IDEA StatiCa Connection Theoretical background

Dit artikel is ook beschikbaar in

General introduction

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.

CBFEM Components

Materiaal model

De meest voorkomende materiaaldiagrammen die worden gebruikt bij het modelleren van eindige elementen van constructiestaal zijn het ideale plastisch of elastisch model met een bijbehorend spanning-rek diagram. Het werkelijke spanning-rek diagram wordt berekend uit de materiaaleigenschappen van staal bij een omgevingstemperatuur verkregen in trektests. De werkelijke spanning en rek kunnen als volgt worden verkregen:

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

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

waar σtrue is true stress, εtrue true strain, σ engineering spanning, and ε engineering rek.

De platen in IDEA StatiCa Connection zijn gemodelleerd met elastisch-plastisch materiaal  volgens 

EN1993-1-5, Par. C.6, (2), tan-1 (E/1000). Het materiaalgedrag is gebaseerd op het von Mises vloeicriterium. Aangenomen wordt dat het elastisch is voordat de ontwerpvloeigrens wordt bereikt, fyd.

Het uiterste grenstoestand criterium voor gebieden die niet vatbaar zijn voor knik, is het bereiken van de grenswaarde van de rek. De waarde van 5% wordt aanbevolen ( EN1993-1-5, App. C, Par. C.8, Note 1).

spannings-rek diagram van materiaal model in CBFEM IDEA CONNECTION

Materiaal diagram of steel in numerical models

De grenswaarde van plastische rek wordt vaak besproken. In feite heeft de uiteindelijke belasting een lage gevoeligheid voor de grenswaarde van plastische rek wanneer het ideale plastisch model wordt gebruikt. Het wordt gedemonstreerd in het volgende voorbeeld van een ligger-kolomverbinding. Een IPE 180 is verbonden met HEB 300 en belast door een buigend moment. De invloed van de grenswaarde van plastische rek op de weerstand van de balk wordt weergegeven in de volgende afbeelding. De limiet plastische rek verandert van 2% naar 8%, maar de verandering in momentweerstand is minder dan 4%.

knoopbelasting, spanningsweergave in platen en rekweergave in IDEA CONNECTION

Een voorbeeld van voorspelling de UGT van een ligger-kolom verbinding in staal 

Plastiche rek weerstand van de verbinding in IDEA CONNECTION

De invloed van de limiet waarde van plastische rek op het momentweerstand

Plate model and mesh convergence

Increase in number of elements provides more precise results but at the cost of higher computational demand.

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 (ux, uy, uz) and 3 rotations (φx, φy, φz). 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

The stresses in contacts may be visualized and the values are shown in the check table of plates. However, the contact stresses are only informative and are not used in any check. Also, the through-thickness stress of shell elements is not considered. 

Lassen

Er bestaan verschillende opties om lassen te benaderen in numerieke modellen. De grote vervormingen maken de mechanische analyse complexer en het is mogelijk om verschillende mesh-beschrijvingen, verschillende kinetische en kinematische variabelen en constitutieve modellen te gebruiken. Over het algemeen worden de verschillende soorten geometrische 2D- en 3D-modellen en daarmee eindige elementen met hun toepasbaarheid voor verschillende nauwkeurigheidsniveaus gebruikt. Het meest gebruikte materiaalmodel is het gebruikelijke plasticiteitsmodel op basis van het von Mises-vloeicriterium. Er worden twee benaderingen beschreven die voor lassen worden gebruikt. Restspanning en vervorming veroorzaakt door lassen worden niet verondersteld in het ontwerpmodel.

De belasting wordt overgedragen via kracht-vervormingsbeperkingen op basis van de Lagrangiaanse formulering op de tegenoverliggende plaat. De verbinding wordt multi-point constraint (MPC) genoemd en relateert de eindige-elementknooppunten van de ene plaatrand aan de andere. De eindige elementen knooppunten zijn niet direct verbonden. Het voordeel van deze aanpak is de mogelijkheid om EE_netten met verschillende dichtheden te verbinden. De constraint maakt het mogelijk om het middenlijnoppervlak van de verbonden platen te modelleren met de offset, waarbij de werkelijke lasconfiguratie en lasdikte worden gerespecteerd. De belastingsverdeling in de las wordt afgeleid van de MPC, dus de spanningen worden berekend in het keelgedeelte. Dit is belangrijk voor de spanningsverdeling in de plaat onder de las en voor het modelleren van T-stubs.

Plastische herverdeling van spanningen in lassen

Het model met alleen multi-point constraints houdt geen rekening met de stijfheid van de las en de spanningsverdeling is conservatief. Spanningspieken die verschijnen aan het einde van plaatranden, in hoeken en afrondingen, bepalen de weerstand over de gehele lengte van de las. Om dit effect te elimineren, wordt tussen de platen een speciaal elastoplastisch element toegevoegd. Het element respecteert de dikte, positie en oriëntatie van de lasnaad. Het equivalente laslichaam wordt ingevoegd met de bijbehorende lasafmetingen. De niet-lineaire materiaalanalyse wordt toegepast en het elastoplastische gedrag in een gelijkwaardige lasmassa wordt bepaald. De plasticiteitstoestand wordt geregeld door spanningen in de lasdoorsnede. De spanningspieken worden herverdeeld over het langere deel van de laslengte.

Het elastoplastische model van lassen geeft echte spanningswaarden en het is niet nodig om de spanning te middelen of te interpoleren. Berekende waarden bij het meest belaste laselement worden direct gebruikt voor controles van de las. Op deze manier is het niet nodig om de weerstand van multi-oriented lassen, lassen aan niet-verstijfde flenzen of lange lassen te verminderen.

Lasmodel van Lasdefinitie in van elastoplastich materiaal in IDEA CONNECTION

Constraint tussen laselement en netknooppunten

Algemene lassen kunnen, terwijl ze plastische herverdeling gebruiken, worden ingesteld als continu, gedeeltelijk en onderbroken. Doorlopende lassen zijn over de gehele lengte van de rand, gedeeltelijk stelt de gebruiker in staat om offsets van beide kanten van de rand in te stellen, en onderbroken lassen kunnen bovendien worden ingesteld met een ingestelde lengte en een opening.

Bolts and preloaded bolts

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
  • As – cross-section area of the bolt effective in tension (threaded area)
  • Lb – 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
  • Ft,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 shear bolt connection

Stress distribution in 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, Lb, used for bolt stiffness calculation is taken as a sum of half of the nut thickness, washer thickness, tw, base plate thickness, tbp, grout or gap thickness, tg, 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 As / Lb. 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
  • Ft,Rd – steel tensile resistance of anchor
  • Rm – ultimate (tensile) strength
  • Re – 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. 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
  • Ec – modulus of elasticity of concrete
  • υ – Poisson's coefficient of the concrete block
  • Aeff – effective area in compression
  • Aref = 1 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

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, Vy, Mz
  • Type N-Vz-My – member is able to transfer only loading in XZ plane – internal forces N, Vz, My
  • Type N-Vy-Vz – member is able to transfer only normal force N and shear forces Vy and Vz

Plate to plate connection transfers all components of internal forces

Fin plate connection can transfer only loads in XZ plane – internal forces N, Vz, My

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

The loads in any node in the structural model need to be in equilibrium. Any unbalanced forces are taken by supports. It is recommended to use a load combination instead of internal forces envelope.

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

Mc = MVr

Vc = V

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

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 Mr 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, Vy, Vz, Mx, My, Mz) 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

Strength analysis is the most important analysis of joints. Strain check of plates together with code checks of components are performed by elastic-plastic 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 practical design. The first one is preferable for detailed analysis of complex joints.

Stijfheidsberekening en vervormingscapaciteit

Verbindingen worden geclassificeerd op basis van stijfheid tot stijf, flexibel of scharnierend. De ingenieur moet ervoor zorgen dat de stijfheid van de verbinding overeenkomt met de stijfheid waarvan uitgegaan wordt in de CAE-software.

De CBFEM-methode maakt het mogelijk om de stijfheid van de verbinding van individuele aangesloten staven te berekenen. Voor de juiste stijfheidsberekening moet voor elke geanalyseerde staaf een afzonderlijk analysemodel worden gemaakt. Vervolgens wordt de stijfheidsberekening niet beïnvloed door de stijfheid van andere verbindingselementen, maar alleen door het knooppunt zelf en de constructie van de verbinding van de berekende staaf. Terwijl de dragende staaf wordt ondersteund voor de sterkteberekening (staaf SL in de onderstaande afbeelding), worden alle staven behalve de geanalyseerde ondersteund door de stijfheidsberekening (zie twee afbeeldingen hieronder voor stijfheidsberekening van staven B1 en B3).

Sterkteberekening van de verbinding met opleggingen in IDEA CONNECTION

Opleggingen op staven voor sterkteberekening

Stijfheidsberekening van de verbinding met berekende staaf in plaats van dragende staaf
Opleggingen op staven voor stijfheidsberekening van staaf B1Opleggingen op staven voor stijfheidsberekening van staaf B3

Belastingen kunnen alleen op de berekende staaf worden toegepast. Als het buigmoment My is gedefinieerd, wordt de rotatiestijfheid rond de y-as geanalyseerd. Als het buigmoment Mz is gedefinieerd, wordt de rotatiestijfheid om de z-as geanalyseerd. Als axiale kracht N is gedefinieerd, wordt de axiale stijfheid van de verbinding geanalyseerd.

Het programma genereert automatisch een compleet diagram, het wordt direct weergegeven in de resultaten en kan worden toegevoegd aan het rapport. Rotatie- of axiale stijfheid kan worden bestudeerd voor specifieke ontwerpbelastingen. IDEA StatiCa Connection kan ook omgaan met de interactie van de andere snedekrachten.

Het diagram laat zien :

  • Niveau van ontwerpbelasting MEd
  • Grenswaarde van de capaciteit van de verbinding voor 5% equivalente rek, Mj, Rd; limiet voor plastische rek kan worden gewijzigd in Norm-instellingen
  • Grenswaarde van capaciteit van aangesloten staaf (ook nuttig voor seismisch ontwerp) Mc, Rd
  • 2/3 van de limietcapaciteit voor de berekening van de initiële stijfheid
  • Waarde van initiële stijfheid Sj, ini
  • Waarde van secant stijfheid Sjs ( op basis van de MEd)
  • Limieten voor de classificatie van verbinding - stijf en scharnierend
  • Rotatievervorming Φ
  • Rotatiecapaciteit Φc
Stijve verbinding in moment rotatie diagram in IDEA CONNECTION

Stijve gelaste verbinding

flexibele geboute verbinding in IDEA CONNECTION

Felxibele geboute verbinding

Ontwerpweerstand van de verbinding in IDEA CONNECTION

Na het bereiken van de 5% rek in het kolomlijf bij afschuiving, worden de plastische zones snel meer.

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:

De verbinding wordt op basis van zijn stijfheid geclassificeerd in starre, semi-rigide of scharnierende categorie volgens de relevante norm. De theoretische lengte van de staaf kan worden ingesteld voor de berekende staaf:

theoretische liggerlengte in IDEA CONNECTION

Vervormings capaciteit

De vervormingscapaciteit / ductiliteit δCd hoort bij de weerstand en de stijfheid bij de drie basisparameters die het gedrag van verbindingen beschrijven. Bij momentvaste verbindingen wordt de ductiliteit bereikt door voldoende rotatiecapaciteit φCd. De vervormings- / rotatie capaciteit wordt voor elke aansluiting in de verbinding afzonderlijk berekend.

De schatting van de rotatiecapaciteit is belangrijk bij verbindingen die zijn blootgesteld aan seismiek, zie Gioncu en Mazzolani (2002) en Grecea (2004) en bij extreme belasting, zie Sherbourne en Bahaari (1994 en 1996). De vervormingscapaciteit van componenten is bestudeerd vanaf het einde van de vorige eeuw (Foley en Vinnakota, 1995). Faella et al. (2000) voerden tests uit op T-stubs en leidden de analytische formules af ​​voor het vervormingsvermogen. Kuhlmann en Kuhnemund (2000) voerden tests uit op het kolomlijf dat werd onderworpen aan transversale druk op verschillende niveaus van axiale compressiekracht in de kolom. Da Silva et al. (2002) voorspelde vervormingscapaciteit op verschillende niveaus van axiale kracht in de verbonden staaf. Op basis van de testresultaten gecombineerd met FE-analyse, worden vervormingscapaciteiten voor de basiscomponenten vastgesteld door analytische modellen van Beg et al. (2004). In het werk worden componenten weergegeven door niet-lineaire veren en op de juiste manier gecombineerd om de rotatiecapaciteit van de kopplaat aansluitingenin de verbinding te bepalen, met een verlengde of vlakke kopplaat en lasverbindingen. Voor deze verbindingen werden de belangrijkste componenten die significant kunnen bijdragen aan het rotatievermogen herkend als het kolomlijf onder druk, het kolomlijf onder trek, het kolomlijf in afschuiving, de kolomflens onder buiging en de kopplaat onder buiging. Componenten die verband houden met het kolomlijf zijn alleen relevant als er geen verstijvers in de kolom zijn die weerstand bieden aan compressie-, trek- of afschuifkrachten. De aanwezigheid van een verstijver elimineert de corresponderende component, en zijn bijdrage aan het rotatievermogen van de verbinding kan daarom worden verwaarloosd. Kopplaten en kolomflenzen zijn alleen van belang voor kopplaatverbindingen waarbij de componenten fungeren als een T-stub, waarbij ook de vervormingscapaciteit van de bouten onder trek is inbegrepen. De vragen en grenzen van de vervormingscapaciteit van verbindingen van hogesterkte-staal werden bestudeerd door Girao et al. (2004).

Capacity design

Capacity design is a part of a joint check in seismic design. When relying on the ductility of a structure, the capacity design must be performed. 

The objective of capacity design is to confirm a building undergoes controlled ductile behavior in order to avoid a collapse in a design-level earthquake.

A dissipative item is selected with increased strength and modified material diagram. An overstrength factor \(\gamma_{ov}\) is defined in Materials and a strain-hardening factor \(\gamma_{sh}\) at the dissipative item operation. Note that the nomenclature differs between the codes. A dissipative item is excluded from the strain check of plates. 

Modified material diagram for dissipative item

IDEA Connection checks the connection on applied design load, which should create a plastic hinge in the selected dissipative item, usually the beam. The plastic strain in the dissipative item should be around 5 %. This can serve as a confirmation that the magnitude and position of loads were determined properly. 

Plastic hinge created at the intended place of the dissipative item – the beam

The supports of the continuous member are automatically defined as supported at one end and with restrained moments at the other end. This way, the continuous column may be loaded by normal force and shear forces and also one side may move sideways so that the failure of the column web in shear is revealed.

Note, that detailing is very important for seismic resistant joints but is not checked in IDEA StatiCa. 

Weerstand van de verbinding

Weerstand van de verbinding helpt om reserve in de verbindingsweerstand in te schatten.

De ontwerper lost meestal de taak op om de verbinding zo te ontwerpen om de ontwerpbelasting over te dragen. Maar het is ook handig om te weten hoe ver het ontwerp van de grenstoestand is, dus hoe groot de reserve in het ontwerp is en hoe veilig het is. Dit kan eenvoudig worden gedaan door het berekeningstype DR - Weerstand van de verbinding.

De gebruiker voert de ontwerpbelasting in zoals in een standaardontwerp. De software verhoogt automatisch alle belastingscomponenten proportioneel totdat een van de meegeleverde controles niet voldoet.

DR-analyses voeren controles uit op de volgende onderdelen:

  • Plastische spanning in platen 
  • Bouten - afschuiving, spanning en combinatie van spanning en afschuiving 
  • Ankers – trek- en afschuifweerstand van staal 
  • Lassen

Houd er rekening mee dat andere componenten die niet in de bovenstaande lijst zijn opgenomen, niet worden gecontroleerd vanwege onbekende richtingen van krachten in componenten. Voer daarom altijd een EPS-analyse uit om er zeker van te zijn dat alle controles correct worden uitgevoerd. 

De gebruiker krijgt de verhouding  te zien in procenten tussen de maximale belasting en de ontwerpbelasting. Er wordt ook een eenvoudige grafiek gegeven.

UItvoer van ontwerpweerstand van de staalverbinding van IDEA CONNECTION

De resultaten van door de gebruiker gedefinieerde belastinggevallen worden weergegeven, tenzij de gezamenlijke ontwerpweerstandsfactor kleiner is dan 100 %, wat betekent dat de berekening niet voldoet aan de ontwerpbelasting en de laatste geconvergeerde stap van het belastinggeval wordt dan weergegeven.

Buckling analysis

Buckling is usually not an important issue in joints however, it should be checked that there are no buckling issues and the results of strength analysis, which uses only geometrically linear analysis, are correct.

IDEA StatiCa Connection is able to perform linear buckling analysis of a model of a joint. The results are predicted in buckling modes. Critical load, at which buckling of perfect model occurs, is calculated for each buckling mode. Critical load is presented by multipliers of the load acting on the joint. According to the buckling mode and critical load multiplier, the user can determine the safe buckling design.

Some codes, e.g. Eurocode (EN 1993-1-1, Chapter 5.2.1), recommend a critical load multiplier higher than 15 for bar models of structures. If the critical load multiplier is higher than 15, the code does not require buckling check of members.

For joints, the matter is different and the code does not provide any specific recommendation. Design of local buckling must be tackled in another way. Generally, the local buckling may be divided into three groups:

  1. Plates connecting individual members
  2. Stiffening plates in the joint – stiffeners, ribs, short haunches
  3. Closed sections and thin-walled sections

Buckling of plates from group 1 affects the buckling shape of the whole member. Therefore, it is recommended to apply the same rules as for these members also to these plates, i.e. consider safe critical load multiplier 15 and higher. The engineer should verify that real execution of the joint corresponds to the boundary conditions of the model used for buckling analysis of the whole structure.

Plates from group 2 affect local buckling of the joint. For such plates, the safe boundary of critical load multiplier 15 is conservative, but specific guidance is missing in codes. The guidance is provided by research papers that recommend safe boundary of critical load multiplier equal to 3.

Buckling of plates and members from group 3 is very problematic and individual assessment of each particular case is necessary.

For plates with critical load multiplier smaller than suggested values (15 for group 1, 3 for group 2), plastic design cannot be used. Other methods that are not offered by IDEA StatiCa are necessary for their check.

The result of buckling analysis in IDEA Connection is not a definite check. The codes do not give sufficient guidance. The assessment requires engineering judgment and IDEA StatiCa provides unique tools not available in standard design software.

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.

Theoretische achtergrond - Convergeren van de berekening

De eindige-elementenanalyse kan om verschillende redenen niet convergeren, meestal vanwege een element dat niet voldoende wordt ondersteund en vrij kan bewegen of roteren.

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.

Eindige elementenanalyse vereist een toenemend spannings-rek diagram van materiaalmodellen. In sommige gevallen van complexe modellen, b.v. bij meerdere contacten kan een toename van divergerende iteraties helpen bij de convergentie. Deze waarde kan worden ingesteld in Code-instellingen. De meest voorkomende oorzaken van mislukte berekeningen zijn singulariteiten of instabieliteiten wanneer de onderdelen van een model niet goed zijn aangesloten en vrij kunnen bewegen of roteren. Een gebruiker wordt op de hoogte gebracht en moet het model controleren op ontbrekende lassen of bouten. De vervormde vorm wordt weergegeven met de items die de eerste singulariteit veroorzaakten, zodat singulariteit gemakkelijk kan worden gedetecteerd.

Missende lassen bij een schetsplaat zorgen voor een instabiliteit

Missende lassen bij een schetsplaat zorgen voor een instabiliteit/onvolkomendheid

Thin-walled members

IDEA Connection for design of joints of thin-walled members should be left only to experienced engineers. Buckling analysis is a must and each mode shape must be carefully analyzed.

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.”

Lateral-torsional restraint

Beams are often restrained against buckling by ceilings or cladding. Simulation of such restriction is provided by manufacturing operation Lateral-torsional restraint (LTR).

Model description

Lateral-torsional restraint is simulated by two stiffnesses added to any plate:

  • Lateral (shear) S [N] applied in the direction of y axis of plate local coordinate system
  • Torsional C [Nm/m] applied around x axis of a plate local coordinate system

Users may select any plate of a member, length of the restraint, type (continuous or discrete with set spacing), and lateral and torsional stiffnesses.

Lateral-torsional restraint

Local coordinate system of a plate with applied LTR

Nodes of finite elements are connected along the plate width by rigid body elements type 3 (RBE3) to one point at the plate longitudinal axis. Torsional stiffness is applied at this point by a special element with only one stiffness, rotation around x axis. This point is also connected by two other RBE3 with a special element between them with one stiffness, displacement in y axis. 

The lateral stiffness is set by the user as free, rigid, or with set stiffness. Rigid stiffness is sufficiently high, set as 1000 times the shear stiffness of the plate. Stiffness \(S\) is set per unit length (one meter) with a force unit [N]. The stiffness of one element \(S_i\) has a force unit divided by length unit [N/m] and is then:

\[ S_i = \frac{S}{s_d} \]

where:

  •  \(s_d\) – distance between two points [m]

For discrete type, spacing is set directly by the user. For continuous type, the spacing is sufficiently small so that the behavior of the plate is not affected by spacing.

Similarly, the torsional stiffness is set by the user as free, rigid, or with set stiffness. Rigid stiffness is sufficiently high, set as 1000 times the bending stiffness of the plate. Stiffness \(C\) is set per unit length (one meter) with a unit of bending moment divided by length unit [Nm/m]. The stiffness of one element \(C_i\) has a bending moment unit divided by length unit squared [Nm/m2] and is then:

\[ C_i = \frac{C}{s_d} \]

Hidden finite elements and RBE3 provide lateral and torsional stiffness to member plate

Note that RBE3 are only interpolation links that do not provide any stiffness on their own.

Verification

A model providing LTR was verified by LTBeam software, which uses bar (1D) elements with seven degrees of freedom. That means the cross-section is not deformed but the element can capture warping. The comparison is shown on an example of IPE 180 cross-section from steel grade S355 with a length of 6 m. The beam is fixed at both ends with a uniform load of 20 kN/m applied at the top flange. Software LTBeam is able to determine the elastic critical moment that corresponds to the result of linear buckling analysis (LBA) in IDEA StatiCa Member.

Comparison of LTBeam and IDEA StatiCa Member for lateral and torsional stiffness 

The critical load multiplier to elastic buckling \(\alpha_{cr}\) with lateral stiffness is very similar according to both software. The limit lateral stiffness where lateral-torsional buckling has an effect up to only 5 % of beam bending resistance is calculated according to EN 1993-1-1 as \(S_{lim} = 8589\, \textrm{kN}\). However, the results with torsional restraint are diverging at higher levels of rotational stiffness. Observing the deformed shape in IDEA StatiCa Member, the difference is caused by the deformation of the cross-section that can be captured only by the shell model. LTBeam provides unrealistically high critical load multipliers for high torsional stiffness. 

To verify this claim, the ABAQUS shell element model was created at ETH university. The beam is again fixed on both ends, made of steel grade S355 and with a length of 6 m. Beam cross-section IPE 240 was used. Limit torsional stiffness, i.e. lateral-torsional buckling has an effect up to only 5 % of beam bending resistance, was calculated as \(C_{lim} = 27.13\, \textrm{kNm/m}\). The model is loaded by a force in the mid-span at the top flange. 

Comparison of ABAQUS, LTBeam, and IDEA StatiCa Member for torsional stiffness

The effect of torsional stiffness is very similar in both models made of shell elements and LTBeam diverges. Most importantly, ABAQUS and IDEA StatiCa Member buckling resistances provided by GMNIA almost coincide – the differences are up to 4 %.

Stiffness estimation

LTR provided by floors filled with concrete and with composite action provided by shear studs may be assumed as rigid at least in the case of lateral stiffness. The stiffnesses provided by trapezoidal sheets of sandwich panels are much smaller and may be determined by experiments or calculations. Most often, the values of lateral and torsional stiffness would be recommended by manufacturers of sandwich panels or other types of cladding. 

The calculation of lateral stiffness S [N] provided by trapezoidal sheets is provided in EN 1993-1-3, Chapter 10:

\[S=1000 \sqrt{t^3} \left ( 50+10 \sqrt[3]{b_{roof}} \right ) \frac{s}{h_w} \]

where:

  • t – design thickness of trapezoidal sheeting [mm]
  • broof – roof width, i.e. for gable roof it is the distance between a ridge and an eave [mm]
  • s – distance between beams [mm]
  • hw – trapezoidal sheet profile depth [mm] 

The formula is valid if the trapezoidal sheet is connected to the beam at each rib. If the sheeting is connected to the beam at every second rib only, then S should be substituted by 0.2 S.

Lateral stiffness of sandwich panels is described in ECCS recommendation. The stiffness of fasteners is essential:

\[S=\frac{k_v}{2B} \sum_{k=1}^{n_k}c_k^2\]

where:

  • kv – shear stiffness of a fastening
  • B – width of a sandwich panel
  • nk – number of pairs of fasteners per panel and support
  • ck – distance between the two fasteners of a pair

Torsional stiffness is more complicated and can be also estimated by ECCS recommendation. It contains the contribution of fasteners, sandwich panel, and beam distortion. The beam distortion may be neglected because it is already included by the shell element model.

Torsional (on the left) and lateral stiffness (on the right) provided by sandwich panels (ECCS, 2014)

In American practice, restraint against lateral torsional buckling is typically assumed to be full or negligible based on the type and orientation of decking. For example, Table 8.1 of the AISC Seismic Design Manual identifies restraint conditions for beams subject to axial compression. However, where necessary, the lateral stiffness can be derived from the diaphragm stiffness, G’, computed in accordance with AISI S310. Denavit et al. (2020) present a method of calculating torsional stiffness. 

References

  • CTICM, LTBeam v. 1.0.11, available at: https://www.cesdb.com/ltbeam.html
  • Abaqus. Reference manual, version 6.16. Simulia, Dassault Systéms. France, 2016.
  • EN 1993-1-3: Eurocode 3: Design of steel structures – Part 1-3: General rules – Supplementary rules for cold-formed members and sheeting, CEN, 2006.
  • ECCS TC7 – Technical Working Group TWG 7.9 Sandwich Panels and Related Structures, European Recommendations on the Stabilization of Steel Structures by Sandwich Panels, 2nd edition, 2014. ISBN 978-90-6363-081-2
  • Denavit, M.D.; Jacobs, W.P.; Helwig, T.A. (2020). "Continuous Bracing Requirements for Constrained-Axis Torsional Buckling," Engineering Journal, American Institute of Steel Construction, Vol. 57, pp. 69-89.

Verbindingen staven met holle doorsnedes

Joints of hollow section members may undergo serious deformations while able to carry still higher loads. On the other hand, the plates may buckle in inelastic range, for which purpose, geometrically and materially nonlinear analysis is implemented.

Verbindingen van holle profielen kunnen ernstige vervormingen ondergaan terwijl ze nog hogere belastingen kunnen dragen. Aan de andere kant kunnen de platen knikken in een niet-elastisch bereik, waarvoor geometrische en materieel niet-lineaire analyse wordt geïmplementeerd.

Uit-het-vlak vervorming 

Een van de criteria voor de uiterste grenstoestand van holle profielverbindingen is de uit-het-vlak vervorming van de holle doorsnede. De controle is beschikbaar in de software (in Code Setup als Lokale vervormingscontrole, voor holle doorsnedes standaard ingeschakeld). Het wordt herkend door CIDECT design guides. De limieten zijn 3% van de kleinere afmeting van de doorsnede (0,03 d0 voor CHS en 0,03 b0 voor RHS) voor de uiterste grenstoestand en 1% voor de bruikbaarheidsgrenstoestand.

lokale vervormingen van holle doorsnedes in IDEA CONNECTION

Definitie van doorsnedematen voor ronde buisprofielen (CHS) en rechthoekige kokerprofielen (RHS)

falen van holle dunwandige doorsnedes in IDEA CONNECTION

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

Typische belastings-vervormingsdiagrammen voor buisprofiel-verbindingen; de rode curve is voor dunwandige staven die op druk worden belast, de groene curve voor normale staven die op druk worden belast, de blauwe curve is b.v. voor X-verbinding belast onder trek.

Geometrisch en materiaal niet-lineare analyse (GMNA)

In het geval van sommige verbindingen van holle profielen, vooral met een hoge diameter / dikte-verhouding, kan de geometrisch lineaire analyse het gedrag van de verbinding niet met voldoende precisie vastleggen en kan de belastingsweerstand worden onderschat of overschat. Het wordt aanbevolen om meer geavanceerde geometrische en materieel niet-lineaire analyse te gebruiken voor verbindingen van holle profielen, ook al is de rekentijd iets hoger. Als GMNA-analyse voor holle profielen is geselecteerd in norm-instellingen, wordt GMNA gebruikt in plaats van geometrisch lineaire en materieel niet-lineaire analyse (MNA, gebruikt als standaard in IDEA Statica Connection) voor modellen met hol profiel als aangesloten staaf

Vermoeiings berekeningstype

Vermoeiingsberekening dient om het normaal- en schuifspanningsbereik tussen twee lasteffecten te bepalen. De spanningen komen overeen met nominale spanningen en moeten verder worden geëvalueerd met behulp van Norm-ontwerpmethoden.

 Het moet worden gebruikt voor het ontwerp van hoogcyclische vermoeiingsdetails, waarbij geen vloeien wordt verwacht.

Het type vermoeiingsanalyse biedt geen uiteindelijke weerstand of aantal cycli dat het detail kan nemen. Het levert alleen input voor verdere berekeningen volgens de bedoelde normen.

Er moeten altijd ten minste twee belastinggevallen worden ingesteld. Het eerste belastingsgeval is de referentielast. Het wordt bijvoorbeeld aangenomen als een eigen gewicht van de constructie en kan nullasten bevatten. De andere belastinggevallen simuleren vermoeidheidsacties. De nominale normaal- en schuifspanning geleverd door IDEA StatiCa is het spanningsbereik tussen de vermoeiingsactie, b.v. LE2 en de referentielast.

De schuifspanning op een bepaalde locatie is bijvoorbeeld 50 MPa in het referentielast en 180 MPa in LE2. De weergegeven nominale schuifspanning op deze plaats is:

\[\tau = 180-50=130\, \textrm{MPa}\]

Houd er rekening mee dat platen niet mogen vloeien als gevolg van vermoeiingsacties, anders worden de spanningsbereiken vervormd. 

De spanningen zijn beschikbaar voor:

  • Bouten
  • Lassen
  • Platen

Bouten

Bij bouten worden de spanningen eenvoudig bepaald door de kracht te delen door het overeenkomstige gebied:

  • \(\sigma = F_t / A_s \)
  • \(\tau = V / A \)

waarbij:

  • \(F_t\) – trekkracht in de bout
  • \(A_s\) – trekspanningsgebied van de bout
  • \(V\) – afschuifkracht in bout; als er meerdere afschuifvlakken zijn, wordt de hoogste afschuifkracht gebruikt
  • \(A\) – gebied van de bout dat weerstand biedt aan afschuiving

Lassen

Lassen in CBFEM bestaan uit het laselement met multipoint constraints die de platen verbinden. De spanningsverdeling in de las wordt verstoord door de constraints en daarom worden de spanningen genomen van een sectie die zich op 1,5 keer van de lasgrootte van de las bevindt. Er worden drie secties gemaakt voor een dubbelzijdige hoeklas. Twee secties vallen in dezelfde detailcategorie en alleen de meer benadrukte wordt getoond. De maximale normaalspanning en de bijbehorende schuifspanning op dezelfde locatie, evenals de maximale schuifspanning en de bijbehorende normaalspanning op dezelfde locatie worden weergegeven.

Vermoeiingsberekening van de las in IDEA CONNECTION

Platen

The stress in plates may be visualized by creating a user-defined section by a Workplane manufacturing operation. In the figure below, two workplanes were created to see the stresses around bolt holes. The maximum normal stress and the corresponding shear stress at the same location, as well as the maximum shear stress and the corresponding normal stress at the same location are shown.

De spanning in platen kan worden gevisualiseerd door een door de gebruiker gedefinieerde sectie te maken door een Workplane-bewerking. In de onderstaande afbeelding zijn twee werkvlakken gemaakt om de spanningen rond boutgaten te kunnen zien. De maximale normaalspanning en de bijbehorende schuifspanning op dezelfde locatie, evenals de maximale schuifspanning en de bijbehorende normaalspanning op dezelfde locatie worden weergegeven.

Gerelateerde artikelen

Check of components according to AISC (American standards)

Controle van componenten volgens de Eurocode

Check of components according to CISC (Canadian standards)

Check of components according to GB (Chinese standards)

Check of components according to AS (Australian standards)

Check of components according to HKG (Hong Kong Code of Practice)

Check of components according to IS 800 (Indian standards)

Check of components according to SP (Russian standards)