Content uploaded by Farhaan Zaidi Bhat
Author content
All content in this area was uploaded by Farhaan Zaidi Bhat on Jul 23, 2021
Content may be subject to copyright.
International Journal of Engineering Applied Sciences and Technology, 2021
Vol. 6, Issue 1, ISSN No. 24552143, Pages 223227
Published Online May 2021 in IJEAST (http://www.ijeast.com)
223
FINITE ELEMENT ANALYSIS OF CONCRETE
SPECIMEN
Farhaan Zaidi Bhat Shaista Kanni
Bachelor Candidate, Department of Civil Engineering Associate Professor, Department of Civil Engineering
SSM College of Engineering, Kashmir, India SSM College of Engineering, Kashmir, India
Abstract—Finite element analysis is a numerical
technique that uses computational power to calculate
approximate solution to given problem. Since this method
is based on energy principle, it can be used to solve
problems related to solid mechanics, fluid mechanics, heat
transfer and electrodynamics. This paper compares the
experimental results of compression test performed on
concrete specimen in laboratory with the numerical results
obtained using the finite element analysis of concrete
model simulated in ABAQUS software. Compression test
of ceramic concrete cubes and cylindrical specimen with
M20 concrete characteristics and coarse aggregate
partially replaced by BoneChina ceramic was performed
in a laboratory. The experimental results obtained were
then used as input parameters for the numerical
simulations. The strength of the concrete depends on a lot
of factors including curing time, temperature, water
cement ratio, moisture condition etc., and hence the
modelling of the concrete specimen should be done
carefully. Concrete damaged plasticity (CDP) model
available in software package was used to reflect the
behavior of the concrete model in compression as well as
tension. Threedimensional nonlinear finite element
model was developed and analyzed by the Quasistatic
technique using the ABAQUS explicit module. Results
show that the model simulated using Finite element
method was able to predict the damage behavior of
concrete specimen fairly accurately despite the variable
nature of concrete. Hence, finite element analysis is an
economical and timeefficient method of advanced
structural analysis that can be used to study the structural
behavior of concrete in compression.
Keywords—Finite element analysis; Concrete; Concrete
damage plasticity (CDP); ABAQUS
I. INTRODUCTION
Concrete is the most widely used construction material in the
world and is second only to water as the most utilized
substance on the planet. It is obtained by mixing cementing
materials, water, aggregates and sometimes admixture. An
estimated 33 billion tons of concrete are manufactured
globally each year. According to the Press Information
Bureau, India generates 62 million tons of waste (mixed waste
containing both recyclable and nonrecyclable waste) every
year, with an average annual growth rate of 4% (PIB 2016).
Time to time, different waste materials have been used to
replace the constituent material of concrete and determine its
effect on the strength of concrete. This paper reports:
(a) the findings on an experimental investigation of the effect
of partial replacement of coarse aggregate with BoneChina
ceramic waste on strength properties of concrete and
(b) the accuracy of the finite element analysis in comparison
to experimental results.
Compressive strength tests were conducted using
150x150x150mm cube specimen and 150x300 mm cylindrical
specimen.
In this paper, a 3D nonlinear finite element model is presented
to analyze BoneChina ceramic concrete cube subjected to
compression load to obtain its ultimate compressive strength.
Material damage criteria and analysis technique are very
important to be considered in nonlinear finite element analysis
in order to obtain a good result up to the ultimate load bearing
capacity of the material. Considering the brittle nature of the
concrete material, explicit dynamics analysis procedure was
employed using ABAQUS/Explicit module. The concrete
damaged plasticity (CDP) model as depicted in Figure 1 was
used to simulate the Bone China ceramic concrete. It uses
stressstrain relationships obtained using experimental
methods to correlate parameters for relative concrete damage
for both tension and compression. The concrete damaged
plasticity model in Abaqus:
provides a general capability for modelling concrete
and other quasibrittle materials;
uses concepts of isotropic damaged elasticity in
combination with isotropic tensile and compressive
plasticity to represent the inelastic behavior of
concrete;
is designed for applications in which concrete is
subjected to monotonic, cyclic, and/or dynamic
loading under low confining pressures (Abaqus 6.9,
2009).
International Journal of Engineering Applied Sciences and Technology, 2021
Vol. 6, Issue 1, ISSN No. 24552143, Pages 223227
Published Online May 2021 in IJEAST (http://www.ijeast.com)
224
Figure 1. Concrete damaged plasticity modified stress/strain
curve
II. EXPERIMENTAL PROCEDURE
A. Mix Proportion for producing BoneChina Ceramic
concrete
Materials used in the boneChina ceramic concrete are Coarse
aggregate (20mm – 10mm), Bone China Ceramic waste
(20mm – 10mm), Ordinary Portland cement and fine sand
passing through 4.75mm sieve. The ratios of the materials are
listed in Table 1. 10% of the coarse aggregate was replaced
by boneChina ceramic to determine its effects on the
structural strength of concrete having nominal mix ratio of
1:1.5:3 (M20) and a fixed water: cement ratio of 0.45. The
boneChina ceramic concrete was cast into cubes and
cylinders. The compression test was conducted over 28 days
of casting.
Table 1. Mixture ratio for casting of BoneChina ceramic
concrete cube
Coarse aggregate: Bone
China
Water: Cement
Ratio
1 : 0.1
0.48
B. Test Configuration & Instrumentation
The compressive strength of boneChina ceramic concrete
was obtained from the compression test on cubes which was
carried out using Universal Testing Machine (Capacity 3000
KN) according to IS 516: Part 5: 1959. The tensile strength of
boneChina ceramic concrete was determined from split test
on cylinders according to IS 5816:1999 and IS 456:2000. The
Young’s Modulus value was obtained according to IS
456:2000 as Ec = 5000√fck. Poisson’s Ratio was assumed as
0.2. The difference in the mean compressive strength between
the Control sample and the Ceramic specimen was found to
vary only about 4% which is negligible considering the
varying nature of the concrete. Hence, it can be concluded
that we can use the ceramic waste to replace the coarse
aggregate in the concrete satisfactorily up to 10% without
compromising the strength of the concrete.
Table 2. Properties of BoneChina Ceramic concrete
Dimension
(mm3)
Pc
(MPa)
Fc
(KN)
Ft
(KN)
E (MPa)
Mass
Density
(p)
(kg/m3)
Poisson
Ratio, v
150 x 150
x 150
23.17
521.325
1.68
24067.61
2456.47
0.2
0
5
10
15
20
25
Control Specimen Bone China
replacement
24.14 23.17
Mean 28day compressive
strength
( in MPa )
Specimen Type
Laboratory Result
Figure 2. Variation of strength due to coarse aggregate
replacement.
III. FINITE ELEMENT ANALYSIS
A. Material Properties
A 3D nonlinear, quasistatic finite element model was
developed using ABAQUS/Explicit module to study the
behavior of the boneChina concrete cube under compression.
Since the variation in result between the M20 concrete and the
boneChina replaced concrete was fairly less, material
properties required to calculate the concrete damage
parameters as input variable to the FE model were obtained
from (1) Milad Hafezolghorani, Farzad Hejazi, et al.
(Simpliﬁed Damage Plasticity Model for Concrete). The
damage parameters are calculated based on the stressstrain
relations under uniaxial tension and compression loading.
Table 3 shows the constitutive parameters used in simulating
the concrete damaged plasticity model in ABAQUS software
for both compressive and tensile behavior of M20 concrete
material. The parameters listed in Table 3 which were not
measurable from the experiment were assumed using values
of normal strength concrete (Abaqus 6.9, 2009). Since the
concrete damaged plasticity of boneChina ceramic concrete
had not been identified by previous research, the concrete
damaged plasticity parameters were assumed based on the
parameters of normal strength concrete.
Table 3. Concrete damaged plasticity of M20 concrete
Concrete Damaged
Plasticity
Dilation
angle
Eccentricity
Uniaxial/Biaxial
ratio σc0/σb0
K
Viscosity
parameter
31o
0.1
1.16
0.67
0
Compressive Behavior from
Tensile Behavior from experiment
International Journal of Engineering Applied Sciences and Technology, 2021
Vol. 6, Issue 1, ISSN No. 24552143, Pages 223227
Published Online May 2021 in IJEAST (http://www.ijeast.com)
225
experiment
Yield
Stress
(MPa)
Inelastic
Strain
Damage
Parameter
(D)
Yield
Stress
(MPa)
Inelastic
Strain
Damage
Parameter
(D)
10.2
0
0
2
0
0
12.8
7.74E05
0
0.02
0.000943
0.99
15.0
0.0001736
0



16.8
0.0002887
0



18.2
0.0004226
0



19.2
0.0005755
0



19.8
0.0007472
0



20.0
0.0009377
0



19.8
0.0011472
0.01



19.2
0.0013755
0.04



18.2
0.0016226
0.09
16.8
0.0018887
0.16
15.0
0.0021736
0.25
12.8
0.0024774
0.36
10.2
0.0028000
0.49
7.20
0.0031415
0.64
3.80
0.0035019
0.81
B. Modelling of Concrete, Interaction, Loading and
Analysis Control
In the ABAQUS model, C3D8R elements, a continuum 3
Dimensional, eightnoded, reduced integration point element,
were selected. For boundary conditions, constant
displacement was applied at the rigid body on top until the
failure occurred and the bottom surface was encastered.
Coupling was defined for interaction between different nodes
to eliminate local stress condition; Concrete crushing issue
and spalling were neglected. In order to reduce the impact and
inertia effects from explicit dynamic procedure and to ensure
the equivalent static response is obtained, the loading period
was adjusted until the kinetic effect become minimum.
Loading period was fixed at 1 second after the process of trial
and error with the initial trial value based on the natural
frequency of the M20 concrete cube.
IV. RESULTS AND DISCUSSION
A. Effectiveness of Mesh Density
Models with different mesh refinement were analyzed to
determine the best mesh density that gives reasonable
accuracy of results and reasonable analysis time. Results of
compressive force, Fc for various refined element meshes are
shown in Table 4 and plotted in Figure 3. From the
comparison of compressive strength with experimental
results, mesh density with 10164 elements provided a
reasonable result as the experiment with reasonable
computing time. Table 4. Result of mesh refinement study
ABAQUS
Mesh Type
Size
Total
Nodes
Total
Elements
Fc (kN)
% Difference from
Experiment
Experimental
Data


521.32

C3D8R – 50
100
48
681.133
23.46
C3D8R – 40
125
64
653.64
20.24
C3D8R – 25
343
216
633.043
17.64
C3D8R – 18
729
512
617.965
15.63
C3D8R – 15
1331
1000
610.213
14.56
C3D8R – 12
2366
1872
603.375
13.59
C3D8R – 11
3375
2744
597.843
12.79
C3D8R – 10
4624
3840
596.0.13
12.53
C3D8R – 9
5202
4352
595.23
12.41
C3D8R – 8
7220
6156
592.217
11.97
C3D8R – 7
11638
10164
586.57
10.78
0
5
10
15
20
25
30
35
Stress (in MPa)
Strain
Convergence Study Mesh 7
Mesh 8
Mesh 9
Mesh 10
Mesh 11
Mesh 12
Mesh 15
Mesh 18
Mesh 25
Mesh 40
Mesh 50
Figure 3. Mesh density study of finite element analysis
B. Failure Behaviour and Crack Pattern
The stressstrain curves from FE analysis (10164 elements
model) were plotted in Figure 4. It can be seen that result
achieved ultimate compressive stress with 90% accuracy as
compared to the experimental result with former having a
mean value of 23.17 N/mm2 and latter having value just over
25 N/mm2.
International Journal of Engineering Applied Sciences and Technology, 2021
Vol. 6, Issue 1, ISSN No. 24552143, Pages 223227
Published Online May 2021 in IJEAST (http://www.ijeast.com)
226
Figure 4. Finite element analysis result
Failure modes were compared as shown in Figure 5(a) and
5(b). It can be seen that the crack in the experiment had
occurred at one corner and along the height of the cube which
is identical to the contour plot of the analysis. In the
experiment, imperfection of the test specimen, such as uneven
cube surface and uneven distribution of bonechina ceramic
might had caused the crack to occur only at one corner of the
cube.
(a) Experimental result (b) Numerical result
Figure 5. Comparison of failure mode for boneChina ceramic
concrete cube
Crack propagations in the concrete cube model are shown in
Figure 6 (a), (b), (c), and (d). In Figure 6 (a), the uncracked
section is shown. Then, as shown in Figure 6 (b) crack
appears near the edge and along the height of concrete and
propagate towards the center of the cube and then Figure 6(c)
to (d), the concrete cube expended at the middle height due to
the compression force applied to it. The maximum load was
achieved on stage (b) when the damage occurred. Figure 6 (c)
to Figure 6 (d) are the condition beyond the maximum load.
Stage(a)
Stage(b)
Stage (c)
Stage(d)
Figure 6. Damage wave propagation of cube from failure, (b)
to post failure, (c) & (d)
Once the constitutive parameters used in concrete damaged
plasticity model are known, the resulting ultimate stress of
concrete specimen of any shape having those characteristics
can be simulated using Finite element analysis. Figure (7)
shows the FEA analysis of a cylindrical specimen having
same failure criteria as obtained from the experimental results.
a) Experimental Result b)Numerical Result
International Journal of Engineering Applied Sciences and Technology, 2021
Vol. 6, Issue 1, ISSN No. 24552143, Pages 223227
Published Online May 2021 in IJEAST (http://www.ijeast.com)
227
Figure 7. Comparison of failure mode for
cylindrical specimen
V. CONCLUSION
Compression test of the boneChina ceramic concrete cube
was modelled and analyzed using finite element method. The
concrete was modelled using C3D8R element. The damage
criterion for the concrete was modelled with concrete damage
plasticity and the material property parameters were obtained
from experimental results and partially from (1) Milad
Hafezolghorani, Farzad Hejazi, et al. Quasistatic analysis
using ABAQUS/ Explicit was employed and the equivalent
static result was ensured by controlling the loading period.
The result of the study shows that finite element procedure
employed in this study can simulate the compression test of
the bone China ceramic concrete cube/M20 concrete
accurately to a great extent. Increase in the accuracy of
concrete parameters results in increased accuracy in finite
element results. In spite of the variable nature of concrete and
computational limitation, around 90% accuracy of finite
element model in comparison to the experimental results was
achieved. Hence, it can be concluded that finite element
analysis is a useful computational tool which can be used to
solve problems in an economical and timeefficient manner
and with the advancement in the field of computer science,
this field is bound to reach its full potential. The model and
analysis method employed in this study can be used as a guide
in modelling the boneChina ceramic concrete/M20 concrete
under compression and the accuracy of the model may be
increased by variation in the methodology.
VI. ACKNOWLEDGEMENTS
The author would like to thank SSM College of
Engineering and Technology Parihaspora, Pattan, Kashmir
especially Shaista Ma’am and Muzammil sir for supporting,
guiding me throughout the process. I would also like to thank
Chief Engineers office, Rajbagh for providing facilities and
services for concrete testing.
VII. REFERENCES
[1] Milad Hafezolghorani, Farzad Hejazi et al (2017)
Simpliﬁed Damage Plasticity Model for Concrete DOI:
10.2749/101686616X1081
[2] Wan In Goh, Norida Mohamad, et al (2014) Compression
Test and Finite Element Analysis of Foamed Concrete
cube Journal of Engineering and Technology Vol 5, No.
1,
[3] Jankowial, T., & Lodygowski T. (2005). Quasi static
failure criteria for concrete. Foundations of Civil and
Environmental Engineering, 6, 5369. ISSN 16429303
[4] Simulia D. ABAQUS 6.11 analysis user’smanual.
ABAQUS 611 Documentation, 2011
[5] Jason. L, Cabot, P, Huerta G. & Ghavamian. S. (2004).
Damage and plasticity for concrete behavior. European
Congress on Computational Methods in Applied Sciences
and Engineering, German. pp 116.
[6] Lee, J. & Fenves, G. (1998). PlasticDamage Model for
Cyclic Loading of Concrete Structures. Journal of
Engineering Mechanical, 124(8), 892–900.
[7] S. N. Mokhatar & R. Abdullah. (2012). Computational
Analysis of Reinforced Concrete Slabs Subjected to
Impact Loads. International Journal of Integrated
Engineering, 4(2), 7076.
[8] Sourav Basak and D.K Paul (2012). Damage Evaluation
of a RCC Containment Structure subjected to internal
pressure. International Journal of Engineering Science
and Technology 4(6), 2823282
[9] Farhaan Zaidi Bhat (2021) Application of Finite Element
Analysis, Researchgate 352017598
[10] Lee J, & Fenves GL. Plasticdamage modelfor cyclic
loading of concrete structures.J. Eng.Mech.1998;124(8):
892–900
[11] Zhang J, Zhang Z, & Chen C. Yield criterion in plastic
damage models for concrete.Acta Mech. Solida
Sin.2010;23(3): 220–230
[12] Grassl P, Nystrom U, Rempling R,Gylltoft K. A
damageplasticity model for thedynamic failure of
concrete. arXiv preprint2011; arXiv:11031288
[13] Grassl P, Xenos D, Nyström U,Rempling R, &
Gylltoft K. CDPM2: adamageplasticity approach to
modelling thefailure of concrete.Int. J. Solids
Struct.2013;50(24): 3805–3816.