1318
Proceedings of the 18
th
International Conference on Soil Mechanics and Geotechnical Engineering, Paris 2013
2 THREE-DIMENSIONAL ANALYSES
The earlier 2D stability analyses with Plaxis 2D 2010 contained
evaluation of different material models for soft clays. It was
shown that anisotropic S-CLAY1 based (Wheeler et.al. 2003)
material models can well express most of the important features
of soft clay, such as failure induced pore pressure. The Soft Soil
model was also found to be suitable with adjusted soil
parameters. It was also found that the counter weight berms can
be significantly smaller if design is conducted with the effective
strength parameters and a suitable material model compared to
the traditional undrained analysis.
The scope of the 3D analyses was to compare them with the
2D analyses and to model stability improvement objects, which
would be indefinite to model as plane strain. The 3D FEM
analyses were conducted with the Plaxis 3D program (version
2010.2.0.7044). At the first phase the whole test site was
modeled to compare 2D and 3D analyses. The geometry model
is shown in figure 2.
Figure 2. Full 3D geometry model containing 240 000 nodes and the
2 bogie section (12 m) with a pile row.
However, for the needs of modeling reinforcements,
geometry was reduced to two different options. The larger
model contained a section of two bogies (12 m) and the smaller
geometry was only a 1.0 m thick section from the middle of the
site. Larger model was used to evaluate different pile row
installations and the smaller model to observe an influence of a
single pile in more detail. Observations from the latter analyses
are shown in this study.
The Plaxis Soft Soil model was used for the soft clay, while
the Hardening Soil model was used for the coarse layers.
Parameters and soil behavior is calibrated with the displacement
and pore pressure data gathered from the conducted failure test.
The basic parameters of each soil layer are shown in table 1.
Table 1. Basic material parameters of the soil layers. Corresponding
layers are shown in figure 3.
γ
[kN/m
3
]
E
50
[MPa]
λ
*
‐
φ'
[°]
c'
[kPa]
POP
[kPa]
1 Ballast
20
50
38
0.2
2 Sandy fill
19
15
35
0.2
3 Dry crust
16
12
0
30
4 Clay
15
0.166 25
0.2
13
5 Clayey silt
17
0.08
27
0.2
20
3 MODELING WOODEN PILES
Wooden piles can be a cost-efficient method to improve
stability in a railway environment. There is also a lot of research
data available about the laterally loaded piles (Cai and Ugai
2000, Thompson et. al. 2005).
There are several options available to model laterally loaded
piles in a FEM program. The most convenient way is to use
Embedded pile elements, which are special beam (line)
elements creating a elastic region around them imitating real
structural element with a volume. The elastic region around the
pile is equal to the pile diameter. The element does not create
new geometry points to the model and therefore the analysis can
be conducted with coarser mesh compared to the volume pile.
Embedded pile elements cannot take into account a soil-pile
interaction. There is no interface between pile and soil and
therefore pile always moves with soil without sliding (Plaxis 3D
2010, Dao 2011).
Other options to model piles in a 3D program are a volume
pile and a plate element. In practice, the volume pile is a solid
soil element, which material model is linear elastic and diameter
equal with the pile diameter. To be able to inspect forces
affecting the pile, a beam element with very low elastic
modulus was inserted to the center of the pile. A plate element
is also applicable when the lateral forces are studied. In that
case width and stiffness of the plate should be equal to the
wooden pile. One should notice that the skin surface area of the
plate is not equal to a cylinder shaped pile, which should be
accounted in interface strength between soil and pile.
In this case the strength of the soil was fully accounted for
the pile skin, even though with a volume pile and a plate
element it is possible to use reduced interface strength. The
geometry model was a 1 m thick cross section, where one
vertical d200 mm wooden pile was inserted 5 m from the center
line of the track, equal to 2 m from the embankment toe. The
pile was installed through the clayey silt layer to the surface of
the sand layer, where the approximated tip resistance of the pile
head would be 24 kN.
Figure 3. Vertical pile and displacements in 1 m thick cross section.
Location of the pile is 5.0 m from the center line. Displacement
contours are in 5 mm steps from 10 to 55 mm. Soil layers are sketched
and numbered.
Train load was set to 70.0 kN/m
3
. With this load the overall
safety factor of the embankment is F=1.23 without a pile and
maximum displacement of the embankment is 60 mm, as shown
in figure 3. Number of nodes was 19700 in the original
geometry without a pile. Volume of the elements was
0.02…0.03 m
3
which is very dense mesh for 3D analysis. The
embedded pile was modeled using 2 different meshing options.
First calculation conducted with the original mesh and then with
a refined mesh, where a 200 mm diameter tube was created
around the embedded pile. The tube had equal properties with
the surrounding soil but it induced a mesh refinement around
the embedded pile similar with the mesh, which was
automatically created around the volume pile. Otherwise the
meshing options were similar for soil layers in the parallel
analysis.
In figure 4 a lateral displacement of different pile types from
parallel analysis at the end of the loading is shown. From left to
right the piles are embedded pile, embedded pile with refined
mesh, volume pile and plate element. Maximum displacement
was very similar at every case; 29, 31, 32 and 33 mm
respectively. Maximum value was slightly smaller for the
original embedded pile which could be due to coarser element
mesh. On the other hand it also indicates slightly smaller
bending moments.
