CFD modeling of turbulent flow through fire sprinkler nozzle: Effects of inlet geometry

Automatic fire sprinkler systems are considered to be the most effective and economical way to apply water to suppress a fire (Fleming 2016). The automatic sprinkler itself is the key component of the sprinkler system. Automatic sprinklers must be well designed so that, when flames appear, they can detect the fire’s heat, activate the water flow and begin suppression.

It is required by the authorization agencies that a variety of performance tests be passed before the developed automatic sprinkler can be approved or listed (FM Approvals 2018; UL 2008). One of these tests is the test of discharge coefficient, also known as K-factor.

K-factor of fire sprinkler is defined as: K=Q/√p

where Q is volumetric flow rate in liter per minute (lpm) or gallon per minute (gpm), and p is pressure in bar or psi. For typical automatic fire sprinklers, it is required that individual K-factor values at each pressure be within ±5 percent of the calculated mean discharge coefficient for the range of pressure that are tested (UL 2008).

Although fire sprinklers have been in use for over 100 years, automatic fire sprinklers are developed mainly on the basis of experimental testing and there has been little progress toward developing analytical or numerical methods of calculating their effectiveness (Yao 1997; Sheppard 2002). Engineering calculations are restricted within a limited number of tasks, such as: water flow through piping. With rapid progress in computer hardware and numerical algorithms during the past decades, Computational Fluid Dynamics (CFD) has increasingly received attention. Computer simulations allow designers and engineers to design ever more challenging structures, components and processes with minimal use of expensive experimental testing. CFD has been widely used to determine flow field and pressure distribution in nozzles, orifices, valves and many others. Some of these published results include: effects of the primary nozzle geometries on the performance of an ejector in the steam jet refrigeration cycle were numerically investigated (Ruangtrakoon et al. 2013); CFD simulations were performed for flow through an orifice meter and CFD was proposed as a cost-effective tool to estimate discharge coefficient (Shah et al. 2013), and Lisowshi and Grzegorz (2017) reported determination of flow coefficient curve of a control valve based on CFD simulations.

In order to determine the discharge coefficient or K-factor value of sprinkler nozzles, it is straightforward to assume that the inlet boundary is fully-developed flow in a circular pipe. However, a specific test setup which is designated in the test standards must be used in the real tests of discharge coefficient (FM Approvals 2018; UL 2008). The inlet geometry in such test equipment is very different from the assumption of a straight pipe. Effects of the inlet geometry with such difference on the discharge coefficient, to the author’s best knowledge, were not reported. The present work is motivated by such a need.

Problem Statement and Numerical Methods

In the present work, two numerical models were developed for the purpose of simulating turbulent fluid flow through an automatic fire sprinkler nozzle. The studied sprinkler nozzle has an inlet diameter (D_i) of 0.016 m, an exit diameter (D_e) of 0.01 m, and a length (L_n) of 0.022 m. This sprinkler nozzle is designed for an expected K-factor value of 70.56 lpm/bar^1/2 (4.9 gpm/psi^1/2). Material properties of fluid are assumed to be constant, and they are evaluated for water at 1 atm and 20°C: density (p) is 998.2 kg/m³ and dynamic viscosity (µ) is 0.001 kg/(m.s). In addition, flow is assumed to be stable and steady state. Constant pressures are specified at both the inlet and the outlet boundaries, with the pressure difference in the range of 0.048 MPa to 1.03 MPa. The Reynolds number based on the exit diameter (Re=u_eD_e/v, where v is kinematic viscosity) is estimated to be in the range of 4.6 × 10⁶ to 2.1 × 10⁷. Here, u_e denotes the exit velocity.

In the first model, a segment of straight pipe is extended by 0.102 m upstream from the inlet of the nozzle. In the second model, the dimensions from the inlet geometry are based on the test equipment for discharge coefficient, as depicted in the test standards (FM Approvals 2018; UL 2008). Per the aforementioned test standards, the test equipment has a nominal diameter of 0.152m. The water way is shown in Figure 1. This is referred to as “Standard” geometry in this present work. Due to symmetry, an axisymmetric domain is used for the present simulations, as displayed in Figure 1.

The shear-stress transport (SST) k-w model is selected for modeling turbulent separated flow (Menter 1994). Compared with the standard k-w model, the SST k-w model includes the term accounting for the transport of the turbulence shear stress in the definition of the turbulent viscosity (µ_t). This allows the SST k-w model to be more accurate and reliable for flows with adverse pressure gradient than the standard k-w model (Ansys Inc. 2018).

The Reynolds averaged Navier-Stokes equation, the equations of the turbulent kinetic energy (k), and its specific dissipation rate (w) are solved numerically together with the continuity equation. Numerical solution of the governing equations and boundary conditions was performed by utilizing the SIMPLE algorithm for the pressure correction in the iteration procedure. The CFD package, Fluent v19.3, is used for solving the flow and pressure fields. More details about Ansys Fluent and the numerical method can be found in the Theory Guide (Ansys Inc. 2018). During the numerical calculations, the convergence criterion required that the maximum relative mass residual based on the inlet mass be smaller than 5 × 10^-6.

The developed CFD model was first validated with a benchmark problem: turbulent separated flow over backward-facing steps. This is one popular benchmark problem to validate CFD programs for separated flow (Drive and Seegmiller 1985; Chen et al. 2006). Comparisons of the predicted and the measured velocity profiles at several locations are shown in Figure 2. In the figure, x and y are coordinate directions, S is step height, u is velocity, and u_ref is reference velocity. More descriptions of this benchmark problem can be found in Drive and Seegmiller (1985) and Chen et al. (2006). The agreement between the numerical results and the measured data is very favorable, which provided confidence in next simulations.

Meshed computational domains for the straight and the “Standard” inlets are displayed in Figures 3 and 4, respectively. Mesh refinement is employed near solid walls or in the region where velocity gradient is expected to be high. Grid independence tests were performed using several grid densities. Different mesh densities were examined from 3,000 to 1.3 million elements. Finally, a mesh with 202,033 elements and 203,079 nodes is used for the model with “Standard” inlet geometry. Using a mesh with more elements does not lead to significant difference in the computed flow field and discharge coefficient (K-factor value).

Results and Discussion

Numerical simulations of turbulent water flow through a fire sprinkler nozzle with two different inlet geometries are performed for the inlet pressure in the range of 0.048 MPa (7 psi) to 1.03 MPa (150 psi). Velocity and pressure fields are obtained and presented.

Streamlines and pressure distribution in the nozzle with straight inlet geometry at 0.689 MPa (100 psi) are shown in Figure 5. It can be seen that pressure in the upstream pipe is relatively uniform. It is also relatively uniform in the straight exit section. Pressure drops primarily develop near the inlet of the sprinkler nozzle and in the contraction region inside the nozzle.

Streamlines and pressure distribution in the nozzle with “Standard” inlet geometry at 0.689 MPa (100 psi) are exhibited in Figure 6. Pressure in the test chamber is relatively uniform, except near the orifice plate where the sprinkler is installed. Compared with the straight inlet geometry, the “Standard” inlet geometry leads to faster pressure drop near the inlet region of the nozzle.

Computed K-factor values for two inlet geometries at different pressures are shown in Figure 7. While the pressure is low (for example, at 0.048 MPa), the K-factor value is relatively smaller. Then, it slightly increases with the increase of pressure and remains almost constant in most of the studied pressure range. Variation in the K-factor values is 1.6% and 1.1% of the minimum value for the straight and the “Standard” inlet models, respectively.

As shown in Figure 7, the predicted K-factor values using the assumption of straight inlet geometry is noticeably higher than those with the “Standard” inlet geometry. The difference, which is defined with the “Standard” values as reference, is as high as 7.6%. Parallel measurements of discharge coefficient for this sprinkler head are available, and the measured K-factor values are in the range of 69.69 lpm/bar^0.5 to 70.56 lpm/bar^0.5 (between 4.85 gpm/psi^1/2 and 4.91 gpm/psi^1/2). In comparison, the predicted K-factor values from the CFD model with the “Standard” inlet geometry provides better agreement. It is recommended that the model with “Standard” inlet geometry be used for the purpose of sufficiently accurate sizing of sprinkler nozzle.

Conclusions

Numerical simulations of two-dimensional axisymmetric water flow were performed for the purpose of examining pressure and velocity in the fire sprinkler nozzle. Pressure drops primarily develop near the inlet of the sprinkler nozzle and in the contraction region inside the nozzle. Using the assumption of a straight inlet geometry upstream of the fire sprinkler nozzle will lead to the predicted K-factor values approximately 7.0% to 7.6% higher than those with the “Standard” inlet geometry. Numerical models with the “Standard” inlet geometry provide better agreement with the measured data.

For more information, email [email protected]

References

1. Ansys Inc. (2018). Ansys Fluent Theory Guide 19.0, Canonsburg, PA.
2. Chen, Y. T., Nie, J. H., Armaly, B. F., and Hsieh, H. T. (2006). “Turbulent separated convection flow adjacent to backward-facing step – effects of step height,” International Journal of Heat and Mass Transfer, 49 (19-20), 3670-3680.
3. Driver, D., and Seegmiller, H. (1985). “Features of a reattaching turbulent shear layer in divergent channel flow,” AIAA Journal, 23 (2), 163-171.
4. Fleming, R. P. (2016). “Automatic sprinkler system calculations,” In: M. J. Hurley, et al. (eds) SFPE Handbook of Fire Protection Engineering, Fifth Edition, pp. 1423-1449. Springer, New York, NY, 2016.
5. FM Approvals. (2018). “Approval Standard for Quick Response Storage Sprinklers for Fire Protection, Class Number 2008”, pp. 57.
6. Lisowski, E., and Grzegorz, F. (2017). “Analysis of a proportional control valve flow coefficient with the usage of a CFD method,” Flow Measurement and Instrumentation, 53(B), 269-278.
7. Menter, F. R. (1994). “Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications,” AIAA Journal, 32(8), 1598-1605.
8. Shah, M. S., Joshi, J. B., Kalsi, A. S., Prasad, C. S. R., and Shukla, D. S. (2013). “Analysis of flow through an orifice meter: CFD simulation,” Chemical Engineering Science, 71, 300-309.
9. Sheppard, D. (2002), “Spray Characteristics of Fire Sprinklers,” Ph.D. dissertation, Mechanical Engineering Department, Northwestern University, Evanston, IL.
10. Ruangtrakoon, N., Thongtip, T., Aphornratana, S., and Sriveerakul, T. (2013). “CFD simulation on the effect of primary nozzle geometries for a steam ejector in refrigeration cycle,” International Journal of Thermal Sciences, 63, 133-145.
11. UL (Underwriters Laboratories). (2008). “UL Standard for Safety for Residential Sprinklers for Fire-Protection Service, UL 1626.” Fourth Edition, pp. 41-43.
12. Yao, C. (1997). “Overview of sprinkler technology research,” Fire Safety Science, 5, 93-110.