A new study from the Health and Safety Laboratory (HSL), Buxton, Derbyshire, United Kingdom, provides guidelines, recommendations and best practices for the practical application of Computational Fluid Dynamics (CFD) to the modeling of smoke movement in enclosed spaces.1 HSL modeled three fire safety engineering cases: a subway station, an accommodation module on an offshore platform and a high-rise building under construction.2 Aspects of the modeling process, including the computational grid, the discretization scheme and the turbulence model, were varied for each scenario and resulting predictions of smoke transport were compared.

Since it was impractical to gather experimental data for these scenarios and compare the predictions with the real behavior of smoke, laboratory-scale experiments were designed. Although the geometries of the four configurations investigated were relatively simple, they still retained some of the complex features found in the real scenarios, for example, inclined corridors, a corridor leading to a hall and a corridor leading to an atrium. Measurements of temperatures and visualization of smoke by a laser technique were undertaken. Each small-scale configuration was reproduced by CFD, and the predicted smoke behavior was compared with the experimental data, allowing the level of agreement to be quantified. As for the real scenarios, several CFD modeling approaches were employed and compared.

All of the different approaches provided realistic results, indicating they can be used as the basis for an engineered approach to fire safety. However, a comparison of quantitative data, such as the temperature of the hot layer, showed that key output results can vary greatly depending on the modeling approach used. Recommendations developed as part of this study1 provide guidelines that will help both CFD practitioners and regulators identify the most appropriate CFD modeling approach for the scenario under investigation and for the purpose of the simulation whether it is, for example, to evaluate the time available for evacuation before smoke becomes too dense or to check the effectiveness of a ventilation design in clearing the smoke from exit routes.

Use of CFD as a Fire Safety Engineering Tool
CFD is a powerful technique that provides an approximate solution to the coupled governing fluid flow equations for mass, momentum and energy transport. The flexibility of the technique makes it possible to solve these equations in very complex spaces, unlike simpler modeling methods that are sometimes used to predict smoke movement. CFD is now being increasingly used in fire protection engineering to predict the movement of smoke in complex enclosed spaces such as atria, shopping malls and warehouses. It is likely that regulatory agencies will increasingly be faced with assessing fire safety cases that are either entirely or partly based on the results of CFD simulations.

The main aim of the project is to quantify the advantages and limitations of CFD for predicting smoke movement in complex enclosed spaces. The project began with modeling of real scenarios. Investigators next checked the sensitivity of CFD results to a range of modeling approaches widely employed by the fire protection engineering community. This is because when setting up a model, CFD practitioners have to make numerous numerical and physical approximations. For example, the physical processes of the fire itself can be described by a variety of different submodels of varying complexity.

Small-scale experiments were performed in order to focus on areas identified by the initial simulations as potentially challenging for CFD. Then the small-scale experiments were modeled with CFD and the results were compared against the experimental results. The ANSYS CFX code was used for all cases. ANSYS CFX is a commercial CFD package with a wide range of physical and numerical submodels suited for fire safety engineering, and CFX has been widely used for smoke movement applications.

Modeling the Three Scenarios
A four-level underground station on the Jubilee Line Extension of the London Underground was used as one representative fire scenario. It was assumed that the main source of the fire was a suitcase containing clothes. In the underground station, none of the fittings or equipment are highly flammable. It was therefore assumed that the main fire source in the public areas could be the suitcase. The fire was assumed to occur in the ticket hall, in front of the shops on the unpaid side of the ticket barrier. This location was suggested by fire services. An unstructured mesh was created, and the mesh was refined at strategic locations.

An offshore accommodation with four main floors was modeled as the second case. The fire was assumed to start in the first-floor laundry, and smoke was transported into the corridors and upper levels via the stairwells. In this work, linen was assumed to burn in the laundry on the first floor. The main interest is in the transport of smoke out of the laundry into corridors and upper levels via the stairwells. The reduced complexity of the interior space compared to the underground station made it possible to use a structured grid.

An 18-story office building under construction in London was selected as the third example. Buildings under construction where fire safety equipment often is not operational are particular fire risks. The fire was assumed to start on the first floor when an armchair caught on fire. The main interest here was the transport of smoke to remote upper stories of the building via the stairwell and atrium. This was also a relatively simple geometry, so a structured mesh was also used in this application.

In the underground station, a fire with a peak heat output of 0.2 MW was used. For both the offshore accommodation module and the building under construction, a 1 MW fire was used. The offshore accommodation module and the building under construction were considered to be completely sealed, so no inlet or outlet boundary conditions were defined and quiescent conditions were imposed at the start. Large fans were provided in the underground station to generate a ventilation flow in the event of a fire to clear smoke from the ticket hall and exhaust it via the passenger exits. To model this situation, imposed flow boundary conditions were applied on the surfaces that correspond to the exits. A small background ventilation flux was used as the initial condition.

The ANSYS CFX results for the underground station show that in the five-minute period before forced ventilation is initiated, smoke is transported throughout most of the ticket hall and appears to extend to the main exit routes. Other emergency routes existed that enabled passengers and staff to escape without going through the ticket hall. Following the startup of forced ventilation, smoke is cleared from the large parts of the paid side of the ticket hall, the part past the ticket barrier, by being convected towards the exits and into the dome. Analysis of the results in the offshore accommodation module showed that at approximately 60 seconds after ignition, smoke makes its way into the adjoining corridor and 120 seconds later it has risen halfway up the nearest staircase. In the building under construction, smoke spreads as a ceiling layer within the third floor open-plan office. Shortly after one minute, smoke has entered the atrium and 120 seconds later it has risen five stories. At four minutes after ignition, it has reached the highest floor and is also rising in the stairwell.

Design of Small-Scale Experiments and Evaluation of CFD
A series of small-scale experiments was undertaken to provide data for the evaluation of CFD modeling of smoke movement. A number of CFD modeling approaches were evaluated against this data. Experiments were performed at approximately one-tenth scale in four different test configurations. The movement of a hot layer was studied in a horizontal and an inclined tunnel. The evolution of the temperature field was studied in two larger spaces connected to the tunnel, a domain with a large floor area and a domain with a large ceiling height, representing a booking hall and atrium, respectively. A well-characterized heat source was used. Laser light sheet flow visualization and time-dependent temperature measurements were performed.

Overall, the CFD simulations captured many of the observed gross flow conditions.2 In some cases, details of the temperature field were also well-predicted. However, the simulations were very sensitive to the wall heat transfer boundary condition. For example, the CFD simulations of hot gas flow in the horizontal and inclined tunnel configurations tended to overpredict the measured temperature. This overprediction is particularly pronounced with an adiabatic wall boundary condition. The CFD-predicted flow behavior for the booking hall configuration generally matched the experiments, but the temperatures were too high as the smoke entered the booking hall. In the atrium configuration, the simulated hot layer rose immediately when it entered the atrium while the experimental plume propagated across the atrium and rose along the far wall.

Sensitivity of the Results to Key CFD Parameters
The sensitivity of the results to the following CFD parameters was investigated: grid resolution, convection discretization scheme, compressibility of the flow, inclusion of buoyancy effects in the k-epsilon turbulence model, volumetric heat source and eddy breakup combustion models, and boundary conditions of heat transfer at the walls. There was not enough time to make all of these sensitivity tests for all three scenarios, but some general lessons learned were readily apparent. Surprisingly, different grid resolutions did not lead to significant differences in smoke movement. This was because both size grids employed in these problems were fine enough to capture adequately the key flow phenomena. The use of a high-order convection discretization scheme resulted in the prediction of more flow detail and a more rapid rate of smoke spread.

A Boussinesq approximation, used to account for the thermal effects of flow compressibility, underpredicted the temperatures and the rate of smoke propagation when compared to calculating the air density from an equation of state. A standard k-epsilon turbulence model also failed to predict the correct behavior of the flow. When an additional buoyancy-related production term was added (so buoyancy terms existed in both turbulence equations), the model successfully reproduced the features of the flow. A volumetric heat source model and an eddy breakup combustion model both provided acceptable and similar results for smoke propagation.

However, a realistic prescription of the fire source was found to be crucial for both models. Since a volumetric heat source model requires more assumptions than an eddy breakup model, the latter is likely to provide more realistic results where the fire shape is not well-defined initially or may vary with time. The boundary conditions for heat transfer at the walls were found to have an impact on the transport of smoke, but this was highly dependent upon the scenario. They were more important for a confined fire and in the absence of forced ventilation.

Nathalie Gobeau is with the Health and Safety Laboratory.

References

1Gobeau, N., et al., "Guidance for HSE Inspectors: Smoke movement in complex enclosed spaces and Assessment of Computational Fluid Dynamics," HSL/2002/29, Health and Safety Laboratory, Buxton, UK, 2002. Available from http://www.hse.gov.uk/ research/hsl_pdf/2002/hsl02-29.pdf.
2Gobeau, N., Zhou, X.X. "Evaluation of CFD to predict smoke movement in complex enclosed spaces Application to three real scenarios: an underground station, an offshore accommodation module and a building under construction" HSL CM/02/12, Health and Science Laboratory, Buxton, UK, 2002.