The theoretical background is based on COMPATIBLE STRESS FIELD DESIGN OF STRUCTURAL CONCRETE
(Kaufmann et al., 2020)

Structural design of concrete discontinuities in IDEA StatiCa Detail

General introduction for the structural design of concrete details
Main assumptions and limitations
Reinforcement structural design
Finite element implementation in IDEA StatiCa Detail
   - Supports and load transmitting components
   - Load transfer at trimmed ends of beams
   - Geometric modification of cross-sections
   - Finite element types
   - Meshing
   - Solution method and load-control algorithm
   - Presentation of results
Structural element verification in IDEA StatiCa Detail
Verification of the structural concrete elements (EN)
   - Material models
   - Safety factors
   - Ultimate limit state analysis
   - Partially loaded areas (PLA)
   - Serviceability limit state analysis

General introduction for the structural design of concrete details

The design and assessment of concrete elements are normally performed at the sectional (1D-element) or point (2D-element) level. This procedure is described in all standards for structural design, e.g., in (EN 1992-1-1), and it is used in everyday structural engineering practice. However, it is not always known or respected that the procedure is only acceptable in areas where Bernoulli-Navier hypothesis of plane strain distribution applies (referred to as B-regions). The places where this hypothesis does not apply are called discontinuity or disturbed regions (D-Regions). Examples of B and D regions of 1D-elements are given in (Fig. 1). These are, e.g., bearing areas, parts where concentrated loads are applied, locations where an abrupt change in the cross-section occurs, openings, etc. When designing concrete structures, we meet a lot of other D-Regions such as walls, bridge diaphragms, corbels, etc. 

\[ \textsf{\textit{\footnotesize{Fig. 1\qquad Discontinuity regions (Navrátil et al. 2017)}}}\]

In the past, semi-empirical design rules were used for dimensioning discontinuity regions. Fortunately, these rules have been largely superseded over the past decades by strut-and-tie models (Schlaich et al., 1987) and stress fields (Marti 1985), which are featured in current design codes and frequently used by designers today. These models are mechanically consistent and powerful tools. Note that stress fields can generally be continuous or discontinuous and that strut-and-tie models are a special case of discontinuous stress fields.

Despite the evolution of computational tools over the past decades, Strut-and-Tie models are essentially still used as hand calculations. Their application for real-world structures is tedious and time-consuming since iterations are required, and several load cases need to be considered. Furthermore, this method is not suitable for verifying serviceability criteria (deformations, crack widths, etc.).

The interest of structural engineers in a reliable and fast tool to design D-regions led to the decision to develop the new Compatible Stress Field Method, a method for computer-aided stress field design that allows the automatic design and assessment of structural concrete members subjected to in-plane loading.

The Compatible Stress Field Method is a continuous FE-based stress field analysis method in which classic stress field solutions are complemented with kinematic considerations, i.e., the state of strain is evaluated throughout the structure. Hence, the effective compressive strength of concrete can be automatically computed based on the state of transverse strain in a similar manner as in compression field analyses that account for compression softening  (Vecchio and Collins 1986; Kaufmann and Marti 1998) and the EPSF method (Fernández Ruiz and Muttoni 2007). Moreover, the CSFM considers tension stiffening, providing realistic stiffnesses to the elements, and covers all design code prescriptions (including serviceability and deformation capacity aspects) not consistently addressed by previous approaches. The CSFM uses common uniaxial constitutive laws provided by design standards for concrete and reinforcement. These are known at the design stage, which allows the partial safety factor method to be used. Hence, designers do not have to provide additional, often arbitrary material properties as are typically required for non-linear FE-analyses, making the method perfectly suitable for engineering practice.

To foster the use of computer-aided stress fields by structural engineers, these methods should be implemented in user-friendly software environments. To this end, the CSFM has been implemented in IDEA StatiCa Detail; a new user-friendly commercial software developed jointly by ETH Zurich and the software company IDEA StatiCa in the framework of the DR-Design Eurostars-10571 project.

Reinforcement structural design

Workflow and goals

The goal of reinforcement design tools in the CSFM is to help designers determine the location and required amount of reinforcing bars efficiently. The following tools are available to help/ guide the user in this process: linear calculation, topology optimization, and area optimization.

Reinforcement design tools consider more simplified constitutive models than the models used for the final verification of the structure. Therefore, the definition of the reinforcement in this step should be considered a pre-design to be confirmed/refined during the final verification step. The use of the different reinforcement design tools will be depicted on the model shown in Fig. 5, which consists of one end of a simply supported beam with variable depth subjected to a uniformly distributed load.

\[ \textsf{\textit{\footnotesize{Fig. 5\qquad Model used to illustrate the use of the reinforcement design tools.}}}\]

Reinforcement locations

For regions where the reinforcement layout is not known beforehand, there are two methods available in the CSFM to help the user determine the optimum location of reinforcing bars: linear analysis and topology optimization. Both tools provide an overview of the location of tensile forces in the uncracked region for a certain load case.

Linear analysis

The linear analysis considers linear elastic material properties and neglects reinforcement in the concrete region. It is, therefore, a very fast calculation that provides a first insight into the locations of tension and compression areas. An example of such a calculation is shown in Fig. 6.

\[ \textsf{\textit{\footnotesize{Fig. 6\qquad Results from the linear analysis tool for defining reinforcement layout}}}\]

\[ \textsf{\textit{\footnotesize{(red: areas in compression, blue: areas in tension).}}}\]

Topology optimization

Topology optimization is a method that aims to find the optimal distribution of material in a given volume for a certain load configuration. The topology optimization implemented in Idea StatiCa Detail uses a linear finite element model. Each finite element may have a relative density from 0 to 100 %, representing the relative amount of material used. These element densities are the optimization parameters in the optimization problem. The resulting material distribution is considered optimal for the given set of loads if it minimizes the total strain energy of the system. By definition, the optimal distribution is also the geometry that has the largest possible stiffness for the given loads.

The iterative optimization process starts with a homogeneous density distribution. The calculation is performed for multiple total volume fractions (20%, 40%, 60% and 80%), which allows the user to select the most practical result, as proposed by . The resulting shape consists of trusses with struts and ties and represents the optimum shape for the given load cases (Fig. 7).

\[ \textsf{\textit{\footnotesize{Fig. 7\qquad Results from the topology optimization design tool with 20\% and 40\%  effective volume}}}\]

\[ \textsf{\textit{\footnotesize{(red: areas in compression, blue: areas in tension).}}}\]

Finite element implementation in IDEA StatiCa Detail

Introduction

The CSFM considers continuous stress fields in the concrete (2D finite elements), complemented by discrete “rod” elements representing the reinforcement (1D finite elements). Therefore, the reinforcement is not diffusely embedded into the concrete 2D finite elements, but explicitly modeled and connected to them. A plane stress state is considered in the calculation model.

\[ \textsf{\textit{\footnotesize{Fig. 8\qquad Visualization of the calculation model of a structural element (trimmed beam) in Idea StatiCa Detail.}}}\]

Both entire walls and beams, as well as details (parts) of beams (isolated discontinuity region, also called trimmed end), can be modeled. In the case of walls and entire beams, supports must be defined in such a way that an (externally) isostatic (statically determinate) or hyperstatic (statically indeterminate) structure results. The load transfer at the trimmed ends of beams is introduced by means of a special Saint-Venant transfer zone (described in Section 3.3), which ensures a realistic stress distribution in the analyzed detail region.

Load transfer at trimmed ends of beams

In many cases, we need to model only some detail (part) of a structural member, such as beam support, opening in the middle of the beam, etc. This approach can lead to support configurations that are unstable but admissible in IDEA StatiCa Detail (including the case of no supports). However, in such cases, it is also necessary to model the section representing the connection to the adjoining B-region, including internal forces at this section that satisfy the equilibrium. In certain cases (e.g., when modeling beam support), these internal forces can be determined automatically by the program.

Between the B-region and the analyzed discontinuity region, a Saint-Venant transfer zone is automatically created to ensure a realistic stress distribution in the analyzed region. The width of the transfer zone is determined as half of the section’s depth. As the only purpose of the Saint-Venant zone is to achieve a proper stress distribution in the rest of the model, no results from this area are displayed in verification, and no stop criteria are considered here.

The edge of the Saint-Venant zone that represents the trimmed end of the beam is modeled as rigid, i.e., it may rotate but must rest plane. This is done by connecting all the FEM nodes of the edge to a separate node at the centre of inertia of the section using a rigid body element (RBE2). The internal forces of the element may then be applied at this node, as shown in Fig. 10.

\[ \textsf{\textit{\footnotesize{Fig. 10\qquad Transfer of internal forces at a trimmed end.}}}\]

Finite element types

The non-linear (inelastic) finite element analysis model is created by several types of finite elements used to model concrete, reinforcement, and the bond between them. Concrete and reinforcement elements are first meshed independently and then connected to each other using multi-point constraints (MPC elements). This allows the reinforcement to occupy an arbitrary, relative position in relation to the concrete. If anchorage length verification is to be calculated, bond and anchorage end spring elements are inserted between the reinforcement and the MPC elements.

\[ \textsf{\textit{\footnotesize{Fig. 13\qquad Finite element model: reinforcement elements mapped to concrete mesh using MPC elements and bond elements.}}}\]

Concrete

Concrete is modeled using quadrilateral and trilateral shell elements, CQUAD4 and CTRIA3. These can be defined by four or three nodes, respectively. Only plane stress is assumed to exist in these elements, i.e., stresses or strains in the z-direction are not considered.

Each element has four or three integration points which are placed at approximately 1/4 of its size. At each integration point in every element, the directions of principal strains α₁, α₂ are calculated. In both of these directions, the principal stresses σ_c1, σ_c2 and stiffnesses E₁, E₂ are evaluated according to the specified concrete stress-strain diagram, as per Fig. 2. It should be noted that the impact of the compression softening effect couples the behavior of the main compressive direction to the actual state of the other principal direction.

Reinforcement

Rebars are modeled by two-node 1D “rod” elements (CROD), which only have axial stiffness. These elements are connected to special “bond” elements which were developed in order to model the slip behavior between a reinforcing bar and the surrounding concrete. These bond elements are subsequently connected by MPC (multi-point constraint) elements to the mesh representing the concrete. This approach allows the independent meshing of reinforcement and concrete, while their interconnection is ensured later.

Bond elements

The anchorage length is verified by implementing the bond shear stresses between concrete elements (2D) and reinforcing bar elements (1D) in the finite element model. To this end, a “bond” finite element type was developed.

The definition of the bond element is similar to that of a shell element (CQUAD4). It is also defined by 4 nodes, but in contrast to a shell, it only has a non-zero stiffness in shear between the two upper and two lower nodes. In the model, the upper nodes are connected to the elements representing reinforcement and the lower nodes to those representing concrete. The behavior of this element is described by the bond stress, τ_b, as a bilinear function of the slip between the upper and lower nodes, δ_u, see Fig. 14.

\[ \textsf{\textit{\footnotesize{Fig. 14\qquad (a) conceptual illustration of the deformation of a bond element; (b) a stress-deformation function.}}}\]

The elastic stiffness modulus of the bond-slip relationship, G_b, is defined as follows:

\[G_b = k_g \cdot \frac{E_c}{Ø}\]

where:

k_g            coefficient depending on the reinforcing bar surface (by default k_g = 0.2)

E_c            modulus of elasticity of concrete (taken as E_cm in case of EN)

Ø             the diameter of the reinforcing bar

The design values (factored values) of ultimate bond shear stress, f_bd, provided in the respective selected design codes EN 1992-1-1 or ACI 318-19 are used to verify the anchorage length. The hardening of the plastic branch is calculated by default as G_b/10⁵.

Anchorage spring

The provision of anchorage ends to the reinforcing bars (i.e., bends, hooks, loops…), which fulfills the prescriptions of design codes, allows the reduction of the basic anchorage length of the bars (l_b,net) by a certain factor β (referred to as the ‘anchorage coefficient’ below). The design value of the anchorage length (l_b) is then calculated as follows:

\[l_b = \left(1 - \beta\right)l_{b,net}\]

The intended reduction in l_b,net is equivalent to the activation of the reinforcing bar at its end at a percentage of its maximum capacity given by the anchorage reduction coefficient, as shown in Fig. 15a.

\[ \textsf{\textit{\footnotesize{Fig. 15\qquad  Model for the reduction of the anchorage length:}}}\]

\[ \textsf{\textit{\footnotesize{(a) anchorage force along the anchorage length of the reinforcing bar; (b) slip-anchorage force constitutive relationship.}}}\]

The reduction of the anchorage length is included in the finite element model by means of a spring element at the end of the bar (Fig. 15), which is defined by the constitutive model shown in Fig. 15b. The maximum force transmitted by this spring (F_au) is:

\[F_{au} = \beta \cdot A_s \cdot f_{yd}\]

where :

β             the anchorage coefficient based on anchorage type,

A_s            the cross-section of the reinforcing bar,

f_yd           the design value (factored value) of the yield strength of the reinforcement.

Meshing

The finite elements are implemented internally, and the analysis model is generated automatically without any need for proficient user interaction. An important part of this process is meshing.

Concrete

All concrete members are meshed together. A recommended element size is automatically computed by the application based on the size and shape of the structure and taking into account the diameter of the largest reinforcing bar. Moreover, the recommended element size guarantees that a minimum of 4 elements are generated in thin parts of the structure, such as slim columns or thin slabs, to ensure reliable results in these areas. The maximum number of concrete elements is limited to 5000, but this value is sufficient to provide the recommended element size for most structures. Designers can always select a user-defined concrete element size by modifying the multiplier of the default mesh size.

Reinforcement

The reinforcement is divided into elements with approximately the same length as the concrete element size. Once the reinforcement and concrete meshes are generated, they are interconnected with bond elements as shown in Fig. 13.

Bearing plates

Auxiliary structural parts, such as bearing plates, are meshed independently. The size of these elements is calculated as 2/3 of the size of concrete elements in the connection area. The nodes of the bearing plate mesh are then connected to the edge nodes of the concrete mesh using interpolation constraint elements (RBE3).

Loads and supports

Patch loads and patch supports are connected only to the reinforcement, as shown in Fig. 16. Therefore, it is necessary to define the reinforcement around them. Connection to all nodes of the reinforcement within the effective radius is ensured by RBE3 elements with equal weight.

\[ \textsf{\textit{\footnotesize{Fig. 16\qquad  Patch load mapping to reinforcement mesh.}}}\]

Line supports, and line loads are connected to the nodes of the concrete mesh using RBE3 elements based on the specified width or effective radius. The weight of the connections is inversely proportional to the distance from the support or load impulse.

• Read more about the interconnection between individual loads and mesh in General description of Load impulses in Detail application

Serviceability limit state analysis

SLS assessments are carried out for stress limitation, crack width, and deflection limits. Stresses are checked in concrete and reinforcement elements according to EN 1992-1-1 in a similar manner to that specified for the ULS.

Stress limitation

The compressive stress in the concrete shall be limited in order to avoid longitudinal cracks. According to EN 1992-1-1 chap. 7.2 (2), longitudinal cracks may occur if the stress level under the characteristic combination of loads exceeds a value k₁f_ck. The concrete stress in compression is evaluated as the ratio between the maximum principal compressive stress σ_c3 obtained from FE analysis for serviceability limit states and the limit value σ_c3,lim. Then:

\[\frac{σ_{c3}}{σ_{c3,lim}}\]

\[σ_{c3,lim} = k_1\cdot f_{ck}\]

where:

f_ck        characteristic cylinder strength of concrete,

k₁         =0.6.

Unacceptable cracking or deformation may be assumed to be avoided if, under the characteristic combination of loads, the tensile stress in the reinforcement does not exceed k₃f_yk (EN 1992-1-1 chap. 7.2 (5)). The strength of the reinforcement is evaluated as the ratio between the stress in the reinforcement at the cracks σ_sr and the specified limit value σ_sr,lim:

\[\frac{σ_{sr}}{σ_{sr,lim}}\]

\[σ_{sr,lim} =  k_3\cdot f_{yk}\]

where:

f_yk        yield strength of the reinforcement,

k₃        =0.8.

Deflection

Deflections can only be assessed for walls or isostatic (statically determinate) or hyperstatic (statically indeterminate) beams. In these cases, the absolute value of deflections is considered (compared to the initial state before loading), and the maximum admissible value of deflections must be set by the user. Deflections at trimmed ends cannot be checked since these are essentially unstable structures where the equilibrium is satisfied by adding end forces, and hence deflections are unrealistic. Short-term u_z,st or long-term u_z,lt deflection can be calculated and checked against user-defined limit values:

\[\frac{u_ z}{u_{z,lim}}\]

where:

u_z         short- or long-term deflection calculated by FE analysis,

u_z,lim    limit value of the deflection defined by the user.

Crack width

Crack widths and crack orientations are calculated only for permanent loads, either short-term or long-term. The verifications with respect to limit values specified by the user according to the Eurocode are presented as follows:

\[\frac{w_ z}{w_{z,lim}}\]

where:

w         short- or long-term crack width calculated by FE analysis,

w_lim     limit value of the crack width defined by the user.

There are two ways of computing crack widths (stabilized and non-stabilized cracking). In the general case (stabilized cracking), the crack width is calculated by integrating the strains on 1D elements of reinforcing bars. The crack direction is then calculated from the three closest (from the center of the given 1D finite element of reinforcement) integration points of 2D concrete elements. While this approach to calculating the crack directions does not correspond to the real position of the cracks, it still provides representative values that lead to crack width results that can be compared to code-required crack width values at the position of the reinforcing bar.

References

ACI Committee 318. 2009a. Building Code Requirements for Structural Concrete (ACI 318-08) and Commentary. Farmington Hills, MI: American Concrete Institute.

Alvarez, Manuel. 1998. Einfluss des Verbundverhaltens auf das Verformungsvermögen von Stahlbeton. IBK Bericht 236. Basel: Institut für Baustatik und Konstruktion, ETH Zurich, Birkhäuser Verlag.

Beeby, A. W. 1979. “The Prediction of Crack Widths in Hardened Concrete.” The Structural Engineer 57A (1): 9–17.

Broms, Bengt B. 1965. “Crack Width and Crack Spacing In Reinforced Concrete Members.” ACI Journal Proceedings 62 (10): 1237–56. https://doi.org/10.14359/7742.

Burns, C.. 2012. “Serviceability Analysis of Reinforced Concrete Members Based on the Tension Chord Model.” IBK Report Nr. 342, Zurich, Switzerland: ETH Zurich.

Crisfield, M. A. 1997. Non-Linear Finite Element Analysis of Solids and Structures. Wiley.

European Committee for Standardization (CEN). 2015. 1 Eurocode 2: Design of concrete structures - Part 1-1:  General rules and rules for buildings. Brussels: CEN, 2005.

Fernández Ruiz, M., and A. Muttoni. 2007. “On Development of Suitable Stress Fields for Structural Concrete.” ACI Structural Journal 104 (4): 495–502.

Kaufmann, W., J. Mata-Falcón, M. Weber, T. Galkovski, D. Thong Tran, J. Kabelac, M. Konecny, J. Navratil, M. Cihal, and P. Komarkova. 2020. “Compatible Stress Field Design Of Structural Concrete. Berlin, Germany.”AZ Druck und Datentechnik GmbH, ISBN 978-3-906916-95-8.

Kaufmann, W., and P. Marti. 1998. “Structural Concrete: Cracked Membrane Model.” Journal of Structural Engineering 124 (12): 1467–75. https://doi.org/10.1061/(ASCE)0733-9445(1998)124:12(1467).

Kaufmann, W.. 1998. “Strength and Deformations of Structural Concrete Subjected to In-Plane Shear and Normal Forces.” Doctoral dissertation, Basel: Institut für Baustatik und Konstruktion, ETH Zürich. https://doi.org/10.1007/978-3-0348-7612-4.

Konečný, M., J. Kabeláč, and J. Navrátil. 2017. Use of Topology Optimization in Concrete Reinforcement Design. 24. Czech Concrete Days (2017). ČBS ČSSI. https://resources.ideastatica.com/Content/06_Detail/Verification/Articles/Topology_optimization_US.pdf.

Marti, P. 1985. “Truss Models in Detailing.” Concrete International 7 (12): 66–73.

Marti, P. 2013. Theory of Structures: Fundamentals, Framed Structures, Plates and Shells. First edition. Berlin, Germany: Wiley Ernst & Sohn.

http://sfx.ethz.ch/sfx_locater?sid=ALEPH:EBI01&genre=book&isbn=9783433029916.

Marti, P., M.Alvarez, W. Kaufmann, and V. Sigrist. 1998. “Tension Chord Model for Structural Concrete.” Structural Engineering International 8 (4): 287–298.

https://doi.org/10.2749/101686698780488875.

Mata-Falcón, J. 2015. “Serviceability and Ultimate Behaviour of Dapped-End Beams (In Spanish: Estudio Del Comportamiento En Servicio y Rotura de Los Apoyos a Media Madera).” PhD thesis, Valencia: Universitat Politècnica de València.

Meier, H. 1983. “Berücksichtigung Des Wirklichkeitsnahen Werkstoffverhaltens Beim Standsicherheitsnachweis Turmartiger Stahlbetonbauwerke.” Institut für Massivbau, Universität Stuttgart.

Navrátil, J., P. Ševčík, L. Michalčík, P. Foltyn, and J. Kabeláč. 2017. A Solution for Walls and Details of Concrete Structures. 24. Czech Concrete Days.

Schlaich, J., K. Schäfer, and M. Jennewein. 1987a. “Toward a Consistent Design of Structural Concrete.” PCI Journal 32 (3): 74–150.

Vecchio, F.J., and M.P. Collins. 1986. “The Modified Compression Field Theory for Reinforced Concrete Elements Subjected to Shear.” ACI Journal 83 (2): 219–31.

Toegevoegde downloads

• Theoretical Background 20.pdf (PDF, 2,1 MB)