​

El objeto de la presente tesina es el de presentar una metodología novedosa para el cálculo de estructuras de hormigón posteso, basada en las posibilidades que brinda el uso de la teoría Serie Paralelo para la modelización de materiales compuestos. Se exponen, así mismo, las ventajas de esta metodología frente a los mecanismos actuales de cálculo que aparecen en los estándares de diseño de estructuras y aquellos otros basados en la simulación numérica a través del método de elementos finitos (MEF).

​

La teoría Serie Paralelo permite la modelización individualizada de los materiales componentes, actuando como una gestora de modelos constitutivos con el objetivo de simular el comportamiento del material compuesto en cuestión. Se modela el hormigón pretensado como un material compuesto de fibras largas en que la orientación de la fibra la marca el tendón de acero.

​

Así pues, se puede usar el modelo constitutivo que más convenga para la matriz - hormigón (modelo de daño isótropo) y para la fibra - acero (modelo de viscoelasticidad) logrando gran nivel de detalle en la micro-escala. El ánalisis se fundamenta en el MEF, que combinado con la teoría Serie Paralelo permite abordar estructuras de gran envergadura y adaptándose a los requerimientos geométricos específicos en cada caso.

​

Se incluyen tres ejemplos de aplicación de la metodología presentada, los cuales pretenden servir de validación y demostrar el potencial de cálculo de la misma. En los dos primeros casos se analizan dos vigas isoestáticas que permiten la comparativa con los resultados que se obtienen del ánalisis mediante métodos analíticos y, en el tercer caso se presentan los resultados de un Benchmark en el cual se ha trabajado en los últimos meses en que se estudia el comportamiento de un modelo a escala de un edificio de contención de una central nuclear.

​

​

=Abstract=

​

The main objective of this monograph is to present a novel methodology for the analysis of post-tensioned concrete structures, based on the potential offered by the use of the Serial-Parallel Rule of Mixtures when modelling composite materials. The advantages of this methodology are studied in comparison to the available approaches, i.e. the formulation proposed by the standards used in the design of structures and the mechanism used in numerical simulation based on the finite element method (FEM).

​

The Serial-Parallel Rule of Mixtures allows the modelization of each component material in depth, working as a constitutive model manager in order to simulate the composite material being studied. The prestressed concrete is modelled as a composite material with long fibres where the fibre orientation is defined by the steel tendon direction.

​

Therefore, the most suitable constitutive model can be used in each case. In the present monograph this is: for the matrix - concrete an isotropic damage model and for the fibre - steel a viscoelasticity model, achieving an extraordinary accuracy in the micro-scale. The analysis is based on the FEM, which combined with the Serial-Parallel Rule of Mixtures theory allows the study of large-scale structures, taking into account the specific geometric requirements of the construction.

​

Three application examples are included which are used for validating the methodology and the potential of this approach. The first two cases are two isostatic beams that allow the comparison with the results obtained through the study using analytical methods. Finally, the third case shows the results obtained recently for the analysis of a Benchmark, in which the behaviour of a mock-up of a reactor containment building has been studied.

​

​

''Al equipo del proyecto ANAV. Éste es el fruto de más de un año de trabajo, que nos ha convertido en lo que somos, una familia''

​

​

=1 Introduction: motivation and objectives=

​

In the last decades engineering researchers have bet on the use of numerical modelling as a recurring tool for their work. Computational calculation improvements have set the suitable scenario for a prompt development, achieving a wide range of useful techniques which can be applied in many fields, from structures to agriculture engineering or soil mechanics.

​

The Finite Element Method (FEM) <span id='citeF-1'></span>[[#cite-1|[1]]] is one of the most well known computational techniques and it will be of interest for the purpose of the monograph. However, there are other methodologies such as the Finite Difference Method (FDM), the Discrete Element Method (DEM) <span id='citeF-2'></span><span id='citeF-3'></span>[[#cite-2|[2,3]]], the Particle Finite Element Method (PFEM) <span id='citeF-4'></span>[[#cite-4|[4]]] or the Multiscale Analysis <span id='citeF-5'></span>[[#cite-5|[5]]] that are also widely extended.

​

Thanks to the application of FEM in the structural analysis scope, a deeper assessment of the structure can be driven compared to those obtained using conventional techniques, which include notorious geometric and constitutive simplifications. Despite this, the results obtained from numerical modelling strongly depend on the model quality and on the veracity of the implemented attributes, i.e. boundary conditions, applied loads and material properties..

​

According to this, complex structures with singular areas, material heterogeneities, non-linear behaviours, etc. require more sophisticated models that could bring suitable results.

​

Post-tensioned reinforced concrete elements are an example of this. Their behaviour is controlled by the three materials that conform the structure, i.e. concrete, reinforcing steel and prestressing steel. Codes and standards <span id='citeF-6'></span>[[#cite-6|[6]]] provide sufficient guidance to carry out the design and validation of a multiple number of cases, but the applicability of the proposed formulation becomes questionable when the studied element has not a simple geometry. Numerical modelling is then used.

​

The present monograph aims to introduce a new approach that increases the range of structures that can be analysed and solves many of the problems that other techniques have (see Section [[#2 State of the art|2]]). This is the study of post-tensioned structures by means of a serial-parallel rule of mixtures (SP RoM) <span id='citeF-7'></span><span id='citeF-8'></span><span id='citeF-9'></span>[[#cite-7|[7,8,9]]].

​

The document is divided in two main sections. In the first one, the theoretical bases are introduced in order to fully comprehend the mechanisms that govern the proposed method. Thus, a brief presentation of the FEM is done, paying special attention to the 3-D formulation and then the SP RoM bases are introduced. 

​

The second part is centred on verifying the robustness and accuracy of the approach through several cases. The complexity of these examples progressively increases from a straight rectangular beam to a real structure. Thus, the initial cases will be useful to compare those results that could be calculated using analytical techniques and the ones obtained with the computational mechanisms introduced in the monograph. And the last examples will be useful to exemplify the full potential of the technique using a real structure.

​

=2 State of the art=

​

Prestressed concrete appeared at the beginning of the twentieth century when high resistance concrete and steel were available. The function of that new material was to solve the cracking problems that the reinforced concrete structures had <span id='citeF-10'></span>[[#cite-10|[10]]].

​

Eugene Fryssinet is considered the father of this material which quickly became popular in France and Germany. It was after Second World War when its uses expands all around the world and started competing with great magnitude steel structures. Nowadays prestressed concrete is used in a wide range of structures like braces, railway sleepers, bridges, slabs, runways, reactor containment buildings, etc. This generalised use accentuates the priority of having the correct tools to evaluate these structures.

​

==2.1 Codes approach==

​

National and international standards such as EHE-08 <span id='citeF-6'></span>[[#cite-6|[6]]], EC2 <span id='citeF-11'></span>[[#cite-11|[11]]] or BPEL <span id='citeF-12'></span>[[#cite-12|[12]]] propose their own procedure that helps the engineer at the design and/or at the analysis stage of the prestressed concrete structure. The methodology presented is similar in all of them and works through the analysis of the structure critical sections at Ultimate Limit State (ULS) (Figure [[#img-1|1]]). The prestressing steel effect is included in the section equilibrium equations (Equation [[#eq-2.1|2.1]] and [[#eq-2.2|2.2]]) as a force applied at the tendon position and a bending moment, if needed, that accounts for hyperstatic effects <span id='citeF-13'></span>[[#cite-13|[13]]].

​

<div id='img-1'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-SeccionEHEJPG.png|540px|Section analysis]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 1:''' Section analysis

|}

​

<span id="eq-2.1"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>P=C- \Delta T-A_sf_{yd} </math>

|-

| style="text-align: center;" | <math>   y=\dfrac{A_pf_{pyd}+A_sf_{yd}}{f_{cd}b}=\dfrac{U_p+U_s}{f_{cd}b}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.1)

|}

​

<span id="eq-2.2"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>M_d+P(d_s-d_p) =C(d_s-\frac{y}{2})- \Delta T(d_s-d_p) </math>

|-

| style="text-align: center;" | <math>    U_p+U_s=f_{cd}bd_s\left(1-\sqrt{1-\dfrac{2\left(M_d+U_p\left(d_s-d_p\right)\right)}{f_{cd}bd_{s}^2}}\right)  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.2)

|}

​

The rectangular section represented in Figure [[#img-1|1]] and analysed in Equations [[#eq-2.1|2.1]] and [[#eq-2.2|2.2]] corresponds to the mid-span of a simple supported beam. Only prestressing steel and tensile reinforcing steel has been considered and the final equation has been written in the format that EHE-08 proposes for reinforced concrete rectangular sections subjected to flexure (EHE-08, ''Anejo 7. Cálculo simplicado de secciones en Estado Lite de Agotamiento frente a solicitaciones normales'' <span id='citeF-6'></span>[[#cite-6|[6]]]) where <math display="inline"> P </math> and <math display="inline"> M_d </math> are acting forces on the beam section, i.e. the prestressing force and the bending moment due to external forces, respectively, <math display="inline"> C </math>, <math display="inline"> A_s f_{yd} </math> and <math display="inline"> \Delta T </math> are the resulting efforts due to external action, i.e. the compression in concrete due to <math display="inline"> M_d </math> and the resulting tension in reinforcing and prestressing steel respectively, <math display="inline"> f_{cd} </math>, <math display="inline"> f_{yd} </math> and <math display="inline"> f_{pd} </math> are the strengths of concrete in compression, reinforcing steel and prestressing steel, respectively, <math display="inline"> U_p </math> and <math display="inline"> U_s </math> are notation parameters used in the same way that EHE-08 and the other variables are geometric parameters defined in Figure [[#img-1|1]]. The analysis would be complete when all the efforts have been studied, i.e. bending, shear and axial analysis.

​

Alternatively, codes provide stress limits at section level that must be respect for the design. These limits are grouped at Magnel equations (Equations [[#eq-2.3|2.3]], [[#eq-2.4|2.4]], [[#eq-2.5|2.5]] and [[#eq-2.6|2.6]]) <span id='citeF-14'></span>[[#cite-14|[14]]] which create the space of feasible solutions for a specified tendon geometry on elastic analysis. This theory has been already extended to non-linear behaviour needed when studying partially prestressed concrete sections <span id='citeF-15'></span>[[#cite-15|[15]]].

​

<u>Stress at transfer</u>

​

<span id="eq-2.3"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\sigma _{c,\, top}^{tra}=d\frac{\gamma _p P }{A_{c,\, net}}+\dfrac{\gamma _p P e_{net} v_{net}}{I_{c,\, net}}+d\frac{M_{sw} v_{net}}{I_{c,\, net}} \geq \left\{ \begin{array}{c} -f_{ctmj} \\   0 \end{array}  \right. </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.3)

|}

​

<span id="eq-2.4"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\sigma _{c,\, bot.}^{tra}=\dfrac{\gamma _p P }{A_{c,\, net}}+\dfrac{\gamma _p P e_{net}{ v'}_{net}}{I_{c,\, net}}+\dfrac{M_{sw}{ v'}_{net}}{I_{c,\, net}}\leq 0.6f_{ckj} </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.4)

|}

​

<u>Stress at service</u>

​

<span id="eq-2.5"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\sigma _{c,\, top}^{ser}=\dfrac{\gamma _p P }{A_{c,\, hom}}+\dfrac{\gamma _p P e_{hom} v_{hom}}{I_{c,\, hom}}+\dfrac{M_{char}^{SLS} v_{hom}}{I_{c,\, hom}}\leq 0.6f_{ckj} </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.5)

|}

​

<span id="eq-2.6"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\sigma _{c,\, bot}^{ser}=\dfrac{\gamma _p P }{A_{c,\, hom}}+\dfrac{\gamma _p P e_{hom}{ v'}_{hom}}{I_{c,\, hom}}+\dfrac{M_{char}^{SLS}{ v'}_{hom}}{I_{c,\, hom}}\geq \left\{ \begin{array}{c} -f_{ctmj} \\   0 \end{array}  \right. </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.6)

|}

​

In these equations, the stress is computed at the top and the bottom of the studied concrete section (<math display="inline"> i </math>) and at transfer or service (<math display="inline"> j </math>), i.e. <math display="inline"> \sigma _{c, \, i}^{j} </math> generated by the prestressing force <math display="inline"> P </math> factorized using <math display="inline"> \gamma _p </math> and the corresponding bending moment <math display="inline"> M </math> and it is compared with the specific concrete strength <math display="inline"> f_c,\, i </math> in each case. The other parameters are geometric variables: the section inertia (<math display="inline"> I </math>), the section area (<math display="inline"> A </math>) and the distance between the studied extreme of the section (top or bottom) and the neutral axis, i.e. <math display="inline"> v </math> and <math display="inline"> v' </math>. And all them considering the net area or the full concrete.

​

In addition to the section equilibrium done at ULS, Service Limit State (SLS) is also checked at the codes approach. In fact, post-tensioned concrete structures are usually designed according to a limit in the maximum crack width (<math display="inline"> w_{max} </math>) as shown in Table [[#2.1 Codes approach|2.1]] obtained from EHE-08 and EC2.

​

In all the cases, the parameter that governs the design of a structure is the prestressing force value at the studied section. Codes provide the needed formulation that transforms the initial force applied at the anchorage area into the one transmitted along the studied element, i.e. prestressing losses calculation of post-tensioned elements <span id='citeF-11'></span><span id='citeF-6'></span><span id='citeF-12'></span>[[#cite-11|[11,6,12]]].

​

​

{|  class="floating_tableSCP wikitable" style="text-align: center; margin: 1em auto;min-width:50%;"

|+ style="font-size: 75%;" |<span id='table-1'></span>Table. 1 Maximum crack width from EHE-08 and EC2

|-

| colspan='3' | '''EHE 08'''

|-

| colspan='1' style="text-align: right;" | 

| colspan='2' | <math> w_{max} \, [mm] </math>

|-

| rowspan='2' colspan='1' | 

| colspan='1' | Reinforced members (quasi-permanent load combination)

| colspan='1' | Prestressed members (frequent load combination)

|-

|  0.4   

|  0.2 

|-

| colspan='1' style="text-align: left;" | IIa, IIb, H

|  0.3   

|  0.2 

|-

| colspan='1' style="text-align: left;" | IIIa, IIIb, IV, F, Qa

|  0.2   

| rowspan='2' | Decompression

|-

| colspan='1' style="text-align: left;" | IIIc, Qb, Qc

|  0.1   

|-

| colspan='3' | '''EC2'''

|-

| colspan='1' | 

| colspan='2' | <math> w_{max} \, [mm] </math>

|-

| rowspan='2' colspan='1' | 

| colspan='1' | Reinforced members and prestressed members with unbounded tendons (quasi-permanent load combination)

| colspan='1' | Prestressed members with bounded tendons (frequent load combination)

|-

|  0.4   

|  0.2 

|-

| colspan='1' style="text-align: left;" | XC2, XC3, XC4

| rowspan='2' | 0.3

|  0.2 

|-

| style="text-align: left;" |    XD1, XD2, XD3, XS1, XS2, XS3 

| Decompression

​

|}

​

===Immediate losses===

​

Immediate losses are those generated during the application of the prestressing force and at the wedge blocking operation. These losses have different origin and are studied independently, differentiating between:

​

​

* <u>Friction losses, <math> \Delta P_{\mu } </math></u>. The contact between tendons and ducts prevent the force transmission from the active end, where tendons are being tensioned. The expression proposed at codes that calculates these losses from the applied force (<math display="inline"> P_0 </math>) is:

​

<span id="eq-2.7"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>

​

\Delta P_{\mu }=P_{0}\left(1-e^{-\left(\mu \alpha{+}kx \right)}\right)   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.7)

|}

​

The variables that control force losses in Equation [[#eq-2.7|2.7]] are <math display="inline"> \mu </math> and <math display="inline"> k </math>.  This evidences the existence of two kind of friction that have different nature. <math display="inline"> \mu </math> is related to the contact produced at curve zones of the tendon path and therefore it appears next to <math display="inline"> \alpha </math>, that is the total angular displacement. On the other hand, <math display="inline"> k </math> is related to a friction produced by an unintentional angular displacement at straight areas of the tendon path and so it is proportional to the length <math display="inline"> x </math> (Figure [[#img-2|2]]).

​

Values for these two parameters are obtained experimentally. Standards provide their own proposal depending on the type of steel that is used, the kind of bounding that is used, the duct diameter, etc. (Figure [[#img-3|3]]).

​

<div id='img-2'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-MuKCoefficientsDraw.png|240px|Graphical description for  k  coefficient <span id='citeF-10'></span>[[#cite-10|[10]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 2:''' Graphical description for <math> k </math> coefficient <span id='citeF-10'></span>[[#cite-10|[10]]]

|}

​

<div id='img-3'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-MuKCoefficients.png|540px| μ and  k  values from the American Concrete Institue (ACI 318-05) <span id='citeF-16'></span>[[#cite-16|[16]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 3:''' <math> \mu </math> and <math> k </math> values from the American Concrete Institue (ACI 318-05) <span id='citeF-16'></span>[[#cite-16|[16]]]

|}

​

Equation [[#eq-2.7|2.7]] is usually applied discreetly at sections with curvature changes and then these values are linearly interpolated for the whole structure. A visual example that helps to fully comprehend the result that could be obtained using the previous expression is shown at Figure [[#img-4|4]], where the prestressing force distribution after friction losses is drawn for a three-span continuous beam.

​

<div id='img-4'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-PerdidasRozamiento.png|480px|Prestressing force distribution after friction losses <span id='citeF-10'></span>[[#cite-10|[10]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 4:''' Prestressing force distribution after friction losses <span id='citeF-10'></span>[[#cite-10|[10]]]

|}

​

* <u>Losses due to wedge draw-in of the anchorage devices, <math> \Delta P_{a} </math></u>. When post-tensioned tendons are anchored, some of the force applied during the post-tensioning operation is lost. It is important to minimize the amount of stress lost and the affected length by this phenomenon. Expression [[#eq-2.8|2.8]] <span id='citeF-17'></span>[[#cite-17|[17]]] point out the variables involved in the problem:

​

<span id="eq-2.8"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>

​

a=\int _{0}^{L}\dfrac{\Delta P_{a}(x)}{E_pA_p}dx   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.8)

|}

​

Where <math display="inline"> A_p </math> and <math display="inline"> E_p </math> are the prestressing steel total area and longitudinal elastic modulus, <math display="inline"> a </math> is the pull-in at wedge blocking and <math display="inline"> L </math> is the tendon length. Considering that the function that describes the force loss due to wedge blocking behaves in the same way than the one used for friction losses (Figure [[#img-5|5]]), then Equation [[#eq-2.8|2.8]] can be rewritten as:

​

<span id="eq-2.9"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>

​

a=\dfrac{S}{A_p E_p}=\dfrac{\Delta P_{a} l_p}{2E_p A_p}=\dfrac{P_A \left[1-e^{-\left(\mu \alpha{+}kl_p\right)}\right]l_p}{A_p E_p}    </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.9)

|}

​

Where <math display="inline"> P_A </math> is the applied force at the active end of the tendon and <math display="inline"> l_p </math> is the affected length due to anchorage operation.  <div id='img-5'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-PenetracionCuna.png|480px|Prestressing force redistribution after wedge blocking <span id='citeF-17'></span>[[#cite-17|[17]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 5:''' Prestressing force redistribution after wedge blocking <span id='citeF-17'></span>[[#cite-17|[17]]]

|}

​

* <u>Losses due to concrete instantaneous deformation, <math> \Delta P_{el} </math></u>. The stress transmission from tendons to concrete during anchorage operations generates a deformation in concrete that reduces the prestressing force at tendon. This is only a problem when several tendons are tensioned and the operation cannot be done simultaneously. The consecutive concrete deformations generate force losses at tendons that have been previously anchored.

​

Standards provide formulas with similar format to Equation [[#eq-2.10|2.10]], which consider that concrete deformations remain in the elastic domain.

​

<span id="eq-2.10"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>

​

\Delta P_{el}=A_p E_p \sum{\left[\dfrac{j \, \Delta \sigma _c (t)}{E_{cm}(t)}\right]}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.10)

|}

​

Where <math display="inline"> A_p </math> and <math display="inline"> E_p </math> are again the prestressing steel total area and the longitudinal elastic modulus, <math display="inline"> E_{cm}(t) </math> is the concrete elastic modulus at the age that tension operations take place, <math display="inline">  \Delta \sigma _c (t) </math> is the variation of concrete stress at the centre of gravity of the tendons applied at time <math display="inline"> t </math> and <math display="inline"> j </math> is a coefficient equal to <math display="inline"> \dfrac{n-1}{2n} </math> as shown by Aguado, Mirambell, Murcia and Marí (1983) <span id='citeF-18'></span>[[#cite-18|[18]]] that can be approximated to <math display="inline"> j=0.5 </math> when the number of tendons, <math display="inline"> n </math>, is high.

​

According to Murcia, Aguado and Marí (1993) <span id='citeF-10'></span>[[#cite-10|[10]]] and the EHE-08 <span id='citeF-6'></span>[[#cite-6|[6]]], <math display="inline"> \Delta \sigma _c (t) </math> value can be computed as <math display="inline"> P_0-\Delta P_{\mu }-\Delta P_{a} </math> and should be checked the transfer state where only prestressing force and self weight are applied because this situation could be more restrictive <span id='citeF-10'></span>[[#cite-10|[10]]].

​

The formulas introduced in this section are valid only for post-tensioned concrete structures, which are the object of study of this monograph. Pre-tensioned concrete structures are treated in a different way.

​

===Time dependent losses===

​

Once the prestressing operations have taken place, rheological mechanisms start to develop which lead to a generalised stress loss in the prestressing system. These procedures are known as time dependent losses, which are originated by creep and shrinkage at concrete and relaxation at the prestressing system.

​

The incorporation of these mechanisms into the structure analysis is complex due to the existing interdependence between them, e.g. shrinkage generates stress losses that affect creep and steel relaxation procedures. In practice standards try to simplify these calculations by uncoupling the mechanisms and study them independently <span id='citeF-12'></span>[[#cite-12|[12]]] or by using specific formulation depending on the structure conditions <span id='citeF-19'></span>[[#cite-19|[19]]]. EC2 and EHE-08, for example, propose a simplified method based on the ageing coefficient (<math display="inline"> \chi </math>):

​

<span id="eq-2.11"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\Delta P_{c+s+r}=A_p \dfrac{\varepsilon _{cs}+E_p +0.8\Delta \sigma _{pr}+\dfrac{E_p}{E_{cm}}\varphi (t,t_0)\sigma _{c,QP}}{1+\dfrac{E_p}{E_{cm}}\dfrac{A_p}{A_c}\left(1+\dfrac{A_c}{I_c}z_{cp}^2\right)\left[1+\chi \varphi (t,t_0)\right]}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (2.11)

|}

​

Where:

​

* is the force loss due to    <u>c</u>reep, <u>s</u>hrinkage and steel <u>r</u>elaxation at location <math display="inline"> x </math>, at time <math display="inline"> t </math>

* shrinkage strain

* Young modulus for the prestressing steel

* Young modulus for the concrete

* stress loss due to steel relaxation

* is the creep coefficient at a time <math display="inline"> t </math> and load application at time <math display="inline"> t_0 </math>

* concrete stress due to the prestressing effect, the self-weight and the dead loads. This stress is measured at the centre of gravity of the prestressing steel area (<math display="inline"> A_p </math>).

* is tendons total area at the location <math display="inline"> x </math>

* is concrete total area at the location <math display="inline"> x </math>

* is the moment of inertia of the concrete section

* is the distance between the centre of gravity of the tendons and the concrete section

* is the ageing coefficient that can be approximated as <math display="inline"> \chi=0.8 </math> when time tends to infinity

​

==2.2 FEM approach==

​

The use of numerical techniques in the structural analysis field has provided researchers a powerful tool that permits a global study of the structure. The accuracy level that these methodologies can achieve and the potential for solving complex cases make them attractive for many research lines.

​

Despite this, these computational techniques have also drawbacks. Therefore, it is important to know when to use them and which is the best type of analysis to be performed. For example, regions with discontinuities in geometry or actions, also known as D-regions <span id='citeF-11'></span><span id='citeF-6'></span>[[#cite-11|[11,6]]], not necessarily have to be designed using a finite element (FE) model, strud-and-tie method <span id='citeF-20'></span>[[#cite-20|[20]]] can be used instead. Another example is the case of bridges. For these structures it is not always needed a 3-D FEM design, many bridge decks have been designed using simplified methodologies such as the Grillage method <span id='citeF-21'></span>[[#cite-21|[21]]].

​

Prestressed concrete structures can be studied using the FEM and the interest on its use increases as the structure becomes more complex. There is no standardised procedure for the analysis of these structures, research papers can show the wide range of options that exist <span id='citeF-22'></span><span id='citeF-23'></span><span id='citeF-24'></span><span id='citeF-25'></span>[[#cite-22|[22,23,24,25]]]. The difficulties that arise from their analysis are originated by the coexistence of three different materials: concrete, reinforcing steel and prestressing steel.

​

While the concrete modelization is similar in all cases, the way that strands and tendons are included in the FE analysis make the difference between the existing approaches. Some of these are:

​

===3-D solid elements===

​

The use of 3-D elements for the prestressing steel modelization (see Figure [[#img-6|6]]) is used mainly in pre-tensioned beams <span id='citeF-25'></span>[[#cite-25|[25]]] where one of the main stress transfer mechanisms between strands and concrete (Hoyer effect <span id='citeF-26'></span>[[#cite-26|[26]]]) is also of 3-D nature.

​

<div id='img-6'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-3DTendon.png|420px|Tendon modelization using 3-D solid elements <span id='citeF-25'></span>[[#cite-25|[25]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 6:''' Tendon modelization using 3-D solid elements <span id='citeF-25'></span>[[#cite-25|[25]]]

|}

​

Modelling through 3-D elements introduces the need for using rectangular equivalent cross section for the prestressing steel but this allows an easy optimization of the contact between concrete and steel elements.

​

The use of this modelization scheme restricts the range of structures that can be studied. In fact, only construction with straight tendons are valid for this approach, i.e. only pre-tensioned structures or simple post-tensioned ones.

​

===Truss discrete elements===

​

This is probably the most extended option when using FEMs. In this case, tendons are simulated using trusses, which are linked somehow to the 3D FE mesh of the structure and the prestressing effect is considered as an imposed strain to the bar elements.

​

At the beginning, this methodology was only used in small structures because it had a big restriction: the FE mesh depended on the trusses path. This was because the methodology took into account the tendons effect by coupling the strengths of the prestressing steel and the concrete at the FE mesh nodes <span id='citeF-22'></span><span id='citeF-23'></span><span id='citeF-24'></span>[[#cite-22|[22,23,24]]].

​

Building a mesh adjusted to the tendons path is only possible in those cases where there are few tendons or when their geometry is simple, therefore this technique could not be used in most of the real life scenarios.

​

Despite this, it exists an approach introduced by the commercial code Abaqus <span id='citeF-27'></span>[[#cite-27|[27]]] that solves this big restriction. It is currently used in most of the prestressed concrete simulations and it is based on the so called ''embedded elements'' <span id='citeF-28'></span>[[#cite-28|[28]]].

​

<div id='img-7'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-EmbeddedAbacus.png|540px|Abaqus example of an embedded element <span id='citeF-28'></span>[[#cite-28|[28]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 7:''' Abaqus example of an embedded element <span id='citeF-28'></span>[[#cite-28|[28]]]

|}

​

Figure [[#img-7|7]] shows an example of two embedded elements. This approach constrains the degrees of freedom of the embedded element to the closest nodes of the hosting element using weight factors, which are determined based on their geometric location. This technique is not limited to truss elements. It can be used for membranes for example.

​

In spite of this improvement, the procedure has limitations. This is, in fact, an interpolation technique, where the results obtained in the analysis for the 3D FE mesh are used to compute results for the embedded elements. In the scenario of prestressed concrete structures, where the non-linear behaviour of concrete and the time dependent mechanisms of prestressing steel have to be considered, the use of this approach only solves partially the problem and there are still things to improve.

​

Figure [[#img-8a|8a]] shows an example of a structure solved using Abaqus embedded elements.

​

===Truss smeared elements===

​

This last approach is usually applied for big structures where using the other techniques is not feasible. In these cases, tendons are introduced in the analysis as ''embedded reinforcement'', i.e. the prestressing steel only appears in the analysis as an increment of the strength of the concrete FE. Therefore, this methodology introduces big simplifications in the analysis and has to be used carefully.

​

In fact, this approach is commonly used in current analysis to account for the reinforcing steel effect. In real prestressed concrete structures, this material is distributed more or less uniformly in specific directions (longitudinal rebars and shear reinforcement), which constitutes the perfect scenario to apply this approach.

​

This is the strategy followed by Tavakkoli, Kianoush et al. (2017) <span id='citeF-24'></span>[[#cite-24|[24]]] for the analysis of the reactor containment building shown in Figure [[#img-8b|8b]].

​

<div id='img-8a'></div>

<div id='img-8b'></div>

<div id='img-8'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-TrussE2.png|321px|FE mesh of a containment building analysed using Abaqus <span id='citeF-23'></span>[[#cite-23|[23]]]]]

|[[Image:Draft_Samper_351239591-TrussE1.png|540px|Containment building model where truss smeared elements are used for rebars <span id='citeF-24'></span>[[#cite-24|[24]]]]]

|- style="text-align: center; font-size: 75%;"

| (a) FE mesh of a containment building analysed using Abaqus <span id='citeF-23'></span>[[#cite-23|[23]]]

| (b) Containment building model where truss smeared elements are used for rebars <span id='citeF-24'></span>[[#cite-24|[24]]]

|- style="text-align: center; font-size: 75%;"

| colspan="2" | '''Figure 8:''' Examples where tendons and reinforcement have been modelled using truss elements

|}

​

=3 Modelization through the FEM=

​

This section intends to introduce the FEM, which is used as a base for the application of the SP RoM. In particular, the text will be focused on the development of the three-dimensional formulation using an elastic constitutive model.

​

==3.1 Introduction to FEM==

​

The FEM is a numerical method used in the analysis of structures to give an approximate solution to the differential equations that govern the problem. The use of this technique allows obtaining a continuum solution and therefore, getting a global vision of the structural behaviour. This is very attractive for studying the response of complex areas, e.g. D-regions or full structures with non-intuitive behaviour.

​

This methodology is build around the concept of FEs. These should be understood as each division in which the structure is split and analysed. Depending on the analysis nature, FEs can be 1-D (truss elements), 2-D (triangular or quadrilateral elements) or 3-D (tetrahedral or hexahedral elements) (Figure [[#img-9|9]]). For the development of the approach introduced at this monograph, hexahedral elements are needed, therefore the formulation presented in this section is the one used for 3-D problems.

​

<div id='img-9a'></div>

<div id='img-9b'></div>

<div id='img-9c'></div>

<div id='img-9'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|colspan="2"|[[Image:Draft_Samper_351239591-puente1D.png|480px|Bridge modelled using truss elements]]

|-

|- style="text-align: center; font-size: 75%;"

| colspan="2" |(a) Bridge modelled using truss elements

|-

|[[Image:Draft_Samper_351239591-presa2D.png|600px|Dam mesh using triangle elements]]

| [[Image:Draft_Samper_351239591-presa3D.png|480px|Dam mesh using tetrahedral elements]]

|- style="text-align: center; font-size: 75%;"

| (b) Dam mesh using triangle elements

| (c) Dam mesh using tetrahedral elements

|- style="text-align: center; font-size: 75%;"

| colspan="2" | '''Figure 9:''' Examples of the type of mesh that can be build using the FEM

|}

​

In the end, the FEM solves the whole structure working through many simple element equations over many small domains, i.e. the FEs. The procedure followed while performing a simulation using the FEM can be summed up in the following steps <span id='citeF-29'></span><span id='citeF-30'></span>[[#cite-29|[29,30]]]:

​

* Generate an appropriate model. The first thing to be done is a correct modelization of the problem. This includes:

​

* Build a geometrical model that represents the studied structure, paying attention to the possibility of including simplifications that could lighten the simulation, e.g. symmetries, plane stress case, plane strain case <span id='citeF-1'></span>[[#cite-1|[1]]], etc.

* Consider how the real constraints and the applied forces should be included in the model and so define the boundary conditions.

* Apply the correct material properties to the model.

* Define the scope of the analysis, e.g. small or large displacements, static or dynamic analysis, etc.

* Generate the mesh of FEs. The model is discretized in sub-domains in which the problem is solved locally. This mesh can be structured, unstructured or semi-structured <span id='citeF-31'></span>[[#cite-31|[31]]] and coarse or fine as needed.

* Define the equilibrium condition through the Principle of Virtual Work (PVW). The PVW is a necessary and sufficient condition for the equilibrium of the whole analysed structure or any of its sub-domains <span id='citeF-1'></span>[[#cite-1|[1]]].

* Compute the stiffness matrix <math display="inline"> K^e </math>  and load vector <math display="inline"> f^e </math> for each element. These are obtained from the PVW expression in terms of the nodal displacement of the FE mesh, i.e. <math display="inline"> K^e \, a^e - f^e =\Delta f^e </math>. This expression will be analysed later on.

* Obtain the global stiffness matrix (<math display="inline"> K </math>) and the global load vector (<math display="inline"> f </math>). These are obtained assembling all the <math display="inline"> K^e </math>'s and <math display="inline"> f^e </math>'s that come from the FE's analysis.

* Solve the system of equations <math display="inline"> K \, a=f </math>. The unknown displacement <math display="inline"> a </math> is obtained.

* Result assessment. Once the system of equations has been solved and the displacement vector <math display="inline"> a </math> has been found out, strains and stresses can be evaluated at each element. Also reactions at the restraint nodes can be computed. These results can be load into the model and presented graphically to their assessment. This is known as ''post-processing step''.

* Possible modifications. The last step of the FEM consists in considering possible changes that could improve the analysis performed. For example, consider a finer FE mesh or changing the FE typology.

​

Once the general procedure has been introduced, it is important to go in depth with the 3-D formulation and introduce the main concepts that are relevant for the monograph.

​

==3.2 FEM three dimensional formulation==

​

The use of a 3-D analysis using the FEM is usually related to the impossibility of using less costly procedures. This is the case of structures with irregular shapes and situations where the load patterns are arbitrary or the material properties are heterogeneous (Figure [[#img-10|10]]). In general, this is the case of post-tensioned concrete structures. Thus, the understanding of the subsequent formulation is essential for the progress of this dissertation.

​

<div id='img-10'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-3DExamples.png|420px|Structures which require a 3-D analysis <span id='citeF-1'></span>[[#cite-1|[1]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 10:''' Structures which require a 3-D analysis <span id='citeF-1'></span>[[#cite-1|[1]]]

|}

​

Isotropic elasticity theory is used at this stage in order to facilitate introducing the 3-D formulation although any other constitutive model could have been used instead.

​

Before dealing with the equations derived from the FEM, the formulas that control the 3-D elasticity problem must be introduced.

​

===3.2.1 Displacement, strain and stress field===

​

In a 3-D solid, the movement description of any point that belongs to that solid is done through the three components of the displacement vector:

​

<span id="eq-3.1"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{u}=\left[u,v,w\right]^T  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.1)

|}

​

Where <math display="inline"> u </math>, <math display="inline"> v </math> and <math display="inline"> w </math> are the displacement components of vector <math display="inline"> \mathbf{u} </math> in the directions of a cartesian reference system <math display="inline"> x </math>, <math display="inline"> y </math> and <math display="inline"> z </math>, respectively.

​

The strain field is then defined through the six strain components of the 3-D elasticity:

​

<span id="eq-3.2"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\boldsymbol{\varepsilon }  = \left[\varepsilon _x,\varepsilon _y,\varepsilon _z,\gamma _{xy}, \gamma _{xz},\gamma _{yz}\right]^T </math>

|-

| style="text-align: center;" | <math>     = \left[\dfrac{\partial u}{\partial x},\dfrac{\partial v}{\partial y},\dfrac{\partial w}{\partial z},\dfrac{\partial u}{\partial y}+\dfrac{\partial v}{\partial x}, \dfrac{\partial u}{\partial z}+\dfrac{\partial w}{\partial x},\dfrac{\partial v}{\partial z}+\dfrac{\partial w}{\partial y}\right]^T   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.2)

|}

​

Where <math display="inline"> \varepsilon _x </math>, <math display="inline"> \varepsilon _y </math> and <math display="inline"> \varepsilon _z </math> are the normal strains and <math display="inline"> \gamma _{xy} </math>, <math display="inline"> \gamma _{xz} </math> and <math display="inline"> \gamma _{yz} </math> are the tangential strains. These can be written in terms of the displacement vector components as shown in Equation [[#eq-3.2|3.2]].

​

Likewise, stress field can be defined through the six stress components as:

​

<span id="eq-3.3"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\boldsymbol{\sigma }=\left[\sigma _x,\sigma _y,\sigma _z,\tau _{xy}, \tau _{xz},\tau _{yz}\right]^T  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.3)

|}

​

Where <math display="inline"> \sigma _x </math>, <math display="inline"> \sigma _y </math> and <math display="inline"> \sigma _z </math> are the normal stresses and <math display="inline"> \tau _{xy} </math>, <math display="inline"> \tau _{xz} </math> and <math display="inline"> \tau _{yz} </math> are the tangential stresses defined according to the sign criterion shown in Figure [[#img-11|11]].

​

<div id='img-11'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-StressSignCriterion.png|420px|Sign criterion for the stresses in a 3-D solid <span id='citeF-1'></span>[[#cite-1|[1]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 11:''' Sign criterion for the stresses in a 3-D solid <span id='citeF-1'></span>[[#cite-1|[1]]]

|}

​

Finally, the relation between the strain and stress fields is expressed through a constitutive equation. In terms of isotropic elasticity this relationship can be written as:

​

<span id="eq-3.4"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\boldsymbol{\sigma }=\mathbf{C} \left(\boldsymbol{\varepsilon }-\boldsymbol{\varepsilon ^0}\right)+ \boldsymbol{\sigma ^0}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.4)

|}

​

Where the isotropic constitutive matrix (<math display="inline"> \mathbf{C} </math>) depends only on two material parameters, i.e. the Young modulus (<math display="inline"> E </math>) and the Poisson's ratio (<math display="inline"> \nu </math>). Therefore, the symmetric tensor <math display="inline"> \mathbf{C} </math> is given by:

​

<span id="eq-3.5"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{C}= \dfrac{E \left(1-\nu \right)}{\left(1+\nu \right)\left(1-2\nu \right)}    \left[\begin{matrix}1 & \dfrac{\nu }{1-\nu } & \dfrac{\nu }{1-\nu } & 0 & 0 & 0 \\     & 1 & \dfrac{\nu }{1-\nu } & 0 & 0 & 0 \\     &  & 1 & 0 & 0 & 0 \\     &  &  & \dfrac{1-2\nu }{2\left(1-\nu \right)} & 0 & 0 \\     & \mathrm{Sym.} &  &  & \dfrac{1-2\nu }{2\left(1-\nu \right)} & 0 \\     &  &  &  &  & \dfrac{1-2\nu }{2\left(1-\nu \right)}           \end{matrix}\right]  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.5)

|}

​

And the initial strain vector (<math display="inline"> \boldsymbol{\varepsilon ^0} </math>) due to thermal strains is:

​

<span id="eq-3.6"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\boldsymbol{\varepsilon ^0}=\alpha \left(\Delta T\right)\left[1,1,1,0,0,0\right]^T  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.6)

|}

​

===3.2.2 Equilibrium equation in 3-D (PVW)===

​

Equilibrium is guaranteed through the PVW <span id='citeF-1'></span>[[#cite-1|[1]]] expression that for 3-D solids is:

​

<span id="eq-3.7"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\iiint _V \delta \boldsymbol{\varepsilon }^T\boldsymbol{\sigma } \, dV = \iiint _V \delta \mathbf{u}^T\mathbf{b} \, dV + \iint _A \delta \mathbf{u}^T\mathbf{t} \, dA + \sum _i \delta \mathbf{a}_i^T\mathbf{p}_i  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.7)

|}

​

Where <math display="inline"> \delta \boldsymbol{\varepsilon } </math> and <math display="inline"> \delta \mathbf{u} </math> are respectively the virtual strains and virtual displacements, <math display="inline"> V </math> and <math display="inline"> A </math> are respectively the volume and the surface in which the body forces (<math display="inline"> \mathbf{b}=\left[b_x,b_y,b_z\right]^T </math>) and the surface tractions (<math display="inline"> \mathbf{t}=\left[t_x,t_y,t_z\right]^T </math>) are applied and <math display="inline"> \mathbf{p}_i=\left[P_{x_i},b_{y_i},b_{z_i}\right]^T </math> are the point loads acting at node <math display="inline"> i </math>. It is important to notice that <math display="inline"> C^0 </math> continuity is required for the finite element approximation because only first derivatives of the displacement are involved in Equation [[#eq-3.7|3.7]].

​

===3.2.3 Finite element formulation. The 8-noded hexahedra===

​

Once the equilibrium expression has been defined and all the involved variables have been introduced analytically, the FEM can be applied. For the purpose of this tmonograph, hexahedral elements are used and so it is interesting to present the finite element formulation using these elements.

​

There are several type of hexahedral elements but the current code used to run the methodology presented in this monograph is prepared to work using 8-noded linear hexahedras (Figure [[#img-12|12]]).

​

<div id='img-12'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-8NodedHexa.png|420px|Example of a 8-noded hexahedra with linear shape function <span id='citeF-1'></span>[[#cite-1|[1]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 12:''' Example of a 8-noded hexahedra with linear shape function <span id='citeF-1'></span>[[#cite-1|[1]]]

|}

​

===Shape functions===

​

Shape functions (<math display="inline"> N_i^{\left(e\right)} </math>) are polinomial interpolating functions defined over the domain of each element in the FE mesh that take the value one at node <math display="inline"> i </math> and zero at all other nodes. Therefore, Equation [[#eq-3.11|3.11]] satisfies <math display="inline"> u\left(x_i\right)=u_i^{\left(e\right)} </math>.

​

For 8-noded linear hexahedra, the nodal shape function can be written as:

​

<span id="eq-3.8"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>N_i\left(\xi , \eta , \zeta \right)= \dfrac{1}{8} \left(1+\xi _i\xi \right)\left(1+\eta _i\eta \right)\left(1+\zeta _i\zeta \right)  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.8)

|}

​

Where <math display="inline"> \xi , \eta , \zeta </math> are the natural coordinates as shown in Figure [[#img-13|13]]. This expression satisfies the two necessary conditions of a shape function: condition of nodal compatibility (Equation [[#eq-3.9|3.9]]) and rigid body condition (Equation [[#eq-3.10|3.10]]).

​

<span id="eq-3.9"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>N_i\left(\xi _j, \eta _j, \zeta _j\right)=\left\{\begin{array}{lll} 1 & \mathrm{if} & i=j \\ 0 & \mathrm{if} &  i \neq j\end{array}    \right.  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.9)

|}

​

<span id="eq-3.10"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\sum _{i=1}^{n}N_i\left(\xi , \eta , \zeta \right)=1  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.10)

|}

​

Further details about the procedure to be followed when obtaining shape functions can be found in specialised bibliography <span id='citeF-29'></span><span id='citeF-1'></span>[[#cite-29|[29,1]]].

​

<div id='img-13'></div>

{| class="floating_imageSCP" style="text-align: center; border: 1px solid #BBB; margin: 1em auto; width: 100%;max-width: 100%;"

|-

|[[Image:Draft_Samper_351239591-HexaNormGeom.png|600px|Example of a generic hexahedra FE and its normalized geometry <span id='citeF-1'></span>[[#cite-1|[1]]]]]

|- style="text-align: center; font-size: 75%;"

| colspan="1" | '''Figure 13:''' Example of a generic hexahedra FE and its normalized geometry <span id='citeF-1'></span>[[#cite-1|[1]]]

|}

​

===Discretization of the displacement field===

​

Considering a 3-D solid discretized into 8-noded hexahedras, the displacement field within each element can be expressed as:

​

<span id="eq-3.11"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{u}= \left\lbrace \begin{matrix}u\\   v\\   w   \end{matrix} \right\rbrace =\sum _{i=1}^{8} \mathbf{N}_i \mathbf{a}_i^{\left(e\right)}=\mathbf{N} \mathbf{a}^{\left(e\right)}   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.11)

|}

​

Where

​

<span id="eq-3.12"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{N}=\left[\mathbf{N}_1,\mathbf{N}_2,\dots ,\mathbf{N}_8\right]\qquad \qquad \mathbf{N}_i=\left[\begin{matrix}N_i & 0 & 0\\   0 & N_i & 0\\   0 & 0 & N_i   \end{matrix}\right]  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.12)

|}

​

and

​

<span id="eq-3.13"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{a}^{\left(e\right)} = \left\lbrace \begin{matrix}\mathbf{a}_1^{\left(e\right)}\\   \mathbf{a}_2^{\left(e\right)}\\   \vdots \\   \mathbf{a}_8^{\left(e\right)}   \end{matrix} \right\rbrace \qquad \qquad \mathbf{a}_i^{\left(e\right)} = \left\lbrace \begin{matrix}u_i\\   v_i\\   w_i   \end{matrix} \right\rbrace  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.13)

|}

​

are the shape function matrix and the displacement vector for each element and a node <math display="inline"> i </math>.

​

===Discretization of the strain field===

​

The new expression for representing the strain field in terms of the FEM is obtained combining Equation [[#eq-3.2|3.2]] and Equation [[#eq-3.11|3.11]]. The result is:

​

<span id="eq-3.14"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\boldsymbol{\varepsilon }=\sum _{i=1}^{8} \left\lbrace \begin{matrix}\dfrac{\partial N_i}{\partial x}u_i \\   \dfrac{\partial N_i}{\partial y}v_i \\   \dfrac{\partial N_i}{\partial z}w_i \\   \dfrac{\partial N_i}{\partial y}u_i+\dfrac{\partial N_i}{\partial x}v_i \\   \dfrac{\partial N_i}{\partial z}u_i+\dfrac{\partial N_i}{\partial x}w_i \\   \dfrac{\partial N_i}{\partial z}v_i+\dfrac{\partial N_i}{\partial y}w_i \\   \end{matrix} \right\rbrace = \sum _{i=1}^{8} \mathbf{B}_i \mathbf{a}_i^{\left(e\right)} = \sum _{i=1}^{8} \mathbf{B} \mathbf{a}^{\left(e\right)} </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.14)

|}

​

Where <math display="inline"> \mathbf{B} </math> is the element strain matrix that can be written as:

​

<span id="eq-3.15"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{B}=\left[\mathbf{B}_1,\mathbf{B}_2,\dots ,\mathbf{B}_8\right]  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.15)

|}

​

and <math display="inline"> \mathbf{B}_i </math> is the strain matrix of the node <math display="inline"> i </math>:

​

<span id="eq-3.16"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{B}_i=\left[\begin{matrix}\dfrac{\partial N_i}{\partial x} & 0 & 0 \\   0 & \dfrac{\partial N_i}{\partial y} & 0 \\   0 & 0 & \dfrac{\partial N_i}{\partial z} \\   \dfrac{\partial N_i}{\partial y} & \dfrac{\partial N_i}{\partial x} & 0 \\   \dfrac{\partial N_i}{\partial z} & 0 & \dfrac{\partial N_i}{\partial x} \\   0 & \dfrac{\partial N_i}{\partial z} & \dfrac{\partial N_i}{\partial y}   \end{matrix} \right]  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.16)

|}

​

Obtaining the shape function derivatives with respect to cartesian coordinates requires the use of the chain rule because they are expressed in normalized coordinates.

​

===Equilibrium equation in terms of the FEM===

​

Finally, the PVW expression (Equation [[#eq-3.7|3.7]]) can be written using the described formulas (Equations [[#eq-3.8|3.8]] to [[#eq-3.16|3.16]]). Therefore:

​

<span id="eq-3.17"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\iiint _V \mathbf{B}^T\boldsymbol{\sigma } \, dV = \iiint _V \mathbf{N}^T\mathbf{b} \, dV + \iint _A \mathbf{N}^T\mathbf{t} \, dA + \Delta \mathbf{f}^{\left(e\right)}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.17)

|}

​

Where it has been taken into account that virtual strain and virtual displacement are:

​

<span id="eq-3.18"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\delta \boldsymbol{\varepsilon }=\mathbf{B} \delta \mathbf{a} \qquad \qquad \delta \mathbf{u}=\mathbf{N} \delta \mathbf{a}   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.18)

|}

​

Equation [[#eq-3.17|3.17]] sets the equilibrium of internal and external forces at each element. <math display="inline"> \iiint _V \mathbf{B}^T\boldsymbol{\sigma } \, dV </math> is the internal nodal force vector for the element <math display="inline"> f_{int}^{\left(e\right)} </math> and the term <math display="inline"> \iiint _V \mathbf{N}^T\mathbf{b} \, dV + \iint _A \mathbf{N}^T\mathbf{t} \, dA </math> is the external load vector, which gives the information of the forces applied in each element <math display="inline"> f_{ext}^{\left(e\right)} </math>. Thus, this expression is equivalent to <math display="inline"> f_{int}^{\left(e\right)} - f_{ext}^{\left(e\right)} = \Delta \mathbf{f}^{\left(e\right)} </math>. Finally, <math display="inline"> \Delta \mathbf{f}^{\left(e\right)} </math> is the vector of equilibrating nodal forces, i.e. it has the information that guarantees the equilibrium of each element. Therefore, when the assembling is done it only contains the information related with the reaction forces.

​

Equation [[#eq-3.17|3.17]] can be rewritten as a system of equations considering the relation between strain and stress given by Equation [[#eq-3.4|3.4]]:

​

<span id="eq-3.19"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\iiint _V \mathbf{B}^T\mathbf{C}\mathbf{B} \, dV \mathbf{a}^{\left(e\right)}    -\iiint _V \mathbf{B}^T\mathbf{C} \boldsymbol{\varepsilon }^0 \, dV + </math>

|-

| style="text-align: center;" | <math>     + \iiint _V \mathbf{B}^T\mathbf{C} \boldsymbol{\sigma }^0 \, dV - \iiint _V \mathbf{N}^T\mathbf{b} \, dV - \iint _A \mathbf{N}^T\mathbf{t} \, dA=\Delta \mathbf{f}^{\left(e\right)}   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.19)

|}

​

Using the stiffness matrix (<math display="inline"> \mathbf{K}^{\left(e\right)} </math>) and the equivalent force vector (<math display="inline"> \mathbf{f}^{\left(e\right)} </math>) concepts, this equation is equivalent to:

​

<span id="eq-3.20"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{K}^{\left(e\right)} \mathbf{a}^{\left(e\right)} - \mathbf{f}^{\left(e\right)} = \Delta \mathbf{f}^{\left(e\right)}   </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.20)

|}

​

Where:

​

<span id="eq-3.21"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathrm{Stiffness \, matrix:} \qquad \mathbf{K}^{\left(e\right)} =\iiint _V \mathbf{B}^T\mathbf{C}\mathbf{B} \, dV </math>

|-

| style="text-align: center;" | <math>    \mathrm{Equivalent \, force \, vector:} \qquad  \mathbf{f}^{\left(e\right)} =\iiint _V \mathbf{B}^T\mathbf{C} \boldsymbol{\varepsilon }^0 \, dV - \iiint _V \mathbf{B}^T\mathbf{C} \boldsymbol{\sigma }^0 \, dV + </math>

|-

| style="text-align: center;" | <math>     \qquad +\iiint _V \mathbf{N}^T\mathbf{b} \, dV + \iint _A \mathbf{N}^T\mathbf{t} \, dA   </math>

|}

|}

​

Equation [[#eq-3.20|3.20]] sets the problem to be solved element by element and the global linear system of equation:

​

<span id="eq-3.21"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\mathbf{K} \mathbf{a} = \mathbf{f}  </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.21)

|}

​

can be obtained assembling the <math display="inline"> \mathbf{K}^{\left(e\right)} </math> and <math display="inline"> \mathbf{f}^{\left(e\right)} </math> contributions.

​

==3.3 Solving the system of equations==

​

At this stage of the analysis, the system of equations must be solved in order to finally obtain the strain values, the stress values, etc. at the studied structure. The procedure to be followed now depends on the type of analysis performed: linear or non-linear.

​

Prestressed concrete structures are a clear example of non-linear behaviour. The main procedures that can drive the structure in this range are related with the material degradation (damage in concrete, plasticity in steel, etc.) and the unavoidable changes that take place with time (creep, stress relaxation in prestressing steel, etc.). Therefore, for the purpose of this monograph, a strategy to solve non-linear systems of equations must be followed.

​

In these problems, the existence and uniqueness of the solution is not guaranteed. This makes it necessary to use an approach that follows the equilibrium path by using incrementation or continuity, which gives more information on the mechanical behaviour of the system and it also helps tracing the equilibrium path near critical points and facilitates convergence.

​

There are several techniques that can be used in order to solve a non-linear system of equations, which can be classified in explicit or implicit methods. For the purpose of this monograph an implicit approach has been used due to the robustness and the stability of these mechanisms: the ''Newton-Raphson'' technique <span id='citeF-32'></span>[[#cite-32|[32]]].

​

This iterative method assumes that, in a static analysis, the equilibrium equation has the general form:

​

<span id="eq-3.22"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;" 

|-

| 

{| style="text-align: left; margin:auto;width: 100%;" 

|-

| style="text-align: center;" | <math>\Delta \mathbf{f} = \left[\mathbf{f}^{int}\left(\mathbf{u}\right)\right]^{t+\Delta t} - \left[\mathbf{f}^{ext}\right]^{t+\Delta t} = \mathbf{0} </math>

|}

| style="width: 5px;text-align: right;white-space: nowrap;" | (3.22)

|}

​

Where <math display="inline"> \mathbf{f}^{int} </math> and <math display="inline"> \mathbf{f}^{ext} </math> are the internal and external force vectors that have already been introduced.

​

Equation [[#eq-3.22|3.22]] is the objective function and thus, the algorithm will iterate until this condition is reached. This expression can be written using the Taylor approximation series truncated at the second term:

​

<span id="eq-3.23"></span>

{| class="formulaSCP" style="width: 100%; text-align: left;"