Nonlinear Static and Dynamic Analysis of Steel Structures with ...

Δθνικό Μεηζόβιο Πολσηετνείο 

Σρνιή Πνιηηηθώλ Μεραληθώλ 

Εξγαζηήξην Σηαηηθήο θαη Αληηζεηζκηθώλ Εξεπλώλ 

ΔΠΜΣ: Δνκνζηαηηθόο Σρεδηαζκόο θαη Αλάιπζε Καηαζθεπώλ 

Μη Γραμμική ΢ηαηική και Γσναμική Ανάλσζη Μεηαλλικών 

Καηαζκεσών με Λεπηομερή Προζομοιώμαηα Πεπεραζμένφν 

΢ηοιτείφν 

Αποζηόλης Α. Βράκας 

Επηβιέπσλ: Μ. Παπαδξαθάθεο, Καζεγεηήο ΕΜΠ 

Αζήνα, 2011

National Technical University of Athens 

School of Civil Engineering 

Institute of Structural Analysis and Antiseismic Research 

M.Sc.: Analysis and Design of Earthquake Resistant Structures (ADERS) 

Nonlinear Static and Dynamic Analysis of Steel Structures with 

Detailed Finite Element Models 

Apostolis A. Vrakas 

Supervisor: Professor Manolis Papadrakakis 

Athens, 2011


School of Civil Engineering 


M.Sc.: Analysis and Design of Earthquake Resistant Structures (ADERS) 

Nonlinear Static and Dynamic Analysis of Steel Structures with Detailed 

Finite Element Models 

postgraduate thesis 

by 

Apostolis A. Vrakas, Civil Engineer NTUA 

apostolis.vrakas@gmail.com 


© 2011 

i

Nonlinear Static and Dynamic Analysis of Steel Structures with Detailed 

Finite Element Models 

Apostolis A. Vrakas 




Zografou Campus, Athens 15780, Greece 


ABSTRACT 

The objective of this thesis is the nonlinear detailed finite element analysis of steel moment 

resisting frames with extended end-plate bolted beam-to-column joints. Firstly, the 

simulation of the joints is performed, using structural (beam and shell) and threedimensional 

continuum (eight-node hexahedral solid) elements. Material as well as 

geometric nonlinearities with contact between the appropriate components of the 

connections are taken into account. The moment-rotation (Μ-θ) response of characteristic 

joints, subjected to static loads, is calculated and compared with experimental results and 

EC3 predictions for the validation of the corresponding numerical models. 

Then, multistory steel frames are examined with detailed modeling of their joints via 

structural elements according to the above study, capturing all types of nonlinearities. 

Frame members are modeled either with shell (full simulation) or with beam-column 

elements combined with proper compatibility constraints at the interfaces with the joints 

(hybrid simulation) accounting for the excessive computational effort required to perform 

nonlinear analyses with detailed finite element models. Pushover static and implicit directintegration 

dynamic analyses taking into consideration P-delta effects are performed 

demonstrating the effect of joints on the overall response of the structure. El Centro 

earthquake horizontal accelerogram is considered for the seismic excitation. In order to 

study the influence of the joints end-plate and bolts, parametric analyses are performed 

demonstrating the effect of each component on the overall behavior of the frame. Finally, 

stiffening of the joints with supplementary web plates takes place in order to examine the 

influence of the panel zone deformations. 

The detailed finite element discretization of the joint and frame models is produced 

automatically from their corresponding geometric description via appropriate code that has 

been developed, while Abaqus/Standard software is used for the numerical analyses. 

iii

Μη Γραμμική ΢ηαηική και Γσναμική Ανάλσζη Μεηαλλικών 

Καηαζκεσών με Λεπηομερή Προζομοιώμαηα Πεπεραζμένφν ΢ηοιτείφν 

Αποζηόλης Α. Βράκας 

Δπιβλέπφν: Μ. Παπαδρακάκης, Καθηγηηής ΔΜΠ 

Εξγαζηήξην Σηαηηθήο θαη Αληηζεηζκηθώλ Εξεπλώλ 

Εζληθό Μεηζόβην Πνιπηερλείν 

Πνιπηερλεηνύπνιε Ζσγξάθνπ, Αζήλα 15780, Ειιάδα 


ΠΔΡΙΛΗΨΗ 

Σθνπόο απηήο ηεο εξγαζίαο είλαη ε κε γξακκηθή αλάιπζε κε ιεπηνκεξή πξνζνκνηώκαηα 

πεπεξαζκέλσλ ζηνηρείσλ κεηαζεηώλ κεηαιιηθώλ πιαηζίσλ απνηεινύκελσλ από 

θνριησηνύο θόκβνπο δνθνύ-ππνζηπιώκαηνο κε πξνεμέρνπζα κεησπηθή πιάθα. Αξρηθά, 

πξαγκαηνπνηείηαη πξνζνκνίσζε ησλ θόκβσλ: α) κε επηθαλεηαθά ζηνηρεία θειύθνπο ζε 

ζπλδπαζκό κε ξαβδσηά ζηνηρεία δνθνύ, θαη β) κε εμαεδξηθά-νθηαθνκβηθά ηξηζδηάζηαηα 

πεπεξαζκέλα ζηνηρεία. Λακβάλνληαη ππόςε ηόζν κε γξακκηθόηεηεο πιηθνύ όζν θαη 

γεσκεηξηθέο κε γξακκηθόηεηεο ζπκπεξηιακβαλνκέλσλ ησλ επαθώλ κεηαμύ ησλ δηαθόξσλ 

ζπζηαηηθώλ κεξώλ ησλ ζπλδέζεσλ. Υπνινγίδνληαη θακπύιεο ξνπήο-ζηξνθήο (Μ-θ) 

ραξαθηεξηζηηθώλ θόκβσλ ππνβαιιόκελσλ ζε ζηαηηθά θνξηία, θαη ζπγθξίλνληαη κε 

πεηξακαηηθά απνηειέζκαηα θαη πξνβιέςεηο ηνπ EC3 γηα ηελ απνηίκεζε ησλ δηαθόξσλ 

αξηζκεηηθώλ κνληέισλ. 

Αθνινπζεί ε αλάιπζε πνιπώξνθσλ κεηαιιηθώλ πιαηζίσλ κε ιεπηνκεξή πξνζνκνίσζε 

ησλ θόκβσλ ηνπο γηα ηελ εκθάληζε θάζε είδνπο κε γξακκηθήο ζπκπεξηθνξάο. Γηα ηα 

δνκηθά κέιε ρξεζηκνπνηνύληαη ηόζν πεπεξαζκέλα ζηνηρεία θειύθνπο (πιήξε κνληέια) 

όζν θαη ξαβδσηά ζηνηρεία δνθνύ-ππνζηπιώκαηνο κε ζεώξεζε θαηάιιεισλ θηλεκαηηθώλ 

εμαξηήζεσλ ζηηο δηεπηθάλεηεο (πβξηδηθά κνληέια) γηα ηελ αληηκεηώπηζε ηνπ κεγάινπ 

ππνινγηζηηθνύ θόζηνπο πνπ απαηηείηαη γηα ηελ πξαγκαηνπνίεζε κε γξακκηθώλ αλαιύζεσλ 

κε ιεπηνκεξή πξνζνκνηώκαηα πεπεξαζκέλσλ ζηνηρείσλ. Πξαγκαηνπνηνύληαη ηόζν κε 

γξακκηθέο ζηαηηθέο αλαιύζεηο ππό νξηδόληηα θνξηία (pushover) όζν θαη δπλακηθέο 

αλαιύζεηο ρξνλντζηνξίαο επηδεηθλύνληαο ηελ επηξξνή ησλ θόκβσλ ζηε ζπκπεξηθνξά ηνπ 

θνξέα. Ωο νξηδόληηα ζεηζκηθή δηέγεξζε ρξεζηκνπνηείηαη ν ζεηζκόο ηνπ El Centro. 

Πξαγκαηνπνηνύληαη παξακεηξηθέο αλαιύζεηο σο πξνο ηε κεησπηθή πιάθα θαη ηνπο θνριίεο 

κε ζθνπό λα θαλεί ε επηξξνή ησλ δηαθόξσλ ζπζηαηηθώλ κεξώλ ησλ θόκβσλ ζηελ 

θαζνιηθή απόθξηζε ηνπ θνξέα. Τέινο, εμεηάδεηαη ε επίδξαζε ηεο δηάηκεζεο ζηνλ θνξκό 

ηνπ ππνζηπιώκαηνο κέζσ ελίζρπζεο ηνπ κε πξόζζεηα ειάζκαηα. 

Η δηαθξηηνπνίεζε ησλ θόκβσλ θαη ησλ πιαηζίσλ ζε πεπεξαζκέλα ζηνηρεία γίλεηαη κέζσ 

θαηάιιεινπ ινγηζκηθνύ πνπ αλαπηύρζεθε. Γηα ηηο αξηζκεηηθέο αλαιύζεηο ρξεζηκνπνηείηαη 

ην Abaqus/Standard. 

v

CONTENTS 

Abstract .................................................................................................................... iii 

Περίληυη .................................................................................................................... v 

Contents .................................................................................................................... vii 

Chapter 1 Design of Steel Structures with Eurocode 3 ................................ 1 

1.1 Materials .................................................................................................................... 1 

1.2 Classification of cross sections ................................................................................ 2 

1.3 Finite element methods of analysis .................................................................... 4 

1.3.1 General ........................................................................................................ 4 

1.3.2 Modeling ........................................................................................................ 5 

1.3.3 Use of imperfections ................................................................................ 5 

1.3.4 Material properties ................................................................................ 7 

1.3.5 Loads, limit state criteria and partial factors ............................................ 8 

1.4 Design of joints ........................................................................................................ 8 

1.4.1 Introduction ............................................................................................ 8 

1.4.2 Connections made with bolts .................................................................... 10 

1.4.3 Categories of bolted connections .................................................................... 10 

1.4.4 Positioning of holes for bolts and rivets ........................................................ 11 

1.4.5 Design resistance of individual fasteners ........................................................ 13 

1.4.6 Analysis of joints ............................................................................................ 15 

1.4.7 Classification of joints ................................................................................ 17 

1.4.8 Modeling of beam-to-column joints ........................................................ 18 

1.4.9 Design moment-rotation characteristic ........................................................ 21 

1.4.10 Basic components of a joint .................................................................... 21 

Chapter 2 Finite Element Modeling with ABAQUS/Standard .................... 25 

2.1 Solid (continuum) elements ................................................................................ 25 

2.1.1 Choosing between first- and second-order elements ................................ 25 

2.1.2 Choosing between full- and reduced-integration elements ................................ 26 

2.1.3 Choosing between bricks/quadrilaterals and tetrahedra/triangles .................... 27 

2.1.4 Choosing between regular and hybrid elements ............................................ 27 

2.1.5 Incompatible mode elements .................................................................... 28 

2.1.6 Summary of recommendations for element usage ............................................ 28 

2.1.7 Naming convention ................................................................................ 29 

2.1.8 Node ordering and face numbering on elements ............................................ 30 

2.1.9 Numbering of integration points for output ............................................ 31 

2.2 Structural elements ............................................................................................ 32 

2.2.1 Beam elements ............................................................................................ 32 

2.2.2 Shell elements ............................................................................................ 34 

2.3 Interactions ........................................................................................................ 37 

2.3.1 Defining contact pairs ................................................................................ 37 

vii

2.3.2 Discretization of contact pair surfaces ........................................................ 37 

2.3.3 Contact tracking approaches .................................................................... 39 

2.3.4 Choosing the master and slave roles in a two-surface contact pair .................... 39 

2.3.5 Contact pressure-overclosure relationships ............................................ 40 

2.3.6 Contact constraint enforcement methods ............................................ 41 

2.3.7 Frictional behavior ................................................................................ 42 

2.3.8 Tied contact ............................................................................................ 44 

Chapter 3 Static Analysis of Beam-to-Column Joints ............................................ 45 

3.1 Introduction ........................................................................................................ 45 

3.2 Finite element modeling ............................................................................................ 45 

3.2.1 Simulation with shell elements .................................................................... 45 

3.2.2 Simulation with solid (continuum) elements ............................................ 46 

3.3 Experimental data ............................................................................................ 48 

3.4 Numerical results ............................................................................................ 49 

Chapter 4 Static Analysis of Steel Frames ........................................................ 61 

4.1 Introduction ........................................................................................................ 61 


4.3 Frame A .................................................................................................................... 62 

4.4 Frame B .................................................................................................................... 68 

Chapter 5 Dynamic Analysis of Steel Frames ........................................................ 73 

5.1 Introduction ........................................................................................................ 73 


5.3 Frame 1 .................................................................................................................... 76 

5.4 Frame 2 .................................................................................................................... 80 

Chapter 6 Conclusions ............................................................................................ 89 

References .................................................................................................................... 91 

viii

Chapter 1 

Design of Steel Structures with Eurocode 3 

1.1 Materials 

Standard and 

steel grade 

Nominal thickness of the element t [mm] 

t ≤ 40 mm 40 mm < t ≤ 80 mm 

fy [N/mm 2 ] fu [N/mm 2 ] fy [N/mm 2 ] fu [N/mm 2 ] 

EN 10025-2 

S 235 235 360 215 360 

S 275 275 430 255 410 

S 355 355 510 335 470 

S 450 440 550 410 550 

EN 10025-3 

S 275 N/NL 275 390 255 370 

S 355 N/NL 355 490 335 470 

S 420 N/NL 420 520 390 520 

S 460 N/NL 460 540 430 540 

EN 10025-4 

S 275 M/ML 275 370 255 360 

S 355 M/ML 355 470 335 450 

S 420 M/ML 420 520 390 500 

S 460 M/ML 460 540 430 530 

EN 10025-5 

S 235 W 235 360 215 340 

S 355 W 355 510 335 490 

EN 10025-6 

S 460 

Q/QL/QL1 

460 570 440 550 

Table 1.1: Nominal values of yield strength fy and ultimate tensile strength fu for hot rolled 

structural steel 

The material coefficients to be adopted in calculations for the structural steels should be 

taken as follows: 

– Modulus of elasticity E = 210 000 N/mm 2 

– Shear modulus G = E / 2(1+v) = 81 000 N/mm² 

– Poisson’s ratio in elastic stage v = 0.30 

– Coefficient of linear thermal expansion 12 x 10 -6 per o C (for T ≤ 100 o C) 

1

Chapter 1 Design of steel structures with Eurocode 3 

The bilinear stress-strain relationship indicated in Figure 1.1 may be used for the grades of 

structural steel specified above. Alternatively, a more precise relationship may be adopted, 

as described in section 1.3. 

1.2 Classification of cross sections 

2 

Fig. 1.1: Bilinear stress-strain relationship 

The role of cross section classification is to identify the extent to which the resistance and 

rotation capacity of cross sections is limited by its local buckling resistance. 

(1) Four classes of cross-sections are defined, as follows: 

– Class 1: cross-sections are those which can form a plastic hinge with the rotation 

capacity required from plastic analysis without reduction of the resistance. 

– Class 2: cross-sections are those which can develop their plastic moment resistance, 

but have limited rotation capacity because of local buckling. 

– Class 3: cross-sections are those in which the stress in the extreme compression fibre 

of the steel member assuming an elastic distribution of stresses can reach the yield 

strength, but local buckling is liable to prevent development of the plastic moment 

resistance. 

– Class 4: cross-sections are those in which local buckling will occur before the 

attainment of yield stress in one or more parts of the cross-section. 

(2) In Class 4 cross sections effective widths may be used to make the necessary 

allowances for reductions in resistance due to the effects of local buckling, see EN 

1993-1-5, 5.2.2. 

(3) The classification of a cross-section depends on the width to thickness ratio of the parts 

subject to compression. 

(4) Compression parts include every part of a cross-section which is either totally or 

partially in compression under the load combination considered. 

(5) The various compression parts in a cross-section (such as a web or flange) can, in 

general, be in different classes. 

(6) A cross-section is classified according to the highest (least favorable) class of its 

compression parts. Exceptions are specified in EN 1993-1-1, 6.2.1(10), 6.2.2.4(1). 

(7) Alternatively the classification of a cross-section may be defined by quoting both the 

flange classification and the web classification. 

(8) The limiting proportions for Class 1, 2, and 3 compression parts should be obtained 

from Table 1.2. A part which fails to satisfy the limits for Class 3 should be taken as 

Class 4.


Stress 

distribution 

in parts 

(compression 

positive) 

4 

3 c / t 124 

c / t 42 

42 

when 1: 

c / t 

0, 

67 0, 

33 

when 1 

*) 

: c / t 62 

( 1 

) ( 

) 

235/ 

f y 

fy 

 

235 

1,00 

275 

0,92 

355 

0,81 

420 

0,75 

460 

0,71 

*) 

where ς ≤ -1 applies where either the compression stress ζ < fy or the tensile strain εy > fy/E 

Table 1.2: Maximum width-to-thickness ratios for compression parts 

1.3 Finite element methods of analysis 

1.3.1 General 

The choice of the FE-method depends on the problem to be analysed and based on the 

following assumptions: 

No Material 

behavior 

f y 

- 

+ 

f y 

c/2 

c 

Geometric 

behavior 

Imperfections Example of use 

1 linear linear no elastic shear lag effect, elastic resistance 

2 nonlinear linear no plastic resistance in ULS 

3 linear nonlinear no critical plate buckling load 

4 linear nonlinear yes elastic plate buckling resistance 

5 nonlinear nonlinear yes elastic-plastic resistance in ULS 

Table 1.3: Assumptions for FE-methods 

Use 

In using FEM for design, special care should be taken to: 

– the modeling of the structural component and its boundary conditions; 

– the choice of software and documentation; 

– the use of imperfections; 

– the modeling of material properties; 

– the modeling of loads; 

– the modeling of limit state criteria; 

– the partial factors to be applied. 

+ 

f y 

c 

- 

f y 

+ 

f y 

c

Design of steel structures with Eurocode 3 Chapter 1 

1.3.2 Modeling 

(1) The choice of FE-models (shell models or volume models) and the size of mesh 

determine the accuracy of results. For validation sensitivity checks with successive 

refinement may be carried out. 

(2) The FE-modeling may be carried out either for: 

– the component as a whole or 

– a substructure as a part of the whole structure. 

NOTE: An example for a component could be the web and/or the bottom plate of 

continuous box girders in the region of an intermediate support where the bottom plate is 

in compression. An example for a substructure could be a subpanel of a bottom plate 

subject to biaxial stresses. 

(3) The boundary conditions for supports, interfaces and applied loads should be chosen 

such that results obtained are conservative. 

(4) Geometric properties should be taken as nominal. 

(5) All imperfections should be based on the shapes and amplitudes of section 1.3.5. 

(6) Material properties should conform to section 1.3.6. 

Choice of software and documentation 

(1) The software should be suitable for the task and be proven reliable. 

NOTE: Reliability can be proven by appropriate benchmark tests. 

(2) The mesh size, loading, boundary conditions and other input data as well as the output 

should be documented in a way that they can be reproduced by third parties. 

1.3.3 Use of imperfections 

(1) Where imperfections need to be included in the FE-model these imperfections should 

include both geometric and structural imperfections. 

(2) Unless a more refined analysis of the geometric imperfections and the structural 

imperfections is carried out, equivalent geometric imperfections may be used. 

NOTE 1: Geometric imperfections may be based on the shape of the critical plate buckling 

modes with amplitudes given in the National Annex. 80% of the geometric fabrication 

tolerances is recommended. 

NOTE 2: Structural imperfections in terms of residual stresses may be represented by a 

stress pattern from the fabrication process with amplitudes equivalent to the mean 

(expected) values. 

(3) The direction of the applied imperfection should be such that the lowest resistance is 

obtained. 

(4) For applying equivalent geometric imperfections Table 1.4 and Figure 1.2 may be used. 

Type of 

imperfection 

Component Shape Magnitude 

global member with length l bow 

see EN 1993-1-1, 

Table 5.1 

global longitudinal stiffener with length a bow min (a/400, b/400) 

local 

panel or subpanel with short span 

a or b 

buckling shape min (a/200, b/200) 

local stiffener or flange subject to twist bow twist 1 / 50 

Table 1.4: Equivalent geometric imperfections 

5


6 

Type of 

imperfection 

global member 

with length l 

global 

longitudinal 

stiffener with 

length a 

local panel or 

subpanel 

local stiffener or 

flange subject to 

twist 

b 

Component 

e 0y 

Fig. 1.2: Modeling of equivalent geometric imperfections 

 

e 0z 

b a 

e 0w 

a 

b 

a 

b 

__ 1 

50 

e 0w 

e 0w 

a


(5) In combining imperfections a leading imperfection should be chosen and the 

accompanying imperfections may have their values reduced to 70%. 

NOTE 1: Any type of imperfection should be taken as the leading imperfection and the 

others may be taken as the accompanying imperfections. 

NOTE 2: Equivalent geometric imperfections may be substituted by the appropriate 

fictitious forces acting on the member. 

1.3.4 Material properties 

(1) Material properties should be taken as characteristic values. 

(2) Depending on the accuracy and the allowable strain required for the analysis, the 

following assumptions for the material behaviour may be used, see Figure 1.3: 

a) elastic-plastic without strain hardening; 

b) elastic-plastic with a nominal plateau slope; 

c) elastic-plastic with linear strain hardening; 

d) true stress-strain curve modified from the test results as follows: 

ζtrue = ζ (1+ε) 

εtrue = ln (1+ε) 

Model 

with yielding 

plateau 

with strainhardening 

ζ 

f y 

ζ 

f y 

tan -1 (E) 

tan -1 (E) 

α) a) β) b) 

γ) c) 

ε 

ε 

tan -1 (E/100) 

ζ 

f y 1 

tan -1 (E) 

1 tan -1 (E/10000) 

(or similarly small value) 

ζ 

f y 

1 

tan -1 (E) 

Fig.1.3: Modeling of material behavior 

2 

δ) d) 

1 true stress-strain curve 

2 stress-strain curve from tests 

ε 

ε 

7


1.3.5 Loads, limit state criteria and partial factors 

Loads 

(1) The loads applied to the structures should include relevant load factors and load 

combination factors. For simplicity a single load multiplier a may be used. 

Limit state criteria 

(1) The ultimate limit state criteria should be used as follows: 

1. for structures susceptible to buckling: attainment of the maximum load. 

2. for regions subjected to tensile stresses: attainment of a limiting value of the principal 

membrane strain. 

NOTE 1: The National Annex may specify the limiting of principal strain. A value of 5% 

is recommended. 

NOTE 2: Other criteria may be used, e.g. attainment of the yielding criterion or limitation 

of the yielding zone. 

Partial factors 

(1) The load magnification factor au to the ultimate limit state should be sufficient to 

achieve the required reliability. 

(2) The magnification factor au should consist of two factors as follows: 

1. a1 to cover the model uncertainty of the FE-modeling used. It should be obtained from 

evaluations of test calibrations; 

2. a2 to cover the scatter of the loading and resistance models. It may be taken as γΜ1 if 

instability governs and γΜ2 if fracture governs. 

(3) It should be verified that: au > a1 a2 

NOTE: The National Annex may give information on γΜ1 and γΜ2. The use of γΜ1 and γΜ2 

as specified in the relevant parts of EN 1993 is recommended. 

1.4 Design of joints 

1.4.1 Introduction 

Joint is defined as the zone where two or more members are interconnected. For design 

purposes it is the assembly of all the basic components required to represent the behaviour 

during the transfer of the relevant internal forces and moments between the connected 

members. A beam-to-column joint consists of a web panel and either one connection 

(single sided joint configuration) or two connections (double sided joint configuration), see 

Figure 1.4. 

Connection is defined as the location at which two or more elements meet. For design 

purposes it is the assembly of the basic components required to represent the behaviour 

during the transfer of the relevant internal forces and moments at the connection. 

8


1 

3 

2 

Joint = web panel in shear + connection Left joint = web panel in shear + left connection 

Right joint = web panel in shear + right connection 

1 

1 

a)Single-sided joint configuration b)Double-sided joint configuration 

1 web panel in shear 

2 connection 

3 components (e.g. bolts, endplate) 

Fig.1.4: Parts of a beam-to-column joint configuration 

3 3 

a) Major axis joint configurations 

2 

2 

5 

5 

2 

4 

1 

1 Single-sided beam-to 

column joint 

configuration; 

2 Double-sided beam-tocolumn 

joint 

configuration; 

Double-sided beam-to-column Double-sided beam-to-column 

joint configuration joint configuration 

b) Minor-axis joint configurations (to be used only for balanced moments Mb1,Ed = Mb2,Ed) 

3 

3 Beam splice; 

4 Column splice; 

5 Column base 

2 

9


Fig.1.5: Joint configurations 

1.4.2 Connections made with bolts 

The yield strength fyb and the ultimate tensile strength fub for bolt classes 4.6, 5.6, 6.8, 8.8 

and 10.9 are given in Table 1.5. These values should be adopted as characteristic values in 

design calculations. 

10 

Bolt class 4.6 5.6 6.8 8.8 10.9 

fyb (N/mm 2 ) 240 300 480 640 900 

fub (N/mm 2 ) 400 500 600 800 1000 

Table 1.5: Nominal values of the yield strength fyb and the ultimate tensile strength fub for 

bolts 

Only bolt assemblies of classes 8.8 and 10.9 conforming to the requirements given in 2.8 

Reference Standards: Group 4 for High Strength Structural Bolting with controlled 

tightening in accordance with the requirements in 2.8 Reference Standards: Group 7 may 

be used as preloaded bolts. 

1.4.3 Categories of bolted connections 

Shear connections 

Bolted connections loaded in shear should be designed as one of the following: 

a) Category A: Bearing type 

In this category bolts from class 4.6 up to and including class 10.9 should be used. 

No preloading and special provisions for contact surfaces are required. The design 

ultimate shear load should not exceed the design shear resistance nor the design 

bearing resistance. 

b) Category B: Slip-resistant and serviceability limit state 

In this category preloaded bolts should be used. Slip should not occur at the 

serviceability limit state. The design serviceability shear load should not exceed the 

design slip resistance. The design ultimate shear load should not exceed the design 

shear resistance nor the design bearing resistance. 

c) Category C: Slip-resistant at ultimate limit state 

In this category preloaded bolts should be used. Slip should not occur at the 

ultimate limit state. The design ultimate shear load should not exceed the design 

slip resistance nor the design bearing resistance. In addition for a connection in 

tension, the design plastic resistance of the net cross-section at bolt holes Nnet,Rd, 

(see 6.2 of EN 1993-1-1), should be checked, at the ultimate limit state. 

The design checks for these connections are summarized in Table 1.6. 

Tension connections 

Bolted connection loaded in tension should be designed as one of the following: 

a) Category D: non-preloaded 

In this category bolts from class 4.6 up to and including class 10.9 should be used. 

No preloading is required. This category should not be used where the connections 

are frequently subjected to variations of tensile loading. However, they may be 

used in connections designed to resist normal wind loads.


b) Category E: preloaded 

In this category preloaded 8.8 and 10.9 bolts with controlled tightening in 

conformity with 2.8 Reference Standards: Group 7 should be used. 

The design checks for these connections are summarized in Table 1.6. 

Category Criteria Remarks 

Shear connections 

A 

bearing type 

B 

slip-resistant at 

serviceability 

C 

slip-resistant at 

ultimate 

D 

non-preloaded 

E 

preloaded 

Fv,Ed ≤ Fv,Rd 

Fv,Ed ≤ Fb,Rd 

Fv,Ed.ser ≤ Fs,Rd,ser 

Fv,Ed ≤ Fv,Rd 


Fv,Ed ≤ Fs,Rd 


Fv,Ed ≤ Nnet,Rd 

Ft,Ed ≤ Ft,Rd 

Ft,Ed ≤ Bp,Rd 

Ft,Ed ≤ Ft,Rd 

Ft,Ed ≤ Bp,Rd 

Tension connections 

No preloading required. 

Bolt classes from 4.6 to 10.9 may be used. 

Preloaded 8.8 or 10.9 bolts should be used. 

For slip resistance at serviceability see EN 

1993-1-8, 3.9. 


For slip resistance at ultimate see EN 1993- 

1-8, 3.9. 

Nnet,Rd see EN 1993-1-1. 

No preloading required. 

Bolt classes from 4.6 to 10.9 may be used. 

Bp,Rd see Table 1.8. 


Bp,Rd see Table 1.8. 

The design tensile force Ft,Ed should include any force due to prying action, see EN 

1993-1-8, 3.11. Bolts subjected to both shear force and tensile force should also satisfy 

the criteria given in Table 1.8. 

Table 1.6: Categories of bolted connections 

1.4.4 Positioning of holes for bolts and rivets 

Minimum and maximum spacing and end and edge distances for bolts and rivets are given 

in Table 1.7. 

Distances and 

spacings, 

see Figure 1.6 

Minimum Maximum 

1) 2) 3) 

Structures made from steels conforming to 

EN 10025 except steels conforming to EN 

10025-5 

Steel exposed to the 

weather or other 

corrosive influences 

Steel not exposed to 

the weather or other 

corrosive influences 

Structures made from 

steels conforming to 

EN 10025-5 

Steel used 

unprotected 

End distance e1 1,2d0 4t + 40 mm The larger of 

8t or 125 mm 

Edge distance e2 1,2d0 4t + 40 mm The larger of 

Distance e3 

in slotted holes 

1,5d0 4) 

8t or 125 mm 

11


Distance e4 

in slotted holes 

Spacing p1 2,2d0 The smaller of 

14t or 200 mm 

12 

1,5d0 4) 

Spacing p1,0 The smaller of 

14t or 200 mm 

Spacing p1,i The smaller of 

28t or 400 mm 

The smaller of 

14t or 200 mm 

The smaller of 

14tmin or 175 mm 

Spacing p2 5) 2,4d0 The smaller of The smaller of The smaller of 

14t or 200 mm 14t or 200 mm 14tmin or 175 mm 

1) Maximum values for spacings, edge and end distances are unlimited, except in the following 

cases: 

– for compression members in order to avoid local buckling and to prevent corrosion in exposed 

members and; 

– for exposed tension members to prevent corrosion. 

2) The local buckling resistance of the plate in compression between the fasteners should be 

calculated according to EN 1993-1-1 using 0,6 pi as buckling length. Local buckling between the 

fasteners need not to be checked if p1/t is smaller than 9 ε. The edge distance should not exceed the 

local buckling requirements for an outstand element in the compression members, see EN 1993-1- 

1. The end distance is not affected by this requirement. 

3) t is the thickness of the thinner outer connected part. 

4) The dimensional limits for slotted holes are given in 2.8 Reference Standards: Group 7. 

5) For staggered rows of fasteners a minimum line spacing of p2 = 1,2d0 may be used, provided that 

the minimum distance, L, between any two fasteners is greater than 2,4d0, see Figure 1.6 b). 

Table 1.7: Minimum and maximum spacing, end and edge distances 

Staggered rows of fasteners 

a) Symbols for spacing of fasteners b) Symbols for staggered spacing 

p1 ≤ 14 t and ≤ 200 mm p2 ≤ 14 t and ≤ 200 mm p1,0 ≤ 14 t and ≤ 200 mm p1,i ≤ 28 t and ≤ 400 mm 

1 outer row 2 inner row 

c) Staggered spacing – compression d) Spacing in tension members


e) End and edge distances for slotted holes 

Fig. 1.6: Symbols for end and edge distances and spacing of fasteners 

1.4.5 Design resistance of individual fasteners 

Failure mode Bolts Rivets 

Shear resistance per shear 

plane 

Fv,Rd = 

Bearing resistance 1), 2), 3) Fb,Rd = 

 

v 

f 

 

ub 

M 2 

A 

- where the shear plane passes through the 

threaded portion of the bolt (A is the tensile 

stress area of the bolt As): 

- for classes 4.6, 5.6 and 8.8: 

av = 0,6 

- for classes 4.8, 5.8, 6.8 and 10.9: 

av = 0,5 

- where the shear plane passes through the 

unthreaded portion of the bolt (A is the gross 

cross section of the bolt): av = 0,6 

k a f d t 

1 

b 

 

u 

M 2 

where αb is the smallest of αd or 

f 

f 

ub 

u 

or 1,0; 

In the direction of load transfer: 

e1 

- for end bolts: αd = , for inner bolts: αd = 

3d 

Perpendicular to the direction of load transfer: 

0 

0 

Fv,Rd = 

p1 

1 

 

d 4 

3 0 

e2 

- for edge bolts: k1 is the smallest of 2, 

8 1, 

7 or 2,5 

d 

0, 

6 

p2 

- for inner bolts: k1 is the smallest of 1, 

4 1, 

7 or 2,5 

d 

0 

f 

 

ur A0 

M 2 

13


Tension resistance 2) 

14 

Ft,Rd = 

k 

2 

ub s A f 

 

M 2 

where k2 = 0,63 for countersunk bolt, 

otherwise k2 = 0,9. 

Ft,Rd = 

Punching shear resistance Bp,Rd = 0,6 π dm tp fu / γM2 No check needed 

Combined shear and 

tension 

F 

F 

v, 

Ed 

v, 

Rd 

Ft 

, Ed 

 

1 , 4 Ft 

, 

Rd 

 

1, 

0 

0, 

6 

f 

 

ur 0 A 

1) The bearing resistance Fb,Rd for bolts 

– in oversized holes is 0,8 times the bearing resistance for bolts in normal holes. 

– in slotted holes, where the longitudinal axis of the slotted hole is perpendicular to the direction 

of the force transfer, is 0,6 times the bearing resistance for bolts in round, normal holes. 

2) For countersunk bolt: 

– the bearing resistance Fb,Rd should be based on a plate thickness t equal to the thickness of the 

connected plate minus half the depth of the countersinking. 

– for the determination of the tension resistance Ft,Rd the angle and depth of countersinking should 

conform with 2.8 Reference Standards: Group 4, otherwise the tension resistance Ft,Rd should be 

adjusted accordingly. 

3) When the load on a bolt is not parallel to the edge, the bearing resistance may be verified 

separately for the bolt load components parallel and normal to the end. 

Table 1.8: Design resistance for individual fasteners subjected to shear and/or tension 


1.4.6 Analysis of joints 

General 

(1) The effects of the behaviour of the joints on the distribution of internal forces and 

moments within a structure, and on the overall deformations of the structure, should 

generally be taken into account, but where these effects are sufficiently small they may be 

neglected. 

(2) To identify whether the effects of joint behaviour on the analysis need be taken into 

account, a distinction may be made between three simplified joint models as follows: 

– simple, in which the joint may be assumed not to transmit bending moments; 

– continuous, in which the behaviour of the joint may be assumed to have no effect on the 

analysis; 

– semi-continuous, in which the behaviour of the joint needs to be taken into account in the 

analysis. 

(3) The appropriate type of joint model should be determined from Table 1.9, depending 

on the classification of the joint and on the chosen method of analysis. 

(4) The design moment-rotation characteristic of a joint used in the analysis may be 

simplified by adopting any appropriate curve, including a linearized approximation (e.g. 

bi-linear or tri-linear), provided that the approximate curve lies wholly below the design 

moment-rotation characteristic. 

Method of 

global analysis 

Classification of joints 

Elastic Nominally pinned Rigid Semi-rigid 

Rigid-plastic Nominally pinned Full-strength Partial-strength 

Elastic-plastic Nominally pinned 

Rigid and fullstrength 

Semi-rigid and partial strength 

Semi-rigid and full-strength 

Rigid and partial-strength 

Type of joint 

model 

Simple Continuous Semi-continuous 

Table 1.9: Type of joint model 

Elastic global analysis 

(1) The joints should be classified according to their rotational stiffness, see 1.4.7. 

(2) The joints shall have sufficient strength to transmit the forces and moments acting at 

the joints resulting from the analysis. 

(3) In the case of a semi-rigid joint, the rotational stiffness Sj corresponding to the bending 

moment Mj,Ed should generally be used in the analysis. If Mj,Ed does not exceed 2/3 Mj,Rd 

the initial rotational stiffness Sj,ini may be taken in the global analysis, see Figure 1.10(a). 

(4) As a simplification to (3), the rotational stiffness may be taken as Sj,ini/ε in the 

analysis, for all values of the moment Mj,Ed, as shown in Figure 1.10(b), where ε is the 

stiffness modification coefficient from Table 1.10. 

(5) For joints connecting H or I sections Sj is given in EN 1993-1-8, 6.3.1. 

15


16 

M j,Rd 

2/3 M j,Rd 

M j,Ed 

M j 

S j,ini 

a) Mj,Ed ≤ 2/3 Mj,Rd b) Mj,Ed ≤ Mj,Rd 

Fig. 1.10: Rotational stiffness to be used in elastic global analysis 

Type of connection Beam-to-column 

joints 

 

Other types of joints 

(beam-to-beam 

joints, beam splices, 

column base joints) 

Welded 2 3 

Bolted end-plate 2 3 

Bolted flange cleats 2 3,5 

Base plates - 3 

Table 1.10: Stiffness modification coefficient ε 

Rigid-plastic global analysis 

(1) The joints should be classified according to their strength, see 1.4.7. 

(2) For joints connecting H or I sections Mj,Rd is given in EN 1993-1-8, 6.2. 

(3) For joints connecting hollow sections the method given in EN 1993-1-8, section 7 may 

be used. 

(4) The rotation capacity of a joint shall be sufficient to accommodate the rotations 

resulting from the analysis. 

(5) For joints connecting H or I sections the rotation capacity should be checked according 

to EN 1993-1-8, 6.4. 

Elastic-plastic global analysis 

(1) The joints should be classified according to both stiffness and strength (see 1.4.7). 

(2) For joints connecting H or I sections Mj,Rd is given in EN 1993-1-8, 6.2, Sj is given in 

EN 1993-1-8, 6.3.1 and θCd is given in EN 1993-1-8, 6.4. 

(3) For joints connecting hollow sections the method given in EN 1993-1-8, section 7 may 

be used. 

(4) The moment rotation characteristic of the joints should be used to determine the 

distribution of internal forces and moments. 

(5) As a simplification, the bilinear design moment-rotation characteristic shown in Figure 

1.11 may be adopted. The stiffness modification coefficient should be obtained from Table 

1.10. 

M j,Rd 

M j,Ed 

M j 

S j,ini /


Mj,Rd 

Fig. 1.11: Simplified bilinear design moment-rotation characteristic 

1.4.7 Classification of joints 

Mj 

Sj,ini/ε 

Classification by stiffness 

Nominally pinned joints 

A nominally pinned joint shall be capable of transmitting the internal forces, without 

developing significant moments which might adversely affect the members or the 

structure as a whole and be capable of accepting the resulting rotations under the 

design loads. 

Rigid joints 

Joints classified as rigid may be assumed to have sufficient rotational stiffness to 

justify analysis based on full continuity. 

Semi-rigid joints 

A joint which does not meet the criteria for a rigid joint or a nominally pinned joint 

should be classified as a semi-rigid joint. It should be capable of transmitting the 

internal forces and moments. Semi-rigid joints provide a predictable degree of 

interaction between members, based on the design moment-rotation characteristics of 

the joints. 

Zone 1: rigid, if Sj,ini ≥ kbEIb/Lb 

where 

kb = 8 for frames where the bracing system reduces the horizontal displacement by 

at least 80% 

kb = 25 for other frames, provided that in every storey Kb/Kc ≥ 0.1 *) 

Zone 2: semi-rigid 

All joints in zone 2 should be classified as semi-rigid. Joints in zones 1 or 3 may 

optionally also be treated as semi-rigid. 

Zone 3: nominally pinned, if Sj,ini ≤ 0.5EIb/Lb 

*) For frames where Kb/Kc < 0.1 the joints should be classified as semi-rigid. 

 

θCd 

17


Key: 

18 

Kb is the mean value of Ib/Lb for all the beams at the top of that storey; 

Kc is the mean value of Ic/Lc for all the columns in that storey; 

Ib is the second moment of area of a beam; 

Ic is the second moment of area of a column; 

Lb is the span of a beam (center-to-center of columns); 

Lc is the storey height of a column. 

Fig. 1.12: Classification of joints by stiffness 

Classification by strength 

Nominally pinned joints 

A nominally pinned joint shall be capable of transmitting the internal forces, without 

developing significant moments which might adversely affect the members or the 

structure as a whole. It shall be capable of accepting the resulting rotations under the 

design loads and may be classified as nominally pinned if its design moment resistance 

Mj,Rd is not greater than 0,25 times the design moment resistance required for a fullstrength 

joint, provided that it also has sufficient rotation capacity. 

Full-strength joints 

The design resistance of a full strength joint shall be not less than that of the connected 

members. A joint may be classified as full-strength if it meets the criteria given in 

Figure 1.13. 

Partial-strength joints 

A joint which does not meet the criteria for a full-strength joint or a nominally pinned 

joint should be classified as a partial-strength joint. 

a) Top of column 

b) Within column height 

Key: 

M j,Sd 

M j,Sd 

Mb,pℓ,Rd is the design plastic moment resistance of a beam 

Mc,pℓ,Rd is the design plastic moment resistance of a column 

Fig. 1.13: Full-strength joints 

Either Mj,Rd ≥ Mb,pℓ,Rd 

or Mj,Rd ≥ Mc,pℓ,Rd 

Either Mj,Rd ≥ Mb,pℓ,Rd 

or Mj,Rd ≥ 2 Mc,pℓ,Rd 

1.4.8 Modeling of beam-to-column joints 

(1) To model the deformational behaviour of a joint, account should be taken of the shear 

deformation of the web panel and the rotational deformation of the connections. 

(2) Joint configurations should be designed to resist the internal bending moments Mb1,Ed 

and Mb2,Ed, normal forces Nb1,Ed and Nb2,Ed and shear forces Vb1,Ed and Vb2,Ed applied to the 

connections by the connected members, see Figure 1.14.


(3) The resulting shear force Vwp,Ed in the web panel should be obtained using: 

Vwp,Ed = (Mb1,Ed – Mb2,Ed) / z – (Vc1,Ed – Vc2,Ed) / 2 

where: z is the lever arm 

(4) To model a joint in a way that closely reproduces the expected behaviour, the web 

panel in shear and each of the connections should be modeled separately, taking account of 

the internal moments and forces in the members, acting at the periphery of the web panel, 

see Figure 1.14(a) and Figure 1.15. 

(5) As a simplified alternative to (4), a single-sided joint configuration may be modeled as 

a single joint, and a double-sided joint configuration may be modeled as two separate but 

inter-acting joints, one on each side. As a consequence a double-sided beam-to-column 

joint configuration has two moment-rotation characteristics, one for the right-hand joint 

and another for the left-hand joint. 

(6) In a double-sided, beam-to-column joint each joint should be modeled as a separate 

rotational spring, as shown in Figure 1.16, in which each spring has a moment-rotation 

characteristic that takes into account the behaviour of the web panel in shear as well as the 

influence of the relevant connection. 

(7) When determining the design moment resistance and rotational stiffness for each of the 

joints, the possible influence of the web panel in shear should be taken into account by 

means of the transformation parameters β1 and β2, where: 

β1 is the value of the transformation parameter β for the right-hand side joint; 

β2 is the value of the transformation parameter β for the left-hand side joint. 

(8) Approximate values for β1 and β2 based on the values of the beam moments Mb1,Ed and 

Mb2,Ed at the periphery of the web panel, see Figure 1.14(a), may be obtained from Table 

1.11. 

(9) As an alternative to (8), more accurate values of β1 and β2 based on the values of the 

beam moments Mj,b1,Ed and Mj,b2,Ed at the intersection of the member centerlines, may be 

determined from the simplified model shown in Figure 1.14(b) as follows: 

β1 = | 1 – Mj,b2,Ed / Mj,b1,Ed | ≤ 2 

β2 = | 1 – Mj,b1,Ed / Mj,b2,Ed | ≤ 2 

where: 

Mj,b1,Ed is the moment at the intersection from the right hand beam; 

Mj,b2,Ed Ed is the moment at the intersection from the left hand beam. 

(10) In the case of an unstiffened double-sided beam-to-column joint configuration in 

which the depths of the two beams are not equal, the actual distribution of shear stresses in 

the column web panel should be taken into account when determining the design moment 

resistance. 

a) Values at periphery of web panel b) Values at intersection of members centerlines 

Fig. 1.14: Forces and moments acting on the joint 

19


a) Shear forces in web panel b) Connections, with forces and moments in beams 

20 

Fig. 1.15: Forces and moments acting on the web panel at the connections 

x 

1 

N b2,Ed 

M b2,Ed 

V b2,Ed 

Single-sided joint configuration Double-sided joint configuration 

1 Joint 

2 Joint 2: left side 

3 Joint 1: right side 

Fig. 1.16: Modeling the joint 

Type of joint configuration Action Value of β 

2 

Mb1,Ed 

x x 

Mb1,Ed = Mb2,Ed 

3 

β ≈ 1 

β = 0 *) 

Mb1,Ed / Mb2,Ed > 0 β ≈ 1 

Mb1,Ed / Mb2,Ed < 0 β ≈ 2 

Mb1,Ed + Mb2,Ed = 0 β ≈ 2 

*) In this case the value of β is the exact value rather than an approximation. 

V b1,Ed 

Table 1.11: Approximate values for the transformation parameter β 

N b1,Ed 

M b1,Ed


1.4.9 Design moment-rotation characteristic 

(1) A joint may be represented by a rotational spring connecting the centre lines of the 

connected members at the point of intersection, as indicated in Figure 1.17(a) and (b) for a 

single-sided beam-to-column joint configuration. The properties of the spring can be 

expressed in the form of a design moment-rotation characteristic that describes the 

relationship between the bending moment Mj,Ed applied to a joint and the corresponding 

rotation θEd between the connected members. Generally the design moment-rotation 

characteristic is nonlinear as indicated in Figure 1.17(c). 

(2) A design moment-rotation characteristic, see Figure 1.17(c) should define the following 

three main structural properties: 

– moment resistance; 

– rotational stiffness; 

– rotation capacity. 

NOTE: In certain cases the actual moment-rotation behaviour of a joint includes some 

rotation due to such effects as bolt slip, lack of fit and, in the case of column bases, 

foundation-soil interactions. This can result in a significant amount of initial hinge rotation 

that may need to be included in the design moment-rotation characteristic. 

(3) The design moment-rotation characteristics of a beam-to-column joint shall be 

consistent with the assumptions made in the global analysis of the structure and with the 

assumptions made in the design of the members, see EN 1993-1-1. 

90° 

M 

Ed 

j,Ed 

M j,Rd 

M J,Ed 

1 Limit for Sj 

a) Joint b) Model c) Design moment-rotation characteristic 

Fig. 1.17: Design moment-rotation characteristic for a joint 

1.4.10 Basic components of a joint 

(1) The design moment-rotation characteristic of a joint should depend on the properties of 

its basic components, which should be among those identified in EN 1993-1-8, 6.1.3(2). 

(2) The basic joint components should be those identified in Table 1.12, together with the 

reference to the application rules which should be used for the evaluation of their structural 

properties. 

(3) Certain joint components may be reinforced. Details of the different methods of 

reinforcement are given in EN 1993-1-8, 6.2.4.3 and 6.2.6. 

(4) The relationships between the properties of the basic components of a joint and the 

structural properties of the joint should be those given in the following clauses: 

– for moment resistance in EN 1993-1-8, 6.2.7 and 6.2.8; 

– for rotational stiffness in EN 1993-1-8, 6.3.1; 

– for rotation capacity in EN 1993-1-8, 6.4. 

M j 

Sj 

S j,ini 

1 

 

Ed Xd Cd 

 

21


22 

1 

2 

3 

4 

5 

6 

Column web 

panel in shear 

Column web in 

transverse 

compression 

Column web in 

transverse tension 

Column flange in 

bending 

End-plate in 

bending 

Flange cleat in 

bending 

Component 

Ft,Ed 

VEd 

VEd 

Fc,Ed 

Ft,Ed 

Ft,Ed 

Ft,Ed


7 

8 

9 

Beam or column 

flange and web in 

compression 

Beam web in 

tension 

Plate in tension or 

compression 

10 Bolts in tension 

11 Bolts in shear 

12 

Bolts in bearing 

(on beam flange, 

column flange, 

end-plate or cleat) 

Component 

Fc,Ed 

Ft,Ed 

Ft,Ed 

Fc,Ed 

Fv,Ed 

Fb,Ed 

Fb,Ed 

Ft,Ed 

Fc,Ed 

Ft,Ed 

23


24 

13 

14 

15 

16 

17 

18 

Concrete in 

compression 

including grout 

Base plate in 

bending under 

compression 

Base plate in 

bending under 

tension 

Anchor bolts in 

tension 


shear 


bearing 

19 Welds 

20 Haunched beam 

Component 

Table 1.12: Basic joint components

2.1 Solid (continuum) elements 

Chapter 2 

Finite Element Modeling with 

ABAQUS/Standard 

The solid (or continuum) elements can be used for linear analysis and for complex 

nonlinear analyses involving contact, plasticity, and large deformations. They are available 

for stress, heat transfer, acoustic, coupled thermal-stress, coupled pore fluid-stress, 

piezoelectric, and coupled thermal-electrical analyses. The ABAQUS/Standard solid 

element library includes first-order (linear) interpolation elements and second-order 

(quadratic) interpolation elements in one, two, or three dimensions. Triangles and 

quadrilaterals are available in two dimensions; and tetrahedra, triangular prisms, and 

hexahedra (―bricks‖) are provided in three dimensions. Modified second-order triangular 

and tetrahedral elements are also provided. In addition, reduced-integration, hybrid, and 

incompatible mode elements are available. Solid elements are more accurate if not 

distorted, particularly for quadrilaterals and hexahedra. The triangular and tetrahedral 

elements are less sensitive to distortion. 

2.1.1 Choosing between first- and second-order elements 

In first-order plane strain, generalized plane strain, axisymmetric quadrilateral, hexahedral 

solid elements, and cylindrical elements, the strain operator provides constant volumetric 

strain throughout the element. This constant strain prevents mesh ―locking‖ when the 

material response is approximately incompressible. Second-order elements provide higher 

accuracy than first-order elements for ―smooth‖ problems that do not involve complex 

contact conditions, impact, or severe element distortions. They capture stress 

concentrations more effectively and are better for modeling geometric features: they can 

model a curved surface with fewer elements. Finally, second-order elements are very 

effective in bending-dominated problems. First-order triangular and tetrahedral elements 

should be avoided as much as possible in stress analysis problems; the elements are overly 

stiff and exhibit slow convergence with mesh refinement, which is especially a problem 

with first-order tetrahedral elements. If they are required, an extremely fine mesh may be 

needed to obtain results of sufficient accuracy. The ―modified‖ triangular and tetrahedral 

elements should be used in contact problems with the default ―hard‖ contact relationship 

because the contact forces are consistent with the direction of contact. These elements also 

perform better in analyses involving impact (because they have a lumped mass matrix), in 

analyses involving nearly incompressible material response, and in analyses requiring large 

element distortions, such as the simulation of certain manufacturing processes or the 

response of rubber components. 

2.1.2 Choosing between full- and reduced-integration elements 

Reduced integration uses a lower-order integration to form the element stiffness. The mass 

matrix and distributed loadings use full integration. Reduced integration reduces running 

25

Chapter 2 Finite element modeling with ABAQUS/Standard 

time, especially in three dimensions. For example, element type C3D20 has 27 integration 

points, while C3D20R has only 8; therefore, element assembly is roughly 3.5 times more 

costly for C3D20 than for C3D20R. In Abaqus/Standard you can choose between full or 

reduced integration for quadrilateral and hexahedral (brick) elements. The elements with 

reduced integration are also referred to as uniform strain or centroid strain elements with 

hourglass control. Second-order reduced-integration elements generally yield more 

accurate results than the corresponding fully integrated elements. However, for first-order 

elements the accuracy achieved with full versus reduced integration is largely dependent 

on the nature of the problem. 

Hourglassing 

Hourglassing can be a problem with first-order, reduced-integration elements (CPS4R, 

CAX4R, C3D8R, etc.) in stress/displacement analyses. Since the elements have only one 

integration point, it is possible for them to distort in such a way that the strains calculated 

at the integration point are all zero, which, in turn, leads to uncontrolled distortion of the 

mesh. First-order, reduced-integration elements include hourglass control, but they should 

be used with reasonably fine meshes. Hourglassing can also be minimized by distributing 

point loads and boundary conditions over a number of adjacent nodes. The second-order 

reduced-integration elements, with the exception of the 27-node C3D27R and C3D27RH 

elements, do not have the same difficulty and are recommended in all cases when the 

solution is expected to be smooth. The C3D27R and C3D27RH elements have three 

unconstrained, propagating hourglass modes when all 27 nodes are present. These 

elements should not be used with all 27 nodes, unless they are sufficiently constrained 

through boundary conditions. First-order elements are recommended when large strains or 

very high strain gradients are expected. 

Shear and volumetric locking 

Fully integrated elements in Abaqus/Standard do not hourglass but may suffer from 

―locking‖ behavior: both shear and volumetric locking. Shear locking occurs in first-order, 

fully integrated elements (CPS4, CPE4, C3D8, etc.) that are subjected to bending. The 

numerical formulation of the elements gives rise to shear strains that do not really exist— 

the so-called parasitic shear. Therefore, these elements are too stiff in bending, in particular 

if the element length is of the same order of magnitude as or greater than the wall 

thickness. Volumetric locking occurs in fully integrated elements when the material 

behavior is (almost) incompressible. Spurious pressure stresses develop at the integration 

points, causing an element to behave too stiffly for deformations that should cause no 

volume changes. If materials are almost incompressible (elastic-plastic materials for which 

the plastic strains are incompressible), second-order, fully integrated elements start to 

develop volumetric locking when the plastic strains are on the order of the elastic strains. 

However, the first-order, fully integrated quadrilaterals and hexahedra use selectively 

reduced integration (reduced integration on the volumetric terms). Therefore, these 

elements do not lock with almost incompressible materials. Reduced-integration, secondorder 

elements develop volumetric locking for almost incompressible materials only after 

significant straining occurs. In this case, volumetric locking is often accompanied by a 

mode that looks like hourglassing. Frequently, this problem can be avoided by refining the 

mesh in regions of large plastic strain. If volumetric locking is suspected, check the 

pressure stress at the integration points (printed output). If the pressure values show a 

checkerboard pattern, changing significantly from one integration point to the next, 

volumetric locking is occurring. 

26

Finite element modeling with ABAQUS/Standard Chapter 2 

2.1.3 Choosing between bricks/quadrilaterals and tetrahedra/triangles 

Triangular and tetrahedral elements are geometrically versatile and are used in many 

automatic meshing algorithms. It is very convenient to mesh a complex shape with 

triangles or tetrahedra, and the second-order and modified triangular and tetrahedral 

elements (CPE6, CPE6M, C3D10, C3D10M, etc.) are suitable for general usage. However, 

a good mesh of hexahedral elements usually provides a solution of equivalent accuracy at 

less cost. Quadrilaterals and hexahedra have a better convergence rate than triangles and 

tetrahedra, and sensitivity to mesh orientation in regular meshes is not an issue. However, 

triangles and tetrahedra are less sensitive to initial element shape, whereas first-order 

quadrilaterals and hexahedra perform better if their shape is approximately rectangular. 

The elements become much less accurate when they are initially distorted. First-order 

triangles and tetrahedra are usually overly stiff, and extremely fine meshes are required to 

obtain accurate results. As mentioned earlier, fully integrated first-order triangles and 

tetrahedra in Abaqus/Standard also exhibit volumetric locking in incompressible problems. 

As a rule, these elements should not be used except as filler elements in noncritical areas. 

Therefore, try to use well-shaped elements in regions of interest. 

Tetrahedral and wedge elements 

For stress/displacement analyses the first-order tetrahedral element C3D4 is a constant 

stress tetrahedron, which should be avoided as much as possible; the element exhibits slow 

convergence with mesh refinement. This element provides accurate results only in general 

cases with very fine meshing. Therefore, C3D4 is recommended only for filling in regions 

of low stress gradient in meshes of C3D8 or C3D8R elements, when the geometry 

precludes the use of C3D8 or C3D8R elements throughout the model. For tetrahedral 

element meshes the second-order or the modified tetrahedral elements, C3D10 or 

C3D10M, should be used. Similarly, the linear version of the wedge element C3D6 should 

generally be used only when necessary to complete a mesh, and, even then, the element 

should be far from any areas where accurate results are needed. This element provides 

accurate results only with very fine meshing. 

Modified triangular and tetrahedral elements 

A family of modified 6-node triangular and 10-node tetrahedral elements is available that 

provides improved performance over the first-order triangular and tetrahedral elements and 

that avoids some of the problems that exist for regular second-order triangular and 

tetrahedral elements, mainly related to their use in contact problems with the default ―hard‖ 

contact relationship. 

2.1.4 Choosing between regular and hybrid elements 

Hybrid elements are intended primarily for use with incompressible and almost 

incompressible material behavior. When the material response is incompressible, the 

solution to a problem cannot be obtained in terms of the displacement history only, since a 

purely hydrostatic pressure can be added without changing the displacements. 

2.1.5 Incompatible mode elements 

Incompatible mode elements (CPS4I, CPE4I, CAX4I, CPEG4I, and C3D8I and the 

corresponding hybrid elements) are first-order elements that are enhanced by incompatible 

modes to improve their bending behavior. In addition to the standard displacement degrees 

of freedom, incompatible deformation modes are added internally to the elements. The 

27


primary effect of these modes is to eliminate the parasitic shear stresses that cause the 

response of the regular first-order displacement elements to be too stiff in bending. In 

addition, these modes eliminate the artificial stiffening due to Poisson's effect in bending 

(which is manifested in regular displacement elements by a linear variation of the stress 

perpendicular to the bending direction). In the nonhybrid elements—except for the plane 

stress element, CPS4I—additional incompatible modes are added to prevent locking of the 

elements with approximately incompressible material behavior. For fully incompressible 

material behavior the corresponding hybrid elements must be used. Because of the added 

internal degrees of freedom due to the incompatible modes (4 for CPS4I; 5 for CPE4I, 

CAX4I, and CPEG4I; and 13 for C3D8I), these elements are somewhat more expensive 

than the regular first-order displacement elements; however, they are significantly more 

economical than second-order elements. The incompatible mode elements use full 

integration and, thus, have no hourglass modes. 

Shape considerations 

The incompatible mode elements perform almost as well as second-order elements in many 

situations if the elements have an approximately rectangular shape. The performance is 

reduced considerably if the elements have a parallelogram shape. The performance of 

trapezoidal-shaped incompatible mode elements is not much better than the performance of 

the regular, fully integrated, first-order interpolation elements. Hence, there is a loss of 

accuracy associated with distorted elements. 

Using incompatible mode elements in large-strain applications 

Incompatible mode elements should be used with caution in applications involving large 

compressive strains. Convergence may be slow at times, and inaccuracies may accumulate 

in hyperelastic applications. Hence, erroneous residual stresses may sometimes appear in 

hyperelastic elements that are unloaded after having been subjected to a complex 

deformation history. 

Using incompatible mode elements with regular elements 

Incompatible mode elements can be used in the same mesh with regular solid elements. 

Generally the incompatible mode elements should be used in regions where bending 

response must be modeled accurately, and they should be of rectangular shape to provide 

the most accuracy. While these elements often provide accurate response in such cases, it 

is generally preferable to use structural elements (shells or beams) to model structural 

components. 

2.1.6 Summary of recommendations for element usage 

Make all elements as ―well shaped‖ as possible to improve convergence and accuracy. 

If an automatic tetrahedral mesh generator is used, use the second-order elements 

C3D10. If contact is present, use the modified tetrahedral element C3D10M if the 

default ―hard‖ contact relationship is used or in analyses with large amounts of plastic 

deformation. 

If possible, use hexahedral elements in three-dimensional analyses since they give the 

best results for the minimum cost. 

For linear and ―smooth‖ nonlinear problems use reduced-integration, second-order 

elements if possible. 

28


Use second-order, fully integrated elements close to stress concentrations to capture the 

severe gradients in these regions. However, avoid these elements in regions of finite 

strain if the material response is nearly incompressible. 

Use first-order quadrilateral or hexahedral elements or the modified triangular and 

tetrahedral elements for problems involving contact or large distortions. If the mesh 

distortion is severe, use reduced-integration, first-order elements. 

If the problem involves bending and large distortions, use a fine mesh of first-order, 

reduced-integration elements. 

Hybrid elements must be used if the material is fully incompressible (except when 

using plane stress elements). Hybrid elements should also be used in some cases with 

nearly incompressible materials. 

Incompatible mode elements can give very accurate results in problems dominated by 

bending. 

2.1.7 Naming convention 

The naming conventions for solid elements depend on the element dimensionality. Onedimensional, 

two-dimensional, three-dimensional, and axisymmetric solid elements in 

Abaqus are named as follows. 

Fig. 2.1: Naming convention 

For example, CAX4R is an axisymmetric continuum stress/displacement, 4-node, reducedintegration 

element; and CPS8RE is an 8-node, reduced-integration, plane stress 

piezoelectric element. 

29


2.1.8 Node ordering and face numbering on elements 

Tetrahedral element faces: 

Face 1: 1 – 2 – 3 face 

Face 2: 1 – 4 – 2 face 

Face 3: 2 – 4 – 3 face 

Face 4: 3 – 4 – 1 face 

30 

Fig. 2.2: Node ordering and face numbering on solid elements 

Wedge (triangular prism) element faces: 

Face 1: 1 – 2 – 3 face 

Face 2: 4 – 6 – 5 face 

Face 3: 1 – 4 – 5 – 2 face


Face 4: 2 – 5 – 6 – 3 face 

Face 5: 3 – 6 – 4 – 1 face 

Hexahedron (brick) element faces: 

Face 1: 1 – 2 – 3 – 4 face 

Face 2: 5 – 8 – 7 – 6 face 

Face 3: 1 – 5 – 6 – 2 face 

Face 4: 2 – 6 – 7 – 3 face 

Face 5: 3 – 7 – 8 – 4 face 

Face 6: 4 – 8 – 5 – 1 face 

2.1.9 Numbering of integration points for output 

Fig. 2.3: Numbering of solid elements integration points 

31


2.2 Structural elements 

There are six kinds of structural elements in Abaqus/Standard; membrane, truss, beam, 

frame, elbow and shell elements. The most widely used are the beam-column and shell 

finite elements, which are discussed below. 

2.2.1 Beam elements 

Timoshenko beams (B21, B22, B31, B31OS, B32, B32OS, PIPE21, PIPE22, PIPE31, 

PIPE32, and their ―hybrid‖ equivalents) allow for transverse shear deformation. They can 

be used for thick (―stout‖) as well as slender beams. For beams made from uniform 

material, shear flexible beam theory can provide useful results for cross-sectional 

dimensions up to 1/8 of typical axial distances or the wavelength of the highest natural 

mode that contributes significantly to the response. Beyond this ratio the approximations 

that allow the member's behavior to be described solely as a function of axial position no 

longer provide adequate accuracy. It is assumed that the transverse shear behavior of 

Timoshenko beams is linear elastic with a fixed modulus and, thus, independent of the 

response of the beam section to axial stretch and bending. The Timoshenko beams can be 

subjected to large axial strains. The axial strains due to torsion are assumed to be small. In 

combined axial-torsion loading, torsional shear strains are calculated accurately only when 

the axial strain is not large. The linear Timoshenko beam elements use a lumped mass 

formulation. The quadratic Timoshenko beam elements use a consistent mass formulation, 

except in dynamic procedures in which a lumped mass formulation with a 1/6, 2/3, 1/6 

distribution is used. The shear factor k (Cowper, 1966) is defined as: 

32 

Section type Shear factor, k 

Arbitrary 1.0 

Box 0.44 

Circular 0.89 

Elbow 0.85 

Generalized 1.0 

Hexagonal 0.53 

I (and T) 0.44 

L 1.0 

Meshed 1.0 

Nonlinear generalized 1.0 

Pipe 0.53 

Rectangular 0.85 

Trapezoidal 0.822 

Table 2.1: Shear factor k definition for Timoshenko beams


Circular section 

Geometric input data: Radius 

I-section 

Fig. 2.4: Circular section integration points 

Fig. 2.5: I-section integration points 

Geometric input data: l, h, b1, b2, t1, t2, t3 

Set b1 and t1 or b2 and t2 to zero to model a T-section. 

Beam element cross-section orientation 

The orientation of a beam cross-section is defined in Abaqus in terms of a local, righthanded 

(t, n1, n2) axis system, where t is the tangent to the axis of the element, positive in 

the direction from the first to the second node of the element, and n1 and n2 are basis 

vectors that define the local 1- and 2-directions of the cross-section. n1 is referred to as the 

first beam section axis, and n2 is referred to as the normal to the beam. This beam crosssectional 

axis system is illustrated in Fig. 2.6. 

33


34 

Fig. 2.6: Local axis definition for beam-type elements 

For beams in a plane the n1-direction is always (0.0, 0.0, –1.0); that is, normal to the plane 

in which the motion occurs. Therefore, planar beams can bend only about the first beamsection 

axis. For beams in space the approximate direction of n1 must be defined directly 

as part of the beam section definition or by specifying an additional node off the beam axis 

as part of the element definition. This additional node is included in the element's 

connectivity list. 

If an additional node is specified, the approximate direction of n1 is defined by the 

vector extending from the first node of the element to the additional node. 

If n1 is defined directly for the section and an additional node is specified, the direction 

calculated by using the additional node will take precedence. 

If the approximate direction is not defined by either of the above methods, the default 

value is (0.0, 0.0, –1.0). 

2.2.2 Shell elements 

Shell elements are used to model structures in which one dimension, the thickness, is 

significantly smaller than the other dimensions. Conventional shell elements use this 

condition to discretize a body by defining the geometry at a reference surface. In this case 

the thickness is defined through the section property definition. Conventional shell 

elements have displacement and rotational degrees of freedom. In contrast, continuum 

shell elements discretize an entire three-dimensional body. The thickness is determined 

from the element nodal geometry. Continuum shell elements have only displacement 

degrees of freedom. From a modeling point of view continuum shell elements look like 

three-dimensional continuum solids, but their kinematic and constitutive behavior is 

similar to conventional shell elements. In this thesis, only conventional shells are used.


Fig. 2.7: Conventional versus continuum shell element 

For shells in space the positive normal is given by the right-hand rule going around the 

nodes of the element in the order that they are specified in the element definition. 

Fig. 2.8: Positive normals for three-dimensional conventional shells 

The section points through the thickness of the shell are numbered consecutively, starting 

with point 1. For shell sections integrated during the analysis, section point 1 is exactly on 

the bottom surface of the shell if Simpson's rule is used, and it is the point that is closest to 

the bottom surface if Gauss quadrature is used. For general shell sections, section point 1 is 

always on the bottom surface of the shell. For a homogeneous section the total number of 

section points is defined by the number of integration points through the thickness. For 

shell sections integrated during the analysis, you can define the number of integration 

points through the thickness. The default is five for Simpson's rule and three for Gauss 

quadrature. For general shell sections, output can be obtained at three section points. For a 

composite section the total number of section points is defined by adding the number of 

integration points per layer for all of the layers. For shell sections integrated during the 

analysis, you can define the number of integration points per layer. The default is three for 

Simpson's rule and two for Gauss quadrature. For general shell sections, the number of 

section points for output per layer is three. The default output points through the thickness 

of a shell section are the points that are on the bottom and top surfaces of the shell section 

(for integration with Simpson's rule) or the points that are closest to the bottom and top 

surfaces (for Gauss quadrature). For example, if five integration points are used through a 

single layer shell, output will be provided for section points 1 (bottom) and 5 (top). 

35


36 

Fig. 2.9: Node ordering and face numbering on shell elements 

Fig. 2.10: Numbering of shell elements integration points


2.3 Interactions 

Contact pairs in Abaqus/Standard can be used to define interactions between bodies in 

mechanical, coupled temperature-displacement, coupled pore pressure-displacement, 

coupled thermal-electrical, and heat transfer simulations and do not have to use surfaces 

with matching meshes. 

2.3.1 Defining contact pairs 

To define a contact pair, you must indicate which pairs of surfaces may interact with one 

another or which surfaces may interact with themselves. Contact surfaces should extend far 

enough to include all regions that may come into contact during an analysis; however, 

including additional surface nodes and faces that never experience contact may result in 

significant extra computational cost (for example, extending a slave surface such that it 

includes many nodes that remain separated from the master surface throughout an analysis 

can significantly increase memory usage unless penalty contact enforcement is used). 

2.3.2 Discretization of contact pair surfaces 

Conditional constraints are applied at various locations on interacting surfaces to simulate 

contact conditions. The locations and conditions of these constraints depend on the contact 

discretization used in the overall contact formulation. Two contact discretization options 

are offered: a traditional ―node-to-surface‖ discretization and a true ―surface-to-surface‖ 

discretization. 

Node-to-surface contact discretization 

With traditional node-to-surface discretization the contact conditions are established such 

that each ―slave‖ node on one side of a contact interface effectively interacts with a point 

of projection on the ―master‖ surface on the opposite side of the contact interface (see Fig. 

2.11). Thus, each contact condition involves a single slave node and a group of nearby 

master nodes from which values are interpolated to the projection point. 

Fig. 2.11: Node-to-surface contact discretization 

Traditional node-to-surface discretization has the following characteristics: 

37


The slave nodes are constrained not to penetrate into the master surface; however, the 

nodes of the master surface can, in principle, penetrate into the slave surface (for 

example, see the case on the upper-right of Fig. 2.12). 

38 

Fig 2.12: Comparison of contact enforcement for different master-slave assignments 

with node-to-surface and surface-to-surface contact discretizations. 

The contact direction is based on the normal of the master surface. 

The only information needed for the slave surface is the location and surface area 

associated with each node; the direction of the slave surface normal and slave surface 

curvature are not relevant. Thus, the slave surface can be defined as a group of nodes— 

a node-based surface. 

Node-to-surface discretization is available even if a node-based surface is not used in a 

contact pair definition. 

Surface-to-surface contact discretization 

Surface-to-surface discretization considers the shape of both the slave and master surfaces 

in the region of contact constraints. Surface-to-surface discretization has the following key 

characteristics: 

The surface-to-surface formulation enforces contact conditions in an average sense 

over regions nearby slave nodes rather than only at individual slave nodes. The 

averaging regions are approximately centered on slave nodes, so each contact 

constraint will predominantly consider one slave node but will also consider adjacent 

slave nodes. Some penetration may be observed at individual nodes; however, large, 

undetected penetrations of master nodes into the slave surface do not occur with this 

discretization. Figure 2.12 compares contact enforcement for node-to-surface and 

surface-to-surface contact for an example with dissimilar mesh refinement on the 

contacting bodies. 

The contact direction is based on an average normal of the slave surface in the region 

surrounding a slave node. 

Surface-to-surface discretization is not applicable if a node-based surface is used in the 

contact pair definition.


In general, surface-to-surface discretization provides more accurate stress and pressure 

results than node-to-surface discretization if the surface geometry is reasonably well 

represented by the contact surfaces. 

2.3.3 Contact tracking approaches 

There are two tracking approaches to account for the relative motion of two interacting 

surfaces in mechanical contact simulations. 

The finite-sliding tracking approach 

Finite-sliding contact is the most general tracking approach and allows for arbitrary 

relative separation, sliding, and rotation of the contacting surfaces. For finite-sliding 

contact the connectivity of the currently active contact constraints changes upon relative 

tangential motion of the contacting surfaces. 

The small-sliding tracking approach 

Small-sliding contact assumes that there will be relatively little sliding of one surface along 

the other and is based on linearized approximations of the master surface per constraint. 

The groups of nodes involved with individual contact constraints are fixed throughout the 

analysis for small-sliding contact, although the active/inactive status of these constraints 

typically can change during the analysis. You should consider using small-sliding contact 

when the approximations are reasonable, due to computational savings and added 

robustness. 

2.3.4 Choosing the master and slave roles in a two-surface contact pair 

The following rules are enforced related to the assignment of the master and slave roles for 

contact surfaces: 

Analytical rigid surfaces and rigid-element-based surfaces must always be the master 

surface. 

A node-based surface can act only as a slave surface and always uses node-to-surface 

contact. 

Slave surfaces must always be attached to deformable bodies or deformable bodies 

defined as rigid. 

Both surfaces in a contact pair cannot be rigid surfaces with the exception of 

deformable surfaces defined as rigid. 

When both surfaces in a contact pair are element-based and attached to either deformable 

bodies or deformable bodies defined as rigid, you have to choose which surface will be the 

slave surface and which will be the master surface. This choice is particularly important for 

node-to-surface contact. Generally, if a smaller surface contacts a larger surface, it is best 

to choose the smaller surface as the slave surface. If that distinction cannot be made, the 

master surface should be chosen as the surface of the stiffer body or as the surface with the 

coarser mesh if the two surfaces are on structures with comparable stiffnesses. The 

stiffness of the structure and not just the material should be considered when choosing the 

master and slave surface. For example, a thin sheet of metal may be less stiff than a larger 

block of rubber even though the steel has a larger modulus than the rubber material. If the 

stiffness and mesh density are the same on both surfaces, the preferred choice is not always 

obvious. 

The choice of master and slave roles typically has much less effect on the results with a 

surface-to-surface contact formulation than with a node-to-surface contact formulation. 

However, the assignment of master and slave roles can have a significant effect on 

performance with surface-to-surface contact if the two surfaces have dissimilar mesh 

39


refinement; the solution can become quite expensive if the slave surface is much coarser 

than the master surface. 

2.3.5 Contact pressure-overclosure relationships 

The following pressure-overclosure relationships can be used to define the contact model: 

the ―hard‖ contact relationship minimizes the penetration of the slave surface into the 

master surface at the constraint locations and does not allow the transfer of tensile 

stress across the interface; 

a modified ―hard‖ contact relationship, which allows some limited penetrations before 

activating contact constraints and allows some transfer of tensile stress across the 

interface before deactivating contact constraints; 

a ―softened‖ contact relationship in which the contact pressure is a linear function of 

the clearance between the surfaces; 

a ―softened‖ contact relationship in which the contact pressure is an exponential 

function of the clearance between the surfaces; 

a ―softened‖ contact relationship in which a tabular pressure-overclosure curve is 

constructed by progressively scaling the default penalty stiffness; 

a ―softened‖ contact relationship in which the contact pressure is a piecewise linear 

(tabular) function of the clearance between the surfaces; and 

a relationship in which there is no separation of the surfaces once they contact. 

The ―softened‖ contact pressure-overclosure relationships might be used to model a soft, 

thin layer on one or both surfaces. In Abaqus/Standard they are also sometimes useful for 

numerical reasons because they can make it easier to resolve the contact condition. The 

softened contact relationship should be used with caution in implicit dynamic impact 

simulations. If this relationship is used in such a simulation, the impact algorithm will not 

be used, which destroys kinetic energy of the nodes on the surface when impact occurs, but 

will instead assume a perfectly elastic collision. The consequence of this change is that the 

slave nodes bounce back immediately after impact with the master surface; hence, 

extensive ―chattering‖ may result, leading to convergence problems and small time 

increments. However, softened contact may work well in implicit dynamic calculations 

where impact effects are not important; for example, if contact changes are primarily due 

to sliding motion along a curved surface, such as may occur in low-speed metal forming 

applications. 

“Hard” contact relationship 

The most common contact pressure-overclosure relationship is shown in Fig. 2.13, 

although the zero-penetration condition may or may not be strictly enforced depending on 

the constraint enforcement method used. When surfaces are in contact, any contact 

pressure can be transmitted between them. The surfaces separate if the contact pressure 

reduces to zero. Separated surfaces come into contact when the clearance between them 

reduces to zero. 

40


Fig. 2.13: ―hard‖ contact relationship 

“Softened” contact defined as a linear function 

In a linear pressure-overclosure relationship the surfaces transmit contact pressure when 

the overclosure between them, measured in the contact (normal) direction, is greater than 

zero. The linear pressure-overclosure relationship is identical to a tabular relationship with 

two data points, where the first point is located at the origin (see Fig. 2.14). Only the slope 

of the pressure-overclosure relationship, k, should be specified. 

Fig. 2.14: ―Softened‖ pressure-overclosure relationship defined in tabular form 

2.3.6 Contact constraint enforcement methods 

Contact constraint enforcement methods in Abaqus/Standard: 

are specified as part of the surface interaction definition; 

determine how contact constraints imposed by a physical pressure-overclosure 

relationship are resolved numerically in an analysis; 

can either strictly enforce or approximate the physical pressure-overclosure 

relationships; 

can be modified to resolve convergence difficulties due to overconstraints*; and 

_________________________________________________________________________ 

* In general, the term overconstraint refers to multiple constraints acting on the same 

degree of freedom. Overconstraints are then categorized as consistent (if all the constraints 

are compatible with each other) or inconsistent (if the constraints are incompatible with 

each other). Consistent overconstraints are also called redundant constraints, and 

inconsistent overconstraints are also called conflicting constraints. 

41


sometimes utilize Lagrange multiplier degrees of freedom. 

There are three contact constraint enforcement methods available: 

The direct method attempts to strictly enforce a given pressure-overclosure behavior 

per constraint, without approximation or use of augmentation iterations. 

The penalty method is a stiff approximation of hard contact. 

The augmented Lagrange method uses the same kind of stiff approximation as the 

penalty method, but also uses augmentation iterations to improve the accuracy of the 

approximation. 

The default constraint enforcement method depends on interaction characteristics, as 

follows: 

The penalty method is used by default for finite-sliding, surface-to-surface contact 

(including general contact) if a ―hard‖ pressure-overclosure relationship is in effect. 

The augmented Lagrange method is used by default for three-dimensional self-contact 

with node-to-surface discretization if a ―hard‖ pressure-overclosure relationship is in 

effect. 

The direct method is the default in all other cases. 

You should consider the following factors when choosing the contact enforcement method: 

The direct method must be used for contact pairs with a ―softened‖ pressureoverclosure 

relationship. 

The direct method strictly enforces the specified pressure-overclosure behavior 

consistent with the constraint formulation. 

The penalty or augmented Lagrange constraint enforcement methods sometimes 

provide more efficient solutions (generally due to reduced calculation costs per 

iteration and a lower number of overall iterations per analysis) at some (typically 

small) sacrifice in solution accuracy. 

Overconstraints due to overlapping contact definitions or the combination of contact 

and other constraint types should be avoided for directly enforced hard contact. 

In many cases the various constraint enforcement methods can be used with or without 

creating Lagrange multiplier degrees of freedom. Lagrange multipliers can add 

significantly to solution cost, but they also protect against numerical errors related to illconditioning 

that can occur if high contact stiffness is in effect. Any Lagrange multipliers 

associated with contact are present only for active contact constraints, so the number of 

equations will change as the contact status changes. Abaqus/Standard will choose whether 

or not to use Lagrange multipliers automatically, based on the contact stiffness. 

2.3.7 Frictional behavior 

The basic concept of the Coulomb friction model is to relate the maximum allowable 

frictional (shear) stress across an interface to the contact pressure between the contacting 

bodies. In the basic form of the Coulomb friction model, two contacting surfaces can carry 

shear stresses up to a certain magnitude across their interface before they start sliding 

relative to one another; this state is known as sticking. The Coulomb friction model defines 

this critical shear stress, ηcrit, at which sliding of the surfaces starts as a fraction of the 

contact pressure, p, between the surfaces (ηcrit = μp). The stick/slip calculations determine 

when a point transitions from sticking to slipping or from slipping to sticking. The fraction, 

μ, is known as the coefficient of friction. 

42


For the case when the slave surface consists of a node-based surface, the contact pressure 

is equal to the normal contact force divided by the cross-sectional area at the contact node. 

The default cross-sectional area is 1.0; you can specify a cross-sectional area associated 

with every node in the node-based surface when the surface is defined or, alternatively, 

assign the same area to every node through the contact property definition. 

The basic friction model assumes that μ is the same in all directions (isotropic friction). For 

a three-dimensional simulation there are two orthogonal components of shear stress, η1 and 

η2, along the interface between the two bodies. These components act in the slip directions 

for the contact surfaces or contact elements. 

Fig. 2.15: Slip regions for the basic Coulomb friction model 

You can specify an optional equivalent shear stress limit, ηmax, so that, regardless of the 

magnitude of the contact pressure stress, sliding will occur if the magnitude of the 

equivalent shear stress reaches this value (see Fig. 2.16). This shear stress limit is typically 

introduced in cases when the contact pressure stress may become very large (as can happen 

in some manufacturing processes), causing the Coulomb theory to provide a critical shear 

stress at the interface that exceeds the yield stress in the material beneath the contact 

surface. A reasonable upper bound estimate for ηmax is fy / √3, where fy is the Mises yield 

stress of the material adjacent to the surface; however, empirical data are the best source 

for ηmax. 

Fig. 2.16: Slip regions for the friction model with a limit on the critical shear stress 

43


2.3.8 Tied contact 

Tied contact in Abaqus/Standard: 

ties two surfaces forming a contact pair together for the duration of a simulation; 

can be used in mechanical, coupled temperature-displacement, coupled pore pressuredisplacement, 

coupled thermal-electrical, or heat transfer simulations; 

constrains each of the nodes on the slave surface to have the same value of 

displacement, temperature, pore pressure, or electrical potential as the point on the 

master surface that it contacts; 

allows for rapid transitions in mesh density within the model; and 

requires the adjustment of the contact pair surfaces. 

The tied contact formulation constrains only translational degrees of freedom in 

mechanical simulations. No constraints are placed on the rotational degrees of freedom of 

structural elements involved in tied contact pairs. Mechanical constraints for tied contact 

are strictly enforced with a direct Lagrange multiplier method by default. Alternatively, 

you can specify that these constraints should be enforced with a penalty or augmented 

Lagrange constraint method. The constraint enforcement method specified will be applied 

to the tangential constraints in addition to the normal constraints. Softened contact 

pressure-overclosure relationships (exponential, tabular, or linear) are ignored for tied 

contact. Slave nodes are not constrained to the master surface unless they are precisely in 

contact with the master surface at the start of the analysis. Any slave nodes not precisely in 

contact at the start of the analysis (either open or overclosed) will remain unconstrained for 

the duration of the simulation; they will never interact with the master surface. In 

mechanical simulations an unconstrained slave node can penetrate the master surface 

freely. In a thermal, electrical, or pore pressure simulation an unconstrained slave node will 

not exchange heat, electrical current, or pore fluid with the master surface. 

44

Chapter 3 

Static Analysis of Beam-to-Column Joints 

3.1 Introduction 

Bolted beam-to-column joints with extended end-plates are used widely in steel 

structures. They form moment-resistant connections between steel members, but their 

behavior can be either rigid or semi-rigid depending on the stiffness and strength of their 

components. The consideration of semi-rigid connections corresponds to a more realistic 

simulation of the joints behavior leading to more reliable solutions. However, the large 

number of variables related to connection geometry makes the task of incorporating semirigid 

behavior of the connections into the frame design a complicated process. 

Additionally, structural joints may exhibit nonlinear behavior such as localized 

elastoplastic deformations, unilateral contact and slip phenomena. The behavior of steel 

joints has been the subject of both experimental and numerical studies by a number of 

researchers. 

For the estimation of the joint response, apart from experimental testing [20-25], three 

modeling options are available practically. These are analytical or empirical models [8], 

mechanical models [9] and advanced finite element models [10-19]. This thesis presents a 

finite element study of semi-rigid joints subjected to static loading. Stiffness, moment 

resistance and rotation capacity derived from the calculation of moment-rotation (M-θ) 

curves are compared with experimental results by Coelho et al. [20] and Eurocode 3 

suggestions [5]. The finite element discretization of beam-to-column joints is produced 

automatically from their geometric description via appropriate code that has been 

developed during the preparation of this thesis. ABAQUS/Standard software is used for the 

numerical analyses [1-2]. 

3.2 Finite element modeling 

3.2.1 Simulation with shell elements 

Two different element types are used for modeling the end-plate bolted beam-tocolumn 

joint (Fig. 3.1). Plane components of the joint (beam/column flanges and web, endplate, 

transverse web stiffeners) are modeled with the S4 quadrilateral shell element of 

appropriate thickness, while the bolts are modeled with beam elements of circular section. 

The interaction between the column flange and the end-plate is considered through surfacebased 

contact simulation with element-based surface definition, which enables contact 

between independent meshes without node compatibility. 

The S4 ABAQUS element is a four-node fully integrated, general-purpose, finitemembrane-strain 

quadrilateral shell element. The element’s membrane response is treated 

with an assumed strain formulation that gives accurate solutions to in-plane bending 

problems, is not sensitive to element distortion, and avoids parasitic locking. It allows 

transverse shear deformation using thick shell theory as the shell thickness increases and 

becomes discrete Kirchhoff thin shell element as the thickness decreases (transverse shear 

45

Chapter 3 Static analysis of beam-to-column joints 

deformation becomes very small). There are four integration locations per element and five 

integration points through its thickness. 

The B31 element is a two-node linear Timoshenko (shear flexible) beam element that 

allows transverse shear deformation. It is assumed that the transverse shear behavior is 

linear elastic with a fixed modulus and, thus, independent of the response of the beam 

section to axial stretch and bending. 

Column flange behaves as master surface and end-plate as slave surface (contact pair). 

Small sliding contact formulation assumes that although the surfaces may undergo large 

motions, there will be relatively little sliding of one surface along the other, which means 

that a slave node will interact with the same local area of the master surface throughout the 

analysis. This assumption is realistic for the bolted beam-to-column joints. A linear 

pressure-overclosure relationship is considered with a slope of the corresponding curve 

equal to 10 5 kN/cm 3 . In static analysis, the results coincide to those considering a hard 

contact relationship, because of the high p-o slope magnitude. In a linear p-o relationship 

the surfaces transmit contact pressure when the overclosure between them, measured in the 

contact normal direction, is greater than zero, while arbitrary separation is allowed. Finally, 

when surfaces are in contact, they usually transmit shear as well as normal forces across 

their interface. The basic isotropic Coulomb friction model is used for this purpose with a 

constant friction coefficient μ equal to 0.30. 

46 

Fig. 3.1: Joint simulation with shell (quadrilateral) finite elements 

3.2.2 Simulation with solid (continuum) elements 

Three-dimensional eight-node hexahedral solid elements are used for the detailed 

simulation of the extended end-plate bolted beam-to-column joint (Figs. 3.2, 3.3). Apart 

from the finite element discretization difficulties using three-dimensional solid elements, 

there are many complexities related to the contacts between the different components of a 

beam-to-column bolted joint. Particularly, there are five interactions that should be 

considered: (a) column flange with end-plate; (b) column flange with bolt nuts; (c) endplate 

with bolt heads; (d) column flange hole with bolt shanks; and (e) end-plate hole with

Static analysis of beam-to-column joints Chapter 3 

bolt shanks. All of them are modeled by using surface-based contacts with element-based 

surface definition that enables connection of independent meshes. Surfaces are defined 

through the appropriate faces of the hexahedral solids. 

For contact cases (a), (d) and (e) small sliding contact formulation is considered with a 

softened contact relationship. The slope of the linear pressure-overclosure curve is taken 

equal to 10 5 kN/cm 3 . The tangential behavior of the interfaces is modeled through the basic 

isotropic Coulomb friction model with a constant coefficient μ equal to 0.30. For the other 

cases tied contact simulation is considered, where each node on the slave surface has the 

same displacement with the corresponding contact point on the master surface. 

Three different ABAQUS element types are examined: 

The C3D8 element with full integration (8 Gauss points). Fully integrated elements do 

not hourglass, but may suffer from shear locking behavior. Shear locking occurs in 

first-order, fully integrated elements that are subjected to bending. The numerical 

formulation of the elements gives rise to shear strains that do not really exist, the socalled 

parasitic shear. Therefore, these elements are too stiff in bending. 

The C3D8R element with reduced integration (1 Gauss point) and hourglass control. 

Reduced integration uses a lower-order integration to form the element stiffness. The 

mass matrix and distributing loadings use full integration. Reduced integration reduces 

running time, especially in three dimensions. It is suitable for problems involving 

contact, bending and large distortions. 

The C3D8I element with full integration (8 Gauss points) and incompatible modes. 

Incompatible mode elements are first-order elements that are enhanced by incompatible 

modes to improve their bending behavior. In addition to the standard displacement 

degrees of freedom, incompatible deformation modes are added internally to the 

elements through thirteen additional variables. The primary effect of these modes is to 

eliminate the parasitic shear stresses that cause the response of the regular first-order 

displacement elements to be too stiff in bending. This element is more expensive than 

C3D8, but can give very accurate results in problems dominating by bending. 

Nut 

Shank 

Head 

Fig. 3.2: Bolt simulation with continuum (8-node hexahedral solid) finite elements 

47


48 

Fig. 3.3: Joint simulation with continuum (8-node hexahedral solid) finite elements 

3.3 Experimental data 

An experimental investigation of eight statically loaded extended end-plate moment 

connections was undertaken at the Delft University of Technology to provide insight into 

the behaviour of this joint type up to collapse. The specimens were designed to confine 

failure to the end-plate and/or bolts without development of the full plastic moment 

capacity of the beam. The parameters investigated were the end-plate thickness and steel 

grade. The results show that an increase in end-plate thickness results in an increase in the 

connection flexural strength and stiffness and a decrease in rotation capacity. Similar 

conclusions are drawn for the effect of the end-plate steel grade, though no major 

variations in the initial stiffness are observed. The failure modes involved weld failure in 

two test specimens, nut stripping in four tests and bolt fracture in the remaining, always 

after significant yielding of the end-plate and bolt bending. 

The experimental programme essentially comprised four test details (two specimens for 

each testing type) on the above joint configuration. Two main parameters were varied in 

the four sets: the end-plate thickness, tp and the end-plate steel grade. The specimens were 

fabricated from one column/beam set, as detailed in Table 3.1. End-plates were connected 

to the beam-ends by full-strength 45 o continuous fillet welds. The fillet welds were done in 

the shop in a down-hand position. The procedure involved manual metal arc welding in 

which consumable electrodes were used. Basic, soft, low hydrogen electrodes have been 

used in the process. Hand tightened full-threaded M20 grade 8.8 bolts in 22 mm drilled 

holes were employed in all sets. Two different batches of bolts were employed. The first 

batch of bolts were employed in tests FS1a-b, FS2a-b and FS3a in both tension and 

compression zones; the second batch of bolts were used to fasten the end plate and the 

beam in the tension zone in the remaining tests. The column had a section profile HE340M 

that was chosen so that it behaves almost as a rigid element. In addition, for the available 

column, the clearance above and below the end plate was less than 400 mm. However,


since this is a rigid column, this limitation proved not to be severe. The actual geometry of 

the various connection elements was recorded before starting the test. Moreover, the values 

for the Young modulus, E, the strain hardening modulus, Est, the static yield and tensile 

stresses, fy and fu, the strain at the strain hardening point, εst, the uniform strain, εuni, and the 

ultimate strain, εu have been measured. 

Test 

ID 

Number Column Beam Endplate 

Profile 

Steel 

grade 

Profile Steel 

grade 

tp (mm) Steel 

grade 

FS1 2 HEM340 S355 IPE300 S235 10 S355 

FS2 2 HEM340 S355 IPE300 S235 15 S355 

FS3 2 HEM340 S355 IPE300 S235 20 S355 

FS4 2 HEM340 S355 IPE300 S235 10 S690 

3.4 Numerical results 

Table 3.1: Details of the test specimens [20] 

The detailed geometry of the connections is considered in the numerical analyses 

performed. The bolts are modeled via an equivalent diameter of 18.80 mm that derives 

from the average of the gross diameter 20.00 mm and the effective diameter of the bolt 

shank (effective cross-section corresponding to the threaded part of the shank As=245 

mm 2 , for M20). Boundary conditions and loading procedures are the same as in the 

experiments. Particularly, each node of the back column flange has been constrained and a 

vertical load is applied on the transverse web stiffener of the beam. The finite element 

analysis procedure is based on incremental Newton-Raphson technique, while material and 

geometric nonlinearities are taken into account via the von Mises isotropic plasticity model 

and large displacement consideration. 

The moment-rotation (Μ-θ) curves for the several connections are obtained from the 

beam vertical displacements and the applied load. The bending moment, M, acting on the 

connection corresponds to the applied load, L, multiplied by the distance, d, between the 

load application point and the face of the end-plate: 

M = L d (3.1) 

The rotational deformation of the joint is the sum of the shear deformation of the 

column web panel zone and the connection rotational deformation. In these tests, the 

column hardly deforms as it behaves as a rigid element. Thus, the connection rotation θ is 

taken into account, which is defined as the change in angle between the centerlines of 

beam and column and is approximately given by: 

θ = arctan(δ / d) – ζb.el (3.2) 

where δ: vertical displacement of the beam at the load application point, and ζb.el: beam 

elastic rotation (neglected in this study). 

EC3-1-8 states that a bolted end-plate joint may be assumed to have sufficient rotation 

capacity for plastic analysis, provided that both conditions are satisfied: (i) the moment 

resistance of the joint is governed by the resistance of either the column flange in bending 

49


or the end-plate in bending; and (ii) the thickness, t, of either the column flange or the endplate 

(not necessarily the same basic component as in (i)) satisfies: 

50 

t ≤ 0.36 θb √ (fu.b / fy) (3.3) 

where θb: bolt diameter, fu.b: tensile strength of the bolt, and fy: yield strength of the 

relevant basic component. EC3-1-8 prediction for stiffness Sj is given by the relationship: 

Sj = Sj.ini / ε (3.4) 

where Sj.ini: initial stiffness evaluated according to the component method, and ε: stiffness 

modification factor which in the context of an elastic-plastic global structural analysis is 

taken as 2.0 for bolted end-plate beam-to-column joints. 

Moment-rotation (M-θ) curves of the above test specimens are presented in the next 

figures and compared with the experimental results by Coelho et al. [20] and Eurocode 3 

suggestions [5]. There are also von Mises stress distributions for models C3D8R and S4 at 

the last/failure step of the nonlinear analysis plotted on the deformed shape of the joint 

with deformation scale factor equal to one. The first three models are plotted in stress scale 

0-35.5 kN/cm 2 and the fourth in 0-69.0 kN/cm 2 according to each end-plate nominal yield 

stress. Moreover, horizontal deformation of the end-plate is observed for each test for 

elastic and elastoplastic behavior of the joint. See Figs. 3.4-23. 

Four models are examined, one with shell elements and three with continuum elements. 

All of them predict accurately the elastic stiffness of the joints and generally are reliable in 

linear elastic static analysis. Bending of end-plates is the main reason for differences 

between these simulations in the elastoplastic region. For thin end-plates, which are 

dominated by bending (FS1, FS4), the use of continuum elements with reduced integration 

performs better. This simulation (C3D8R) predicts almost exactly the three main joint 

behavioral characteristics, which are stiffness, resistance and rotation capacity. The normal 

brick element (C3D8) overestimates the elastic behavior of the joint, while the enhanced 

with incompatible modes (C3D8I) gives more accurate results but remains stiff for this 

type of problems underestimating their high rotation capacity. Joint modeling with shell 

elements has a drawback. Bolt forces are applied locally to the nodes that connect the 

column flange with the end-plate and as a result there is local concentration of stresses, 

especially for very thin end-plates and/or column flanges. As the thickness of end-plate 

increases (FS2, FS3) the simulations tend to coincide. Brick elements with reduced 

integration remain the more flexible, while bricks with incompatible modes give also 

reliable results. Simulation with shell elements behaves very satisfactory and can be used 

for such type of problems.


Moment [kNm] 

200 

150 

100 

50 

FS1 

EC3-1-8 

0 

0 20 40 60 80 100 120 

Rotation [mrad] 

Fig. 3.4: Moment-rotation curves for FS1 

Coelho et al. - FS1a 

Coelho et al. - FS1b 

C3D8 

C3D8R 

C3D8I 

S4 

Fig. 3.5: von Mises stresses distribution for FS1 (C3D8R) 

51


52 

End-plate height [cm] 

40 

35 

30 

25 

20 

15 

10 

5 

0 

Fig. 3.6: von Mises stresses distribution for FS1 (S4) 

M = 57.0 kNm 

Bolt - tension 

Beam flange 


Bolt - compression 

Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 

End-plate Horizontal Displacement [cm] 

ABAQUS - C3D8 

ABAQUS - C3D8R 

ABAQUS - C3D8I 

ABAQUS - S4 

Fig. 3.7: End-plate horizontal displacements for FS1 (M = 57.0 kNm)


Moment [kNm] 


40 

35 

30 

25 

20 

15 

10 

5 

0 

200 

150 

100 

0 0.2 0.4 0.6 0.8 1 1.2 

Fig. 3.8: End-plate horizontal displacements for FS1 (M = 95.0 kNm) 

50 

M = 95.0 kNm 


FS2 

EC3-1-8 



Beam flange 


ABAQUS - C3D8 



ABAQUS - S4 


Beam flange 

0 

0 20 40 60 80 100 120 




C3D8 

C3D8R 

C3D8I 

S4 

53


54 


Fig. 3.11: von Mises stresses distribution for FS2 (S4)




40 

35 

30 

25 

20 

15 

10 

5 

0 


Beam flange 



Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 


40 

35 

30 

25 

20 

15 

10 

5 

0 

M = 110.0 kNm 


M = 176.0 kNm 

ABAQUS - C3D8 



ABAQUS - S4 


Beam flange 



Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 


ABAQUS - C3D8 



ABAQUS - S4 


55


56 

Moment [kNm] 

200 

150 

100 

50 

FS3 

EC3-1-8 

0 

0 20 40 60 80 100 120 





C3D8 

C3D8R 

C3D8I 

S4 

Fig. 3.15: von Mises stresses distribution for FS3 (C3D8R)



40 

35 

30 

25 

20 

15 

10 

5 

0 


M = 120.0 kNm 


Beam flange 



Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 


ABAQUS - C3D8 



ABAQUS - S4 


57


58 

Moment [kNm] 


40 

35 

30 

25 

20 

15 

10 

5 

0 

0 0.2 0.4 0.6 0.8 1 1.2 


200 

150 

100 

50 

M = 192.0 kNm 


FS4 

EC3-1-8 



Beam flange 


ABAQUS - C3D8 



ABAQUS - S4 


Beam flange 

0 

0 20 40 60 80 100 120 




C3D8 

C3D8R 

C3D8I 

S4



Fig. 3.21: von Mises stresses distribution for FS4 (S4) 

59


60 



40 

35 

30 

25 

20 

15 

10 

5 

0 

M = 88.0 kNm 


Beam flange 



Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 


ABAQUS - C3D8 



ABAQUS - S4 


40 

35 

30 

25 

20 

15 

10 

5 

0 

M = 154.0 kNm 


Beam flange 



Beam flange 

0 0.2 0.4 0.6 0.8 1 1.2 


ABAQUS - C3D8 



ABAQUS - S4 

Fig. 3.23: End-plate horizontal displacements for FS4 (M = 154.0 kNm)


Chapter 4 

Static Analysis of Steel Frames 

Multistory steel frames with detailed modeling of their joints according to Chapter 3 are 

examined, while parametric studies are performed demonstrating the effect of geometric 

characteristics variations of joint components on the connection behavior and consequently 

on the overall response of the frames. The finite element discretization of joints and 

structural elements is produced automatically from their geometric description via 

appropriate code that has been developed, while ABAQUS/Standard software is used for 

the numerical analyses [1-2]. 


Hybrid models have been developed with beam-column elements for the structural 

members and detailed modeling of the joints according to section 3.2.1 with shell elements. 

Proper compatibility constraints are assumed at the nodes of the interfaces, while the 

length of the detailed joint part (beam/column) is taken as 0.10 of the corresponding total 

member length. There are also some results from simple models with beam-column 

elements for the members and no specific modeling of the joints (regarded as rigid). 

Nonlinear static analyses under horizontal loads taking into consideration P-delta effects 

have performed. The pushover analyses distribution of the horizontal loads is considered 

triangular along the height of the structure, while the base joints are fixed. Two different 

frame models are examined with the connections as shown below and steel grade S235. A 

bilinear stress-strain relationship is assumed with E = 21000 kN/cm 2 , fy = 23.5 kN/cm 2 , fu = 

36.0 kN/cm 2 and εu = 0.25. The elastic modulus E of bolts is taken equal to 21000 kN/cm 2 , 

while the strain-hardening modulus Est = 210 kN/cm 2 for every diameter and grade. 

Transverse web stiffeners are added to the columns at the height of the beam flanges (ts = 

tfb), while in next step supplementary web plates are added to the column webs (t’wc = 3 twc) 

for the decrease of the panel zone deformations. Full finite element models with shell 

elements for the structural members (beams and columns) are examined in the next chapter 

where nonlinear dynamic analyses are performed. Hybrid models give the same results 

with the full models at reduced computational times. It should be mentioned that the 

simulation of joints with three-dimensional solid elements according to section 3.2.2 in a 

frame model requires excessive computational time to perform static and dynamic analyses 

that take into account material and geometric nonlinearities including contacts. The 

simulation with structural elements is practically and computationally more efficient, even 

though there are some drawbacks in the modeling. 

61

Chapter 4 Static analysis of steel frames 

4.3 Frame A 

62 

Fig. 4.1: Connections of Frame A & B respectively 

The first steel frame has four openings (4 x 7m = 28m) and three stories (3 x 4m = 12m) as 

shown in Fig. 4.2. Columns have a section profile HEB320 and beams IPE400. Details of 

the beam-to-column connections are shown in Fig. 4.1. Each beam is assumed to have 20 

times higher weight to account for the floor mass (~ 36000kg), while each column carries 

its own weight. The first two natural periods of the frame are 0.60 and 0.20 seconds 

respectively, while the corresponding modes are shown in Figs. 4.4 and 4.5. 

Fig. 4.2: Finite element model of Frame A

Static analysis of steel frames Chapter 4 

Fig. 4.3: Frame A, finite element model of double-sided joint 

Fig. 4.4: First natural mode of Frame A (T = 0.60 sec) 

63


64 

Fig. 4.5: Second natural mode of Frame A (T = 0.18 sec) 

The results of various response analyses are presented in the next figures. In Fig. 4.6 a 

parametric study of bolts diameter is presented with a constant end-plate thickness equal to 

25 mm and bolts grade 8.8, while in Fig. 4.7 there is a parametric analysis of end-plate 

thickness with a constant bolts diameter equal to 24 mm (M24) and bolts grade 8.8. In both 

cases, the influence of column web panel deformations is examined via appropriate 

stiffening of it with supplementary web plates (realized by thickness increase of the 

column web shell elements). These analyses show that adding column supplementary web 

plates (cswp, with final web thickness t’wc = 3 twc) to the joints is very effective, decreasing 

the shear deformation of the column web panel zones and improving the overall behavior 

of the frame. Then, joints inelastic response is dominated by the connection rotational 

deformation. Hence, early bolt failures appear (shown with circles on the graphs). The 

drawback of modeling bolted beam-to-column joints with shell and beam elements appears 

in Fig. 4.7 (see also FS1 in section 3.4). When the stiffness of the end-plate becomes very 

low compared with the stiffness of the column web panel zone and the bolts, the local 

concentration of stresses at the end-plate nodes that the bolts are connected leads to 

premature plastic deformations (see black dashed curve). Finally, the analysis with beamcolumn 

elements regarding the joints as rigid gives an elastic response that coincides with 

this of hybrid models with stiffened joints, but underestimates the final strength of the 

frame. This can be attributed to various factors. One of them is the little higher in-plane 

bending strength of the column edges above and below the joints due to the thickness 

increase of the corresponding shell elements which simulate the column web of the 

detailed parts (the thickness increase is not applied only between the transverse web 

stiffeners (see Fig. 4.3).


Base Shear [kN] 


1200 

1000 

800 

600 

4 x 3 frame - End plate t = 25 mm 

400 

Bolts M16 

Bolts M16 + cswp 

Bolts M20 


200 

Bolts M24 


Beam-Column elements 

0 

0 50 100 150 

Roof Displacement [cm] 

1200 

1000 

800 

600 

Fig. 4.6: Bolts diameter parametric analysis of Frame A 

4 x 3 frame - Bolts M24 8.8 

400 

End-plate 15 mm 

End-plate 15 mm + cswp 



200 




0 

0 50 100 150 


Fig. 4.7: End-plate thickness parametric analysis of Frame A 

In the next figures (4.8-11), von Mises stress distributions are presented at the last/failure 

step of the nonlinear static analysis plotted on the deformed shape of each model with 

deformation scale factor equal to one. The stress contours are plotted in scale 0-23.5 

kN/cm 2 according to the steel nominal yield stress. Particularly, the frame whose 

connections have end-plate thickness equal to 25 mm and bolts M20 is shown with and 

without column supplementary web plates (cswp). The effect of panel zone deformations, 

(which depend on its stiffness and strength) on the overall joint behavior is observed. 

65


Figs. 4.8-9: Frame A, t=25mm, D=20mm, von Mises stresses distribution (stress scale 0: fy, 

deformation scale factor: 1) 

66


Figs. 4.10-11: Frame A, t=25mm, D=20mm, + cswp, von Mises stresses distribution (stress 

scale 0: fy, deformation scale factor: 1) 

67


4.4 Frame B 

The second frame has three openings (3 x 6m = 18m) and six stories (6 x 4m = 24m) as 

shown in Fig. 4.8. Columns have a section profile HEA400 and beams IPE330. Details of 

the beam-to-column connections are shown in Fig. 4.1. Each beam is assumed to have 10 

times higher weight to account for the floor mass (~ 8500kg), while each column carries its 

own weight. The first two natural periods of the frame are 0.80 and 0.25 seconds 

respectively, while the corresponding modes are shown in Figs. 4.10 and 4.11. 

68 

Figs. 4.12-13: Finite element model of Frame B


Fig. 4.14: First natural mode of Frame B (T = 0.80 sec) 

Fig. 4.15: Second natural mode of Frame B (T = 0.25 sec) 

69


The results of various response analyses are presented in the next figures. In Fig. 4.12 a 

parametric study of bolts diameter is presented with a constant end-plate thickness equal to 

20 mm and bolts grade 8.8, while in Fig. 4.13 there is a parametric analysis of end-plate 

thickness with a constant bolts diameter equal to 20 mm (M20) and bolts grade 8.8. In both 

cases, the influence of column web panel deformations is examined via appropriate 

stiffening of it with supplementary web plates (realized by thickness increase of the 

column web shell elements). These analyses show that adding column supplementary web 

plates (cswp, with final web thickness t’wc = 3 twc) to the joints is effective for the overall 

behavior of the structure, but not in the extent of Frame A (see Figs. 4.6, 4.7) because of 

the higher shear strength of the columns profile and the lower depth of the beams. But 

looking at Figs. 4.18-21, the effect of these plates on the stresses distribution of joints is 

high. Failure of beam edges is observed via development of plastic hinges due to the 

stiffening/strengthening of the column web panel zone. Two cases of early bolt failures 

appear (shown with circles on the graphs). The analysis with beam-column elements 

regarding the joints as rigid gives an elastic response that coincides with this of hybrid 

models with stiffened joints, but underestimates the final strength of the frame. 

70 



700 

600 

500 

400 

3 x 6 frame - End plate t = 20 mm 

300 

200 

Bolts M16 


Bolts M20 


100 

Bolts M24 



0 

0 50 100 150 200 250 


700 

600 

500 

400 

Fig. 4.16: Bolts diameter parametric analysis of Frame B 

3 x 6 frame - Bolts M20 8.8 

300 

200 





100 




0 

0 50 100 150 200 250 


Fig. 4.17: End-plate thickness parametric analysis of Frame B


Figs. 4.18-19: Frame B, t=20mm, D=20mm, von Mises stresses distribution (stress scale 0: 

fy, deformation scale factor: 1) 

71


Figs. 4.20-21: Frame B, t=20mm, D=20mm, + cswp, von Mises stresses distribution (stress 

scale 0: fy, deformation scale factor: 1) 

72


Chapter 5 

Dynamic Analysis of Steel Frames 

Multistory steel frames with detailed modeling of their connections according to Chapter 3 

are subjected to seismic excitation in order to examine the influence of the rigidity of joints 

on the dynamic response of moment-resistant steel structures [24-29]. Parametric studies 

are performed demonstrating how variations of geometric characteristics of joint 

components can change the connection behavior and consequently the seismic response of 

steel frames. Moreover, various finite element simulations are investigated in order to find 

hybrid models of detailed finite element simulation of joints combined with beam 

simulation for the structural elements in an effort to combine accuracy and low 

computational cost. The finite element discretization of joints and structural elements is 

produced automatically from their geometric description via appropriate code that has been 

developed, while ABAQUS/Standard software is used for the time-history numerical 

analyses of this chapter [1-2]. 


Three different finite element simulations are examined: 

a. Type 1: Simulation with beam elements for the members, while the joints are regarded 

as rigid; 

b. Type 2: Full simulation with shell elements for the members and detailed modeling of 

the joints according to section 3.2.1 with shell and beam elements; and 

c. Type 3: Hybrid simulation with beam elements for the members and detailed modeling 

of the joints according to 3.2.1 with shell and beam elements. For this type of modeling 

proper compatibility constraints are assumed at the nodes of the interfaces. The length 

of the detailed joint part (beam/column) is taken as 0.10 of the corresponding total 

member length. The joints of this frame type are stiffened in two steps. In the first step 

(Type 3 – stiff-a), transverse web stiffeners are added to the columns at the height of the 

beam flanges (ts = tfb), and in the second (Type 3 – stiff-b), apart from these stiffeners, 

supplementary web plates are added to the column webs (t’wc = 2 twc). 

It should be mentioned that the simulation with three-dimensional solid elements 

requires excessive computational time to perform an implicit direct-integration dynamic 

analysis that takes into account material and geometric nonlinearities including contacts. 

The simulation with structural elements is practically and computationally more efficient, 

even though there are some drawbacks in the modeling. 

The hysteretic stress-strain model that has been adopted for the steel subjected to 

dynamic loading is displayed in Fig. 5.1. The steel grade specified for every component of 

each model, except for the bolts, is S235 with the following characteristics: modulus of 

elasticity, E = 21000 kN/cm 2 , yield stress, fy = 23.5 kN/cm 2 , ultimate stress, fu = 36.0 

kN/cm 2 , and ultimate strain, εu = 0.25. The grade of bolts is 8.8 which means that fy.b = 

73

Dynamic analysis of steel frames Chapter 5 

be taken conservatively as 6% = 0.06. In the analyses of this thesis, only α1 is used with α1 

= 0.0020 for the first frame test example and α1 = 0.0025 for the second. 

The frames are subjected to the 1940 Imperial Valley (El Centro) S00E horizontal 

component acceleration record. The 10 seconds acceleration history is shown in Fig. 5.2, 

while Fig. 5.3 depicts the response spectra for 2% and 6% damping. Peak ground 

acceleration (PGA) of 0.60g is chosen for the numerical analyses of the frames that follow. 

PSA [cm/sec 2 ] 

Ground Acceleration [cm/sec 2 ] 

400 

300 

200 

100 

0 

-100 

-200 

-300 

0 10 20 30 

Time [sec] 

40 50 60 

1400 

1200 

1000 

800 

600 

400 

200 

Fig. 5.2: Acceleration time history of El Centro 

0 

0 0.5 1 1.5 

T [sec] 

2 2.5 3 

Fig. 5.3: Response Spectra of El Centro 

= 2% 

= 6% 

75

Chapter 5 Dynamic analysis of steel frames 

5.3 Frame 1 

A steel frame of one opening (6 m) and two storeys (5 m each) is examined. Columns have 

a section profile HEB280 and beams IPE400. Details of the beam-to-column connections 

are shown in Fig. 5.4. Parametric studies on extended end-plate thickness, t, and bolts 

diameter, D, are performed. Each beam is assumed to have 20 times higher density than the 

density of steel (7850 kg/m 3 ) to account for the floor mass, while each column carries its 

own weight. 

76 

Fig. 5.4: Bolted extended end-plate beam-to-column connection 

The natural frequencies and periods are demonstrated in Table 5.1, while the first two 

modes are shown in Figs 5.5 and 5.6 for the full (Type 2) and the hybrid (Type 3) frame 

simulation. 

Simulation type t (mm) D (mm) σ1 (rad/s) σ2 (rad/s) T1 (sec) T2 (sec) 

1 - - 13.04 42.10 0.48 0.15 

2 15 20 12.44 42.42 0.50 0.15 

2 20 20 12.52 42.58 0.50 0.15 

3 15 20 12.54 42.99 0.50 0.15 

3 20 20 12.62 43.16 0.50 0.15 

Table 5.1: Frame 1, Dynamic characteristics


Fig. 5.5: Frame 1, 1 st mode 

Fig. 5.6: Frame 1, 2 nd mode 

The results of various response analyses are presented in the next figures. The parametric 

analyses (Figs. 5.7, 5.8) show that connection geometric characteristics do not affect the 

overall behavior of the frame with regard to the absolute maximum values. The tests 

performed showed that hybrid simulation is reliable and can be used instead of the full 

simulation, assuming that member beam elements do not exceed the yield stress, fy, in 

order to account for the excessive computational effort required to perform nonlinear 

dynamic analyses with detailed finite element models. The comparisons between the 

different simulations are presented in Figs. 5.9-11. 

77


Fig. 5.7: Frame 1, Simulation type 2, parametric analysis of end-plate thickness (2 nd floor) 

Fig. 5.8: Frame 1, Simulation type 2, parametric analysis of bolts diameter (2 nd floor) 

78 

Relative Displacement [cm] 


15 

10 

5 

0 

-5 

-10 

-15 

Bolts D = 20 mm 

-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

15 

10 

5 

0 

-5 

-10 

-15 

End-plate t = 15 mm 

Simulation type t (mm) D (mm) Iterations Total CPU Time (sec) 

1 - - 1007 20 

2 15 20 5018 8561 

3 15 20 5002 5281 

3 – stiff-a 15 20 4930 5688 

3 – stiff-b 15 20 4593 5363 

Table 5.2: Frame 1, CPU times 







-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10




6 

4 

2 

0 

-2 

-4 

Bolts D = 20 mm & End-plate t = 15 mm 

-6 

Simulation type 1 



-8 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

15 

10 

5 

0 

-5 

-10 

-15 

-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

Fig. 5.9-10: Frame 1, Comparison of simulation types (1 st & 2 nd floor respectively) 


15 

10 

5 

0 

-5 

-10 

-15 








Simulation type 3 - stiff-a 

Simulation type 3 - stiff-b 

-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

Fig. 5.11: Frame 1, Influence of joint rigidity (2 nd floor) 

79


5.4 Frame 2 

A steel frame of two openings (6 m each) and three storeys (4 m each) is examined. There 

are also double-sided joints apart from single-sided of Frame No1. Columns have a section 

profile HEB280 and beams IPE400. Beam-to-column connections are shown in Fig. 5.4. 

Parametric studies on extended end-plate thickness, t, and bolts diameter, D, are 

performed. Each beam is assumed to have 20 times higher density than the density of steel 

(7850 kg/m 3 ) to account for the floor mass, while each column carries its own weight. The 

natural frequencies and periods are demonstrated in Table 5.3, while the first two modes 

are shown in Figs 5.12-15 for the full (Type 2) and the hybrid (Type 3) frame simulation. 

80 

Fig. 5.12: Frame 2, 1 st mode, Simulation type 2 

Fig. 5.13: Frame 2, 1 st mode, Simulation type 3


Fig. 5.14: Frame 2, 2 nd mode, Simulation type 2 

Fig. 5.15: Frame 2, 2 nd mode, Simulation type 3 

Simulation type t (mm) D (mm) σ1 (rad/s) σ2 (rad/s) T1 (sec) T2 (sec) 

1 - - 10.66 34.25 0.59 0.18 

2 15 20 10.00 33.51 0.63 0.19 

2 20 20 10.10 33.79 0.62 0.19 

3 15 20 10.10 34.01 0.62 0.18 

3 20 20 10.20 34.29 0.62 0.18 

Table 5.3: Frame 2, Dynamic characteristics 

81


The results of the dynamic response of this test frame are presented in the next figures. 

Parametric analyses (Figs. 5.16 and 5.17) show that the geometric characteristics of the 

connections do not affect the overall behavior of the frame. As in the previous example, 

hybrid simulation is reliable and can be used instead of the full simulation. As the size of 

the problem increases, the computational effort required to perform nonlinear time-history 

dynamic analysis with a detailed finite element model increases and the adoption of hybrid 

models becomes very useful and effective. For example, the time needed for a full 

simulation with shell elements of this frame is ~ 1.5 times greater than the time needed for 

a hybrid simulation. The comparisons between the different simulations are presented in 

Figs. 5.18-21. 

Fig. 5.16: Frame 2, Simulation type 3, parametric analysis of end-plate thickness (3 rd floor) 

82 



15 

10 

5 

0 

-5 

-10 

-15 





-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

15 

10 

5 

0 

-5 

-10 

-15 





-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

Fig. 5.17: Frame 2, Simulation type 3, parametric analysis of bolts diameter (3 rd floor)





6 

4 

2 

0 

-2 

-4 

-6 





-8 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

15 

10 

5 

0 

-5 

-10 





-15 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

15 

10 

5 

0 

-5 

-10 

-15 





-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

Fig. 5.18-20: Frame 2, Comparison of simulation types (1 st , 2 nd and 3 rd floor) 

83


84 


15 

10 

5 

0 

-5 

-10 


-15 



Simulation type 3 - stiff-a 

Simulation type 3 - stiff-b 

-20 

0 1 2 3 4 5 

Time [sec] 

6 7 8 9 10 

Fig. 5.21: Frame 2, Influence of joint rigidity (3 rd floor) 

Simulation type t (mm) D (mm) Iterations Total CPU Time (sec) 

1 - - 1021 44 

2 15 20 5401 22747 

3 15 20 5368 15396 

3 25 20 5694 17320 

3 – stiff-a 25 20 5420 18232 

3 – stiff-b 25 20 5390 18018 

Table 5.4: Frame 2, CPU times 

Finally, there are some stress distributions for this frame at 2.20 seconds which are 

presented in the next graphs. When the joints are not stiffened, the column web panels 

present high shear stresses, while when they are stiffened, the beam flanges yield and the 

connection rotational deformation becomes significant. The effect of column web panel 

deformations can be shown also from Fig. 5.21. So, in many practical cases, the panel zone 

can dominate the inelastic response of a steel moment frame, and accurate panel zone 

models are needed to realistically predict overall frame performance. Another detailed 

model that uses beam-column elements for the structural members and appropriate 

simulation of the panel zones is shown in Fig. 5.26 [26]. The panel zones are modeled 

using a combination of the standard beam-column module and the rotational spring 

module. The model uses rigid beam-column elements to form a parallelogram of 

dimensions db (depth of beam) by dc (depth of column). The panel zone shear strength and 

stiffness can be modeled by providing a trilinear rotational spring (for monotonic loading) 

in any of the four corners as shown in Fig. 5.26. Usually, two bilinear springs are 

superimposed to model the trilinear behavior. The remaining three corners are modeled as 

simple pin connections. The boundary elements for the panel zone model are rigid beamcolumn 

elements with very high axial and flexural rigidity. The properties for the rotational 

spring(s) that model the shear strength and stiffness of the panel zone are evaluated using 

the principle of virtual work applied to a deformed configuration of the panel zone.


Fig. 5.22: Frame 2, t=25mm, D=20mm, von Mises stresses distribution (t = 2.20 sec, stress 

scale 0: fy), simulation type 3 


scale 0: fy), simulation type 3 

85



scale 0: fy), simulation type 3 – stiff-b 


scale 0: fy), simulation type 3 – stiff-b 

86


Fig. 5.26: Analytical model for panel zone [26] 

87

Chapter 5 

Conclusions 

Detailed finite element modeling considering material and geometric nonlinearities 

including appropriate contacts of bolted extended end-plate beam-to-column joints is 

performed, which can capture all local phenomena that affect the behavior of the joints 

under static or dynamic loads. 

Experimental results can be reproduced accurately using detailed joint models of 

hexahedral eight-node solid continuum finite elements with either reduced integration 

or incompatible modes depending on the plate thickness. 

Simulation with shell elements can be used for the modeling of steel joints with high 

level of accuracy in realistic problems, instead of continuum elements, which are 

computationally very demanding. 

Hybrid frame models, where the joints are modeled with shell elements and the 

connecting structural elements with beam elements, with appropriate kinematic 

constraints at the nodes of the interfaces, give reliable results at reduced computational 

times. 

Modeling of frames with beam-column elements considering rigid joints fails to predict 

the semi-rigidity and the various types of failure of the joint structural components that 

may affect considerably the joint behavior. Detailed joint models with appropriate 

simulation of the panel zone (shear deformation) and the connections (rotational 

deformation) should be used instead. 

The shear deformation of the column web panel zone of a joint is of equal importance 

to the connection rotational deformation and can dominate the inelastic response of a 

moment frame. Hence, joint modeling is needed to realistically predict the overall 

frame performance. 

Pushover analyses of steel moment frames show that stiffness and strength of the 

column web panel zone is of major importance for the overall response of a moment 

frame. 

Parametric studies on extended end-plate thickness and bolts diameter of semi-rigid 

joints show that the connection geometric characteristics do not have a substantial 

effect on the seismic response of the overall structure, especially compared with the 

corresponding effect of the column web panel zone. 

89

REFERENCES 

[1] ABAQUS version 6.5, Analysis User’s Manual. 2004 

[2] ABAQUS version 6.10, Analysis User’s Manual. 2010 

[3] European Committee for Standardization (CEN), EN 1993-1-1 – Eurocode 3: Design 

of Steel Structures – Part 1.1: General Rules and Rules for Buildings. 2005 


of Steel Structures – Part 1.5: Plated Structural Elements. 2005 


of Steel Structures – Part 1.8: Design of Joints. 2005 

[6] K.J. Bathe, Finite Element Procedures. Prentice-Hall, 1996 

[7] Anil K. Chopra, Dynamics of Structures, Theory and Applications to Earthquake 

Engineering, 3 rd edition. Pearson Prentice Hall, 2007 

[8] Darko Beg, Erik Zupancic, Ioannis Vayas, On the rotation capacity of moment 

connections. Journal of Constructional Steel Research, 60, 601-620, 2004 

[9] Minas E. Lemonis, Charis J. Gantes, Mechanical modeling of the nonlinear response 

of beam-to-column joints. Journal of Constructional Steel Research, 65, 879-890, 

2009 

[10] M.R. Bahaari, A.N. Sherbourne, Computer modelling of an extended end-plate 

bolted connection. Computers and Structures, 52(5), 879-893, 1994 

[11] Archibald N. Sherbourne & Mohammed R. Bahaari, 3D simulation of bolted 

connections to unstiffened columns – I. T-stub connections. Journal of 

Constructional Steel Research, 40(3), 169-187, 1996 

[12] Archibald N. Sherbourne & Mohammed R. Bahaari, 3D simulation of bolted 

connections to unstiffened columns – II. Extended endplate connections. Journal of 

Constructional Steel Research, 40(3), 189-223, 1996 

[13] Mohammed R. Bahaari, Archibald N. Sherbourne, Behavior of eight-bolt large 

capacity endplate connections. Computers and Structures, 77, 315-325, 2000 

[14] O.S. Bursi & J.P. Jaspart, Benchmarks for finite element modelling of bolted steel 

connections. Journal of Constructional Steel Research, 43(Nos. 1-3), 17-42, 1997 

[15] O.S. Bursi & J.P. Jaspart, Calibration of a finite element model for isolated bolted 

end-plate steel connections. Journal of Constructional Steel Research, 44(3), 225- 

262, 1997 

[16] O.S. Bursi, J.P. Jaspart, Basic issues in the finite element simulation of extended end 

plate connections. Computers and Structures, 69, 361-382, 1998 

[17] Y.I. Maggi, R.M. Goncalves, R.T. Leon, R.F.L. Ribeiro, Parametric analysis of steel 

bolted end plate connections using finite element modeling. Journal of 

Constructional Steel Research, 61, 689-708, 2005 

[18] Anant R. Kukreti, Feng-Feng Zhou, Eight-bolt endplate connection and its influence 

on frame behavior. Engineering Structures, 28, 1483-1493, 2006 

[19] Charis J. Gantes, Minas E. Lemonis, Influence of equivalent bolt length in finite 

element modeling of T-stub steel connections. Computers and Structures, 81, 595- 

604, 2003 

[20] Ana M. Girao Coelho, Frans S. K. Bijlaard, Luis Simoes da Silva, Experimental 

assessment of the ductility of extended end plate connections. Engineering 

Structures, 26, 1185-1206, 2004 

[21] Ana M. Girao Coelho, Frans S.K. Bijlaard, Experimental behaviour of high strength 

steel end-plate connections. Journal of Constructional Steel Research, 63, 1228- 

1240, 2007 

91

[22] L.R.O. de Lima, L. Simoes da Silva, P.C.G. da S. Vellasco, S.A.L. de Andrade, 

Experimental evaluation of extended endplate beam-to-column joints subjected to 

bending and axial force. Engineering Structures, 26, 1333-1347, 2004 

[23] Yongjiu Shi, Gang Shi, Yuanqing Wang, Experimental and theoretical analysis of 

the moment-rotation behaviour of stiffened extended end-plate connections. Journal 

of Constructional Steel Research, 63, 1279-1293, 2007 

[24] Gang Shi, Yongjiu Shi, Yuanqing Wang, Behaviour of end-plate moment 

connections under earthquake loading. Engineering Structures, 29, 703-716, 2007 

[25] A.S. Elnashai & A.Y. Elghazouli, Seismic Behaviour of Semi-rigid Steel Frames. 

Journal of Constructional Steel Research, 29, 149-174, 1994 

[26] Akshay Gupta, Helmut Krawinkler, Seismic demands for performance evaluation of 

steel moment resisting frame structures. The John A. Blume Earthquake Engineering 

Center, Report No. 132, 1999 

[27] H. Krawinkler and S. Mohasseb, Effects of panel zone deformations on seismic 

response. Journal of Constructional Steel Research, 8, 233-250, 1987 

[28] Akshay Gupta and Helmut Krawinkler, Estimation of seismic drift demands for 

frame structures. Earthquake Engineering and Structural Dynamics, 29, 1287-1305, 

2000 

[29] Kee Dong Kim, Michael D. Engelhardt, Monotonic and cyclic loading models for 

panel zones in steel moment frames. Journal of Constructional Steel Research, 58, 

605-635, 2002 

[30] Marc Braham, Jean-Pierre Jaspart, Is it safe to design a building structure with 

simple joints, when they are known to exhibit a semi-rigid behaviour? Journal of 

Constructional Steel Research, 60, 713-723, 2004 

[31] A.A. Vrakas & M. Papadrakakis, A study of the influence of the rigidity of joints on 

the dynamic response of steel structures. 3 rd ECCOMAS Thematic Conference on 

Computational Methods in Structural Dynamics and Earthquake Engineering 

(COMPDYN 2011), Corfu, Greece, 25-28 May 2011 

[32] A.A. Vrakas, A.G. Papachristidis & M. Papadrakakis, Detailed finite element 

analysis of steel moment frames. 7 th National Conference on Steel Structures, Volos, 

Greece, 29-30 Sep. & 1 Oct. 2011 

92

Nonlinear Static and Dynamic Analysis of Steel Structures with ...

You also want an ePaper? Increase the reach of your titles

Delete template?

Save as template?