Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

2005-01-3314

SAE TECHNICAL
PAPER SERIES

The Application of VCCT for ABAQUS® to

Prediction and Simulation of Delamination
Growth in Composite Structures
Mohan Rathinasabapathy
ABAQUS East, LLC

AeroTech Congress & Exhibition

Grapevine,Texas
October 3-6, 2005

400 Commonwealth Drive, Warrendale, PA 15096-0001 U.S.A. Tel: (724) 776-4841 Fax: (724) 776-5760 Web: www.sae.org
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

The Engineering Meetings Board has approved this paper for publication. It has successfully completed
SAE's peer review process under the supervision of the session organizer. This process requires a
minimum of three (3) reviews by qualified reviewers.

All rights reserved. No part of this publication may be reproduced, stored in a retrieval system, or
transmitted, in any form or by any means, electronic, mechanical, photocopying, recording, or otherwise,
without the prior written permission of SAE.

For permission and licensing requests contact:

SAE Permissions
400 Commonwealth Drive
Warrendale, PA 15096-0001-USA
Email: permissions@sae.org
Fax: 724-772-4891
Tel: 724-772-4028

For multiple print copies contact:

SAE Customer Service

Tel: 877-606-7323 (inside USA and Canada)
Tel: 724-776-4970 (outside USA)
Fax: 724-776-1615
Email: CustomerService@sae.org

ISSN 0148-7191
Copyright © 2005 SAE International
Positions and opinions advanced in this paper are those of the author(s) and not necessarily those of SAE.
The author is solely responsible for the content of the paper. A process is available by which discussions
will be printed with the paper if it is published in SAE Transactions.

Persons wishing to submit papers to be considered for presentation or publication by SAE should send the
manuscript or a 300 word abstract of a proposed manuscript to: Secretary, Engineering Meetings Board, SAE.

Printed in USA
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

2005-01-3314

The Application of VCCT for ABAQUS® to Prediction and

Simulation of Delamination Growth in Composite Structures
Mohan Rathinasabapathy
ABAQUS East, LLC

Copyright © 2005 SAE International

ABSTRACT laminated composites. In these cases, it was necessary

to program the VCCT capability within FEA codes with
This paper presents the application of VCCT for user defined subroutines. The use of user subroutines
ABAQUS software for prediction and simulation of also made post processing of the VCCT results a
delamination growth in composite structures. Pure cumbersome task.
Mode-I (2D and 3D) and mixed-mode cases are
analyzed as part of validation study and the strain VCCT for ABAQUS is an add-on module for the
energy release rates for each case are calculated. The ABAQUS commercial software that predicts interfacial
strain energy release rate versus the crack length is crack propagation due to delamination/debonding in
computed and compared with analytical solutions. A 3D brittle materials using the Virtual Crack Closure
Double Cantilever Beam (DCB) model is investigated to Technique. The technique allows for progressive crack
simulate the unidirectional Mode-I growth and a growth between bonded surfaces based on the fracture
laminated composite panel with an initial delamination of toughness of the bond and the strain energy release rate
arbitrary shape is analyzed to demonstrate the ability of at the crack tip. VCCT for ABAQUS uses the existing
simulating the mixed-mode multi-directional surface-based modeling capabilities and element
delamination growth. These results are compared with a formulations available within ABAQUS. The models can
previously published numerical solution. be created with ABAQUS/CAE and the results can be
post processed with ABAQUS/CAE or ABAQUS/Viewer.
INTRODUCTION VCCT for ABAQUS is found to be very easy to use since
it leverages the existing capabilities of ABAQUS.
Composites technology is playing increasingly important
role in the aerospace industry and composite structures This paper presents the application of the VCCT for
are often susceptible to delamination growth. The ABAQUS to calculate strain energy release rate values
Virtual Crack Closure Technique (VCCT) is generating at the crack tip and to simulate the progressive
interest from aerospace industry engineers and delamination growth in composite structures. As part of
researchers who wish to apply fracture mechanics validation study, three 2D Mode-I cases: (1) a Single
methodologies to composite materials. VCCT is based Edge Notched Tension (SENT) specimen, (2) a 2D DCB
on the assumption that the strain energy released when specimen and (3) a three-point bend specimen are
a crack is extended by a certain amount is the same as analyzed. To test the validity of 3D Mode-I results, a
the energy required to close the crack by the same semi-elliptical surface crack in a flat plate specimen is
amount. VCCT was proposed for 2D crack investigated. To verify the accuracy of solutions for the
configurations by Rybicki and Kanninen [1] and was 3D mixed-mode case, a laminate with a postbuckled
extended to three dimensions (3D-VCCT) by embedded delamination under compression is analyzed.
Shivakumar, Tan and Newman [2]. Krueger [3] recently The strain energy release rate versus the crack length is
presented a summary of historical development and a computed and compared with the analytical solutions
discussion with respect to different applications. and/or available previous numerical solutions. Also, a
3D DCB model is investigated for the simulation of
Recently, researchers have combined VCCT with finite unidirectional Mode-I delamination growth and a
element methods to calculate the strain energy release laminated composite panel with an initial delamination of
rates numerically. Combining 2D-VCCT and finite irregular shape is analyzed for mixed-mode multi-
element analysis, Sun and Qian [4] evaluated the strain directional delamination growth. These results are
energy release rates for interfacial cracks between two compared with a previously published numerical
isotropic materials. Xie [5] developed an 18-node solution.
“interface element” using the UEL option in ABAQUS to
calculate strain energy release rates numerically based
on 3D-VCCT and to simulate the delamination growth in
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

Comparison of Results - SENT

VALIDATION STUDY 6.00E-03

5.00E-03 GI-Analytical
The first part of this paper discusses the validity of GI-VFA
results produced by VCCT for ABAQUS. Though the 4.00E-03
intended use of VCCT for ABAQUS is to simulate crack

GI
3.00E-03
growth, crack growth is prevented in all the validation
test cases by specifying large fracture toughness values. 2.00E-03
This allows the maximum strain energy release rate
1.00E-03
values to be calculated at the crack tip for the prescribed
crack length and loading using VCCT for ABAQUS. 0.00E+00
These strain energy release rate values are compared 0 0.0005 0.001 0.0015 0.002 0.0025
with the analytical solutions and/or available numerical Crack length, a
solutions.
Figure 2. Comparison of results – SENT specimen
2D MODE-I TEST CASES

Single Edge Notched Tension Specimen

Figure 2 shows that the VCCT for ABAQUS GI results
Figure 1 shows the schematic representation of the match with the analytical results well though, it slightly
single edge notched tension specimen. The length of under predicted for a crack length of 0.002 units.
the specimen is modeled as 0.04 units, width ‘W’ is
0.005 units and the applied concentrated force ‘P’ is Double cantilever Beam specimen
0.0625 units.
Figure 3 presents the schematic diagram of the double
cantilever beam specimen. The length of the specimen
‘L’ is 9 mm, ‘h’ is 1 mm and the applied concentrated
force ‘P’ is 1 N. The out of plane thickness ‘B’ is 1 mm.

Figure 1. Single Edge Notched Tension Specimen

ABAQUS/CAE V6.5-3 is used to create the finite

element model. Even though the problem is symmetric,
the entire specimen is modeled so the surface based Figure 3. Double Cantilever Beam Specimen
contact features in VCCT for ABAQUS can be utilized.
4-node plane strain elements (CPE4) are used to
discretize the model with an out-of-plane thickness of
0.005 units. A linear elastic isotropic material model is ABAQUS/CAE V6.5-3 is used to create the entire model
defined with Young’s modulus ‘E’ as 2.91E7 units and and it has been meshed with 4-node plane strain
Poisson’s ratio ‘Q’ as 0.3. Four models are created by incompatible mode elements (CPE4I). Again, symmetry
varying the crack length ‘a’ ranging from 0.0005 units to conditions are not used so a contact pair can be defined.
0.002 units. To prevent the crack growth and measure Five models are created by varying the crack length ‘a’
the maximum strain energy release rates at the crack between 2 mm and 5 mm. A linear elastic isotropic
tip, large critical strain energy release rate values – material model is defined with Young’s modulus ‘E’ as
100.0, 100.0 and 100.0 for GIC, GIIC and GIIIC respectively 2.0E5 N/mm2 and Poisson’s ratio as 0.3. To prevent the
– are specified. Mode-I strain energy release rate crack propagation and measure the maximum strain
values, GI, are plotted versus crack length ‘a’ and energy release rates at the crack tip, large fracture
compared with the analytical solution given in reference toughness values – 100.0, 100.0 and 100.0 for GIC, GIIC
[6]. Figure 2 shows the results from VCCT for ABAQUS and GIIIC respectively – are specified. Mode-I strain
and the comparison with the analytical solution. energy release rate values, GI, are plotted versus crack
‘a’ and compared with the analytical solution given by
Kanninen [7]. Figure 4 presents the comparison
between the results obtained using VCCT for ABAQUS
and Kanninen’s analytical solution.
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

The Mode-I strain energy release rate results from

Comparison of Results - DCB
VCCT for ABAQUS are compared with the theoretical
results from Tada et. al. [8].
2.50E-03
GI-Kanninen
GI (N-mm/mm^2)

2.00E-03 The theoretical result from Tada et. al. [8] for a/b < 0.6
GI-VFA gives:
1.50E-03
6M
1.00E-03 V (1)
b2
5.00E-04

0.00E+00 KI V Sa F (a / b) (2)
0 1 2 3 4 5 6
Crack Length, a (mm) F (a / b) 1.122  1.40(a / b)  7.33(a / b) 2
(3)
Figure 4. Comparison of Results – DCB specimen  13.08(a / b) 3  14.0(a / b) 4

The comparison of results is presented in Figure 6.

The VCCT for ABAQUS results show reasonably good

agreement with the analytical solution as presented in Comparison of Results - 3-Point Bending
Figure 4.
7.00E-01
GI-Tada et. al.
Three-point bend specimen 6.00E-01
GI-VFA
GI (N-mm/mm^2)
5.00E-01
As a third test for the 2D Mode-I case, an edge crack in
4.00E-01
a three-point bend specimen in plane strain, as shown in
Figure 5, is considered. The length of the specimen is 3.00E-01
55 mm, the span ‘s’ is 43 mm and the width ‘b’ is 10 mm. 2.00E-01
The loading is in the form of a bending moment ‘M’,
1075 N-mm, applied to the ends of the specimen. 1.00E-01
0.00E+00
0 1 2 3 4 5 6
Crack length, a (mm)
Figure 6. Comparison of Results – Three-point Bend
Specimen

Figure 6 shows that VCCT for ABAQUS results match

very well with the theoretical results for this case.
Figure 5. Three-Point Bend Specimen
3D MODE-I TEST

Semi-Elliptical Surface Crack in a Flat Plate

The finite element model is created using ABAQUS/CAE
V6.5-3. The specimen is meshed with 4-node plane A Semi-Elliptical Crack (SEC) in a flat plate specimen is
strain incompatible mode elements (CPE4I). The full analyzed for the 3D Mode-I case. The schematic
model without the symmetry boundary conditions is diagram of the half specimen is shown in Figure 7.
again considered to take advantage of the surface
based VCCT for ABAQUS. The crack length is varied
between 2 mm and 5 mm to create five different models.
A linear elastic isotropic material model is assumed with
Young’s modulus ‘E’ as 2.0E5 MPa and Poisson’s ratio
as 0.3. The bending moments are applied to the ends of
the specimen using kinematic coupling constraints.
Large fracture toughness values – 100.0, 100.0 and
100.0 for GIC, GIIC and GIIIC respectively – are specified
to avoid the crack propagation and measure the
maximum strain energy release rates at the crack tip.
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

Figure 8. Mesh for Semi-Elliptical Crack Flat Plate

Figure 9 shows the mesh profile at the bottom crack

surface, which is the slave surface in the contact pair.
VCCT for ABAQUS results are available only at the
slave surface nodes and hard points (i.e. points where
nodes will be located) are placed at the crack tip so that
strain energy release rate outputs can be requested at
these points.

Figure 7. Semi-Elliptical Surface Crack in a Flat Plate

The specimen has thickness ‘t’ of 0.5 units, width ‘2W’ of

2 units and height ‘h’ of 1 unit. Due to symmetry, only
half the specimen along the width is modeled. The other
symmetry along ‘h’ is not modeled so that the top and
bottom surfaces of the crack can be defined in the
contact pair, as required for VCCT for ABAQUS. A
linear elastic isotropic material is assumed with the Figure 9. Mesh Profile on the Bottom Crack Surface
Young’s modulus ‘E’ as 1.0E7 units and the Poisson’s
ratio as 0.3. A pressure load ‘Vm’ of 100 units is applied
on the top face of the plate as shown in Figure 7.
ABAQUS/CAE V6.5-3 is used to create the finite Similar to the 2D Mode-I test cases, large critical strain
element model and the plate is meshed with 8-node energy release rates – 100.0, 100.0 and 100.0 for GIC,
brick (C3D8) elements. The mesh for the flat plate is GIIC and GIIIC respectively – are specified to prevent the
shown in Figure 8. As shown in Figure 8, the top and crack from propagating and measure the maximum
bottom crack surfaces have mismatched meshes. strain energy release rates at the crack tip. The results
VCCT for ABAQUS doesn’t require matching meshes at obtained using VCCT for ABAQUS are compared with
the crack surfaces. the analytical solution given in reference [9].
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

Due to symmetry, only a quarter of the specimen as

Comparison of Results - 3D SEC
shown in Figure 11 is modeled and symmetry boundary
conditions are defined accordingly. The width ‘W’ of the
0.0003
quarter specimen is 50 mm and the radius of the circular
0.00025 embedded delamination ‘a’ is 15 mm. The sublaminate
0.0002 thickness ‘h’ and the laminate thickness ‘H’ are 0.4 mm
and 4 mm respectively. An in-plane compressive axial
GI

0.00015 strain ‘Hx’, 0.005, is applied. A small imperfection is

0.0001 GI-T. L. Anderson introduced in the geometry at the crack area to induce
GI-VFA buckling during numerical simulation. A “homogeneous
0.00005
quasi-isotropic” material with a [r45/0/90]s stacking
0 sequence is selected for this study with the following
0 20 40 60 80 100 typical graphite/epoxy mechanical properties:
Crack location, phi (deg)
E11 = 134 GPa; E22 = E33 = 10.2 GPa; Q12 = Q13 = 0.3;
Figure 10. Comparison of Results – Semi-Elliptical
Q23 = 0.49; G12 = G13 = 5.52 GPa; and G23 = 3.43 GPa.
Surface Crack in a Flat Plate
The specimen is meshed with 8-node incompatible
mode brick (C3D8I) elements. The geometry and mesh
are created using ABAQUS/CAE V6.5-3. The mesh for
In Figure 10, Mode-I strain energy release rates from this specimen is shown in Figure 12.
VCCT for ABAQUS are plotted at various points along
the crack tip and compared with the theoretical solution
from reference [9]. As shown in Figure 10, VCCT for
ABAQUS slightly over-predicted the GI values for this
case.

3D MIXED-MODE TEST

Embedded Delamination under Compression

To test the validity of mixed-mode results, a laminate

with postbuckled embedded circular delamination under
in-plane compression is analyzed. The schematic
representation of the quarter specimen is shown in
Figure 11.

Figure 12. Mesh for Embedded Circular Delamination

Laminate

A large critical strain energy release rate values – 100.0,

100.0 and 100.0 for GIC, GIIC and GIIIC respectively – are
specified to avoid delamination growth and measure the
maximum strain energy release rates at the crack tip.
The maximum strain energy release rates from VCCT
for ABAQUS are compared with the finite element
analysis results by Whitcomb [10]. In Figure 13, the
Mode-I strain energy release rates along the
delamination front ‘S’ are plotted and compared. Figure
14 shows the results and comparison of Mode-II strain
energy release rates plotted along the delamination front
‘S’ for this case.
Figure 11. Postbuckled Embedded Circular
Delamination under In-Plane Compression
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

mm. Displacement controlled analysis is performed and

Comparison of Results - Embedded Delamination
ABAQUS/CAE V6.5-3 is the pre-processor.
300
GI-Whitcomb
GI-VFA
250

200
GI (J/m**2)

150

100

50

0
0 0.005 0.01 0.015 0.02 0.025
S (m)

Figure 13. Mode-I Results and Comparison Plotted

Figure 15. Mode-I Delamination Growth – DCB Model
along the Delamination Front ‘S’

The following orthotropic Carbon/Epoxy laminate

Comparison of Results - Embedded Delamination properties are defined for the specimen:
300
GII-Whitcomb E11 = 21.07 GPa; E22 = 20.76 GPa; E33 = 8.27 GPa;
250
GII-VFA Q12 = 0.0357; Q13 = Q23 = 0.0426; G12 = 2.5 GPa;
G13 = G23 = 2.0 GPa.
200
GII (J/m**2)

The specimen is meshed with linear incompatible mode

150 hexahedral (C3D8I) elements. The finite element mesh
is shown in Figure 16. It has 218 elements along x-
100 direction, 1 each for the sublaminate in the y-direction
and 8 elements along z-direction.
50

0
0 0.005 0.01 0.015 0.02 0.025
S (m)

Figure 14. Mode-II Results and Comparison Plotted

along the Delamination Front ‘S’

In this case, for Mode-I, VCCT for ABAQUS slightly

under-predicted and for Mode-II, significant differences
in results can be seen at S=0. For Mode-II, significant
differences occur at various positions of S as well.
These differences can be attributed to the “approximate”
contact procedure implemented by Whitcomb [10].

DELAMINATION GROWTH SIMULATION Figure 16. Finite Element Mesh – DCB Model

MODE-I UNIDIRECTIONAL GROWTH

To simulate the baseline Mode-I unidirectional VCCT for ABAQUS is surface based which requires a
delamination growth, Guenon’s [11, 12] Double master surface, a slave surface and a set of nodes
Cantilever Beam specimen is modeled with VCCT for named “BNodes” that are initially bonded. VCCT for
ABAQUS. The schematic representation of the ABAQUS identifies the crack tip based on the “BNodes”
specimen and the boundary conditions are presented in set and the crack propagation is simulated using the
Figure 15. As shown in Figure 15, the length of the *Debond keyword in ABAQUS. VCCT for ABAQUS is
specimen ‘L’ is 152.4 mm, width ‘B’ is 19 mm, thickness invoked using “Ucrack” parameter in the *Surface
‘2h’ is 4.44 mm and the initial delamination ‘a0’ is 25.2 Interaction keyword. The properties required by VCCT
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

for ABAQUS such as critical strain energy release rates, As shown in Figure 17, some differences in reaction
fracture criterion to simulate crack growth etc. are force values between VCCT for ABAQUS and
defined as datalines for *Surface Interaction keyword. Rathinasabapathy et. al. [14, 15] are observed in the
More information on setting up VCCT for ABAQUS crack opening displacement range from approximately 3
models can be found in reference [13]. In this case, the mm to 10 mm. For all other crack opening displacement
bottom surface of the top sublaminate is defined as values, excellent agreement in the reaction force results
master surface, the top surface of the bottom is observed between both the cases.
sublaminate is defined as slave surface and the initially
bonded nodes shown in Figure 15 that belong to the To verify the accuracy between the two numerical
slave surface are defined as “BNodes.” The following solutions, the VCCT for ABAQUS results are compared
critical strain energy release rate values are specified: with the experimental solutions provided by Guenon
0.307 N-mm/mm2, 0.632 N-mm/mm2 and 0.817 N- [12]. As shown in Figure 18, the VCCT for ABAQUS
mm/mm2 for GIC, GIIC and GIIIC respectively. A power law results matched very well with the experimental results.
fracture criterion with coefficients am = an = ao = 1 is
defined. The mixed-mode power law is given below: VFA versus Experimental Results

am an ao 70
Gequiv § GI · §G · §G ·
¨¨ ¸¸  ¨¨ II ¸¸  ¨¨ III ¸¸ (4) 60
Experiment-Guenon et. al.
GequivC © G IC ¹ © G IIC ¹ © G IIIC ¹ VFA
50

Reaction Force (N)

Some convergence difficulties are experienced with 40
VCCT for ABAQUS when the crack is about to grow. To
overcome these convergence difficulties, contact 30
stabilization is turned on. When using contact
stabilization, the users need to be careful to make sure 20

that the stabilization value is not too high and the results 10
make physical sense. To confirm this, the static
dissipation is plotted against the strain energy and the 0
static dissipation is found to be minimal compared to the 0 5 10 15 20
strain energy. Crack Opening Displacement, delta (mm)

Figure 18. Comparison of Results – VCCT for ABAQUS

Rathinasabapathy and Biggers [14] previously simulated versus Experiment
the delamination growth for this specimen using Xie’s [5]
interface element as an unstitched case. More
information on this DCB growth simulation can be found
in reference [15]. The results from VCCT for ABAQUS Also, excellent agreement is observed between the final
are compared with the unstitched DCB case of crack lengths from both numerical solutions. At the end
Rathinasabapathy et. al. [14,15]. Comparison of the of the analysis, i.e. when crack opening displacement ‘G’
load-displacement curves for this specimen is shown in is 20 mm, VCCT for ABAQUS predicted the final crack
Figure 17. length to be 85.3 mm whereas Rathinasabapathy et. al.
[14, 15] predicted it to be 85.4 mm.
Comparison of Load-Displacement Curves
70 MIXED-MODE MULTI-DIRECTIONAL GROWTH

60 Rathinasabapathy et. al.

De Moura’s [16] [04/904]s Carbon/Epoxy laminate
VFA specimen that contains an initial delamination of
50
Reaction Force (N)

arbitrary shape created by low-velocity impact is

40 modeled with VCCT for ABAQUS to simulate the mixed-
mode multi-directional growth. Assuming symmetry
30 about x-axis and z-axis, one quarter of the geometry is
modeled. The schematic representation of the quarter
20
specimen is presented in Figure 19.
10

0
0 5 10 15 20
Crack Opening Displacement, delta (mm)

Figure 17. Load-Displacement Plot Comparison – DCB

Model
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

The geometry is partitioned in ABAQUS/CAE to get the

initial delamination shape and the master surface, slave
surface and the “BNodes” are defined accordingly. The
initial delamination shape in the finite element model is
shown in Figure 21.

Figure 19. Initial Irregular Shape Delamination Quarter

Specimen

The length and width of the quarter specimen is 30 mm

and the laminate thickness is 2 mm. The initial
delamination of arbitrary shape exists at the interface of
Figure 21. Initial Delamination Shape in the Finite
the top 0° and 90° plies. ABAQUS/CAE V6.5-3 is the
Element Model
pre-processor and displacement controlled analysis is
performed. A compressive end displacement of 0.15 mm
along x-axis as shown in Figure 19 is applied. The
following orthotropic Carbon/Epoxy laminate properties
are defined for each sublaminate in the finite element The following critical strain energy release rate values
model with respect to a local material coordinate system are specified: 0.306 N-mm/mm2, 0.632 N-mm/mm2 and
to represent the [04/904]s laminate: 0.817 N-mm/mm2 for GIC, GIIC and GIIIC respectively.
These critical strain energy release rate values are
obtained from reference [16]. Mixed-mode power law
E11 = 109.34 GPa; E22 = E33 = 8.82 GPa; Q23 = 0.52;
with coefficients am = an = ao = 1 is defined as the
Q12 = Q13 = 0.342; G12 = G13 = 4.32 GPa; G23 = 3.2 GPa.
fracture criterion.
As shown in Figure 19, there are four sublaminates in
Similar to Mode-I unidirectional growth, some
the model. The top and bottom layers represent the 04
convergence difficulties are experienced when the initial
sublaminates and the second and third layers represent
delamination is about to grow. To overcome these
904 sublaminates. A small imperfection in the geometry
convergence difficulties, contact stabilization is turned
is introduced at the crack region to induce buckling
on with the value of 1.0E-5. It has been confirmed that
under compression. The specimen is meshed with
the static stabilization is minimal when compared with
linear incompatible mode hexahedral (C3D8I) elements.
the strain energy of this model.
The finite element mesh is shown in Figure 20. The
model has 20 elements each in x- and z-axis directions.
Rathinasabapathy and Biggers [14] previously simulated
the delamination growth for this specimen using Xie’s [5]
interface element as an unstitched case. More
information on this mixed-mode growth simulation can
be found in reference [15]. The results from VCCT for
ABAQUS are compared with the unstitched mixed-mode
case of Rathinasabapathy et. al. [14,15]. The load-
displacement curve comparison for this specimen is
shown in Figure 22.

Figure 20. Finite Element Mesh – Initial Irregular Shape

Delamination Model
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

Comparison of Load-Displacement Curves simulation of delamination growth. A validation study is

performed for 2D and 3D Mode-I and mixed-mode
8000
cases. A large fracture toughness values are specified
Rathinasabapathy et. al.
7000 for these cases to prevent the crack propagation and
6000
VFA measure the maximum strain energy release rates
calculated by VCCT for ABAQUS at the crack tip. These
Reaction Force (N)

5000 maximum strain energy release rate values are

4000 compared against the analytical solutions and/or
previous numerical solutions. Excellent agreement in
3000
results is observed in most of the cases. Also, because
2000 VCCT for ABAQUS uses a surface based algorithm,
1000
mismatched meshes between the top and bottom crack
surfaces are permissible.
0
0 0.02 0.04 0.06 0.08 0.1 0.12 0.14
Compressive End Displacement, u (mm) As part of delamination growth simulation, a Double
Cantilever Beam specimen and a laminate with initial
Figure 22. Load-Displacement Plot Comparison – delamination of arbitrary shape are analyzed. The
Mixed-Mode Delamination Growth results from VCCT for ABAQUS matched very well when
compared with the previously published numerical
solutions and available experimental data.
ABAQUS/CAE is used to set up all the models for VCCT
Again, in this mixed-mode delamination growth model, for ABAQUS. Based on the validation case studies and
some differences in the reaction force results is delamination growth simulations, it is concluded that the
observed when the applied compressive end VCCT for ABAQUS produces accurate results and is
displacement is between approximately 0.06 mm and easy to use because there is no need of additional
0.1 mm. In this case, VCCT for ABAQUS slightly under- programming of user subroutines or manual
predicted the reaction force compared to the results from calculations. Similarly, it is found that post processing of
references [14, 15]. For all other compressive end VCCT results is easy with VCCT for ABAQUS.
displacement values, excellent agreement in results is Furthermore, it is observed that VCCT for ABAQUS
observed. results are relatively mesh insensitive.

Mesh Sensitivity REFERENCES

8000
VFA-20x20 mesh 1. Rybicki, E. F., and Kanninen, M. F., “A Finite
7000 VFA-40x40 mesh Element Calculation of Stress Intensity Factors by a
6000 Modified Crack Closure Integral,” Engineering
Reaction Force (N)

5000 Fracture Mechanics, Vol. 9, pp. 931-938, 1977.

2. Shivakumar, K. N., Tan, P. W., and Newman, Jr., J.
4000
C., “A Virtual Crack-Closure Technique for
3000
Calculating Stress Intensity Factors for Cracked
2000 Three Dimensional Bodies,” International Journal of
1000 Fracture, Vol. 36, R43-R50, 1988.
3. Krueger, R., “The Virtual Crack Closure Technique:
0
0 0.02 0.04 0.06 0.08 0.1 0.12 0.14
History, Approach and Applications,” NASA/CR-
Compressive End Displacement, u (mm)
2002-211628.
4. Sun, C. T., and Qian, W., “The Use of Finite
Figure 23. Mixed-Mode Growth Load-Displacement Extension Strain Energy Release Rates in Fracture
Curve Comparison between Coarse and Fine Mesh
of Interfacial Cracks,” International Journal of Solids
Structures, Vol. 34, pp. 2595-2609, 1997.
5. Xie, D., “Damage Progression in Tailored Laminated
Panels with a Cutout and Delamination Growth in
To study the effect of mesh sensitivity in VCCT for
Sandwich Panels with Tailored Face Sheets,” Ph.D.
ABAQUS, the mixed-mode delamination growth model is
rerun after doubling the number of elements along x- Dissertation, Clemson University, 2002.
and z-axis. Figure 23 shows that the VCCT for 6. Hertzberg, R. W., “Deformation and Fracture
ABAQUS results are not mesh sensitive. Mechanics of Engineering Materials,” Fourth Edition,
1995.
CONCLUSION 7. Kanninen, M. F., “An Augmented Double Cantilever
Beam Model for Studying Crack Propagation and
The VCCT for ABAQUS V1.1 software is applied to Arrest,” International Journal of Fracture, Vol. 9, pp.
various fracture mechanics cases for prediction and 83-92, 1973.
 Downloaded from SAE International by University of Liverpool, Sunday, September 09, 2018

8. Tada, H., Paris, P. C., and Irwin, G. R., “The Stress as a Means for Delamination Growth Control,”
Analysis of Cracks Handbook,” Second Edition, Proceedings of ABAQUS User’s Conference, pp.
1985. 563-588, 2004.
9. Anderson, T. L., “Fracture Mechanics Fundamentals 15. Rathinasabapathy, M., “Finite Element Simulation of
and Applications,” Second Edition, 1994. Through-Thickness Stitching as a Means for
10. Whitcomb, J. D., “Analysis of a Laminate with a Delamination Growth Control,” Master’s Thesis,
Postbuckled Embedded Delamination, Including Clemson University, 2003.
Contact Effects,” Journal of Composite Materials, 16. de Moura, M. F. S. F., Goncalves, J. P. M., Marques,
Vol. 26, pp. 1523-1535, 1992. A. T., and de Castro, P. M. S. T., “Prediction of
11. Guenon, V. A., Chou, T. W., and Gillespie, Jr., J. W., Compressive Strength of Carbon-Epoxy Laminates
“Toughness Properties of a Three-Dimensional Containing Delamination by Using a Mixed-Mode
Carbon-Epoxy Composite,” Journal of Material Damage Model,” Composite Structures, Vol. 50, pp.
Science, Vol. 24, pp. 4168-4175, 1989. 151-157, 2000.
12. Guenon, V. A., “Toughness Properties of a Three-
Dimensional Carbon-Epoxy Composite,” Master’s CONTACT
Thesis, University of Delaware, 1987.
13. “VCCT for ABAQUS User’s Manual,” Version 1.1, Mohan Rathinasabapathy, ABAQUS East, LLC,
ABAQUS, Inc., 2005. mohan@abaquseast.com
14. Rathinasabapathy, M., and Biggers, S. B., “Finite
Element Simulation of Through-Thickness Stitching