Three dimensional nonlinear finite element modeling of charpy impact test

International Journal of Mechanical Engineering and Technology (IJMET), ISSN 0976 –
6340(Print), ISSN 0976 – 6359(Online) Volume 4, Issue 4, July - August (2013) © IAEME
377
THREE DIMENSIONAL NONLINEAR FINITE ELEMENT MODELING OF
CHARPY IMPACT TEST
Fadi A. Ghaith*
, Fahad A. Khan
Department of Mechanical Engineering, Heriot-Watt University, Dubai Campus, P O Box 294345,
United Arab Emirates
ABSTRACT
In this paper, a three-dimensional Finite Element (FE) model was performed to simulate the
impact test ofnormalized carbon steel and aluminum specimens. The model specifications were
developed according to ASTM E-23 standard requirements. Also the established FE model took into
account all sources of non-linearity such as geometric, material and contact nonlinearities. A failure
criterion is assumed to be at 10 % of plastic strain based on the tensile experiment data. Based on the
simulation results, it was found that the absorbed energy required for fracture of the steel and
aluminum specimens under the impact load at room temperature are44.6J and 20.4J, respectively. In
comparison with the corresponding values resulted from the experimental Charpy impact test, the
percentage of error didn’t exceed 7 % for both steel and aluminum specimens. Also this paper
demonstrated the influences of the notch depth and shape on the absorbed energyby conducting the
relevant parametric studies. Finally, the importance of the present 3-dimensional model over the 2-
dimensional model was demonstrated in terms of applicability, accuracy and reliability.
Keywords: Charpy test, impact energy, nonlinear, finite element, three dimensional.
1. INTRODUCTION
The failure of engineering materials is an undesirable event for several reasons; that include
safety of human lives and economic losses. Therefore impact testing techniques were established so
as to ascertain the fracture characteristics of materials. Charpy impact test involves measuring the
energy consumed in breaking a notched specimen simply supported at both ends when it is
hammered by a swinging pendulum. The presence of a notch simulates the pre-existing cracks found
in large structures and increases the probability of brittle fracture. Charpy impact testing is a low-cost
and reliable test method, which is commonly required by the construction codes for fracture of
critical structures such as bridges and pressure vessels. It took from about 1900 to 1964, for impact
INTERNATIONAL JOURNAL OF MECHANICAL ENGINEERING
AND TECHNOLOGY (IJMET)
ISSN 0976 – 6340 (Print)
ISSN 0976 – 6359 (Online)
Volume 4, Issue 4, July - August (2013), pp. 377-386
© IAEME: www.iaeme.com/ijmet.asp
Journal Impact Factor (2013): 5.7731 (Calculated by GISI)
www.jifactor.com
IJMET
© I A E M E

378
test technology and procedures to reach the levels of accuracy and reproducibility so that they could
be broadly applied, started from Charpy tests in 1905 up to the issue of the revised Standard of
ASTM E-23 in 1964. Many researchers developed simple mathematical models to describe the
impact phenomena [1, 2], but some of themdidn’t address the geometric and contact nonlinearities
while other studies were limited to the lumped analysis. Recently, Computer simulation method has
been developed in order to accurately simulate the fracture phenomena that can be considered during
impact test. Belytschko and Bartel [3] research is considered one of the earliest work in developing a
nonlinear transient analysis for large scale deformation using the finite element analysis. Full three
dimensional analyses of the failure modes in Charpy impact test was carried out by Mathur et al. [4].
This workaimed to investigate the influence of the specimen dimensionson the plastic straining at the
notch. It was found that there are some three-dimensional effects in that material failure grows more
rapidly at the center of the specimen than near the free surface end of the notch. Also it was found
that the force against time dependence predicted by the plane strain computations produced a
reasonably good approximation of the corresponding three-dimensional results. Tvergaard and
Needleman [5] investigated the ductile-brittle transition for a weld by means of numerical analyses
of Charpy impact specimens. The material response was characterized by an elastic-visco-plastic
constitutive relation for a porous plastic solid, with adiabatic heating due to plastic dissipation. The
predicted work to fracture showed a strong sensitivity to the location of the notch relative to the
weld, with the most brittle behavior for a notch close to the narrow heat affected zone. This analysis
illustrated the strong dependence of the transition temperature on stress triaxiality. Lorriot [6]
proposed an experimental method based on the specimen displacement measurement using laser
sensor in order to determine the actual specimen loading in instrumented impact test. The prediction
resulting from this approach was compared with results deduced from dynamic analysis of impact
tests with mass-spring model. Altenhof et al. [7] focused on their research on the development of a
material model for the AM50A magnesium alloy, which is frequently used in the automotive
industry. Computer model was developed and validated through experimental setup and numerical
simulation of standardized Charpy and tensile tests. The material model was further used to predict
the behavior of an AM50A magnesium alloy steering wheel armature by performing experimental
and numerical impact tests. Chao et al. [8] examined the advanced high strength steels (AHSS) that
gradually adopted in vehicle structures as lightweight materials in the past years. In this work, results
from Charpy V-Notch impact tests on dual phase 590 (DP590) steel were presented and tests were
conducted at temperatures ranging from 120°
C to 90 °
C and DBTT was determined.Rubio-Gonzalez
et al. [9] performed an analysis of dynamic fracture toughness of pre-fatigued materials using the
split Hopkinson bar apparatus. This setup had been arranged to measure the dynamic loads acting on
notched and pre-fatigued bend specimens made of AISI 4140-T steel and A6061-T6 aluminum.
Same metal specimens with identical properties were used in the FE simulation presented in this
work for the purpose of validation. Ghaith [10] developed a two-dimensional FE model to estimate
the impact energy required for the fracture of carbon steel AISI 4140 specimen. Also he was able to
estimate the Ductile to Brittle Transition Temperature (DBTT) by estimating the impact energy at
different temperatures.
In the present work, a three dimensional model with appropriate and realistic assumptions
was developed to represent the actual practice of Charpy impact test using finite element analysis
(i.e. Abaqus 6.1, Explicit). The geometry was modeled according toASTM E-23 [11]. The main
objective of this work is to estimate numerically the impact energy required for the fracture of
normalized steel and Aluminum specimens and to compare the obtained results with the
corresponding experimental ones at common test conditions.Anothercontribution of this work is to
investigate the effects of varying the notch depth and shapeon the absorbed energy.

International Journal of Mechanical Engineering and Technology (IJMET), ISSN 0976
6340(Print), ISSN 0976 – 6359(Online) Volume 4, Issue 4, July
2. FINITE ELEMENT MODEL
The impact test apparatus is
supports. The material of all components
inherits the properties and condition of an actual Charpy rig (i.e.
2.1.Geometry
The dimensions of both steel and aluminum
E23 requirements as illustrated by Fig. 1.
cracks found in large structures, noting that concentrated stresses are developed on such sharp
corners. In order to investigate the influence of the shape of the notch on the fracture,
were selected; V-notch and U-notch as
Fig.1. Geometry of the testing specimen (mm)
As the main focus of this study
specimen, the striker is modeled as a rigid body.The mass of the striker was set to30.24 kg and the
density was selected just to match the mass of the pendulum in the actual test.According to ASTM
E23 standard, the round pointed face of the striker that strikes the specimen is
with a radius equivalent to the distance of the V
important dimensions of the striker.
Fig.2. Illustration
Mechanical Engineering and Technology (IJMET), ISSN 0976
6359(Online) Volume 4, Issue 4, July - August (2013) © IAEME
379
is modeled as three main parts; the specimen,the striker,
components was assumed to be isotropic and homogenous.
ndition of an actual Charpy rig (i.e.Instron SI-1K3).
both steel and aluminum specimens were assigned according to
E23 requirements as illustrated by Fig. 1. The presence of a notch may simulate the pre
found in large structures, noting that concentrated stresses are developed on such sharp
In order to investigate the influence of the shape of the notch on the fracture,
notch as described later in section 3.3.
Geometry of the testing specimen (mm)
of this study is towards the mechanical and material properties of the
as a rigid body.The mass of the striker was set to30.24 kg and the
selected just to match the mass of the pendulum in the actual test.According to ASTM
und pointed face of the striker that strikes the specimen is designed as a fillet
ivalent to the distance of the V-notch (i.e. 1.6567 mm). Fig. 2 shows the shape and
Illustration of the striker from sketch to extrusion
Mechanical Engineering and Technology (IJMET), ISSN 0976 –
August (2013) © IAEME
the striker, and the
assumed to be isotropic and homogenous.This model
assigned according to ASTM
The presence of a notch may simulate the pre-existing
found in large structures, noting that concentrated stresses are developed on such sharp
In order to investigate the influence of the shape of the notch on the fracture, two shapes
material properties of the
as a rigid body.The mass of the striker was set to30.24 kg and the
selected just to match the mass of the pendulum in the actual test.According to ASTM
designed as a fillet
shows the shape and

380
2.2.Material properties
In this work, AISI 4140-tempered steel and A6061-T6aluminumweresimulated for the purpose of
prediction ofthe absorbed energyresulted from impact test. Table 1 shows the physical properties of
both test specimens.
Table1.Physical properties of the tested specimens
Specimen Density
(kg/m3
)
Poisson’s
ratio
Young’s
modulus
(GPa)
Yeild
strength
(MPa)
Ultimate tensile
strength (MPa)
AISI 4140-T Steel 8030 0.3 207 655 1020
Aluminum A6061 2700 0.33 80 276 310
In the current FE analysis, the bilinear isotropic hardening material model(i.e. a piecewise
linear plasticity model)was used to describe the stress/strain relationship of the normalized steel.
Such a model is used widely in automotive industry to its ease implementation. Fig. 3 shows the
stress-strain curves for both steel and aluminum.
2.3.Computational model setup
After introducing the geometry, assigning the material via sections and assembling the
individual parts, it is necessary to define the parameters of the computational simulation.
Fig.3.Stress-strain curve for AISI 4140-T steel and aluminum A6061
Firstly, since the model deals with a time dependent problem (i.e. impact), Dynamic/Explicit
step was utilized. In order to consider the contact effects, two types of contact interactions were
defined; specimen- to- support contact and striker –to- specimen impact. These contact interactions

381
were assigned with a frictional interaction property. Regarding the boundary conditions, a coupling
constraint was assigned to the striker which restricted the striker’s movement only to towards the
specimen (i.e. y-direction). As the main objective is to simulate the actual practice of Charpy impact
test, the mass of the striker and the gravity field were considered. It should be recognized that the
velocity of the striker was set according to a realistic ‘high latch’ velocity of an actual Charpy rig.
3. RESULTS AND DISCUSSION
Numerical analysis was carried out based on the developed FE model described in section 2.
This analysis aimed to predict numerically the absorbed impact energy required for fracture of both
steel and aluminum specimens as well as the influence of notch shape and depth on the absorbed
energy. The fundamental step of any FE analysis is to check the mesh convergence and to assign the
most appropriate mesh size. Fig. 4 shows that the mesh is converged at an overall No. of elements
equals to 64683. However, a mesh of element numbers 214678 was selected as common for all
simulation runs to guaranteethe required accuracy especially around the notch.
Fig.4. Illustration of mesh convergence
3.1. Impact energy
The impact energy required for fracture for both AISI 4140-T steel and aluminium A6061-T6
were predicted by considering the area under the force-displacement curve. The displacement has
been estimated directly from the FE simulation. Fig. 5 show the Von Mises stresses and
corresponding displacements for steel specimen at the maximum permissible plastic strain of 10 %.
Fig. 6 shows the force-displacement diagram for the steel specimen. The area under the curve
represents the absorbed energy required for fracture which equals 46.64 J. In order to validate the FE
findings, the obtained impact energy was compared with the corresponding experimental Charpy
impact test. It was found that the impact energy of a V-notch AISI 4140-T steel is 50 J [14]. Hence,
the percentage of error that is observed in the suggested FE model is6.6 %only.

382
(a)
(b)
Fig.5. (a) Von Mises stresses for steel specimen (b) corresponding displacement distribution
Fig.6. Force-displacement curve for AISI 4140-T steel specimen
Similar analysis was carried out for aluminum A6061-T6 specimen. The main findings are
summarized in Table 2. The obtained results showed generally that the established FE model was
able to capture the impact energy accurately of steel and aluminum specimen with very slight
difference if compared to the actual Charpy impact test.

383
Table 2. Estimated impact energy and relevant parameters
Specimen
Max. Von
MisesStress
(MPa)
Max.
displacement
(mm)
Impact
Energy
calculated
using FE
simulation
Impact
energy
generated
from
experimental
setup
Error
Percentage
(%)
AISI 4140-T
Steel
982.3 1.502 46.64 50 -6.6
Aluminum
A6061
376.6 1.303 20.4 21.7 6
3.2.Influence of the notch depth on the absorbed energy
In order to check the influence of the notch depth, numerical run has been performedfor the
case in which the V-notch increased by 1.5 % compared to the standard dimension. Fig.7 shows the
notch geometry for both cases. Fig. 8 shows the absorbed energy versus the notch depth for AISI
4140. The obtained results demonstrated that as the depth of the notch increases, the absorbed energy
decreases accordingly. In other words, the specimen tends to fracture faster and easier in case of
higher notch depth. It should be mentioned that according to ASTM E 23 standard, changing the
notch depth by 1.5% can give an energy change of up to 8%. On the other hand, the obtained
numerical results showed a difference of about 10.1% which is still quite close to the ASTM
standards,
Fig.7. Notch geometry at different depths
Fig.8. Absorbed energy versus the V-Notch depth for a AISI 4140-T Steel specimen

384
3.3.Influence of the notch shape on the absorbed energy
The main objective of this part is to investigate the effect of the notch shape on the absorbed
energy required for fracture of AISI 4140-T steel. Hereafter, V-Notch and U-Notch were
considered. The dimensions for both notch shapes are shown schematically by Fig. 9.
Fig.9. Dimensions of V-Notch andU-Notch
Table 3 shows a comparison between the V-notch and U-notch in terms of absorbed energies,
relevant stresses and deformationswhich were generated from two different simulation runs. Based
on the obtained results, the absorbed energy required for the fracture of U-Notch specimen is higher
than that of a V-Notch by 15.5%. This is due to the fact that V-notch is considered as higher stress
concentrator compared to U-notch.
Table 3. Comparative study of the absorbed energy results of a V-Notch and U-Notch steel
specimens
V-Notch AISI 4140-T Steel Specimen U-Notch AISI 4140-T Steel Specimen
Stress in the Specimen
(MPa)
982.3 Stress in the Specimen
(MPa)
871.2
Displacement in the
Specimen (mm)
1.502 Displacement in the
Specimen (mm)
0.9
Impact Energy absorbed
at fracture
46.64 J Impact Energy Absorbed
at fracture
54 J
3.4.Comparative study between the conducted 3D analysis and 2D approximation
The main objective of this section is to check the applicability and accuracy of using 2-
dimensional approximation in comparison with the most comprehensive 3-dimensional model. For
this purpose, pure 2D plain strain Charpy impact model was designed. For simplicity, the striker was
replaced by an acting point impact force. The stress and displacement contours for AISI 4140
specimen are shown in Fig.10.

385
Fig.10. (a) Von Mises stresses forAISI 4140 under the impact influence using 2D model (b)
Corresponding displacement contours
For the sake of comparison, the simulation results obtained from 2D and 3D analyses are
summarized in Table 4. It was shown that 2D model was insufficient to predict accurate values of the
impact energy as the percentage of error reached 50.8 % compared to the corresponding values
generated from the actual test, whereas for 3D model it is only 6.7 %.This can be explained if we
considered that the one point impact force acts as very high stress concentrator in the case of 2D
model, while for 3D model, the impact force applied by the striker has certain impact surface areaand
less generated stresses accordingly.
3D Model
2D Model
Specimen Material: AISI 4140-T Steel
Specimen Material: AISI 4140-T Steel
Stress in the
Specimen (MPa)
982.3 Stress in the
Specimen (MPa)
982
Displacement in the
Specimen (mm)
1.502 Displacement in the
Specimen (mm)
0.792
Impact Absorbed Energy: 46.64 J
Impact Absorbed Energy: 24.6 J
Percentage Error: 6.6 %
Percentage Error: 50.8 %

386
4. CONCLUSIONS
In this work, a 3-dimensional FE model of Charpy impact test was developed. The model was
designed under the influence of the ASTM E 23standard and considered the effects of geometric,
material and contact nonlinearities. The proposed model was implemented to investigate the
absorbed energy required for fracture under the impact load ofAISI 4140 steeland aluminum
specimens. The obtained results showed that the developed model was able to predict the absorbed
energy accurately when appropriate mesh size was selected. In comparison with the absorbed energy
values resulted from the practical Charpy test, it was found that the obtained FE results have minimal
percentage of errors of 6.71 % and 6 % for steel and aluminum, respectively.Moreover, this study
included wide variety of parametric studies which aimed to investigate the influences of notch depth
and shape on the absorbed energy required for fracture. The obtained results showed that increasing
the notch depth by 1.5 % of the standard dimension, may lead to decrease the absorbed energy of 10
%. This was found matching the ASTM E 23 section concerned with the uncertainty due to specimen
dimension. The obtained 3D model in this study showed superiority over the 2D model
approximation in term of the accuracy of the estimated absorbed energy.
REFERENCES
[1] P. R.Marur, P. S.Nair, and K. R. Simha, Two degrees of freedom modeling of pre-cracked
Beams under Impact.Engineering Fracture Mechanics, 53 (3), 1996, 481-491.
[2] Yu-Chi Su and Chien-Ching Ma, Transient wave analysis of a cantilever Timoshenko beam
subjected to impact loading by Laplace transform and normal mode methods. International
Journal of solids and structures 49, 2012, 1158-1176
[3] T. Belytschkoand HD., Bartel,Efficient large scale non-linear transient analysis by finite
element ,International Journal of Numerical methods for Engineers10, 1976, 579-596.
[4] K. K. Mathur, A. Needleman and V. Tvergaard ,3D analysis of failure modes in the charpy
impact test, Modelling and Simulation of Materials Science and Engineering 2, 1994, 617-
635.
[5] V. Tvergard and A. Needleman, Analysis of the Charpy V-notch test for welds,Engineering
Fracture Mechanics65, 2000, 627-643.
[6] T.Lorrit, Specimen loading detemined by displacement measurement in instrumented Charpy
impact test, Engineering Fracture Mechanics65, 2000, 703-713.
[7] W.Altenhof, A. Raczy, M. Laframboise, J. Loscher and A. Alpas, Numerical Simulation of
AM50A magnesium alloy under large deformation, International Journal of Impact
Engineering30, 2004, 117-142.
[8] Y. J. Chao, J. Ward and R. Sands, Charpy impact fracture energy and ductile-brittle transition
temperature of dual-phase590 Steel. Material and Design 28, 2007, 551-557.
[9] C. Rubio-Gonza´lez, J.A. Gallardo-Gonza´lez, G. Mesmacque, U. Sanchez-Santana,
Dynamic fracture toughness of pre-fatigued materials, International Journal of Fatigue 30,
2008, 1056–1064.
[10] Fadi A. Ghaith, Nonlinear finite element modelling of Charpy impact test. Advanced
Materials Research 83-86, 2010, 182-189.
[11] ASTM E-23-99, Standard methods for notched bar impact testing of metallic materials,1999.
[12] West Yorkshire Steel Company, Material Property Catalogue.Web site Link:
http://www.westyorkssteel.com/AISI_4140.html .
[13] Prabhat Kumar Sinha and Rohit, “Analysis of Complex Composite Beam by using
Timoshenko Beam Theory & Finite Element Method”, International Journal of Design and
Manufacturing Technology (IJDMT), Volume 4, Issue 1, 2013, pp. 43 - 50, ISSN Print:
0976 – 6995, ISSN Online: 0976 – 7002.

Three dimensional nonlinear finite element modeling of charpy impact test

Recomendados

Recomendados

Más contenido relacionado

La actualidad más candente

La actualidad más candente (20)

Similar a Three dimensional nonlinear finite element modeling of charpy impact test

Similar a Three dimensional nonlinear finite element modeling of charpy impact test (20)

Más de IAEME Publication

Más de IAEME Publication (20)

Último

Último (20)

Three dimensional nonlinear finite element modeling of charpy impact test