Coupled CFD-FE analysis of a long-span truss beam exposed to spreading fires

This paper presents a unidirectional coupling methodology for combining fire simulation based on computational fluid dynamics (CFD) with finite element (FE) analysis to study the response of long-span steel truss beams exposed to non-uniform temperature distributions. Fire Dynamics Simulator (FDS) was used to simulate the fire scenarios, and Abaqus was used for the FE analyses. Adiabatic surface temperatures from the fire simulations were transferred to the Abaqus model using a coupling tool called FDS2FEM. The coupling methodology was validated using two experimental studies, and it was then used to analyse the response of a long-span steel truss beam inside a warehouse building exposed to two travelling fire scenarios (fire spread perpendicular to or along the truss beams) in the building. The fire simulations showed that the fire load arrangement, ignition location and ignition distance from the ventilation opening determined the severity of the thermal field, temperature heterogeneity and the fire spread behaviour. The computational efficiency of the coupling scheme enabled the structural analysis for a large-scale structure under highly time-and space-dependent thermal exposure. The FE analyses indicated that the direction of fire spread with respect to the truss beam determined if either vertical or lateral displacement at the mid-span of the girder was dominant. The analyses also showed that a long truss beam exposed to highly non-uniform temperature fields exhibits a variety of responses like thermal bowing, lateral oscillations, efficient load redistribution, local deformations, and global failure.


Introduction
Modern buildings are expansive and geometrically complex, and the variability of fire load distribution within them increases the possibility of non-uniform, complex fire-spread incidents.As the understanding of the fire dynamics in large structures (floor area > 500 m 2 ) develops, it is also useful to study the influence of fire on the load-bearing structures in these buildings.
In 1996, Clifton had proposed the idea of a fire that moved across the structure, producing a non-uniform temperature field [1], but the idea remained nascent until the occurrence of several fire incidents in open plan structures, such as the ones in the World Trade Centre, TU Delft and others, brought more attention to this behaviour.In 2012, Stern-Gottfried and Rein improved upon the concept of Clifton and published the idea of travelling fires along with an analytical model to analyse fire behaviour [2,3].Currently, only a few well-documented studies exist where a travelling/spreading fire scenario was recreated experimentally, such as the natural fire tests at Cardington [4], the Tisova Fire Test [5], ETFT burns [6] and Malviera fire test [7].All these tests report a high degree of temperature heterogeneity within the compartment and analyse the influence of factors such as ventilation on the travelling fire behaviour.These experiments are usually quite expensive and time-consuming but are needed to develop and validate theoretical models.Computational fluid dynamics (CFD) simulations, on the other hand, also provide detailed insight into the fire behaviour and its influence on the structure through a physics-based analysis.Wellvalidated CFD models can be extremely useful for understanding fire behaviour in situations where experimental results are difficult to produce or do not exist.In [8], we demonstrated a fire spread modelling method using an ignition-temperature-based pyrolysis model for wood and a surface area correction method for the fuel geometry using Fire Dynamics Simulator (FDS) [38].The method was improved further by using a single-step pyrolysis model for wood, thereby coupling the fire spread behaviour to the ventilation conditions [9].The predictive fire spread model was validated using the BST/FRS experiments [10], and it demonstrates that fire spread scenarios can be modelled reliably using computationally feasible mesh sizes.
It is widely agreed that most large-scale structures can realistically be subjected to different types of fire spreading.However, there is no consensus on how structures should be designed against these scenarios.Wald et al. conducted a large-scale experiment to investigate the performance of an 8-storey steel-concrete composite frame exposed to natural fire [11].Under a fire load density of 40 kg⋅m -2 , the natural fire in the experiments caused local buckling and fracture of end plates but no global failure as the other parts of the structure compensated for the loss of performance of certain members.A natural fire does not produce the same level of non-uniformity in temperature and usually lasts for a much shorter duration than travelling fires.Röben et al. investigated the influence of a vertically travelling fire and a simultaneous fire across three floors on the structural performance of a twelve-storey steel building [12].They reported that a cyclic deflection pattern was observed with a slow, vertically travelling fire, a previously unaccounted feature in structural design.The study considered an entire floor to be burning at the same time and did not account for horizontally travelling fires.Based on the analytical models of the travelling fires, several studies have analysed the response of structures under the influence of travelling fires.Stern-Gottfried and Rein applied the travelling fire methodology to a generic concrete structure with a floor area of 1176 m 2 and reported that fires covering 10 % of the floor area were the most detrimental to the structures [3].
The influence of the horizontally travelling fires on the performance of bonded post-tensioned concrete floor was investigated by Ellobody and Bailey [13].They performed a non-linear finite element analysis and concluded that the horizontal movement of fire and the rate at which fire travels have a considerable effect on the deflection of the concrete floor slabs.A subsequent study to that of Röben et al. conducted by Rackauskaite et al. [14] reports that horizontally travelling fires on multiple floors resulted in a quicker failure than a vertically travelling fire.Vertically travelling fires produced higher deflection in the early phases of the fire, whereas simultaneous horizontally travelling fires caused failure sooner.All the studies performed using the travelling fire concept indicate that the heating/cooling effect caused by the movement of fire caused cyclic deflection patterns in the structure.
Several studies have been done to understand the effect of nonuniform fire on steel structures.Steel staggered-truss system (span of 1.5 m) was investigated through tests [15] and simulation [16] using localised fire based on the EN 1991-1-2 [17] method.They concluded that the connection design and the deflection of roof trusses are important in the performance of the truss systems investigated, and fullscale tests and simulations should be conducted in the future for understanding the nature of non-uniform fires further.A longer 12.0 m truss was numerically investigated in [18] using localised fire, based on EN 1991-1-2.The authors pointed out that the restrained thermal expansion should be considered for non-uniform heating; otherwise, the critical temperature of the member can be underestimated.Under the influence of a localised fire, the long-span portal frames can collapse outwards according to the numerical simulations in [19] and [20].In the study [21] using a 33.6 m long steel truss beams, it was pointed out that the structure generates a significant response under a modest temperature rise of 200 • C, and the redesigning of connections was proposed.These studies highlight the intricacies associated with the behaviour of steel structures under the influence of asymmetric temperature distribution in fires.Numerical simulations are vital for the studies of unconventional fire spread and its effect on load-bearing structures.The above-mentioned numerical studies used beam elements to model the main structures, justified by the computational efficiency and the objectives of the study.In order to study the load transfer mechanism leading to local and/or global failure in members, a detailed model of the profile of the structural elements is useful.In finite element analysis of the current study, shell elements in 3D space are adopted, which can display local buckling along with the global deformation modes.
Unconventional fire situations, like localised or travelling fires, produce a non-uniform and time-dependant temperature field over the load-bearing members with distinct heating and cooling stages.To include such complicated thermal distributions in the simulation of mechanical behaviour, a specialized tool for transferring the temperature fields over the surface of the load-bearing members with respect to time is needed.For this reason, in this study, we developed a methodology which uses the FDS2FEM [22] tool for transferring thermal boundary conditions generated in FDS [23,38] onto the FE model created in Abaqus [24].A similar study was conducted in the past using a different coupling tool (FDS2FTMI) between FDS and the FE program Ansys [25].The localised-column fire experiment conducted by Kamikawa et al. was used to validate the coupling tool [26].The authors reported that the lateral and vertical displacement predicted using this coupling was within the limits of experimental uncertainty; the final buckling time was within 10 % of the measured time.
The objective of this work is to study the response of a long-span steel truss beam exposed to fire spread scenarios using a coupled CFD-FE analysis method.The coupling procedure is validated using two tests from literature: a partially protected, restrained steel beam inside a furnace and a column subjected to a localised fire.Both the tests included the heating and cooling phases of fire.For understanding the structural response of the long-span truss beam, two fire spread scenarios were modelled within a realistic warehouse building with exposed steel truss beams.The steel truss beam within the building is analysed using the validated methodology for the two fire spread scenarios.

Coupled CFD-FE analysis
Fire-structure interaction is a problem where both entities constantly influence each other.A complete analysis of the phenomenon requires a fire solver to provide thermal boundary conditions to a finite element solver at each step and the finite element solver to impose mechanical constraints on the fire behaviour.Achieving a fully coupled solution for this interaction would be a challenging task for several reasons, as the numerical approach for solving the equations related to fire and structures are different.To analyse fire-structure interactions at and on a realistic scale and effort, a one-way coupling is the preferred option.The governing equations (Navier-Stokes equations, transport equation, radiation transport equation and the chemical reactions) for fire were solved using a CFD code, and the structural analysis was performed using a finite element code.The thermal field generated by the CFD code was then be transferred as boundary conditions to the finite element solver.In this work, the unidirectional coupling between the fire and the structure was realised by transferring data among three tools or software packages as shown in Fig. 1.

CFD simulations using FDS
FDS [23,38] is a large eddy simulation (LES)-based CFD code which solves low Mach number combustion equations on a rectilinear grid over time.The simulations in this study were performed using FDS versions 6.7.3 and 6.7.5.Turbulence was modelled using the default very large eddy simulation (VLES) mode where eddy viscosity was modelled using the Deardoff turbulence model.The thermal radiation was modelled using the finite volume method, which computes the radiation intensity over multiple solid angles using the gray gas absorption coefficient and a specified radiative fraction of the local heat release rate.The value of the radiative fraction was 0.35 except for the steel column validation, where it was 0.4.
FDS calculates the heat conduction in solids using the onedimensional heat conduction equation using the radiative and convective heat fluxes as boundary conditions [23].However, the solved solid temperatures were not used as such for the structural analyses as the 1D heat conduction solver introduced additional uncertainties.Instead, the radiative and convective heat fluxes were transferred to the finite element solver in the form of adiabatic surface temperatures for the structural analyses.

Coupling method using FDS2FEM
In this work, the CFD and FE models were coupled unidirectionally.This requires the transfer of thermal boundary conditions from the CFD model to the FE model.This transfer consists of measuring local and time-dependent characteristic temperature (called 'adiabatic surface temperature') from the CFD solution and mapping the measured values on the nodes of the FE model.

Adiabatic surface temperature
Consider a solid surface heated by incident radiative heat flux q'' inc , cooled by surface radiative emission, and experiencing convective heating or cooling between the gas stream at temperature T g and surface at temperature T s .In the CFD solver, the net heat flux to the solid would be calculated as where ε is surface emissivity (and absorptivity), σ is the Stefan-Boltzmann constant, and h is the convective heat transfer coefficient.Even if the CFD predictions for q'' inc , T g and h were perfectly accurate, the predicted values of the surface temperature T s could be inaccurate because the CFD models have only limited capabilities for calculating the solid-phase heat transfer.
Classically, finite element solvers for the solid phase have accepted thermal boundary conditions either as a surface temperature T s (Dirichlet type) or as a net heat flux (Neumann type).For the reason explained above, the use of T s from the CFD solution may lead to inaccurate results.The better option is to use net heat flux, which is typically expressed in terms of an effective ambient temperature T g , eff : The aim of the CFD-FE coupling method is to find T g,eff which makes the heat fluxes from Eqs. ( 1) and (2) equal for the same T s .However, as q'' inc generally cannot be calculated as a result of a some effective radiation temperature, it is not possible to calculate the value of T g,eff directly from the CFD solver's primary variables.Also, the transferred boundary condition should not depend on T s of the CFD model.
To enable data exchange between the fire-CFD and FE solvers, Wickström [27] expressed the heat flux in terms of a quantity called 'adiabatic surface temperature' (T AST ).Considering a virtual, adiabatic object in place of the actual solid, the heat flux into this adiabatic surface would be zero, i.e.
and T AST would be the temperature of the adiabatic surface.As the adiabatic surface is in thermal equilibrium with its surroundings, T AST effectively represents the temperature of the local ambient.From the FE perspective, the zero net heat flux of the adiabatic surface would be obtained when T s = T g,eff .
Assuming constant ε and h, we can now take T AST from the CFD and use in place of T g,eff to represent the thermal environment on the FE side.
In our work, at every time step of the CFD solution, FDS solves Eq. ( 3) iteratively for T AST on each wall cell.As the adiabatic surfaces are only virtual (output), they do not influence the CFD solution of the thermal environment itself.Also, as T AST only depends on T g , ε and h but not T s , it is not affected by the inaccuracy of the CFD heat conduction solver.T AST values are then transferred to the FE model and used in place of T g,eff in Eq. (2).

Mapping procedure with FDS2FEM
FDS2FEM, a Fortran-based unidirectional coupling tool that allows the user to transfer time-and space-dependent values of T AST from FDS to Abaqus FE code, was used for the coupling process.The tool parses the FDS and the Abaqus input files to obtain the locations and orientations of the surface nodes.The mapping parameters and the names of the data files are provided in a configuration file.Once the mapping procedure is complete, the tool generates VTK files of the FDS and FE model nodes, which can be visualised using a tool like ParaView [22].
FDS2FEM provides two different approaches for mapping the thermal boundary conditions: Node Set-Boundary File (NSET-BNDF) and Node Set-Devices (NSET-DEVC).In the NSET-BNDF approach, FDS2EM maps the digital boundary files (containing the time-dependent T AST and h values) generated by FDS onto the FE nodes.As the number of nodes in the FE model are greater than in the CFD model, the values for the specific FE nodes are calculated from the CFD solutions using a k-nearest neighbour interpolation, where k can vary between four and eight [22].In the NSET-DEVC approach, the T AST values are obtained from FDS using 'devices' (data points where T AST values are recorded in FDS) placed along the structure.The values from each point are then transferred to a set of nodes (NSET) along with a constant convective heat transfer coefficient (known as film coefficient within the FE model).
The mapping is facilitated using a node-set connectivity file that specifies the relation between the boundary file patches or devices and the node sets of the FE model.Evidently, this requires that the FE model is divided into multiple node sets.The required number of node sets presumably depends on the non-uniformity of the temperature distribution.Fig. 2 shows an example of the mapping process for a rectangular plate with 6 × 6 surface cells in CFD and 12 × 12 elements in FEA.In the NSET-BNDF approach, the data from all the CFD surface cells is utilised as the FE boundary conditions, whereas the NSET-DEVC approach makes use of only the four cells with devices.A smoother and more accurate field of temperature boundary condition can be achieved with the NSET-BNDF approach but with a significant computational cost.In this work, the NSET-BNDF approach is used in the first validation study, and the NSET-DEVC approach in the second validation case and the application example.

FE analysis using Abaqus
FE analysis was performed in two sequential stages, namely thermal analysis and mechanical analysis.The temperature history obtained from thermal analysis was used for the subsequent mechanical analysis.This type of simulation is termed 'sequentially coupled thermal-stress analysis' [28].FE models in the 3D domain were created and discretised in Abaqus using DS4 shell elements for transient thermal analysis and S4R shell elements for mechanical analysis.The density of mesh was selected based on a mesh sensitivity study for each case.An explicit solver was used to capture the highly non-linear behaviour of the structures, including both geometrical and material non-linearity.As the mass acceleration was assumed to be negligible, the dynamic effects created by the solution method were kept within acceptable limits.The thermal properties of steel were adopted from EN 1991-1-2 [17].For the material modelling, the temperature-dependent stress-strain curves for steel defined in EN 1993-1-2 [29] were used.

Validation studies
For the validation of the FDS and FEM coupling process, two tests from the literature were selected.In the first study, the thermo-mechanical response of a uniformly heated beam in a furnace was investigated by Li and Guo [30].In the second study, the thermomechanical response of a steel column subjected to non-uniform heating by a localised fire was investigated by Kamikawa et al. [26].These two tests were chosen for the validation as they impose different temperature boundary conditions on the structure.Detailed explanations about the validation studies are presented in the following sections.

Description of the test
In the experiment, a 4.5 m-long H-beam (H250) made of Q235 steel (Fig. 3) was exposed to a uniform temperature field inside a furnace.The top flange of the beam was insulated with a 3 mm-thick ceramic fibre blanket.Two concentrated loads were applied to the beam using jacks situated 1.5 m apart from each other and were kept constant for the duration of the test.The furnace was turned off after 19 min of heating, and the test was terminated after 148 min.The steel temperatures were measured at three locations along the span of the beam: near the left end, at the centre and near the right end.The vertical displacement was measured at the mid-span of the beam.

The FDS model of the restrained beam
The furnace of the experiment was modelled as a 4.5 m × 3.0 m × 1.8 m domain, and it completely enclosed the beam.Instead of modelling the furnace fire, here the temperature of the domain boundaries was controlled to reproduce the experimental values, with 920 • C being the maximum temperature attained by the walls.The temperature field included small spatial gradients associated with natural convection, but these gradients were small in comparison to the overall temperature range.As the top flange was covered with a ceramic insulation, its surface temperature differed from the temperatures of the other parts of the beam.
The steel beam was modelled in three parts: top flange, web and bottom flange.The web and bottom flange had unprotected steel surfaces with 8 mm and 12 mm thickness, respectively.The top flange was modelled as a sandwich surface with ceramic insulation covering the steel surface.The flange and ceramic insulation were 12 mm and 3 mm in thickness, respectively.The density of steel was 7850 kg⋅m −3 and the emissivity was 0.9.The temperature-dependent values of conductivity and specific heat of steel were obtained from the empirical relations provided in EN-1993-1-2.The density of the modelled ceramic insulation was 100 kg⋅m −3 and its specific heat was specified as a temperature-dependent value: 1.13 kJ⋅kg −1 K −1 at 20 • C and 1.3 kJ⋅ kg −1 K −1 at 800 • C. The conductivity was also temperature dependent: The wall temperatures were measured using k-type thermocouples with a bead diameter of 0.00025 m and bead emissivity of 0.9.Additionally, the adiabatic surface temperature (T AST ) was recorded as a boundary file to transfer the boundary conditions to the FEM model.

The FE model of the restrained beam
For the transient thermal analysis, the beam was discretised with 5400 DS4 elements.The insulation on the top flange was discretised using 17,640 DC3D8 elements.Therefore, 23,040 elements in total were used for the combination of beam and insulation (Fig. 4).For the mechanical analysis, the insulation was not modelled and the same discretisation of the beam as for the thermal analysis model was used with S4R elements.The mechanical boundary conditions for the beam can be seen in Fig. 5.

Transfer of thermal boundary conditions
In this case, the NSET-BNDF mapping is used as the amount of data generated was manageable.The number of FDS nodes was lower than that of the Abaqus nodes because the feasible grid cell size for the fire simulation was larger than the element size in the FEM.The convective heat transfer coefficient used in this case was 10 W⋅m −2 K −1 .

Validation results
The FDS simulations were performed using FDS version 6.7.1, and two different grid resolutions were used in the simulations -2.5 cm and 10 cm.The adiabatic surface temperatures showed that during the heating phase, the top flange experienced higher temperatures, and after the heating was turned off, the lower flange experienced higher temperatures.The overall temperature results of the simulation were within the limits of experimental uncertainty.The results of the FE simulation using the two FDS mesh resolutions are presented in Fig. 6.Both the 2.5 cm and 10 cm grid size of FDS-produced temperature results were within the limits of experimental uncertainty during the FE simulation.Using the temperature history from the FE thermal analysis, the FE mechanical analysis was performed, and the deformation mode of the beam at the end of the analysis can be seen in Fig. 7.The buckling of the lower flange was captured in the simulation, and the overall deformation of the beam was similar to the experiment.
The trend of the mid-span displacement of the beam obtained from the FE mechanical analysis can be seen in Fig. 8.The simulation results slightly underpredicted the mid-span displacement between 5 min and 13 min and then again from 16 min onwards.The simulated displacements were within 8 % of the test values using both the 10 cm and 2.5 cm mesh size of FDS.The axial force response at the support (Fig. 9) was predicted within 10 % of the experimental value.
Due to the presence of fire protection on the top flange of the beam, a non-uniform temperature distribution across the beam cross-section was obtained despite the uniform thermal environment of the furnace.As the beam started to lose its load-bearing capacity at elevated temperatures, the mid-span displacement increased rapidly, accompanied by the local buckling of the lower flange close to the support.The development of axial force demonstrates the magnitude of forces experienced by the supports, which is useful for the connection design.The current methodology was able to capture all these complex responses of the beam, which were compatible with the experimental values reported.

Steel column exposed to a localised fire 3.2.1. Description of the test
This validation study utilises the fire experiments by Kamikawa et al. [26] on columns subjected to localised heating, where a 1.6 m-tall square steel column (STKR400, 0.1 m × 0.1 m, 3.2 mm thick) was heated using a 0.3 m × 0.3 m, square propane burner with a heat release rate of 52.5 kW.The bottom of the column was fully restrained in all the studied cases.Case 1 and Case 4 of the experimental study were selected because they reasonably covered the aspects relevant to loads and boundary conditions (Fig. 10).In Case 1, the column top was left unrestrained, thereby allowing a stress-free deformation of the elastic body under the influence of the temperature field.In Case 4, the horizontal movement of the column top was restrained and the vertical load on the top was increased uniformly after the achievement of steady-state temperature distribution in the column.In the experiments, walls were used on two sides to protect the experimental equipment.

The FDS model of the column
The FDS model of the column was modelled as per the experiment with a domain size of 0.75 m × 0.45 m × 1.8 m.The simulations were performed with the 1 cm, 2.5 cm, 5 cm and 10 cm grid resolutions.The propane burner was modelled as a vent on an obstruction as shown in Fig. 11.The heat of combustion was specified to be 50.3MJ⋅kg −1 .The burner produced the maximum heat release rate (HRR) from 0.5 min to 59 min for Case 1 and from 0.5 min to 94 min for Case 4 with total burning times of 60 and 97 min, respectively.The burner was modelled slightly smaller in height than the actual experimental setup.This was done to reduce the influence of the burner on the adiabatic surface temperatures.
The capability of a LES in resolving the flow field (buoyant plume) above the fire source can be studied using the characteristic diameter where ρ ∞ is the ambient density, c p is the specific heat of air, T ∞ is the ambient temperature and g is acceleration due to gravity.The characteristic diameter divided by the chosen mesh cell size, D*/δx, gives the ).The T AST was recorded along the length of the column, and four values were recorded from the top plate.On the left and right surfaces of the column, the devices were placed towards the hotter edge, as this temperature was found to be the one that controls the deformation of the column.On the front and back surfaces, the values were recorded along the middle of the column.

The FE model of the column
For the transient thermal analysis, the column and the top plate were discretised with 6625 DS4-type elements (Fig. 11).For the mechanical analysis, the same discretisation of the column as for the thermal analysis model was used with S4R-type elements.The mechanical boundary conditions of Case 4 can be seen in Fig. 11.For Case 1, the vertical load and horizontal constraints were ignored.The column was partitioned into several node sets to carry out the NSET-DEVC mapping.

Transfer of thermal boundary conditions
In this case, the NSET-DEVC approach was used to map the thermal boundary conditions.The thermal exposure of the outer surfaces was mapped onto the FE model.The temperature field of the inner surface was then calculated during the FE thermal analysis, taking into account the columns internal radiation exchange.Transferring the boundary conditions only at the outer surface eliminated the propagation of errors associated with the inside temperatures of the CFD model (resulting from the use of the 1D conduction solver) to the FE boundary conditions.
Multiple mapping parameters were tested during the validation process, with several combinations of FDS grid size and Abaqus partition sizes to ensure that the non-uniformity of the temperature field is transferred accurately to the FE model.Mapping the temperature exposure on the top plate was also found to impact the temperature distribution at the top of the column.Finally, the number of devices used to record the T AST in the fire models was found to be crucial for capturing the non-uniformity of the temperature field accurately enough to predict the mechanical response.
The connectivity between the column faces and the devices was specified in the NSET connectivity file where each node set was asso-ciated to the specific device(s).With a vertical partition size of 5.0 cm, FDS device resolutions of 2.5 cm and 5.0 cm were used for the transfer of boundary conditions.A device resolution of 2.5 cm in FDS meant that the T AST values were recorded at every 2.5 cm, and each FE partition would receive an T AST values averaged over two devices.A device resolution of 5.0 cm meant that each partition received information from a single device.Another sensitivity study was performed with a partition size of 10.0 cm in which three different FDS device resolutions were used -2.5 cm, 5.0 cm and 10 cm.The convective heat transfer coefficient used during the transfer of T AST was 25 W⋅m −2 K −1 in both cases.

Validation results
The validation simulations were performed using FDS version 6.7.3 on the Puhti supercomputing cluster.The domain was decomposed into 4 meshes, and each mesh was assigned to a separate parallel process.Four mesh sizes were simulated: 1.0 cm, 2.5 cm, 5 cm and 10 cm.The computational time varied from 6 days for the 1.0 cm mesh to simulate 20 min of experiment to 1 h for the entire simulation with 10 cm mesh.
Fig. 12 shows the flame behaviour and the T AST during the steady burning period of the fire.The front surface is exposed to the flame at all times and experiences the highest T AST of around 750 • C as shown in Fig. 12.The highest temperatures are observed from 0.4 m to 0.8 m along the front surface of the column, but the part of the column below the burner does not experience any notable change in temperatures as shown in Fig. 12.The left surface is slightly hotter than the right surface, as the flame tends to bend towards the left.The steel plate on the top of the column is heated radiatively by the flames and convectively by the smoke plume.This creates a relatively high temperature at the top of the column.Within the hollow column, the back surface is internally heated by radiation from the front and side surfaces along with a small convective contribution from hot air.
The sensitivity of the simulated steel temperatures to the FDS cell size (2.5 cm, 5.0 cm and 10.0 cm) and FE partitioning size (10.0 cm and 5.0 cm) is shown in Fig. 13 by comparing temperatures at 400 mm and 1200 mm heights of Case 1.At 400 mm, the temperature development in the column was due to the flame being directly impinged upon the surface; at 1200 mm, the temperature development was due to conductive, convective, and radiative heating of the column.Using 10.0 cm partitions, the 2.5 cm FDS cell size leads to better agreement with experimental results than cell sizes 5 cm and 10 cm.However, none of the simulations reproduces the negative slope of the semi-steady state temperature, observed at a height of 400 mm.With 5.0 cm partitions, the FE simulation based on the FDS cell size 2.5 cm again showed better agreement with the measured data than the simulation based on the 10 cm FDS cell size.
A convergence study was carried out for the fire simulation with a cell size of 1.0 cm, and the T AST results showed no deviation at 400 mm and 600 mm during the steady burning phase.The T AST at 800 mm and 1200 mm showed a deviation of 9 % and 18 %.Due to the rapidly increasing computational effort and the good agreement of the FE results with the measured temperatures, the 5.0 cm partition with a 2.5 cm FDS cell size was selected for the validation study.
In Fig. 14(a) and (b), the steel temperature development at different heights of the column is compared between the FE analysis and the test for Case 1.The fire-exposed surface of the column in Fig. 14(a) showed a reasonable agreement between the simulation and the test.The temperature was underpredicted in the simulation by 5 % at 400 mm and 1200 mm and overpredicted by 60 % at 1600 mm.The temperature of the back surface of the column in Fig. 14(b) was underpredicted in the simulation by about 15 % at 400 mm, by 11 % at 800 mm and by 30 % at 1200 mm and overpredicted by 60 % at 1600 mm.Fig. 14(c) and 14(d) show a similar comparison for Case 4. The exposed surface temperature in Fig. 14(c) was underpredicted in the simulation by 4 % to 8 % at 400 mm and 1200 mm and overpredicted by almost 60 % at 1600 mm.The temperature of the back surface in Fig. 14 (d) was underpredicted in the simulation by 20 % at 400 mm, 13 % at 800 mm, 35 % at 1200 mm and overpredicted by 70 % at 1600 mm.
The FE results of the temperature development along the height of the column suggest that for the localised fire, the numerical and experimental values for steel temperatures agree, close to the source of the fire, but their difference increases along with the distance from the fire source.
In Fig. 15, the temperature distribution along the column in Case 1 is highly non-uniform which was also observed in Case 4. The maximum temperature occurred at about a column height of 400 mm.Fig. 16 shows the observed buckling mode in Case 4 along with the deformation documented in the experiment.Also, clear similarity between simulated and experimental buckling is observed.
In Fig. 17, the horizontal displacements in Case 1 at different heights of the column are compared.Local heating bowed the column, and the maximum displacements were observed at the highest point of the column, which is 2 mm (8 %) below the experimental value, while the displacement during the steady-state temperature was larger by 4 mm (25 %).Generally, the displacement values of the test and the FE mechanical analysis matched well.
The measured and predicted vertical displacements of the column top in Case 4 are compared in Fig. 18.The column, as shown in Fig. 11, was horizontally constrained, and the results of constraining one of the  axes (x-axis is along the face of the fire-exposed surface) and both x and z horizontal axes are presented in Fig. 18.The vertical displacement was underpredicted in the FE mechanical analysis by 1 mm (20 %).Failure of the column was observed to take place at around 82 min and 96 min for the respective simulations and at 88 min for the test.The overall deformation response of the column was well reproduced.
In terms of engineering applications, the accuracy of the simulated thermal and mechanical responses can be considered sufficient.For the selected steel structures, the temperature development, deformation modes and displacements showed good qualitative correlation with the test results, and the quantitative differences between the simulated and measured values were 30 % (average) for temperature and between 8 % and 25 % for displacement.Zhang et al. [25] performed similar coupled simulations of the column test [26] using Ansys [31].In their study, the horizontal displacement for Case 1 was underpredicted during the first 10 min and overpredicted towards the end of the simulation, similar to the current study.The displacement trend for Case 4 was also similar; however, they provided only a limited temperature comparison for Case 1 and no comparison for Case 4.

Description of the structure and the selected truss beam
The target of the application example was to produce a highly nonuniform travelling fire scenario within the building and then investigate the feasibility of the simulation chain in producing detailed predictions of the structural behaviour.A typical warehouse composed of several unprotected truss beams as load-bearing structures was considered (Fig. 19).The dimensions of the building were 38 m × 31 m × 9.6 m.Two fire scenarios were considered in the simulations: Scenario 1the fire path is perpendicular to the truss beams; Scenario 2 -the fire path is parallel to the truss beams.To achieve a travelling fire, that is, a combination of ventilation and fuel-dependent fire behaviour, only one opening (24 m × 9.6 m) was defined for each scenario.The structure was not equipped with a sprinkler system, and the use of sprinklers could result in significantly different fire behaviour and temperatures.The floor plan design of this structure was provided by Ruukki Building Systems Oy (now Nordec Oy).The frame system was based on planar frames with truss beams and columns.Some of the structural members had rectangular hollow sections.The individual truss beam was composed of a top chord, a bottom chord, six vertical braces and fourteen diagonal braces in the structure.Out of the six identical truss beams, one truss beam was selected to demonstrate the mapping of the FDS temperature field and a sequentially coupled thermal-stress analysis in Abaqus.For simplicity, both beam supports were modelled as columns in Scenario 2 even when the beam was above the doorway or vent.

The FDS model of the truss beam
The computational domain for the fire simulation covered the building interior and an additional 4.0 m-deep domain in front of the doorway or ventilation opening to minimise the influence of the open boundaries and to account for the heat produced by the flaming outside the compartment (Fig. 19).The mesh cell size was 0.2 m within the compartment and double outside it.The exterior walls were sandwich panels of steel plates with mineral wool insulation.The properties of steel were taken from the Eurocode [32], with emissivity set to 1.0.The density of mineral wool was 125 kg⋅m −3 and specific heat was 0.7 kJ⋅kg −1 K −1 .The thermal conductivity of mineral wool was temperature dependent and specified to be 0.034 The truss beam was modelled as a combination of multiple elements: columns, upper and lower chords, vertical and diagonal bracings, as shown in Fig. 20.The columns were 9.2 m high and were modelled with a thickness of 0.2 m.The lower chord and upper chord in the model were 30.4 m and 30.8 m long respectively.The vertical bracings were 2.2 m long and were placed at the same locations as in the actual truss beams.Due to the rectilinear mesh used in the FDS analyses, the diagonal bracings were modelled as grid cell -sized cubical elements, which were placed along the along the centre line of the diagonals in the middle of their spans.The thermal exposure of the diagonal bracings was then obtained by recording the T AST values on the four faces of this cubical    element, as shown in Fig. 21.A similar approach with cubical elements placed at multiple locations can be used for recording the thermal exposure of inclined obstructions.The secondary beams between the main girders were not included in the model.
The fire load distribution represented a rack storage typically used in warehouses.A total of 204 wood piles with a height of 4.2 m were arranged in the compartment with a spacing of 1.0 m between each pile.Each wood stick in the pile was 0.2 m thick and 1.0 m long.Each layer of the pile consisted of 3 sticks, and each pile consisted of 21 layers of sticks.A spacing of 3.6 m and 4.2 m was provided on the long sides of the fire load.The combustible energy of each pile was 7458 MJ⋅m −2 , and the average fire load density was 1300 MJ⋅m −2 This was in line with the Finnish building code [33], which assumes that warehouses have a fire load density>1200 MJ⋅m −2 .
The fire spread was modelled using a combination of the ignition temperature-based pyrolysis model and the single-step pyrolysis model for wooden fuel presented in [9].Two different ignition locations shown in Fig. 19 were assumed to compare the effect of fire spread direction on the results.The initial fire was produced using a 1 m 3 volume of wood crib (represented as the red-coloured section of the wood pile shown in Fig. 19), where the surface pyrolysis was modelled using an ignition temperature of 300 • C and an assumed heat release rate of 320 kW⋅m −2 , following the approach validated in [8].An ignitor was placed under the crib to provide the required ignition energy.The remaining fuel was modelled using the single-step pyrolysis method.The modelling procedure utilised in this simulation has been validated and reported in [9].

The FE model of the truss beam
For the transient thermal analysis, the selected truss beam was discretised with 31,572 DS4-type elements.For the mechanical analysis, the same discretisation was used but with an S4R element type.The mesh discretisation of the top-left part of the truss beam can be seen in Fig. 22.For the purpose of mapping, the members of the truss beam were partitioned as can be seen in Fig. 23.The columns of the truss beam were partitioned at every 0.5 m distance, and the top and bottom chords were partitioned at every 1 m distance.The diagonal elements and the vertical chords were not partitioned.
The bottom of the columns was assigned as rigid supports.It was assumed that secondary beams constraining the out-of-plane displacement of the main girders also underwent material degradation and were unable to restrain the truss beam at elevated temperatures.Therefore, the out-of-plane movement of the truss beam was left unconstrained.The yield strength of the steel material was 355 N⋅mm -2 .The mechanical loads included self-weight of the steel, snow loads (2.28 kN⋅m −2 ) according to EN 1991-1-3 [34] and horizontal wind loads (0.623 kN⋅m −2 ) according to EN 1991-1-4 [35].The loads were combined according to EN 1990 [32].

Transfer of thermal boundary conditions
From both fire scenarios, the truss beam directly above the ignition point was selected for the structural analysis: truss beam 1 from Scenario 1 and truss beam 3 from Scenario 2. In addition to being the first truss beams to experience excessive heating, these truss beams also showed the highest non-uniformity in heat exposure.
Along the four faces of the top and bottom chords, the T AST data was recorded from FDS every 50 cm, which was a little more than the width of two grid cells.The thermal exposure on the vertical and diagonal elements was recorded using four devices with different orientations, placed in the middle of each element.The T AST on the columns was recorded every 20 cm for the three exposed faces.The surfaces of the column facing the walls were not mapped.The convective heat flux coefficient was recorded during the simulations and its peak value of 20 and 25 W⋅m −2 K −1 were used to map the T AST values of both Scenario 1 and Scenario 2, respectively.In the Abaqus model, each face of the top chord and bottom chord was divided into 31 node sets.Similarly, each face of the vertical and diagonal elements was assigned to one node set.For the columns, each face was divided into 19 node sets.A total of 830 devices were used to transfer the thermal field from the fire simulation to 42,464 FEM elements.

Fire simulation results
The fire simulation was performed using FDS v6.7.5 on the Triton supercomputing cluster.The computational domain was decomposed into 40 meshes, and each mesh was assigned to its own parallel process.The overall temporal development of the fire is the same in the two scenarios and can be divided into five phases: 1. ignition phase, 2. local fire, 3. rapid spread to the opening, 4. burning at the opening and 5. backward travelling phase.The time spans of these phases are listed in Table 1 along with the corresponding ranges of the resolution indicators D*/δx.
In Scenario 1, fire spreading started within the ignition pile after about 3 min of heating and forms a hot plume above the wood pile.The maximum gas temperature around the truss beam above the plume was around 700 • C as shown in Fig. 24.By 10 min, the fire spreads to multiple adjacent piles, the gas temperature was around 1000 • C above the plume centreline and a classical two-layered temperature field with a ceiling jet was observed: a hot layer near the ceiling and a cold layer below the top level of the fire load.By 11 min, the fire started to spread towards the opening, and the amount of oxygen around the burning region decreased (Fig. 24).By 16 min, the fire spreads to the fourth row of piles and gas temperatures around all the truss beams of compartment were between 700 • C and 1000 • C.This was followed by a rapid decrease in the oxygen concentrations as the oxygen was consumed faster than it was replenished.This forced the flames towards the opening in about two minutes.By 21 min, the burning front was at the opening, and the truss beams near the opening were exposed to a temperature close to 1000 • C. The other truss beams in the compartment experienced a temperature around 600 • C. Around 25 min from the ignition, the fire started to travel back into the compartment as it completely consumed the fire load at the opening.During this phase, the region of direct fire exposure moved towards the back of the compartment, driving the temporal variation of the truss beam heating, but the truss beams near the openings continued to experience high temperatures due to the hot gases from the burning region flowing out of the compartment.
In Scenario 2, the fire development in the early stage was slightly slower than Scenario 1.The fire spread beyond the ignition region started about 3 min later, and this difference propagated throughout the entire fire development.The predicted temperature and oxygen concentrations of Scenario 2 are shown in Fig. 25.At 10 min, the maximum temperature was about 700 • C but the hot gas layer was thinner than  a Part of the heat release outside the computational domain.The results show that in Scenario 1, the fire spread was driven by the depletion of oxygen at the closed end of the compartment whereas in Scenario 2, it was a combination of both oxygen depletion and fuel burnout.The simultaneous burning observed in Scenario 2 was a result of the shorter fire path to the opening.Also, the oxygen depletion observed in Scenario 1 was not observed in Scenario 2, as oxygen concentrations in the compartment remained high until 25 min.
Fig. 26 compares the occupied flame volumes at 25 min in the two scenarios.A larger burning front covering the length of the fire load distribution was produced at the opening in Scenario 2. This provided the fire with more fuel in Scenario 2 than in Scenario 1, resulting in higher temperatures.The velocity fields in Fig. 27 and Fig. 28 show the flow field in the compartment during the two scenarios.In Scenario 1, a two-layer flow was seen until 21 min, with hot gases at the top and cooler air entrained through the wood cribs.The maximum speed of the hot gases flowing out was approximately 12 m⋅s −1 , and oxygenated air was entrained into the plume at speeds less than 2 m⋅s −1 (Fig. 27).The flow became more turbulent during the back-travelling phase as seen at 22 min.
In Scenario 2, the maximum speed of hot gases flowing out was approximately 6 m⋅s −1 , and the entrainment velocity was below −1.0 m⋅s −1 .The air entrainment velocity at the room centre line was low, as the oxygen levels in the compartment were not significantly depleted.The simultaneous burning further increased the turbulence in the compartment as seen at 23 min in Fig. 28.The high turbulence was high during the back-travelling phase in both the scenarios.Fig. 29 and Fig. 30 show the adiabatic surface temperatures (T AST ) along the top and bottom chords of three truss beams of the compartment.In Scenario 1, truss beam 1 was directly above the ignition point, truss beam 3 in the middle of the compartment and truss beam 6 closed the opening.In Scenario 2, truss beams 1 and 6 were on the sides and truss 3 was the one directly above the ignition point.In both scenarios, the heat exposures during the first 16 min resembled a localised fire, as only a small portion of the truss beam (truss beam 1 in Scenario 1 and truss beam 3 in Scenario 2) was exposed to extremely high temperatures.A variation of approximately 600 • C along the truss beam was observed at 15 min.As the fire developed, the T AST along the truss beam and along the top chords in particular became more uniform due to the formation of a hot gas layer.
In Scenario 1, the T AST on truss beam 3 and truss beam 6 was In Scenario 2, the T AST on truss beam 1 was uniform until 35 min, at which point it showed a significant non-uniformity (≈ 600 • C) in the bottom chord.The T AST on truss beam 6 in Scenario 2 was relatively uniform until the end of the simulation.

FE analysis results
Fig. 31 shows the temperature development along the span of truss beam 1 from Scenario 1 for the different periods of FE simulation.The maximum temperatures were observed close to the mid-span around 20 min in both the top and bottom chords.Temperature non-uniformity along the span was most prominent at 15 min, with maximum differences within the top and bottom chords at about 690 • C and 800 • C, respectively.This temperature non-uniformity gradually reduced as the simulation time progressed.The temperature differences along the beam span between the two chords approached 50 • C at the end of the simulation.
Fig. 32 shows the temperature development along the span of truss beam 3 from Scenario 2. At 15 min, the left part, where the fire originated, had a higher temperature than the rest of the truss beam.This trend of the non-uniform temperature continued until 25 min, when maximum temperatures were observed.The temperature nonuniformity along the truss beam significantly reduced from 30 min, and the temperatures at the right partthe part close to the vent, reached relatively higher values.The temperature non-uniformity along the top and bottom chords was most prominent at 20 min, with maximum differences of about 700 • C and 900 • C, respectively.Specific to the back-travelling behaviour, the cyclic temperature history was observed in the left part where the steel was subjected to two heating stages during the 40 min simulation.
Comparison of the two heating scenarios showed that in Scenario 1, a peak steel temperature of 1060 • C was reached at 20 min at the mid-span while the truss beam ends were about 400 • C cooler.In Scenario 2, the maximum temperature peaks were at 25 min, and the overall temperatures continued to increase in time.The maximum temperature in Scenario 2 was about 1200 • C at the left part of the truss beam, and the temperature of the rest of the span was 300 • C or more.Truss beam 3 in Scenario 2 was thus exposed to higher temperatures than truss beam 1 in Scenario 1.Since carbon steel loses 53 % of its strength capacity at 600 • C and 89 % at 800 • C [ 29 36], it was interesting to see the failure mechanism of the steel truss beams exposed to the aforementioned fire scenarios.
Fig. 33 presents the temperature contours of the studied steel truss beams in scenarios 1 and 2. The time series of the temperature contours corresponded to the highest temperatures in Fig. 31 and Fig. 32.Fig. 33 (a) shows that in Scenario 1, the columns had a temperature gradient from 24 • C at the bottom to 700 • C at the top.Similarly, the temperature of the columns shown in Fig. 33(b) varied from 24 • C to 825 • C in Scenario 2. The right column of the truss beam in Scenario 2 was much colder than the left one because it was placed at the doorway.The temperatures at the bottom chord of the truss beams were higher than that those at the top chord in both the scenarios.The temperature variations along the span and height of the truss beams indicate high nonuniformity in heat exposure.
The temperature history of the FE thermal analysis was used for the subsequent FE mechanical analysis.The deformation behaviours of the truss beams are presented in Fig. 34.The lateral or out-of-plane and vertical deflections are represented as mid-span displacements of the bottom chord of the truss beams.In Scenario 1 (left figure), the truss beam started to deflect laterally 1.6 min before any vertical movement, and the lateral displacement was more significant than the vertical one.The lateral displacement was −471 mm towards the back wall at 11 min, after which the direction of the displacement was reversed, and the peak lateral displacement of 833 mm was observed at 16.6 min.The deformation behaviour was caused by the fire plume moving from the left side of the truss beam to the right side between 11 and 16 min, as shown in Fig. 24.The maximum positive vertical displacement of 335 mm was observed at 18.3 min.The temperature difference between the bottom and the top chord created torsion and bending of the truss system.In Scenario 2 (Fig. 34 right), the vertical displacement was more significant than the lateral displacement.Minimal thermal bowing towards the direction of the top chord was observed, resulting in a peak positive vertical displacement of 142 mm at 22.2 min.Following this, the truss beam gradually deflected downwards with an increasing rate.
To evaluate the global failure of the truss beams, a vertical displacement limit of span/20 can be considered [37].For the 31 m-long truss beam, the span/20 limit is 1550 mm.The truss beam in Scenario 1 had local temperatures as high as 1050 • C, but the vertical displacement did not exceed the displacement limit criterion, thus demonstrating an efficient load redistribution in the truss system.In Scenario 2, the deflection of the truss beam increased rapidly after 32 min and crossed the displacement limit at 35.5 min, indicating global failure.The failure occurred during the back-travelling phase, when the high-temperature region expanded from the doorway towards the back of the compartment.
To observe the extent of deformation, the deformed truss beams were superimposed on the undeformed geometrical forms in Fig. 35.The deformation contours were taken at the time of maximum vertical displacement at the mid-span of the truss beam.Apart from the lateral displacement of the lower chord, torsion of the section was visible in Scenario 1 as seen Fig. 35 (a).In Fig. 34(b), which represents Scenario 2, the whole section of the truss beam had lateral displacement outwards, and the beam had significant downwards displacement at the mid-span.In the Fig. 34(b), a local buckling of the right column just below the bottom chord is also shown.

Discussion on the sources of uncertainty
This work was undertaken to demonstrate the methodology for a unidirectionally coupled fire-structure analysis using FDS and Abaqus.The accuracy was quantified using a pair of validation studies, and the usage demonstrated through an application where a fire spread scenario was simulated within a large-scale building.Inevitably, there are a lot of assumptions and limitations embedded in the fire modelling, data transfer and finite element analysis.The uncertainties and shortcomings that exist in the three phases of a unidirectionally coupled fire-structure analysis is discussed here.
First, the accuracy of the coupled fire-structure analysis requires a fire model that reproduces the thermal field with reasonable accuracy.Fire behaviour (burning rate) in the validation studies was known and, hence, reproduced as well as the experimental uncertainty allowed.In the application case, the fire behaviour was predicted using a previously validated fire spread modelling approach.However, some inherent model and input uncertainties could not be avoided.Predicting the flame and fire spread is extremely challenging, and despite the previous  validation efforts, much more work is needed to enable reliable routine predictions of the fire development.
With any given fire, the mesh resolution is among the most crucial factors affecting the uncertainty of heat exposures.With coarse meshes, flame temperatures can often be underestimated, leading to quite low convective and radiative heat fluxes heat exposures, expressed as adiabatic surface temperatures.High numerical resolution is especially difficult to achieve in the beginning of the fire when the fire power and size are small, as shown in Table 1.It is necessary to prescribe sufficiently strong and long-lasting initial fire to ensure robust prediction of the fire spreading beyond the ignition region.Small differences in the computational setup may lead to temporal differences of several minutes, and these differences will propagate to the timings of all fire -induced events in the simulation.Numerical predictions of the fire resistance ratings will thus suffer from the temporal inaccuracy of early fire spread.
The sensitivity of fire development to input parameters, such as geometry, fire load arrangement and fuel type was not the focus of this study but can be considered in future research.The predicted thermal environment was, however, seen to depend on the fire load arrangement and opening placement.Moreover, the fire load arrangement impacts the burning behaviour as it influences the air entrainment into the burning region, as shown in Fig. 36.The flow above the fire load consists of hot gases flowing out of the compartment whereas the flow between the wood piles changes with the fire stage.During the first 1000 s, air entrained towards the burning region from between the piles and through the aisles on either side of the fire load, shown by the regions of negative u-velocity in Fig. 36.During the backward spreading phase of the fire, the aisles in the middle are behind the flame region but the sides still serve as entrainment paths, maintaining the high heat release rate within the compartment.
As the unidirectional coupling cannot consider possible changes in fuel and ventilation geometries, deep insight is required from the user to ensure that situations following from the possible failures and collapses are included in the investigated scenarios.This may require iterative approach to the fire scenario definition.
Second, the amount of detail captured during the mapping procedure partially determines the accuracy of the coupled analysis and finding the appropriate resolution may require some iterations too.Ideally, mapping the values from each node of the fire model would be desirable as it would capture all the temperature gradients as precisely as modelling allows.In the furnace validation study, data from each FDS cell was mapped onto the FE model, but the accuracy benefit of this approach could not be demonstrated, because the case had very uniform temperatures.When the structure sizes increased in the second validation study and the application example, this approach became too data and time intensive.Therefore, the NSET-DEVC approach was used, and the resolution of the T AST values and node set sizes determined the accuracy of the transferred non-uniform temperature distributions.In the application case, the data was recorded at every 0.5 m in FDS.Even though this might be considered too coarse in other scenarios, in this case, it was the best possible balance between computational effort and mapping precision as it ensured that the gradients across the frame elements and, especially, over the chords were captured.The gradients across the diagonal and vertical elements were not prominent and, hence, were not entirely captured.Also, the sensitivity of the results of the application case against the mapping resolution was not determined.In real applications, it may be difficult to know beforehand the number of measurement points required for a fire scenario; hence, it would be prudent to have more data recording points in the fire simulation to ensure all aspects of the thermal field are captured.
Another mapping parameter that can be a crucial factor is the convective heat transfer coefficient.The current procedure uses a constant convective heat transfer coefficient whereas, ideally, a timedependent value of the convective heat transfer coefficient would be the best solution.This was noticeable in the underpredicted temperatures of the column back surface in the second validation case.
Finally, the accuracy of the coupled fire-structure analysis depends on the FE analysis.The size of the partitions of the FE model as showcased in the column validation case affected the accuracy of the results.The selection of the shell elements DS4 for the FE thermal analysis and S4R for the FE mechanical analysis was vital for capturing the thermal non-uniformity and the development of local stresses in the structures.Another important aspect of performing highly non-linear analysis with geometric and material non-linearity was the selection of the solver type.For the current study, the FE mechanical analysis was done using Abaqus/an explicit solver, which was able to capture the non-linearities without convergence issues.The mass scaling was calibrated for each case, and the resulting dynamic effects were kept under acceptable limits to keep the problem quasi-static.The selection of the modelling parameters was based on the accuracy of results and computational economy, which led to finding the methodology capable of resolving the response of steel structures exposed to non-uniform temperature fields.

Conclusions
In this paper, the structural response of a long-span steel truss beam exposed to fire spreading scenarios was analysed using a coupled CFD-FEA methodology.CFD simulations were performed using FDS, the FE analyses were performed using Abaqus and a unidirectional coupling tool called FDS2FEM was used to transfer thermal boundary conditions between the two interfaces.
The coupling method was validated using experimental results from a steel beam subjected to a furnace fire and a steel column subjected to a localised fire with two different combinations of mechanical boundary conditions.The fire simulations predicted the temperature fields accurately in both the validation setups, and the thermal and mechanical responses obtained through FE analyses correlated with the test results well.The predicted mid-span displacements of the beam and the horizontal displacement of the steel column were within the limits of the experimental uncertainty.The experimentally observed deformation modes and local buckling were also captured by the simulation.Sensitivity analyses showed that, in order to capture the structural response, we need to resolve the temperature gradients across the section profile and also along the steel members.This requires sufficient resolution of the node-set partitions in both the fire model and the FE model.
The validated methodology was then used to study the response of a warehouse truss system exposed to two fire spread scenarios: one where the fire spread path was along the longer dimension of the compartment and perpendicular to the truss beams and another where fire spread occurred along the shorter compartment dimension and along the truss beam direction.Four phases of fire development were recognised: 1. local burning, 2. spread to the opening 3. burning at the opening and 4. backward travelling.The fire spread and temperature heterogeneity were mainly determined by the location of the ignition point with respect to the opening and the temporal variation in the position of flaming.Consequently, the steel temperature distributions along the truss beams were highly non-uniform.
Due to the different orientations of the truss beams with respect to the fire path within the warehouse, they were exposed to different heating scenarios and, according to the FE analyses, had different mechanical responses.The truss beam perpendicular to the fire path (Scenario 1) first experienced a local fire plume, followed by a semistationary hot layer.Lateral displacement at the mid-span was higher than the vertical displacement.The vertical displacement was below the span/20 limit despite the peak temperatures reaching as high as 1050 • C. The survival of this truss beam demonstrated efficient load redistribution within the truss system.In Scenario 2, the truss beam parallel to the fire path first experienced the local plume at one end, followed by the movement of the high temperature region towards the opening and then back.Greater temperature severity and coverage along the truss beam contributed to its overall failure in this scenario.The vertical displacement was greater than the lateral displacement, and the truss beam failed (according to the displacement limit criterion) after about half an hour when the fire was travelling back to the room.The response of the truss beams was, therefore, dependent on the two scenarios which posed different frame orientations with respect to the fire paths.Combined torsion and bending resulted in the lateral displacement at the mid-span to be higher than the vertical displacement.In both scenarios, the truss beams initially exhibited torsion due to the temperature difference with the bottom chord.Both scenarios also showed the change in the direction of the lateral displacement, suggesting that the heat exposure from spreading or travelling fires can lead to a deformation behaviour with an oscillating feature.
The results demonstrate that the proposed unidirectional coupling methodology can predict the response of large structures exposed to highly time-and space-dependent fire conditions.More work is needed to enable automated data transfer and the use of high-resolution data, that is, mapping surface data instead of point measurements.Expanding the current analysis to the entire construction would enable detailed building-level analysis, and recommendations can be made regarding the large-scale structural solutions.Finally, the thermal effects of fire suppression actions, such as automated sprinklers or fire brigade interventions, should be considered to build a complete understanding of the resilience of structures exposed to fires.

Declaration of Competing Interest
The authors declare that they have no known competing financial interests or personal relationships that could have appeared to influence the work reported in this paper.

Fig. 2 .
Fig. 2. Illustration of the differences between NSET-BNDF (top) and NSET-DEVC (bottom) mapping.The FDS model is shown on the left and the FE model on the right.

Fig. 6
Fig. 6 confirms the good agreement between the experimental and simulated steel beam temperature development.The peak temperature of the top flange was overpredicted in the simulation by 25 • C (6 %) and the rest of the temperatures were in good agreement with the test values.The overall temperature results of the simulation were within the limits of experimental uncertainty.The results of the FE simulation using the two FDS mesh resolutions are presented in Fig.6.Both the 2.5 cm and 10 cm grid size of FDS-produced temperature results were within the limits of experimental uncertainty during the FE simulation.Using the temperature history from the FE thermal analysis, the FE mechanical analysis was performed, and the deformation mode of the beam at the end of the analysis can be seen in Fig.7.The buckling of the lower flange was captured in the simulation, and the overall deformation of the beam was similar to the experiment.The trend of the mid-span displacement of the beam obtained from the FE mechanical analysis can be seen in Fig.8.The simulation results slightly underpredicted the mid-span displacement between 5 min and 13 min and then again from 16 min onwards.The simulated displacements were within 8 % of the test values using both the 10 cm and 2.5 cm mesh size of FDS.The axial force response at the support (Fig.9) was predicted within 10 % of the experimental value.Due to the presence of fire protection on the top flange of the beam, a non-uniform temperature distribution across the beam cross-section was obtained despite the uniform thermal environment of the furnace.As the beam started to lose its load-bearing capacity at elevated temperatures, the mid-span displacement increased rapidly, accompanied by the local buckling of the lower flange close to the support.The development of axial force demonstrates the magnitude of forces experienced by the supports, which is useful for the connection design.The current methodology was able to capture all these complex responses of the beam, which were compatible with the experimental values reported.

Fig. 5 .
Fig. 5. Boundary conditions for the FE mechanical analysis of the beam.

Fig. 6 .
Fig. 6.Comparison of the temperature recorded in the test with the results of the FE thermal analysis (TF: top flange; BF: bottom flange).

Fig. 7 .
Fig. 7. Deformed beam at the end of FE mechanical analysis and comparison with the buckling of the lower flange in the test (Unit of Mises stress is N⋅m −2 ).

Fig. 8 .
Fig. 8.Comparison of the mid-span displacement in the test with the results of the FE mechanical analysis.

Fig. 9 .
Fig. 9. Comparison of the axial force response at the support recorded in the test with the results of the FE mechanical analysis.

Fig. 11 .
Fig. 11.Simulation models of the exposed steel column validation test: the FDS model and meshing (left) and the partitioning and meshing of the FE model with mechanical boundary conditions (right).

Fig. 12 .
Fig. 12. Predicted adiabatic surface temperatures along the column during the FDS simulation of Case 1 at 26 min.

Fig. 13 .
Fig. 13.Comparison of simulated and measured steel temperatures at different heights of the exposed side of the column.The simulation results were calculated using different FDS cell sizes with (a) 10.0 cm partitions of the FE model and (b) 5.0 cm partitions of the FE model.

Fig. 14 .
Fig. 14.Comparison of the temperature recorded in the test (dotted lines) at various heights of the column with the results of FE thermal analysis (solid lines) for Case 1: (a) Fire-exposed surface and (b) back surface and Case 4: (c) Fire-exposed surface and (d) back surface.

Fig. 15 .
Fig. 15.Temperature ( • C) distribution in the column at a steady-state temperature condition using the FE thermal analysis for Case 1.

Fig. 16 .
Fig. 16.Comparison of the buckling observed in the test [26] with the FE mechanical analysis for Case 4 (Unit of Mises stress is N⋅m −2 ).

Fig. 17 .
Fig. 17.Comparison of the measured (dotted lines) and simulated (solid lines) horizontal displacements at different heights of the column for Case 1.

Fig. 18 .
Fig. 18.Comparison of the vertical displacement recorded at the column top in the test with the results of the FE mechanical analysis (using two strategies of horizontal constraints) for Case 4.

Fig. 19 .
Fig. 19.The model of the warehouse structure of the application (left) and the FDS model for Scenario 1 (middle) and Scenario 2 (right).The ignition locations and the fire paths in each scenario are also illustrated.

Fig. 20 .
Fig. 20.An FDS model of the truss beam showing the simplified diagonal elements.

Fig. 21 .
Fig. 21.An isometric illustration showing the cubical element as a part of the diagonal bracing in the FE model (left) and the cubical element used to represent the diagonal bracing in the FDS model (right).

Fig. 22 .
Fig. 22. Mesh discretisation of the FE model of the truss beam in the application example.

Scenario 1
was computed until 35 min and Scenario 2 until 43 min.The computations took about 10 and 12 days, respectively.

Fig. 23 .
Fig. 23.Dimension and partition of the selected truss beam in the application example.

Scenario 1 .
Between 14 min and 22 min, the fire spread beyond the initial region and towards the opening along the top of the fire load.The maximum temperatures of about 1300 • C were reached in the compartment during this time.At 24 min, simultaneous burning was observed in the initial fire region and at the opening.By 27 min, the fire load in the initial fire region was completely consumed and burning occurred exclusively at the opening.The fire started travelling back into the compartment by 28 min.The backward travelling phase was faster than in Scenario 1.

Fig. 26 .Fig. 27 .
Fig. 26.Comparison of the flame volumes in the two fire scenarios at 25 min from the ignition.The longer side of the fire load distribution is exposed to the flames in Scenario 2.

Fig. 28 .
Fig. 28.The predicted velocity vectors, coloured by the v-velocity [m⋅s −1 ] along the centreline of the opening in Scenario 2.

Fig. 29 .
Fig. 29.The predicted surface temperature for truss beams 1, 3 and 6 along the bottom and top chord in Scenario 1.

Fig. 32 .
Fig. 32.Steel temperature along the span of truss beam 3 in Scenario 2 for different periods of simulation in (a) bottom chord (b) top chord.

Fig. 33 .
Fig. 33.Steel temperature ( • C) contours from the FE thermal analysis of (a) truss beam 1 of Scenario 1 at 20 min and (b) truss beam 3 of Scenario 2 at 25 min.

Fig. 34 .
Fig. 34.Lateral and vertical displacements at the mid-section of the truss beam bottom chord in Scenario 1 (left) and Scenario 2 (right).

Fig. 36 .
Fig. 36.Illustration of the flow direction at a height of 1.0 m from the floor during the fire development phases (left) and the backward spreading phase (right) in Scenario 1.

Table 1
Durations of fire stages (min) and resolution indicators in the two simulated fire scenarios.