Theoretical background

Introduction

Bar members are preferred by engineers when designing steel structures. However, there are many locations on the structure where the theory of members is not valid, e.g., welded joints, bolted connections, footing, holes in walls, the tapering height of cross-section and point loads. The structural analysis in such locations is difficult and it requires special attention. The behavior is non-linear and the nonlinearities must be respected, e.g., yielding of the material of plates, contact between end plates or base plate and concrete block, one-sided actions of bolts and anchors, welds. Design codes, e.g. EN1993-1-8, and also technical literature offer engineering solution methods. Their general feature is derivation for typical structural shapes and simple loadings. The method of components is used very often.

Component method

The component method (CM) solves the joint as a system of interconnected items – components. The corresponding model is built per each joint type to be able to determine forces and stresses in each component – see the following picture.

The components of a joint with bolted end plates modeled by springs

Each component is checked separately using corresponding formulas. As the proper model must be created for each joint type, the method usage has limits when solving joints of general shapes and general loads.

IDEA StatiCa together with a project team of Department of Steel and Timber Structures of Faculty of Civil Engineering in Prague and Institute of Metal and Timber Structures of Faculty of Civil Engineering of the Brno University of Technology developed a new method for advanced design of steel structural joints.

The new Component Based Finite Element Model (CBFEM) method is:

• General enough to be usable for most of the joints, footings, and details in engineering practice.
• Simple and fast enough in daily practice to provide results in a time comparable to current methods and tools.
• Comprehensive enough to provide structural engineer clear information about joint behavior, stress, strain, and reserves of individual components and about overall safety and reliability.

The CBFEM method is based on the idea that most of the verified and very useful parts of CM should be kept. The weak point of CM – its generality when analyzing stresses of individual components – was replaced by modeling and analysis using the Finite Element Method (FEM).

FEM is a general method commonly used for structural analysis. The usage of FEM for modeling of joints of any shapes seems to be ideal (Virdi, 1999). The elastic-plastic analysis is required, as the steel ordinarily yields in the structure. In fact, the results of the linear analysis are useless for joint design.

FEM models are used for research purposes of joint behavior, which usually apply spatial elements and measured values of material properties.

FEM model of a joint for research. It uses spatial 3D elements for both plates and bolts

Both webs and flanges of connected members are modeled using shell elements in the CBFEM model for which the known and verified solution is available.

The fasteners – bolts and welds – are the most difficult in the point of view of the analysis model. Modeling of such elements in general FEM programs is difficult because the programs do not offer the required properties. Thus, special FEM components had to be developed to model the welds and bolts behavior in a joint.

CBFEM model of bolted connection by end plates

Joints of members are modeled as massless points when analyzing steel frame or girder structure. Equilibrium equations are assembled in joints and internal forces on ends of beams are determined after solving the whole structure. In fact, the joint is loaded by those forces. The resultant of forces from all members in the joint is zero – the whole joint is in equilibrium.

The real shape of a joint is not known in the structural model. The engineer only defines whether the joint is assumed to be rigid or hinged.

It is necessary to create a trustworthy model of joint, which respect the real state, to design the joint properly. The ends of members with the length of a 2-3 multiple of maximal cross-section height are used in the CBFEM method. These segments are modeled using shell elements.

A theoretical (massless) joint and real shape of the joint without modified member ends

For better precision of the CBFEM model, the end forces on 1D members are applied as loads on the segment ends. Sextuplets of forces from the theoretical joint are transferred to the end of the segment – the values of forces are kept, but the moments are modified by the actions of forces on corresponding arms.

The segment ends at the joint are not connected. The connection must be modeled. So-called manufacturing operations are used in the CBFEM method to model the connection. Manufacturing operations are especially: cuts, offsets, holes, stiffeners, ribs, end plates and splices, cleats, gusset plates, and others. Fastening elements (welds and bolts) are also added.

IDEA StatiCa Connection can perform two types of analysis:

1. Geometrically linear analysis with material and contact nonlinearities for stress and strain analysis,
2. Eigenvalue analysis to determine the possibility of buckling.

In the case of connections, the geometrically nonlinear analysis is not necessary unless plates are very slender. Plate slenderness can be determined by eigenvalue (buckling) analysis. For the limit slenderness where geometrically linear analysis is still sufficient, see Chapter 3.9. The geometrically nonlinear analysis is not implemented in the software.

Material model

The most common material diagrams which are used in finite element modeling of structural steel are the ideal plastic or elastic model with strain hardening and the true stress-strain diagram. The true stress-strain diagram is calculated from the material properties of mild steels at an ambient temperature obtained in tensile tests. The true stress and strain may be obtained as follows:

\[ \sigma_{true}=\sigma (1 + \epsilon) \]

\[ \epsilon_{true}=\ln (1 + \epsilon) \]

where σ_true is true stress, ε_true true strain, σ engineering stress, and ε engineering strain.

The plates in IDEA StatiCa Connection are modeled with elastic-plastic material with a nominal yielding plateau slope according to EN1993-1-5, Par. C.6, (2), tan^-1 (E/1000). The material behavior is based on the von Mises yield criterion. It is assumed to be elastic before reaching the design yield strength, f_yd.

The ultimate limit state criterion for regions not susceptible to buckling is reaching the limiting value of the principal membrane strain. The value of 5 % is recommended (e.g. EN1993-1-5, App. C, Par. C.8, Note 1).

Material diagrams of steel in numerical models

The limit value of plastic strain is often discussed. In fact, the ultimate load has low sensitivity to the limit value of plastic strain when the ideal plastic model is used. It is demonstrated in the following example of a beam to a column joint. An open section beam IPE 180 is connected to an open section column HEB 300 and loaded by bending moment. The influence of the limit value of plastic strain on the resistance of the beam is shown in the following figure. The limit plastic strain changes from 2 % to 8 %, but the change in moment resistance is less than 4 %.

An example of prediction of ultimate limit state of a beam to column joint

The influence of the limit value of plastic strain on the moment resistance

Plate model and mesh convergence

Plate model

Shell elements are recommended for modeling of plates in the FEA of structural connection. 4-node quadrangle shell elements with nodes at its corners are applied. Six degrees of freedom are considered in each node: 3 translations (u_x, u_y, u_z) and 3 rotations (φ_x, φ_y, φ_z). Deformations of the element are divided into the membrane and the flexural components.

The formulation of the membrane behavior is based on the work by Ibrahimbegovic (1990). Rotations perpendicular to the plane of the element are considered. Complete 3D formulation of the element is provided. The out-of-plane shear deformations are considered in the formulation of the flexural behavior of an element based on Mindlin hypothesis. The MITC4 elements are applied, see Dvorkin (1984). The shell is divided into five integration layers through thickness of the plate at each integration point and plastic behavior is analyzed in each point. It is called Gauss–Lobatto integration. The nonlinear elastic-plastic stage of material is analyzed in each layer based on the known strains. Only the maximum stresses and strains of all layers are shown.

Mesh convergence

There are some criteria for the mesh generation in the connection model. The connection check should be independent of the element size. Mesh generation on a separate plate is problem-free. The attention should be paid to complex geometries such as stiffened panels, T-stubs and base plates. The sensitivity analysis considering mesh discretization should be performed for complicated geometries.

All plates of a beam cross-section have a common division into elements. The size of generated finite elements is limited. The minimal element size is set to 10 mm and the maximal element size to 50 mm (can be set in Code setup). Meshes on flanges and webs are independent of each other. The default number of finite elements is set to 8 elements per cross-section height as shown in the following figure. The user can modify the default values in Code setup.

The mesh on a beam with constraints between the web and the flange plate

The mesh of the end plates is separate and independent of other connection parts. Default finite element size is set to 16 elements per cross-section height as shown in the figure.

The mesh on an end plate with 7 elements along its width

The following example of a beam to column joint shows the influence of mesh size on the moment resistance. An open section beam IPE 220 is connected to an open section column HEA 200 and loaded by a bending moment as shown in the following figure. The critical component is the column panel in shear. The number of the finite elements along the cross-section height varies from 4 to 40 and the results are compared. Dashed lines are representing the 5%, 10%, and 15% difference. It is recommended to subdivide the cross-section height into 8 elements.

A beam to column joint model and plastic strains at ultimate limit state

The influence of the number of elements on the moment resistance

The mesh sensitivity study of a slender compressed stiffener of column web panel is presented. The number of elements along the width of the stiffener varies from 4 to 20. The first buckling mode and the influence of a number of elements on the buckling resistance and critical load are shown in the following figure. The difference of 5% and 10% is displayed. It is recommended to use 8 elements along the stiffener width.

The first buckling mode and the influence of number of elements along the stiffener on the moment resistance

The mesh sensitivity study of a T-stub in tension is presented. Half of the flange width is subdivided into 8 to 40 elements and the minimal element size is set to 1 mm. The influence of the number of elements on the T-stub resistance is shown in the following figure. The dashed lines are representing the 5%, 10%, and 15% difference. It is recommended to use 16 elements on the half of the flange width.

The influence of the number of elements on the T-stub resistance

Contacts

The standard penalty method is recommended for modeling of a contact between plates. If penetration of a node into an opposite contact surface is detected, penalty stiffness is added between the node and the opposite plate. The penalty stiffness is controlled by a heuristic algorithm during the nonlinear iteration to get a better convergence. The solver automatically detects the point of penetration and solves the distribution of contact force between the penetrated node and nodes on the opposite plate. It allows creating contact between different meshes as shown. The advantage of the penalty method is the automatic assembly of the model. The contact between the plates has a major impact on the redistribution of forces in connection.

An example of separation of plates in contact between the web and flanges of two overlapped Z sections purlins

It is possible to add contact between

• two surfaces,
• two edges,
• edge and surface.

An example of edge to edge contact between the seat and the end plate

An example of edge to surface contact between the lower flange of the beam and the column flange

Welds

There exist several options how to treat welds in numerical models. The large deformations make the mechanical analysis more complex and it is possible to use different mesh descriptions, different kinetic and kinematic variables and constitutive models. The different types of geometric 2D and 3D models and thereby finite elements with their applicability for different accuracy levels are generally used. Most often used material model is the common rate-independent plasticity model based on von Mises yield criterion. Two approaches that are used for welds are described. Residual stress and deformation caused by welding are not assumed in the design model.

The load is transmitted through force-deformation constraints based on the Lagrangian formulation to opposite plate. The connection is called multi-point constraint (MPC) and relates the finite element nodes of one plate edge to another. The finite element nodes are not connected directly. The advantage of this approach is the ability to connect meshes with different densities. The constraint allows to model midline surface of the connected plates with the offset, which respects the real weld configuration and throat thickness. The load distribution in the weld is derived from the MPC, so the stresses are calculated in the throat section. This is important for the stress distribution in the plate under the weld and for modeling of T-stubs.

Plastic stress redistribution in welds

The model with only multi-point constraints does not respect the stiffness of the weld and the stress distribution is conservative. Stress peaks that appear at the end of plate edges, in corners and rounding, govern the resistance along the whole length of the weld. To eliminate the effect, a special elastoplastic element is added between the plates. The element respects the weld throat thickness, position and orientation. The equivalent weld solid is inserted with the corresponding weld dimensions. The nonlinear material analysis is applied and elastoplastic behavior in equivalent weld solid is determined. The plasticity state is controlled by stresses in the weld throat section. The stress peaks are redistributed along the longer part of the weld length.

The elastoplastic model of welds gives real values of stress and there is no need to average or interpolate the stress. Calculated values at the most stressed weld element are used directly for checks of the weld component. This way, there is no need to reduce the resistance of multi-oriented welds, welds to unstiffened flanges or long welds.

Constraint between weld element and mesh nodes

General welds, while using plastic redistribution, can be set as continuous, partial and intermittent. Continuous welds are over the whole length of the edge, partial allows user to set offsets from both sides of the edge, and intermittent welds can be additionally set with a set length and a gap.

Bolts

In the Component-Based Finite Element Method (CBFEM), bolt with its behavior in tension, shear, and bearing is the component described by the dependent nonlinear springs. The bolt in tension is described by spring with its axial initial stiffness, design resistance, initialization of yielding and deformation capacity. The axial initial stiffness is derived analytically in the guideline VDI2230. The model corresponds to experimental data, see Gödrich et al. (2014). For the initialization of yielding and deformation capacity, it is assumed that plastic deformation occurs in the threaded part of the bolt shank only.

Force-deformation diagram for bearing of the plate

The force-deformation diagram is constructed using the following equations:

Elastic stiffness:

\( k=\frac{E A_s}{L_b} \)

Plastic stiffness:

\[ k_t = c_1 k \]

Force at the elastic limit:

\[ F_{t,el} = \frac{F_{t,Rd}}{c_1 c_2 - c_1 +1} \]

Deformation at elastic limit:

\[ u_{el} = \frac{ F_{t,el} }{k} \]

Deformation at plastic limit:

\[ u_{t,Rd} = c_2 u_{el} \]

where:

• E – modulus of elasticity of the bolt
• A_s – cross-section area of the bolt effective in tension (threaded area)
• L_b – elongation length, i.e. bolt grip length (sum of plate thicknesses clamped by the bolt), thickness of washers, half the thickness of the nut, and half the thickness of the bolt head
• F_t,Rd – bolt design resistance in tension
• \( c_1 = \frac{R_m - R_e}{\frac{1}{4} A E - R_e} \)
• \( c_2 = \frac{AE}{4 R_e} \)

Only the compression force is transferred from the bolt shank to the plate in the bolt hole. It is modeled by interpolation links between the shank nodes and holes edge nodes. The deformation stiffness of the shell element modeling the plates distributes the forces between the bolts and simulates the adequate bearing of the plate.

Bolt holes are considered as standard (default) or slotted (can be set in plate editor). Bolts in standard holes can transfer shear force in all directions, bolts in slotted holes have one direction excluded and can move in this selected direction freely.

Interaction of the axial and the shear force can be introduced directly in the analysis model. Distribution of forces reflects the reality better (see enclosed diagram). Bolts with a high tensile force take less shear force and vice versa.

Example of interaction of axial and shear force (EC)

Preloaded bolts

Preloaded bolts are used in cases when minimization of deformation is needed. The tension model of a bolt is the same as for standard bolts. The shear force is not transferred via bearing but via friction between gripped plates.

The design slip resistance of a preloaded bolt is affected by an applied tensile force.

IDEA StatiCa Connection checks the pre-slipping limit state of preloaded bolts. If there is a slipping effect, bolts do not satisfy the check. Then the post-slipping limit state should be checked as a standard bearing check of bolts where bolt holes are loaded in bearing and bolts in shear.

The user can decide which limit state will be checked. Either it is resistance to major slip or post-slipping state in shear of bolts. Both checks on one bolt are not combined in one solution. It is assumed that bolt has a standard behaviour after a major slip and can be checked by the standard bearing procedure.

The moment load of connection has a small influence on the shear capacity. Nevertheless, a friction check on each bolt simply is solved separately. This check is implemented in FEM component of the bolt. There is no information in a general way whether the external tension load of each bolt is from the bending moment or from the tension load of connection.

Stress distribution in standard and slip-resistant shear bolt connection

Anchor bolts

The anchor bolt is modeled with the similar procedures as the structural bolts. The bolt is fixed on one side to the concrete block. Its length, L_b, used for bolt stiffness calculation is taken as a sum of half of the nut thickness, washer thickness, t_w, base plate thickness, t_bp, grout or gap thickness, t_g, and free the length embedded in concrete which is expected as 8d where d is a bolt diameter. The factor 8 is editable in Code setup. This value is in accordance with the Component Method (EN1993-1-8); the free length embedded in concrete can be modified in Code setup. The stiffness in tension is calculated as k = E A_s / L_b. The load-deformation diagram of the anchor bolt is shown in the following figure. The values according to ISO 898:2009 are summarized in the table and in formulas below.

Load–deformation diagram of the anchor bolt

\[ F_{t,el}=\frac{F_{t,Rd}}{c_1 c_2 - c_1 + 1} \]

\[ k_t = c_1 k; \qquad c_1 = \frac{R_m - R_e}{\left ( \frac{1}{4} A - \frac{R_e}{E} \right )E} \]

\[ u_{el} = \frac{F_{t,el}}{k}; \qquad u_{t,Rd} = c_2 u_{el}; \qquad c_2 = \frac{AE}{4R_e} \]

where:

• A – elongation
• E – Young's modulus of elasticity
• F_t,Rd – steel tensile resistance of anchor
• R_m – ultimate (tensile) strength
• R_e – yield strength

The stiffness of the anchor bolt in shear is taken as the stiffness of the structural bolt in shear.

Anchor bolts with stand-off

Anchors with stand-off can be checked as a construction stage before the column base is grouted or as a permanent state. Anchor with stand-off is designed as a bar element loaded by shear force, bending moment and compressive or tensile force. These internal forces are determined by finite element model. The anchor is fixed on both sides, one side is 0.5×d below the concrete level, the other side is in the middle of the thickness of the plate. The buckling length is conservatively assumed as twice the length of the bar element. Plastic section modulus is used. The forces in anchor with stand-off are determined using finite element analysis. Bending moment is dependent on the stiffness ratio of anchors and base plate.

Anchors with stand-off – determination of lever arm and buckling lengths; stiff anchors are safe assumption

Concrete block

Design model

In CBFEM, it is convenient to simplify the concrete block as 2D contact elements. The connection between the concrete and the base plate resists in compression only. Compression is transferred via Winkler-Pasternak subsoil model which represents deformations of the concrete block. The tension force between the base plate and concrete block is carried by the anchor bolts. The shear force is transferred by friction between a base plate and a concrete block, by shear key and by bending of anchor bolts and friction. The resistance of bolts in shear is assessed analytically. Friction and shear key are modeled as a full single point constraint in the plane of the base plate – concrete contact.

Deformation stiffness

The stiffness of the concrete block may be predicted for the design of column bases as an elastic hemisphere. A Winkler-Pasternak subsoil model is commonly used for a simplified calculation of foundations. The stiffness of subsoil is determined using modulus of elasticity of concrete and the effective height of a subsoil as:

\[ k = \frac{E_c}{(\alpha_1 + \upsilon) \sqrt{\frac{A_eff}{A_ref}}} \left( \frac{1}{\frac{h}{a_2 d} + a_3}+a_4 \right) \]

where:

• k – stiffness of concrete subsoil in compression
• E_c – modulus of elasticity of concrete
• υ – Poisson's coefficient of the concrete block
• A_eff – effective area in compression
• A_ref = 10 m² – reference area
• d – base plate width
• h – concrete block height
• a₁ = 1.65; a₂ = 0.5; a₃ = 0.3; a₄ = 1.0 – coefficients

SI units must be used in the formula, the resulting unit is N/m³.

Transfer of shear load at the base plate

The shear load at the base plate can be transferred by three means:

• Friction
• Shear lug
• Anchors

User can choose the mean by editing the base plate operation. No combination of means is allowed in the software, however, EN 1993-1-8 – Cl. 6.2.2 and Fib 58 – Chapter 4.2 allows for the combination of shear transfer by anchors and friction under certain conditions. In general, it is conservative to neglect friction in the design of the anchorage, although it may in some cases lead to an underestimation of concrete cracking at the serviceability level. As a rule, frictional resistance should be neglected if:

• the thickness of the grout layer exceeds one-half the anchor diameter,
• the anchorage capacity is governed by a near-edge condition,
• the anchorage is intended to resist earthquake loads.

The combination with shear lug should never be allowed due to the deformation compatibility.

Transfer of shear load by friction

The shear resistance is equal to the resistance safety factor multiplied by friction coefficient editable in Code setup and compressive load. The compressive load includes all forces, e.g. in case of a column base loaded by compressive force and bending moment, the compressive load used for frictional shear resistance might be higher than the applied compressive force.

Transfer of shear load by shear lug

The shear lug is simulated as a stub encased in concrete under the base plate. The shear load is estimated to be transferred by uniform load distribution acting on the whole portion of the shear lug embedded in concrete block, i.e. all nodes of the shear lug below the concrete surface are uniformly loaded. The portion of the shear lug above the concrete surface in grout is not assumed to transfer the shear load.

Be aware that the lever arm between the applied shear load (at the base plate) and the shear resistance (half-height of the shear lug embedded in concrete) causes a bending moment which must be transferred by compressive force in concrete and tensile forces in anchors.

The shear lug consists of shell finite elements and is checked as regular plates. Also, the welds of the shear lug to the base plate are checked using standard procedures in IDEA Connection. Manual calculation usually assumes beam theory for the shear lug, although it is not accurate because the length to width ratio is very small for shear lug. Therefore, there might be a significant difference between IDEA Connection and manual calculation.

Transfer of shear load by anchors

The shear resistance is determined by the shear resistance of anchors. The steel resistance of anchors have elastoplastic load-deformation curve but the concrete failure modes are considered as perfectly brittle.

Analysis model

The newly developed method (CBFEM – Component Based Finite Element Model) enables fast analysis of joints of several shapes and configurations. The model consists of members, to which the load is applied, and manufacturing operations (including stiffening members), which serve to connect members to each other. Members must not be confused with manufacturing operations because their cut edges are connected via rigid links to the connection node so they are not deformed properly if used instead of manufacturing operations (stiffening members).

The analyzed FEM model is generated automatically. The designer does not create the FEM model, he creates the joint using manufacturing operations – see the figure.

Manufacturing operations/items which can be used to construct the joint

Each manufacturing operation adds new items to the connection – cuts, plates, bolts, welds.

Bearing member and supports

One member of the joint is always set as “bearing”. All other members are “connected”. The bearing member can be chosen by the designer. The bearing member can be “continuous” or “ended” in the joint. “Ended” members are supported on one end, “continuous” members are supported on both ends.

Connected members can be of several types, according to the load, which the member can take:

• Type N-Vy-Vz-Mx-My-Mz – member is able to transfer all 6 components of internal forces
• Type N-Vy-Mz – member is able to transfer only loading in XY plane – internal forces N, V_y, M_z
• Type N-Vz-My – member is able to transfer only loading in XZ plane – internal forces N, V_z, M_y
• Type N-Vy-Vz – member is able to transfer only normal force N and shear forces V_y and V_z

Plate to plate connection transfers all components of internal forces

Fin plate connection can transfer only loads in XZ plane – internal forces N, V_z, M_y

Gusset connection – connection of truss member can transfer only axial force N and shear forces Vy and Vz

Each joint is in the state of equilibrium during the analysis of the frame structure. If the end forces of the individual members are applied to detailed CBFEM model, the state of equilibrium is met too. Thus, it would not be necessary to define supports in analysis model. However, for practical reasons, the support resisting all translations is defined in the first end of the bearing member. It does influence neither the state of stress nor the internal forces in the joint, only the presentation of deformations.

Appropriate support types respecting the type of the individual members are defined at the ends of the connected members to prevent the occurrence of unstable mechanisms.

The default length of each member is twice its height. The length of a member should be at least 1× the height of the member after the last manufacturing operation (weld, opening, stiffener etc.) due to the correct deformations after the rigid links connecting the cut end of a member to the connection node.

Equilibrium in node

Each node of the 3D FEM model must be in equilibrium. The equilibrium requirement is correct, nevertheless, it is not necessary for the design of simple joints. One member of the joint is always „bearing“ and the others are connected. If only the connection of connected members is checked, it is not necessary to keep the equilibrium. Thus, there are two modes of load input available:

• Simplified – for this mode, the bearing member is supported (continuous member on both sides) and the load is not defined on the member
• Advanced (exact with equilibrium check) – the bearing member is supported on one end, the loads are applied to all members and the equilibrium has to be found

The mode can be switched in the ribbon group Loads in equilibrium.

The difference between the modes is shown in the following example of T-connection. The beam is loaded by the end bending moment of 41 kNm. There is also a compressive normal force of 100 kN in the column. In the case of simplified mode, the normal force is not taken into account because the column is supported on both ends. The program shows only the effect of bending moment of the beam. Effects of normal force are analyzed only in the full mode and they are shown in results.

Simplified input: normal force in column is NOT taken into account

Advanced input: normal force in column is taken into account

The simplified method is easier for the user but it can be used only when the user is interested in studying connection items and not the behavior of the whole joint.

For cases where the bearing member is heavily loaded and close to its limit capacity, the advanced mode with respecting all the internal forces in the joint is necessary.

Loads

The end forces of a member of the frame analysis model are transferred to the ends of member segments. Eccentricities of the members caused by the joint design are respected during transfer.

The analysis model created by CBFEM method corresponds to the real joint very precisely, whereas the analysis of internal forces is performed on much idealized 3D FEM bar model, where individual beams are modeled using center lines and the joints are modeled using immaterial nodes.

Joint of a vertical column and a horizontal beam

The internal forces are analyzed using 1D members in the 3D model. There is an example of the internal forces in the following figure.

Internal forces in horizontal beam; M and V are the end forces at joint

The effects caused by a member on the joint are important to design the joint (connection). The effects are illustrated in the following figure:

Effects of the member on the joint; CBFEM model is drawn in dark blue color

Moment M and shear force V act in the theoretical joint. The point of the theoretical joint does not exist in the CBFEM model, thus the load cannot be applied here. The model must be loaded by actions M and V which have to be transferred to the end of segment in the distance r

M_c = M – V ∙ r

V_c = V

In the CBFEM model, the end section of the segment is loaded by moment M_c and force V_c.

When designing the joint, its real position relative to the theoretical point of joint must be determined and respected. The internal forces in the position of the real joint are mostly different from the internal forces in the theoretical point of joint. Thanks to the precise CBFEM model, the design is performed on reduced forces – see moment M_r in the following figure:

Bending moment on CBFEM model: The arrow points to the real position of connection

When loading the joint, it must be respected that the solution of the real joint must correspond to the theoretical model used for calculation of internal forces. This is fulfilled for rigid joints but the situation may be completely different for hinges.

Position of hinge in theoretical 3D FEM model and in the real structure

It is illustrated in the previous figure that the position of the hinge in the theoretical 1D members model differs from the real position in the structure. The theoretical model does not correspond to reality. When applying the calculated internal forces, a significant bending moment is applied to the shifted joint and the designed joint is overlarge or cannot be designed either. The solution is simple – both models must correspond. Either the hinge in 1D member model must be defined in the proper position or the shear force must be shifted to get a zero moment in the position of the hinge.

Shifted distribution of bending moment on beam: zero moment is at the position of the hinge

The shift of the shear force can be defined in the table for the internal forces definition.

The location of load effect has a big influence on the correct design of the connection. To avoid all misunderstandings, we allow the user to select from three options – Node / Bolts / Position.

Note that when selecting the Node option, the forces are applied at the end of a selected member which is usually at the theoretical node unless the offset of the selected member is set in geometry.

Import loads from FEA programs

IDEA StatiCa enables to import internal forces from third-party FEA programs. FEA programs use an envelope of internal forces from combinations. IDEA StatiCa Connection is a program which resolves steel joint nonlinearly (elastic/plastic material model). Therefore, the envelope combinations cannot be used. IDEA StatiCa searches for extremes of internal forces (N, V_y, V_z, M_x, M_y, M_z) in all combinations at the ends of all members connected to the joint. For each such extreme value, also all other internal forces from that combination in all remaining members are used. Idea StatiCa determines the worst combination for each component (plate, weld, bolt etc.) in the connection.

The user can modify this list of load cases. He can work with combinations in the wizard (or BIM) or he can delete some cases directly in IDEA StatiCa Connection.

Warning!

It is necessary to take into account unbalanced internal forces during the import. This can happen in following cases:

• Nodal force was applied to the position of the investigated node. The software cannot detect which member should transfer this nodal force and, therefore, it is not taken into account in the analysis model. Solution: Do not use nodal forces in global analysis. If necessary, the force must be manually added to a selected member as a normal or shear force.
• Loaded, non-steel (usually timber or concrete) member is connected to the investigated node. Such member is not considered in the analysis and its internal forces are ignored in the analysis. Solution: Replace the concrete member with a concrete block and anchorage.
• The node is a part of a slab or a wall (usually from concrete). The slab or the wall is not part of the model and its internal forces are ignored. Solution: Replace the concrete slab or wall with a concrete block and anchorage.
• Some members are connected to the investigated node via rigid links. Such members are not included in the model and their internal forces are ignored. Solution: Add these members into the list of connected members manually.
• Seismic load cases are analysed in the software. Most FEA software offer the modal analysis to solve seismicity. The results of internal forces of seismic load cases provide usually only internal force envelopes in sections. Due to the evaluation method (square root of the sum of squares – SRSS), the internal forces are all positive and it is not possible to find the forces matching to the selected extreme. It is not possible to achieve a balance of internal forces. Solution: Change the positive sign of some internal forces manually.

Strength analysis

The analysis of joint is materially non-linear. The load increments are applied gradually and the state of stress is searched. There are two optional analysis modes in IDEA Connection:

• The response of structure (joint) to the overall load. All defined load (100 %) is applied in this mode and the corresponding state of stress and deformation is calculated.

• Analysis termination at reaching the ultimate limit state. The checkbox in Code setup “Stop at limit strain” should be ticked. The state is found when the plastic strain reaches the defined limit. In the case when the defined load is higher than the calculated capacity, the analysis is marked as non-satisfying and the percentage of used load is printed. Note that the analytical resistance of components, for example of bolts, can be exceeded.

The second mode is more suitable for a practical design. The first one is preferable for detailed analysis of complex joints.

Stiffness analysis

The CBFEM method enables to analyze the stiffness of connection of individual joint members. For the proper stiffness analysis, the separate analysis model must be created for each analyzed member. Then, the stiffness analysis is not influenced by the stiffness of other members of joint but only by the node itself and the construction of connection of the analyzed member. Whereas the bearing member is supported for the strength analysis (member SL in the figure below), all members except the analyzed one are supported by the stiffness analysis (see two figures below for stiffness analysis of members B1 and B3).

Supports on members for strength analysis

Loads can be applied only on the analyzed member. If bending moment, M_y, is defined, the rotational stiffness about the y-axis is analyzed. If bending moment M_z is defined, the rotational stiffness about the z-axis is analyzed. If axial force N is defined, the axial stiffness of connection is analyzed.

The program generates complete diagram automatically, it is directly displayed in GUI and can be added into the output report. Rotational or axial stiffness can be studied for specific design load. IDEA StatiCa Connection can also deal with the interaction of the other internal forces.

Diagram shows:

• Level of design load M_Ed
• Limit value of capacity of connouection for 5% equivalent strain M_j,Rd; limit for plastic strain may be changed in Code setup
• Limit value of capacity of connected member (useful also for seismic design) M_c,Rd
• 2/3 of limit capacity for calculation of initial stiffness
• Value of initial stiffness S_j,ini
• Value of secant stiffness S_js
• Limits for the classification of connection – rigid and pinned
• Rotational deformation Φ
• Rotational capacity Φ_c

Rigid welded connection

Semi-rigid bolted connection

After reaching the 5 % strain in the column web panel in shear, the plastic zones propagate rapidly.

The joint is classified according to its stiffness into rigid, semi-rigid or pinned category according to the relevant code. The theoretical length of the member can be set for the analyzed member:

Member capacity design

IDEA Connection checks the connection on applied design load. In many regions with the danger of seismicity, it is required to check the connection on the maximal moment which can be transferred by the connected member. We calculate this moment in the software and apply it to the specific member. All other members in the joint are supported.

The value of M_y is calculated automatically using full cross-section of the analyzed member and strength properties according to the selected code. User can modify this number, e.g. in case of reduction of the beam cross-section, and can add for example shear force calculated from applied loads and the distance between plastic hinges.

Joints designed to transfer moment equal to the member resistance (full-strength joints) usually need to be much more stiffened than the partial-strength joints.

Connected member is not checked. It has to be properly designed in the global analysis of the structure.

Joint design resistance

The designer usually solves the task to design the connection/joint to transfer the known design load. But it is also useful to know how far the design from the limit state is, i.e., how big the reserve in the design is and how safe it is. This can be done simply by the type of analysis – Design joint resistance.

The user inputs design load like in a standard design. The software automatically proportionally increases all load components until one of the checks does not satisfy. The checks of steel plates, shear and tension resistance of bolts, and approximate weld checks are included. Note that in this analysis type, some checks are neglected, e.g. bearing resistance of bolts. The user gets the ratio of maximal load to the design load. Also, a simple diagram is provided. It is necessary to perform Stress/Strain analysis for accurate joint assessment.

Gusset plate as an elongation of a truss – example of plate from group 1 for which buckling can be neglected if critical buckling factor is higher than 15

Examples of buckling shapes of plates from group 2 where the buckling can be neglected if critical buckling factor is higher than 3

The model used for buckling analysis is supported by different supports than set by the user in stress, strain analysis type (EPS). The bearing member stays fully supported. Model type of a beam set as N-Vy-Vz-Mx-My-Mz (free to move in stress, strain analysis type) is fully supported in buckling analysis. All other beam analysis types have restrained bending moments and normal force but are free to move sideways.

• Model type N-Vy-Vz-Mx-My-Mz: supports in buckling model: N-Vy-Vz-Mx-My-Mz
• Model type N-Vy-Vz: supports in buckling model: N-Mx-My-Mz
• Model type N-Vz-My: supports in buckling model: N-Mx-My-Mz
• Model type N-Vy-Mz: supports in buckling model: N-Mx-My-Mz

It is assumed that in case of rigid joint, user sets bending moment and the buckling of the short beam segment is not relevant. On the other hand, in the case of pinned joint, user sets only normal and shear force and no bending moment but the buckling of the pinned member is relevant so it contributes to the buckling factor. See the figure below. "Model" shows the model in stress strain analysis type and "Buckling" shows the model in the buckling analysis.

Deformation capacity

The deformation capacity/ductility δ_Cd belongs with the resistance and the stiffness to the three basic parameters describing the behavior of connections. In moment-resistant connections, the ductility is achieved by a sufficient rotation capacity φ_Cd. The deformation/rotation capacity is calculated for each connection in the joint separately.

The estimation of the rotation capacity is important in connections exposed to seismic, see Gioncu and Mazzolani (2002) and Grecea (2004) and extreme loading, see Sherbourne and Bahaari (1994 and 1996). The deformation capacity of components has been studied from the end of the last century (Foley and Vinnakota, 1995). Faella et al. (2000) carried out tests on T-stubs and derived the analytical expressions for the deformation capacity. Kuhlmann and Kuhnemund (2000) performed tests on the column web subjected to transverse compression at different levels of compression axial force in the column. Da Silva et al. (2002) predicted deformation capacity at different levels of axial force in the connected beam. Based on the test results combined with FE analysis, deformation capacities are established for the basic components by analytical models by Beg et al. (2004). In the work, components are represented by non-linear springs and appropriately combined in order to determine the rotation capacity of the joint for the end-plate connections, with an extended or flush end-plate and welded connections. For these connections, the most important components that may significantly contribute to the rotation capacity were recognized as the web in compression, column web in tension, column web in shear, column flange in bending, and end-plate in bending. Components related to the column web are relevant only when there are no stiffeners in the column that resist compression, tension or shear forces. The presence of a stiffener eliminates the corresponding component, and its contribution to the rotation capacity of the joint can be therefore neglected. End-plates and column flanges are important only for end-plate connections where the components act as a T-stub, where also the deformation capacity of the bolts in tension is included. The questions and limits of deformation capacity of connections of high strength steel were studied by Girao et al. (2004).

Analysis convergence

Finite element analysis requires slightly increasing stress-strain diagram of material models. In some cases of complicated models, e.g. with multiple contacts, the increase in divergent iterations might help with convergence. This value can be set in Code setup. Most common causes of analysis failure are singularities when the parts of a model are not connected properly and are free to move or rotate. A user is notified and should check the model for missing welds or bolts. The deformed shape is shown with the items which caused the first singularity moved 1 m so that singularity may be easily detected.

Missing welds at gusset plates leading to singularity

Thin-walled members

Software IDEA StatiCa Connection is dedicated to assessment of connections of hot-rolled members which are not significantly affected by buckling. Geometrically linear and materially non-linear analysis is performed because of its fast and stable calculation. However, this analysis is not sufficient for stability loss. If buckling may be a problem, performing a linear buckling analysis helps to detect dangerous areas and provide a factor for Euler’s bifurcation point but this is still not enough for thin-walled members. For thin-walled members, only geometrically nonlinear analysis with imperfections is suitable.

If the user still decides to use IDEA StatiCa Connection software to check connections of thin-walled members, he should:

• Perform linear buckling analysis and carefully evaluate each buckling shape, the first 5 presented buckling shapes might not be enough
• Do not rely on plasticity of steel plates and rather limit the von Mises stress to yield strength or even lower
• Be aware that local buckling which is not taken into account can redistribute internal forces in components differently
• Be aware that stiffness of components may be different due to different failure modes or their combination.
• Be aware that presented checks and detailing of components (e.g. bolts, welds) are following guides for standard members. The checks for thin-walled members may vary and then the provided checks are not correct.

The design of connections of thin-walled members is very case specific and no general guide can be provided. IDEA StatiCa Connection was not validated for this use.

Component checks – EN

In EN 1993-1-1 thin-walled members are defined as: “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.” The main part of Eurocode for steel is limited to members with material thickness t ≥ 3 mm. The chapter 4 – Welded connections applies only to material thickness of t ≥ 4 mm. Therefore, the checks of components provided by software do not apply to cold-formed members with smaller thickness. User should be aware of this and replace the checks with appropriate formulas from EN 1993-1-3 manually.

Analysis of hollow section joints should be also carefully performed for members which are out of the range of validity for welded joints – EN 1993-1-8 – Table 7.1. There are no guidelines for such joints and results of the software have not been validated.

Component checks – AISC

In Chapter A of AISC 360-16 there is a user note stating: “For the design of cold-formed steel structural members, the provisions in the AISI North American Specification for the Design of Cold-Formed Steel Structural Members (AISI S100) are recommended, except for cold-formed hollow structural sections (HSS), which are designed in accordance with this Specification.” AISI S100 and AS/NZS 4600 provide formulas to determine the shear and tension resistance of most common fastener types together with their range of application

Component checks – CISC

CSA S16-14 states in Chapter 1: “Requirements for steel structures such as bridges, antenna towers, offshore structures, and cold-formed steel structural members are given in other CSA Group Standards.”

Joints of hollow section cross-section members

Out-of-plane deformation

One of the criteria for the ultimate limit state of hollow section joints is the out-of-plane deformation of the hollow section cross-section. The check is available in the software. It is recognized by CIDECT design guides. The limits are 3 % of the smaller size of the cross-section (0.03 d₀ for CHS and 0.03 b₀ for RHS) for the ultimate limit state and 1 % for the serviceability limit state.

Definition of cross-section sizes for circular hollow section (CHS) and rectangular hollow section (RHS)

Typical load-deformation diagrams for hollow section joints; the red curve is for thin-walled member loaded in compression, the green curve for regular members loaded in compression, the blue curve is e.g. for X-joint loaded by tension

Geometrically and materially non-linear analysis (GMNA)

In the case of some joints of hollow sections, especially with high diameter to thickness ratio, the geometrically linear analysis may not capture the behavior of the joint with sufficient precision and its load resistance may be underestimated or overestimated. It is recommended to use more advanced geometrically and materially nonlinear analysis for joints of hollow sections even though the computational time is slightly higher. If GMNA analysis for hollow sections is selected in Code setup, GMNA is used instead of geometrically linear and materially nonlinear analysis (MNA, used as a standard in IDEA Statica Connection) for models with hollow section member as a bearing member.