
15: 2 (2015) 8894 

Marian Klasztorny^{1}*, Daniel Nycz^{2}, Marek Cedrowski^{3}
^{1 }Military University of
Technology, Faculty of Mechanical Engineering, Department of Mechanics &
Applied Computer Science, ul. Kaliskiego 2, 00908 Warsaw, Poland
^{2 }DES ART Co. Ltd.,
Headquarters  Gdynia, Branch Office  Sanok, ul. Lipinskiego 113, 38500 Sanok,
Poland
^{3 }B.Sc. student,
Military University of Technology, Faculty of Mechanical Engineering, ul. Kaliskiego
2, 00908 Warsaw, Poland
*Corresponding author. Email:
m.klasztorny@gmail.com
Received (Otrzymano) 17.02.2015
MODELLING,
SIMULATION AND VALIDATION OF BENDING TEST OF BOX SEGMENT FORMED AS TWO
COMPOSITE SHELLS GLUED TOGETHER
The present experimental and numerical research is focused on a box
composite beam, socalled a validation segment, consisting of two
vinylester/glass shells glued together. The top shell has a hat crosssection,
whereas the bottom one is flat. The shells are glued together at two horizontal
contact strips. The validation segment reflects the central part of the cross
and longitudinalsection of a box composite superstructure of a footbridge
designed by the authors. The dimensions of the cross‑section and the
number of fabric layers in the validation segment are decreased twice in
comparison with the footbridge superstructure. Moreover, the composite beam was
rotated by 180° in
relation to the footbridge. The validation segment is 2.35 m long, and the
crosssection overall dimensions are 0.60 m × 0.26 m
(width×height). The laminate components, glue and manufacturing technology of
the validation segment are the same as for the composite footbridge. The study
develops
a methodology for numerical modelling and simulation by the Finite Element
Method of box composite girders formed as two composite shells glued together.
The methodology is developed in reference to the validation segment which is
subjected to the 3point bending test with shear. Experimental validation of
the modelling and simulation was carried out for the basic case of new
laminates at 20°C. FE computer code MSC.Marc 2010 was used for the numerical
modelling and simulation.
Keywords: thinwalled box beam, GFRP laminate, glue layer, threepoint bending test, modelling and
simulation, experimental validation
MODELOWANIE, SYMULACJA I WALIDACJA PRÓBY ZGINANIA SEGMENTU
SKRZYNKOWEGO
W FORMIE DWÓCH POWŁOK KOMPOZYTOWYCH SKLEJONYCH ZE SOBĄ
Przedmiotem badań
eksperymentalnych i numerycznych jest belka kompozytowa o przekroju
skrzynkowym, zwana segmentem walidacyjnym, składająca się z dwóch sklejonych ze
sobą powłok kompozytowych winyloestrowoszklanych. Powłoka górna ma przekrój
kapeluszowy, a powłoka dolna jest płaska. Powłoki są sklejone ze sobą na dwóch
poziomych pasach kontaktu. Segment walidacyjny odwzorowuje środkową część
przekroju poprzecznego i podłużnego konstrukcji nośnej kompozytowej skrzynkowej
kładki dla pieszych zaprojektowanej przez autorów. Wymiary przekroju
poprzecznego oraz liczba warstw tkanin w laminatach segmentu walidacyjnego są
dwukrotnie mniejsze w porównaniu z konstrukcją nośną kładki. Ponadto, segment
belkowy obrócono o 180° w porównaniu z kładką. Długość segmentu wynosi 2,35 m,
a wymiary gabarytowe przekroju poprzecznego są równe 0,60 m × 0,26 m
(szerokość × wysokość). Komponenty laminatów, klej oraz technologia wytwarzania
segmentu walidacyjnego są takie same jak w przypadku kładki kompozytowej.
Opracowano metodykę modelowania numerycznego i symulacji z wykorzystaniem
metody elementów skończonych belek kompozytowych w formie dwóch sklejonych ze
sobą powłok kompozytowych. Metodyka została opracowana w odniesieniu do
segmentu walidacyjnego poddanego trójpunktowemu zginaniu ze ścinaniem.
Walidację eksperymentalną modelowania i symulacji przeprowadzono w podstawowym
przypadku laminatów nowych w temperaturze 20°C. Do numerycznego modelowania i symulacji
zastosowano kod elementów skończonych MSC.Marc 2010.
Słowa kluczowe: cienkościenna
belka skrzynkowa, laminat GFRP, warstwa kleju, próba trójpunktowego zginania,
modelowanie i symulacja, walidacja eksperymentalna
A new structural design of a composite footcycling bridge was proposed in [1]. The bridge span is simply supported, with a theoretical span of 12.00 m and a usable width of 2.50 m. The crosssection of the footbridge is a 5box openclosed girder, formed by two vinylester/glass shells. The components of the GFRP laminates are as follows: Firestop BÜFAS440 flame retardant vinylester resin (producer: BÜFA Gelcoat Plus, Germany); BAT800 [0/90], GBX800 [45/–45] quasibalanced stitched Eglass fabrics (producer: DIPEX, Slovakia). The laminates are manufactured using infusion technology. Glue joints between the top and the bottom shells as well as between the cross members and the shells are made using highstrength and vibrationresistant NORPOL FI184 glue (producer: Reichhold, Norway). The thickness of the adhesive layer is 2 mm. A geometrical model of the considered footbridge in the top isometric view is depicted in Figure 1 (support zone zoomed).
Composite
footbridges are constantly being
researched and developed in terms of forming, numerical modelling, simulation and
design. The Eurocodes for standard footbridges do not include this type of
structural materials. Adequate numerical modelling and simulation of static
processes play an essential role in the design of footbridges.
The study
develops a methodology for numerical modelling and simulation by the Finite
Element Method of box composite girders formed as two composite shells glued
together. The methodology is developed in reference to the central 1box
segment extracted from the whole footbridge superstructure presented in
Figure 1. The test segment has the overall dimensions and number of layers
decreased twice compared to the original segment (half scale model). The test
segment is subjected to a 3point bending test with shear. Experimental
validation of the modelling and simulation is conducted for the basic case of
new laminates at the temperature of 20°C.
The basic
approach to modelling polymermatrix laminates involves homogenization of the
layers, i.e. the replacement of heterogeneous material at the micro
level (twocomponent material) with homogeneous material at the macro level. The laminas
are modelled approximately as linear
orthotropic elasticbrittle materials [2]. The considered laminas are
each reinforced with an Eglass balanced stitched fabric. The
equivalent homogeneous orthotropic material has orthotropy directions 1, 2, 3 coinciding to the warp, weft and
thickness directions, respectively. Each lamina is
described by 9 effective elasticity constants:
E_{i}  Young’s modulus in i  direction,
v_{ij}  Poisson’s ratio in ij  plane, ij = 12, 23, 31
G_{ij}  shear modulus in ij  plane, ij = 12, 23, 31
and 9 effective
strength constants:
R_{it}, R_{ic}  tensile and compressive strengths in i  direction, i = 1, 2, 3
S_{ij}  shear
strength in ij  plane,
The simplest and a very accurate method constitutes experimental
identification of the elasticstrength
properties of a respective uniform laminate reflecting
laminas.
To
assess the strength of the laminate layer in
a complex stress state, various strength
theories are applied, including: the maximum stresses (Max Stress),
maximum strains, TsaiWu, Hashin,
Hashin Fabric, HillTsai, Hoffman, ChangChang, Hill, Malmeister
and others [24]. Based on the identification and validation numerical
and experimental studies [5] and on the MSC.Marc system recommendations [4], the following hypotheses in the MSC.Marc system have been
selected: the Hashin Fabric hypothesis
for layers reinforced with balanced
stitched fabrics and the Max Stress hypothesis for a glue layer.
Fig. 1. Composite
footbicycle bridge  top isometric view [1]
Rys. 1. Kompozytowa kładka
pieszorowerowa  widok izometryczny
z góry [1]
In the case of the Hashin Fabric hypothesis, the following failure indices in each integration point are calculated [4]:

fibre tension in direction 1,

fibre compression in direction
1,

fibre tension in direction 2,

fibre compression in direction
2,

matrix tension,

matrix compression,
where
The effort indices are the true measure of material effort  they are a measure of distance from the yield surface.
In the case of the Max Stress hypothesis, the following failure indices are calculated [10]:
In this case,
the effort indices are equal to the failure indices, i.e.
addition, the following notation is introduced:
The numerical
modelling of mixed laminate shells was developed by the authors in [5, 6].
Study [5] considers the numerical modelling and simulation of static processes,
including progressive failure, for GFRP (glass fibre reinforced plastic)
laminates of a mixed sequence of laminas reinforced with Eglass plain weave
fabric and Eglass mat. The examined laminate was manufactured with contact
technology using polyester resin as the matrix. The purpose of the research was
to determine the options/values, recommended in engineering calculations, of
the parameters for numerical modelling and simulation of static processes
including failure for beam, plate and shell structures built of composites
undertaken, using FE code MSC.Marc [4].
The 3point
bending test was performed in [6] for a singlewave glasspolyester laminate
segment. The geometry and ply sequence of the segment are modelled on the
selected composite tank cover. The main purpose of the research was to develop
numerical modelling and simulation methodology for such a test using FE code
MSC.Marc as well as to perform experimental validation. The numerical tests
included the application of six selected shell finite elements which accept
layered composite materials, available in the MSC.Marc FE library [4]. It was
pointed out that Element_75 (Bilinear Thick Shell) gives results closest to
reality, both qualitatively and quantitatively. A set of options/values of
numerical modelling and simulation parameters determined in [5] is applied in
the present study.
EXPERIMENTAL BENDING TEST
OF VALIDATION SEGMENT
A beam
composite segment of the box crosssection shown in Figure 2 was chosen
for examination. The overall dimensions are as follows: 2350×600×258 mm. The
segment includes a top composite shell (TS) and bottom composite shell (BS)
glued together at the contact surface using a 0.5 mm thick layer. The top
shell has a hat crosssection, whereas the bottom one is flat. The components
of the top and bottom shell laminates are specified in the Introduction. A
single BAT or GBX fabric corresponds to one lamina. The ply sequence for the TS
and BS laminates is [BAT/GBX/BAT]_{2} = = [0/45/0]_{2},
wherein only the fabric warp orientation is reflected. The following
interpretation of angles is assumed:
0  direction parallel to the beam axis
(warp direction in BAT800 fabric)
90  direction perpendicular to the beam
axis (weft direction in BAT800 fabric)
45/–45  directions at 45° to the beam axis (warp and
weft directions in GBX800 fabric).
Fig. 2. Crosssection
of validation segment: 1  top shell TS (4 mm),
2  adhesive layer (0.5 mm), 3  bottom shell BS (4 mm)
Rys. 2. Przekrój poprzeczny
segmentu walidacyjnego: 1  powłoka górna TS (4 mm), 2  warstwa kleju (0,5 mm),
3  powłoka dolna BS
(4 mm)
The
average thickness of a lamina is 0.663 mm, thus the design thickness of
the TS and BS laminate shells is: 6 × 0.663 mm ≈ 4.00 mm.
The shells were made separately using infusion technology and glued together.
Figure 3
depicts the diagram of the experimental stand for the 3point bending test of
the validation segment. The stand was embedded in a SATEC1200 universal
testing machine. The steel supports were made from an IPE300 Ibeam with
stiffening ribs arranged transversely to the axis of the segment. A 20 mm
thick steel plate was attached to the top flange. The contact edge of the plate
was chamfered with a radius of 5 mm. The transverse support Ibeams were
based on I200 longitudinal steel Ibeams located on the rigid bottom table of
the machine. The supports have low vertical susceptibility which was controlled
by an LKG157 laser sensor equipped with an LKGD500 controller.
The 3point
bending test was conducted at kinematic excitation over a vertical distance of
300 mm at
a crosshead speed of 1 mm/s. Force (P),
crosshead position (s) and vertical
displacement of the right support were recorded at a 10 Hz sampling
frequency using
a Traveler ESAM CF strain gauge bridge. Longitudinal strain gauges
EA16240LZ120/E were glued to the bottom surface of the segment at the
midspan and at the halfwidth strips of the adhesive layer.
Fig. 3. Diagram
of stand for 3point bending test of validation segment
Rys. 3. Schemat stanowiska do zginania trójpunktowego segmentu walidacyjnego
Figure 4 shows deformation of the segment at a 200 mm vertical displacement of the stamp. Large deformations and damages of the segment appear in the stamp area only. After completion of the loading (s = 300 mm), a return to the original geometric shape was observed. It indicates that buckling of the vertical walls occurred in the central zone of the segment during the bending process.
The P(s) plot of the stamp force (P) versus the crosshead displacement (s) is presented in Figure 5. In the range of 0÷22 mm, the response of the girder is quasilinearly elastic. The load capacity of the segment is P = 28.8 kN at the crosshead displacement of 22.0 mm. Afterwards, gradual loss of the load capacity with periodic increases is observed. The response in this range is nonlinear with a large number of chart folds corresponding to progressive local destruction of the segment, particularly in the stamp zone.
Fig. 4. Deformation
of validation segment corresponding to crosshead displacement s = 200 mm
Rys. 4. Deformacje segmentu walidacyjnego odpowiadające przemieszczeniu trawersy s = 200 mm
Vertical displacement of right support reaches 0.4 mm in the load capacity point. The relative error at this point is δ = 0.4/22.02 = 1.8%, and it decreases to 0.08% at the end of the test. Therefore, vertical susceptibility of the supports can be omitted in the simulation.
Fig. 5. Stamp
force (P) versus crosshead
displacement (s)
Rys. 5. Wykres siły nacisku stempla (P) w funkcji przemieszczenia trawersy (s)
NUMERICAL MODELLING AND SIMULATION
OF BENDING TEST OF VALIDATION SEGMENT
The numerical model of the validation segment is shown in Figure 6. QUAD4 shell FEs were used. The basic size of a shell element is 20 × 20 mm. The element size was reduced to approximately 12 × 12 mm in the stamp impact zone and chamfered areas. The adhesive layer is one of the layers of the laminates modelled using shell elements. The total number of finite elements and nodes of the segment model is 10836 and 10922, respectively. The supports and movable stamp are modelled as surfaces with perfectly rigid body properties.
Bilinear ThickShell Elements (No. 75) are used for composite shell modelling. They are bilinear, 2dimensional, 4node shell finite elements having three translational and three rotational degrees of freedom in each node. The transverse shear strains are calculated at the middle of the edges and interpolated to the integration points. The appropriate thickness of the shell and corresponding offsets from the midsurfaces were defined in the geometrical properties of the FE elements.
Fig. 6. FE model of validation segment
Rys. 6. Model
numeryczny segmentu walidacyjnego
An orthotropic linear elasticbrittle material
model was applied for the vinylester/glass lamina (B/F code) whereas an
isotropic linear elasticbrittle material model was used with respect to the
adhesive layer. The effective material constants of B/F lamina (after
homogenization), applied in laminate shells in the [0/90] or [45/–45]
configuration, are provided in Table 1, determined from respective
experimental tests. The material constants of NORPOL FI184 glue are provided
in Table 2, based on the manufacturer's material card, wherein: E, n  Young’s modulus, Poisson’s ratio, R_{t}  tensile strength, R_{c}  compressive strength, S  shear strength.
The Selective Gradual Degradation model of progressive failure was used with respect to laminate shells. This model decreases the material constants when failure occurs. Within an increment, it attempts to keep the highest failure index less than or equal to 1. Whenever a failure index larger than 1 occurs, the stiffness reduction factor is calculated based upon the value of the failure index.
TABLE 1. Elasticity and strength constants of B/F
lamina
TABELA 1. Stałe sprężystości i wytrzymałości laminy
B/F
Material
constant 
Unit 
Value 

[MPa] 
23400 

– 
0.153 

[MPa] 
3520 

[MPa] 
2300 

[MPa] 
449 

[MPa] 
336 

[MPa] 
45.2 

[MPa] 
27.2 
TABLE 2. Material constants for NOPROL FI184 glue
model
TABELA 2. Stałe materiałowe modelu kleju NOPROL FI184
Material
constant 
Unit 
Value 
E 
[MPa] 
3100 
n 
– 
0.36 
R_{t} 
[MPa] 
35.0 
R_{c} 
[MPa] 
35.0 
S 
[MPa] 
20.3 
The contact table was created to define contact.
Possible steel  laminate friction pairs were declared in respective subareas
of potential contact of the system components. The SegmenttoSegment contact model with the Touching option, including the Coulomb friction model, was applied.
A coefficient of static friction (m = 0.14)
was specified on the basis of the authors’ experiments. The Gravity Load option was taken into
account during the simulation. An
acceleration of 9810 mm/s^{2} with respect to the vertical axis
(Z) of the global coordinate system was declared.
Theoretically, a system for the 3point bending test of validation segment is perfectly bisymmetric. However, before applying the vertical load, the system is geometrically unstable (horizontal displacements at the supports are possible). Therefore, in order to ensure geometrical stability of the FE model of the validation segment, the translational degrees of freedom in the longitudinal and transverse symmetry planes were fixed. The rotational degrees of freedom were kept since the simulations were carried out with respect to the full numerical model.
The full NewtonRaphson method with the residual convergence criterion (relative tolerance of 0.1) was used to solve the problem. A conventional loading time of 1 s and a constant time step of 0.001 s were applied. Small strains and large rotations were taken into consideration in the calculations. The options/values of the parameters for numerical modelling and simulation of static processes including failure, using the FE code MSC.Marc, assumed in this study, are listed in Table 3.
Figure 7 shows virtual (numerical, simulated) F(s)
diagrams against the background of the experimental diagram, corresponding to
rare mesh (average size of FE is 20 × 20 mm) and dense mesh (average
size of FE is 10 × 10 mm). The experimental plot confirms
the correctness of the applied material models and
values/options of the modelling and simulation parameters listed in Table 3.
The experimental and virtual plots are coincident with regard to the initial
stiffness. After reaching 18% of the load capacity, the virtual chart exhibits
slightly lower stiffness in the range of 18÷36% and above 70% of the load
capacity results in a 46% increased displacement of the crosshead at the load
capacity point. It results from an undervalued shear modulus, G_{13} = G_{23}, which is determined from
the
approximate 3point bending test of the short beam.
The differences in virtual plots in the elastic
response zone (Fig. 7), corresponding to rare and dense meshes are small
whereas the load capacity corresponding to the rare mesh is closer to the
experimental values. After reaching the load capacity, progressive destruction
begins in the stamp operating zone. The virtual plots are similar to the
experimental plot for s < 250 mm,
both qualitatively and quantitatively. Further increasing of the crosshead
displacement leads to significant quantitative differences. The reason is the
undervalued shear strength, S_{13} = S_{23}, determined from the
approximate 3point bending test of the short beam. It can be assessed that the
simulation results corresponding to the rare mesh are validated positively.
TABLE 3. Options/values of parameters for numerical modelling and simulation
TABELA 3. Opcje/wartości
parametrów modelowania numerycznego i symulacji
Methodology component 
Reference [11] 
Presented study 
finite element (FE) type 
185 (Solid Shell) 
75 (Thick Shell) 
element size 
similar to laminate thickness 
20 × 20 mm 
failure criteria 
Hashin
Fabric, 
Hashin
Fabric, 
failure 
progressive 
progressive 
stiffness degradation method 
Gradual Selective 
Gradual Selective 
residual stiffness factor 
0.005 
0.1 
contact distance tolerance 
0.15 
automatic 
bias factor for distance tolerance 
0.95 
0.95 
friction type 
Coulomb bilinear (displacement) 
Coulomb bilinear (displacement) 
iteration method 
Full NewtonRaphson 
Full NewtonRaphson 
convergence criteria 
residual and displacement (0.02) 
residual (0.1) 
stepping procedure 
adaptive 
constant (1000 steps) 
advanced analysis options 
small strain, assumed strain, large rotations 
small strain, assumed strain, large rotations 
In the
virtual plot P(s) in the elastic response zone (Fig. 7), two points (L1, L2)
close to the load capacity point (L3) are visible. A slight decrease in force P with an increasing displacement s and regrowth of force P with a further increase in s can be observed in points L1, L2.
These points were called the load levels:
L1 (s = 19.5 mm, P = 22.6 kN), L2 (s = 27.5 mm, P = 27.5 kN), L3 (s = 32.0 mm, P = 28.0 kN). Contours of
the maximum values (through all layers) of the
effort indices were determined for these points, i.e.
R = max_{i}(R_{i}),
wherein i = 1,2,3,4 for laminates,
and
i = 1,2,3,4,5,6 for the adhesive
layer. For example,
Figure 8 shows a map of the maximum value of R in the composite shells, corresponding to load level L3. The
contour properly reflects the 3point bending test of
a composite thinwalled box beam and shows the failure area of the top shell.
Figure 9 shows the virtual deformation of the validation segment corresponding to the crosshead displacement of s = 200 mm. Comparing the deformation contour with a photo from the experiment (Fig. 4), good qualitative and quantitative agreement of segment deformation can be observed.
The
maximum values (through all layers) of effort indices R_{1}, R_{2},
R_{3}, R_{4} in the composite shells (indices R_{5}, R_{6} are not available in the applied type of shell
elements), corresponding to load levels L1, L2 and L3, are listed in Table 4.
The max max values are written in bold. The max max value of the effort index
for the adhesive layer, R = max R_{i}, i = 1,2,3,4,5,6 is 0.104.
Fig. 7. P(s) plots: E 
experimental; RM  simulation (rare mesh);
DM  simulation (dense mesh)
Rys. 7. Wykresy P(s): E  eksperyment; RM  symulacja (siatka rzadka); DM  symulacja (siatka gęsta)
Fig. 8. Contour of maximum values of effort index R in composite shells, corresponding to
load level L3
Rys. 8. Mapa maksymalnych wartości indeksu wytężenia R w powłokach kompozytowych, odpowiadająca poziomowi obciążenia L3 (skala 0÷1)
Fig. 9. Virtual deformation of
validation segment, corresponding to crosshead displacement of s = 200 mm
Rys. 9. Wirtualna deformacja segmentu walidacyjnego, odpowiadająca przemieszczeniu trawersy s = 200 mm
TABLE 4. List of maximum values of effort indices R_{i}_{ }(maximum values are written in bold)
TABELA 4. Zestawienie maksymalnych wartości indeksów wytężenia R_{i} (wartości maksymalne zapisano czcionką bold)
Load level 
R_{1} 
R_{2} 
R_{3} 
R_{4} 
L1 
0.852 
0.951 
0.806 
0.962 
L2 
0.979 
0.987 
0.978 
0.979 
L3 
0.982 
0.996 
0.985 
0.981 
On the basis of conducted numerical studies, the following conclusions can be drawn:
1) Contours of the effort index R properly reflect the 3point bending test of a composite box beam including the impact of the testing machine movable stamp and immovable supports.
2) A rigid stamp moving vertically down causes effort concentration in the central contact zone of the top shell (TS) with the stamp and in the far contact zones of the bottom shell (BS) with the lateral support plates.
3) Deflection of the beam segment changes contact at the support plates from the surface to the edge one. Lateral bending of the beam bottom at the supports results in quasipoint contact between the beam and the support edge.
4) For load level L1, the effort index of the composite segment is high and it comes to R = 0.962. Quasipoint concentrations of effort under the stamp (intersection of stamp transverse edges with the shell longitudinal edges), as well as close to the supports, are formed.
5) For load level L3, the effort index of the composite segment is very high and it comes to R = 0.996 ≈ 1 (load capacity of segment). Quasilinear concentrations of effort under the stamp (sections of shell longitudinal edges), as well as quasipoint concentrations of effort close to the supports, are formed. The most strenuous layers are 5 (GBX) and 6 (BAT) in the top shell (under stamp) and in the bottom shell (on support edges).
6) Quantitative and qualitative results allow one to interpret the L1 and L2 points on the P(s) plot as points of local slight decrease in load capacity resulting from the assumed methodology of numerical modelling.
7) The system model for the bending test is bisymmetric. However, the effort index contours are not perfectly bisymmetric due to imperfections in the numerical model (an automatically generated FE mesh is not perfectly bisymmetric).
8) The results in terms of F(s) plots and effort indices contours positively validate the numerical modelling and simulation of the bending test of a composite beam segment.
CONCLUSIONS
Experimental and numerical studies of a
composite validation box segment, consisting of two glass/
vinylester shells glued together, have been conducted. Laminate shells were
formed by means of infusion technology and glued one to another. The laminate
components, glue (adhesive layer) and manufacturing
technology of the beam segment are similar to those for the technical object,
i.e. the glued composite box footbridge.
A threepoint bending test of the validation segment was conducted. The experimental stand was designed and built in a SATEC1200 universal testing machine. The test was carried out to partial destruction of the segment, applying kinematic excitation with a crosshead speed of 1 mm/s and maximum vertical distance of 300 mm. The measurements included the following quantities: stamp force (P), vertical displacement of the crosshead (s), vertical displacement of the right support (to control support susceptibility), deformation of the beam segment during the test (photo documentation).
Numerical modelling and simulation of a bending test of the validation segment was conducted using FE code MSC.Marc 2010. The laminates were simulated using thickshell elements with the ortotropic linear elasticbrittle material model for the vinylester lamina, corresponding to a single layer of orthogonal quasibalanced stitched fabric. Numerical modelling and simulation of the static processes in the laminate shells including failure has been developed in comparison with the authors’ previous works (a new type of composite material, infusion technology, composite shells glued one to another).
Acknowledgements
The study
has been supported by the National Centre for Research and Development, Poland,
as a part of a research project No. PBS1/B2/6/2013, realized in the period
2013–2015. This support is gratefully acknowledged.
References
[1] Klasztorny M., Chroscielewski J., Szurgott P., Romanowski R., Design and numerical testing of 5box GFRP shell footbridge, 5th Int. Conf. on Footbridges: Past, Present & Future, London, England, 1618 July 2014, CD Proceed., Paper #1094, 18.
[2] Jones R.M., Mechanics of composite materials, Taylor & Francis, London 1999.
[3] Tsai S.W., Composites design, 4^{th} Edn., Think Composites, Dayton 1987.
[4] MSC.Marc r1, Vol. A, Theory and User Information, MSC.Software Co., Santa Ana, CA, USA, 2008.
[5] Klasztorny M., Bondyra A., Szurgott P., Nycz D., Numerical modelling of GFRP laminates with MSC.Marc system and experimental validation, Computational Material Science 2012, 64, 151156.
[6] Nycz D., Bondyra A., Klasztorny M., Gotowicki P., Numerical modelling and simulation of the composite segment bending test and experimental validation, Composites Theory and Practice 2012, 2(12) 126131.