Dilip Neupane
STRUCTURAL ANALYSIS TECHNIQUE OF SIMPLE STEEL STRUCTURES EXPOSED IN FIRE USING ABAQUS
Examiner(s): Professor Timo Björk
D. Sc. (Tech.) Zhongcheng Ma
LUT Mechanical Engineering Dilip Neupane
Structural analysis technique of simple steel structures exposed in fire using ABAQUS
Master’s thesis 2020
88 pages, 44 figures and 8 table Examiners: Professor Timo Bjork
D. Sc. (Tech.) Zhongcheng Ma
Keywords: Abaqus, thermal analysis, structural analysis, explicit dynamic, structural fire engineering
Fire safety in building design is a significant concern nowadays to ensure people's safety and decrease construction cost. For a structural analyst, understanding the structural fire behaviour is very important in building design phase. To do so, numerical analysis techniques such as the finite element method are used to solve the structure’s response when structures are exposed to the fire. This thesis work aimed to develop a thermal and structural analysis technique to simulate the fire test using Abaqus finite element software. Its main objectives are developing relevant analysis techniques and procedures to replicate the fire test virtually and validating and benchmarking the developed technique for three fire tests.
HAMK Tech Research Unit, Finland commissioned this thesis work. At first, temperature- dependent thermal and mechanical properties of construction material included steel and concrete were collected. Then, thermal and structural analysis procedure is developed.
Finally, structural analysis of simple steel structure exposed in the fire was simulated, and the response between Abaqus and fire test results were compared.
The overall conclusion from this thesis work was that Abaqus could predict the structural response of simple steel structure exposed in the fire with good agreement compared to measured results using beam and shell element model. It was observed that defining nonuniform temperature distribution in the beam section temperature point is difficult because only one temperature versus time curve can be defined. Similarly, it was observed that Abaqus could perform highly nonlinear structural analysis using Abaqus/Explicit dynamics procedure for structures exposed in the fire without convergence issue. Lastly, this thesis project work could be used as a guideline to perform structural fire analysis using Abaqus for simple steel structure exposed to fire.
of Applied Science as a part ongoing research project( FE-SFS project) with an aim to develop structural analysis technique of simple steel structures exposed in fire using Abaqus.
Firstly, I would like to express my deepest gratitude towards my supervisor Zhongcheng Ma (from HAMK Tech) for his continuous support, discussion, and guidance throughout the thesis process. Secondly, I would like to extend my great appreciation toward my thesis supervisor Timo Bjork (LUT University) to provide me constant support, valuable suggestion and feedback during the entire thesis process.
Finally, I would like to thank my beloved wife Ekta for her support and encouragement throughout this process; without her support, love and caring, this work would not be possible.
Dilip Neupane Dilip Neupane
Lappeenranta 1.12.2020
TABLE OF CONTENTS
ABSTRACT ... 1
ACKNOWLEDGEMENTS ... 2
TABLE OF CONTENTS ... 5
LIST OF SYMBOLS AND ABBREVIATIONS ... 7
1 INTRODUCTION ... 9
1.1 Background ... 9
1.2 Research goal and objectives ... 10
1.3 Scope ... 10
1.4 Thesis outline ... 11
2 LITERATURE ... 12
2.1 The Structural Fire Design ... 12
2.1.1 Fire behaviour model ... 13
2.1.2 Thermal response model: ... 14
2.1.3 Structural response model: ... 14
2.2 Structural fire analysis using FEM ... 15
2.2.1 Finite element method ... 15
2.2.2 Heat transfer analysis ... 17
2.2.3 Structural analysis ... 19
3 MATERIAL PROPERTIES AT ELEVATED TEMPERATURE ... 21
3.1 Thermal material properties ... 21
3.1.1 Steel ... 21
3.1.2 Concrete ... 23
3.1.3 Polyisocyanurate (PIR) ... 24
3.1.4 Intumescent coating IC ... 24
3.2 Mechanical properties ... 25
4 STRUCTURAL FIRE ANALYSIS TECHNIQUE USING ABAQUS ... 30
4.1 Material modelling technique ... 32
4.2 Heat transfer analysis technique ... 37
4.3 Structural analysis technique ... 40
5 SIMULATION, BENCHMARKING, AND VALIDATION OF SELECTED FIRE TEST ... 45
5.1 Case 1 Simple beam ... 45
5.1.2 Thermal analysis ... 46
5.1.3 Structural analysis ... 51
5.2 Case 2 Simple frame ... 55
5.2.1 Thermal analysis ... 56
5.2.2 Structural analysis ... 62
5.3 Case 3 Steel cladding system ... 69
5.3.1 Thermal analysis ... 69
5.4 Case 4 Restrained column ... 73
5.4.1 Structural analysis ... 73
6 STRUCTURAL FIRE ANALYSIS GUIDELINES USING ABAQUS ... 83
7 CONCLUSION AND FUTURE WORK ... 85
LIST OF REFERENCES ... 87
LIST OF SYMBOLS AND ABBREVIATIONS
List of symbols
density [kg/m3]
tg elevated gas temperature in ISO curve [°C]
, min
t t time in seconds [s], time in minute [min]
s, c
t t steel temperature, concrete temperature [°C]
, s, c
thermal conductivity, the thermal conductivity of steel, the thermal conductivity of concrete [W/mK]
, ,s c
c c c specific heat capacity, the specific heat capacity of steel, the specific heat capacity of concrete [J/kgK]
/
l l thermal elongation Q the internal heat q the rate of heat flow
k coefficient of thermal conductivity h convection heat transfer coefficient
temperature or surface temperature [°C]
temperature of the surrounding medium for convection and radiation [°C]
a elevated temperature for a stress-strain relationship [°C]
surf surface temperature for convection and radiation [°C]
the temperature of the surrounding medium for convection and radiation [°C]
, the Stefan-Boltzmann constant, the emissivity of the surface A the surface area where heat flow [m2]
Ax area normal to x-direction where heat flow [m2] , ,
t t t
C K F heat capacity matrix, conductivity matrix and thermal loading vector
θ θ , temperature derivative and unknown nodal temperature vector in thermal analysis
, , ,
M C K F mass matrix, damping matrix stiffness matrix and external loading vector
, ,
X X X acceleration, velocity, and displacement vector
a the stress at elevated temperature
, , , , ,
y p E
k k k reduction factor for effective yield strength, proportional limit and the slope of linear elastic range
,
fy the proportional limit at elevated temperature
,
fp the slope of linear elastic range at elevated temperature
,
Ea the slope of the linear elastic range at elevated temperature E the slope of the linear elastic range at room temperature
strain
, p
the strain at the proportional limit at elevated temperature
, y
the yield strain at elevated temperature
, t
the limiting strain for yield strength at elevated temperature
, u
the ultimate strain at elevated temperature
Abbreviations
FE-SFS FE analysis techniques for Structural Fire Safety FE finite element
FEM finite element methods FEA finite element analysis 2D/3D two/three dimensional DOF degree of freedom
CFD computational fluid dynamics CAD computer-assisted design PIR Polyisocyanurate
IC Intumescent coating MPC multiple point constraint
1 INTRODUCTION 1.1 Background
Fire is an accidental disaster that caused the collapse of many structures in the world.
Thousands of people die every year due to the building's structural failure, and billions of euro’s property are destroyed. Different fire disasters worldwide, such as the collapse of the World Trade Center (2001) in the United States and Windsor Tower fire (2005) in Madrid, remind us of those fire disasters. For a structural analyst, understanding the structural fire behaviour is very important in building design phase. Fire safety in building design is a major concern nowadays to ensure people's safety and decrease construction cost. To do so, numerical analysis techniques such as the finite element method are used to solve the structure’s response when structures are exposed in the fire.
In this thesis project, structural analysis technique for simple steel structures exposed in fire using Abaqus finite element software is developed. This thesis aims to develop a thermal analysis technique and structural analysis technique to simulate the fire test. The main objectives of this thesis are developing relevant analysis techniques and procedure to simulate the fire test; using the developed technique to replicate fire test virtually and comparing results predicted by Abaqus finite element software with measured results of those fire test to validated and benchmark the developed technique by this thesis work.
This thesis project work was done as part of the FE-SFS project (FE-SFS,2020) work commenced by HAMK Tech Research Center in HAMK University of Applied Science, Finland (HAMK Tech, 2020). FE-SFS project aims to provide knowledge and skill for using the performance-based method for structural fire safety design of steel structure in Finnish Design companies using two commercial software Abaqus and LS-DYNA.
In this thesis, four fire tests from the literature are selected as benchmark problems and are simulated using Abaqus finite element software. The results obtained from Abaqus temperature analysis and structural analysis are compared with fire test results taken from the four fire test results. The selected fire tests are simple beam direct exposure to fire by Cong et al. (2005), simple frame (concrete infilled steel column and topped steel beam in a simple frame) by Cook and Latham (1987), fire-protected steel members with claddings by
Malaska et al. (2018), and restrained column by Ali and O’Connor (2001). In case of fire test by Malaska et al. (2018), only thermal analysis is performed, and only structural analysis is performed for restrained column fire test by Ali and O’ Connor (2001).
1.2 Research goal and objectives
This thesis's primary goal is to develop a structural analysis technique of simple steel structures exposed to fire using commercial FE software Abaqus. The main objectives are developing relevant numerical analysis techniques for structural fire analysis, including procedures, parameter sensitivity analysis, benchmarking and validation of selected fire tests. Thermal and structural analyses are performed for selected fire tests. Further sub- objectives are summarized as follows.
• Understating structural fire analysis procedure and collecting thermal and mechanical material data for simulation.
• Develop a suitable technique for thermal and mechanical material modelling.
• Develop a suitable thermal analysis technique to simulate temperature distribution in the structure.
• Develop a suitable technique to input temperature history results from 2D thermal analysis to 3D structural analysis.
• Develop relevant structural analysis techniques to simulate fire tests, mainly using structural beam and shell elements.
• Simulate selected fire tests, perform sensitivity analysis, benchmark, and validation for selected fire tests.
• Give guidelines for thermal and structural simulation of simple steel structures exposed in a fire.
1.3 Scope
This thesis is used as guidelines to perform FEM simulation for structural fire safety design of steel buildings using Abaqus. The primary focus will be using beam and shell elements rather than solid elements during the selected fire tests simulation. In this thesis work, 2D thermal analyses are mainly simulated using shell elements, and the nodal temperature histories results are input as predefined temperature fields in structural analysis. Structural analysis is done using beam and shell elements using Abaqus/Explicit dynamic procedure;
however, Abaqus/Standard implicit method is also considered for simple frame benchmark
problem. Temperature histories are defined mainly as predefined temperature filed in beam section temperature points and nodes sets in shell elements.
1.4 Thesis outline
This thesis layout is divided into seven chapters. Following current introduction chapters, the thesis is divided into six remaining chapters summarized as follow.
Chapter two provide a literature review of the basic knowledge of structural fire design and finite element method. This chapter aims to introduce structural fire engineering design approached and using the finite element method for performance-based fire design. The chapter is further dived into structural fire design and Structural fire analysis using FEM section.
Chapter three provides the necessary information and equation needed to obtain thermal and structural material properties at elevated temperature. It provides thermal material modelling equation for steel and concrete at elevated temperature, mechanical material properties of steel at elevated temperature and thermal material properties for two other materials.
Chapter four introduces Abaqus finite element software and provides the necessary information about the material modelling technique to input material data from chapter three.
It also provides guidelines and techniques to perform heat transfer analysis and structural analysis. This chapter provides information about developed techniques to perform structural fire analysis using Abaqus.
Chapter five provides simulation, benchmarking, and validation of the developed technique for four selected fire tests. In this chapter, the complete simulation procedure and comparison of the results are explained for each fire test. This chapter contains four sections and, in each section, thermal analysis and structural analysis of each fire test and comparison of results, are explained in detail.
Chapter six provide a summary of guidelines developed by this thesis work, and finally, chapter seven concludes this thesis work.
2 LITERATURE
This chapter provides a basic knowledge of structure fire design and finite element methods.
The objective of this chapter is to introduce structural fire engineering design approaches and implementing finite element methods for heat transfer analysis and structural analysis for performance-based fire design.
2.1 The Structural Fire Design
The structural fire design is a design process to determine the performance of the structures exposed to fire (Fu, 2018). This design process can be obtained mainly using three approaches; modelling of fire behaviour on the structure, calculating thermal response of the structure when exposed in fire and calculating structural response of the structure with mechanical loading when exposed in the fire. The main goals for structural fire design are to ensure the life safety of all occupants inside building, firefighters and people in the proximity of the building. It should make sure that the occupants have enough time to escape from the building during the fire. Structural fire design codes like Eurocode will be implemented during the building design phase. To meet these safety requirement and legislation approval for building design, either prescriptive based design method or performance-based design method is used in the design codes. Prescriptive based design method a simple design method based on rules outlined in design codes, whereas performance-based method is an advanced method based on real behaviour of the fire and structure response. The performance-based design method required real behaviour of fire and structural response; therefore, these behaviours must be approximated using numerical simulations. Utilization of the finite element method for thermal and structural analysis and using advanced calculation model for fire behaviour is the key for performance-based design method (Institution of Structural, 2007).
The following figure 1 illustrates the three approaches of structural fire design. The arrow and number in figure 1 indicated each model's modelling procedure’s complexity, meaning number four is the most challenging procedure. In this thesis, the fire behaviour model was taken from the fire test and standard iso fire curve. Advanced heat transfer analysis and structures analysis for member or frame are carried out using FEM in the thermal and structural response models. This is the most complex method for the thermal and structural response model.
Figure 1 Structural fire design approaches (Institution of Structural, 2007).
2.1.1 Fire behaviour model
The first stage in structural fire design to estimate the realistic gas temperature over the structural member during the fire. This is the time-temperature curve shown in figure 2, which is used as input for the thermal response model. As explain by Buchanan & Abu (2017), there are two types of fire, pre-flashover and post-flashover fires. For structural fire design, usually post-flashover fire temperature is considered and can be presented by localized fire and fully developed fire as explained by Institution of Structural Engineer (2007) and as shown in figure 2 fire behaviour model. The realistic gas temperature from fire behaviour can be obtained from the standard fire test, natural fire model, zone model and computational fluid dynamic (CFD) model. The most accurate fire behaviour model is obtained using CFD fire models.
As there are several ways of obtaining the time-temperature curve, Eurocode 1 purposes three different time-temperature curves. The most historically used and used in this thesis is the standard temperature-time curve, also called the ISO curve. This ISO curve is given by
20 345log(8min 1)
tg = + t + (2.1)
where tg[°C] is the gas temperature and tmin[min] is the time. Figure 18(a) illustrates the ISO curve.
•Localised fire
•Plume models (1)
•Zonde models (2)
•CFD (3)
•Fully developed fire
•Standaard fire test curves (1)
•Time Equivalence (2)
•Zone model (3)
•CFD (4)
Fire behavior model
•Test data (1)
•Simple heat transfer model (2)
•Advanced Heat transfer model (3)
Thermal
response model
•Member behavior (1)•Frame behavior (2)
•Whole buidling behavior (3)
Strucutral response model
Increase in complexity
• (1)
• (2)
• (3)
• (4)
2.1.2 Thermal response model:
The second stage in structural fire design to predict the temperature distribution in the structural members during the fire. This can be obtained by heat transfer analysis. The transfer of heat in solids is governed by Fourier’s equation (2.3), and the transient solution must be considered to obtained temperature variation in structural members. When the structures have complex geometry, nonlinear boundary conditions, thermal contact, cavity radiation, and temperature-dependent materials properties; the solution of Fourier’s equation is nonlinear and should be done using numerical methods. The temperature distribution in the structural members is dependent on conduction, convection, and radiation mode of heat transfer on the member. These three modes of heat transfer are discussed in section 2.2.2.
After obtaining, time-temperature curves from the fire behaviour model, the time- temperature curve is used as temperature input for convection and radiation definition in the thermal response model. According to the structural fire design approach mention by Institution of Structural (2007), there are three ways of modelling the thermal response of the structure; test data, simple heat transfer models, and advanced heat transfer models. The detailed description of these methods can be found in the Institution of Structural Engineer (2007). In this thesis, an advanced heat transfer model are implemented. Advanced heat transfer model requires the use of the finite element method or finite difference method.
Temperature-dependent material models like thermal conductivity, specific heat, and thermal density are modelled in this approach. The finite element method discretized the structure member into a finite element and solved the structural member's nodal temperature distribution. The detailed heat transfer procedure and implementation of FEM on heat transfer analysis are discussed in section 2.2.2. Figure 19 shows an example of the thermal response of the beam section exposed to fire using Abaqus FEA.
2.1.3 Structural response model:
The final stage in structural fire design is to predict structural member's structural response during the fire. The structural response model can be modelled as one member or a frame, or a whole building, as shown in figure 1. A detailed description of these methods can be found in the Institution of Structural Engineer (2007). The structural fire analysis procedure is highly nonlinear analysis procedure due to high temperature-dependent material nonlinearly, possible contacts, and collapsing behaviour. Therefore, a numerical solution for
the transient equation of motion, defined in equation (2.5) is solved using explicit codes. The detailed structural analysis procedure and implementation of FEM are discussed in section 2.2.3. Figure 2 shows an example of the structural response of a portal frame during a fire.
(a) undefromed shape (b) deformed shape
Figure 2 Structural response of a portal frame partially exposed to ISO fire solved using Abaqus FEA.
2.2 Structural fire analysis using FEM
Structural fire analysis using finite element method required knowledge of the finite element method, heat transfer analysis, and structural analysis. The overview of finite element methods, heat transfer analysis procedure, and structural analysis procedure are discussed in brief in the section.
2.2.1 Finite element method
The finite element method (abbreviated as FEM or FEA) is a numerical technique for solving different engineering field problems. This numerical approach has become one of the dominant calculation methods for academics, designer, and engineer for different engineering application. Table 1 demonstrates the application of the finite element method in different engineering fields. In the finite element method, a real structure is discretized into the finite number of subdivisions called elements. Then, the system's static or dynamics equation is formed and finally, solve the unknown degree of freedom like displacement in static/dynamics analysis, the temperature in heat transfer analysis, etc. provided that the boundary conditions are satisfied. The detailed description of the finite element method and its procedure is provided by Bathe (2016) and Rao (2018).
Frame (red lines) exposed to fire.
Table 1 Summary of Application of FEM (Rao, 2018).
Field of study (structures)
Engineering applications examples (1= Equilibrium problems, 2= Eigenvalue problems and 3 = Propagation problems)
Civil engineering
1: Static structural analysis of different building components, for example, beam, truss, plates, and concrete structures.
2: Vibration analysis (natural frequency and modes shapes) and structure stability (Buckling) structures.
3: Response of structure under fire and other loads. Propagation of stress waves.
Aircraft
1: Static analysis of aircraft wings, rockets, spacecraft 2: Natural frequency and vibration of aircraft structures
3: Response of aircraft structures to random wind loads and its dynamics response
Mechanical engineering
1: Stress analysis of different mechanical components like gear, joints, pressure vessels, linkage
2: Natural frequency and vibration of mechanical structures
3: Crack and fracture problems with under dynamics loads and dynamics response.
Heat conduction
1: Steady-state temperature distribution in solid or gases 2: -
3: Transient heat flow in fire analysis, rocket nozzles, internal combustion engine, turbines, building structures)
The finite element solution process consists of a step-by-step procedure summarized as follows regarding thermal and structural analysis procedures.
1. Create a geometry (2D or 3D) of the structures, simplify the geometry, and apply symmetry condition whether possible.
2. Discretized (Meshing) the structures into finite elements.
3. Apply material properties definition, boundary conditions and forces. (e.g.
convection and radiation boundary conditions for thermal analysis and forces and support for structural analysis)
4. Solve the system of equation (heat transfer equation or structural dynamics equation) for unknown variables (temperature and displacement) at selected nodes and elements. Then finally, calculated other desired variables (stress, heat flux, strain, etc.).
5. Obtained desired results.
For real engineering problems, the finite element analysis is done using a computer because of its iterative process for solving a large degree of freedom. Basically, different free and
commercial FEM codes are available. Abaqus and Ls-Dyna are few examples of general- purpose commercial FEM codes used in fire engineering. All the FEM software’s have a similar procedure which is classified into pre-processing, solving and post-processing.
Pre-processing is the first step which includes defining the geometry of the structures, assigning material properties, section properties, contacts, interface, and boundary conditions of the real structures. Then, the structure is discretized nodes and elements. This step is done using computer-aided engineering CAD tools. The final output of this step is the input file for solving the system of equations. In the second step, the solution of the system of equation is obtained using different solver. For solving, there is mainly two technique, which is the implicit and explicit method. In structural fire analysis, the implicit method is used for thermal analysis and explicit method is used for structural analysis. The detailed discussion about the explicit method is given by the book “ An Explicit Finite Element Primer” authored by Jacobs and Goulding (Jacob & Goulding, 2002). The final output of the solving step is the results files. Finally, the last step is called post-processing, where the results are obtained and further processed.
(a) pre-processing
t + t = t
C θ K θ F
(b) solving
(c) post-processing Figure 3 general FE procedure using commercial FEM codes
2.2.2 Heat transfer analysis
Heat transfer can be simply defined by the exchange of thermal energy between the physical system. A heat transfer analysis simulates the temperature distribution in a structure exposed in the fire. The three modes of heat transfer in the fire are conduction, convection, and radiation. The process in which thermal energy is a transfer within the structures is called conduction, and the process in which thermal energy is transfer between the structure and
hot gas is called convection. Furthermore, the process in which thermal energy is exchanged between two surfaces following electromagnetic law is called radiation (Rao, 2018).
According to Rao (2018), the rate of heat flow by conduction, convection and radiation is given by
4 4
for conduction
( ) for convection
( ) for radiation
x
surf surf
kA x
q hA
A
= −
−
(2.2)
where is temperature, kis the coefficient of thermal conductivity of the material, Ax is the area normal to x-direction where heat flow, x is length parameter for conduction equation. Likewise, for convection equation, h is the heat transfer coefficient, A is the surface area where heat flow, surf surface temperature and is the surrounding medium temperature. Similarly, for radiation equation, is the Stefan-Boltzmann constant, is the emissivity of the surface and is absolute surrounding temperature.
The heat transfer from the fire into the structure's surface by a combination of radiation and convection is treated as a boundary condition, and heat transfer within the structure by conduction is governed by heat conduction equation (Franssen & Vila Real, 2015). 2D thermal analysis is considered in this thesis for solving temperature distribution in the steel section. The governing equation for two-dimensional nonlinear, transient heat conduction takes the following form (Franssen & Vila Real, 2015):
(
a) (
a) Q
a ac
x x x y t
+ + =
(2.3)where is the temperature, t is the time, a is the thermal conductivity, Q is the internal heat source, a is the unit mass of steel, and ca is heat specific heat of steel. The temperature field in the structure given by equation (2.2) must satisfy the following boundary conditions where are: prescribed temperatures of the boundary, specific heat flux of the boundary and heat transfer by convection and radiation on surfaces.
Derivation of finite element equation for heat conduction problem can be derived using a variational approach or Galerkin method (Rao, 2018). The derivation of these approaches is
behind the scope of this thesis. The overall finite element equation using both approaches lead to the following equation
t + t = t
C θ K θ F (2.4)
where Ctis the heat capacity matrix, Ktis the conductivity matrix, Ft is the thermal loading vector, and θis the temperature derivative with respect to time and θis the unknown nodal temperature. The detail derivation of equation 2.4 can be referred to Franssen & Vila Real (2015). The heat transfer finite element equation 2.4 can be steady-state or transient in nature. Since all three modes of heat transfer are present in structure exposed in the fire, the governing differential equation 2.4 becomes nonlinear due to temperature-dependent material properties and inclusion of radiation term. Hence, an iterative solution procedure must be employed for a solution involving radiation. Numerical methods such as backward difference algorithm should be used to solve the differential equation 2.4 to get the temperature distribution. The output of the thermal analysis is the temperature distribution in steel structure which will be used as temperature boundary conditions for structural analysis.
2.2.3 Structural analysis
A structural analysis simulates the response of structure when mechanical loading and fire are present in the structure. The main aim of structural analysis is to find the distribution of displacement and stress under the static or dynamics loading and boundary conditions. For every solution, the dynamic equation motion must be satisfied. Structural analysis can be static and dynamic. The displacement, velocity, acceleration, stress, strain, and loads are all time-dependent in dynamic analysis. In fire engineering, structure analysis predicts the possible time that the steel structure can resist the mechanical loading until it collapses. Due to the dynamic nature of fire temperature curve and nonlinearity, a nonlinear dynamic structural analysis must be considered for structural fire analysis. There are three primary sources of nonlinearity: geometric nonlinearity, material nonlinearity and contact nonlinearity. Geometric nonlinearity occurs when there large displacements in the structure, whereas material nonlinearity occurs due to plasticity beyond the linear-elastic material behaviour. Similarly, contact nonlinearity occurs when boundary conditions in the FE model change during the analysis.
Using the Lagrange equation or Hamilton’s principle state by Rao (2018) in section 8.3.2 of his book, the dynamic equation of motion of a structure can be derived. The derivation of these approaches and deriving a structural matrix for FE analysis are behind this thesis's scope. Thus, the finite element equilibrium equation of motion for the transient dynamics system is given by
+ + =
MX CX KX F (2.5)
where Mis the mass matrix, Cis the damping matrix, K is the stiffness matrix, Xis acceleration vector, Xis the velocity vector, Xis the displacement vector, and Fis the external loading vector. The solution of equation 2.5 can be solved using the implicit and explicit method. There is a trend of using explicit code in structure fire analysis due to the nonlinear material model, large deformation, and structure collapsing behaviour. Implicit and explicit method are approaches used in numerical analysis for solving time-dependent ordinary and partial differential equation.
3 MATERIAL PROPERTIES AT ELEVATED TEMPERATURE
Many civil engineering structures are made of steel and/or concrete materials. Structural steel members are coated with fire protection materials. To perform structural fire analysis, the temperature-dependent thermal and mechanical properties of these materials must be collected. This chapter collects material data from Eurocode for steel and concrete and material data for polyisocyanurate (PIR) and intumescent paint (IC) from different literature sources. The data obtained from this chapter are used to model material behaviour in Abaqus.
3.1 Thermal material properties
The most used thermal material properties in the thermal analysis are specific heat capacity, thermal conductivity, thermal elongation, and thermal density. The equation for obtaining thermal material data for steel and concrete are discussed in this chapter.
3.1.1 Steel
According to EN 1994-1-2, density [kg/m3] for steel is 7850 kg/m3 and independent of temperature. The specific heat capacity of steel cs[J/kgK] for structural steel can be defined by
6 3 3 2 3
2.22 10 1.69 10 7.73 10 425 600
13002
666 735
738 17820
545 90
0 731 0
650 12
7
00 20
60 35 900
s s s s
s s
s
s s
s
t t t t
t t c
r t
t
for for fo
or t
− − −
− + +
−
−
=
+
−
(3.1)
where ts[°C] is the steel temperature. Likewise, the thermal conductivity of steel s[W/mK]
is given by
54 3.33 10 2 20 800
27.3 800 1200
s s
s
s
t t
t for
= − − for
(3.2)
Similarly, the thermal elongation factor l l/ of steel is given by
4 5 8 2
3
3 5
2.416 10 1.2 10 0.4 10 20 750
/ 11 10 750 860
6.2 10 2 10 860 1200
s s s
s
s s
t t for t
l l for t
t for t
− − −
−
− −
− + +
=
− +
(3.3)
A graph figure for specific heat capacity, thermal conductivity, and thermal elongation with steel temperature is depicted in figure 4.
(a) specific heat (b) thermal elongation
(c) thermal conductivity
Figure 4 Specific heat, thermal elongation factor and thermal conductivity of steel at elevated temperature.
3.1.2 Concrete
There are two types of concrete thermal material data definition in Eurocode: normal weight concrete and lightweight concrete. According to EN 1994-1-2, density [kg/m3] for normal weight concrete is 2300 kg/m3 and for lightweight concrete is around 1600-2000 kg/m3. The density of concrete is assumed as independent of temperature. Likewise, the specific heat capacity of concrete cc[J/kgK] for normal weight concrete can be defined by
900 100
900 ( 100) 200
1000 ( 200) / 2 2 400
1100 1
20 100
00
0 200
4 0
c
c c
c
c c
c
t
t t
c
for for for
t o
t t
f r
+ −
= + −
(3.4)
where tc[°C] is the concrete temperature. For lightweight concrete, the heat capacity cc [J/kgK] is 840 [J/kgK] and is assumed as independent of temperature. The thermal conductivity of concrete c[W/mK] for both normal and lightweight concrete is given by
2
2
Normal weight concrete:
upper limit
2 0.2451( / 100) 0.0107( / 100) 20 1200 lower limit
1.36 0.1361( / 100) 0.0057( / 100) 20 1200 Light weight concrete:
1 ( / 1600) 20 800
0.5 8
c c c
c c c c
c c
c
t t for t
t t for t
t for t
for t
− +
= − +
−
00
(3.5)
where tc[°C] is the steel temperature. Thermal elongation factor of concrete l l/ for normal and lightweight concrete is given by
4 6 11 3
3
6
Normal weight concrete:
1.8 10 9.1 10 2.3 10 20 700
14 10 700 1200
/
Light weight concrete:
8 10 ( 20)
c c c
c
c
t t for t
for t
l l
t
− − −
−
−
− + +
=
−
(3.6)
3.1.3 Polyisocyanurate (PIR)
According to Foster (2014), density [kg/m3] and the specific heat capacity for polyisocyanurate is 40 kg/m3 and 1300 J/kgK, respectively. Both density and specific heat are assumed as independent to temperature. The temperature-dependent thermal conductivity for PIR core is based on Wand and Foster (2017) and Foster (2014) and summarized in table 2. The table data are taken from FE-SFS project annual report (Ma and Havula (2019)).
Table 2 Temperature-dependent thermal conductivity for polyisocyanurate (Ma and Havula (2019))
Thermal conductivity (W/mK) Temperature (°C)
0.031 20
0.039 100
0.039 200
0.065 300
0.083 400
0.104 500
0.130 600
0.162 700
0.199 800
0.242 900
0.293 1000
3.1.4 Intumescent coating IC
This is the fire protection material. The thermal properties of IC paint are based on Schauman et al. (2015), Staggs (2010), and Kraus et al. (2013).The density [kg/m3] for intumescent coating is 1300 kg/m3. The temperature-dependent thermal conductivity and specific heat IC paints are summarized in table 3. The table data are taken from FE-SFS project annual report (Ma and Havula (2019)).
Table 3 Temperature-dependent thermal conductivity and specific heat of IC paints (Ma and Havula (2019))
Thermal conductivity (W/mK)
Specific heat
(J/kgK) Temperature (°C)
0.45 1428.6 20
0.0375 1428.6 100
0.278 4285.7 200
0.0714 7857.1 300
0.0084 1857.1 400
0.0052 614.3 500
0.0081 510.7 600
0.0124 307.1 700
0.0164 200 800
0.0205 142.9 900
0.0253 142.9 1000
3.2 Mechanical properties
Mechanical properties of steel are only considered for structural analysis. The stress-strain relationship of carbon steel at elevated temperature are taken according to EN 1993-1-2. EN 1993-1-2 provide the definition of effective yield strength, proportional limit and slope of the linear elastic range based on the stress-strain relationship at elevated temperature. The effective yield strength is related to 2% of the strain limit (Lennon et al., 2006). The variation of the reduction factor with elevated temperature is illustrated in Table 4 and figure 5. The mathematical formulation of the stress-strain relationship is illustrated in figure 7 for the material model without strain hardening. Based on the mechanical material properties given in EN 1993-1-2 and using the mathematical formulation for the stress-strain relationship given in figure 6, the plasticity material data of steel at elevated temperature can be obtained.
Strain hardening model can be implemented for steel temperature below 400°C using the equation given in equation 3.7 and equation 3.8. Table 4 summarized the reduction factor taken from EN 1993-1-2 (Lennon et al., 2006).
Table 4 Reduction factor table for a stress-strain relationship at elevated temperature (Lennon et al., 2006).
Temperature (°C)
a
Effective yield strength
, , /
y y y
k = f f
Proportional limit
, , /
p p y
k = f f
The slope of linear elastic range
, , /
E a a
k =E E
20 1 1 1
100 1 1 1
200 1 0.807 0.9
300 1 0.613 0.8
400 1 0.42 0.7
500 0.78 0.36 0.6
600 0.47 0.18 0.31
700 0.23 0.075 0.13
800 0.11 0.05 0.09
900 0.06 0.0375 0.0675
1000 0.04 0.025 0.045
1100 0.02 0.0125 0.0225
1200 0 0 0
Figure 5 Reduction factor for effective yield strength, proportional limit and slope of linear elastic range at elevated temperature.
Figure 6 illustrates the stress-relations for steel at elevated temperature for the material model with strain hardening and without strain hardening.
(a) without strain hardening
(b) with strain hardening
Figure 6 The stress-strain relationship for steel with and without strain hardening at elevated temperatures.
Figure 7 Mathematical formulation of stress-strain relationship at elevated temperature (Lennon et al., 2006).
To include strain-hardening for steel temperature below 400°C, the following modified mathematical equation can be used in place of the equation shown in figure 7 (Lennon et al., 2006). The stress is given by.
, , , ,
, ,
50( ) 2 0.2 0.04
0.04 0.15
1 20( 0.15) 0.15 0.2
0 0.2
u y y u
u a
u
f f f f for
f for
f for
for
− + −
= − −
(3.7)
where fu, is the ultimate strength at elevated temperature, allowing for strain hardening and can be determined as defined in equation 3.8.
,
, ,
,
1.25 300
(2 0.0025 ) 300 400
400
y a
u y a a
y a
f for
f f for
f for
= −
(3.8)
The stress-strain relationship derived from EN 1993-1-2 gives the nominal stress-strain curve for elevated temperature. Thus, the nominal stress-strain curve must be converted into a true stress-strain curve for numerical simulation. An example of the stress-strain curve taken from Lennon et al. (2006) is depicted in figure 8.
Figure 8 An example of a stress-strain relationship at elevated temperature for S275 steel with strain hardening (Lennon et al., 2006)
4 STRUCTURAL FIRE ANALYSIS TECHNIQUE USING ABAQUS
Abaqus is a general-purpose FE software which has strong capabilities for solving linear and nonlinear problems. Abaqus was developed by Dassault systems and part of 3ds Simulia family. The solution to a general problem by Abaqus involves pre-processing, solving and post-processing steps, as shown in figure 9. Abaqus/CAE is a complete Abaqus environment which integrates modelling, analysis job management, and result evaluation in a single platform. For solving, Abaqus have two solvers: Abaqus/Standard, which is general-purpose solver based on implicit method whereas Abaqus/Explicit is an explicit dynamics solver based on the explicit method (Abaqus, 2011).
Figure 9 Abaqus FEA process
In structural fire analysis using Abaqus, Abaqus/Standard is used for thermal analysis and Abaqus/Explicit is used for structural analysis of the structure during this thesis project.
Abaqus/CAE can be used for preprocessing, postprocessing and job management for solving. Abaqus can be used in the keyword version where the input file is created by keyword definition and mesh from the third-party preprocessor. Similarly, another alternative is to use Abaqus/CAE where the input file is generated automatically.
Abaqus/CAE is used during this thesis project.
After obtaining temperature-curves from fire models, structural fire analysis consists of thermal analysis and structural analysis of the structure exposed to fire. These analyses can be performed using two methods which are sequentially uncoupled and fully coupled thermal-stress analysis. In the sequentially uncoupled thermal-stress analysis, first separate 2D-thermal analysis is performed for the member’s section, and then temperature histories are applied as predefined boundary conditions in structural analysis. This method is most
Preprocessing ( Modelling)
•Abaqus/CAE
•Input file
•Third-party preprocessor
Solving
•Abaqus/Standard (Implicit)
•Abaqus/Explicit
Postprocessing
•Abaqus/CAE
•Thid-party postprocessors
suitable for structural fire analysis. In the case of coupled thermal-stress analysis, both thermal and structural analysis are solved simultaneously.
There is no inherent set of unit’s systems in Abaqus (Abaqus, 2011). Therefore, the use of consistent units’ system must be followed when defining geometry, material data and loading conditions. Table 5 illustrates the consistent units system typically used for structural fire analysis. This system of units must be followed for thermal analysis and structural fire analysis because the temperature curve from fire model is in minutes and it is easy to use SI unit’s system for thermal analysis whereas SI (mm) unit’s system is suitable for structural analysis.
Table 5 Consistent units’ system in Abaqus
Quantity SI system SI (mm)
Length m mm
Force N N
Mass kg tonne (103 kg)
Stress Pa (N/m2) MPa (N/mm2)
Energy J mJ (10-3Jj)
Density kg/m3 tonne/mm3
Temperature K K
Heat flux W/m2 mW/mm2
Conductivity W/m K mW/mm K
Specific heat J/kg K mJ/tonne K
The degree of freedom in Abaqus are labelled with a number from 1 to 6 for three x-y-z translation direction and for three rotational directions about x-y-z, respectively. The temperature degree of freedom is generally labelled with number 11, but in case of shell element, the temperature degree of freedom is labelled with number 1x where x is temperature points in shell thickness. In Abaqus, total time is the total simulation time for thermal or structural analysis procedure and total time is subdivided into different step time which is the total time for each analysis step. This total time is the true time for transient dynamic analysis. The following figure 4 illustrates the degree of freedom system and time measure used in Abaqus.
Figure 10 Degree of freedom and time measure system in Abaqus (Abaqus, 2011).
This chapter provides the material modelling technique, heat transfer procedure and structural analysis procedure using Abaqus/Standard and Abaqus/Explicit.
4.1 Material modelling technique
The building structures are made of different material like steel and concrete. In structural fire analysis, the nonlinear material model should be used. Thermal and structural material properties are temperature-dependent. When structure exposed to fire, the material reach to plastic region and plasticity must be introduced in the material model. This section provides basic thermal and structural material modelling technique in Abaqus (Abaqus, 2011).
The thermal and mechanical material behaviour like density, thermal conductivity, specific heat, elasticity, and plasticity behaviour must be defined for simulation of temperature distribution and the structural response of the structure when exposed in the fire. The process of assigning different material properties to different materials in the input file is called material modelling for Abaqus. Abaqus provided a wide range of material definition suitable for different types of analysis. In Abaqus, material behaviour can be modelled using Abaqus material library keyword or using the user-defined material model. The keyword
*MATERIAL is used to defined Abaqus material model, and keyword *USER MATERIAL is used to define user-defined material. The basic material properties that should be defined for thermal analysis are density, specific heat, and thermal conductivity, whereas density, thermal expansion, elasticity, and plasticity data should be defined for structural analysis. In the following table 6, the material behaviour that falls under different categories is summarized (Abaqus, 2011).
Table 6 Material behaviour categories in Abaqus material definition (Abaqus, 2011).
Material behaviours
General Mechanical Thermal Electrical/Magnetic Other
Density Depvar Regularization User Material User-Defined Field User output variable
Elasticity Plasticity Damage Damping Expansion Viscosity
Conductivity Heat generation Latent heat Specific heat
Electrical Conductivity Dielectric
Piezoelectric
Magnetic Permeability
Acoustic Medium Mass Diffusion Pore fluid Gasket
Thermal material behaviour:
The specific heat per unit mass is defined by one single value or as a function of temperature.
Specific heat can be defined by using keyword *SPECIFIC HEAT or defining specific heat from thermal material behaviour section in Abaqus/CAE. Similarly, when heat flow by conduction, the thermal conductivity is defined by giving conductivity of the material. For simple isotropic conductivity, only one value of conductivity must be defined. For temperature-dependent conductivity, conductivity must be defined as a function of temperature. It can be defined by using keyword *CONDUCTIVITY or defining conductivity from thermal material behaviour section in Abaqus/CAE. The process of defining material behaviours for thermal analysis are presented in table 7.
Table 7 Material behaviour keyword definition technique for thermal analysis
Material behaviours Keyword definition procedure
Specific heat *MATERIAL, NAME=name
*SPECIFIC HEAT
n , n
c
Conductivity *MATERIAL, NAME=steel
*CONDUCTIVITY, TYPE=ISO
n , n
k
Mechanical material behaviours:
The material density is defined by one single value, i.e. density of the material. The density is considered independent to temperature and can be defined by keyword *DENSITY. The simple isotropic linear elastic material can be defined by Young’s modulus and the Poison’
ratio, and for temperature-dependent linear isotropic elasticity, Young’s modulus, and the Poison’s ratio is defined as a function of temperature. Figure 11 show the example of temperature-dependent isotropic elasticity. In this example case, six sets of values are used to specify Young’s modulus and the Poison’s ratio for six temperature values. For temperature outside the range defined by points 1 and 6, Abaqus assumes constant values for Eand v; for temperature between two points (example, 1-2), the linear approximation will be used. The dotted line on the figure represents the linear approximation used in Abaqus, whereas the continuous line represents the actual material behaviours. Therefore, it is always good to use many temperature points to capture actual material behaviours.
Figure 11 Temperature-dependent linear isotropic elasticity material definition example (Abaqus, 2011).
Simple elastic-plastic material can be defined by yield stress and equivalent plastic strain.
For a temperature-dependent elastic-plastic material definition, yield stress which is dependent on equivalent plastic strain and temperature must be defined. The curve of stress- strain should be true stress-strain. The first yield points correspond to zero plastic strain.
Figure 12 shows an example of the temperature-dependent elastic-plastic material model definition. In this example case, the Yield stress vs plastic strain is defined using four points for two temperature 1and 2.
Figure 12 Temperature-dependent isotropic plasticity material definition example (Abaqus, 2011).
The process of defining mechanical properties are presented in table 8.
Table 8 Material behaviour keyword definition technique for structural analysis
Material behaviours Keyword definition procedure
Density *MATERIAL, NAME=steel
*DENSITY
Linear isotropic elasticity *MATERIAL, NAME=steel
*ELASTIC, TYPE=ISOTROPIC ,
E v Temperature-dependent linear
isotropic elasticity
*MATERIAL, NAME=steel
*ELASTIC, TYPE=ISOTROPIC
1 , , 1 1
. . . . . . , ,
n n n
E v
E v
Temperature-dependent plasticity *MATERIAL, NAME=steel
*PLASTIC, TYPE=ISOTROPIC
01 01 1
11 11 1
02 02 2
12 12 2
, , , , , , , , . . . . . .
Thermal elongation *MATERIAL, NAME=steel
*EXPANSION, TYPE=ISOTROPIC
4.2 Heat transfer analysis technique
In structural fire engineering, the process of solving transient heat transfer processes when the structure is exposed in fire is referred to heat transfer procedure. In Abaqus, there are several heat transfer procedures that can be used in fire engineering based on the analysis technique that analyst wish to follow. Typically, an uncoupled heat transfer analysis is performed for structural steel member section, and the temperature distributions are mapped to structural analysis. The common procedure that is suitable for Abaqus in case of structural fire engineering is uncoupled heat transfer analysis and sequentially or fully coupled thermal stress analysis. When modelling the steel structure using beam and shell elements, the temperature distribution in steel member section can be simulated by pure 2D uncoupled heat transfer analysis only, and the temperature can be mapped to structural analysis in beam section temperature points and node sets for shell elements. The following figure 13 illustrates the heat transfer procedure in Abaqus.
Figure 13 Heat transfer procedure in Abaqus
Uncoupled heat transfer analysis procedure is used to model the solid body heat conduction where convection and radiation due to fire are modelled as boundary conditions. The cavity radiation can also be included in this type of analysis. This is complete nonlinear transient heat transfer analysis because of all three modes of heat transfer are included, and the
Preprocessing
•Input time-temperature curve from fire behavior model.
•Abaqus/CAE or input file for modelling the 2D cross-section
•Convectiona and radiation boudnary condition with reference fire temperture curve
•Third-party preprocessor (eg hypermesh)
Analysis
•Abaqus /Standard
•Abaqus/Explicit can be used somtime
•Transient heat transfer analysis using Abaqus/Standard for 2D temperature analysis
Postprocessing
•Visualization an post procesing of results using Abaqus/CAE
•Third-party postprocessor( eg hypermesh)
•Obtained nodal temperature for structural analysis
temperature-dependent material properties, as well as temperature-dependent convection and radiation boundary conditions, are always present in thermal response analysis.
To solve the transient heat transfer equation (2.4), Abaqus use the backward Euler method using implicit time integration and suitable time increment is defined such that the local courant number is always less than one for a stable solution. Automatic or fixed incrementation can be used for time incrementation. The detail about the courant number and stability of the solution can be found in Abaqus manual (Abaqus, 2011).
The general procedure for transient uncoupled thermal analysis for thermal response model is summarized as follow.
• The initial temperature of room temperature (20°C) is defined for all nodes;
otherwise, Abaqus assume zero by default.
• Time-temperature curve from fire response model is defined using amplitude curve using *AMPLITUDE keyword.
• Radiation and convection boundary conditions are defined using convective film condition and radiation conditions along with reference time-temperature curved defined by amplitude curve.
• Thermal loads such as concentrated heat fluxes and body fluxes can be defined if needed.
• Temperature-dependent material properties are modelled, as described in section 4.1.
• Heat transfer elements are defined for the mesh.
• The solution is obtained using a heat transfer procedure, and the nodal temperature distributions are obtained.
The keyword template for heat transfer is as follow.
HEADING
…..
Part definition
*PART, NAME=name_of_part
*NODE
Data lines to define node number and node location (x-y-z co-ordinates)
*ELEMENT, TYPE=type_of_element
Data lines to define element number and node number ...
Data line to define element node and elements sets, section properties, and material definition ...
*END PART
Assembly definition
*ASSEMBLY, NAME=name_of_assembly
Data line to define assembly of the structure, instances, nodes and elements sets, geometry and geometry sets (surface and lines), and so on.
*END ASSEMBLY
Data line to defined time-temperature curve from fire response model
*AMPLITUDE, NAME=name_of_fire_curve, TIME=total time Data line to define the time-temperature curve
Materials properties definition
*MATERIAL, NAME=name_of_material
*CONDUCTIVITY
data line to define temperature-dependent conductivity
*DENSITY
data line to define thermal density
*SPECIFIC HEAT
data line to define temperature-dependent specific heat
Defining physical constants
*PHYSICAL CONSTANTS, ABSOLUTE ZERO=VALUE, STEFAN BOLTZMANN=VALUE
Defining predefined fields
*INITIAL CONDITIONS, TYPE=TEMPERATURE Data line to define initial temperature
Defining nonlinear transient thermal analysis step
*STEP, NAME=FIRE, NLGEOM=NO, INC=VALUE
*HEAT TRANSFER, END=PERIOD, DELTMX=VALUE.
Data line to define simulation time and incrementation definition
Defining convection and radiation interactions
*SFILM, AMPLITUDE=name_of_fire_curve_amplitude Data line to define convection surface and film coefficient
*SRADIATE, AMPLITUDE= name_of_fire_curve_amplitude Data line to define radiation surface and emissivity
Defining output requests
*OUTPUT, FIELD
*NODE OUTPUT NT,
data line to define nodal temperature output Other output variables request here
*END STEP
