Development of a Methodology for Interface Boundary Selection in the Multiscale Road Tunnel Fire Simulations

The simulation cost of a complex dynamical system is an important consideration in engineering design and analysis, especially in fire protection engineering. One of the most common numerical approaches is computational fluid dynamics (CFD). The CFD numerical analysis is often utilized for precise studies of fluid behavior in underground space environments [3, 14, 41, 52]. This kind of numerical analysis is common to be utilized near fire field. For large domains such as road tunnel environments, network modeling software, one-dimensional (1D) simulations, can be a useful tool for fire analysis at the far field, because of low computational requirements. However, the 1D modeling approach cannot analyze the characteristics of complex flow regions encountered close to the fire source. Therefore, the multiscale methodology is a useful approach to couple a CFD solver with a 1D model to keep the accuracy and increase the computational efficiency. This approach has been used extensively in different fields. This technique was applied successfully in environmental engineering, mechanical engineering, and bio engineering [9, 29, 39, 50]. The advantage of proposed method is the reduction in the overall computation time.

Coupling methods have been used in the simulation of airflow and fire in the transportation tunnels. Colella et al. coupled CFD and 1D models of a tunnel ventilation system to decrease the ventilation simulation cost in transportation tunnels. This approach allows for the complexity of full CFD models of flow in tunnels and the inaccuracies of simplified 1D models can be avoided [10]. Colella et al. also worked on simulation of tunnel ventilation flows during fires. In that study, a simple 1D network approach was utilized to simulate tunnel regions where the flow structure is 1D (far field), and for flow conditions require three-dimensional (3D) resolution (near field), CFD was utilized. Different fire sizes ranging from 10 MW to 100 MW were investigated with a variable number of velocities. Both direct and indirect coupling strategies in steady state condition were utilized and compared. Several multiscale simulations were run to identify the interface boundary limit which is referred to as the interface boundary independence study. In that study, the CFD domain was gradually increased while the 1D domain was gradually decreased. Then the associated average error was calculated with the following norm:where \( \vartheta_{j,CFD} \) and \( \vartheta_{j,ms} \) are the values calculated in each grid point j belonging to the reference section of interest and \( \overline{{\vartheta_{CFD} }} \) is the averaged predicted by the full CFD simulation. The subscripts CFD and ms are referred to the full CFD and multiscale simulation results. The summation over j is extended to all the N grid points belonging to the specific section of the domain under study. The average of parameters, such as average temperature and average longitudinal velocity, were used for calculation of errors. It was recommended that the location of downstream interface boundary should be at a distance from the fire larger than 13 times the hydraulic diameter (D_h) when the velocity is close to the critical velocity [12]. The recommended ratio between hydraulic diameter and the distance from the fire to the downstream interface boundary provided good agreement with the same ratio which was recommended by Van Maele for different fire scenarios in a small scale tunnel [45]. In addition, the multiscale approach was utilized to study the transient flow interaction between a growing fire and a ramping-up ventilation scenarios. The time required to reach critical velocity conditions to remove backlayering was investigated in that study. The results from multiscale approach showed that the required computing time decreased by 40 times without any loss of accuracy compare to the full CFD model [13]. In previous research studies, several multiscale simuations were simulated in order to determine the interface boundaries [12]. The lowest average error between CFD and coupled models at different cross sections was the criterion for selection of the interface boundary. Therfore, an iterative method was utilized to reduce the boundary, and to compare the coupled model with the full-order CFD model across the entire domain. However, in this study, a novel methodology was developed based on the fundamental physics of fluid, including the physics of the fluid structure, turbulent kinetic energy (TKE), and the vortex dynamics to determine the interface boundaries. Since this methodology considers the physical mechanism driving flow it can easily be applied to different underground spaces with more complex geometry.

In addition, in previous research studies, the Reynolds-Averaged Navier–Stokes (RANS) equations were used for simulation of the turbulent fluctuations of CFD results. This approach, which has been largely used to simulate fire and smoke propagation [8, 12, 13, 45, 47, 50, 51], can provide results for mean quantities with acceptable accuracy at moderate cost. However, this approach has its own limitations. Van Maele and Merci applied and compared both RANS and Large Eddy Simulation (LES) approaches for well-ventilated horizontal tunnel fires. The measured critical velocity in the experiment was compared to LES and RANS simulations, and the temperature contours of the LES simulations for 30 kW fire showed better agreement with the experimental results than the RANS simulations results. Moreover, the turbulent thermal diffusion in the LES simulation showed better agreement than in the RANS simulations due to the large-scale unsteadiness in the LES [45]. LES bears less modeling uncertainties such as wakes of bluff bodies’ structure in comparison with RANS, because the flow behavior is dominated by large-scale anisotropic vortical structures [17]. Although RANS simulations have lower computation cost, by a factor of 10 to 100 [8], LES was preferred for this study for the reasons just described.

This research focuses on the development of a methodology to determine the interface boundary region upstream and downstream of a fire source in the transportation tunnels to decompose the domain into 3D and 1D domains via detailed fluid dynamics analysis. Consistent with the data from previous research studies, the interface boundary should be located in the regions where the flow structure is 1D [10‐12, 45]. In order to determine the interface boundary, it is necessary to find the region where the flow-field is quasi-1D, meaning that the streamwise component of the fluid dominates the flow-field [13]. On the other hand, the continuity of the following quantities at the interface boundaries (i and j, as shown in Fig. 1) should also be met [15].

Therefore, since the mean information of fluid (mean velocity, mean temperature, mean pressure) are transferred at the 1D–3D interface in both directions, all the node values of the 3D model at the interface should be almost uniform and close to the mean values. Under these circumstances, the single value (mean value) of the 3D model at the interface boundary can be the precise representation of all the nodes in that cross section of a dynamic system. Therefore, a detailed fluid dynamics study was conducted to investigate the distribution and behavior of the longitudinal velocity component (u-velocity) and transversal velocity components (v- and w-velocities) of all nodes at different cross sections. In order to determine the quasi-1D flow structure region, there is a need to investigate the tendency of fluid particles to rotate in the system, the physics of the vortex dynamics, and also the intensity of turbulence of the system. Due to this, the mean vorticity along the X, Y, and Z axes and the mean turbulent kinetic energy at different cross sections of the tunnel were analyzed.

The computational fluid dynamics software Fire Dynamics Simulator (FDS), Version 6.0 was used to determine the regions where the flow structure is 3D versus quasi-1D. In previous research studies it was evident that the direct multiscale fire modelling is achievable by using FDS v.6.0 and Heating, Ventilation and Air Conditioning (HVAC) feature. A significant improvement in reduction of computational time was achieved when the combination of multiple meshes and multiscale fire modelling was applied in simulations [1, 49]. The FDS core algorithm is an explicit predictor–corrector scheme, with second order accuracy in space and time. Turbulence in this software is modeled via (LES) [36]. LES has been used extensively for the simulation of the fire in different research areas such as fire plume studies, flame height studies, plume temperature, mine fires, and etc. [17, 19, 20, 22, 25, 32, 33, 35, 53]. The formulation of the equations and the numerical algorithm are described elaborately in the FDS technical reference guide to which we refer the reader [36]. Although FDS version 6.0 was utilized in this research study, There has been significant changes from FDS 6.0, to 6.6 (current version) in order to improve the robustness and accuracy of the simulations. The improvements to the robustness and accuracy of the simulation influence the simulation cost (CPU time and memory usage). The parallel processing was integerated to the the new version of FDS in order to decrease the simulation cost. Therefore, the new versions can affect the simulations’ time and results’ accuracy significantly.

For the road tunnel fire scenarios two different velocities and two different heat release rates (HRR) were utilized to investigate the effect of HRR and velocity changes on the selection of 1D-3D interface boundary. The interface boundary regions were determined according to study results. Then, the 1D models were simulated via VentFIRE™ in order to couple to the full CFD simulations. VentFIRE™ is a module of Ventsim Visual program which the transport of the smoke and heat are simulated via a discrete sub-cell transport and node mixing method [48]. The indirect coupling strategy was utilized for coupling of CFD models to 1D models; the coupled results were compared to the full CFD and 1D models. In general, there are two different approaches to couple 3D models to 1D models which refered as direct and indirect coupling approaches. In direct coupling methodology, the 1D models and 3D models are simulated and run iteratively together while in indirect coupling methodology the 1D and 3D simulations would be simulated and run separately. For detailed explaination of the direct and indirect coupling methodology, we refer the reader [12]. Ultimately, a methodology was developed and recommended for selection of the interface boundary for multiscale simulation of fire in road tunnels.

Three computational fluid dynamics (CFD) scenarios were considered to investigate the significant parameters for the selection of interface boundaries for the development of a multiscale methodology applied to road tunnel fire simulations. FDS was utilized to predict the conditions that develop due to the 10 MW and 30 MW vehicle fires in a 2 lane road tunnel. A two lane standard cross section of a road tunnel [34], is considered in this study. The height of tunnel was set to 7.7 m. Although pedestrians are not permitted in road tunnels, the sidewalks are required and recommended to be greater than or equal to 0.7 m [24]. Therefore, two 0.96 m sidewalks were considered in the geometry of the road tunnels. The thickness of the walls were set to 0.24 m. The length, the width, and the height of the whole tunnel was 960 m, 9.6 m, and 7.7 m, respectively. The detailed tunnel geometry dimensions used in the simulations are shown in Fig. 2.

Previous studies have shown that smoke generation is affected by different parameters, including HRR, ventilation, and the dimension of the obstruction (National Cooperative Highway Research Program (NCHRP) Synthesis 415 [37]). Babrauskas and Peacock discussed the HRR as the single most important variable in fire hazard [2], while the other important parameter in terms of smoke propagation is ventilation [6].

Studies examining backlayering and critical velocity show that the critical velocity varies from 2.5 m/s to 3 m/s for the 10 MW to 100 MW fires [26, 28, 40, 46, 53]. Critical velocity varies based on the hydraulic diameter of a tunnel. Thus, the critical velocity was calculated for 10 MW and 30 MW vehicle fires in the simulated road tunnel in this study with the following equations: where \( V_{c} \) is critical velocity in (m/s), \( K_{1} \) is Froude number factor 1, \( K_{g} \) is grade factor (1), g is acceleration caused by gravity (m/s²), H is the height of duct or tunnel at the fire site (m), Q is heat fire is adding directly to air at the fire site (kW), ρ is the average density of the approach (upstream) air (kg/m³), \( C_{p} \) is specific heat of air (kJ/kg K), A is the area perpendicular to the flow (m²), \( T_{f} \) is the average temperature of the fire site gases (K), and T is the temperature of the approach air in (K) (National Fire Protection Association (NFPA), “NFPA^® 502 [38]. The calculated hydraulic diameter for the two lane road tunnel was 8.53 m. The critical velocity varied from 2.6 m/s to 3.7 m/s for 10 MW and 30 MW fires in the associated tunnel. The effect of various air velocities on back layering phenomenon in the simulated road tunnels is shown in Fig. 3.

According to NFPA^® 502, the maximum tolerable air velocity under emergency conditions for motorists is 11 m/s. Also, the minimum air velocity should be enough to prevent the backlayering (National Fire Protection Association (NFPA), “NFPA^® 502 [38]. In this study, a velocity less than critical velocity (1.5 m/s < V_c) was selected for investigation of interface boundary region where the smoke and hot gases propagates to the upstream and the downstream of the fire. Moreover, a velocity greater than critical velocity (5 m/s ≥ V_c) was selected for investigation of interface boundaries when the smoke propagates just downstream of the fire. The main purpose of selected velocities was, to investigate the effect of air velocity changes on the interface boundaries determination. Two different HRR (10 MW, 30 MW) were considered as the peak heat release rates for the van and the bus fires respectively (National Fire Protection Association (NFPA), “NFPA^® 502 [38]. The t-squared approach was used for the growth of the vehicle fires. The time to reach maximum HRR (t_max) for van fire and bus fire were recommended to be 5 min and 10 min, respectively [27]. However, because of the simulation cost, the t_max was set to 1 min. Since the focus of the research in this paper is to develop a methodology for selection of interface boundaries for fire simulations in a road tunnel, the decay time period for vehicle fires was not considered in the study. Flexible polyurethane foams were utilized for vehicle fire simulation in the tunnels. The heat of combustion and the yield of fire products were set as shown in Table 1 [43].

Three different scenarios, as shown in Table 2, were simulated for investigation of different parameters in order to determine the interface boundaries. Then, the indirect coupling strategy was utilized for coupling of CFD models to 1D models. The 1D models were simulated using VentFIRE. All the vehicle fires were set in the middle of the road tunnels. A bus with dimensions of 12 × 2.6 × 3.6 m³ as the length, width, and height, respectively, was considered as the fire object for simulations.

The thermal and the physical parameters of the tunnel wall concrete, including, density, thermal conductivity, and specific heat were set to 2400 kg/m³, 1 W/m °C, and 0.96 kJ/kg °C, respectively [4]. The rock types in the concrete were assumed to be limestone, sandstone, and chert, and it was assumed that the sand and aggregate were from the same rock type at an early age. The thermal diffusivity of concrete was set to 0.77 mm²/s [30].

The physical and the thermal characteristics of asphalt depend on the air voids in the dry or wet asphalts. A 5% air voids content was assumed for consideration of different parameters. The physical and the thermal parameters of the dry pavement asphalt, including density, thermal conductivity, and specific heat capacity were set to 2372 kg/m³, 1.16 W/m °C, and 0.9637 kJ/kg °C, respectively [21]. The no-slip boundary condition was considered for all walls and the objects in the domain. In this study, the jet fans used for tunnel ventilation were assumed to be far away from the fire source. Therefore, a fixed air flow was set at the inlet of the computational domains. The cell size near the fire source plays a key role in the accuracy and stability of the numerical computation. A sufficiently fine grid can be achieved when the grid size is \( \le \) 0.1D* [35], where D* is representative of the characteristic length scale which corresponds to the total heat release rate of a fire plume [5, 53]. The D* is defined bywhere \( {\dot{\text{Q}}} \), \( \rho_{\infty } \), \( C_{p} \), \( T_{\infty } \), and g are the heat release rate of the fire in kW, air density (~ 1.2 kg/m³), air thermal capacity (~ 1 kJ/kg K), ambient air temperature (~ 293 K), and gravitational acceleration (~ 9.81 m/s) respectively.

The heat release rates in this study were 10 MW and 30 MW. Therefore, a grid size of 24 cm was considered for the numerical analysis. In all simulations, the ambient air temperature, ambient air density, and air viscosity at ambient temperature were set at 20°C, 1.196 kg/m³, and 1.79e−05 kg/m/s respectively. The simulation of vehicle fires of all scenarios at t = 900 s is shown in Fig. 4.

In order to determine the region where the flow structure behaves in a quasi-1D fashion, there is a need to investigate the longitudinal (u-velocity) and the transversal velocity components (v- and w-velocities), vorticities along different axes (X, Y, and Z), and the turbulent kinetic energy at each node in 3D CFD models. All parameters were calculated every 5 m upwind and downwind from the fire source. The zero line represents the cross section of the tunnel at the center of the fire source. According to Fig. 4c, the upwind transport of the smoke (backlayering) occurred in scenario 3 because the air velocity in this model, was less than the critical velocity. However, just the downwind transport of smoke was observed in scenarios 1 and 2, as shown in Fig. 4a, b. It was observed that the backlayering did not advance significantly along the longitudinal axis after 900 s in scenario 3 and after that, the steady-state flow condition in the tunnel was reached. Therefore, t = 900 s was selected to investigate all parameters upwind and downwind of the fire source in scenarios 1, 2, and 3.

The 1D models were simulated using VentFIRE in order to couple to the full CFD simulations. The airways and the airflow charactristics were embedded in Ventsim Visual™ 4.8 based on the dimensions and the airflow parameters as discussed. The fixed airflow was set at the tunnnel’s inlet and the outlet of the tunnel was set open. The thermal charactristics of the concrete was utilized in the heat simulation and the dynamic increment and maximum subcells were set to 0.1 s and 100 respectively in the dynamic simulation. In addition, every 5 dynamic steps, the airflow was simulated (frequency airflow simulation = 5). It was ensured that the steady state air and heat simulations are balanced and simulated properly before fire simulation. Then the fire events were simulated in the ventFIRE. Flexible polyurethane foam chractristics as shown in Table 1 were utilized for vehicle fire simulation in the tunnels. The same three aforementined scenarios (Table 2) were simulated based on various HRR and the inlet velocities. The t-squared approach was used for the growth of the vehicle fires with a 1 min as the time to reach maximum HRR (t_max). All parameters were calculated every 5 m upwind and downwind from the fire source with the zero as the cross section of the tunnel at the center of the fire source. The multiscale calculations were conducted using indirect coupling strategy with the near fire field characteristic curves implemented in the 1D models. The characteristic curves of near fire field (CFD region) are required in the indirect coupling of 3D models to 1D models [11, 12]. Therefore, the near fire field characteristic points for all scenarios were plotted in terms of mass flow rate versus total pressure drop across the domain boundaries as shown in Appendix 3. Since the continuity of the mean temperature should be met at the interface boundary, the mean temperature along the height of the tunnel at the selected interface boundaries were calculated as shown in Table 3.

The coupled model was simulated and the associated average temperature and velocity errors in the coupled scenarios compare to the full domain CFD simulations were calculated as shown in Fig. 14 (see Fig. 15 for comparison of coupled model results to 1D models’ results for scenarios 1, 2, and 3). According to Fig. 14, the mean temperature and the mean velocity errors at different cross sections after downstream interface boundary were calculated at less than 5%. The error before upstream interface boundary was calculated as a 0%.

Figure 15, shows that the mean temperature errors between 1D and the coupled model at the outlet were 49.2%, 66.5%, and 86% in scenarios 1, 2, and 3, respectively. Due to the inability of VentFIRE to precisely simulate backlayering phenomenon, a higher percentage of error of the mean temperature in scenario 3 was observed. If we assume that the 3D simulation (CFD) over the whole domain is most representative of reality, then the coupling approach results in a drastic improvement in agreement for the mean temperature results at the far fire field when compared with a 1D simulation over the whole domain. In addition, the mean velocity along the height of the tunnel at the inlet and outlet was improved. The approximate total computational time (CPU time) required for runnning the CFD model, 1D model, and the coupled model for scenario 1 was at 72.8 h, 28 s, and 32 s respectively. The CPU time for CFD simulations in scenarios 2 and 3 increased due to higher HRR and the backlayering phenomenon in scenarios 2 and 3 respectively. It was observed that the coupling strategy is able to increase the computational efficiency conspicuously while retaining the physics and producing results within 5% of the full order CFD model.

Based on the velocity components analysis and the TKE and the vorticity analysis, it is recommended the interface boundary selection procedure for indirect coupling of 3D and 1D models as shown in Fig. 16. First CFD model is the reference model and the most expensive part of the process. Based on the results, we recommend a computational domain of 5D_h upstream and 20D_h downstream of the fire source as the reference CFD model if the inlet velocity was greater than equal to critical velocity V ≥ V_c (e.g., there is no backlayering). However, if the inlet velocity was less than critical velocity V < V_c, the backlayering length should be calculated and be added to the upstream computational domain. Next, the CFD model is simulated and the inlet velocity of the domain is determined. If the the determined inlet velocity is greater that or equal to V_c, the upstream interface boundary is selected at least 0.5D_h from upwind the end of the fire object. If the selected inlet velocity is less than V_c, the backlayering length should be calculated and (1.2 D_h m + backlayering length) should be selected as the upstream interface boundary. For the determination of the downstream interface boundary in both V ≥ V_c and V < V_c scenarios, the longitudinal and the transversal velocities analysis and the mean TKE and mean vorticity analysis for the outlet cross section should be conducted. Next, the 12D_h cross section from the centerline of the object is selected as the downstream interface boundary which number 12 is the coupling variable (C_v). If the longitudinal velocity of all nodes is streamwise, and the distribution of the longitudinal and transversal velocities are almost similar to the outlet values, and the standard deviation of the longitudinal and transversal velocities of the determined section are less than 0.3 compared to the outlet values, that cross section can be accepted as the downstream interface boundary. If one of the explained requirements was not met, then (C_v +1)*D_h is selected as the downstream interface boundary to repeat the longitudinal and the transversal velocities analysis and the mean TKE and mean vorticity analysis for that selected downstream interface boundary. The method will be iterated till all requirements are met. Ultimately, that cross section is accepted as the downstream interface boundary.

It is crucial to consider that the tunnel used in this study was a straight tunnel with just a burning object in the computational domain. Previous studies [18, 31, 42] have shown that the vehicular blockage influences the flow behavior of tunnel fires, critical velocity (V_c), and the backlayering length. If other objects or fire sources (e.g., vehicles) were considered in the simulation domain, the same study should be conducted for determination of the interface boundaries before and after the extra objects are included in the tunnel, because of the effects of the temperature and the vehicular blockage on the fluid structure in the computational domain. The other influential parameter on the interface boundaries is the presence of the jet-fans in the computational domain [11] which the same study should be conducted for determination of the quasi-1D region before and after the considered jet-fans in the domain.

By utilizing this approach, the interface boundaries can be easily selected and adequately applied to couple 3D and 1D simulations as shown in Fig. 16. In Fig. 16, IB_Up, IB_Down, and C_v are upstream interface boundary, downstream interface boundary, and coupling variable respectively.

The fundamental longitudinal and the transversal velocities analysis and the TKE and the vorticity analysis for the steady state condition of the full CFD models were utilized to determine interface boundaries for coupling of 1D and 3D simulations. The selected downstream interface boundary was 12D_h m downstream of the fire for the simulations. The upstream interface boundary selection depends on the utilized velocity in the model. The upstream interface boundary was selected at (0.5 D_h) 4 m upstream the tip of the object when the velocity was greater than equal to the V_c. In the simulations with backlayering (V < V_c), the interface boundary was selected 10 m further from the tip of the backlayering (1.2 D_h). The novel methodology was applied to a tunnel with 73.73 m² cross section and 960 m in length. The indirect coupling strategy was utilized to couple 3D sub-domain to 1D sub-domains. The calculated temperature and velocity errors between multiscale models and the full CFD models were less than 5%. It was evident that the longitudinal velocity component was affected by the temperature more than the transversal velocity components in the whole computational domain. In other words, the longitudinal velocity (u-velocity) was temperature dependent in the whole computational domain while the transversal velocity components (v and w velocities) were temperature dependent just at the near field. It was observed that the temperature did not impact the transversal velocities at the far field. Due to this, the fluid field was observed the quai-1D fluid which the longitudinal velocity dominated the fluid structure.

Consequently, a novel iterative methodology was developed according to the physics of the fluid structure, TKE, and the vortex dynamics for selection of interface boundary to couple 3D and 1D models for all kinds of fire in the road tunnel or more complex underground space environments. Additionally, the work agrees well with previous work that uses a more exhaustive systematic method (gradually increasing the CFD domain and decreasing the 1D domain until a predetermined error level is encountered.) The proposed methodology was demonstrated to be a useful technique for the determination of near and far fire fields, and could be applied across a broad range of flow simulations.