II-46

XIII-та МЕЖДУНАРОДНА НАУЧНА КОНФЕРЕНЦИЯ ВСУ’2013 13th INTERNATIONAL SCIENTIFIC CONFERENCE VSU'2013

A FINITE ELEMENT NUMERICAL SIMULATION ON DIFFERRENT TYPES OF PRE-STRESSED CONCRETE COLUMNS 1 2 3 Magellan Chiritescu , Zoltan Kiss , Roxana Maria Muresan

Technical University of Cluj-Napoca, Romania, Faculty of Civil Engineering, Concrete and Steel Structures Department Abstract: Pre-stressing of concrete elements subjected to compression due to external loads is meaningful for: precast slender elements, as a safety measure against the cracking of concrete, columns subjected to long term, high intensity loads, to which a sudden unload may cause cracking, columns subjected to dynamic loads, to witch pre stressing of concrete brings an additional safety parameter towards the problem of cracking. An analysis of a partially pre-stressed concrete concrete column is carried out, following the provisions in EuroCode2, EuroCode2, using a cantilever static model. The analysis is done using Abaqus 6.11 6.11 finite element analysis software. The parameters considered in the analysis included longitudinal reinforcement ratio, degree of pre-stress, cross-section (active and passive) reinforcement positioning and the results are compared. Some conclusions are presented upon the influence of different parameters to the studied static model.

Key words: words: pre-stressed, columns, numerical analysis

1. Introduction. General presentation of the analysis Differentiated and antagonistic behavior of concrete in compression and respectively tension states makes the numerical modeling of it in finite element modeling programs a problem in itself. Within a certain numerical study of a concrete / reinforced reinforced concrete / prestressed concrete element, it is especially important the way the constitutive materials are defined, along with the definitions of geometrical conditions, boundary conditions, meshing characteristics of each constituent element and choosing the most favorable problem solving algorithm. The paper carries out a presentation of a numerical model analysis for a longitudinally pre-stressed, steel reinforced concrete specimen. The analysis is performed in Abaqus 6.11 commercial software program. The behavior of a cantilever model column type element was fulfilled. The analyzed models were subjected to a combined axial compression and bending loading pattern.

1 Magellan Chiritescu, PhD Student - Engineer, 25 Baritiu st., Cluj-Napoca, Romania, [email protected] 2 Zoltan Kiss, Professor of Structural Engineering, Phd -Engineer, 25 Baritiu st., Cluj-Napoca, Romania, [email protected] 3 Roxana Maria Muresan, PhD Student - Engineer, 25 Baritiu st., Cluj-Napoca, Romania, [email protected]


2. Finite element (FE) modeling The column’s geometry is based on an experimental model, designed, executed and tested within an extended experimental program developed by the Faculty of Civil Engineering in Cluj-Napoca. The replicated dimensions are 250 x 250 x 4700 mm. The boundary conditions and constraints are defined so that they would simulate an end restraint of a prefabricated concrete footing on the studied element. Thus, an encastre boundary condition was used, suppressing all displacement at one end of the specimen, consequently resulting in a 3900 mm long console type column. The simulation of a C60/75 concrete material was obtained by implementing within Abaqus 6.11 the Concrete Damaged Plasticity model (CDP). The meshing of concrete was done with type C3D8 tridimensional brick elements, with 8 nodes, 25 mm in dimension. The concrete part was defined as deformable solid with homogenous section. The parameters used to define the constitutive material laws for C60/75 concrete were determined in laboratory conditions and theoretically, following EC2 provisions, and are presented below: 2 - Elastic modulus: Ecm = 19700 N/mm ; - Poisson’s ratio: υc= 0.19; 3 - Mass density: ρc= 2500 daN/m ; 2 - Concrete compressive strength: f ck = 75.20 N/mm ; 2 - Concrete medium tensile strength: f ctm = 4.40 N/mm ; The constitutive parameters for the CDP model used are presented in table 1. Implementing the concrete compression damage and concrete tension damage CDP sub branches was done using the general stress-strain curves (figure 2.1), plotted in particular for a C60/75 concrete mix, thru experimental determinations and theoretical calculations following EC2. The individual plot defining points were tabularized and implemented in Abaqus. Table 1. Values for the constitutive parameters of Concrete Damage Plasticity model Dilation angle ψ ρ (Kc) Eccentricity m f 0/f cm γ Viscosity η

38

0.521

Fig. 2.1.

1.12

0.667

0.05

Left – longitudinal strain volumetric σ -ε plot; Right - σ -ε plot for damage plasticity;

The pre-stressing reinforcement ϕ12.9 mm, passive reinforcement ϕ14 mm and transversal ties ϕ6 mm were modeled as deformable trusses with wire type sections. All steel bars were meshed to 50 mm long, T3D2 truss type segments. In the case of the present study, perfect bond was admitted, this being implemented thru the embedded element option. Tendons modeled in the simulation were defined using the following characteristics:


- Elastic modulus: E p = 195000 N/mm2; - Poisson’s ratio: υ p= 0.29; 3 - Mass density: ρ p= 7850 daN/m ; - Tendon cross section area: A p12.90 = 100 mm2; 2 - Characteristic ultimate resisting force: f pk = 1860 N/mm ; 2 - Characteristic 0.1% proof stress: f p0.1k = 1680 N/mm ; Passive reinforcement and transversal ties modeled in the simulation used the following characteristics: 2 - Elastic modulus: Es = 195000 N/mm ; - Poisson’s ratio: υs= 0.29; 3 - Mass density: ρs= 7850 daN/m ; 2 - Passive reinforcement cross section area: A s14 = 154 mm ; 2 - Transversal tie cross section area: A s6 = 28.27 mm ; 2 - Characteristic ultimate resisting force: f yk = 500 N/mm ; Two distinct reinforcing models were studied, as part of the simulation. They are presented in figure 2.2. It can be observed that, steel quantity wise, the longitudinal reinforcement is basically the same. The differentiation is made by the distinct solutions for positioning the passive reinforcement bars within the concrete columns’ cross-sections.

Fig. 2.2 Analyzed cross-section types Four loading steps were defined. Throughout step 1, the initial state of the element, the tendons are pre-tensioned. The option is implemented as a predefined field. The pre2 stressing force for one tendon is set out to 110 kN, thus a 1100 N/mm tension being induced to each tendon wire. Obviously, total initial pre-stressing force in the concrete element is N p0=440 kN. Step 2 is necessary for allowing the pre-stressing force to be transmitted thoroughly to the entire concrete element. The element is loaded with the external compressive axial load (N ext=110 kN) during step 3. This is defined as a uniform pressure applied to the top surface of the concrete element. Step 4 consists in loading of the specimen with the external lateral force (P ext=0÷40 kN), developing with an incremental growth. As with the axial force, P ext consists of a uniform pressure load, applied to a 250 x 200 mm surface situated at the free end of the cantilever element. The integration method used was Newton-Raphson, with a maximum number of iterations of 500, so that the analysis can continue until ultimate fail force is reached.


a)

b)

c)

Fig. 2.3

Deformed shape of type S02 column a) lateral view 1; b) top view Deformed shape of type S03 column c) lateral view 1; d) top view

3. Analysis results The aim of the analysis was to record and monitor the behavior of the specimen and compare the results with estimates resulted from calculations or inferred from previous experimental research. The most influential factors to the results of the simulations were proven to be the constitutive laws of materials for concrete (mainly) and steel. Firstly, the plotting of a Lateral Force – Lateral Displacement curve was desired. The objective of this was to properly evaluate a real, experimental force, applied by the same principles. Plots showed in figure 3.1 were obtained after numerous tries in which different parameters were varied to calibrate, optimize and refine the initial models.

Fig. 3.1 Lateral Force – Lateral Displacement plot Differences to the behaviour of the two studied models are observed. In this way, though failing under almost identical lateral loads, P ext S02 =38.64 kN and P ext S03 =38.87 kN, type 02 column demonstrates a more ductile behaviour, with top maximum


displacement dmax S02 =201 mm, as opposed to d max S03 =173 mm, the top maximum displacement of type 03 column. This was predicted in the preliminary calculations and is explained by the more favourable positioning of the passive reinforcement within the specimen’s cross-section, thus leading to an increase in ductility near the fixed end of the element. A notable phenomenon is the relatively liniar behaviour of both types studied until itteration stop. The lack of a plastic plateau is somehow plausible, taking into consideration that the load is applied monotoniously until faliure, with no ciclicity in the service loading range what so ever. Another objective of the analysis was to monitor the stress and strain values resulting in the reinforcement bars, both pre-stressed and passive, to the main tensioned-stressed points. The purpose of this was to have an accurate estimate to how a real concrete element would suffer ultimate failure.

a) b) Fig. 3.2 a) stress-strain plot for tendon in tension; b) stress-strain plot for passive reinforcement in tension It is observed from figures 3.2.a) and 3.2.b) that tendons and passive reinforcement bars within type S02 element reaches the defined flow plateau, experiencing great strain growth, under relatively small stress increment. This leads one to predicting a ductile behavior prior to a warned failure, by rupture of tensioned reinforcement bars. In contrast, type S03 element is far from reaching the predefined elastic limit stress, both for tendons and passive reinforcement bars. This outlines a brittle failure, unwarned, by reaching the characteristic compressive strength and spalling of concrete on the compressed section’s side, near the fixed end.

Conclusions The purpose of the study was to arrive at an optimized prototype of a pre-stressed concrete column, aiding to the design, execution and essay within an experimental program developed at the Faculty of Civil Engineering in Cluj-Napoca. The results obtained from the numerical parametric analysis are of use because a good estimation of the real test specimens’ behavior in reached. Based on the results shown in chapter 3 of the paper, the proposed model and its constitutive parameters seem to be suitable for predicting the response of a cantilever static model concrete column subjected to combined compression – lateral loading.


Acknowledgement This paper was supported by the project "Improvement of the doctoral studies quality in engineering science for development of the knowledge based society-QDOC” contract no. POSDRU/107/1.5/S/78534, project co-funded by the European Social Fund through the Sectorial Operational Program Human Resources 2007-2013. REFERENCES [1] ABAQUS. Abaqus analysis user's manual, Version 6.11, Dassault Systèmes. [2] Bompa D. V., Oneț T. Flat slab-column connection model calibration using Concrete Damaged Plasticity, Proceedings CIBv, pp. 29-36, 2010. [3] Grijalba D. Centrally pre-stressed fiber reinforced concrete columns, Boca Raton Florida, 2011. [4] Socaciu N. Phd Thesis: Behavior and calculation of reinforced concrete columns subjected to eccentric loading, UTCN, Cluj-Napoca, 1995.

II-46

Recommend Documents