Engineering methods in fire safety and structural design

Background

ETH Zurich is planning the full-scale renovation, over the next few years, of two historic buildings located directly in the city center: the machine laboratory (ML) and the district heating plant (FHK) (Figures 1 and 2).

Existing construction

Dating from 1933, the ML building takes the form of a fully welded steel construction. It is some 64 m long and is divided into six approx. 12 m bays. The approx. 11 m tall steel frames have a span of around 22 m and are designed as two-hinged frames, with hinged joints at the base points and rigid frame corners.

General procedure based on Eurocodes

With the introduction of the Eurocodes (as SN EN standards) in Switzerland, the fire resistance rating of elements and structures can be verified by means of general natural fire methods to SN EN 1991-1-2 (Eurocode 1) in conjunction with the advanced calculation models to SN EN 1993-1-2 (Eurocode 3). The steel structure is assessed on the basis of the requirements specified in Eurocodes [3-6], including the associated national application documents. These specify various approaches in relation to heat transfer conditions, temperature-dependent thermal and mechanical material properties as well as the load combinations from SN EN 1990 (Eurocode 0).

The flow chart in Figure 5 shows the three individual processes that make up the method, together with the input/output data and required process parameters.

The results comprise details of the thermal deformations and stress-strain distribution in the structure. Performance criteria for determining the fire resistance rating are defined on the basis of SN EN 1993-1-2 and other standards. Compliance with these is assessed by means of finite-element models:

• Global deformation of primary structural elements in combination with the performance criteria for elements subject to compressive and bending loads to SN EN 1363-1 (test standard for building elements) and 13501-2 (classification based on test results).
• Deformation speed in combination with the performance criteria for elements subject to compressive and bending loads to SN EN 1363-1 (test standard for building elements) and 13501-2 (classification based on test results).
• Plastic strains affecting element profiles and connections, ductile material failure at local peaks of fracture strain with fracture strains as limit tolerance analysis of load-bearing structure.

Temperature determination by natural fire simulation

Under the ETH Zurich's utilization concept, the following uses are planned for the ML:

• basic electronics workshop
• robotics laboratory
• mechanical workshops
• basic engineering workplaces
• exhibition and promotional spaces
• clearly defined laboratory activities subject to risk analysis

These uses served as the basis for determining the design fire in accordance with the requirements of SN EN 1991-1-2 and the described considerations. 

For a fire area of just under 1,000 m², the ultimately applied values for the maximum specific heat release rate, specific fire load and fire growth rate yielded a maximum heat release rate of approx. 250 MW. The pattern of heat release rate over time taken as the design fire can – given the same fire area, (maximum) specific heat release rate, fire load and fire growth rate – feed into the fire simulation model in two different ways. Two variants, for uniform and circular fire spread, were investigated for the ML at ETH Zurich. Variant R1 quickly leads to locally high temperatures which may, in turn, precipitate early local failure of the roof areas. Variant R2 results in a uniform and slower temperature rise. Fire modeling based on Variant R1 allows the definition of a fire location. In this case, the critical fire location was the frame column supporting the upper reinforced-concrete building.

In agreement with the fire department, due allowance was made in the fire simulation for the planned mechanical smoke and heat exhaust ventilation system (SHEVS) together with the projected replacement air supply. The CFD program "Fire Dynamics Simulator" (FDS) was used for the computational fire simulation-based verification. Figure 6 shows the ceiling with its large areas of glass blocks, the building envelope and the steel structure itself, and thus provides an overall impression of the fire simulation model.

Implemented fire perfomrance of the variants R1 and R2 compared to the design fire

Due to the prevailing ventilation conditions, the maximum heat release rate of over 250 MW in the design fire scenario is not fully achievable, even with the mechanical SHEVS in operation. Nor does the atmospheric oxygen supplied via the replacement air openings suffice, given a heat release rate of approx. 25 MW (roughly equivalent to five fully burning cars) between minute 25 and minute 30, to achieve the further increase in heat release rate shown in the design fire scenario. After a short drop to approx. 15 MW, the fire simulation model predicts a generally constant heat release rate of around 20 MW. As shown in Figure 7, this applies for both fire spread variants.

Structural analysis and procedure

The primary numerical model of the ML steel frame for the thermal and mechanical analysis was created with the FEM program ABAQUS. The use of 2D and 3D element types allowed precise modeling of the steel construction geometry. The temperature-dependent material properties of the historic steel were determined by the ETH Zurich Institute for Steel, Timber and Composite Structures, headed by Prof. Mario Fontana, from tensile tests on specimens taken from the steel construction. Precise modeling of a reinforced-concrete wall section spanning several stories, subject to a temperature-dependent crack model for the reinforced concrete, would have severely limited the numerical efficiency of the overall model. The supported section of the reinforced-concrete structure was thus created in ABAQUS using shell elements (concrete) and bar elements (reinforcement), without any allowance for crack behavior. The material properties for steel and concrete were set up in compliance with Eurocode 2 [7, 8]. To obtain results, for comparison purposes, on the loading and deformation behavior of the upper reinforced-concrete building and to investigate crack behavior, a second model was created in SOFiSTiK with the same geometry and validated material properties, based on the Eurocodes for reinforced concrete and steel. The boundary conditions for the two models were harmonized. The deformations determined by the two models were checked against each other for the applied load and temperature. The identified discrepancies were deemed insignificant. The advantage of this procedure lies in the conservative assumption for the stiffness of the supported reinforced-concrete element and exact results for the temperature distribution and stability failure of the frame columns. Numerically laborious computations were thus optimized by means of conservative simplifications. At the same time, the method delivered a precise engineering assessment of the structural behavior under fire action.

Modeling in ABAQUS

The numerical idealization of the steel frames involved the creation of an FEM model of a frame (Figure 9) connected to the adjoining frames by longitudinal girders in the roof area and at the top of the columns. Under the applied predefined boundary conditions, horizontal expansion of the girders in the longitudinal and deflection in the vertical direction were permissible. The deformation of the frame columns in the vertical direction had to be coordinated with the support conditions of the reinforced-concrete structure in order to conservatively account for the impact of thermally induced column restraint while efficiently modelling the buckling of the frame columns. As the mechanical analysis took account of geometric non-linearity, allowance was also made for factors affecting stability as well as localized buckling in elements. The material non-linearity of the steel was defined by tensile tests under thermal action. Contact conditions were also applied for the relevant element surfaces in order to avoid any theoretical penetration of building elements and achieve a physically accurate interaction of the detailed construction. The concrete elements of the supported building were modeled as 2D elements (concrete) and 1D elements (reinforcement) [9], with one section of the overall structural model represented as a mechanically active area. The hollow core slabs above the ML frame were assumed to have hinged connections to the edge beam, were not therefore subject to bending due to thermal expansion of the laboratory frame and were not modeled. As in the SOFiSTiK model, the reinforcement is as specified in the as-completed drawings.

ABAQUS model of the hall frame with supported building section

Modeling in SOFiSTiK

The finite-element model in SOFiSTiK likewise takes account of the material behavior for structural steel determined by the specimen tests. For a non-linear computation of deformation and cracking in the reinforced-concrete elements, the reinforcement applied in the model corresponds to the specifications of the as-completed drawings. As in ABAQUS, the SOFiSTiK model (Figure 10) is a partial model of a shed frame, with purlins, the stabilizing girder at the frame corner under the neighboring building and the two crane girders. All transverse elements were assigned suitable boundary conditions so as to allow simulation of the overall action of all frames in the longitudinal direction of the ML. As in the existing construction, the column bases are formed with hinged joints. The specially designed support below the neighboring reinforced-concrete building was modeled with rocking piers (hinged columns) such that the reinforced-concrete building and ML structure can move independently of each other in longitudinal direction. The reinforced-concrete structure of the teaching block, with reinforced-concrete edge beam and facade columns, was represented as a diaphragm in the plane of the facade spanning two laboratory bays.

Numerical model for mechanical analysis in SOFiSTiK

Both the reinforced-concrete elements and all steel sections were modeled in SOFiSTiK with layered shell elements. The analysis over the fire duration was geometrically and materially non-linear, with imperfections assumed. Allowance was made for the material non-linearity of the structural steel, as is standard, through the temperature-dependent stress/strain relationship with plastic redistribution. For the reinforced concrete, the temperature-dependent material law and redistribution due to crack initiation was applied.

Comparison of the two finite-element models

The applied time-dependent temperature distribution in the steel members of the ML frame was determined by thermal analysis using the ABAQUS model and transferred for the individual zones to the SOFiSTiK model. The action of the thermal strain on the reinforced-concrete structure brings about a deformation that was transferred to the reinforced-concrete geometry of the ABAQUS model. The fact that the two models were harmonized and the impact of non-linear factors was low made it possible to compare the results and thereby check the two models against each other. The ABAQUS model was used to assess the load-bearing and stability behavior of the steel frame for the various fire load cases. The SOFiSTiK model allowed evaluation of the cracks in the reinforced-concrete element induced by thermal strain from the steel frame as well as their relevance for the structural stability of the reinforced-concrete building.

Results

With the exception of localized areas, the thermal analysis for the variants R1 and R2 over the 120 min exposure period in the two fire scenarios does not yield any element temperatures exceeding 500 °C (Figure 11). The plastic strain development in the steel structure is accordingly low, reaching a maximum of 2.4 %. No stability failure of the frame columns occurs while, in fire scenario R2, the specially designed support is lifted by a maximum of 17 mm (Figure 12).

According to the results of the SOFiSTiK analysis, only local plastic areas with strains of less than 4 % occur in the steel construction. These lie significantly below the strain at yield point or the elongation at break. The analysis provides no evidence – nor even the slightest indication – of any global failure of the steel structure.

Thermal expansion of the steel construction in the critical fire scenario causes the reinforced-concrete structure of the neighboring building to be lifted by approx. 17 mm above the frame column. In relation to the (approx. 24 m) span of the edge beam across two bays of the ML building, this amounts to less than L/1,000. The reinforced-concrete structure exhibits adequate ductility to accommodate this deformation. The concrete compressive stresses and concrete reinforcement strains determined by the model lie in an uncritical range. The calculated theoretical average crack widths remain below approx. 1 mm. The thermal strain from the ML structure is therefore unlikely to induce any critical crack formation in the reinforced-concrete building.

Component temperatures from the relevant fire load of scenario R2

Development of the vertical deformation at the support stamp

Summary

A simulation method based on natural fire scenarios was adopted to verify adequate fire resistance to SN EN 1991-1-2 for the historic machine laboratory (ML) at ETH Zurich. Given the complex structural interactions between the ML and neighboring building, the mechanical analysis was performed with two different FEM programs for multi-physical computational tasks. The results show the ML building's steel structure, without any protective fire encasement, to exhibit adequate fire resistance.

Your contact person