A Novel Multiscale Methodology for Simulating Tunnel Ventilation Flows During Fires
- First Online:
- Cite this article as:
- Colella, F., Rein, G., Borchiellini, R. et al. Fire Technol (2011) 47: 221. doi:10.1007/s10694-010-0144-2
- 464 Downloads
This paper applies a novel and fast modelling approach to simulate tunnel ventilation flows during fires. The complexity and high cost of full CFD models and the inaccuracies of simplistic zone or analytical models are avoided by efficiently combining mono-dimensional (1D) and CFD (3D) modelling techniques. A simple 1D network approach is used to model tunnel regions where the flow is fully developed (far field), and a detailed CFD representation is used where flow conditions require 3D resolution (near field). This multi-scale method has previously been applied to simulate tunnel ventilation systems including jet fans, vertical shafts and portals (Colella et al., Build Environ 44(12): 2357–2367, 2009) and it is applied here to include the effect of fire. Both direct and indirect coupling strategies are investigated and compared for steady state conditions. The methodology has been applied to a modern tunnel of 7 m diameter and 1.2 km in length. Different fire scenarios ranging from 10 MW to 100 MW are investigated with a variable number of operating jet fans. Comparison of cold flow cases with fire cases provides a quantification of the fire throttling effect, which is seen to be large and to reduce the flow by more than 30% for a 100 MW fire. Emphasis has been given to the discussion of the different coupling procedures and the control of the numerical error. Compared to the full CFD solution, the maximum flow field error can be reduced to less than few percents, but providing a reduction of two orders of magnitude in computational time. The much lower computational cost is of great engineering value, especially for parametric and sensitivity studies required in the design or assessment of ventilation and fire safety systems.
KeywordsTunnel Ventilation systems Multiscale modelling CFD Jet fans
Fan characteristic curve coefficients
Air specific heat [kJ/kg K]
Hydraulic diameter [m]
Diameter of the fire source [m]
Major losses coefficient
Mass flow rate through a branch [kg/s]
Mass flow rate exchanged with the external environment in a node [kg/s]
Mass flow rate of the gases released from the fire source [kg/m3]
Gravity acceleration [m/s2]
Convective heat transfer coefficient [W/m2 K]
Branch length [m]
Distance from the fan/fire region to the downstream boundary interface [m]
Length of the CFD domain in the multi-scale representation [m]
Branch perimeter [m]
Wall-lining thermal resistance [K m2/W]
External environment temperature [K]
Temperature of the gases released from the fire source [K]
Overall heat transfer coefficient [W/m2 K]
Flow velocity [m/s]
Node elevation [m]
Minor losses coefficient
Generic flow quantity [temperature or velocity]
Average error of the multiscale model [%]
Fire heat release rate [W]
Dimensionless fire heat release rate
Convective fire heat release rate per unit length [W/m]
Flame radiative fraction
Air density [kg/m3]
Air density at external environment [kg/m3]
Pressure gain induced by jet fan [Pa]
Pressure losses due to friction [Pa]
In the past decade over four hundred people worldwide have died as a result of fires in road, rail and metro tunnels. In Europe alone, fires in tunnels have destroyed over a hundred vehicles, brought vital parts of the road network to a standstill––in some instances for years––and have cost the European economy billions of euros . Disasters like the Mont Blanc tunnel fire (Italy–France, 1999) and the more three Channel Tunnel fires (2008, 2006 and 1996) show that fire events within tunnels should be managed by a global system capable of integrating detection, ventilation and fire fighting strategies in order to facilitate evacuation of occupants, assist the fire service and minimise damage to the structure. The ventilation system, installed in most tunnels, plays a crucial role controlling the smoke and maintaining acceptable conditions within the tunnel during evacuation, rescue and fire fighting procedures. The response of the ventilation system during a fire is a complex problem. The resulting air flow within a tunnel is dependent on the combination of the fire-induced flows and the active ventilation devices (jet fans, axial fans), tunnel layout, atmospheric conditions at the portals and the presence of vehicles. Depending on the accuracy required and the resources available, a solution to the problem can be reached using different numerical tools.
The overall behaviour of the ventilation system can be approximated using 1D fluid dynamics models under the assumptions that all the fluid-dynamic quantities are effectively uniform in each tunnel cross section and gradients are only present in the longitudinal direction. 1D models have low computational requirements and are specially attractive for parametric studies where a large number of simulations have to be conducted. In the last two decades several contributions on the application of 1D models to tunnel flows have been published. Ferro et al.  presented a 1D computer model for tunnel ventilation. The model was designed to deal with complex tunnel network including phenomena like piston effect and evolution of pollutant concentration. The calculations were performed in steady state and without fire. The same theoretical approach was used in the contribution by Jacques  presenting a numerical simulation of a complex urban tunnel longer than 2.5 km.
More recent applications of this methodology to real tunnels were presented by Riess et al.  and Cheng et al. . The model presented by Riess and co-workers was tested on experimental data gathered from real tunnels whose length ranged between 0.8 km and 11 km. The model presented by Cheng and co-workers was tested on experimental data from a small scale underground transportation system and then applied to simulate a hypothetical fire outbreak in the Taipei Mass Rapid Transit System. Jang and Chen  provided also a methodology to estimate the aerodynamic coefficients of a 1.7 km long road tunnel using numerical modelling and experimental measurements. All the previous contributions underline the strength of 1D models to investigate ventilation scenarios within tunnels. However, this modelling approach cannot predict the characteristics of complex three-dimensional (3D) flow regions typically encountered close to operating ventilation devices (jet fans), intersection of galleries (shafts) or close to the fire, where air entrainment, plume formation and thermal stratification dominate the flow movement. Thus, in order to account for these important elements, 1D models must rely on approximated overall aerodynamics coefficients calculated somewhere else .
Several applications of 1D modelling of fire events in tunnels have been also proposed by Institutions including CETU and U.S. Department of Transportation. Among the calculation codes there are: SPRINT , MFIRE , ROADTUN  and SES .
Computational fluid dynamics (CFD) remains the most powerful method to predict the flow behaviour due to ventilation devices, large obstructions or fire but its use requires much larger computational resources than simpler 1D models. In the last two decades, the application of CFD as a predictive tool for fire safety engineering has become widespread. The results are still limited due to the difficulties of modelling turbulence, combustion, buoyancy and radiation in large enclosures  but great achievements have been made. Woodburn and Britter [10, 11] performed a CFD study of a 360 m long longitudinally ventilated tunnel and the numerical results agreed well with the experimental measurements. Wu and Bakar , Vaquelin and Wu  and Van Maele and Merci  used CFD tools to calculate the critical velocity and its dependency on the tunnel width. The experiments were conducted in a 15 m long small scale tunnel. All the previous works confirmed the capability of CFD tool as instrument to predict the critical velocity.
Only a limited number of CFD studies directly focuses on the performance of tunnel ventilation systems like jet fans or axial fans. This kind of analysis usually requires the adoption of a very large computational domain including the tunnel regions where the operating ventilation devices are located. Armstrong  and Tabarra  studied the flow generated by fans in a rectangular tunnel. Both of these works dealt with cold flow and resulted in a good agreement between experimental and numerical measurements. Karki and Patankar  described an application of CFD to simulate ventilation flows during a fire. The model has been previously validated using the 1995 Memorial Tunnel tests  and showed an acceptable agreement with the experimental measurements in the far-field of the domain. The agreement is not favourable in the vicinity of the fire. The Memorial Tunnel tests  have also been used by Galdo Vega  to validate a CFD model which included ventilation devices (jet fans).
CFD analysis of fire phenomena within tunnels suffers from the limitations set by the size of the computational domains. The high aspect ratio between longitudinal and transversal length scales leads to very large meshes. The number of grid points escalates with the tunnel length and often becomes impractical for engineering purposes, even for short tunnels domains less than 500 m long. An assessment of the mesh requirements for tunnel flows is made by Colella et al.  for active ventilation devices and no fire and by Van Maele and Merci  for fire-induced flows without active ventilation devices.
The high computational cost leads to the practical problem that arises when the CFD model has to consider boundary conditions or flow characteristics in locations far away from the region of interest. This is the case of tunnel portals, ventilation stations or jet fan series located long distances away from the fire. In these cases, even if only a limited region of the tunnel has to be investigated for the fire, an accurate solution of the flow movement requires that the numerical model includes all the active ventilation devices and the whole tunnel layout. For typical tunnels, this could mean that the computational domain is several kilometres long.
2 Multiscale Model
The study of ventilation and fire-induced flows in tunnels [12, 13, 14, 17, 19, 20] provides the evidence that in the vicinity of operating jet fans or close to the fire source the flow field has a complex 3D behaviour with large transversal and longitudinal temperature and velocity gradients. The flow in these regions needs to be calculated using CFD tools since any other simpler approach would only lead to inaccurate results. These regions are hereafter named as the near field . However, it has been demonstrated for cold flow scenarios  and for fire scenarios  that at some distance downstream of these regions, temperature and velocity gradients in the transversal direction tend to disappear and the flow becomes 1D. In this portion of the domain the transversal components of the flow velocity can be up to two orders of magnitude smaller than the longitudinal components. These regions are hereafter named as the far field . The use of CFD models to simulate the fluid behaviour in the far field leads to large increases in the computational requirements but very small improvements in the accuracy of the results.
The adoption of multiscale models represents a way to avoid the large computational cost of the full CFD and the inaccuracies of simplistic assumptions of 1D models. A multiscale method uses different levels of detail when describing the fluid dynamic behaviour of near field and far field. The behaviour of far field and near field regions is modelled by using a 1D model and CFD model, respectively. The 1D and the CFD models exchange information at the 1D–3D interfaces and thus run in parallel.
This approach allows a significant reduction of the computational time. At the moment multiscale modelling techniques have been applied to design tunnel ventilation systems in no-fire operating conditions . The application of multiscale techniques coupling the fire to the ventilations systems is the subject of this paper. For sake of simplicity and given the uncertainties related to transient phenomena during a tunnel fire (fire growth, decay phase, and delay time of the ventilation devices) only steady state calculations are discussed here. Nevertheless, the same multiscale methodology can be applied to perform transient simulations but this is out of the scope of the work.
In this work, the prediction capabilities of full CFD and multiscale models are compared in terms of accuracy and computational time using a modern tunnel as case study.
2.1 Mono-Dimensional Model of the Far Field
The general methodology of the 1D network model for tunnels is presented in [2, 20] and only an overview is given here. The first step is to generate a network of elements representing the tunnel layout. The longitudinal domain is discretised in oriented elements called branches, interconnected by nodes. The nodes are volume-less elements connecting different branches. Each node is characterized by vertical elevation and by the value of mass flow rate exchanged with the ambient (leaving or entering the domain). Pressures, densities and temperatures are defined in each node. The branches are oriented elements connecting two nodes. The characteristics of each branch are section, perimeter, length, wall roughness, coefficient for minor losses and pressure gain due to fan action. Velocities and mass flow rates are defined in each branch.
In most cases, the fan characteristic curve is unknown or not well quantified because the fan behaviour is strongly coupled with the surrounding tunnel galleries and thus is dependent on installation details . The jet fan thrust curve provided by a manufacturer only applies to the isolated jet fan and it does not describe its behaviour once installed in a particular tunnel gallery. Usually, in situ measurements or further CFD analysis are required to quantify accurately the fan characteristic curve (see  for an example in a real modern tunnel).
2.2 CFD Model of the Near Field
The CFD modelling of the near field has been conducted using the commercial CFD code FLUENT. This code has been extensively used for simulating duct flows and it has demonstrated its capability to model ventilation flows within tunnels as well as fire induced flows [12, 13, 14, 19, 20, 22].
The turbulent fluctuations of the fluid-dynamic quantities have been modelled by means of Reynolds-averaged Navier–stokes equations (RANS). Among all the RANS turbulence models, the k–ε model has been applied in this work. The production and the destruction of turbulence kinetic due to the buoyancy have been also accounted for. RANS models have been extensively used and largely validated by the scientific community to simulate fire induced flows [10, 11, 12, 13, 14, 17, 19, 22, 23].
The standard k–ε model is not valid for fluid regions characterized by low Reynolds numbers, like in locations close to walls . In these regions the standard wall functions have been used providing adequate results for high Reynolds flows , and avoiding the need of high resolution meshes to solve the viscous sub-layer . The wall function approach is valid as long as the first mesh point is located within the logarithmic region of the boundary layer. This constraint has been verified by means of a posteriori post-processing of the CFD results.
The flame radiative fraction λ can be up to 50%  but most measured values are around 35% (value used in this work). The main limitation of this approach is that the maximum flame temperatures are not accurate close to the fire source. However, as demonstrated by Vega et al.  and by Karki and Patankar , this methodology produces a good agreement with experimental temperature measurements of away from the flames. There is little information in the literature on the gas phase temperature in a tunnel close to the fire and its dependence on the ventilation conditions and fire size. Some experimental data are reported in the Runehamar tests in Norway , where the measured gas temperature above the centre of fire ranged between 1100 K and 1500 K. The same temperature range has been considered in this paper and the corresponding sensitivity of the solution investigated.
Once defined Φ* equal to 1, the resulting top surface areas are 4.5 m2, 11 m2, 16 m2 and 27 m2, respectively for the 10 MW, 30 MW, 50 MW and 100 MW fire scenarios.
The tunnel walls have been assumed as adiabatic. Other heat transfer boundary conditions to the walls could be used, but the adiabatic condition represents the worst case in terms of buoyancy strength, threat to people and damage to the structure .
The CFD model requires also a representation of the jet fans. Previous works on CFD of tunnel ventilation [17, 19] simulated the jet fans as a combination of discharge source and intake sink of momentum and mass. This kind of approach has not been used in this paper avoiding the discrepancies in energy, momentum and species conservations that are generated by uncoupling discharge source and intake sink. The methodology used here simulates the real construction of the jet fans as a cylindrical fluid region delimitated by walls and containing an internal cross surface where a constant positive pressure jump is enforced. In order to accurately predict the thrust with this approach or any other, it is highly recommended to use experimental data for calibration or validation of the results. This approach has been implemented successfully to model jet fan installed in a real tunnel where the comparison with experimental flow measurements is excellent .
The simulations have been considered to be converged when the scaled residuals were lower than 10−5 with the exception of the energy equation where the maximum allowed value was 10−7.
2.3 Coupling Strategies at the Interfaces
provide the CFD model with the pressure and temperature boundary conditions at the interfaces i and i + 1 calculated by the 1D model
perform one iteration of the CFD model using a segregate solver
integrate the air velocities at the interfaces i and i + 1 to calculate the global mass flow rate and fix them as boundary for the 1D model (see Figure 2)
average the temperature at the interfaces i and i + 1 to provide the boundary conditions for the 1D model (see Figure 2)
solve the 1D model
repeat back to step 1 until convergence is reached.
proceed to the following time step (for transient calculations)
However, for most ventilation studies, bulk flow velocities and average temperature values in steady state or quasi steady state conditions are needed. In this case an indirect coupling method can be adopted and 1D and CFD simulations would be run separately. After identifying the near field, a series of CFD runs has been conducted for a range of uniform boundary conditions at the interfaces. In this manner, the CFD results are arranged in terms of bulk flow velocities as a function of the total pressure differences across the near field allowing the definition of characteristic curves. These curves represent the coupling of the active element of interest (shaft, jet fan, or fire) with the surrounding tunnel gallery. The 1D model takes into account these curves, accurately calculated by the CFD model and, hence, it couples them to the rest of the tunnel.
Generally, direct coupling leads to longer computational times since the solving speed is set by the CFD model. Indirect coupling leads to higher set-up times, mainly on the calculation of the characteristic curves, but then provides almost instantaneous results of tunnel flows and temperatures.
Further considerations are required when dealing with the turbulent kinetic energy and the dissipation rate at the CFD domain boundaries. Since these quantities are not calculated by the 1D model, they are introduced as a function of turbulence intensity, turbulent length scale and Reynolds number using well known relations that can be found in the literature .
The 3D region must be sized appropriately, such that the boundary interfaces are located in regions where the flow is fully developed. In a previous work the effect of the multiscale interface location in the vicinity of an operating jet fan pair has been investigated . It demonstrates that if the 1D–3D interface is located more than 150 m downstream the operating jet fans, the multiscale solution deviates from the full CFD solution by less than 1%. In this paper the effect of the interface location when modelling a tunnel fire is investigated and results presented in Sect. 3.2. In this paper both direct and indirect couplings have been used to model the behaviour of a longitudinal ventilated tunnel in normal operating conditions and in case of fire.
3 Case Study of a Modern Tunnel 1.2 km in Length
The fires are located in middle of the tunnel and four different sizes ranging from 10 MW to 100 MW are considered. The HRR is assumed to be constant and that steady state conditions are reached within the tunnel.
The emergency ventilation strategy, as for most longitudinally ventilated tunnels, requires the ventilation system to push all the smoke downstream from the incident region in the same direction as the road traffic flow, thus avoiding the smoke spreading against the ventilation flow (back-layering effect). The vehicles downstream the fire zone are assumed to leave the tunnel safely. All the studies on back layering show that the maximum critical velocity is in the range from 2.5 m/s to 3 m/s [12, 13, 34, 35]. Thus, an adequate ventilation system has to provide air velocities higher than this range in the region of the fire incident.
3.1 Grid Independence Study
Grid Independence Study of the Full CFD Domain for a 30 MW Fire and Three Operating Jet Fan Pairs
Mesh density [cells/m]
Predicted air velocity [m/s]
Deviation from mesh 4 [%]
As expected from the previous results, the computed solutions show larger deviations for the coarse meshes 1 and 2 while convergence of the temperature and velocity fields is obtained for finer meshes 3 and 4. Based on the results, grid independence is considered reached for mesh 3 and therefore, all the following simulations have been conducted using this mesh.
3.2 Boundary Independence Study
The downstream interface boundary between 1D and CFD domain must be located where the flow evolves to fully developed. Otherwise, the coupling would induce an error and the multiscale results would depend on the interface location. The previous paper on multiscale modelling of tunnel flows  provides the analysis of the effect of the interface location for cold flow scenarios. It shows that notable accuracy in the computed mass flow rate (error smaller than 1%) could be achieved when the ratio between Ld (distance from the fan to the downstream boundary interface) and Dh (tunnel hydraulic diameter) is around 20 .
In order to identify the boundary independence limit for cases including fire-induced flows, several runs of the multiscale model were conducted for a range of fire sizes. In each run the interface was placed progressively further downstream of the fire, increasing the longitudinal extension of the CFD domain L3D (see Figure 6) and consequently reducing the extension of the 1D domain by the same amount. The position of the upstream interface between 1D and CFD domain is not as critical as the downstream one where the focus is put here, but for sake of generality the CFD domain is centered on the fire source. However, if the modeller is sure that during the simulated scenarios the ventilation velocity does not change direction and the air velocity is super-critical (therefore no back-layering occurs), the upstream boundary can be moved significantly closer to the fire. This would produce a further reduction of computing time.
In order to isolate the effect of the interface location on fire-induced flows, the jet fans at this stage are assumed to be located far away from the fire and thus simply modelled as a pressure difference between portals. This pressure difference is given by combining the characteristics curves of the operating fans.
In terms of the distance from the fire to the downstream boundary interface LD (see Figure 6), the minimum ratio between LD and the tunnel hydraulic diameter DH is around 13. In a previous work Van Maele and Merci  simulated two different fire scenarios (3 kW and 30 kW) in a small scale tunnel (0.25 × 0.25 m2 cross section) under ventilation conditions close to the critical velocity. The CFD solution in the vicinity of the fire plume became independent from the boundary location if the distance LD was at least 12 times the hydraulic diameter. The agreement between the present and previous result is excellent.
Combining Figures 8, 9, and 10 allows identifying a range of module lengths between 20 m and 200 m where the average quantities at the outlet boundary as well as temperature and velocity show high deviation from the reference full CFD solution. In particular, average and flow field temperatures show a deviation from the CFD solution up to 25%; average and flow field velocities show a deviation up to 40%. However, if the CFD module is larger than 200 m, average and flow field deviations can be significantly reduced with error of few percents.
3.3 Calculation of the Fan and Fire Characteristic Curves
4.1 Cold-Flow Scenarios
The computational time required to run the full CFD model ranged between 48 h and 72 h. The multiscale model with indirect coupling runs almost instantaneously (few seconds).
4.2 Fire Scenarios
Comparison of the Results from Two Coupling Strategies for Multiscale Modelling and Full CFD for a Wide Range of Fire Sizes and Ventilation Scenarios
Jet fan pairs #1–2
Jet fan pair #3
Jet fan pair #4
Jet fan pair #5
Jet fan pairs #6–10
Full scale CFD
Mass flow rate [kg/s]
Mass flow rate [kg/s]
Mass flow rate [kg/s]
The same conclusions are reached when analyzing the results for scenarios 2–4. The differences in the predicted flow rate range between 0.01% and 1.4% for the direct coupling, and between 0.3% and 2.3% for indirect coupling (see Appendix C for comparison of field results). These results confirm the high accuracy that can be achieved by using a multiscale model. Furthermore, it must be stressed that the simulations of tunnel ventilation flows suffer of high uncertainty on the real boundary conditions at the portals, effective wall roughness, fire load and its geometry, and throttling effects of vehicles. For these reasons, the largest error induced by using the multiscale model is by far within the uncertainty range of the enforced boundary conditions and it is acceptable. On the other hand, the significantly lower computational time required by the multiscale methodology (2 h for the direct coupling, few seconds for the indirect coupling against the 48 h to 72 h for the full CFD model) is of great advantage because several ventilation scenarios can be explored and extensive sensitive analysis and parametric studies can be conducted.
Table 2 also shows that the number of operating jet fans required to achieve critical ventilation velocity in the fire region varies with the fire size. In particular 2, 4 and 5 jet fan pairs must be activated to provide super-critical ventilation velocity for a 10 MW, 50 MW and 100 MW fire, respectively. These results show that the fire throttling effect is large.
Comparing the effect of the number of operating jet fans in cold flow scenarios (Figure 14) to the fire scenarios (Table 2), the fire throttling effect can be quantified. For a 100 MW fire, the mass flow when five jet fan pairs are activated is ~200 kg/s. When five jet fan pairs are activated in cold flow scenario, the flow is ~290 kg/s. Thus, the effect of the 100 MW is to decrease the ventilation flow by more 30%. The analysis presented shows that the fire throttling effect is large and must be taken into account in tunnel flow calculations. This phenomenon was already observed experimentally in 1979 .
In this work, the ventilation scenarios are set for super-critical velocities preventing smoke back-layering. Thus, the assumption of 1D flow at the upstream boundary is guaranteed. In order to use the multiscale model to investigate sub-critical ventilation scenarios, the upstream boundary must be moved to ensure that all the back-layering is captured within the CFD domain. If otherwise, the results will be dependent on the length of the 3D domain. A rough estimation of the back-layering distance to properly design the dimension of the CFD zone for sub-critical ventilation scenarios can be obtained using the experimental correlation presented in . However, great care must be adopted as the correlation is based on small scale experimental data. A posteriori post-processing of the CFD results must always be conducted to clarify this matter.
5 Concluding Remarks
A novel and fast modelling approach is applied to simulate tunnel ventilation flows during fires. The technique is based on the evidence that there are very long tunnel regions where the flow is fully developed (far field), and relatively short portions showing 3D flow conditions (near field). The multiscale methodology uses different levels of computational sophistication to model each tunnel region saving computational time without decreasing the numerical accuracy. In particular, the far field is modelled using a 1D model and the near field using a CFD model.
Both direct and indirect coupling strategies are used and compared for steady state conditions. The methodology has been applied to a modern tunnel with 53 m2 cross section and 1.2 km in length. Different fire scenarios ranging from 10 MW to 100 MW are investigated with a varying number of operating jet fans. The effects of the mesh size and location of the 1D–3D interfaces have also been investigated.
It is shown that the accuracy of the multiscale model is high when compared to the full CFD solution. In particular, the error for all the studied scenarios is below few percents. The small numerical error is more than acceptable when compared to the large uncertainty of the real meteorological conditions at the portals, actual fire load, effective lining roughness, presence of vehicles and obstructions, etc.
To the best knowledge of the authors, this is the first time that a ventilation system has been coupled to a fire. This has allowed, among other things, to quantify the fire throttling effect, which is seen to be large and to reduce the flow up to 30% for a 100 MW fire.
The multiscale model has been demonstrated to be a valid technique for the simulation of complex tunnel ventilation systems. It can be successfully adopted to conduct parametric and sensitivity studies, to design ventilation systems, to assess system redundancy and to assess the performance under different hazards conditions. Furthermore, the authors believe that the multiscale methodology represents the only feasible tool to conduct accurate simulations in tunnels longer than few kilometres, when the limitation of the computational cost becomes too restrictive.
The authors would like to thank Dr Vittorio Verda and Dr Ricky Carvel for their help and the interesting discussions on the subject permitting the publication of this paper.