^{1}

^{1}

^{1}

This paper verifies the accuracy of a methodology recently proposed on reinforced concrete beam tested in flexure available from literature. This was implemented using the general purpose FEA software Abaqus. A very good agreement between numerical and experimental study was obtained. The compression failure, tension failure matched with experimental findings which shows the applicability of the methodology.

Reinforced concrete beam is an important element in a structure as it carries and distributes the lateral loads coming on it. Manual design of reinforced concrete beams is a laborious task hence various FEA software were developed to fasten the design and analysis of reinforced concrete beams, among various available FEA software’s Abaqus provides much convenience to the user as the properties of materials can be tailored to suit the analysis. Hence, Abaqus was chosen to analyse a reinforced concrete beam from literature [

The test specimen consists of two 8 mm bars as tensile reinforcement, two numbers of 12 mm bars as compression reinforcement. Shear links were arranged closely in the shear spans at a spacing of 75 mm c/c whereas the constant

Concrete | Concrete Properties | ||
---|---|---|---|

fc, MPa | ft, MPa | Ec, MPa | |

C19.9 | 19.9 | 2.1 | 22,904.69 |

fc, Concrete compressive strength; Ft, Concrete tensile strength; Ec, Elastic Modulus.

Steel | Steel Properties | |
---|---|---|

fy, MPa | fu, MPa | |

8 mm | 569 | 631 |

12 mm | 561 | 637 |

fy, Yield stress; fu, Ultimate stress.

bending region was provided at 120 mm c/c as shown in

The numerical model consists of modelling all the components of the reinforced concrete beam as shown above. Concrete and loading steel plates were modelled using C3D8R, an 8-node linear hexahedral element, reinforcement including shear link was modelled as truss element, supports were modelled as roller with restraint in only y direction. Loading was applied as displacement controlled.

Concrete ModelConcrete was modelled using Concrete Damage Plasticity parameter (CDP). A standard model in compression and tension as provided by BAlfarah [

Various values from 0 to 0.0005 were tried to check the convergence of the numerical model. A value of zero always led to non-convergence, hence after running a check, it was identified 0.0005 would better suit to the needs of the numerical model and hence it was selected for the present simulation.

Three mesh sizes were studied in order to study its influence on the numerical results. A mesh size of 15 mm was chosen as it showed good correlation with the experimental results. A plot showing the influence of different mesh size ranging from 15, 20, 25, 30 is shown in

Dilation angle is a parameter which can influence the CDP parameters. Lesser values make the concrete material brittle whereas higher values make the concrete stiffer [

From the previous parameters chosen the numerical model was run to ascertain its ability to predict experimental findings using the parameters shown in

Concrete Damage Plasticity Parameters | K | m | ||
---|---|---|---|---|

y | l | fbo/fco | ||

50 | 2.1 | 22,904.69 | 0.667 | 0.0005 |

The CDP model requires damage parameters to be input as compressive and tensile damages. These damage parameters were obtained as per the model and a damage value of 0 implies no crushing or tensile rupture whereas a damage value of 1 indicates total crushing of concrete in concrete and rupture in tension respectively.

As it can be seen from

Figures 8-10 shows various damage patterns as obtained from the FEA model. The extensive tensile damage seen in the FEA model agrees well with the experiment. The compression failure observed in

Load | Displacement | |||||
---|---|---|---|---|---|---|

First Crack Load (kN) | Yield Load (kN) | Ultimate Load (kN) | First Crack (mm) | Yield (mm) | Ultimate (mm) | |

Experiment | 9.8 | 30.1 | 34.6 | 1.06 | 6.1 | 30 |

FEA | 14.70 | 35.15 | 38.92 | 1.66 | 8.20 | 34.63 |

*[

loading plate span. The plastic strain is also used to trace cracking in reinforced concrete members, from the observed trend in PE, max most of the critical cracks are located with the pure moment region which again agrees well with the experiment.

From the study undertaken in this paper, the following conclusions can be drawn:

1) The FEA model adequately predicts the overall behaviour of the reinforced concrete beam, hence it can be further developed to model other types of reinforced concrete specimens.

2) Although the results from FEA model are on higher side compared to experimental findings, the yield load, ultimate load, yield displacement and ultimate displacement are very well close to the experimental findings which show that the current model could be accepted.

3) The FEA simulation perfectly predicts the compression crushing failure observed in the experiment.

4) The tensile damage obtained from the FEA study is also in line with the experimental findings.

5) From the above points it can be inferred that the developed FEA model could possibly be improved to further predict the accurate values of first crack, yield and ultimate loads.

The authors would like to acknowledge RDF 16-01-17 financial support from XJTLU.

The authors declare no conflicts of interest regarding the publication of this paper.

Revanna, N., Moy, C.K.S. and Krevaikas, T. (2020) Verifying a Finite Element Analysis Methodology with Reinforced Concrete Beam Experiments. Journal of Applied Mathematics and Physics, 8, 2549-2556. https://doi.org/10.4236/jamp.2020.811190