DEGREE PROJECT, IN STEEL STRUCTURES, SECOND LEVEL
STOCKHOLM, SWEDEN 2015
Difficulties in FE-modelling of an
I-beam subjected to torsion, shear and
bending
Difficulties in FE-modelling of an I-beam
subjected to torsion, shear and bending
Miriam Alexandrou
June 2015
TRITA-BKN. Master thesis 464, KTH 2015
ISSN 1103-4297
©Miriam Alexandrou 2015
Royal institute of technology (KTH)
Department of Civil and Architectural engineering
Division of Structural design and Bridges
ABSTRACT
In this thesis six different models of IPE240 have been created in order to study their behavior under shear, bending and torsion. These models simulate IPE240 but differ in the boundary conditions, in the loading and the length of the beam and in some connections which connect certain elements. In this study the modeling and simulation of the steel member is executed in ABAQUS Finite Element
Analysis software with the creation of input files. When developing a model for the finite element
analysis a typical analysis process is followed. All the parameters that are required to perform the analysis are defined initially to geometry which is half the beam due to symmetry, and the material properties of each model are defined too. Then a mesh is generated for each model, the loads of each model are applied which are expressed as initial displacement. Subsequently, the boundary conditions for each model are defined and finally the model is submitted to the solver when the kind of analysis has been defined. Namely, the analysis which is performed in this thesis is static stress analysis. When the ABAQUS has run the models, the contour plots for the von Mises stresses for each model are studied. In these contour plots, a large concentration of stresses and problems which arise in each one of the models are notified. As it has been observed in all models, the beam yields at the flanges of the mid-span and collapses at the mid-span. Therefore, the failure at the mid-span is more critical than the failure at the support. Moreover, the beams are weak in bending due to the fact that they twist almost 60-90 degrees under a large initial displacement at the control node. Additionally, much localized failure and buckling occurred at the mid-span, and local concentrated stresses also occurred at the bottom flange at the support due to the boundary conditions details.
Thereafter, a verification of the results of the ABAQUS through the simple analytical hand calculations is performed. It is concluded that the error appearing in most selected points is small. However, in some points in the web of the mid-span the error is greater. Additionally, while comparing the load-displacement curves of the two different plastic behaviors, it is observed that the model with an elastic-plastic with a yielding plateau slope behavior has smaller maximum load resistance than the model with a true stress-strain curve with strain hardening behavior.
Finally, some errors and warning messages have occurred during the creation of the input files of the models and a way of solving them is suggested.
ACKNOWLEDGEMENTS
This work was carried out under the supervision of Bert Gunnar Norlin, University Lector at the KTH Royal Institute of Technology, School of Architecture and the Built Environment. I would like to express my deep gratitude to him for the help, expert instruction, guidance and support he has been providing throughout the project.
CONTENTS
ABSTRACT ... v
ACKNOWLEDGEMENTS ... vii
LIST OF FIGURES ... xi
LIST OF TABLES ... xii
LIST OF SYMBOLS ... xii
LIST OF ABBREVIATIONS ... xii
1. INTRODUCTION ... 1
1.1. Background ... 1
1.2. Scope of the study ... 1
2. LITERATURE REVIEW ... 3
2.1. Shear, bending and torsion ... 3
2.2. Stiffeners ... 5
2.3. Elastic and plastic behavior ... 5
2.4. FEM modeling ... 7
2.4.1. Shell, beam and truss elements ... 8
2.4.2. Multi-Point Constraints ... 9
3. FINITE ELEMENT MODEL DEVELOPMENT ... 11
3.1. Model definition and material properties... 11
3.2. Generated models ... 14
3.3. Mesh generation ... 16
3.4. Loading ... 17
3.5. Boundary conditions ... 19
3.5.1. Mid span ... 19
3.5.2. End of the beam ... 20
3.5.3. Load system ... 21
3.6. Elastic and plastic behavior ... 21
3.7. Analysis ... 22
4. HAND CALCULATION OF STRESSES IN THE CROSS SECTION ... 23
5.1. Problems that occurred in the finite element results ... 25 5.1.1. Model 1... 25 5.1.2. Model 2 ... 27 5.1.3. Model 3 ... 31 5.1.4. Model 4 ... 33 5.1.5. Model 5 ... 35
5.2. Validation of the finite element model ... 36
5.3. Comparison of two types of plastic behaviors ... 38
5.4. Problems and errors obtained during the generation of the input file ... 40
4. CONCLUSIONS ... 43
REFERENCES ... 45
APPENDIX A – HAND CALCULATION OF THE STRESSES IN THE CROSS SECTION ... 47
APPENDIX B – INPUT FILES FOR ALL MODELS ... 59
Model 1 ... 59 Model 2 ... 69 Model 3 ... 77 Model 4 ... 82 Model 5 ... 89 Model 6 ... 96
LIST OF FIGURES
Figure 2.1 Uniform and non-uniform torsion of an I-section member ... 4
Figure 2.2: Effect of cross-section on torsional behaviour1 ... 4
Figure 2.3 Stress-Strain diagram for steel ... 6
Figure 2.4 Elastic-plastic with a nominal yielding plateau slope... 7
Figure 2.5: True stress-strain curve with strain hardening3 ... 7
Figure 3.1 Configuration of the beam up to the symmetry line ... 11
Figure 3.2: Beam cross-section ... 11
Figure 3.3: Model 1 ... 14 Figure 3.4: Model 2 ... 14 Figure 3.5 Model 3 ... 15 Figure 3.6 Model 4 ... 15 Figure 3.7 Model 5 ... 15 Figure 3.8 Model 6 ... 15 Figure 3.9 Model 6 ... 15
Figure 3.10: Visualization of the load system for models 1 and 2 ... 17
Figure 3.11 Visualization of the load system for models 4 to 6 ... 17
Figure 3.12: The load system for models 1 and 2 ... 18
Figure 3.13: The load case of the beam ... 18
Figure 4.1: The selected points for the hand calculation ... 23
Figure 4.2: The corresponding section points 1 and 5 for ABAQUS ... 23
Figure 5.1: Von Mises stress distribution at the support – Model 1 ... 25
Figure 5.2: Von Mises stress distribution at the mid-span – Model 1... 26
Figure 5.3: Plastic strain distribution at the mid-span – Model 1 ... 26
Figure 5.4: Von Mises stress distribution at the support – ... 27
Figure 5.5: Von Mises stress distribution at the support – ... 28
Figure 5.6: Von Mises stress distribution at the support – ... 28
Figure 5.7: Shear stress distribution at the support – ... 29
Figure 5.8: Shear stress distribution at the support – ... 29
Figure 5.9: Shear stress distribution at the support – ... 29
Figure 5.10: Von Mises stress distribution – Model 2 – Boundary condition case 1 ... 30
Figure 5.11: Von Mises stress distribution – Model 2 – Boundary condition case 2 ... 30
Figure 5.12: Von Mises stress distribution – Model 2 – Boundary condition case 3 ... 30
Figure 5.13: Plastic strain distribution at the support – Model 2 ... 31
Figure 5.14: Plastic strain distribution at the mid-span – Model 2 ... 31
Figure 5.15: Von Mises stress distribution – Model 3 ... 32
Figure 5.16: Plastic strain distribution at the support – Model 3 ... 32
Figure 5.17: Von Mises stress distribution – Model 4 ... 33
Figure 5.18: Von Mises stress distribution – Model 4 ... 34
Figure 5.19: Plastic strain distribution at the support – Model 4 ... 34
Figure 5.21: Von Mises stress distribution – Model 5 ... 35
Figure 5.22: Von Mises stress distribution – Model 5 ... 35
Figure 5.23: Load – displacement curve for the two plastic behaviors ... 39
LIST OF TABLES
Table 3.1 Data of the cross section ... 11Table 3.2: Yield strength and ultimate tensile strength of S355 steel... 12
Table 3.3: Material coefficients of steel ... 12
Table 3.4: SI Units ... 12
Table 3.5: Material properties of beam elements ... 13
Table 3.6: Applied initial displacement for model 1, 2 and 4 – 6 ... 19
Table 3.7: Applied initial displacement and rotation for model 3 ... 19
Table 3.8: Boundary conditions at the end of the beam for models 1 and 2 ... 20
Table 3.9: Boundary conditions at the end of the beam for models 3 to 6 ... 20
Table 3.10: True stress-strain curve with strain hardening ... 21
Table 3.11: Elastic-plastic with a nominal yielding plateau slope ... 21
Table 4.1: The selected points for the hand calculation and the corresponding nodes in ABAQUS . 24 Table 5.1: Total axial stress of the selected nodes ... 36
Table 5.2: Total shear stress of the selected nodes ... 37
Table 5.3: Angle of twist of the nodes at the symmetry line ... 37
LIST OF SYMBOLS
ε = Strain
h = Depth of the cross-section
b = Width of the cross-section
tw = Thickness of the web
tf = Thickness of the flanges
r = Root radius
A = Area of the cross-section
hi = Clear height between the flanges
Iy = Moment of inertia around y-axis
Wel,y = Elastic section modulus around y-axis
Wpl,y = Plastic section modulus around y-axis
Iz = Moment of inertia around z-axis
Wel,z = Elastic section modulus around z-axis
Wpl,z = Plastic section modulus around z-axis
LIST OF ABBREVIATIONS
FEM = Finite Element Method
FEA = Finite Element Analysis
CPU TIME = Central Processing time
1.
INTRODUCTION
1.1. Background
Steel buildings first gained popularity in the early 20th century. Their use became more widespread in the 50’s when steel became more available. Since then steel has become the dominating material for the construction of buildings and bridges. The less costly production process gave birth to modern structural steel building industry and to the construction of the world’s first skyscrapers. The range of use of steel has expanded with improved materials, products and design capabilities with the availability of computer aided design software. Nowadays structural steel is used to build high quality, sustainable structures such as multi-storey office buildings, industrial buildings, residential or leisure buildings and bridges. Steel has numerous advantages namely high strength, uniformity, and elasticity. Considering the abovementioned potentials of steel structures, it is useful to investigate structural steel behavior.
1.2. Scope of the study
The aim of this project is to study an open steel cross section (IPE240) which is subjected to shear, bending and torsion, and to investigate the problems which occur under this kind of loading. Several models of the I-beam will be created and studied in linear and non-linear analysis using ABAQUS
Finite Element Analysis software.
Thereafter, the outcome results of the stresses in the finite element linear analysis will be compared to the analytical hand calculation results of the cross section.
Finally, a load – displacement curve of two different plastic behaviors will be compared, namely: - An elastic-plastic with a nominal yielding plateau slope behavior (less accurate plastic
behavior).
2.
LITERATURE REVIEW
2.1. Shear, bending and torsion
In most cases, structural members are required to resist numerous kinds of loading. The combined loading causes several internal-force resultants on a section. Each kind of load produces stresses as if each load was acting separately. Then the total stress is found by adding the stress components which arise in the cross section.
It is known, that when a beam is loaded by transverse loads in their planes, the following two resultants occur in the beam: the shear force and the bending moment. The bending moment is a function of force and distance and also depends on the boundary conditions of the beam. The sign conventions for these internal forces and moments are related to the deformation of the member. Torsion is a consequence of direct actions (eccentric forces or moments) and indirect actions (applied torsion forces) acting on the cross section of the member. Therefore, when a member is subjected to torsion, it will twist about a longitudinal axis which passes through the shear center of the cross section.
If the section is loaded in such a way that the resultant force passes through the shear center of the cross section, the torsion will be eliminated. In many cases, the applied forces pass through the center of gravity. In addition, if the section is double symmetric then the torsion is eliminated because the center of gravity matches with the center of shear. Torsional effects may be influenced by many factors such as the boundary conditions of the beam, the load arrangement, the warping restrains and the cross section type (open or close cross section).
Generally in steel structures, torsion should be avoided as much as possible because it is not an appropriate method of resisting loads. When torsion cannot be avoided, a use of closed sections or box girders is suggested because they have an increased torsional resistance compared to the torsional resistance of the open sections. Briefly, closed sections are preferred when they are subjected to torsion.
However, there are cases when the resultant force does not pass through the shear center of the cross section, causing torsional loading in the cross section. Moreover, the cross section might be an open cross section which has decreased torsional resistance. Therefore, in this study, the case of varying torque (Figure 2.1, case b), combined with shear resultant in an open double symmetric cross section has been chosen for further analysis.
Figure 2.1 Uniform and non-uniform torsion of an I-section member1
In the case of non-uniform torsion the structural member is not free to warp, and the applied torque is resisted by St. Venant's torsional shear stress and warping torsion. Therefore, the non-uniform torsion consists of pure (St. Venant’s) torsion and warping (Vlasov) torsion. This can also be determined by calculating the torsion parameter K. When calculating the torsion parameter K, the kind of torsion can be distinguished as indicated below.
Figure 2.2: Effect of cross-section on torsional behaviour1
Consequently, as it is also mentioned in the Eurocode 3, EN 1993-1-1, the total torsional resistance TEd of a cross section is considered as the summation of two components:
- Pure, plane torsion or Saint Venant torsion, Tt,Ed (uniform) which causes twist and
- Warping torsion or Vlasov torsion, Tw,Ed (non – uniform)which causes warping.
In this study, the I-beam is subjected to stresses due to torsion, shear and due to bending. The kinds of stress components that occur and influence the resistance of cross sections are:
- Shear stresses τt,Ed due to Saint Venant torsion Tt,Ed
- Warping axial stresses σ w,Ed due to Bi-moment BEd
- Shear stresses τw,Ed due to warping torsion Tw,Ed
- Shear stress τv,Ed due to shear force VEd
- Bending axial stress σ m,Ed due to bending moment MEd
The abovementioned stress components are evaluated from an elastic analysis for open cross sections as described in section 4 “Hand Calculations of stresses in the cross section”.
2.2. Stiffeners
Stiffeners are usually required to control buckling effects from shear stresses in steel members. They are added to a slender girder to ensure that the web panel is able to develop its shear strength and shear buckling resistance. Even if stiffeners are not essential, they may still be provided if desired to increase the shear resistance of the web panel and decrease the local deformations due to the external loading.
There are two types of stiffeners: the longitudinal stiffeners which are placed along the span direction and the transverse stiffeners which are placed perpendicularly to the span direction of the beam. The latter, is categorized into bearing stiffeners and intermediate stiffeners. The bearing stiffeners are provided at the supports (above the reaction) or below the position of the concentrated loads while the intermediate stiffeners are provided at intervals along the web.
According to Eurocode 3, EN 1993-1-5, end stiffeners can be considered as rigid end post or flexible (non-rigid) end post stiffeners. A rigid end post is the case when more than one double-sided transverse stiffeners are placed as close to the support. A non-rigid end post may be a single double sided stiffener.
In this study, a flexible end post stiffener which may act as bearing stiffener resisting the reaction at the girder support has been chosen, reducing therefore large local deformations due to the external loading and preventing local failure. Moreover stiffeners have been used to provide more realistic conditions for the model.
2.3. Elastic and plastic behavior
This study is carried out with linear and non-linear analysis.
The linear analysis is used to calculate the stresses and deformations of the steel member. There are three basic assumptions that need to be valid: the steel member should be deformed with small rotations and displacements, the loading is constant during time and the Hooke’s law is valid (constant stress – strain relationship and the member’s stiffness never changes). In this linear range
the steel remains elastic and returns to its original shape on unloading. Moreover, it is not required to update anything in the FE-program while the model is deforming.
On the other hand, the non-linear analysis is a more complicated analysis and it is used to approach the real behavior of the steel member. If the basic assumptions of the linear analysis are invalid, the results are more accurate than the ones in the linear analysis. Having non-linear geometry means that the material has nonlinear behavior and therefore its stiffness changes during the deformation and needs to be updated while the model is deforming. This occurs when the deformations are large and cannot be neglected. Moreover, the plastic deformations at failure are larger than the elastic ones. This procedure increases the amount of time needed to get the accurate solution.
The plastic behavior of the beam was calculated according to the Swedish standard “Boverkets handbok om stålkonstruktioner, BSK 07” and the Eurocode 3, 1993-1-5: 2006, “Plated structural elements” as described below:
Figure 2.3 Stress-Strain diagram for steel2
= (1) = 0.02 + 50
−
(3)
= 0.025 − 5 (2) = 0.6 (4)
One case with realistic plastic behavior was studied in which the true stress-strain curve (Figure 2.5) was used whereas another case with less accurate plastic behavior was also studied in which an elastic-plastic with yielding plateau slope (Figure 2.4) was used. According to Eurocode 3, EN 1993-1-5, in the case with the realistic plastic behavior the true stress and strain should be calculated as follows:
= (1 + ) (5)
= (1 + ) (6)
These two cases were executed in order to be compared to each other.
Figure 2.4 Elastic-plastic with a nominal
yielding plateau slope3
Figure 2.5: True stress-strain curve with
strain hardening3
2.4. FEM modeling
Nowadays, the finite element method has become a great tool used by engineers worldwide in most fields of engineering. The FEA has many advantages. It can be used for solving many types of problems. There are no geometric, boundary conditions, loading and material properties restrictions. Additionally, components that have different behaviors and different mathematical descriptions can be combined. Therefore, the FEM is most suitable for increasing the success condition of this study. There are no other known existent experimental solutions to compare rather than the numerical solution that have been conducted in this study. Certain hand calculations of the stresses have been performed in order to verify the results of the FEA.
It is imperative that the FEA be recognized as simulation, not as reality. Moreover, the obtained output results from the FEA are only approximations. Namely, there is a difference between the finite element solution and the exact solution. The type of the model should be as complex as needed to obtain the required accuracy of the structure, but also as simple as possible to minimize the computational time.
In this study the modeling and simulation of the steel I-beam has been executed in ABAQUS Finite
Element Analysis software (ABAQUS/standard) in order to study its behavior under a specific loading.
2.4.1. Shell, beam and truss elements
The elements used in this study include ABAQUS’s shell, beam and truss elements, namely, S4 shell elements, B33 beam elements and T3D2 truss elements.
Shell elements are used to model structures which have one dimension (thickness) smaller than the other dimensions. Moreover, they are used to model structures in which the stresses in the thickness direction are negligible.
S4 type shell elements are 4-noded general-purpose, finite-membrane-strain, quadrilateral shell elements. These elements are conventional / displacement shell elements which discretize the reference surface, with full integration and linear interpolation.In case of full integration more CPU time is required than in the case of reduced integration.
In general, shell problems are included in one of two categories: thin shell problems (Kirchoff elements) and thick shell problems (Mindlin elements). In this case, S4 is included in the thick shell problems which assume that the shear deformation is important to the solution and therefore the shear deformations are built in the solution. In addition, S4 shell elements do not have hourglass modes neither in the membrane nor in the bending response of the element and therefore, the element does not require hourglass control.
The resultant displacements are calculated at the nodes and the resultant stresses are calculated at the integration points. At the location of the integrations points, there are section points through the thickness of the shell. When ABAQUS uses numerical integration to calculate the stresses and strains independently at each section point, it allows nonlinear material behavior. According to Simpson’s rule, five section points through the thickness of a shell can be used, which are adequate for most nonlinear design problems. Moreover, if Simpson’s rule is used, the section point 1 is exactly on the bottom surface of the shell and the section points through the thickness of the shell are numbered consecutively, starting with point 1.
Additionally, a shell element consists of the top surface (SPOS) which is the surface in the positive normal direction, the bottom surface (SNEG) which is the surface in the negative normal direction, and the mid-surface. The positive normal direction is defined by the connectivity of the shell elements and the positive and negative direction can be distinguished by plotting the normals in the model.
When defining the shell element section properties, the offset parameter in the input file was defined as zero which indicates that the reference surface is the mid-surface of the shell element.
Another element chosen for this study is truss elements. Truss elements are used to model long, slender structural members that can carry only tensile and compressive axial loads (loading only along the axis or the center line of the element) but cannot carry moments (moments or forces perpendicular to the centerline). They also have no initial stiffness to resist loading perpendicular to their axis.
T3D2 type truss elements are three dimensional, 2-noded truss elements with linear displacement. Due to the fact that the 2-noded truss elements have no bending resistance, they are useful for modelling pin-jointed frames. They are also suitable since they allow the model to move properly in torsion. Moreover, in order to define the section properties of the truss elements their cross-sectional area should be defined. The cross-sectional area has been chosen to be large enough compared to the other dimensions of the model.
Finally, beam elements are also applied. Beam elements are used to model structures which have one dimension (length) greater than the other two dimensions of the cross section (slenderness assumption). Moreover, they are used to model structures in which the longitudinal stresses is of great importance.
B33 type beam elements are 3D elements and 2-noded cubic beam elements. The cubic interpolation functions indicate that the element has 3 integration points which makes them accurate for cases involving distributed loading along the beam. They are also beam-column elements which allow axial, bending, and torsional deformation.
In general, beam elements are included in one of two categories: Euler Bernoulli beam elements and Timoshenko beam elements. In this case, B33 is included in the Euler Bernoulli beam elements which neglect and do not allow the transverse shear deformation. Therefore, this type of elements are most effective for modeling slender beams.
In general, as previously mentioned, structural members are often subjected to torsional moments which (torsional moments) also produce warping in the cross-section. The torsional response of beams depends on the shape of their cross-section. The effects of torsion and warping are considered in ABAQUS only in the three-dimensional elements and the warping calculation of warping assumes that the warping displacements are small.
2.4.2. Multi-Point Constraints
Using multi-point constraints is an efficient way to connect the elements between them and to impose constraints between different degrees of freedom of the model.
The MPC types that are used in the models are: MPC Linear for mesh refinement and MPC Beam, MPC Tie, MPC Link and MPC Pin for connections and joints.
The MPC type Linear is used when a mesh refinement of first-order elements is needed. It can be applied to all active degrees of freedom at the involved nodes.
The MPC type Beam provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node. It can also be applied at node sets. The two nodes or node sets should be at a distance between them.
The MPC type Link is used keep the distance between the two nodes constant and to provide a pinned rigid link between two nodes. The displacements of the first node are adjusted to impose this constraint and the existing rotations at the nodes are not involved in this constraint.
The MPC type Pin is used to make the global displacements equal between two nodes but leaves the
existing rotations independent of each other and to provide pinned joint between two nodes. It can
also be applied at node sets. The two nodes or node sets should be at the same position in the model.
The MPC type Tie is used to make all the common active degrees of freedom, global displacements and rotations of the two nodes equal. It can also be applied at node sets. The two nodes or node sets should be at the same position in the model.
3.
FINITE ELEMENT MODEL DEVELOPMENT
In this study the modeling and simulation of the steel I-beam has been executed in ABAQUS Finite
Element Analysis software (ABAQUS/standard) in order to study its behavior under a specific loading.
When developing a model for the finite element analysis (FEA), a typical analysis process is followed. The finite element models were initially generated by creating input files as seen in Appendix B.
The first step of the analysis refers to the classification and identification of the steel beam that is analyzed. All the parameters that influence the results, the most important physical phenomena involved, the results sought from analysis and the required accuracy have been questioned. The answers tothese questions have influenced the amount of information that has been collected to implement the analysis and the method that the problem has been modeled.
3.1. Model definition and material properties
The model is an IPE240 steel beam which is subjected to an eccentric loading that is causing torsion, shear force and bending on the beam as shown in the Figure 3.1 and Figure 3.2.
Figure 3.1 Configuration of the beam up to the symmetry line
Figure 3.2: Beam cross-section The material and cross-section definitions related to the steel sections were defined in the model. Specifically, the cross-sectional data of the IPE240 steel beam are shown in the following table:
Table 3.1 Data of the cross section
h (mm) 240 Iy (cm4) 3892 b (mm) 120 Wel,y (cm3) 324.3 tw (mm) 6.2 Wpl,y (cm3) 366.6 tf (mm) 9.8 Iz (cm4) 283.6 r (mm) 15 Wel,z (cm3) 47.27 A (cm2) 39.12 Wpl,z (cm3) 73.92 hi (mm) 220.4
The double symmetric section is made of structural steel of quality S355. The nominal values of yield strength fy and ultimate tensile strength fu for this steel grade are shown at Table 3.2. Therefore, the
cross section belongs to class 1 with respect to bending and to class 2 with respect to compression. Table 3.2: Yield strength and ultimate tensile strength of S355 steel
fy fu
S355 355 MPa 510 MPa
The material coefficients for the steel are shown in the following table. Table 3.3: Material coefficients of steel
Modulus of elasticity E 210 GPa
Shear modulus G 81 GPa
Poisson’s ratio in elastic range ν 0.3
Density ρ 7800 kg/m3
ABAQUS has no built-in system of units. Therefore, it is important to define all the input data in consistent units. The SI system of units is used throughout this project as shown in the following table. Table 3.4: SI Units Quantity SI units Length m Force N Mass kg Time s Stress Pa (N/m2) Energy J Density Kg/m3
The geometry and the loads of the model are symmetric and therefore the created model is symmetric too. Consequently, the model has been divided to enable working with symmetric section instead of working with the entire model. By modeling only the symmetric section, the number of elements in the model and the CPU time are reduced.
For models 1 and 2, as presented in section 3.2 “Generated models”, the span length up to the symmetry is 2.88 m and therefore the total length of the beam is 5.76 m. For models 3 – 6, the span length up to the symmetry is 0.72 m and therefore the total length of the beam is 1.44 m.
The material properties of each element type are described below:
The thickness of the S4 type shell elements is equal to the thickness of the flanges, the web and the stiffeners according to the relevant region. An offset equal to zero and Simpson’s rule with five integration points through the shell section were used as described in section 2.4.1. “Shell, beam, and truss elements”.
The material properties of the B33 type beam element are presented in the following table where the values of the first data line in the input file are shown in Table 3.5. The values of the second data line in the input file are the default values.
Table 3.5: Material properties of beam elements
Area, A (m2) 0.003912
Moment of inertia for bending about the 1-axis, I11 (m4) 0.00003892
Moment of inertia for cross bending, I12 (m4) 0
Moment of inertia for bending about the 2-axis, I22 (m4) 0.00003892
Torsional constant, J(m4) 0.00001892
In model 6, where truss elements are used, the area was defined as 0.0025 m2.
Thereafter, a simplification of the physical geometry into a mathematical model (idealization) and then into a discrete model (discretization) has been done consecutively. In brief, the member has been divided – discretized into elements.
3.2. Generated models
As previously mentioned, the following models have been created to examine problems emerged when the beams are subjected to torsion, shear and bending.
The main features of each model are the following:
- Model 1 consists of three types of meshes, a load system and a stiffener at the end of the beam.
- Model 2 consists of three types of meshes, a load system and truss elements which substitute
the stiffener of model 1 at the end of the beam.
- Model 3 consists of one type of mesh, a stiffener at the end of the beam and a concentrated
force and torsional moment at mid-span.
- Model 4 consists of one type of mesh, a load system and a stiffener at the end of the beam.
- Model 5 consists of one type of mesh, a load system and stiffeners at both the end of the
beam and the mid-span.
- Model 6 consists of one type of mesh, a load system, stiffeners at both the end of the beam
and the mid-span and truss elements connecting all the nodes of the upper and bottom flange to the nodes.
More details about each models are described in the following sections.
Figure 3.5 Model 3 Figure 3.6 Model 4
Figure 3.7 Model 5
3.3. Mesh generation
A series of nodes and elements were used to represent the geometry. As mentioned previously, the elements that have been used for the I-beam and stiffeners in all models are shell elements without reduced integration (S4 type shell elements). A node and element sequence was generated in such a way that their numbering does not coincide with each other.
For models 1 and 2, the mesh size varies along the span (longitudinal direction) depending on the region. The mesh is divided into three sections along the beam. The area of interest at the support possessed the smallest element size with the larger element sizes appearing further from the support. Namely, the mesh of the first section at the support is fine, whereas the second section becomes coarser and the third one at the mid-span even coarser. This procedure is performed so as more accurate results are obtained at the support and the analysis-CPU time is reduced. The mesh in models 3 – 6 is the same as the finest mesh in models 1 and 2.
In all models, each element and the mesh in general should have a square shape. To achieve this, the following considerations for each direction have been taken into account:
The dimensions of the model
The number of nodes and elements in each row should be an integer
The increment in the node and element numbers in each row should be an integer The length of the element should be approximately the same
In order to achieve a successful mesh refinement, the numbering of the nodes in the z – direction should be an integer, even number and should be divided three times by two so that the mesh will be symmetric in z-axisandget a node in the middle of the flanges in the z – direction
The node numbering of the elements in the y – direction should be an integer and even number
The number of elements in the x – direction should be an integer and even number so that the evenly distributed load is created for the load system which will be explained later. When all the nodes and elements of the I-beam and stiffeners have been generated, the nodes which are situated at the top and bottom of the web along the span are connected to the corresponding nodes of the flange which are situated in middle of the flange along the span by using the MPC type Beam.
Similarly, the nodes of the perimeter of the stiffeners are connected to the corresponding nodes of the flange by using the MPC type Beam and to the web by using the MPC type Tie.
3.4. Loading
In this study, the loads that are acted on the beam are placed and simulated in the most efficient way so that they reach the desirable load case on the beam, as shown in Figure 3.13
The load for models 1, 2, 4 – 6 should be able to create shear and torsion diagrams of the beam which vary from zero value at the mid span to maximum value at the supports. This is done to achieve a more realistic simulation of the loading.
A load system which is applied at a distance from the neutral axis, consists of nodes which are placed at consequent intervals. This was created in order to generate the above kind of loading. The nodes are connected to each other with beam elements which are also connected to each other vertically, using multi-point constraints type PIN as shown in Figure 3.10 and Figure 3.11 . The lengths of each beam element are set in such a way that the reaction forces that are transferred to the nodes of each level are equal.
Figure 3.11 Visualization of the load system for models 4 to 6 Figure 3.10: Visualization of the load system for models 1 and 2
The above figure is used exclusively to visualize the load system. In fact, all the beam elements are at the same level as shown below.
Figure 3.12: The load system for models 1 and 2
Moreover, all nodes at the level 0 (Figure 3.10 and Figure 3.11) are connected to the middle nodes of the upper and bottom flange using multi-point constraints type LINK. In this way, there is no bending stiffness in the x-axis and therefore the model is free to warp. This occurs in models 1, 2, 4 and 5. It does not occur in model 6 where the connection of the middle nodes of the upper and bottom flange to the load system has been achieved by using truss elements instead.
The load is expressed as an initial displacement which is given at the control node 20003694 for models 1 and 2 and at the control node 20004550 for models 4 to 6. This initial displacement is defined by using the “direct” format of the boundary conditions, by specifying the y-direction in which the displacement is applied and by specifying the magnitude of the displacement. This is defined in the history data in the input file.
This way of expressing the load was chosen to be able to control the reaction forces which are transferred to the each one of the nodes of the load system.
Finally, an equal value of the reaction forces are transferred to the nodes at level 0. Because the intervals between these reaction forces are small, the reaction forces are considered as evenly distributed load which acts at a distance 0,31 m from the neutral axis as shown in the figure below.
On the other hand, the loads that are applied in model 3 are concentrated force and concentrated torsional moment around x-axis. These two loads are acting at node 10514. All the nodes of the upper and bottom flange and the nodes of the web are connected to the middle node of the web (node 10514) by using multi-point constraints type BEAM. This is done to restrain warping at mid-span.
Similarly, the loads are expressed as an initial displacement and rotation which are given at the control node 10514. The initial displacement and rotation are defined by using the “direct” format of the boundary conditions, by specifying their directions and magnitude. These are defined in the history data in the input file.
The magnitude of the initial displacements which are applied in each case are summarized in the following tables.
Table 3.6: Applied initial displacement for model 1, 2 and 4 – 6
Model Initial Displacement (m)
Elastic Analysis Plastic Analysis
1 0.3 0.5
2 0.3 0.5
4 0.3 0.5
5 0.3 0.6
6 0.3 0.6
Table 3.7: Applied initial displacement and rotation for model 3
Model Initial Displacement (m) Initial Rotation (rad)
3 0.3 0.2
3.5. Boundary conditions
Boundary conditions have also been applied to appropriate nodes throughout the analysis of each model. Various boundary condition cases have been applied in each model. Moreover, different boundary condition cases have been applied in the same model to study how its behavior varies under these cases.
3.5.1. Mid span
In all the nodes which are in the symmetry line, the constraints are given directly by using the named constraint XSYMM. This is valid for all models except model 3. XSYMM is defined as the symmetry constraint about a plane of constant x1. Namely, the displacement in x-direction, the rotation in
y-direction and the rotation in z-y-direction are zero (U1= UR2=UR3=0). These restraints provide such
conditions in the symmetry line that the strong axis rotation is allowed. Therefore the model is free
to move around x-axis, thus enabling torsion and bending.
3.5.2. End of the beam
In models 3 and 4, the node 4000002 is constrained in y and z-directions and the node 4000502 is constrained in z-direction. Similarly, these constraints provide such conditions that the strong axis rotation and therefore torsion and bending are allowed.
In model 1, two cases of boundary conditions have been studied. The first case is the same as the boundary conditions in models 3 and 4. In the second case nodes 4000002 and 4000502 are constrained in z-direction and nodes 2 – 8000502 of the bottom flange are constrained in y-direction. In model 2, three cases of boundary conditions have been studied. The first two cases are the same as the two boundary condition cases in model 1. In the third case node 4000002 is constrained in y-direction and node 4000502 and nodes 2000 – 18828 of the web are constrained in z-y-direction. In model 5 and 6, nodes 4000002 and 4000502 are constrained in z-direction and nodes 2 – 8000502 of the bottom flange are constrained in y-direction.
All the boundary conditions that are applied at the end of the beam, namely the degrees of freedom which are constrained are summarized in the following tables.
Table 3.8: Boundary conditions at the end of the beam for models 1 and 2
Model 1 Model 2
Case 1 Case 2 Case 1 Case 2 Case 3
Boundary conditions at the end of the
beam
Table 3.9: Boundary conditions at the end of the beam for models 3 to 6
Model 3 Model 4 Model 5 Model 6
Boundary conditions at the end of the
3.5.3. Load system
At least one node of each beam element in the load system is constrained at the rotation around x-axis in order to avoid the rotation of the beam elements and therefore not contribute to the deformation of the I-beam. This is valid to all models except model 3 which has concentrated force and concentrated torsional moment instead of the load system.
In models 1 and 2, control node 20003694 of the load system is constrained in x-direction in order to avoid the movement of the load system in x-direction and to allow the load system to move in the same way with the middle nodes of the upper flange and avoid instability.
In model 3, control node 10514 of web at the mid-span is constrained in x and z-directions and to rotations around y and z-directions.
In models 4 to 6, control node 20004550 of the load system is constrained in x-direction in order to avoid the movement of the load system in x-direction and to allow the load system to move in the same way with the middle nodes of the upper flange and avoid instability.
3.6. Elastic and plastic behavior
The following values of the plastic behavior, which are used in the input file, were calculated as described in section 2.3 “Elastic and plastic behavior”.
For models 1 to 6, a realistic behavior was used. The values used in the input file to describe this behavior are shown below:
Table 3.10: True stress-strain curve with strain hardening
Stress (MPa) Strain Plastic Strain
0 0 0
355.600 0 0
359.564 0.001689 0.011063
539.021 0.012775 0.052778
561.000 0.055345 0.092639
Model 6 was also studied in the case with less accurate plastic behavior. Similarly, the values that are used in the input file to describe this behavior are shown below:
Table 3.11: Elastic-plastic with a nominal yielding plateau slope
Stress (MPa) Strain Plastic Strain
0 0 0
355 0.00169 0
365 0.10000 0.09831
3.7. Analysis
After defining the abovementioned input data, the history data and the type of the analysis has been defined. Then, the model has been submitted to the analysis solver. A time step has been defined and the equilibrium equation system has been solved.
The finite element analysis that has been used is a static stress analysis, which is used for stable problems and when inertia effects can be neglected. It may include linear or nonlinear response. In general, in elastic analysis, the model has small deflections and no time step is required to be defined. In this case the solution can be calculated by solving a system of linear equations. In plastic analysis, ABAQUS/Standard uses Newton’s method to solve the nonlinear equilibrium equations. In this case the solution cannot be calculated as in the case of elastic analysis. However, the solution can be calculated by specifying the loading as a function of time and by using time increments to obtain thenonlinear response and the equilibrium solution in each increment.
Therefore, in all models, the geometry in the elastic analysis has been defined as linear and no time step has been defined. However, the geometry in the plastic analysis has been defined as non-linear and a time step has been specified. Namely, the initial time increment has been set to 0.01 and the time period of the step has been set to 1.0. The maximum number of increments in a step has been set to 300 so as not to limit the analysis and cause its termination. In addition to this, in model 6, the
4.
HAND CALCULATION OF STRESSES IN THE
CROSS SECTION
Simple analytical calculations and handbook formulas from an elastic analysis have been used to evaluate the stress components at specific points in the cross-section of the I–beam. The finite element results will be compared to these hand calculations so as to check the accuracy of the finite element results.
Specifically, the hand calculations have been executed for model 1. The model is considered as simply supported beam with distributed load along the span of the beam with an eccentricity from the neutral axis as shown in Figure 3.12 in section 3.4 “Loading”.
The method which was followed for the calculation of the stresses is described below:
The points 1 – 12 on the cross-section where the stresses are to be determined have been selected as shown in Figure 4.1. The stress resultant at the selected points of the cross section has been determined for each one of the reaction forces and moments which were caused by the external loading. The axial stresses have been calculated at the selected points at the mid-span of the beam and the shear stresses have been calculated at the selected points at a distance 0.24 m from the support. Then, all the stress components of each one of the selected points have been combined separately and therefore the total stress of the selected points has been calculated.
The hand calculations of the total stress of the selected points 1 – 12 are shown in Appendix A. The selected points at the cross-section of the hand calculations are equivalent to the section points 1
and 5 of some certain nodes at the cross-section of ABAQUS as shown inTable 4.1. It is essential
that while comparing the results between the hand calculations and ABAQUS, the selected points of the hand calculations should correspond to the proper section points of ABAQUS as shown in Figure 4.2.
Figure 4.1: The selected points for the hand calculation
Figure 4.2: The corresponding section points 1 and 5 for ABAQUS
Table 4.1: The selected points for the hand calculation and the corresponding nodes in ABAQUS
Selected points for the hand calculations
Corresponding nodes at mid-span
Corresponding nodes at 0.24 m from the support
1 and 2 6000886 6000534 3 and 4 2000886 2000534 5 and 6 14404 14052 7 and 8 7192 6840 9 and 10 6000386 6000034 11 and 12 2000386 2000034
The results from ABAQUS are the approximated values and the results from the hand calculations are the exact values. The error of these values is calculated as follows:
5.
RESULTS
AND DISCUSSION
5.1. Problems that occurred in the finite element results
The results of the six models analyzed using ABAQUS are presented in the following figures. The von Mises and the shear stress distributions were plotted. The contour plots of the finite element mesh of all models provide an overview of the distribution of the stresses. Moreover, an enlarged portion of the mesh of the models is discussed in this section.
The stresses at each point are calculated directly from the solution variables. The interpolation functions in a displacement based finite element analysis are used to obtain the strains from the nodal point displacements.
5.1.1. Model 1
A problem occurred in the elastic analysis of model 1 and in both boundary condition cases that were applied in the model. In Figure 5.1, the contour plot represents the stress distribution of the von Mises stresses at the negative surface of the shell element. An enlarged portion at the end of the beam has been studied.
The stress values obtained at the corners of the upper flange are too large compared to the stresses of the region area. Specifically, the red region shows that the total stresses are approximately 2186 MPa while the stresses in the middle of the flange are approximately 34.5 MPa. This also occurs in the bottom flange and it is visible when the stresses are plotted in the positive surface of the shell elements. This leads to a bending failure at the corners of both flanges, fact that should not have occurred and therefore these results were not the expected ones.
As presented in the figure below, the von Mises stress distribution at the mid-span is smaller than the one in the support which is reasonable because the reaction forces of the load system create shear and torsion diagrams of the beam which vary from zero value at the mid span to maximum value at the supports.
Figure 5.2: Von Mises stress distribution at the mid-span – Model 1
Moreover, in the plastic analysis, the initial displacement (0.5 m) which is applied at the control node of the load system causes yielding of the material at the mid-span but does not cause yielding at the support nor at the web panel, as shown in the figure below.
Comparing the results from the two boundary condition cases of the model it is observed that the stresses of the first case are slightly smaller than the stresses of the second case of the boundary conditions. In general, the results are similar to each other in both cases.
5.1.2. Model 2
In the elastic analysis of model 2, different results were obtained for the three different boundary condition cases that were applied in the model. Figure 5.4, Figure 5.5 and Figure 5.6, illustrate the contour plot of the von Mises stress distribution at the negative surface of the shell elements. The problem in these cases occurs at the corners of the web panel.
The first case of the boundary conditions produces too large stresses at the corners of the web compared to the stresses of the region area. Specifically, the red region shows that the total stresses are approximately 2063 MPa while the total stresses in the middle of the web are approximately 945.95 MPa. The stresses at the upper and bottom flange at the support in the same area are much smaller than the ones on the web.
Similar problem occurs in the third case of the boundary conditions where the total stress values obtained at the corners of the web are approximately 4486 MPa compared to the overall area of the support where the values of the total stresses vary between 0.314 MPa and 1122 MPa.
In the second case of the boundary conditions the large concentration of stresses at the bottom corner of the web has disappeared because all the nodes of the bottom flange are constrained in the y-direction, thus restraining warping of the bottom flange. On the other hand, the large concentration of stresses at the upper corner of the web still remains. The stresses at that point are approximately 1764 MPa. In addition, the stresses of the bottom flange are larger than the stresses of the upper flange.
Figure 5.4: Von Mises stress distribution at the support – Model 2 – Boundary condition case 1
Figure 5.5: Von Mises stress distribution at the support – Model 2 – Boundary condition case 2
Figure 5.6: Von Mises stress distribution at the support – Model 2 – Boundary condition case 3
Additionally, in all boundary condition cases the shear stresses of the web panel at the support area are too large compared to the region area. As shown in Figure 5.7 the shear stresses in the middle of the web vary from 386 MPa to 619 MPa. The shear stresses in case 2 (Figure 5.8) vary from 134 MPa to 535 MPa and the stresses in case 3 (Figure 5.9) vary from 432 MPa to 560 MPa.
Figure 5.7: Shear stress distribution at the support –
Model 2 – Boundary condition case 1
Figure 5.8: Shear stress distribution at the support –
Model 2 – Boundary condition case 2
Figure 5.9: Shear stress distribution at the support – Model 2 – Boundary condition case 3
The large stresses at the corners of the web and the large shear stresses at the web panel are caused by the boundary conditions and especially by the restrained degree of freedom 2 at the bottom flange which acts as if a force is applied upwards the support.
In the plastic analysis, the applied initial displacement causes a large torsional moment and a twisting of almost 90 degrees of the cross section at the mid-span as shown in Figure 5.10, Figure 5.11 and Figure 5.12. The magnitude of the initial displacement has been given the value of 0.5 m to cause yielding at the beam. Despite this, yielding appeared only in small areas in the flange at the mid-pan and in the web at the support as shown in Figure 5.13 and Figure 5.14.
Figure 5.10: Von Mises stress distribution – Model 2 – Boundary condition case 1
Figure 5.13: Plastic strain distribution at the
support – Model 2 Figure 5.14: Plastic strain distribution at the
mid-span – Model 2
In general, the stresses that occurred in models 1 and 2 are large. The study of these models has been done in order to observe how the behavior of the beam varies with different boundary conditions and support details.
The beam yields at the flanges of the mid-span and collapses at the mid-span. The resistance to bi-moment is larger than the shear resistance of the beam. Therefore, the mid-span area is more critical than the support area. Moreover, the beam is weak in bending due to the fact that a too long beam twists almost 90 degrees under a large initial displacement at the control node.
5.1.3. Model 3
Model 3 was created in order to eliminate the abovementioned problems at the support and the large torsion which occurs at mid-span of model 1 and 2. As previously mentioned, the beam in model 3 is shorter than the beams in model 1 and 2 and has a consecrated load and torsional moment acting at the middle node of the web at mid-span.
In the plastic analysis of model 3, the total stress distribution and the deformed shape, as shown in Figure 5.15, represents a realistic behavior of the beam when subjected to such loading. Constraining all the nodes of the flanges and the web at the symmetry line to the middle node of the web enables the beam to act as a rigid beam. Therefore, the cross-section remains constant during the deformation of the beam.
Even if the results are reasonable, there is a much localized failure at the mid-span. There is a combined failure due to the shear force, the bending moment and the warping of the beam. In addition to this, local buckling of the flanges and the web is occurred at the same region area.
The stresses at the mid-span are larger than the stresses at the support and the beam yields firstly at the mid-span. Local concentrated stresses also occurred at the bottom flange at the support due to the boundary conditions as shown in Figure 5.16.
Figure 5.15: Von Mises stress distribution – Model 3
5.1.4. Model 4
In order to avoid the local failure and buckling of the beam in model 3, the load system was applied in the same model instead of the concentrated load and torsional moment to enable a more even distribution of the load along the beam length.
In the plastic analysis of model 4, the total stress distribution of the von Mises stresses at the negative surface of the shell element are presented in Figure 5.17. It is observed that the large local buckling does not occur anymore, but the cross-section at mid-span does not remain constant. Namely, there is a local buckling at the upper flange at the mid-span and a bending of the web panel.
The applied initial displacement also causes a large torsional moment and a twisting of almost 60 degrees of the cross section at the mid-span as shown inFigure 5.18.
The stresses at the mid-span are larger than the stresses at the support and the beam. Local concentrated stresses also occurred at the bottom flange at the support due to the boundary conditions as shown in Figure 5.19 and Figure 5.20.
Figure 5.18: Von Mises stress distribution – Model 4
Figure 5.19: Plastic strain distribution at the support – Model 4
Figure 5.20: Plastic strain distribution at the support – Model 4
5.1.5. Model 5
In model 5, another stiffener was added to the mid span so that the cross section of the beam would remain constant during the deformation as shown in Figure 5.22. Figure 5.21, illustrates the deformed shape of the plastic analysis and the contour plot of the von Mises stress distribution at the negative surface of the shell elements.
Figure 5.21: Von Mises stress distribution – Model 5
Comparing models 4 and 5, it is observed that the stresses which occurred at the mid-span in model 5 are smaller than the stresses in model 4. Therefore, adding the stiffener to the mid-span the stresses decrease. Specifically, the total stress values obtained at the support in model 5 vary from 299 MPa to 358.7 MPa, whereas in model 4 they vary from 314 MPa to 390 MPa. Additionally, the total stress values obtained at the mid-span in model 5 are approximately 567 MPa whereas in model 4 they are approximately 618.8 MPa.
Moreover, a small local buckling appears at the upper flange.
Finally, in model 5 the stresses of the stiffener at the support are larger than the stresses of the stiffener at the mid-span.
5.2. Validation of the finite element model
The finite element results have been compared to the hand calculation results. The stresses which are extracted from ABAQUS are taken from .dat file. In order to limit the results which are given to the .dat file, node sets and element sets have been created which include the selected nodes and elements that the stresses are calculated. The stresses are calculated at the integration points of the elements. In order to get the stresses at the nodes, the stresses at the integration points are extrapolated at the nodes. The values of the total axial and shear stresses and the values of the angle of twist are presented in the following tables.
Table 5.1: Total axial stress of the selected nodes Selected
Nodes
Section Point
Total axial stress - ABAQUS value - S11
(MPa)
Total axial stress - Hand
Calculations value (MPa) Error (%)
6000886 5 -426.550 -439.441 2.933 6000886 1 -450.750 -427.719 5.385 2000886 5 121.800 152.359 20.057 2000886 1 171.320 164.082 4.411 6000386 5 451.010 427.719 5.445 6000386 1 425.690 439.441 3.129 2000386 5 -171.060 -164.082 4.253 2000386 1 -122.660 -152.359 19.493 14404 1 -95.157 -56.494 68.437 14404 5 -24.412 -56.494 56.788 7192 1 95.885 56.494 69.726 7192 5 25.140 56.494 55.500
Table 5.2: Total shear stress of the selected nodes Selected
Nodes
Section Point
Total shear stress - ABAQUS value - S12
(MPa)
Total shear stress - Hand
Calculations value (MPa) Error (%)
6000534 5 670.050 644.391 3.829 6000534 1 -635.250 -612.233 3.623 2000534 5 664.320 644.391 3.000 2000534 1 -641.170 -612.233 4.513 6000034 5 635.890 612.233 3.720 6000034 1 -670.100 -644.391 3.837 2000034 5 640.060 612.233 4.348 2000034 1 -664.370 -644.391 3.007 14052 1 370.300 417.241 12.676 14052 5 -414.940 -377.766 8.959 6840 1 371.190 417.241 12.406 6840 5 -414.340 -377.766 8.827
Table 5.3: Angle of twist of the nodes at the symmetry line Nodes at the
symmetry line
Angle of twist - ABAQUS value - UR1
(rad)
Angle of twist - Hand Calculations value (rad) Error (%) 386 1.428 1.494 4.410 886 1.428 1.494 4.410 4788 1.435 1.494 3.941 7192 1.440 1.494 3.607 9596 1.442 1.494 3.473 12000 1.442 1.494 3.473 14404 1.44 1.494 3.607 16808 1.435 1.494 3.941 2000386 1.428 1.494 4.410 2000886 1.428 1.494 4.410 4000386 1.429 1.494 4.343 4000886 1.429 1.494 4.343 6000386 1.428 1.494 4.410 6000886 1.428 1.494 4.410 8000386 1.428 1.494 4.410 8000886 1.428 1.494 4.410
Referring to axial stresses, it is observed that the error that occurs in most of nodes varies from 3 to 5 %. However, nodes 2000886 (section point 5) and 2000386 (section point 1) have relatively high rate of error which reaches approximately up to 20%. In addition, nodes 14404 and 7192 of the web in the mid-span have a very high rate of error which varies from 55-70 %.
This error may appear for the following reasons:
- The stresses in the web are influenced only by the axial bending stresses. Therefore, the problem is caused by the axial bending stresses either in the hand calculations or in ABAQUS. Consequently, the bending theory might not work properly.
- When the nodes of interest are located close to the line of the load at z-direction, the results of the stresses show a greater influence.
- The mesh at mid-span is the coarsest mesh in the model. If the finite element mesh is too
coarse, the equilibrium conditions are satisfied poorly and the errors in the stresses can be considerable, thus causing a discretization error.
- When linear static analysis, compatible meshes and full numerical integration are used, the error might be caused by the fact that the equilibrium equations are not locally satisfied everywhere.
- The boundary conditions might not have been simulated properly. At the boundaries of the
finite element model it can be observed how much calculated stresses deviate from known stresses.
- In order to minimize the global error in the model, the finite element method allows local
inaccuracies.
Referring to shear stresses, it is observed that the error that occurs in the nodes varies from 3 to 12.5%. Similarly, the error in the angle of twist that occurs in all nodes at the symmetry line varies from 3.5 to 4.5%. The error is relatively small and is within the acceptable limits.
In general, it is observed that in both axial and shear stresses, the nodes 14404 and 7192 of the web have the highest rates of error. Despite this, the finite element results of the rest of the nodes and the hand calculation results are in a good agreement. Therefore, this indicates that the finite element model reflects fairly accurately the real behavior of the structure.
5.3. Comparison of two types of plastic behaviors
In model 6, a load – displacement curve was plotted, showing the change in the reaction force at the y-direction acting on the control node 20004550. This is done in order to obtain extra information about model 6.
The graph has been plotted for two cases:
- When the model has an elastic-plastic with a nominal yielding plateau slope behavior (less accurate plastic behavior).
- When the model has a true stress-strain curve with strain hardening behavior (realistic behavior).
The comparison of the load-displacement curves related to the abovementioned plastic behaviors is displayed in the following graph.
Figure 5.23: Load – displacement curve for the two plastic behaviors
As observed in the graph, the two load-displacement curves have different max load resistance. Comparing the load capacity of the two load-displacement curves, it is observed that the model with the realistic plastic behavior has a higher maximum load resistance than the model with the less accurate plastic behavior. Specifically, the load capacity of the former is 362.29 kN and occurs when the displacement is 0.454 m. The load capacity of the latter is 85.95 kN and occurs when the displacement is 0.176 m.
It is interesting to note that both load-displacement relationships show linear elastic response at low reaction force values. This occurs when the reaction force extends from 0 to 25.40 kN. The behavior then becomes non-linear in which the beam exhibits material and geometric non-linearity and may cause the deformations to become very large. The magnitude of the deformations and the non-linear behavior depends on the elastic modulus E and the shear modulus G.
In the case of the realistic plastic behavior, there is a sharp increase of the reaction force between 0.427 m and 0.454 m reaching the first maximum value at 0.454 m. Thereafter, there is a slight fluctuation in the force values with a second maximum value of 364.06 kN, and then it drops quickly to 114.18 kN. Finally, the reaction force increases up to 259.88 kN and decreases again to 238.40 kN at the 0.6 m.
In the case of the less accurate plastic behavior, a more steady increase in the reaction force is observed. There is a first maximum force value, which is the load resistance as mentioned previously, and a second maximum force value of 171.73 kN at 0.531 m.
0.00 50.00 100.00 150.00 200.00 250.00 300.00 350.00 400.00 0.00 0.10 0.20 0.30 0.40 0.50 0.60 0.70 Reaction Force (kN) Displacement (m)
