2.1. Experimental Study
The construction of the air terminal device was based on the change in its diameter. The design concept is shown in
Figure 1 and
Figure 2. The goal was to adapt the ATD geometry to change the inlet diameter as the flow of the system lowered, allowing the air throw to remain constant. The air flow was changed in steps and the diameter of the ATD was changed by installing a gasket between the elements. The detailed geometry of the device can be found in [
47].
To test the ATD, a laboratory stand was constructed and installed in a space with controlled environmental conditions. It was designed according to European standard EN12238: 2002 [
48], and the concept of the stand is shown in
Figure 3.
The temperature and humidity of the controlled lab space where the experiments were conducted were equal to 20 °C and 48%, respectively. The ambient air velocity was equal to zero as the laboratory was a closed room. A VAV system with a frequency inverter attached to the fan was installed, which allowed alteration of the airflow. The airflow itself was calculated according to the current standards and regulations [
49] by using an orifice plate. The laboratory set up in shown in
Figure 4.
The pressure drop on the orifice was measured using a micromanometer with the range of ±3500 Pa and the accuracy of ±1% at temperature equal to 20 °C. After the orifice, the air flew into the equalizing chamber where the flow was evened out by a series of grilles to eliminate turbulence. The air stream then flew into the ATD; turbulence from ducts and bends did not influence the flow into the test room thanks to the equalizing chamber.
After the air flew into the test zone, a thermal-resistant anemometer was used to measure its velocity and temperature. It had the range of 0.08 m/s to 20 m/s and an accuracy of ±2%. The summarized accuracy of the instruments used in the analysis are shown in
Table 1. Velocity measurements were conducted every 30 cm from the air terminal device (
Figure 5). The position of the anemometer was established for each measuring point by laser beam guidance. Thanks to the small diameter of the probe (6 mm), disruption of the air stream was minimalized. The anemometer can be seen in
Figure 4 along with a cross laser beam. Velocity measurements were carried out for a period of one minute. The sampling frequency of the anemometer was 6 s, meaning that the final result was the average of 10 partial measurements.
According to EN ISO 5167-1 [
50], the mass flow was calculated by defining the correlation between the flow and the pressure drop on an orifice using the following equation:
where
C is the flow coefficient,
is the ratio of the diameter of the duct to the diameter of the orifice,
is the expansion number,
is the diameter of the orifice (m) with its uncertainty equal to 0.0005 m,
is the measured pressure drop (Pa), and
is the air density (kg/m
3).
When the flow is calculated according to Equation (2), the measurement uncertainty is defined according to ISO 5167 [
50], and the error propagation rule as follows:
To calculate the uncertainty shown in Equation (3), the uncertainty of each individual element must be defined. The uncertainty was calculated for the maximum flow as it differed the most from the simulations.
In Equations (2) and (3), the flow coefficient when using an orifice plate is defined as follows:
where
D is the diameter of the duct, equal to 0.315 m, and
d is the diameter of the orifice, equal to 0.09 m.
The calculation of the uncertainty of the flow coefficient is shown below in Equation (7).
and
The value of coefficient A was equal to 3.6477 with an uncertainty of 1.95 × 10−5.
The calculation of the uncertainty of
(ratio of the diameter of the duct to the diameter of the orifice) is shown below in Equation (9).
where
D is the diameter of the duct, equal to 0.315 m, and
d is the diameter of the orifice, equal to 0.09 m.
Consequently, was calculated to be equal to 1.9 × 10−6 and was calculated to be equal to 1.898 × 10−7.
The expansion number
, presented in Equation (2), can be shown as
where
p1 and
p2 are the pressure upstream and downstream from the orifice, respectively, with their uncertainties equal to 0.1 Pa.
The uncertainty of
can be calculated as shown below.
The calculations gave the results of the expansion number equal to 0.9993 with its uncertainty equal to 3.52 × 10−6.
Additionally, the density of the air in Equation (2) can be defined as shown below.
where
p1 is the air pressure in the duct before the orifice (Pa), with its uncertainty equal to 0.1 Pa,
is the temperature of the air inside the duct (K), with an uncertainty of 1 K, and
is the gas constant, calculated using Equation (13).
where
pa is the atmospheric air pressure (Pa), with its uncertainty equal to 0.1 Pa, and
pv is the partial pressure for water vapor at temperature
(Pa).
The values of air density and gas constant were equal to 1.192 kg/m3 and 288.15 J/(kg∙K), respectively.
The uncertainty of partial pressure for water vapor can be calculated from the following formula:
where
psat is the saturation pressure of water vapor according to the dry-bulb thermometer.
The uncertainty of the gas constant can be calculated as follows:
In order to obtain
from Equation (3), the following equation should be used:
The calculation results were = 6.42 Pa, = 0.019 J/(kg∙K), and = 0.004 kg/m3.
After the calculation of each individual component’s uncertainty, it was possible to calculate the uncertainty for Equation (3), which was 0.00026 kg/s, giving a relative uncertainty of mass flow measurement equal to 0.25%. Such a small value indicates the very high quality of the measurements and the measurement stand.
2.2. Numerical Simulation
Air distribution has been extensively studied with CFD methods. CFD was first introduced in the ventilation industry in the 1970s, and it is widely used today to assist in the design of ventilation systems [
51]. The purpose of the CFD study was to develop and validate a computer model that could be used for accurate airflow assessment, considering different strategies, as well as different structures. CFD methods have been used by researchers before to evaluate air distribution methods [
40,
44,
52,
53,
54].
The program ANSYS Fluent version 17.0 was chosen for the study as it provides comprehensive modeling capabilities for a wide range of incompressible and compressible, laminar, and turbulent fluid flow problems [
55] where steady-state or transient analyses can be performed. The CFD simulations were carried out for the same conditions as the laboratory measurements. This allowed the simulation to be evaluated and used for future research. It was also used for the investigation of the thermal confront conditions.
To test how the turbulence models available in the ANSYS Fluent application preformed in this study, simulations were carried out to compare the k–ε and k–ω models, which are widely used for turbulent flow simulations [
56,
57]. For all cases, the ATD had the maximum diameter and maximum flow. Numerical studies were performed by selecting different turbulence models to determine the flow characteristics. The experimental and numerical results of the average velocities along the axis of the flow in the occupancy zone are compared in
Table 2. The numerical results were compared with the experimental results, and the RNG k–ε turbulence model gave the best results.
For the geometry of the experiment, an axisymmetric model was used. The geometry of the case is shown in
Figure 6 and was adapted to reflect the conditions in the laboratory stand. An equalizing chamber was designed, which served as the air inlet boundary condition. The outlet boundary conditions were located along the edges of the outlet area (
Figure 6) and were 15 m long, deliberately much larger than the air throw to not influence the simulation results.
A mech independence analysis was conducted to check how the number of elements influenced the results of the simulation. The results are shown in
Table 3. The mesh with 8,799,416 elements was used in the simulations as it had suitable parameters and the number of elements was optimal for the simulation to converge.
As shown in
Figure 6, cells with different element sizes were created in different parts of the model for a better mesh structure. Smaller cell sizes were created in the regions near the ATD and equalizing chamber, resulting in a better-quality mesh structure. The dimensional properties of these regions are given in
Table 4. Additionally, the y+ parameter was calculated as it is an important parameter concerning the wall function and is the nondimensional distance from the wall to the first node from the wall [
55]. Ideally, while using the enhanced wall treatment option, the wall y+ should be on the order of 1 (at least less than 5) to resolve the viscous sublayer [
55]. In this study, the value of the parameter was below 1 for all the wall boundaries.
After conducting the above analyses, it was decided that the simulations would be carried out using the RNG k–ε model with enhanced wall treatment and took into account gravity working in the Y-direction. The solution method settings are displayed in
Table 5. The convergence criterion was set to 10
−6 which is adequate according to the literature [
58,
59].
To study how adapting the ATD changed the air distribution, three cases were taken under consideration for three different airflows. The flow was assessed by previous measurements done in a typical office building. The air magnitude in the cases was equal to the following:
330 m3/h as the maximum airflow,
220 m3/h as the medium airflow,
150 m3/h as the minimum airflow.
The air terminal device settings were as follows:
ATD setting 1—all three rings are opened; ATD diameter DATDef = 200 mm, ATD area AATD = 30,961 mm2;
ATD setting 2—the largest ring is closed and two smaller are opened; ATD diameter DATDef = 160 mm, ATD area AATD = 19,745 mm2;
ATD setting 3—only the smallest ring is opened; ATD diameter DATD = 100 mm, ATD area AATD = 7631 mm2.