piecewise-linear, or piecewise-polynomial function of
velocity, or a constant value.
Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the pressure loss coefficient:
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 button to open the dialog box where you will define the function.)
In the dialog box that appears for the definition of the Loss Coefficient function (for example, Figure 6.59: Polynomial Profile Dialog Box for Loss Coefficient 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.
To define a constant loss coefficient, follow these steps:
Choose constant in the Loss Coefficient drop-down list.
Enter the value for in the Loss Coefficient field.
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 6.60: 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 6.2: Air-side Radiator Data, 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, , as a function of pressure drop,
, and
the ratio of these two values,
(from Equation 6–127). (The air density, defined in Figure 6.60: A Simple Duct with a Radiator, is 1.0 kg/
.) The reduced
data are shown in Table 6.3: Reduced Radiator Data.
Table 6.2: Air-side Radiator Data
| Velocity (m/s) | Upstream Temp (K) | Downstream Temp (K) | Pressure Drop |
|---|---|---|---|
| 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 6.3: Reduced Radiator Data
| v (m/s) |
| | |
|---|---|---|---|
| 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
(6–135) |
where is now the absolute value of the
velocity through the radiator.
As mentioned in Radiator Equations, you
can either define the actual heat flux in the Heat Flux field, or set the heat transfer coefficient and radiator temperature
. All inputs
are in the Radiator Dialog Box.
To define the actual heat flux, specify a Temperature of 0 K, and set the constant Heat Flux value.
To define the radiator temperature, enter the value for 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.
Follow these steps to set a polynomial, piecewise-linear, or piecewise-polynomial function for the heat transfer coefficient:
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 the button to open the dialog box where you will define the function.)
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 Defining Properties Using Temperature-Dependent Functions to find out how to use them.
To define a constant heat transfer coefficient, follow these steps:
Choose constant in the Heat-Transfer-Coefficient drop-down list.
Enter the value for in the Heat-Transfer-Coefficient field.
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 6.60: A Simple Duct with a Radiator.
The data supplied in Table 6.2: Air-side Radiator Data along
with values for the air density (1.0 kg/) and specific heat
(1000 J/kg-K) can be used to obtain the following values for the heat
transfer coefficient
:
| Velocity (m/s) | |
|---|---|
| 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
(6–136) |
Note that the velocity is assumed to be the absolute
value of the velocity passing through the radiator.
If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the radiator. See Setting Boundary Conditions for the Discrete Phase for details.
You can use the Surface Integrals Dialog Box to report the pressure drop across the radiator, as described in Surface Integration. There are two steps to this procedure:
Create a surface on each side of the radiator zone. Use the Transform Surface Dialog Box (as described in Transforming Surfaces) to translate the radiator 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 radiator. You can then calculate the pressure drop across the radiator.
To check this value against the expected value based on Equation 6–127, 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 ,
, or
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 6–128 to determine the loss coefficient and then Equation 6–127 to calculate the expected pressure
loss.
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 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.
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 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.)