Plaxis 3d tutorial manual

PLAXIS 3D Tutorial Manual
CONNECT Edition V20

TABLE OF CONTENTS
TABLE OF CONTENTS
1 Foundation in overconsolidated clay 6
1.1 Case A: Rigid foundation 7
1.2 Case B: Raft foundation 19
1.3 Case C: Pile-Raft foundation 26
2 Excavation in sand 31
2.1 Geometry 32
2.2 Mesh generation 37
2.3 Performing calculations 37
2.4 Viewing the results 40
3 Loading of a suction pile 44
3.1 Geometry 44
4 Construction of a road embankment 54
4.1 Geometry 54
4.5 Safety analysis 65
4.6 Using drains 68
5 Stability of a diaphragm wall excavation 70
5.1 Geometry 70
6 Phased excavation of a shield tunnel 78
6.1 Geometry 78
7 Rapid drawdown analysis 98
7.1 Geometry 98
8 Dynamic analysis of a generator on an elastic foundation 110
8.1 Geometry 110
PLAXIS 3D CONNECT Edition V20 | Tutorial Manual 3

TUTORIAL MANUAL
9 Free vibration and earthquake analysis of a building 120
9.1 Geometry 120
Appendix A - Menu tree 134
Appendix B - Calculation scheme for initial stresses due to soil weight 138
4 Tutorial Manual | PLAXIS 3D CONNECT Edition V20

INTRODUCTION
INTRODUCTION
PLAXIS is a finite element package that has been developed specifically for the analysis
of deformation, stability and flow in geotechnical engineering projects. The simple
graphical input procedures enable a quick generation of complex finite element models,
and the enhanced output facilities provide a detailed presentation of computational
results. The calculation itself is fully automated and based on robust numerical
procedures. This concept enables new users to work with the package after only a few
hours of training.
Though the various tutorials deal with a wide range of interesting practical applications,
this Tutorial Manual is intended to help new users become familiar with PLAXIS 3D. The
tutorials and the respective material data sets should therefore not be used as a basis for
practical projects.
Users are expected to have a basic understanding of soil mechanics and should be able
to work in a Windows environment. It is strongly recommended that the tutorials are
followed in the order that they appear in the manual. Please note that minor differences in
results maybe found, depending on hardware and software configuration.
The Tutorial Manual does not provide theoretical background information on the finite
element method, nor does it explain the details of the various soil models available in the
program. The latter can be found in the Material Models Manual, as included in the full
manual, and theoretical background is given in the Scientific Manual. For detailed
information on the available program features, the user is referred to the Reference
Manual. In addition to the full set of manuals, short courses are organised on a regular
basis at several places in the world to provide hands-on experience and background
information on the use of the program.

TUTORIAL MANUAL
1 FOUNDATION IN OVERCONSOLIDATED CLAY
In this chapter a first application of PLAXIS 3D is considered, namely the settlement of a
foundation in clay. This is the first step in becoming familiar with the practical use of the
program.
The general procedures for the creation of a geometry, the generation of a finite element
mesh, the execution of a finite element calculation and the evaluation of the output results
are described here in detail. The information provided in this tutorial will be utilised in the
following tutorials. Therefore, it is important to complete this first tutorial before
attempting any further tutorial examples.
18.0 m
75.0 m
75.0 mBuilding
Clay
x
x
y
z
z = 0
z = -2
z = -40
40.0 m
Figure 1.1 Geometry of a square building on a raft foundation
GEOMETRY
This exercise deals with the construction and loading of a foundation of a square building
in a lightly overconsolidated lacustrine clay. Below the clay layer there is a stiff rock layer
that forms a natural boundary for the considered geometry. The rock layer is not included
in the geometry; instead an appropriate boundary condition is applied at the bottom of the
clay layer. The purpose of the exercise is to find the settlement of the foundation.
The building consists of a basement level and 5 floors above the ground level (Figure
1.1). To reduce calculation time, only one-quarter of the building is modelled, using
symmetry boundary conditions along the lines of symmetry. To enable any possible

FOUNDATION IN OVERCONSOLIDATED CLAY
mechanism in the clay and to avoid any influence of the outer boundary, the model is
extended in both horizontal directions to a total width of 75 m.
The model is considered in three different cases:
Case A: The building is considered very stiff and rough. The basement is simulated by
means of non-porous linear elastic volume elements.
Case B: The structural forces are modelled as loads on a raft foundation.
Case C: Embedded beams are included in the model to reduce settlements.
1.1 CASE A: RIGID FOUNDATION
In this case, the building is considered to be very stiff. The basement is simulated by
means of non-porous linear elastic volume elements. The total weight of the basement
corresponds to the total permanent and variable load of the building. This approach leads
to a very simple model and is therefore used as a first exercise, but it has some
disadvantages. For example it does not give any information about the structural forces in
the foundation.
Objectives:
• Starting a new project.
• Creation of soil stratigraphy using a single borehole.
• Creation of material data sets.
• Creation of volumes using Create surface and Extrude tools.
• Assigning material.
• Local mesh refinement.
• Generation of mesh.
• Generating initial stresses using the K0 procedure.
• Defining a Plastic calculation.
1.1.1 GEOMETRY INPUT
• Start the PLAXIS 3D program. The Quick select dialog box will appear in which you
can select an existing project or create a new one (Figure 1.2).
• Click Start a new project. The Project properties window appears, consisting of
Project and Model tabsheets.
Project properties
The first step in every analysis is to set the basic parameters of the finite element model.
This is done in the Project properties window. These properties include the description of
the problem, the basic units and the size of the drawing area.

TUTORIAL MANUAL
Figure 1.2 Quick select dialog box
To enter the appropriate properties for the foundation calculation follow these steps:
• In the Project tabsheet, enter "Tutorial 1" as the Title of the project and type
"Settlements of a foundation" in the Comments box (Figure 1.3).
Figure 1.3 Project tabsheet of the Project properties window
• Proceed to the Model tabsheet by clicking either the Next button or the Model tab
(Figure 1.4).
• Keep the default units in the Units box (Length = m; Force = kN; Time = day).
• The General box indicates a fixed gravity of 1.0 G, in the vertical downward direction
(-z).
• In the γwater box the unit weight of water can be defined. Keep this to the default
value of 10 kN/m3
.
• Define the limits for the soil contour as xmin = 0, xmax = 75, ymin = 0 and ymax = 75 in
the Contour group box.
• Click the OK button to confirm the settings.
Hint: In case of a mistake or for any other reason that the project properties need
to be changed, you can access the Project properties window by selecting
the corresponding option in the File menu.

Figure 1.4 Model tabsheet of the Project properties window
Definition of soil stratigraphy
When you click the OK button the Project properties window will close and the Soil mode
view will be shown. Information on the soil layers is entered in boreholes.
Boreholes are locations in the drawing area at which the information on the position of
soil layers and the water table is given. If multiple boreholes are defined, PLAXIS 3D will
automatically interpolate between the boreholes, and derive the position of the soil layers
from the borehole information.
Hint: PLAXIS 3D can also deal with layers that are discontinuous, i.e. only locally
present in the model area. See Section 4.2.2 of the Reference Manual for
more information.
In the current example, only one soil layer is present, and only a single borehole is
needed to define the soil stratigraphy. In order to define the borehole, follow these steps:
Click the Create borehole button in the side toolbar to start defining the soil
stratigraphy. Click on position (0 0 0) in the geometry. A borehole will be located at
(x, y) = (0 0). The Modify soil layers window will appear.
• In the Modify soil layers window add a soil layer by clicking on the Add button. Keep
the top boundary of the soil layer at z = 0 and set the bottom boundary to z = −40
m.
• Set the Head value in the borehole column to −2 m (Figure 1.5).
The creation of material data sets and their assignment to soil layers is described in the
following section.
1.1.2 MATERIAL DATA SETS
In order to simulate the behaviour of the soil, a suitable material model and appropriate
material parameters must be assigned to the geometry. In PLAXIS soil properties are
collected in material data sets and the various data sets are stored in a material
database. From the database, a data set can be assigned to one or more clusters. For
structures (like beams, plates, etc.) the system is similar, but different types of structures

TUTORIAL MANUAL
Figure 1.5 Modify soil layers window
have different parameters and therefore different types of data sets.
PLAXIS 3D distinguishes between material data sets for Soils and interfaces, Plates,
Geogrids, Beams, Embedded beams and Anchors.
Open the Material sets window by clicking the Materials button in the Modify soil
layers window.
Hint: In the case that the Modify soil layers window was closed by mistake, it can
be re-opened by double-clicking the borehole in the drawing area or by
selecting the Modify soil layers option from the Soil menu.
• Click the New button in the lower part of the Material sets window. The Soil window
will appear. It contains ﬁve tabsheets: General, Parameters, Groundwater,
Interfaces and Initial.
• In the Material set box of the General tabsheet (Figure 1.6), write "Lacustrine Clay"
in the Identiﬁcation box.
• Select Mohr-Coulomb as the material model from the Material model drop-down
menu and Drained from the Drainage type drop-down menu.
• Enter the unit weights in the General properties box according to the material data
as listed in Table 1.1. Keep the unmentioned Advanced parameters as their default
values.
Hint: To understand why a particular soil model has been chosen, see Appendix B
of the Material Models Manual.

Figure 1.6 General tabsheet of the Soil and interfaces data set window
Table 1.1 Material properties
Parameter Name Lacustrine clay Building Unit
General
Material model Model Mohr-Coulomb Linear elastic −
Drainage type Type Drained Non-porous −
Unit weight above phreatic level γunsat 17.0 50 kN/m3
Unit weight below phreatic level γsat 18.0 − kN/m3
Parameters
Young's modulus (constant) E' 1 · 104
3 · 107
kN/m2
Poisson's ratio ν' 0.3 0.15 −
Cohesion (constant) c'ref 10 − kN/m2
Friction angle ϕ' 30.0 − ◦
Dilatancy angle ψ 0.0 − ◦
Initial
K0 determination − Automatic Automatic −
Lateral earth pressure coefficient K0 0.5000 0.5000 −
• Click the Next button or click the Parameters tab to proceed with the input of model
parameters. The parameters appearing on the Parameters tabsheet depend on the
selected material model (in this case the Mohr-Coulomb model). The Mohr-Coulomb
model involves only five basic parameters (E', ν', c', ϕ', ψ'). See the Material Models
Manual for a detailed description of the different soil models and their corresponding
parameters.
• Enter the model parameters E', ν', c'ref , ϕ' and ψ of Lacustrine clay according to
Table 1.1 in the corresponding boxes of the Parameters tabsheet (Figure 1.7).
• No consolidation will be considered in this exercise. As a result, the permeability of
the soil will not influence the results and the Groundwater window can be skipped.
• Since the geometry model does not include interfaces, the Interfaces tab can be
skipped.
• Click the Initial tab and check that the K0 determination is set to Automatic. In that

TUTORIAL MANUAL
Figure 1.7 Parameters tabsheet of the Soil and interfaces data set window
case K0 is determined from Jaky's formula: K0 = 1 − sin ϕ.
• Click the OK button to confirm the input of the current material data set. The created
data set appears in the tree view of the Material sets window.
• Drag the set Lacustrine clay from the Material sets window (select it and hold down
the left mouse button while moving) to the graph of the soil column on the left hand
side of the Modify soil layers window and drop it there (release the left mouse
button).
Hint: Notice that the cursor changes shape to indicate whether or not it is possible
to drop the data set. Correct assignment of the data set to the soil layer is
indicated by a change in the colour of the layer.
The building is modelled by a linear elastic non-porous material. To define this data set,
follow these steps:
• Click the New button in the Material sets window.
• In the Material set box of the General tabsheet, write "Building" in the Identification
box.
• Select Linear elastic as the material model from the Material model drop-down
menu and Non-porous from the Drainage type drop-down menu.
• Enter the unit weight in the General properties box according to the material data set
as listed in Table 1.1. This unit weight corresponds to the total permanent and
variable load of the building.
• Click the Next button or click the Parameters tab to proceed with the input of the

model parameters. The linear elastic model involves only two basic parameters (E',
ν').
• Enter the model parameters of Table 1.1 in the corresponding edit boxes of the
Parameters tabsheet.
• Click the OK button to confirm the input of the current material data set. The created
data set will appear in the tree view of the Material sets window, but it is not directly
used.
• Click the OK button to close the Material sets window.
• Click the OK button to close the Modify soil layers window.
Hint: PLAXIS 3D distinguishes between a project database and a global database
of material sets. Data sets may be exchanged from one project to another
using the global database. The global database can be shown in the Material
sets window by clicking the Show global button. The data sets of all tutorials
in the Tutorial Manual are stored in the global database during the installation
of the program.
1.1.3 DEFINITION OF STRUCTURAL ELEMENTS
The structural elements are created in the Structures mode of the program. Click the
Structures button to proceed with the input of structural elements. To model the building:
Click the Create surface button. Position the cursor at the coordinate (0 0 0). Check
the cursor position displayed in the cursor position indicator. As you click, the first
surface point of the surface is defined.
• Define three other points with coordinates (0 18 0), (18 18 0), (18 0 0) respectively.
Press the right mouse button or Esc to finalize the definition of the surface. Note
that the created surface is still selected and displayed in red.
Click the Extrude object button to create a volume from the surface.
• Change the z value to -2 in the Extrude window (Figure 1.8). Click the Apply button
to close the window.
Figure 1.8 Extrude window

TUTORIAL MANUAL
Click the Select button. Select the created surface using the right mouse button.
Select Delete from the appearing menu. This will delete the surface but the building
volume is retained.
The building volume, as well as the corresponding material data sets have now been
created.
1.1.4 MESH GENERATION
The model is complete. In order to proceed to the Mesh mode click the Mesh tab.
PLAXIS 3D allows for a fully automatic mesh generation procedure, in which the
geometry is divided into volume elements and compatible structure elements, if
applicable. The mesh generation takes full account of the position of the geometry
entities in the geometry model, so that the exact position of layers, loads and structures is
accounted for in the finite element mesh. A local refinement will be considered in the
building volume. To generate the mesh, follow these steps:
Click the Refine mesh button in the side toolbar and click the created building
volume to refine the mesh locally. It will colour green.
Figure 1.9 The indication of the local refinement in the model
Click the Generate mesh button in the side toolbar or select the Generate mesh
option in the Mesh menu. Change the Element distribution to Coarse in the Mesh
options window (Figure 1.10) and click OK to start the mesh generation.
After the mesh is generated, click the View mesh button. A new window is opened
displaying the generated mesh (Figure 1.11).
• Click on the Close tab to close the Output program and go back to the Mesh mode
of the Input program.
1.1.5 PERFORMING CALCULATIONS
Once the mesh has been generated, the finite element model is complete. Click Staged
construction to proceed with the definition of calculation phases.

Figure 1.10 Mesh options window
Figure 1.11 Generated mesh in the Output window
Hint: By default, the Element distribution is set to Medium. The Element
distribution setting can be changed in the Mesh options window. In addition,
options are available to refine the mesh globally or locally (Section 7.1 of
Reference Manual).
» The finite element mesh has to be regenerated if the geometry is modified.
» The automatically generated mesh may not be perfectly suitable for the
intended calculation. Therefore it is recommended that the user inspects the
mesh and makes refinements if necessary.
Initial conditions
The 'Initial phase' always involves the generation of initial conditions. In general, the initial
conditions comprise the initial geometry configuration and the initial stress state, i.e.
effective stresses, pore pressures and state parameters, if applicable. The initial water
level has been entered already in the Modify soil layers window. This level is taken into
account to calculate the initial effective stress state. It is therefore not needed to enter the
Flow conditions mode.

TUTORIAL MANUAL
When a new project has been defined, a first calculation phase named "Initial phase", is
automatically created and selected in the Phases explorer (Figure 1.12). All structural
elements and loads that are present in the geometry are initially automatically switched
off; only the soil volumes are initially active.
Figure 1.12 Phases explorer
In this tutorial lesson the properties of the Initial phase will be described. This part of the
tutorial gives an overview of the options to be defined even though the default values of
the parameters are used.
The Phases window (Figure 1.13) is displayed by clicking the Edit phase button or
by double clicking on the phase in the Phases explorer.
Figure 1.13 The Phases window for Initial phase
By default the K0 procedure is selected as Calculation type in the General subtree
of the Phases window. This option will be used in this project to generate the initial
stresses.
The Staged construction option is selected as the Loading type. This is the only
option available for the K0 procedure.
The Phreatic option is selected by default as the Pore pressure calculation type.
• The other default options in the Phases window will be used as well in this tutorial.
Click OK to close the Phases window.
• In the Model explorer expand the Model conditions subtree.
• Expand the Water subtree. The water level generated according to the Head value
assigned to boreholes in the Modify soil layers window (BoreholeWaterLevel_1) is
automatically assigned to GlobalWaterLevel.

• Make sure that all the soil volumes in the project are active and the material
assigned to them is Lacustrine clay.
Hint: The K0 procedure may only be used for horizontally layered geometries with
a horizontal ground surface and, if applicable, a horizontal phreatic level.
See Section 7.3 of the Reference Manual for more information on the K0
procedure.
Construction stage
After the deﬁnition of the initial conditions, the construction of the building can be
modelled. This will be done in a separate calculation phase, which needs to be added as
follows:
Click the Add button in the Phases explorer. A new phase, named Phase_1 will be
added in the Phases explorer.
• Double-click Phase_1 to open the Phases window.
• In the ID box of the General subtree, write (optionally) an appropriate name for the
new phase (for example "Building").
• The current phase starts from Initial phase, which contains the initial stress state.
The default options and values assigned are valid for this phase (Figure 1.14).
Figure 1.14 The Phases window for Building phase
• Click OK to close the Phases window.
• Right-click the building volume as created in Section 1.1.3. From the Set material
option in the appearing menu select the Building option. The 'Building' data set has
now been assigned to the building volume.
Hint: Calculation phases may be added, inserted or deleted using the Add, Insert
and Delete buttons in the Phases explorer or in the Phases window.

TUTORIAL MANUAL
Execution of calculation
All calculation phases (two phases in this case) are marked for calculation (indicated by a
blue arrow). The execution order is controlled by the Start from phase parameter.
Click the Calculate button to start the calculation process. Ignore the warning that
no nodes and stress points have been selected for curves. During the execution of a
calculation, a window appears which gives information about the progress of the
actual calculation phase (Figure 1.15).
Figure 1.15 Active task window displaying the calculation progress
The information, which is continuously updated, shows, amongst others, the calculation
progress, the current step number, the global error in the current iteration and the number
of plastic points in the current calculation step. It will take a few seconds to perform the
calculation. When a calculation ends, the window is closed and focus is returned to the
main window.
The phase list in the Phases explorer is updated. A successfully calculated phase is
indicated by a check mark inside a green circle.
Save the project before viewing results.
Viewing calculation results
Once the calculation has been completed, the results can be displayed in the Output
program. In the Output program, the displacement and stresses in the full
three-dimensional model as well as in cross sections or structural elements can be
viewed. The computational results are also available in tabular form. To view the current
results, follow these steps:

• Select the last calculation phase (Building) in the Phases explorer tree.
Click the View calculation results button in the side toolbar to open the Output
program. The Output program will, by default, show the three-dimensional deformed
mesh at the end of the selected calculation phase. The deformations are scaled to
ensure that they are clearly visible.
• Select Total Displacements → |u| from the Deformations menu. The plot shows
colour shadings of the total displacements (Figure 1.16).
• A legend is presented with the displacement values at the colour boundaries. When
the legend is not present, select the Legend option from the View menu to display it.
In the Output window click the Iso surfaces button to display the areas having the
same displacement.
Figure 1.16 Shadings of Total displacements at the end of the last phase
Hint: In addition to the Total displacements, the Deformations menu allows for the
presentation of Incremental displacements and Phase displacements.
» The incremental displacements are the displacements that occurred in one
calculation step (in this case the ﬁnal step). Incremental displacements may
be helpful in visualising failure mechanisms.
» Phase displacements are the displacements that occurred in one calculation
phase (in this case the last phase). Phase displacements can be used to
inspect the impact of a single construction phase, without the need to reset
displacements to zero before starting the phase.
1.2 CASE B: RAFT FOUNDATION
In this case, the model is modiﬁed so that the basement consists of structural elements.
This allows for the calculation of structural forces in the foundation. The raft foundation

TUTORIAL MANUAL
consists of a 50 cm thick concrete floor stiffened by concrete beams. The walls of the
basement consist of 30 cm thick concrete. The loads of the upper floors are transferred
to the floor slab by a column and by the basement walls. The column bears a load of
11650 kN and the walls carry a line load of 385 kN/m, as sketched in Figure 1.17.
12.0 m12.0 m
6.0 m6.0 m
385 kN/m385 kN/m
11650 kN
5.3 kN/m2
Figure 1.17 Geometry of the basement
In addition, the floor slab is loaded by a distributed load of 5.3 kN/m2
. The properties of
the clay layer will be modified such that stiffness of the clay will increase with depth.
Objectives:
• Saving project under a different name.
• Modifying existing data sets.
• Defining a soil stiffness that increases with depth.
• Modelling of plates and defining material data set for plates.
• Modelling of beams and defining material data set for beams.
• Assigning point loads.
• Assigning line loads.
• Assigning distributed loads to surfaces.
• Deleting phases.
• Activation and deactivation of soil volumes.
• Activation and deactivation of structural elements.
• Activation of loads.
• Zooming in Output.
• Drawing cross sections in Output.
• Viewing structural output.
Geometry input
The geometry used in this exercise is the same as the previous one, except that
additional elements are used to model the foundation. It is not necessary to create a new
model; you can start from the previous model, store it under a different name and modify
it. To perform this, follow these steps:

Start the PLAXIS 3D program. The Quick select dialog box will appear in which the
project of case A should be selected.
• Select the Save project as option in the File menu to save the project under a
different name (e.g. "Tutorial 1b").
The material set for the clay layer has already been defined. To modify this material set to
take into account the stiffness of the soil increasing with depth, follow these steps:
Open the Material sets window by clicking the Show materials button.
• Make sure that the option Soil and interfaces is selected as Set type.
• Select the Lacustrine clay material set and click the Edit button.
• In the Parameters tabsheet, change the stiffness of the soil E' to 5000 kN/m2
.
• Enter a value of 500 in the E'inc box in the Advanced parameters. Keep the default
value of 0.0 m for zref . Now the stiffness of the soil is defined as 5000 kN/m2
at
z = 0.0 m and increases with 500 kN/m2
per meter depth.
• Click OK to close the Soil window.
• Click OK to close the Material sets window.
Definition of structural elements
Proceed to the Structures mode to define the structural elements that compose the
basement.
Click the Selection button.
• Right-click the volume representing the building. Select the Decompose into
surfaces option from the appearing menu.
• Delete the top surface by selecting it and pressing the Delete key.
Select the volume representing the building. Click the visualisation toggle in the
Selection explorer to hide the volume.
• Right-click the bottom surface of the building. Select the Create plate option from
the appearing menu.
• Assign plates to the two vertical basement surfaces that are inside the model.
Delete the remaining two vertical surfaces at the model boundaries.
Hint: Multiple entities can be selected by holding the Ctrl button pressed while
clicking on the entities.
» A feature can be assigned to multiple similar objects the same way as to a
single selection.
Open the material data base and set the Set type to Plates.
• Create data sets for the basement floor and for the basement walls according to
Table 1.2.
• Drag and drop the data sets to the basement floor and the basement walls
accordingly. It may be needed to move the Material sets window by clicking at its

TUTORIAL MANUAL
Figure 1.18 Location of plates in the project
header and dragging it.
Table 1.2 Material properties of the basement floor and basement walls
Parameter Name Basement floor Basement wall Unit
Type of behaviour Type Elastic, isotropic Elastic, isotropic −
Thickness d 0.5 0.3 m
Weight γ 15 15.5 kN/m3
Young's modulus E1 3 · 107
3 · 107
kN/m2
Poisson's ratio ν12 0.15 0.15 −
Hint: When specifying a unit weight, please consider the fact that the element itself
does not occupy any volume and overlaps with the soil elements. Hence, it
might be considered to subtract the unit soil weight from the real unit weight
of the plate, beam or embedded beam material in order to compensate for
the overlap. For partially overlapping plates, beams or embedded beams the
reduction of the unit weight should be proportional.
• Right-click the bottom of the surface of the building volume and select the Create
surface load option from the appearing menu. The actual value of the load can be
assigned in the Structures mode as well as when the calculation phases will be
defined (Phase definition mode). In this example, the value will be assigned in the
Phase definition modes.
Click the Create line button in the side toolbar.
Select the Create line load option from the additional tools displayed.
• Click the command input area, type "0 18 0 18 18 0 18 0 0 " and press Enter. Line
loads will now be defined on the basement walls. The defined values are the

coordinates of the three points of the lines. Click the right mouse button to stop
drawing line loads.
Click the Create line button in the side toolbar.
Select the Create beam option from the additional tools displayed.
• Click on (6 6 0) to create the first point of a vertical beam. Keep the Shift key
pressed and move the mouse cursor to (6 6 -2). Note that while the Shift key is
pressed the cursor will move only vertically. As it can be seen in the cursor position
indicator, the z coordinate changes, while x and y coordinates will remain the same.
Click on (6 6 -2) to define the second point of the beam. To stop drawing click the
right mouse button.
• Create horizontal beams from (0 6 -2) to (18 6 -2) and from (6 0 -2) to (6 18 -2).
Hint: By default, the cursor is located at z=0. To move in the vertical direction,
keep the Shift key pressed while moving the mouse.
Open the material data base and set the Set type to Beams.
• Create data sets for the horizontal and for the vertical beams according to Table 1.3.
Assign the data set to the corresponding beam elements by drag and drop.
Table 1.3 Material properties of the basement column and basement beams
Parameter Name Basement column Basement beam Unit
Material type Type Elastic Elastic −
Young's modulus E 3 · 107
3 · 107
kN/m2
Volumetric weight γ 24.0 6.0 kN/m3
Cross section area A 0.49 0.7 m2
Moment of Inertia I2 0.020 0.029 m4
I3 0.020 0.058 m4
Click the Create load button in the side toolbar.
Select the Create point load option from the additional tools displayed. Click at (6 6
0) to add a point load at the top of the vertical beam.
Proceed to the Mesh tabsheet to generate the mesh.
Mesh generation
Click the Generate mesh. Keep the Element distribution as Coarse.
Inspect the generated mesh.
As the geometry has changed, all calculation phases have to be redefined.
1.2.1 PERFORMING CALCULATIONS
Proceed to the Staged construction mode.

TUTORIAL MANUAL
Initial conditions
As in the previous example, the K0 procedure will be used to generate the initial
conditions.
• All the structural elements should be inactive in the Initial Phase.
• No excavation is performed in the initial phase. So, the basement volume should be
active and the material assigned to it should be Lacustrine clay.
Construction stages
Instead of constructing the building in one calculation stage, separate calculation phases
will be used. In Phase 1, the construction of the walls and the excavation is modelled. In
Phase 2, the construction of the floor and beams is modelled. The activation of the loads
is modelled in the last phase (Phase 3).
The calculation type for the phases representing the construction stages is set by
default to Plastic.
• In the Phases window rename Phase_1 to "Excavation".
• In the Staged construction mode deactivate the soil volume located over the
foundation by selecting it and by clicking on the checkbox in front of it in the
Selection explorer.
• In the Model explorer click the checkbox in front of the plates corresponding to the
basement walls to activate them.
In the Phases explorer click the Add phase button. A new phase (Phase_2) is
added. Double-click Phase_2. The Phases window pops up.
• Rename the phase by defining its ID as "Construction". Keep the default settings of
the phase and close the Phases window.
• In the Model explorer click the checkbox in front of the plate corresponding to the
basement floor to activate it.
• In the Model explorer click the checkbox in front of the beams to activate all the
beams in the project.
Add a new phase following the Construction phase. Rename it to "Loading".
• In the Model explorer click the checkbox in front of the Surface loads to activate the
surface load on the basement floor. Set the value of the z-component of the load to
-5.3. This indicates a load of 5.3 kN/m2
, acting in the negative z-direction.
• In the Model explorer, click the checkbox in front of Line loads to activate the line
loads on the basement walls. Set the value of the z-component of each load to
-385. This indicates a load of 385 kN/m, acting in the negative z-direction.
• In the Model explorer click the checkbox in front of Point loads to activate the point
load on the basement column. Set the value of the z-component of the load to
-11650. This indicates a load of 11650 kN, acting in the negative z-direction.
Click the Preview phase button to check the settings for each phase.
As the calculation phases are completely defined, calculate the project. Ignore the
warning that no nodes and stress points have been selected for curves.

Save the project after the calculation.
Viewing calculation results
• Select Construction phase in the Phases explorer.
Click the View calculation results button to open the Output program. The deformed
mesh at the end of this phase is shown.
• Select the last phase in the Displayed step drop-down menu to switch to the results
at the end of the last phase.
In order to evaluate stresses and deformations inside the geometry, select the
Vertical cross section tool. A top view of the geometry is presented and the Cross
section points window appears. As the largest displacements appear under the
column, a cross section here is most interesting.
• Enter (0.0 6.0) and (75.0 6.0) as the coordinates of the first point (A) and the second
point (A') respectively in the Cross section points window.
• Click OK. A vertical cross section is presented. The cross section can be rotated in
the same way as a regular 3D view of the geometry.
• Select Total displacements → uz from the Deformations menu (Figure 1.19). The
maximum and minimum values of the vertical displacements are shown in the
caption. If the title is not visible, select this option from the View menu.
Figure 1.19 Cross section showing the total vertical displacement
• Press CTRL+ and CTRL− to move the cross section.
• Return to the three-dimensional view of the geometry by selecting this window from
the list in the Window menu.
• Double-click the floor. A separate window will appear showing the displacements of
the floor. To look at the bending moments in the floor, select M11 from the Forces
menu.

TUTORIAL MANUAL
Click the Shadings button. The plot in Figure 1.20 will be displayed.
Figure 1.20 Bending moments in the basement floor
To view the bending moments in tabulated form, click the Table option in the Tools
menu. A new window is opened in which a table is presented, showing the values of
bending moments in each node of the floor.
1.3 CASE C: PILE-RAFT FOUNDATION
As the displacements of the raft foundation are rather high, embedded beams will be
used to decrease these displacements. These embedded beams represent bored piles
with a length of 20 m and a diameter of 1.5 m.
Objectives:
• Using embedded beams.
• Defining material data set for embedded beams.
• Creating multiple copies of entities.
Geometry input
The geometry used in this exercise is the same as the previous one, except for the pile
foundation. It is not necessary to create a new model; you can start from the previous
model, store it under a different name and modify it. To perform this, follow these steps:

Start the PLAXIS 3D program. The Quick select dialog box will appear in which the
project of Case B should be selected.
• Select the Save project as option in the File menu to save the project under a
different name (e.g. "Tutorial 1c").
Definition of embedded beam
• Proceed to the Structures mode.
Click the Create line button at the side tool bar and select the Create embedded
beam from the additional tools that appear.
• Define a pile from (6 6 -2) to (6 6 -22).
Open the material data base and set the Set type to Embedded beams.
• Create a data set for the embedded beam according to Table 1.4. The value for the
cross section area A and the moments of inertia I2 and I3 are automatically
calculated from the diameter of the massive circular pile. Confirm the input by
clicking OK.
Table 1.4 Material properties of embedded beam
Parameter Name Pile foundation Unit
kN/m2
Unit weight γ 6.0 kN/m3
Beam type - Predefined −
Predefined beam type - Massive circular beam −
Diameter Diameter 1.5 m
Axial skin resistance Type Linear −
Maximum traction allowed at the top of the
embedded beam
Tskin,start,max 200 kN/m
Maximum traction allowed at the bottom of
the embedded beam
Tskin,end,max 500 kN/m
Base resistance Fmax 1 · 104
kN
• Drag and drop the Embedded beam data to the embedded beam in the drawing
area. The embedded beam will change colour to indicate that the material set has
been assigned successfully.
Hint: A material set can also be assigned to an embedded beam by right-clicking it
either in the drawing area or in the Selection explorer and the Model explorer
and selecting the material from the Set material option in the displayed menu.
Click the Select button and select the embedded beam.
Click the Create array button.
• In the Create array window, select the 2D, in xy plane option for shape.
• Keep the number of columns as 2. Set the distance between the columns to x = 12
and y = 0.
• Keep the number of rows as 2. Set the distance between the rows to x = 0 and

TUTORIAL MANUAL
y = 12 (Figure 1.21).
• Press OK to create the array. A total of 2x2 = 4 piles will be created.
Figure 1.21 Create array window
Mesh generation
As the geometry model is complete now, the mesh can be generated.
Create the mesh. Keep the Element distribution as Coarse.
View the mesh.
• Click the eye button in front of the Soil subtree in the Model explorer to hide the soil.
The embedded beams can be seen (Figure 1.22).
Performing calculations
After generation of the mesh, all construction stages must be redeﬁned. Even though in
practice the piles will be constructed in another construction stage than construction of
the walls, for simplicity both actions will be done in the same construction stage in this
tutorial. To redeﬁne all construction stages, follow these steps:
• Switch to the Staged construction mode.
• Check if the K0 procedure is selected as Calculation type for the initial phase. Make
sure that all the structural elements are inactive and all soil volumes are active. The
material assigned to it is Lacustrine clay.
• Select the Excavation phase in the Phases explorer.
• Make sure that the basement soil is excavated and the basement walls are active.

Figure 1.22 Partial geometry of the model in the Output
• Activate all the embedded beams.
• In the Phases explorer select the Construction phase. Make sure that all the
structural elements are active.
• In the Phases explorer select the Loading phase. Make sure that all the structural
elements and loads are active.
Calculate the project.
Save the project after the calculation.
• Select the Loading phase and view the calculation results.
• Double-click the basement ﬂoor. Select the M11 option from the Forces menu. The
results are shown in Figure 1.23.
• Adjust the legend by changing scaling settings into:
• Scaling: manual
• Minimum value: -450
• Maximum value: 550
• Number of intervals: 18
• Select the view corresponding to the deformed mesh in the Window menu.
Click the Toggle visibility button in the side toolbar.
• To view the embedded beams press Shift and keep it pressed while clicking on the
soil volume in order to hide it.
Click the Select structures button. To view all the embedded beams, press
Ctrl+Shift keys and double click on one of the piles.
• Select the option N in the Forces menu to view the axial loads in the embedded
beams. The plot is shown in Figure 1.24.

TUTORIAL MANUAL
Figure 1.23 Bending moments in the basement ﬂoor
Figure 1.24 Resulting axial forces (N) in the embedded beams

EXCAVATION IN SAND
2 EXCAVATION IN SAND
This tutorial describes the construction of an excavation pit in soft clay and sand layers.
The pit is a relatively small excavation of 12 by 20 m, excavated to a depth of 6.5 m
below the surface. Struts, walings and ground anchors are used to prevent the pit from
collapsing. After the full excavation, an additional surface load is added on one side of
the pit.
50.0 m
80.0 m
(30 20) (50 20)
(30 32) (50 32)
Strut
Ground anchors
(34 19) (41 19)
(34 12) (41 12)
4.0 m
4.0 m
4.0 m
5.0 m5.0 m5.0 m5.0 m
Figure 2.1 Top view of the excavation pit
The proposed geometry for this exercise is 80 m wide and 50 m long, as shown in Figure
2.1. The excavation pit is placed in the center of the geometry. Figure 2.2 shows a cross
section of the excavation pit with the soil layers. The clay layer is considered to be
impermeable.
Objectives:
• Using the Hardening Soil model
• Modelling of ground anchors
• Using interface features
• Deﬁning over-consolidation ratio (OCR)
• Prestressing a ground anchor
• Changing water conditions
• Selection of stress points to generate stress/strain curves
• Viewing plastic points

TUTORIAL MANUAL
z = 0
z = -1
z = -4
z = -9.5
z = -11
z = -20
Fill
Sand
Sand
Soft clay
Sheet pile walls
(62 24 -9)(18 24 -9)
Figure 2.2 Cross section of the excavation pit with the soil layers
2.1 GEOMETRY
To create the geometry model, follow these steps:
Project properties
• Start a new project.
• Enter an appropriate title for the project.
• Define the limits for the soil contour as xmin = 0, xmax = 80, ymin = 0 and ymax = 50.
2.1.1 DEFINITION OF SOIL STRATIGRAPHY
In order to define the soil layers, a borehole needs to be added and material properties
must be assigned. As all soil layers are horizontal, only a single borehole is needed.
Create a borehole at (0 0 0). The Modify soil layers window pops up.
• Add 4 layers with bottom levels at -1, -9.5, -11, -20. Set the Head in the borehole
column to -4 m.
Open the Material sets window.
• Create a new data set under Soil and interfaces set type.
• Identify the new data set as "Fill".
• From the Material model drop-down menu, select Hardening Soil model. In contrast
with the Mohr-Coulomb model, the Hardening Soil model takes into account the
difference in stiffness between virgin-loading and unloading-reloading. For a
detailed description of the Hardening Soil model, see the Chapter 6 in the Material
Models Manual.
• Define the saturated and unsaturated unit weights according to Table 2.1.
• In the Parameters tabsheet, enter values for Eref
50 , Eref
oed , Eref
ur , m, c'ref , ϕ'ref , ψ and
ν'ur according to Table 2.1. Note that Poisson's ratio is an advanced parameter.
• As no consolidation will be considered in this exercise, the permeability of the soil
will not influence the results. Therefore, the default values can be kept in the Flow
parameters tabsheet.

EXCAVATION IN SAND
Table 2.1 Material properties for the soil layers
Parameter Name Fill Sand Soft Clay Unit
General
Material model Model Hardening Soil
model
Hardening Soil
model
Hardening Soil
model
−
Drainage type Type Drained Drained Undrained A −
Unit weight above phreatic level γunsat 16.0 17.0 16.0 kN/m3
Unit weight below phreatic level γsat 20.0 20.0 17.0 kN/m3
Parameters
Secant stiffness for CD triaxial
test
Eref
50 2.2 · 104
4.3 · 104
2.0 · 103
kN/m2
Tangent oedometer stiffness Eref
oed 2.2 · 104
2.2 · 104
2.0 · 103
kN/m2
Unloading/reloading stiffness Eref
ur 6.6 · 104
1.29 · 105
1.0 · 104
kN/m2
Power for stress level
dependency of stiffness
m 0.5 0.5 1.0 −
Cohesion c'ref 1 1 5 kN/m2
Friction angle ϕ' 30.0 34.0 25.0 ◦
Dilatancy angle ψ 0.0 4.0 0.0 ◦
Poisson's ratio ν'ur 0.2 0.2 0.2 −
Interfaces
Interface strength − Manual Manual Manual −
Interface reduction factor Rinter 0.65 0.7 0.5 −
Initial
K0 determination − Automatic Automatic Automatic −
Lateral earth pressure coefficient K0 0.5000 0.4408 0.7411 −
Over-consolidation ratio OCR 1.0 1.0 1.5 −
Pre-overburden pressure POP 0.0 0.0 0.0 −
• In the Interfaces tabsheet, select Manual in the Strength box and enter a value of
0.65 for the parameter Rinter . This parameter relates the strength of the interfaces to
the strength of the soil, according to the equations:
ci = Rinter csoil and tanϕi = Rinter tanϕi ≤ tanϕsoil
Hence, using the entered Rinter -value gives a reduced interface friction and interface
cohesion (adhesion) compared to the friction angle and the cohesion in the adjacent
soil.
Hint: When the Rigid option is selected in the Strength drop-down, the interface
has the same strength properties as the soil (Rinter = 1.0).
» Note that a value of Rinter < 1.0, reduces the strength as well as the stiffness
of the interface (Section 6.1.6 of the Reference Manual).
• In the Initial tabsheet, define the OCR-value according to Table 2.1.
• Click OK to close the window.
• In the same way, define the material properties of the "Sand" and "Soft Clay"
materials as given by Table 2.1.
• After closing the Material sets window, click the OK button to close the Modify soil
layers window.
• In the Soil mode right click on the upper soil layer. In the appearing right hand

TUTORIAL MANUAL
mouse button menu, select the Fill option in the Set material menu.
• In the same way assign the Soft Clay material to the soil layer between y = -9.5 m
and y = -11.0 m.
• Assign the Sand material to the remaining two soil layers.
• Proceed to the Structures mode to deﬁne the structural elements.
Hint: The Tension cut-off option is activated by default at a value of 0 kN/m2
. This
option is found in the Advanced options on the Parameters tabsheet of the
Soil window. Here the Tension cut-off value can be changed or the option
can be deactivated entirely.
The creation of sheet pile walls, walings, struts and surface loads and ground anchors is
described below.
Create a surface between (30 20 0), (30 32 0), (50 32 0) and (50 20 0).
Extrude the surface to z = -1, z = -6.5 and z = -11.
• Right-click on the deepest created volume (between z = 0 and z = -11) and select
the Decompose into surfaces option from the appearing menu.
• Delete the top surfaces (2 surfaces). An extra surface is created as the volume is
decomposed.
• Hide the excavation volumes (do not delete). The eye button in the Model explorer
and the Selection explorer trees can be used to hide parts of the model and simplify
the view. A hidden project entity is indicated by a closed eye.
Click the Create structure button.
Create beams (walings) around the excavation circumference at level z = −1m.
Press the Shift key and keep it pressed while moving the mouse cursor in the
-z-direction. Stop moving the mouse as the z− coordinate of the mouse cursor is
−1 in the cursor position indicator. Note that as you release the Shift key, the
z-coordinate of the cursor location does not change. This is an indication that you
can draw only on the xy-plane located at z = -1.
• Click on (30 20 -1), (30 32 -1), (50 32 -1), (50 20 -1), (30 20 -1) to draw the walings.
Click on the right mouse button to stop drawing walings.
Create a beam (strut) between (35 20 -1) and (35 32 -1). Press Esc to end deﬁning
the strut.
Create data sets for the walings and strut according to Table 2.2 and assign the
materials accordingly.
Copy the strut into a total of three struts at x = 35 (existing), x = 40, and x = 45.

EXCAVATION IN SAND
Table 2.2 Material properties for the beams
Parameter Name Strut Waling Unit
Material type Type Elastic Elastic −
Young's modulus E 2.1 · 108
2.1 · 108
kN/m2
Unit weight γ 78.5 78.5 kN/m3
Cross section area A 0.007367 0.008682 m2
Moment of Inertia I2 5.073 · 10−5
3.66 · 10−4
m4
I3 5.073 · 10−5
1.045 · 10−4
m4
Modelling ground anchors
In PLAXIS 3D ground anchors can be modelled using the Node-to-node anchor and the
Embedded beam options as described in the following:
First the ungrouted part of the anchor is created using the Node-to-node anchor
feature. Start creating a node-to-node anchor by selecting the corresponding button
in the options displayed as you click on the Create structure button.
• Click on the command line and type "30 24 -1 21 24 -7 " . Press Enter and Esc to
create the ungrouted part of the first ground anchor.
• Create a node-to-node anchor between the points (50 24 -1) and (59 24 -7).
The grouted part of the anchor is created using the Embedded beam option. Create
embedded beams between (21 24 -7) and (18 24 -9) and between (59 24 -7) and (62
24 -9). Set the Behaviour to Grout body (Section 5.8.4 of the Reference Manual).
Create a data set for the embedded beam and a data set for the node-to-node
anchor according to Table 2.3 and Table 2.4 respectively. Assign the data sets to the
node-to-node anchors and to the embedded beams.
Table 2.3 Material properties for the node-to-node anchors
Parameter Name Node-to-node anchor Unit
Material type Type Elastic −
Axial stiffness EA 6.5·105
kN
Table 2.4 Material properties for the embedded beams (grout body)
Parameter Name Grout Unit
kN/m2
Unit weight γ 24 kN/m3
Beam type − Predefined −
Predefined beam type − Massive circular beam −
Diameter Diameter 0.14 m
Axial skin resistance Type Linear −
Skin resistance at the top of the
embedded beam
Tskin,start,max 200 kN/m
Skin resistance at the bottom of the
embedded beam
Tskin,end,max 0.0 kN/m
Base resistance Fmax 0.0 kN
Hint: The colour indicating the material set assigned to the entities in project can
be changed by clicking on the Colour box of the selected material set and
selecting a colour from the Colour part of the window.

TUTORIAL MANUAL
The remaining grouted anchors will be created by copying the defined grouted anchor.
Click on the Select button and click on all the elements composing both of the
ground anchors keeping the Ctrl key pressed.
Use the Create array function to copy both ground anchors (2 embedded beams + 2
node-to-node anchors) into a total of 4 complete ground anchors located at y = 24
and y = 28 by selection the 1D, in y direction option in the Shape drop-down menu
and define the Distance between columns as 4 m.
Multi-select all parts of the ground anchors (8 entities in total). While all parts are
selected and the Ctrl key is pressed, click the right mouse button and select the
Group from the appearing menu.
In the Model explorer tree, expand the Groups subtree by clicking on the (+) in front
of the groups.
• Click the Group_1 and rename it to "GroundAnchors".
Hint: The name of the entities in the project should not contain any space or
special character except "_" .
To define the sheet pile walls and the corresponding interfaces, follow these steps:
Select all four vertical surfaces created as the volume was decomposed. Keeping
the Ctrl key pressed, click the right mouse button and select the Create plate option
from the appearing menu.
Create a data set for the sheet pile walls (plates) according to Table 2.5. Assign the
data sets to the four walls.
• As all the surfaces are selected, assign both positive and negative interfaces to
them using the options in the right mouse button menu.
Hint: The term 'positive' or 'negative' for interfaces has no physical meaning. It
only enables distinguishing between interfaces at each side of a surface.
Table 2.5 Material properties of the sheet pile walls
Parameter Name Sheet pile wall Unit
Type of behaviour Type Elastic, non-isotropic −
Thickness d 0.379 m
Weight γ 2.55 kN/m3
Young's modulus E1 1.46 · 107
kN/m2
E2 7.3 · 105
kN/m2
Poisson's ratio ν12 0.0 −
Shear modulus G12 7.3 · 105
kN/m2
G13 1.27 · 106
kN/m2
G23 3.82 · 105
kN/m2
Non-isotropic (different stiffnesses in two directions) sheet pile walls are defined. The
local axis should point in the correct direction (which defines which is the 'stiff' or the 'soft'
direction). As the vertical direction is generally the stiffest direction in sheet pile walls,

EXCAVATION IN SAND
local axis 1 shall point in the z-direction.
In the Model explorer tree expand the Surfaces subtree, set AxisFunction to Manual
and set Axis1z to −1. Do this for all the pile wall surfaces.
Create a surface load defined by the points: (34 19 0), (41 19 0), (41 12 0), (34 12
0). The geometry is now completely defined.
Hint: The first local axis is indicated by a red arrow, the second local axis is
indicated by a green arrow and the third axis is indicated by a blue arrow.
More information related to the local axes of plates is given in the Reference
Manual.
2.2 MESH GENERATION
• Click on the Mesh tab to proceed to the Mesh mode.
• Select the surface representing the excavation. In the Selection explorer set the
value of Coarseness factor to 0.25.
Set the element distribution to Coarse. Uncheck the box for Enhanced mesh
refinements. Generate the mesh.
View the mesh. Hide the soil in the model to view the embedded beams.
Hint: The Enhanced mesh refinements are automatically used in mesh generation.
More information is available in Section 7.1.4 of Reference Manual.
2.3 PERFORMING CALCULATIONS
The calculation consists of 6 phases. The initial phase consists of the generation of the
initial stresses using the K0 procedure. The next phase consists of the installation of the
sheet piles and a first excavation. Then the walings and struts will be installed. In phase
3, the ground anchors will be activated and prestressed. Further excavation will be
performed in the phase after that. The last phase will be the application of the additional
load next to the pit.
• Click on the Staged construction tab to proceed with definition of the calculation
phases.
• The initial phase has already been introduced. Keep its calculation type as K0
procedure. Make sure all the soil volumes are active and all the structural elements
are inactive.
Add a new phase (Phase_1). The default values of the parameters will be used for

TUTORIAL MANUAL
this calculation phase.
• Deactivate the ﬁrst excavation volume (from z = 0 to z = −1).
• In the Model explorer, activate all plates and interfaces by clicking on the checkbox
in front of them. The active elements in the project are indicated by a green check
mark in the Model explorer.
• In the Model explorer activate all the beams.
• In the Model explorer activate the GroundAnchors group.
Select one of the node-to-node anchors.
In the Selection explorer expand the node-to node anchor features.
• Click on the Adjust prestress checkbox. Enter a prestress force of 200 kN (Figure
2.3).
• Do the same for all the other node-to-node anchors.
Figure 2.3 Node-to-node anchor in the Selection explorer
Add another phase (Phase_4). The default values of the parameters will be used for
Select the soil volume to be excavated in this phase (between z = −1 and
z = −6.5).
In the Selection explorer under WaterConditions feature, click on the Conditions and
select the Dry option from the drop-down menu.
Figure 2.4 Water conditions in the Selection explorer

EXCAVATION IN SAND
• Deactivate the volume to be excavated (between z = -1 and z = -6.5).
• Hide the soil and the plates around the excavation.
Select the soil volume below the excavation (between z = -6.5 and z = -9.5).
In Selection explorer under WaterConditions feature,
• click Conditions and select Head from the drop-down menu. Enter zref = -6.5 m.
Select the soft clay volume below the excavation.
• Set the water conditions to Interpolate.
Preview this calculation phase.
Click the Vertical cross section button in the Preview window and deﬁne the cross
section by drawing a line across the excavation.
• Select the psteady option from the Stresses menu.
Hint: Hold Shift key when drawing to get a straight line.
Display the contour lines for steady pore pressure distribution. Make sure that the
Legend option is checked in View menu. The steady state pore pressure distribution
is displayed in Figure 2.5. Scroll the wheel button of the mouse to zoom in or out to
get a better view.
• Change the legend settings to:
• Scaling: manual
Figure 2.5 Preview of the steady state pore pressures in Phase_4 in a cross section
• Click on the Close button to return to the Input program.
Add another phase (Phase_5). The default values of the parameters will be used for
• Activate the surface load and set σz = -20 kN/m2
.

TUTORIAL MANUAL
Defining points for curves
Before starting the calculation process, some stress points next to the excavation pit and
loading are selected to plot a stress strain curve later on.
Click the Select points for curves button. The model and Select points window will
be displayed in the Output program.
• Define (37.5 19 -1.5) as Point-of-interest coordinates.
Hint: The visualization settings can be changed from the menu. For more
information refer Section 8.5.2 of Reference Manual .
• Click the Search closest button. The number of the closest node and stress point
will be displayed.
• Click the checkbox in front of the stress point to be selected. The selected stress
point will be shown in the list.
• Select also stress points near the coordinates (37.5 19 -5), (37.5 19 -6) and (37.5 19
-7) and close the Select points window.
• Click the Update button to close the Output program.
Start the calculation process.
Save the project when the calculation is finished.
Hint: Instead of selecting nodes or stress points for curves before starting the
calculation, points can also be selected after the calculation when viewing
the output results. However, the curves will be less accurate since only the
results of the saved calculation steps will be considered.
» To plot curves of structural forces, nodes can only be selected after the
calculation.
» Nodes or stress points can be selected by just clicking them. When moving
the mouse, the exact coordinates of the position are given in the cursor
location indicator bar at the bottom of the window.
2.4 VIEWING THE RESULTS
After the calculations, the results of the excavation can be viewed by selecting a
calculation phase from the Phases tree and pressing the View calculation results button.
Select the final calculation phase (Phase_5) and click the View calculation results
button. The Output program will open and will show the deformed mesh at the end
of the last phase.
• The stresses, deformations and three-dimensional geometry can be viewed by
selecting the desired output from the corresponding menus. For example, choose
Plastic points from the Stresses menu to investigate the plastic points in the model.

EXCAVATION IN SAND
• In the Plastic points window, Figure 2.6, select all the options except the Elastic
points and the Show only inaccurate points options. Figure 2.7 shows the plastic
points generated in the model at the end of the ﬁnal calculation phase.
Figure 2.6 Plastic points window
Figure 2.7 Plastic points at the end of the ﬁnal phase
The graph will now show the major principal strain against the major principal stress.
Both values are zero at the beginning of the initial conditions. After generation of the
initial conditions, the principal strain is still zero whereas the principal stress is not zero
anymore. To plot the curves of all selected stress points in one graph, follow these steps:
• Select Add curve → From current project from right mouse button menu.
• Generate curves for the three remaining stress nodes in the same way.
The graph will now show the stress-strain curves of all four stress points (Figure 2.9). To
see information about the markers, make sure the Value indication option is selected
from the View menu and hold the mouse on a marker for a while. Information about the
coordinates in the graph, the number of the point in the graph, the number of the phase
and the number of the step is given. Especially the lower stress points show a
considerable increase in the stress when the load is applied in the last phase.
To create a stress path plot for stress node (37.5 19 -1.5) follow these steps:

TUTORIAL MANUAL
Figure 2.8 Curve generation window
Figure 2.9 Stress - Strain curve
Hint: To re-enter the Curve generation window (in the case of a mistake, a desired
regeneration or a modiﬁcation), the Curve settings option from the Format
menu can be selected. As a result the Curves settings window appears, on
which the Regenerate button should be clicked.
» The Chart settings option in the Format menu may be used to modify the
settings of the chart.
• Create a new chart.
• In the Curves generation window, select node (37.5 19 -1.5) from the drop-down
menu of the x−axis of the graph and σ'yy under Cartesian effective stresses.
• Select node (37.5 19 -1.5) from the drop-down menu of the y−axis of the graph.
Select σ'zz under Cartesian effective stresses.

EXCAVATION IN SAND
• Click OK to conﬁrm the input (Figure 2.10).
Figure 2.10 Vertical effective stress (σ'zz ) versus horizontal effective stress (σ'yy ) at stress node
located near (37.5 19 -1.5)

TUTORIAL MANUAL
3 LOADING OF A SUCTION PILE
In this tutorial a suction pile in an offshore foundation will be considered. A suction pile is
a hollow steel pile with a large diameter and a closed top, which is installed in the seabed
by pumping water from the inside. The resulting pressure difference between the outside
and the inside is the driving force behind this installation.
In this exercise, the length of the suction pile is 10 m and the diameter is 5.0 m. An
anchor chain is attached on the side of the pile, 7 m from the top. The water depth at the
considered location is 50 m above the ground. The soil consists of clay but because of
the short duration of the load, an undrained stress analysis with undrained strength
parameters will be performed (Section 6.2 of the Reference Manual).
This exercise will investigate the displacement of the suction pile under working load
conditions. Four different angles of the working load will be considered. The installation
process itself will not be modelled. Only one symmetric half will be modelled. The
geometry for the problem is sketched in Figure 3.1.
Objectives:
• Using shape designer
• Using rigid body objects
• Undrained effective stress analysis with undrained strength parameters
• Undrained shear strength increasing with depth
• Copying material data sets
• Changing settings in Output
• Helper objects for local mesh refinements
z = -6.5 m
z = -7.0 m
z = -7.5 m
z = -10 m
z
x
5.0 m
α
Figure 3.1 Geometry of the suction pile
3.1 GEOMETRY
An area of 30 m wide and 60 m long with half of the suction pile will be modelled in this
example. With these dimensions the model is sufficiently large to avoid any influence
from the model boundaries.

LOADING OF A SUCTION PILE
Project properties
To define the geometry for this exercise, follow these steps:
• Start the Input program and select New project from the Create/Open project dialog
box.
• Enter an appropriate title for the exercise.
• Keep the standard units and set the model dimensions to xmin = -30 m, xmax = 30 m,
ymin = 0 m, ymax = 30 m.
• Click OK.
In the current example only one horizontal soil layer is present. A single borehole is
sufficient to define it.
Create a borehole at (0 0 0). The Modify soil layers pops up.
• In the Modify soil layers window add a soil layer with top boundary at z = 0 m and
bottom boundary at z = -30 m.
• The water depth at the considered location is 50 m. This would imply that the head
is set to 50 m, but the results will be equal as long as the whole geometry is below
the water level (the water above the ground is a total load and not an effective load).
Hence, a head of 1.0 m is sufficient. Set the head to 1.0 m.
Open the Material sets window and create the data sets given in Table 3.1. In the
Parameters tabsheet deselect the Tension cut-off option in the advanced
parameters for strength. In this exercise, the permeability of the soil will not
influence the results. Instead of using effective strength properties, the cohesion
parameter will be used in this example to model undrained shear strength.
Advanced parameters can be entered after expanding the Advanced data tree in the
Parameters tabsheet.
Hint: The Interface data set can be quickly created by copying the 'Clay' data set
and changing the Rinter value.
• Assign the 'Clay' material data set to the soil layer and close the Material sets
window.
The suction pile is modelled in the Structures mode as half a cylindrical surface and this
is then defined as a rigid body.
Create a suction pile
In the Structures mode the suction pile as a rigid body will be defined. This is done by
creating a polycurve at the soil surface and extruding it downward.
Click the Create polycurve button in the side toolbar.

TUTORIAL MANUAL
Table 3.1 Material properties of the clay layer and its interface
Parameter Name Clay Interface Unit
General
Material model Model Mohr-Coulomb Mohr-Coulomb −
Drainage type Type Undrained B Undrained B −
Soil weight γunsat , γsat 20 20 kN/m3
Parameters
Young's modulus E' 1000 1000 kN/m2
Poisson's ratio ν' 0.35 0.35 −
Shear strength su,ref 1.0 1.0 kN/m2
Friction angle ϕu 0.0 0.0 ◦
Dilatancy angle ψ 0.0 0.0 ◦
Increase in stiffness E'inc 1000 1000 kN/m2
/m
Reference level zref 0.0 0.0 m
Increase in cohesion su,inc 4.0 4.0 kN/m2
/m
Reference level zref 0.0 0.0 m
Tension cut-off − Inactive Inactive −
Interfaces
Interface strength − Manual Rigid −
Interface strength reduction Rinter 0.7 1.0 −
Initial
K0 determination − Manual Manual −
Lateral earth pressure coeff. K0,x , K0,y 0.5 0.5 −
• Click at (2.5 0 0) on the drawing area to deﬁne the insertion point. The Shape
designer window pops up.
Hint: From the Options menu, choose Visualization settings. Set the Intervals to 2,
while leaving the Spacing to 1 m. This allows to move the mouse with 0.5 m
interval.
• In the General tabsheet, the default option Free is valid for Shape.
• The polycurve is drawn in the xy-plane (Figure 3.2). Hence the default orientation
axes are valid for this example. For more information refer to Section 5.9.2 of
Reference Manual.
In the Segments tabsheet, click on the Add section on the top toolbar.
• Set the Segment type to Arc, the Relative start angle to 90◦
, the Radius to 2.5 m
and the Segment angle to 180◦
(Figure 3.3).
• Click OK to add the polycurve to the geometry and to close the Shape desginer.
Click on the created polycurve and select the Extrude object and set the z value to
-10 m.
• Right click the created surface, and select Create positive interface to create a
positive interface for the suction pile. Similarly create a negative interface for the
surface.
• Right click the polycurve and select Close from the appearing menu. Further, right
click the closed polycurve and select Create surface. This creates the top surface of

Figure 3.2 General tabsheet of the Shape designer
Figure 3.3 Segment tabsheet of the Shape designer
the suction pile.
To create the suction pile, the Rigid body functionality is used. For more information on
Rigid bodies, refer to Section 5.8.8 of the Reference Manual.
• Right click the top surface and create a negative interface.

TUTORIAL MANUAL
• Select the Interfaces in the Model explorer. In the Selection explorer tree, select
Custom for the Material mode from the dropdown menu.
• Select Interface for the Material from the dropdown menu (Figure 3.4).
Figure 3.4 Interface material assignment in Selection explorer
• Multi-select the top and the curved surface. Right click on the selected surfaces and
select the option Create rigid body from the appearing menu (Figure 3.5).
Figure 3.5 Rigid body creation
• In the Selection explorer, set the reference point as (2.5 0 -7) for the rigid bodies by
assigning the values to xref , yref and zref .
• Set the Translation conditiony to Displacement, the Rotation conditionx and Rotation
conditionz to Rotation . Their corresponding values are uy = φx = φz = 0 (Figure
3.6).
Create helper objects for local mesh reﬁnements
A surface is created around the suction pile to achieve better mesh reﬁnements. This is
done by creating a circular surface around the suction pile using the Shape designer.

Figure 3.6 Rigid body in the Selection explorer
Click the Create polycurve button in the side toolbar and click on (7.5 0 0) in the
drawing area.
• In the General tabsheet the default option for the shape (Free) and the default
orientation axes (x-axis, y-axis) are valid for this polycurve.
In the Segments tabsheet, click on the Add segment on the top toolbar. Set the
Segment type to Arc, Relative start angle to 90◦
, Radius to 7.5 m and Segment
angle to 180◦
.
Click Close polycurve from the top toolbar to close the polycurve.
• Click OK to add the polycurve to the geometry and to close the Shape desginer.
Click on the created polycurve and select the Extrude object and set the z value to
-15 m.
• Multi select the two created polycurves, right click and select Delete from the
appearing menu (Figure 3.7).
The geometry of the project is deﬁned. A screenshot of the geometry is shown in Figure
3.8.

TUTORIAL MANUAL
Figure 3.7 Deleting the two created polycurves
Figure 3.8 Geometry of the suction pile
3.2 MESH GENERATION
In order to generate the mesh:
• Hide the soil volume around the suction pile. Multi-select the suction pile, the
surface around the suction pile and the top surface of the suction pile.

• In the Selection explorer set the value of Coarseness factor to 0.25.
The element distribution is Medium. Generate the mesh.
• Proceed to the Staged construction mode.
The calculation for this exercise will consist of 6 phases. These are the determination of
initial conditions, the installation of the suction pile and four different load conditions. The
effect of the change of the load direction while keeping the magnitude unchanged will be
analysed.
• Click on the Staged construction tab to proceed with the deﬁnition of the calculation
phases. Keep the calculation type of the Initial phase to K0 procedure. Ensure that
all the structures and interfaces are switched off.
Add a new calculation phase and rename it as 'Install pile'.
• For this phase, we use the option of Ignore undrained behaviour.
• Activate all the rigid bodies and interfaces in the project.
Add a new phase and rename it as 'Load pile 30 degrees'.
• In the Phases window, check the Reset displacements to zero checkbox in the
Deformation control parameters subtree.
• Set the Solver type to Paradiso (multicore direct) to enable a faster calculation for
this particular project.
• In the Numerical control parameters subtree uncheck the Use default iter
parameters checkbox, which allows you to change advanced settings.
• Set the Max load fraction per step to 0.1.
• Click on the Rigid bodies in the Model explorer.
• In the Selection explorer tree, set Fx = 1949 kN and Fz = 1125 kN for the selected
rigid bodies.
• Deﬁne the remaining phases according to the information in Table 3.2. For each
phase select the Reset displacements to zero option and set Solver type to Pardiso
(multicore direct) and Max load fraction per step to 0.1.
The order of the phases is indicated in the Phases explorer (Figure 3.9). Calculation of
Phase_1 starts after the calculation of Initial phase is completed. The calculation of the
remaining phases starts after the calculation of the pile installation phase is completed.
Table 3.2 Load information at the chain attachment point
Phase Start from phase Fx Fz
Load pile 30 degrees [Phase_2] Phase_1 1949 kN 1125 kN

TUTORIAL MANUAL
To view the results:
• View the results of the last calculation phase. The deformed mesh of the whole
geometry will be shown. In particular, the displacements of the suction pile itself are
of interest.
Select the shadings representation and rotate the model such that the x−axis is
perpendicular to the screen.
• If the axes are not visible, select this option from the View menu. It is quite clear that
the point force acting on the pile does not disturb the displacement field locally
indicating that the pile is sufficiently thick here.
• In the same manner, the total displacements of the suction pile under a different
direction of the load can be inspected by selecting the appropriate phase from the
drop-down menu. In particular, Phase_2 is of interest, as in this phase the horizontal
part of the load will have the largest value (Figure 3.10).
Hint: As an alternative for true 3D finite element calculations, the online tool
SPCalc from XG-Geotools provides a quick solution for multiple bearing
capacity calculations of suction piles. For more information see
www.xg-geotools.com.

Figure 3.10 Total displacement of the suction pile at the end of Phase_2

TUTORIAL MANUAL
4 CONSTRUCTION OF A ROAD EMBANKMENT
The construction of an embankment on soft soil with a high groundwater level leads to an
increase in pore pressure. As a result of this undrained behaviour, the effective stress
remains low and intermediate consolidation periods have to be adopted in order to
construct the embankment safely. During consolidation the excess pore pressures
dissipate so that the soil can obtain the necessary shear strength to continue the
construction process.
This tutorial concerns the construction of a road embankment in which the mechanism
described above is analysed in detail. In the analysis two new calculation options are
introduced, namely a consolidation analysis and the calculation of a safety factor by
means of a safety analysis (phi/c-reduction). It also involves the modelling of drains to
speed up the consolidation process.
12 m12 m 16 m
4 m
3 m
3 m
road embankment
peat
clay
dense sand
Figure 4.1 Situation of a road embankment on soft soil
Objectives:
• Modelling drains
• Consolidation analysis
• Change of permeability during consolidation
• Safety analysis (phi-c reduction)
4.1 GEOMETRY
Figure 4.1 shows a cross section of a road embankment. The embankment is 16 m wide.
The slopes have an inclination of 1: 3. The problem is symmetric, so only one half is
modelled (in this case the right half is chosen). A representative section of 2 m is
considered in the project. The embankment itself is composed of loose sandy soil. The
subsoil consists of 6 m of soft soil. The upper 3 m of this soft soil layer is modelled as a
peat layer and the lower 3 m as clay. The phreatic level is located 1 m below the original
ground surface. Under the soft soil layers there is a dense sand layer of which 4 m are
considered in the model.
• Start the Input program and select Start a new project from the Quick select dialog
box.
• In the Project tabsheet of the Project properties window, enter an appropriate title.
• Keep the default units and set the model dimensions to xmin = 0, xmax = 60, ymin = 0
and ymax = 2.

CONSTRUCTION OF A ROAD EMBANKMENT
The soil layers comprising the embankment foundation are defined using a borehole. The
embankment layers are defined in the Structures mode.
Create a borehole by clicking at (0 0 0). The Modify soil layers window pops up.
• Define three soil layers as shown in Figure 4.2.
• The water level is located at z = -1 m. In the borehole column specify a value of -1 to
Head.
• Create soil material data sets according to Table 4.1 and assign them to the
corresponding layers in the borehole (Figure 4.2).
• Close the Modify soil layers window and proceed to the Structures mode to define
the structural elements.
Figure 4.2 Soil layer distribution
Hint: The initial void ratio (einit ) and the change in permeability (ck ) should be
defined to enable the modelling of a change in the permeability due to
compression of the soil. This option is recommended when using advanced
models.

TUTORIAL MANUAL
Table 4.1 Material properties of the road embankment and subsoil
Parameter Name Embankment Sand Peat Clay Unit
General
Material model Model Hardening soil Hardening soil Soft soil Soft soil -
Drainage type Type Drained Drained Undr. (A) Undr. (A) -
Soil unit weight above
phreatic level
γunsat 16 17 8 15 kN/m3
Soil unit weight below
phreatic level
γsat 19 20 12 18 kN/m3
Initial void ratio einit 0.5 0.5 2.0 1.0 -
Parameters
Secant stiffness in
standard drained
triaxial test
Eref
50 2.5· 104
3.5· 104
- - kN/m2
Tangent stiffness for
primary oedometer
loading
Eref
oed 2.5· 104
3.5· 104
- - kN/m2
Unloading / reloading
stiffness
Eref
ur 7.5· 104
1.05· 105
- - kN/m2
Power for stress-level
dependency of stiffness
m 0.5 0.5 - - -
Modified compression
index
λ∗
- - 0.15 0.05 -
Modified swelling index κ∗
- - 0.03 0.01 -
Cohesion cref ' 1.0 0.0 2.0 1.0 kN/m2
Friction angle ϕ' 30.0 33.0 23.0 25.0 ◦
Dilatancy angle ψ 0.0 3.0 0.0 0.0 ◦
Advanced: Set to
default
- Yes Yes Yes Yes -
Groundwater
Data set - USDA USDA USDA USDA -
Model - Van
Genuchten
Van
Genuchten
Van
Genuchten
Van
Genuchten
-
Soil type - Loamy sand Sand Clay Clay -
< 2µm - 6.0 4.0 70.0 70.0 %
2µm − 50µm - 11.0 4.0 13.0 13.0 %
50µm − 2mm - 83.0 92.0 17.0 17.0 %
Use defaults - From data set From data set None From data set -
Horizontal permeability
(x-direction)
kx 3.499 7.128 0.1 0.04752 m/day
(y-direction)
ky 3.499 7.128 0.1 0.04752 m/day
Vertical permeability kz 3.499 7.128 0.05 0.04752 m/day
Change of permeability ck 1· 1015
1· 1015
1.0 0.2 -
Interfaces
Interface strength − Rigid Rigid Rigid Rigid -
Strength reduction
factor
Rinter 1.0 1.0 1.0 1.0 -
Initial
K0 determination − Automatic Automatic Automatic Automatic -
Over-consolidation ratio OCR 1.0 1.0 1.0 1.0 -
Pre-overburden
pressure
POP 0.0 0.0 5.0 0.0 kN/m2
4.1.2 DEFINITION OF EMBANKMENT AND DRAINS
The embankment and the drains are defined in the Structures mode. To define the
embankment layers:

Reorientate the model such that the front view is displayed by clicking the
corresponding button in the toolbar.
Create a surface by defining points at (0 0 0), (0 0 4), (8 0 4) and (20 0 0).
Create a line passing through (0 0 2) and (14 0 2) to define the embankment layers.
Select both the created line and surface by keeping the Ctrl key pressed while
clicking them in the model.
Click the Extrude object button. Assign a value of 2 to the y-component of the
extrusion vector as shown in Figure 4.3 and click Apply.
Figure 4.3 Extrusion window
• Delete the surface and the line with its corresponding points that were created
before the extrusion.
• Right-click the volume created by extrusion and point to the Soil_4 option in the
appearing menu.
• A new menu is displayed. Point to the Set material option and select Embankment.
In this project the effect of the drains on the consolidation time will be investigated by
comparing the results with a case without drains. Drains will only be active for the
calculation phases in the case with drains.
Drains are arranged in a square pattern, having a distance of 2 m between two
consecutive drains in a row (or column). Only one row of drains will be considered in this
tutorial. To create the drain pattern:
Click the Create hydraulic conditions button in the side toolbar.
Click the Create line drain button in the appearing menu. Define a line drain in the
model between points (1 1 0) and (1 1 -6).
Click the Create array button to define the drain pattern.
• In the Create array window select the 1D, in x direction in the Shape drop-down
menu and specify the pattern as shown in Figure 4.4.

TUTORIAL MANUAL
Figure 4.4 Settings of the drain pattern
The model geometry is shown in Figure 4.5.
Figure 4.5 Model geometry
4.2 MESH GENERATION
• Proceed to the Mesh mode.
• Select all volumes, including the embankment and in the Selection explorer set the
Coarseness factor to 0.3.
Click the Generate mesh button. Set the element distribution to Coarse.
View the generated mesh. The resulting mesh is shown in Figure 4.6.

Figure 4.6 The generated mesh
The embankment construction process will be considered twice. In the first calculation
the drains will not be considered.
Initial phase
In the initial situation the embankment is not present. Therefore, the corresponding soil
volumes are deactivated in the initial phase. The K0 procedure can be used to calculate
the initial stresses. The initial water pressures are fully hydrostatic and based on a
general phreatic level defined by the Head value assigned to the boreholes. For the Initial
phase, the Phreatic option is selected for the pore pressure calculation type and the
Global water level is set to BoreholeWaterlevel_1 corresponding to the water level
defined by the heads specified for the boreholes.
The boundary conditions for flow can be specified in the Model conditions subtree in the
Model explorer. In the current situation the left vertical boundary (Xmin) must be closed
because of symmetry, so horizontal flow should not occur. The bottom is open because
the excess pore pressures can freely flow into the deep and permeable sand layer. The
upper boundary is obviously open as well. The view of the GroundwaterFlow subtree
after the definition is given in Figure 4.7.
4.3.1 CONSOLIDATION ANALYSIS
A consolidation analysis introduces the dimension of time in the calculations. In order to
correctly perform a consolidation analysis a proper time step must be selected. The use
of time steps that are smaller than a critical minimum value can result in stress
oscillations. The consolidation option in PLAXIS allows for a fully automatic time stepping
procedure that takes this critical time step into account. Within this procedure there are
three main possibilities for the Loading type parameter:
1. Consolidate for a predefined period, including the effects of changes to the active
geometry (Staged construction).
2. Consolidate until all excess pore pressures in the geometry have reduced to a
predefined minimum value (Minimum excess pore pressure).

TUTORIAL MANUAL
Figure 4.7 Boundary conditions for groundwater flow
3. Consolidate until the soil has reached a specified degree of consolidation (Degree of
consolidation).
Consolidation process - No drains
The embankment construction is divided into two phases. After the first construction
phase, a consolidation period of 30 days is introduced to allow the excess pore pressures
to dissipate. After the second construction phase another consolidation period is
introduced from which the final settlements may be determined.
To define the calculation phases, follow these steps:
Phase 1:
Click the Add phase button to introduce the first construction phase.
In the General subtree select the Consolidation option in the Calculation type
drop-down menu.
The Loading type is by default set to Staged construction. This option will be used
for this phase.
The Phreatic option is automatically selected for the pore pressure calculation type.
Note that the global water level for a calculation phase can be defined in the Water
subtree available under the Model conditions in the Model explorer.
• Specify a value of 2 days to the Time interval and click OK to close the Phases
window.
• In the Staged construction mode activate the first part of the embankment.
Phase 2: The second phase is also a Consolidation analysis. In this phase no changes
to the geometry are made as only a consolidation analysis to ultimate time is required.
Click the Add phase button to introduce the next calculation phase.

Define the calculation type as Consolidation.
• Specify a value of 30 days to the Time interval. The default values of the other
parameters are used for this phase.
Phase 3:
• Specify a value of 1 day to the Time interval. The default values of the other
parameters are used.
• In the Staged construction mode activate the second part of the embankment.
Phase 4: The fourth phase is a Consolidation analysis to a minimum excess pore
pressure.
Select the Minimum excess pore pressure option in the Loading type drop-down
menu. The default value for the minimum pressure (|P-stop| = 1.0 kN/m2
) as well as
the default values for other parameters are used.
The definition of the calculation phases is complete.
Before starting the calculation, click the Select points for curves button and select
the following points: As the first node, select the toe of the embankment at (20 0 0).
The second node will be used to plot the development (and decay) of excess pore
pressures. To this end, a point somewhere in the middle of the soft soil layers is
needed, close to (but not actually on) the left boundary (e.g. (0.7 0 -3)).
Start the calculation.
During a consolidation analysis the development of time can be viewed in the upper part
of the calculation info window (Figure 4.8). In addition to the multipliers, a parameter
Pmax occurs, which indicates the current maximum excess pore pressure. This
parameter is of interest in the case of a Minimum excess pore pressure consolidation
analysis, where all pore pressures are specified to reduce below a predefined value.

TUTORIAL MANUAL
Figure 4.8 Calculation progress displayed in the Active tasks window
After the calculation has ﬁnished, select the third phase and click the View
calculation results button. The Output window now shows the deformed mesh after
the undrained construction of the ﬁnal part of the embankment (Figure 4.9). Considering
the results of the third phase, the deformed mesh shows the uplift of the embankment toe
and hinterland due to the undrained behaviour.
Figure 4.9 Deformed mesh after undrained construction of embankment (Phase 3)
• In the Deformations menu select the Incremental displacements → |∆u|.
Select the Arrows option in the View menu or click the corresponding button in the
toolbar to display the results arrows.
On evaluating the total displacement increments, it can be seen that a failure mechanism
is developing (Figure 4.10).
• Click Ctrl + 7 to display the developed excess pore pressures (see Appendix C of
Reference Manual for more shortcuts). They can be displayed by selecting the

Figure 4.10 Displacement increments after undrained construction of embankment
corresponding option in the side menu displayed as the Pore pressures option is
selected in the Stresses menu.
Click the Center principal directions. The principal directions of excess pressures
are displayed at the center of each soil element. The results are displayed in Figure
4.11. It is clear that the highest excess pore pressure occurs under the embankment
centre.
Figure 4.11 Excess pore pressures after undrained construction of embankment (Phase 3)
• Select Phase 4 in the drop down menu.
Deﬁne a vertical cross section passing through (0 1) and (60 1).
Click the Contour lines button in the toolbar to display the results as contours.
• In the View menu select the Viewpoint option. The corresponding window pops up.
• In the Viewpoint window select the Front view option as shown in Figure 4.12.
Use the Draw scanline button or the corresponding option in the View menu to
deﬁne the position of the contour line labels.
It can be seen that the settlement of the original soil surface and the embankment
increases considerably during the fourth phase. This is due to the dissipation of the
excess pore pressures (= consolidation), which causes further settlement of the soil.
Figure 4.13 shows the remaining excess pore pressure distribution after consolidation.
Check that the maximum value is below 1.0 kN/m2
.
The Curves manager can be used to view the development, with time, of the excess pore
pressure under the embankment. In order to create such a curve, follow these steps:

TUTORIAL MANUAL
Figure 4.12 Viewpoint window
Figure 4.13 Excess pore pressure contours after consolidation to Pexcess < 1.0 kN/m2
Click the Curves manager button in the toolbar. The corresponding window pops up.
• In the Charts tabsheet click New. The Curve generation window pops up
• For the x-axis, select the Project option from the drop-down menu and select Time
in the tree.
• For the y-axis select the point in the middle of the soft soil layers (the second node
(0.7 0.0 -3)) from the drop-down menu. In the tree select Stresses → Pore pressure
→ pexcess.
• Select the Invert sign option for y-axis.
• Click the Ok to generate the curve.
Click the Settings button in the toolbar. The Settings window will appear displaying
the tabsheet of the created curve.
• Click the Phases button and select the phases 1 to 4 in the appearing window.
• Rename the curve by typing 'Phases 1 - 4' in the Curve title cell.
• Click Apply to update the plot.
Save the chart in Output and save the project in Input.
Hint: To display the legend inside the chart area right-click on the name of the
chart, point to the View option and select the Legend in chart option in the
appearing menu.
Figure 4.14 clearly shows the four calculation phases. During the construction phases
the excess pore pressure increases with a small increase in time while during the

Figure 4.14 Development of excess pore pressure under the embankment
consolidation periods the excess pore pressure decreases with time. In fact,
consolidation already occurs during construction of the embankment, as this involves a
small time interval.
4.5 SAFETY ANALYSIS
In the design of an embankment it is important to consider not only the final stability, but
also the stability during the construction. It is clear from the output results that a failure
mechanism starts to develop after the second construction phase.
It is interesting to evaluate a global safety factor at this stage of the problem, and also for
other stages of construction.
In structural engineering, the safety factor is usually defined as the ratio of the collapse
load to the working load. For soil structures, however, this definition is not always useful.
For embankments, for example, most of the loading is caused by soil weight and an
increase in soil weight would not necessarily lead to collapse. Indeed, a slope of purely
frictional soil will not fail in a test in which the self weight of the soil is increased (like in a
centrifuge test). A more appropriate definition of the factor of safety is therefore:
Safety factor =
Smaximum available
Sneeded for equilibrium
(4.1)
Where S represents the shear strength. The ratio of the true strength to the computed
minimum strength required for equilibrium is the safety factor that is conventionally used
in soil mechanics. By introducing the standard Coulomb condition, the safety factor is
obtained:
Safety factor =
c − σn tan ϕ
cr − σn tan ϕr
(4.2)
Where c and ϕ are the input strength parameters and σn is the actual normal stress
component. The parameters cr and ϕr are reduced strength parameters that are just
large enough to maintain equilibrium. The principle described above is the basis of a
Safety analysis that can be used in PLAXIS to calculate a global safety factor. In this
approach the cohesion and the tangent of the friction angle are reduced in the same
proportion:

TUTORIAL MANUAL
c
cr
=
tan ϕ
tan ϕr
= ΣMsf (4.3)
The reduction of strength parameters is controlled by the total multiplier ΣMsf. This
parameter is increased in a step-by-step procedure until failure occurs. The safety factor
is then defined as the value of ΣMsf at failure, provided that at failure a more or less
constant value is obtained for a number of successive load steps.
The Safety calculation option is available in the Calculation type drop-down menu in the
Phases window.
To calculate the global safety factor for the road embankment at different stages of
construction, follow these steps:
• In the Phases window and select Phase 1 in the Start from phase drop-down menu.
Add a new calculation phase.
In the General subtree, select Safety as calculation type.
The Loading type is automatically changed to Incremental multipliers.
• The first increment of the multiplier that controls the strength reduction process, Msf,
is set automatically to 0.1. This value will be used in this tutorial.
Note that the Use pressures from the previous phase option in the Pore pressure
calculation type drop-down menu is automatically selected and grayed out indicating
that this option cannot be changed
• In order to exclude existing deformations from the resulting failure mechanism,
select the Reset displacements to zero option in the Deformation control parameters
subtree. The default values of all the remaining parameters will be used. The first
safety calculation has now been defined.
• Follow the same steps to create new calculation phases that analyse the stability at
the end of each consolidation phase. In addition to selecting Safety as calculation
type, select the corresponding consolidation phase as the Start from phase
parameter. The Phases explorer displaying the Safety calculation phases is shown
in Figure 4.15.
Calculate the safety phases.
Hint: The default value of Max steps in a Safety calculation is 100. In contrast to
an Staged construction calculation, the specified number of steps is always
fully executed. In most Safety calculations, 100 steps are sufficient to arrive
at a state of failure. If not, the number of steps can be increased to a
maximum of 10000.
» For most Safety analyses Msf = 0.1 is an adequate first step to start up the
process. During the calculation process, the development of the total
multiplier for the strength reduction, ΣMsf, is automatically controlled by the
load advancement procedure.

Figure 4.15 Phases explorer displaying the Safety calculation phases
4.5.1 EVALUATION OF THE RESULTS - SAFETY
Additional displacements are generated during a Safety calculation. The total
displacements do not have a physical meaning, but the incremental displacements in the
ﬁnal step (at failure) give an indication of the likely failure mechanism.
In order to view the mechanisms in the three different stages of the embankment
construction:
Select the last Safety phase (Phase_8) and click the View calculation results button.
• From the Deformations menu select Incremental displacements → |∆u|.
Change the presentation from Arrows to Shadings. The resulting plots give a good
impression of the failure mechanisms (Figure 4.16). The magnitude of the
displacement increments is not relevant.
Figure 4.16 Shadings of the total displacement increments indicating the most applicable failure
mechanism of the embankment in the ﬁnal stage
The safety factor can be obtained from the Calculation info option of the Project menu.
The value of ΣMsf represents the safety factor, provided that this value is indeed more or
less constant during the previous few steps.
The best way to evaluate the safety factor, however, is to plot a curve in which the

TUTORIAL MANUAL
parameter ΣMsf is plotted against the displacements of a certain node. Although the
displacements are not relevant, they indicate whether or not a failure mechanism has
developed.
In order to evaluate the safety factors for the three situations in this way, follow these
steps:
• Click the Curves manager button in the toolbar.
• Click New in the Charts tabsheet.
• In the Curve generation window, select the embankment toe (the first node) for the
x-axis. Select Deformations → Total displacements → |u|.
• For the y-axis, select Project and then select Multiplier → ΣMsf. The Safety
phases are considered in the chart. As a result, the curve of Figure 4.17 appears.
• Set x-axis interval maximum to 1 in Chart tab.
The maximum displacements plotted are not relevant. It can be seen that for all curves a
more or less constant value of ΣMsf is obtained. Hovering the mouse cursor over a point
on the curves, a box showing the exact value of ΣMsf can be obtained.
Figure 4.17 Evaluation of safety factor
4.6 USING DRAINS
In this section the effect of the drains in the project will be investigated. The embankment
constructions will be redefined by introducing four new phases having the same
properties as the first four consolidation phases. The differences in the new phases are:
• The drains should be active in all the new phases.
• The Time interval in the first three of the consolidation phases (1 to 3) is 1 day. The
last phase is set to Minimum excess pore pressure and a value of 1.0 kN/m2
is
assigned to the minimum excess pressure (|P-stop|).
After the calculation is finished, select the last phase and click the View calculation
results button. The Output window now shows the deformed mesh after the drained
construction of the final part of the embankment. In order to compare the effect of the
drains, the excess pore pressure dissipation in node (0.7 0 -3) can be used.

Open the Curves manager.
• In the Chart tabsheet double click Chart 1 (pexcess of node (0.7 0 -3) versus time).
Select the displaying phases to Phases 1-4. Close the Curves manager.
Click the Settings button in the toolbar. The Settings window pops up.
• Click the Add curve button and select the Add from current project option in the
appearing menu. The Curve generation window pops up.
Hint: Instead of adding a new curve, the existing curve can be regenerated using
the corresponding button in the Curves settings window.
• Select the Invert sign option for y-axis.
• Click OK to accept the selected options and close the Curve generation window.
• In the chart a new curve is added and a new tabsheet corresponding to it is opened
in the Settings window.
• Click the Phases button. From the displayed window select the Initial phase and the
last four phases (drains) and click OK.
• In the Settings click Apply to preview the generated curve.
• Click OK to close the Settings window. The chart (Figure 4.18) gives a clear view of
the effect of drains in the time required for the excess pore pressures to dissipate.
Figure 4.18 Effect of drains

TUTORIAL MANUAL
5 STABILITY OF A DIAPHRAGM WALL EXCAVATION
This lesson is concerned with a diaphragm wall that is constructed in a stiff sandy clay
layer with a groundwater level at 1.0 m below the surface. The excavation process of a
diaphragm wall is executed in a specific sequence to obtain the maximum support from
the surrounding soil and to prevent soil collapse. A diaphragm wall consists of a number
of individually constructed sections. The construction of one such section is modelled in
this exercise.
A single diaphragm section is excavated in three parts, and the construction can be
modelled in five phases. In the first three phases, the wall is excavated part by part in the
sequence as shown in Figure 5.1. During the excavation, fluid bentonite with a unit
weight of 11 kN/m3
is simultaneously pumped in the trench so that the bentonite pressure
and the arching in the soil prevents the surrounding soil from collapse. After digging of
the trench has been completed, in the fourth phase, fluid concrete is poured in the trench
replacing the bentonite. In the fifth phase the concrete hardens, and the diaphragm wall
section is complete. The stability of the excavation is lowest in the third phase, when the
section is entirely excavated and filled with bentonite. A safety factor is calculated through
a phi-c reduction procedure after each phase to observe the stability of the excavation.
Objectives:
• Defining user-defined water conditions
• Modelling of diaphragm walls installation
Figure 5.1 Geometry of the diaphragm wall
5.1 GEOMETRY
The diaphragm wall considered in this exercise is 30 m deep and 1.2 m thick. One
section is 7.0 m wide and consists of three excavation parts; part I and II are 2.5 m wide
and part III is 2.0 m wide. The wall is symmetric about its central plane, so only one half

STABILITY OF A DIAPHRAGM WALL EXCAVATION
of the thickness needs to be modelled. The interaction between the wall and the soil is
considered to be fully rough, therefore interfaces are not required.
Project properties
To define the geometry for this exercise, follow these steps:
• Start the Input program and select New project from the Create/Open project dialog
box.
• Enter an appropriate title for the exercise.
• Keep the standard units and set the model dimensions to xmin = 0 m, xmax = 20 m,
ymin = 0 m, ymax = 10 m.
• Click OK.
In the current example only one horizontal soil layer is present. A single borehole is
sufficient to define it.
Create a borehole at (0 0 0). The Modify soil layers pops up.
• In the Modify soil layers window add a soil layer with top boundary at z = 40 m and
bottom boundary at z = 0 m.
• Set the head to 39 m.
Open the Material sets window and create the data sets for the soil layer and the
concrete as specified in Table 5.1.
• Assign the 'Stiff sandy clay' material data set to the soil layer and close the Material
sets window.
Table 5.1 Material properties of the stiff sandy clay layer and the concrete
Parameter Name Stiff sandy clay Concrete Unit
General
Material model Model Mohr-Coulomb Linear elastic −
Drainage type Type Drained Non-porous −
Soil unit weight above p.l. γunsat 15 24 kN/m3
Soil unit weight below p.l. γsat 20 − kN/m3
Parameters
Young's modulus E' 50 · 103
2.6 · 107
kN/m2
Poisson's ratio ν' 0.3 0.2 kN/m2
Cohesion c'ref 15 − kN/m2
Friction angle ϕ' 30 − ◦
Dilatancy angle ψ 0.0 − ◦
Interfaces
Interface strength − Rigid Rigid −
Initial
K0 determination − Automatic Automatic −
5.1.2 DEFINITION OF THE DIAPHRAGM WALL
The diaphragm wall is modelled in the Structures mode. The volume elements
composing the diaphragm wall are generated by extruding rectangular surfaces.

TUTORIAL MANUAL
Click the Create surface button in the side toolbar and create three surfaces
accordingly to Table 5.2.
Select the created surfaces by keeping the Ctrl key pressed while clicking them in
the model.
Click the Extrude object button in the side toolbar. Set the extrusion vector to (0 0
-30) and the extrusion vector length to 30 (Figure 5.2).
• Delete the surfaces.
Table 5.2 Surfaces composing the diaphragm wall
Segment Points coordinates
I (6.5 0 40) (9 0 40) (9 0.6 40) (6.5 0.6 40)
II (11 0 40) (13.5 0 40) (13.5 0.6 40) (11 0.6 40)
III (9 0 40) (11 0 40) (11 0.6 40) (9 0.6 40)
Figure 5.2 Extrude surfaces
5.2 MESH GENERATION
In order to generate the mesh:
• Multi-select all the volume elements of the diaphragm wall.
• In the Selection explorer set the value of Coarseness factor to 0.50.
Click the Generate mesh button. The default option (Medium) is used to generate

the mesh.
Click the View mesh button to inspect the generated mesh (Figure 5.3).
The calculation consists of five phases. In the first phase, part I of the excavation is
removed and simultaneously filled with bentonite. The bentonite, with a unit weight of 11
kN/m3
, is simulated employing an artificial ’water’ pressure that increases linearly with
depth. This pressure replaces the original water pressure inside the excavation. In the
second and third phases of the excavation parts, II and III are removed and filled with
bentonite. In the fourth phase, the entire excavated trench is filled with fluid concrete. The
fluid concrete with a unit weight of 24 kN/m3
is simulated by a change in the artificial
’water’ pressure. In phase 5, the hardening of the concrete is simulated by removing the
artificial pressures, reactivating the excavated clusters and assigning the concrete
material set to these clusters.

TUTORIAL MANUAL
Initial phase
The initial phase consists of the generation of the initial stresses using the K0 procedure.
The default settings for the initial phase are valid.
Phase 1 - Excavation of part I
Add the first calculation phase.
• Select the first excavation volume (part I).
• In the selection explorer, deactivate the soil volume. Set the water condition to
User-defined and enter zref = 40 m, pref = 0.0 kN/m2
and pinc = -11 kN/m2
/m (Figure
5.4).
Figure 5.4 User-defined water condition in part I
A bentonite pressure is now defined in part I of the excavation, starting at 0 kN/m2
at
the reference level of 40 m and increasing at 11 kN/m2
per m depth, resulting in 330
kN/m2
at the bottom of the excavation.
Click the Preview phase button to check the settings for the current phase.
Phase 2 - Excavation of part II
Add a new phase.
• Select the second excavation volume (part II).
/m.
Phase 3 - Excavation of part III
Add a new phase.
• Select the third excavation volume (part III).

/m.
Phase 4 - Fluid concrete
The bentonite in the excavation is now replaced by fluid concrete with a weight of 24.0
kN/m3
.
Add a new phase.
• Select the three excavation volumes.
• In the selection explorer, change the User-defined water conditions and enter pinc =
-24 kN/m2
/m. The other parameters must be kept at their original values (zref = 40
m, pref = 0.0 kN/m2
).
Phase 5 - Cured concrete
Add a new phase.
• Select the three excavation volumes.
• In the selection explorer, reactivate the soil volumes and set the material to concrete.
• Set the water condition to Dry.
Hint: Although the concrete is non-porous and the calculation program will
automatically assume zero pore pressures in these elements, it is a good
practise to regenerate the water pressures such that the generated pore
pressures correspond to those used in the calculation program.
Phase 6 to 9 - Safety analysis
In Phases 6 to 9, stability calculations are defined for the previous phases respectively
except for the fluid concrete phase (less critical than the bentonite phase thanks to the
higher unit weight). Phase 3 should be the most critical because the support pressure
from the bentonite is low. Also, the excavation is at its full width, which reduces the
possibility for lateral arching. A check on whether Phase 3 is the most critical stage can
be carried out by calculating the safety factors for the first three phases through a Safety
analysis.
• Select Phase_1 in the Phases explorer.
Add a new calculation phase and proceed to the Phases window.
Set Calculation type to Safety. The Incremental multipliers option is valid as Loading
type.
• Select the Reset displacements to zero option in the Deformation control subtree.
• In the Numerical control parameters subtree set the Max steps parameter to 40.
• Follow the same procedure to add Safety analysis phases following phases 2, 3 and
5.
In the Staged construction mode select some nodes near (10 1 40) and (10 4.5 40)

TUTORIAL MANUAL
for curves.
The stability of the excavation can be evaluated from the calculated safety factor after
each excavation stage. Use the Curves program to plot ΣMsf (the safety factor) as a
function of the displacements |u| (Figure 5.5). In Phase 3, the stability is the lowest.
However, ΣMsf remains greater than 1 and so collapse would not be expected.
In order to evaluate the safety factors for the three situations in this way, follow these
steps:
• Click the Curves manager button in the toolbar.
• Click New in the Charts tabsheet.
• In the Curve generation window, select one of the two nodes for the x-axis. Select
Deformations → Total displacements → |u|.
• For the y-axis, select Project and then select Multiplier → ΣMsf. The Safety
phases are considered in the chart. As a result, the curve of Figure 5.5 appears.
• Set x-axis interval maximum to 0.1 in Chart tab.
Figure 5.5 ΣMsf (safety factor) as a function of the total displacement
An important phenomenon that keeps the excavation stable is arching in the soil. This
phenomenon is shown in Figure 5.6, Figure 5.7 and Figure 5.8. To see the principal
stresses directions at a chosen depth, make a horizontal cross section by clicking the
Horizontal cross section button.
To create such plots, make a horizontal cross-section by clicking the Horizontal

cross section button in the side bar.
• In the window that appears ﬁll in a cross section height of 25 m (at the mid-height of
the diaphragm wall).
• Select Total principal stresses from Principal total stresses of the Stresses menu.
Select the top view in Viewpoint from the View menu to reorientate the model in
order to obtain a clearer view of the arch effect.
Figure 5.6 Principal stresses directions at z = 25 m at the end of Phase_1

TUTORIAL MANUAL
6 PHASED EXCAVATION OF A SHIELD TUNNEL
The lining of a shield tunnel is often constructed using prefabricated concrete ring
segments, which are bolted together within the tunnel boring machine to form the tunnel
lining. During the erection of the tunnel lining the tunnel boring machine (TBM) remains
stationary. Once a tunnel lining ring has been fully erected, excavation is resumed, until
enough soil has been excavated to erect the next lining ring. As a result, the construction
process can be divided into construction stages with a length of a tunnel ring, often about
1.5 m long. In each of these stages, the same steps are repeated over and over again.
In order to model this, a geometry consisting of slices each 1.5 m long can be used. The
calculation consists of a number of Plastic phases, each of which models the same parts
of the excavation process: the support pressure at the tunnel face needed to prevent
active failure at the face, the conical shape of the TBM shield, the excavation of the soil
and pore water within the TBM, the installation of the tunnel lining and the grouting of the
gap between the soil and the newly installed lining. In each phase the input for the
calculation phase is identical, except for its location, which will be shifted by 1.5 m each
phase.
contraction of shield
final lining grout
pressure
TBM
cref = 0.5%
cinc, axial = -0.0667%
cref = 0.0%
cinc, axial = -0.0667%
Figure 6.1 Construction stages of a shield tunnel model
Objectives:
• Modelling of the tunnel boring process with a TBM
• Modelling of the cone shape of the TBM
• Using Tunnel designer to define geometry, trajectory and sequencing of the tunnel
6.1 GEOMETRY
In the model, only one symmetric half is included. The model is 20 m wide, it extends 80
m in the y-direction and it is 20 m deep. These dimensions are sufficient to allow for any
possible collapse mechanism to develop and to avoid any influence from the model
boundaries.
When starting PLAXIS 3D set the proper model dimensions in the Project properties
window, that is xmin = -20, xmax = 0, ymin = 0 and ymax = 80.

PHASED EXCAVATION OF A SHIELD TUNNEL
The subsoil consists of three layers. The soft upper sand layer is 2 m deep and extends
from the ground surface to Mean Sea Level (MSL). Below the upper sand layer, there is a
clay layer of 12 m thickness and this layer is underlain by a stiff sand layer that extends to
a large depth. Only 6 m of the stiff sand layer is included in the model. Hence, the bottom
of the model is 18 m below MSL. Soil layer is assumed to be horizontal throughout the
model and so just one borehole is sufficient to describe the soil layers. The present
groundwater head corresponds to the MSL.
Press the Create borehole button and click at the origin of the system of axis to
create a borehole at (0 0 0). The Modify soil layers window will open.
• Define 3 layers: Upper sand with the top at 2 m and the bottom at 0 m, Clay with the
bottom at -12 m and Stiff sand with the bottom at -18 m.
Open the materials database by clicking the Materials button and create the data
sets for the soil layers and the final concrete lining in the tunnel as specified in Table
6.1.
Parameter Name Upper sand Clay Stiff sand Concrete Unit
General
Material model Model Mohr-Coulomb Mohr-Coulomb Mohr-Coulomb Linear elastic −
Drainage type Type Drained Drained Drained Non porous −
Unit weight above
phreatic level
γunsat 17.0 16.0 17.0 27.0 kN/m3
Unit weight below
phreatic level
γsat 20.0 18.0 20.0 − kN/m3
Parameters
Young's modulus E' 1.3 · 104
1.0 · 104
7.5 · 104
3.1 · 107
kN/m2
Poisson's ratio ν' 0.3 0.35 0.3 0.1 −
Cohesion c'ref 1.0 5.0 1.0 − kN/m2
Friction angle ϕ' 31 25 31 − ◦
Dilatancy angle ψ 0 0 0 − ◦
Interfaces
Interface strength − Rigid Rigid Rigid Rigid −
Initial
K0 determination − Automatic Automatic Automatic Automatic −
• Assign the material data sets to the corresponding soil layers (Figure 6.2) and close
the Modify soil layers window. The concrete data set will be assigned later.
The tunnel excavation is carried out by a tunnel boring machine (TBM) which is 9.0 m
long and 8.5 m in diameter. The TBM already advanced 25 m into the soil. Subsequent
phases will model an advancement by 1.5 m each.
Create tunnel
In Structures mode both the geometry of the tunnel and the TBM will be defined.
Click the Start designer ... button in the side toolbar.
Click the Create tunnel button from the list.

TUTORIAL MANUAL
Figure 6.2 Soil layer distribution
• Click anywhere on the drawing area to define the insertion point. The Tunnel
designer window pops up.
• In the Selection explorer set the insertion point of the tunnel to (0 0 -13.25) (Figure
6.3).
Figure 6.3 Insertion point of the tunnel
• In the General tabsheet select the Circular option in the drop-down menu for the
Shape type.
• The left half of the tunnel is generated in this example. Select the Define left half
option in the drop-down menu for the Whole or half tunnel. A screenshot of the
General tabsheet after the proper assignment is given in Figure 6.4.
• Click the Segments tabsheet to proceed to the corresponding tabsheet. A segment
is automatically created. A new box is shown under the segment list where the
properties of the segment can be defined.
• In the Segment box set Radius to 4 m. This is the inner radius of the tunnel.
• Proceed to the Subsections tabsheet.
Click the Generate thick lining button in the side toolbar. The Generate thick lining
window pops up.
• Assign a value of 0.25 m and click OK. A screenshot of the Cross section tabsheet

Figure 6.4 General tabsheet of the Tunnel designer
after the proper assignment is given in Figure 6.5.
Figure 6.5 The Cross section tabsheet of the Tunnel designer
• Proceed to the Properties tabsheet. Here we deﬁne the properties for the tunnel
such as grout pressure, surface contraction, jack forces and the tunnel face
pressure.
• In the Slice tabsheet, right-click the outer surface and select Create plate from the
appearing menu (Figure 6.6).
Click on the Material in the lower part of the explorer. Create a new material dataset.
Specify the material parameters for the TBM according to Table 6.2.

TUTORIAL MANUAL
Hint: In the tunnel, as considered here, the segments do not have a specific
meaning as the tunnel lining is homogeneous and the tunnel will be
constructed at once. In general, the meaning of segments becomes
significant when:
• It is desired to excavate or construct the tunnel (lining) in different
stages.
• Different tunnel segments have different lining properties.
• One would consider hinge connections in the lining (hinges can be
added after the design of the tunnel in Staged construction mode,
Section 7.9.4 of the Reference Manual).
• The tunnel shape is composed of arcs with different radii (e.g. NATM
tunnels).
Figure 6.6 The Properties tabsheet of the Tunnel designer for the creation of a Plate
Table 6.2 Material properties of the plate representing the TBM
Parameter Name TBM Unit
Type of behaviour - Elastic; Isotropic -
Thickness d 0.17 m
Material weight γ 247 kN/m3
Young’s modulus E1 200·106
kN/m2
Poisson’s ratio ν12 0 -
Shear modulus G12 100·106
kN/m2
Hint: A tunnel lining consists of curved plates (shells). The lining properties can be
specified in the material database for plates. Similarly, a tunnel interface is
nothing more than a curved interface.
A soil-structure interaction has to be added on the outside of the tunnel due to the slight
cone shape of the TBM. Typically, the cross-sectional area at the tail of the TBM is about

0.5% smaller than the front of the TBM. The reduction of the diameter is realised over the
first 7.5 m length of the TBM while the last 1.5 m to the tail has a constant diameter. This
means that the section tail has a uniform contraction of 0.5% and the remaining 5
sections have a linear contraction with a reference value Cref = 0.5% and an increment
Cinc,axial = -0.0667%. The reference is set on the front surface of the excavated slice in
the tunnel during the tunnel construction. This is done while setting the Sequencing
steps. The Cinc,axial = -0.0667%/m and remains the same in every step (1_1 to 1_5). For
further information on Surface contraction refer to Section 5.5.4 of the Reference Manual.
• Right-click the same outer surface and select Create negative interface from the
appearing menu to create a negative surface around the entire tunnel.
• Next step is to create Surface contraction for the tunnel. Right-click the outer
surface and select Create surface contraction.
• In the properties box, select the Axial increment option for the contraction
distribution and define Cref = 0.5% and Cinc,axial = -0.0667%/m. The increment must
be a negative number because the contraction decreases in the direction of the
positive local 1-axis.
Hint: A surface contraction of the tunnel contour of 0.5% corresponds
approximately to a volume loss of 0.5% of the tunnel volume (applicable only
for small values of surface contractions).
» The entered value of contraction is not always fully applied, depending on the
stiffness of the surrounding clusters and objects.
Grout pressure
The surface load representing the grout pressure is constant during the building process.
In the specifications of the tunnel boring process, it is given that the grout pressure
should be -100 kN/m2
at the top of the tunnel (z = -4.75m) and should increase with -20
kN/m2
/m depth. To define the grout pressure:
• Right-click the outer surface and select Create surface load from the appearing
menu to create a surface load around the entire tunnel.
• In the properties box, select Perpendicular, vertical increment from the drop-down
menu for Distribution.
• Set the σn,ref to -100 and σn,inc to -20 and define (0 0 -4.75) as the reference point
for the load by assigning the values to xref , yref and zref (Figure 6.7).
Tunnel face pressures
The tunnel face pressure is a bentonite pressure (Bentonite Slurry, BS) or an earth
pressure (Earth Pressure Balance, EPB) that increases linearly with depth. For the initial
position of the TBM and the successive four positions when simulating the advancement
of the TBM, a tunnel face pressure has to be defined.
• Select the Plane tabsheet above the displayed tunnel cross section.
• Multi-click both the surfaces, right-click and select Create surface load from the

TUTORIAL MANUAL
Figure 6.7 Slice tabsheet in the Tunnel designer
appearing menu to create a surface load around the entire tunnel.
• In the properties box, select Perpendicular, vertical increment from the drop-down
menu for Distribution.
• Set the σn,ref to -90 and σn,inc to -14 and deﬁne (0 0 -4.75) as the reference point for
the load by assigning the values to xref , yref and zref (Figure 6.8).
Figure 6.8 Plane tabsheet in the Tunnel designer
Jack forces
In order to move forward during the boring process, the TBM has to push itself against
the existing tunnel lining. This is done by hydraulic jacks. The force applied by the jacks
on the ﬁnal tunnel lining has to be taken into account. This will be assigned to the tunnel

lining in Sequencing tab.
Trajectory
The next step is to create the path of the boring process. The TBM already advanced
25m into the soil and then proceeds from 25m to 41.5m excavating slices of 1.5m each:
• Click the Trajectory tab to proceed to the corresponding tabsheet.
In the Segments tabsheet, click on the Add segment on the left toolbar.
• In the properties box set the length to 25.
• Add the next segment and set the length to 16.5.
• To create the slices, proceed to the Slices tabsheet.
• Click on the second created segment. In the properties box, select Length as the
Slicing method and set the Slice length as 1.5m (Figure 6.9).
Figure 6.9 Trajectory tabsheet in the Tunnel designer
Sequencing
In order to simplify the definition of the phases in Staged construction mode, the
sequencing of the tunnel is defined. The soil in front of the TBM will be excavated, a
support pressure will be applied to the tunnel face, the TBM shield will be activated and
the conicity of the shield will be modelled, at the back of the TBM the pressure due to the
back fill grouting will be modelled as well as the force the hydraulic jacks driving the TBM
exert on the already installed lining, and a new lining ring will be installed.
• Click the Sequencing tab to proceed to the corresponding tabsheet.
• In the Sequencing tabsheet, set the Excavation method as TBM.
NOTE: For the steps Step_1_1 to Step_1_5 keep in mind that the contraction
increment Cinc,axial has to be -0.0667%.

TUTORIAL MANUAL
Step_1_1, face excavation: Select the Slice tabsheet above the displayed tunnel
cross section and select the volumes inside the tunnel. In the Selection explorer,
deactivate the soil and set the WaterConditions to Dry.
In the Slice tabsheet as well, select the outer surface. In the Selection explorer,
activate the negative interface, the plate and the surface contraction (Figure 6.10).
Set Cref = 0% for the surface contraction (since this is on the front of the excavation).
Figure 6.10 Slice tabsheet in the Tunnel designer for Step_1_1
Go to the Plane Front tabsheet and select all the surfaces. Activate the surface load
corresponding to the face pressure (Figure 6.11).
Step_1_2, TBM with conicity: click on the Add Step to add a new step. The
difference with the front of the TBM is only the face pressure.
Go to the Plane Front tabsheet and select all the surfaces. In the Selection explorer,
the surface load corresponding to the face pressure is deactivated by default.
Go to the Slice tabsheet, select the outer surface and set Cref = 0.1%, see Figure
6.12.
From Step_1_3 to Step_1_5, TBM with conicity: click on the Add Step button
three times to add three new steps. These steps are necessary to deﬁne the
remaining cone part of the TBM shield (Figure 6.13).
For each step go to the Slice tabsheet, select the outer surface and set the following
values for the surface contraction in the Selection explorer:
Step 1_3: Cref = 0.2%
Step 1_4: Cref = 0.3%
Step 1_5: Cref = 0.4%, see Figure 6.13

Figure 6.11 Plane Front tabsheet in the Tunnel designer for Step_1_1
Step_1_6, tail of the shield: The last slice of the shield has a constant diameter.
From the Slice tabsheet select the outer surface and select the surface contraction.
In the Selection explorer select the Uniform option with Cref = 0.5% (Figure 6.14).
Step_1_7, grouting and jack thrusting: Select the Slice tabsheet and select the
outer surface. Deactivate the negative interface, the plate and the surface
contraction. In the Selection explorer, activate the surface load corresponding to the
grout pressure (Figure 6.15).
Select the Plane rear tabsheet and select the outer surface to define the jack
thrusting against the final lining. In the Selection explorer, activate the surface load
and select the Perpendicular option for the distribution with σn,ref = 635.4 (Figure
6.16).
Step_1_8, final lining: Select the Slice tabsheet and select the outer surface. In
the Selection explorer, deactivate the grout pressure and activate the negative
interface. In the Slice tabsheet again, select the outer volume. Activate it, click the
material and select the Concrete option from the drop-down menu (Figure 6.17).
Select the Plane rear tabsheet and select the outer surface. In the Selection
explorer, deactivate the surface load corresponding to the thrusting jacks (Figure
6.18).
• Click on Generate to include the defined tunnel in the model.
• Close the Tunnel designer window.
This concludes the model creation in Structures mode (Figure 6.19).

TUTORIAL MANUAL
Figure 6.13 Slice tabsheet in the Tunnel designer from Step_1_3 to Step_1_5

Figure 6.15 Slice tabsheet in the Tunnel designer Step_1_7

TUTORIAL MANUAL
Figure 6.16 Plane Rear tabsheet in the Tunnel designer Step_1_7
Figure 6.17 Slice tabsheet in the Tunnel designer Step_1_8

Figure 6.18 Plane rear tabsheet in the Tunnel designer Step_1_8
Figure 6.19 The created tunnels in Structures mode

TUTORIAL MANUAL
6.2 MESH GENERATION
In the Mesh mode it is possible to specify global and local refinements and generate the
mesh. The default local refinements are valid for this example.
Click the Generate mesh button in order to generate the mesh. The Mesh options
window appears.
• The default option (Medium) will be used to generate the mesh.
Click the View mesh button to inspect the generated mesh (Figure 6.20).
After inspecting the mesh, the output window can be closed. Mesh generation has now
been finished, and so creating all necessary input for defining the calculation phases has
been finished.
The excavation of the soil and the construction of the tunnel lining will be modelled in the
Staged construction mode. Since water levels will remain constant the Flow conditions
mode can be skipped. It should be noted that due to the mesh generation the tunnel
effectively has been split into an upper part, located in the clay, and a lower part located
in the stiff sand. As a result, both the lower and the upper part of the tunnel should be
considered.
The first phase differs from the following phases, as in this phase the tunnel is activated
for the first time. This phase will model a tunnel that has already advanced 25 m into the
soil. Subsequent phases will model an advancement by 1.5 m each.
Initial phase
The initial phase consists of the generation of the initial stresses using the K0 procedure.
The default settings for the initial phase are valid.

Phase 1 - Initial position of the TBM
In the first phase, it is assumed that the TBM has already advanced 25 m. The section
next to the first 25 m (section 25 m - 26.5 m), will represent the area directly behind the
TBM were grout is injected in the tail void. In the next 6 sections (26.5 m - 35.5 m) the
TBM will be modelled.
Add the first calculation phase.
• In the Model explorer expand Tunnels and then expand Tunnel_1. Scroll down the
Model explorer until the option Advancement step and set it to 7 in order to simulate
the advancement of the first 25 m.
The final lining will be activated in the following phase. In order to consider the conicity of
the TBM in the first 25 m, the clusters representing final lining need to be deactivated, the
plates representing the TBM are activated and 0.5% contraction is applied.
Select the right view to reorientate the model in order to obtain a clearer view of the
inside of the tunnel.
• In the drawing area select the soil volumes corresponding to the lining in the first 25
m (Figure 6.21).
Figure 6.21 Selection of soil volumes (0 m - 25 m)
• In the Selection explorer deactivate the soil. The soil is switched off, but the
wireframe representing the deactivated soil is still coloured red as the deactivated
soil is still selected.
Hint: An object that is deactivated will automatically be hidden as a volume or
surface, but a wireframe representing the hidden object will remain. The
visibility of the object not active in a calculation phase can be defined in the
corresponding tabsheet of the Visualization settings window (Section 3.6.3 of
the Reference Manual).
The interface is already activated. To activate the plate and the contraction in the first 25
m of the tunnel:
Select the Select plates option in the appearing menu. Select the surfaces between
0 m and 25 m in the model to which plates are assigned (Figure 6.22).
• In the Selection explorer activate plate and uniform contraction by checking the
corresponding boxes.
• In the drawing area select the lateral surfaces of the outer volume, corresponding to

TUTORIAL MANUAL
Figure 6.22 Selection of plate (0 m - 25 m)
the last slice of the TBM (grout and jack thrusting) at 25.0 m (Figure 6.23). In the
Selection explorer, deactivate the surface load corresponding to the jack thrusting,
because the TBM is only placed in this phase and it’s not moving.
Click the Preview button to get a preview of everything that has been deﬁned
(Figure 6.24). Make sure that both grout pressure and tunnel face pressure are
applied and that both increase from top to bottom.
Figure 6.23 Selection of soil surfaces (25.0 m)
Phase 2 - TBM advancement 1
In this phase, the advancement of the TBM by 1.5 m (from y = 35.5 to y = 37) will be
modelled.
Add a new phase.
• In the Model explorer expand Tunnels and then expand Tunnel_1. Scroll down the
Model explorer until the option Advancement step and set it to 8 in order to simulate
the advancement of the ﬁrst 26.5 m.
In this phase, the TBM advances from y = 37 to y = 38.5.
Add a new phase.
• In the Model explorer expand Tunnels and right-click Tunnel_1. Then click on
Advance to next tunnel step.

Figure 6.24 Preview of the Phase 1
In this phase, the TBM advances from y = 38.5 to y = 40.
Add a new phase.
In this phase, the ﬁnal advancement of the TBM is modelled (from y = 40 to y = 41.5).
Add a new phase.
Press the Calculate button to start the calculation. Ignore the message "No nodes or
stress points selected for curves" as any load-displacement curves are drawn in this
example, and start the calculation.

TUTORIAL MANUAL
Figure 6.25 The Advance to next tunnel step option from Model explorer
Once the calculation has been completed, the results can be evaluated in the Output
program. In the Output program the displacement and stresses are shown in the full 3D
model, but the computational results are also available in tabular form. To view the
results for the current analysis, follow these steps:
• Select the last calculation phase (Phase 5) in the Phases explorer.
Click the View calculation results button in the side toolbar to open the Output
program. The Output program will by default show the 3D deformed mesh at the
end of the selected calculation phase.
• From the Deformations menu, select Total displacements and then uz in order to
see the total vertical displacements in the model as a shaded plot (Figure 6.26).
In order to see the settlements at ground level make a horizontal cross section by
choosing the Horizontal cross section button. In the window that appears ﬁll in a cross
section height of 1.95 m. The window with the cross section opens (Figure 6.27). The
maximum settlement at ground level is about 1.9 cm.

Figure 6.26 Total vertical displacements after the ﬁnal phase uz ≈ 3.1cm
Figure 6.27 Settlement trough at ground level |u| ≈ 1.9cm

TUTORIAL MANUAL
7 RAPID DRAWDOWN ANALYSIS
This example concerns the stability of a reservoir dam under conditions of drawdown.
Fast reduction of the reservoir level may lead to instability of the dam due to high pore
water pressures that remain inside the dam. The dam to be considered is 30 m high. The
top width and the base width of the dam are 5 m and 172.5 m respectively. The dam
consists of a clay core with a well graded fill at both sides. The geometry of the dam is
depicted in Figure 7.1. The normal water level behind the dam is 25 m high. A situation is
considered where the water level drops 20 m. The normal phreatic level at the right hand
side of the dam is 10 m below ground surface. The sub-soil consists of overconsolidated
silty sand.
x
y
50 m 77.5 m
5 m
5 m
25 m
20 m 120 m120 m
37.5 m
30 m
30 m
90 m
Core
FillFill
Subsoil
Figure 7.1 Geometry of the dam
Objectives:
• Performing fully coupled flow deformation analysis
• Defining time-dependent hydraulic conditions
• Using unsaturated flow parameters
7.1 GEOMETRY
• Start the Input program and select the Start a new project from the Quick select
dialog box.
• In the Project properties window enter a proper title.
• Keep the default units and set the model dimensions to xmin = −130, xmax = 130,
ymin = 0 and ymax = 50.
Assuming the dam is located in a wide valley, a representative length of 50 m is
considered in the model in order to decrease the model size. The geometry of the model
is shown in Figure 7.2.
In order to define the underlying foundation soil, a borehole needs to be added and
material properties must be assigned. A layer of 30 m overconsolidated silty sand is
considered as sub-soil in the model.
Create a borehole at (0.0 0.0). The Modify soil layers window pops up.

RAPID DRAWDOWN ANALYSIS
• Add a soil layer extending from ground surface (z = 0) to a depth of 30 m (z= -30).
• Set the Head in the borehole to -10 m. A horizontal water level will be automatically
generated. This water level in combination with surface groundwater flow boundary
conditions will be used in the Fully coupled flow deformation analyses.
• Create data sets under Soil and interfaces set type according to the information
given in Table 7.1. Note that the Interfaces and Initial tabsheets are not relevant (no
interfaces or K0 procedure used).
• Assign the Subsoil material data set to the soil layer in the borehole.
Table 7.1 Material properties of the dam and sub-soil
Parameter Name Core Fill Subsoil Unit
General
Material model Model Mohr
Coulomb
Mohr
Coulomb
Mohr
Coulomb
-
Drainage type Type Undrained B Drained Drained -
Soil unit weight above p.l. γunsat 16.0 16.0 17.0 kN/m3
Soil unit weight below p.l. γsat 18.0 20.0 21.0 kN/m3
Parameters
Young's modulus E' 1.5·103
2.0·104
5.0·104
kN/m2
Poisson's ratio ν' 0.35 0.33 0.3 -
Cohesion c'ref - 5.0 1.0 kN/m2
Undrained shear strength su,ref 5.0 - - kN/m2
Friction angle ϕ' - 31 35.0 ◦
Dilatancy angle ψ - 1.0 5.0 ◦
Young's modulus inc. E'inc 300 - - kN/m2
Reference level zref 30 - - m
Undrained shear strength inc. su,inc 3.0 - - kN/m2
Reference level zref 30 - - m
Groundwater
Data set Model Hypres Hypres Hypres -
Model - Van
Genuchten
Van
Genuchten
Van
Genuchten
-
Soil - Subsoil Subsoil Subsoil -
Soil coarseness - Very fine Coarse Coarse -
kx 1.0·10-4
0.25 0.01 m/day
ky 1.0·10-4
0.25 0.01 m/day
Vertical permeability kz 1.0·10-4
0.25 0.01 m/day
7.1.2 DEFINITION OF THE EMBANKMENT
The embankment will be defined in the Structures mode.
Define a surface by specifying points located at (-80 0 0), (92.5 0 0), (2.5 0 30) and
(-2.5 0 30).
Define a surface by specifying points located at (-10 0 0), (10 0 0), (2.5 0 30) and
(-2.5 0 30).
• Multi-select the created surfaces and right-click on the drawing area. Select the
Intersect and recluster option from the appearing menu.
• Multi-select the surfaces and extrude along (0 50.0 0) The volumes representing the
dam are generated.

TUTORIAL MANUAL
• Delete the surfaces used to create the soil volumes.
• Assign the corresponding material data sets to the soil volumes.
Time dependent conditions can be assigned to surface groundwater flow boundary
conditions. Define surface groundwater flow boundary conditions (under the Create
hydraulic conditions tool) according to the information in Table 7.2.
Figure 7.2 The geometry of the model
Table 7.2 Surface groundwater flow boundary conditions
Surface Points
1 (-130 0 0), (-80 0 0), (-80 50 0), (-130 50 0)
2 (-80 0 0), (-2.5 0 30), (-2.5 50 30), (-80 50 0)
3 (-130 0 0), (-130 0 -30), (-130 50 -30), (-130 50 0)
7.2 MESH GENERATION
For the generation of the mesh it is advisable to set the Element distribution parameter to
Fine. To modify the global coarseness:
Click the Generate mesh button in the side toolbar. The Mesh options window is
displayed.
• Select the Fine option form the Element distribution drop-down (Figure 7.3).
Figure 7.3 Modification of the Global coarseness
• Click OK to close the Mesh options window and to generate the mesh.
Click the View mesh button in the side toolbar to preview the mesh. The resulting
mesh is displayed in Figure 7.4.

Figure 7.4 The resulting mesh
In the calculation process the initial state (high reservoir), the rapid drawdown case, the
slow drawdown case and finally the low water level case will be considered. A safety
analysis will be performed for each of the cases.
• Proceed to the Flow conditions mode.
Create water levels corresponding to the full reservoir and the low water level cases
according to the information given in Table 7.3.
• In the Attributes library of the Model explorer rename the created user water levels
as 'High_Reservoir' and 'Low_Reservoir'.
Table 7.3 Water levels
Level Points
High reservoir (-130 0 25), (-10 0 25), (93 0 -10), (130 0 -10), (130 50 -10), (93 50 -10), (-10 50 25), (-130 50 25)
Low reservoir (-130 0 5), (-10 0 5), (93 0 -10), (130 0 -10), (130 50 -10), (93 50 -10), (-10 50 5), (-130 50 5)
Hint: No modifications, such as Time dependency is possible for Borehole water
levels and non-horizontal User water levels.
Initial phase - High reservoir
• Double-click the initial phase in the Phases explorer.
• In the General subtree of the Phases window rename the phase as 'High reservoir'.
Select the Gravity loading option as Calculation type. Note that Staged construction
is the only option available for Loading type.
Select the Steady state groundwater flow option as pore pressure calculation type.
• Note that the options Ignore undr. behaviour (A,B) and Ignore suction are by default
selected in the Deformation control parameters subtree. The default values will be
used for the parameters in the Numerical control parameters and Flow control
parameters subtrees.

TUTORIAL MANUAL
• In the Staged construction mode activate the soil clusters representing the
embankment.
• In the GroundwaterFlow subtree set BoundaryYMin, BoundaryYMax and
BoundaryZMin to Closed. The remaining boundaries should be Open (Figure 7.5).
• In the Water subtree select the high reservoir water level (High_Reservoir) as
GlobalWaterLevel.
Figure 7.5 Boundary conditions for groundwater flow
Phase 1 - Rapid drawdown
In the rapid drawdown phase the water level in the reservoir will be lowered from z = 25 m
to z = 5 m in a period of 5 days. To define the function describing the fluctuation of the
water level:
Add a new calculation phase
• In the Phases explorer double-click the newly added phase. The Phases window is
displayed.
• In the General subtree specify the name of the phase (e.g. Rapid drawdown).
Set the Calculation type to Fully coupled flow-deformation.
• Set the Time interval to 5 days.
• The Reset displacements to zero option is automatically selected in the Deformation
control parameters subtree.

• Expand the Attributes library in the Model explorer.
• Right-click on Flow functions and select the Edit option in the appearing menu. The
Flow functions window is displayed.
In the Head functions tabsheet add a new function by clicking the corresponding
button. The new function is highlighted in the list and options to define the function
are displayed.
• Specify a proper name to the function for the rapid drawdown (e.g. Rapid).
• Select the Linear option from the Signal drop-down menu.
• Assign a value of -20 m to ∆ Head, representing the amount of the head decrease.
• Specify a time interval of 5 days. A graph is displayed showing the defined function
(Figure 7.6).
• Click OK to close the Flow functions window.
Figure 7.6 The flow function for the rapid drawdown case
• Activate all the surface groundwater flow boundary conditions.
• Multi-select the surface groundwater flow BCs in the drawing area.
• In the Selection explorer select the Head option as behaviour. The distribution of
the head is Uniform. Assign a value of 25 m to href .
• Set the time dependency to Time dependent and select the Rapid option as Head
function. Information related to the head function is displayed in the Object explorers
as well.
• In the Water subtree in the Model explorer select the BoreholeWaterLevel_1 option
as GlobalWaterLevel.

TUTORIAL MANUAL
Phase 2 - Slow drawdown
In the slow drawdown phase the water level in the reservoir will be lowered from z = 25 m
to z = 5 m in a period of 50 days. To define the function describing the fluctuation of the
water level:
• Select the initial phase (High reservoir) in the Phases explorer.
Add a new calculation phase
displayed.
• In the General subtree specify the name of the phase (e.g. Slow drawdown).
Set the Calculation type to Fully coupled flow-deformation.
• Set the Time interval option to 50 days.
• The Reset displacements to zero option is automatically selected in the Deformation
control parameters subtree.
• Create a new flow function following the steps previously described.
• Specify a proper name to the function for the slow drawdown (e.g. Slow).
• Select the Linear option from the Signal drop-down menu.
• Assign a value of -20 m to ∆ Head, representing the amount of the head decrease.
• Specify a time interval of 50 days. The window displaying the defined function is
shown in Figure 7.7.
Figure 7.7 The flow function for the slow drawdown case

• Activate all the surface groundwater flow boundary conditions and multi-select them
in the drawing area.
• In the Selection explorer select the Head option as behaviour. The distribution of
the head is Uniform. Assign a value of 25 m to href .
• Set the time dependency to Time dependent and select the Slow option as Head
function.
• In the Water subtree in the Model explorer select the BoreholeWaterLevel_1 option
as GlobalWaterLevel.
Phase 3 - Low level
This phase considers the steady-state situation of a low reservoir level.
• Select the initial phase (High reservoir) in the Phases explorer.
Add a new calculation phase.
displayed.
• In the General subtree specify the name of the phase (ex: Low level).
The default calculation type (Plastic) is valid for this phase.
The default Pore pressure calculation type (Steady state groundwater flow) is valid
for this phase.
• In the Deformation control subtree, select Ignore und. behaviour (A,B) and make
sure that the Reset displacements to zero is selected as well.
• The surface groundwater flow BCs should be deactivated in the Model explorer.
• In the Water subtree select the low reservoir water level (Low_Reservoir) as
GlobalWaterLevel.
Phase 4 to 7 - Safety analysis
In Phases 4 to 7, stability calculations are defined for the previous phases respectively.
• Select Phase_1 in the Phases explorer.
Add a new calculation phase and proceed to the Phases window.
• In the General subtree specify the name of the phase (ex: Rapid drawdown -
Safety).
Set Calculation type to Safety. The Incremental multipliers option is valid as Loading
type.
• Select the Reset displacements to zero option in the Deformation control subtree.
• In the Numerical control parameters subtree set the Max steps parameter to 50 for
Phase 4.
• Follow the same procedure for Phases 5 to 7. The final view of the Phases explorer
is given in Figure 7.8.

TUTORIAL MANUAL
Figure 7.8 The final view of the Phases explorer
In the Staged construction mode select a node located at the crest (-2.5 25.0 30.0 ).
Start the calculation process. Ignore the calculation warnings.
After the calculation is finished click the View the calculation results
button. The Output window now shows the deformed mesh for the selected phase.
• In the Stresses menu point the Pore pressures option and select the pwater option
Define a vertical cross section passing through (-130 15) and (130 15)
The results of the four groundwater flow calculations in terms of pore pressure distribution
are shown in Figures 7.9 to 7.12. Four different situations were considered:
Hint: Note that by default the legend is locked in cross section plots, meaning that
the same layer distribution will be used if the cross section is relocated in the
model or if the results are displayed for other phases.
The legend can be unlocked by clicking on the Lock icon under the legend. A
'free' legend is indicated by the Open lock icon.
• The situation with a high (standard) reservoir level (Figure 7.9).
• The situation after rapid drawdown of the reservoir level (Figure 7.10).
• The situation after slow drawdown of the reservoir level (Figure 7.11).
• The situation with a low reservoir level (Figure 7.12).
When the change of pore pressure is taken into account in a deformation analysis, some
additional deformation of the dam will occur. These deformations and the effective stress
distribution can be viewed on the basis of the results of phases 1 to 4.
For the phases 1 and 2 change the legend settings to Manual and set the values as
follows:

• Minimum value: -480
In this tutorial attention is focused on the variation of the safety factor of the dam for the
different situations. Therefore, the development of ΣMsf is plotted for the phases 4 to 7
as a function of the displacement of the dam crest point (see Figure 7.13).
Figure 7.9 Pore water pressure distribution for high reservoir level (Initial phase)
Figure 7.10 Pore water pressure distribution after rapid drawdown (Phase_1)

TUTORIAL MANUAL
Figure 7.11 Pore water pressure distribution after slower drawdown (Phase_2)
Figure 7.12 Pore water pressure distribution for low reservoir level (Phase_3)
Rapid drawdown of a reservoir level can reduce the stability of a dam signiﬁcantly. Fully
coupled ﬂow-deformation and stability analysis can be performed with PLAXIS 3D to
effectively analyse such situations.

Figure 7.13 Safety factors for different situations

TUTORIAL MANUAL
8 DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION
In this tutorial the influence of a vibrating source on its surrounding soil is studied. To
reduce the calculation time, only one-quarter of the overall geometry is modelled, using
symmetry boundary conditions along the lines of symmetry. The physical damping due to
the viscous effects is taken into consideration via Rayleigh damping. Also, due to radial
wave propagation, 'geometric damping' can be significant in attenuating the vibration.
The modelling of the boundaries is one of the key points in the dynamic calculation. In
order to avoid spurious wave reflections at the model boundaries (which do not exist in
reality), special conditions have to be applied in order to absorb waves reaching the
boundaries.
Objectives:
• Performing a Dynamic calculation
• Defining dynamic boundary conditions (viscous)
• Defining dynamic loads by means of load multipliers
• Defining material damping by means of Rayleigh damping
8.1 GEOMETRY
The vibrating source is a generator founded on a 0.2 m thick concrete footing of 1 m in
diameter, see Figure 8.1. Oscillations caused by the generator are transmitted through
the footing into the subsoil. These oscillations are simulated as a uniform harmonic
loading, with a frequency of 10 Hz and amplitude of 10 kN/m2
. In addition to the weight of
the footing, the weight of the generator is modelled as a uniformly distributed load of 8
kN/m2
.
0.5 m
20 m
20 mGenerator
sandy clay
x
z
z = 0
z = -10
10 m
Figure 8.1 Generator founded on elastic subsoil
The model boundaries should be sufficiently far from the region of interest, to avoid
disturbances due to possible reflections. Although special measures (absorbent
boundaries) are adopted in order to avoid spurious reflections, there is always a small
influence and it is still a good habit to put boundaries far away. In a dynamic analysis,
model boundaries are generally taken further away than in a static analysis.

DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION
8.1.1 GEOMETRY MODEL
• Start the Input program and select the Start a new project from the Quick select
dialog box.
• In the Project properties window enter a proper title.
• Keep the default units and set the model dimensions to xmin = 0, xmax = 20, ymin = 0
and ymax = 20. The geometry model is shown in Figure 8.2.
Figure 8.2 Geometry of the model
The subsoil consists of one layer with a depth of 10 m. The ground level is defined at z =
0. Create the material data set according to Table 8.1 and assign it to the soil layer. Note
that water conditions are not considered in this example and the hydraulic head is set at z
= -10.
Parameter Name Sandy clay Unit
General
Material model Model Linear elastic −
Drainage type Type Drained −
Unit weight above phreatic level γunsat 20.0 kN/m3
Unit weight below phreatic level γsat 20.0 kN/m3
Parameters
Young's modulus E' 5 · 104
kN/m2
Poisson's ratio ν' 0.3 −
Interfaces
Interface strength − Rigid −
Initial
K0 determination − Automatic −
Lateral earth pressure coefficient K0 0.5 −
The generator is defined in the Structures mode. The Polycurve feature is used to define
the geometry.

TUTORIAL MANUAL
Click the Create polycurve button in the side toolbar and click on (0 0 0) in the
drawing area.
• In the General tabsheet the default option for shape (Free) and the default
orientation axes (x-axis, y-axis) are valid for this polycurve.
• In the Segments tabsheet three segments are defined as given in Table 8.2. The
insertion point is located at (0 0 0).
Table 8.2 Segments composing the polycurve
Segment Segment 1 Segment 2 Segment 3
Segment type Line Arc Line
Segment properties
Relative start angle = 90◦
Relative start angle = 0◦
Radius = 0.5 m Relative start angle = 90◦
Length = 0.5 m Segment angle = 90◦
Length = 0.5 m
• Right-click the polycurve and select the Create surface option from the appearing
menu.
• Right-click the created surface and select the Create surface load option in the
appearing menu.
• In the Selection explorer, the Uniform distribution is valid for the surface load.
Assign (0 0 -8) to the pressure components.
Definition of dynamic multipliers
Dynamic loads are defined on the basis of input values of loads or prescribed
displacements and corresponding time-dependent multipliers.
To create the multipliers of the dynamic load:
• In the Model explorer expand the Attributes library subtree.
• Right-click the Dynamic multipliers subtree and select the Edit option from the
appearing menu. The Multipliers window pops up.
• Click the Load multipliers tab.
Click Add button to introduce a multiplier for the loads.
• Define a Harmonic signal with an Amplitude of 10, a Frequency of 10 Hz and a
Phase of 0◦
as shown in Figure 8.3.
In the Selection explorer, under DynSurfaceLoad_1 specify the components of the
load as (0 0 -1).
• Click Multiplierz in the dynamic load subtree and select the LoadMultiplier_1 option
Hint: The dynamic multipliers can be defined in the Geometry modes as well as in
the Calculation modes.

Figure 8.3 Deﬁnition of a Harmonic multiplier
8.2 MESH GENERATION
• Reﬁne the surface corresponding to the generator by assigning a Coarseness factor
of 0.125.
Click the Generate mesh button. The Medium option will be used for Element
distribution.
View the generated mesh.
Figure 8.4 Geometry and mesh

TUTORIAL MANUAL
Hint: In all dynamic calculations, the user should pay special attention to the
element size to decrease numerical dispersion of waves. It should be noted
that large elements are not able to transmit high frequencies. The
transmission of waves is governed by both wave speed and wave length. If
dynamic input contains high frequencies, either high frequencies should be
filtered out or a finer mesh should be used.
The calculation consists of 4 phases. The initial phase consists of the generation of the
initial stresses using the K0 procedure. The second phase is a Plastic calculation where
the static load is activated. The third phase is a Dynamic calculation where the effect of
the functioning generator is considered. The fourth and final phase is a Dynamic
calculation as well where the generator is turned off and the soil will vibrate freely.
Initial phase
phases.
• The initial phase has already been introduced. The default settings of the initial
phase will be used in this tutorial.
Phase 1
Add a new phase (Phase_1). The default settings of the added phase will be used
for this calculation phase.
• In the Staged construction mode activate the static component of the surface load.
Do not activate the dynamic load (Figure 8.5).
Figure 8.5 Applied load in the Phase_1

Phase 2
Add a new phase (Phase_2).
In the General subtree in the Phases window, select the Dynamic option as
calculation type.
• Set the Time interval parameter to 0.5 s.
• In the Deformation control parameters subtree in the Phases window select the
Reset displacement to zero parameter. The default values of the remaining
parameters will be used for this calculation phase.
parameters checkbox, which allows you to change advanced settings and set the
Time step determination to Manual.
• Set the Max steps to 250.
• In the Staged construction mode activate the dynamic component of the surface
load. Note that the static component of the load is still active (Figure 8.6).
Figure 8.6 Applied load in the Phase_2
Special boundary conditions have to be defined to account for the fact that in reality the
soil is a semi-infinite medium. Without these special boundary conditions the waves
would be reflected on the model boundaries, causing perturbations. To avoid these
spurious reflections, viscous boundaries are specified at Xmax, Ymax and Zmin. The
dynamic boundaries can be specified in the Dynamics subtree located under the Model
conditions in the Model explorer (Figure 8.7).
Phase 3
In the General subtree in the Phases window, select the Dynamic option as
calculation type.

TUTORIAL MANUAL
Figure 8.7 Boundary conditions for Dynamic calculations
• Set the Dynamic time interval parameter to 0.5 s.
• Set the Max steps to 250.
• In the Staged construction mode deactivate the dynamic component of the surface
load. Note that the static load is still active. The dynamic boundary conditions of this
phase should be the same as in the previous phase. Figure 8.8 shows the Phases
explorer of this tutorial.
Select nodes located at the ground surface (ex: (1.4 0 0), (1.9 0 0), (3.6 0 0)) to
consider in curves.
Execute the calculation.
Save the project.
8.3.1 ADDITIONAL CALCULATION WITH DAMPING
In a second calculation, material damping is introduced by means of Rayleigh damping.
Rayleigh damping can be entered in the material data set. The following steps are
necessary:
• Save the project under another name.
• Open the material data set of the soil.

• In the General tabsheet click the box next to the Rayleigh α parameter. Note that the
display of the General tabsheet has changed displaying the Single DOF equivalence
box.
• Set the value of the ξ parameter to 5% for both targets.
• Set the frequency values to 9 and 11 for the Target 1 and Target 2 respectively.
• Click on one of the definition cells of the Rayleigh parameters. The values of α and
β are automatically calculated by the program.
• Click OK to close the data base.
• Check whether the phases are properly defined (according to the information given
before) and start the calculation.
Figure 8.9 Input of Rayleigh damping
The Curve generator feature is particularly useful for dynamic analysis. You can easily
display the actual loading versus time (input) and also displacements, velocities and
accelerations of the pre-selected points versus time. The evolution of the defined
multipliers with time can be plotted by assigning Dynamic time to x-axis and uz to the
y-axis. Figure 8.10 shows the response of the pre-selected points at the surface of the
structure. Even with no damping, the waves are dissipated thanks to the geometric
damping.
Figure 8.11 shows the response of the pre-selected points at the surface of the structure
with material damping. The vibration is seized when some time is elapsed after the
removal of the dynamic component of the surface load (at t = 0.5 s). Comparing Figure
8.10 (without damping) with Figure 8.11 (with damping), also the displacement

TUTORIAL MANUAL
Figure 8.10 Vertical displ.- time on the surface at different distances to the vibrating source (without
damping)
amplitudes are lower.
Figure 8.11 Vertical displ.- time (with damping)
It is possible in the Output program to display displacements, velocities and accelerations
at a particular time, by choosing the appropriate option in the Deformations menu. Figure
8.12 shows the total accelerations in the soil at the end of phase 2 (t = 0.5 s).

Figure 8.12 Total accelerations in the soil at the end of phase 2 (with damping)

TUTORIAL MANUAL
9 FREE VIBRATION AND EARTHQUAKE ANALYSIS OF A BUILDING
This example demonstrates the natural frequency of a long five-storey building when
subjected to free vibration and earthquake loading. The two calculations employ different
dynamic boundary conditions:
• In the free vibration, the Viscous boundary conditions are considered. This option is
suitable for problems where the dynamic source is inside the mesh.
• For the earthquake loading, the Free-field and Compliant base boundary conditions
are considered. This option is preferred for earthquake analysis, where the dynamic
input is applied along the model boundary.
The building consists of 5 floors and a basement. It is 10 m wide and 17 m high including
the basement. The total height from the ground level is 5 x 3 m = 15 m and the basement
is 2 m deep. A value of 5 kN/m2
is taken as the weight of the floors and the walls. The
building is constructed on a clay layer of 15 m depth underlayed by a deep sand layer. In
the model, 25 m of the sand layer will be considered.
Objectives:
• Performing a Dynamic calculation
• Defining dynamic boundary conditions (free-field and compliant base)
• Defining earthquakes by means of displacement multipliers
• Modelling of free vibration of structures
• Modelling of hysteretic behaviour by means of HS small model
• Calculating the natural frequency by means of Fourier spectrum
9.1 GEOMETRY
The length of the building is much larger than its width and the earthquake is supposed to
have a dominant effect across the width of the building. Taking these facts into
consideration, a representative section of 3 m will be considered in the model in order to
decrease the model size. The geometry of the model is shown in Figure 9.1.
9.1.1 GEOMETRY MODEL
• Start the Input program and select Start a new project from the Quick select dialog
box.
• In the Project tabsheet of the Project properties window, enter an appropriate title.
• Keep the default units and set the model dimensions to Xmin = −80, Xmax = 80, Ymin
= 0 and Ymax = 3.
The subsoil consists of two layers. The Upper clayey layer lies between the ground level
(z = 0) and z = -15. The underlying Lower sandy layer lies to z = -40. Define the phreatic
level by assigning a value of -15 to the Head in the borehole. Create the material data set

FREE VIBRATION AND EARTHQUAKE ANALYSIS OF A BUILDING
15 m
15 m
25 m
3 m
Figure 9.1 Geometry of the model
according to Table 9.1 and assign it to the corresponding soil layers. The upper layer
consists of mostly clayey soil and the lower one consists of sandy soil.
Table 9.1 Material properties of the subsoil layers
Parameter Name Upper clayey layer Lower sandy layer Unit
General
Material model Model HS small HS small -
Drainage type Type Drained Drained -
Soil unit weight above phreatic level γunsat 16 20 kN/m3
Soil unit weight above phreatic level γsat 20 20 kN/m3
Parameters
Secant stiffness in standard drained triaxial test Eref
50 2.0·104
3.0·104
kN/m2
Tangent stiffness for primary oedometer loading Eref
oed 2.561·104
3.601·104
kN/m2
Unloading / reloading stiffness Eref
ur 9.484·104
1.108·105
kN/m2
Power for stress-level dependency of stiffness m 0.5 0.5 -
Cohesion c'ref 10 5 kN/m2
Friction angle ϕ' 18.0 28.0 ◦
Dilatancy angle ψ 0.0 0.0 ◦
Shear strain at which Gs = 0.722G0 γ0.7 1.2·10-4
1.5·10-4
-
Shear modulus at very small strains Gref
0 2.7·105
1.0·105
kN/m2
Poisson's ratio ν'ur 0.2 0.2 -
When subjected to cyclic shear loading, the HS small model will show typical hysteretic
behaviour. Starting from the small-strain shear stiffness, Gref
0 , the actual stiffness will
decrease with increasing shear. Figures 9.2 and 9.3 display the Modulus reduction
curves, i.e. the decay of the shear modulus with strain.

TUTORIAL MANUAL
0
100000
50000
150000
200000
250000
Shearmodulus
Shear strain
0.00001 0.0001 0.001 0.01
Gt Gs
γ0.7
0.722G0
G used
Figure 9.2 Modulus reduction curves for the upper clayey layer
20000
40000
60000
80000
100000
Shearmodulus
Shear strain
0.00001 0.0001 0.001 0.01
Gt
Gs
γ0.7
0.722G0
G used
Figure 9.3 Modulus reduction curve for the lower sandy layer
In the HS small model, the tangent shear modulus is bounded by a lower limit, Gur .
Gur =
Eur
2(1 + νur )
The values of Gref
ur for the Upper clayey layer and Lower sandy layer and the ratio to Gref
0
are shown in Table 9.2. This ratio determines the maximum damping ratio that can be
obtained.
Table 9.2 Gur values and ratio to Gref
0
Parameter Unit Upper clayey
layer
Lower sandy
layer
Gur kN/m2
39517 41167
Gref
0 /Gur - 6.83 2.43
Figures 9.4 and 9.5 show the damping ratio as a function of the shear strain for the
material used in the model. For a more detailed description and elaboration from the

modulus reduction curve to the damping curve can be found in the literature∗
.
0
0.2
0.15
0.1
0.05
Dampingratio
Cyclic shear strain
0.00001 0.0001 0.001 0.01
Figure 9.4 Damping curve for the upper clayey layer
0
0.2
0.15
0.1
0.05
Dampingratio
Cyclic shear strain
0.00001 0.0001 0.001 0.01
Figure 9.5 Damping curve for the lower sandy layer
The structural elements of the model are defined in the Structures mode.
Building
The building consists of 5 floors and a basement. It is 10 m wide and 17 m high including
the basement. The total height from the ground level is 5 x 3 m = 15 m and the basement
is 2 m deep. A value of 5 kN/m2
is taken as the weight of the floors and the walls. To
define the structure:
Define a surface passing through the points (-5 0 -2), (5 0 -2), (5 3 -2) and (-5 3 -2).
Create a copy of the surface by defining an 1D array in z-direction. Set the number
of the columns to 2 and the distance between them to 2 m.
Select the created surface at z = 0 and define a 1D array in the z-direction. Set the
number of the columns to 6 and the distance between consecutive columns to 3 m.
Define a surface passing through the points (5 0 -2), (5 3 -2), (5 3 15) and (5 0 15).
∗ Brinkgreve, R.B.J., Kappert, M.H., Bonnier, P.G. (2007). Hysteretic damping in small-strain stiffness model. In
Proc. 10th Int. Conf. on Comp. Methods and Advances in Geomechanics. Rhodes, Greece, 737 − 742

TUTORIAL MANUAL
Create a copy of the vertical surface by defining an 1D array in x-direction. Set the
number of the columns to 2 and the distance between them to -10 m.
• Multiselect the vertical surfaces and the horizontal surface located at z = 0.
• Right-click on the selection and select the Intersect and recluster option from the
appearing menu. It is important to do the intersection in the Structures mode as
different material data sets are to be assigned to the basement and the rest of the
building.
Select all the created surfaces representing the building (basement, floors and
walls), right-click and select the Create plate option from the appearing menu.
• Define the material data set for the plates representing the structure according to
Table 9.3. Note that two different material data sets are used for the basement and
the rest of the building respectively.
• Assign the Basement material data set to the horizontal plate located at z = -2 and
the vertical plates located under the ground level.
• Assign the corresponding material data set to the rest of the plates in the model.
Table 9.3 Material properties of the building (plate properties)
Parameter Name Rest of building Basement Unit
Type of behaviour Type Elastic; Isotropic Elastic; Isotropic -
Thickness d 0.3 0.3 m
Material weight γ 33.33 50 kN/m3
Young’s modulus E1 3·107
3·107
kN/m2
Poisson’s ratio ν12 0 0 -
Rayleigh damping
α 0.2320 0.2320 -
β 8·10-3
8·10-3
-
In order to model the soil-structure intersection at the basement of the building assign
interfaces to the outer side of the basement. Note that depending on the local coordinate
system of the surfaces an interface either positive or negative is assigned.
The central column of the structure is modelled using the Node-to-node anchor feature.
To create the central column of the structure:
Create a Line through points (0 1.5 -2) and (0 1.5 0) corresponding to the column in
the basement floor.
• Create a Line through points (0 1.5 0) and (0 1.5 3) corresponding to the column in
the first floor.
Create a copy of the last defined line by defining an 1D array in z-direction. Set the
number of the columns to 5 and the distance between them to 3 m.
Select the created lines, right-click and select the Create node-to-node anchor
option from the appearing menu.
• Create the material data set according to the Table 9.4 and assign it to the anchors.
Table 9.4 Material properties of the node-to-node anchor
Parameter Name Column Unit
Material type Type Elastic -
Normal stiffness EA 2.5· 106
kN

Loads
A static lateral force of 10 kN/m is applied laterally at the top left corner of the building. To
create the load:
Create a line load passing through (-5 0 15) and (-5 3 15).
• Specify the components of the load as (10 0 0).
The earthquake is modelled by imposing a prescribed displacement at the bottom
boundary. To define the prescribed displacement:
Create a surface prescribed displacement passing through (-80 0 -40), (80 0 -40),
(80 3 -40) and (-80 3 -40).
• Specify the x-component of the prescribed displacement as Prescribed and assign
a value of 1.0. The y and z components of the prescribed displacement are Fixed.
The default distribution (Uniform) is valid.
To define the dynamic multipliers for the prescribed displacement:
• In the Model explorer expand the Attributes library subtree. Right-click on Dynamic
multipliers and select the Edit option from the appearing menu. The Multipliers
window pops up displaying the Displacement multipliers tabsheet.
To add a multiplier click the corresponding button in the Multipliers window.
• From the Signal drop-down menu select the Table option.
• The file containing the earthquake data is available in the PLAXIS Knowledge Base
(tutorial Free vibration and earthquake analysis of a building).
• Open the page in a web browser, copy all the data to a text editor (e.g. Notepad)
and save the file in your computer with the extension ∗
.smc. Alternatively this file
can also be found in the Importables folder in the PLAXIS directory.
In the Multipliers window click the Open button and select the saved file. In the
Import data window select the Strong motion CD-ROM files option from the Parsing
method drop-down menu and press OK to close the window.
• Select the Acceleration option in the Data type drop-down menu.
• Select the Drift correction options and click OK to finalize the definition of the
multiplier.
• In the Dynamic multipliers window the table and the plot of the data is displayed
(Figure 9.6).
• In the Model explorer expand the Surface displacements subtree and assign the
Multiplierx to the x- component by selecting the option in the drop-down menu.
Create interfaces on the boundary
Free-field and Compliant base require the manual creation of interface elements along
the vertical and bottom boundaries of the model in the Structures mode. The interface
elements must be added inside the model, else the Free-field and Compliant base
boundary conditions are ignored. To define the interfaces:
Create a surface passing through (-80 3 0), (-80 0 0), (-80 0 -40) and (-80 3 -40).
Right-click the created surface and and click Create positive interface to add an

TUTORIAL MANUAL
Figure 9.6 Dynamic multipliers window
interface inside the model.
Create a surface passing through (80 3 0), (80 0 0), (80 0 -40) and (80 3 -40).
Right-click the created surface and and click Create negative interface to add an
interface inside the model.
• The surface at the bottom of the model is already created by the prescribed
displacement. Right-click the surface at the bottom of the model and click Create
positive interface to add an interface inside the model.
9.2 MESH GENERATION
• Click the Generate mesh button. Set the element distribution to Fine.
• View the generated mesh (Figure 9.7).

Figure 9.7 Geometry and mesh
The calculation process consists of the initial conditions phase, simulation of the
construction of the building, loading, free vibration analysis and earthquake analysis.
Initial phase
phases.
• The initial phase has already been introduced. The default settings of the initial
phase will be used in this tutorial.
• In the Staged construction mode check that the building and load are inactive.
Phase 1
Add a new phase (Phase_1). The default settings of the added phase will be used
for this calculation phase.
• In the Staged construction mode construct the building (activate all the plates, the
anchors and only the interfaces of the basement) and deactivate the basement
volume (Figure 9.8).
Phase 2
• In the Phases window select the Reset displacement to zero in the Deformation
control parameters subtree. The default values of the remaining parameters will be
used in this calculation phase.
• In the Staged construction mode activate the line load. The value of the load is
already deﬁned in the Structures mode.

TUTORIAL MANUAL
Figure 9.8 Construction of the building
Phase 3
In the Phases window select the Dynamic option as Calculation type.
• Set the Time interval parameter to 5 sec.
• In the Staged construction mode deactivate the line load.
• Expand the Dynamics subtree. By default the boundary conditions in the x and y
directions are set to viscous. Select the None option for the boundaries in the y
direction. Set the boundary Zmin to viscous (Figure 9.9).
Figure 9.9 Boundary conditions for Dynamic calculations (Phase_3)

Hint: For a better visualisation of the results, animations of the free vibration and
earthquake can be created. If animations are to be created, it is advised to
increase the number of the saved steps by assigning a proper value to the
Max steps saved parameter in the Parameters tabsheet of the Phases
window.
Phase 4
• In the Phases window set the Start from phase option to Phase 1 (construction of
building).
Select the Dynamic option as Calculation type.
• Set the Dynamic time interval parameter to 20 sec.
• Select the Reset displacement to zero in the Deformation control parameters
subtree. The default values of the remaining parameters will be used in this
calculation phase.
• Set the Max steps to 1000 and the Max number of sub steps to 4.
• Expand the Dynamics subtree. Set the Free-ﬁeld option for the boundaries in the x
direction. The boundaries in the y direction are already set to None. Set the
boundary Zmin to Compliant base (Figure 9.10).
• Make sure that the interfaces on the boundary of the model are not activated in the
Model explorer.
• In the Model explorer activate the Surface displacement and its dynamic
component. Set the value of ux to 0.5 m. Considering that the boundary condition at
the base of the model will be deﬁned using a Compliant base, the input signal has to
be taken as half of the outcropping motion.
Select points for load displacement curves at (0 1.5 15), (0 1.5 6), (0 1.5 3) and (0
1.5 -2). The calculation may now be started.

TUTORIAL MANUAL
Figure 9.10 Boundary conditions for Dynamic calculations (Phase_4)
Figure 9.11 shows the deformed structure at the end of the Phase 2 (application of
horizontal load). Figure 9.12 shows the time history of displacements of the selected
points A (0 1.5 15), B (0 1.5 6), C (0 1.5 3) and D (0 1.5 -2) for the free vibration phase. It
may be seen from the figure that the vibration slowly decays with time due to damping in
the soil and in the building.
In the Chart tabsheet of the Settings window select the Use frequency representation
(spectrum) and Use standard frequency (Hz) options in the Dynamics box. The plot is
shown in Figure 9.13. From this figure it can be evaluated that the dominant building
frequency is around 1 Hz. For a better visualisation of the results animations of the free
vibration and earthquake can be created.
Figure 9.14 shows the time history of displacements of the point A (0 1.5 15) for the
earthquake phase. It may be seen from the figure that the vibration slowly decays with
time due to damping in the soil and in the building.
The time history signature of the point A (0 1.5 15) of the earthquake phase has been
transformed to normalised power spectra through Fast Fourier transform for Phase 4 and
is plotted in Figure 9.15.

Figure 9.11 Deformed mesh of the system at the end of Phase_2
Figure 9.12 Time history of displacements (Free vibration)

TUTORIAL MANUAL
Figure 9.13 Frequency representation (spectrum - Free vibration)
Figure 9.14 Time history of displacements of the top of the building (Earthquake)

Figure 9.15 Acceleration power spectra at (0 1.5 15)

TUTORIAL MANUAL
APPENDIX A - MENU TREE
A.1 INPUT MENU
INPUTMENU1
FileEditViewSoilStructuresMesh
NewprojectUndoPancameraModifysoillayersShowdynamicmultipliersSelect
OpenprojectRedoRotatecameraSelectSelectSelectmultipleobjects
RecentprojectsCopyscreenimageZoominSelectmultipleobjectsSelectmultipleobjectsReﬁnemesh
SaveprojectDeleteZoomoutMoveobjectMoveobjectCoarsenmesh
SaveprojectasSelectallResetzoomAdjustsoilcontourRotateobjectResetlocalcoarseness
CloseprojectDeselectallDefaultviewsCreateboreholeExtrudeobjectGeneratemesh
ProjectpropertiesExplodeImportsoilCreatearrayViewmesh
PrintImplodeShowmaterialsCreatepointSelectpointsforcurves
ExitCreateline
Createpolycurve
Createsurface
Createload
Createprescribeddisplacement
Createstructure
Createhydraulicconditions
Importstructures
Showmaterials

INPUTMENU2
WaterlevelsPhasesOptionsExpertHelp
SelectEditphasesSnaptogridExaminecommandsManuals
SelectmultipleobjectsShowmaterialsShowgridandrulerRuncommandsCommandreference
MoveobjectShowdynamicmultipliersShowcursorlocationMacrolibraryInstructionmovies
CreatewaterlevelShowflowfunctionsShowlocalaxisConfigureremotescriptingserverRequestsupport
PreviewphaseVisualisatonsettingsViewfilesUpdatelicence
http://www.plaxis.nl
Disclaimer
About

TUTORIAL MANUAL
A.2 OUTPUT MENUOUTPUTMENU(1)
FileViewProjectGeometryMesh
OpenprojectZoomoutNodeﬁxitiesDisabledstructuresQuality
CloseactiveprojectResetviewLoadinformationPhreaticlevelQualitytable
CloseallprojectsViewpointWaterloadinformationLoadsVolume
WorkdirectorySaveviewPrescribeddisplacementinformationFixitiesVolumetable
ExporttoﬁleShowsavedviewsVirtualinterfacethicknessPrescribeddisplacementsConnectivityplot
ReportgenerationScaleVolumeinformationFilterElementcontours
CreateanimationUseresultsmoothingMaterialinformation(allloadcases)Elementdeformationcontours
PrintLegendsettingsMaterialinformation(currentloadcases)Materials
(Listofrecentprojects)ScanlineGeneralprojectinformationElementnumbers
ExitTitleCalculationinformationMaterialsetnumbers
LegendCalculationinfoperstepStructurematerialsetnumbers
AxesStepinfoClusternumbers
ShrinkStructuresperphaseNodes
ExpandStresspoints
ExplodeNodenumbers
ImplodeStresspointnumbers
MovecrosssectionforwardSelectionlabels
Movecrosssectionbackward
Settings

OUTPUTMENU(2)
DeformationsStressesForcesToolsWindowHelp
ElevationCrosssectionAxialforcesCopyProjectmanagerManuals
Deformedmesh|u|CartesianeffectivestressesShearforcesSelectpointsforcurvesDuplicatemodelviewInstructionmovies
TotaldisplacementsCartesiantotalstressesBendingmomentsMeshpointselectionClosewindowhttp://www.plaxis.nl/
PhasedisplacementsPrincipaleffectivestressesTableCurvesmanagerCascadeDisclaimer
IncrementaldisplacementsPrincipaltotalstressesTableofstresspointsTableTileverticallyAbout
VelocitiesStateparametersVerticalcrosssectionTilehorizontally
AccelerationsTotalincrementsHorizontalcrosssection(Listofactiveviews)
TotalcartesianstrainPorepressuresFreecrosssection
Accelerations(in'g')GroundwaterﬂowLinecrosssection
PhasecartesianstrainPlasticpointsHintbox
IncrementalcartesianstrainFixed-endanchorsDistancemeasurement
TotalstrainNodetonodeanchor
PhasestrainWells
IncrementalstrainsDrains

TUTORIAL MANUAL
APPENDIX B - CALCULATION SCHEME FOR INITIAL STRESSES DUE TO SOIL
WEIGHT
Start
Yes NoHorizontal
surface
Initial stresses
Gravity loading
Gravity loading
Ready
K0-Procedure
-Mweight = 1-Mweight = 1
Loading input:
Total multipliers
calculation
Examples of non-horizontal surfaces, and non-horizontal weight stratiﬁcations are:

Plaxis 3d tutorial manual

More Related Content

What's hot (20)

Similar to Plaxis 3d tutorial manual (20)

Recently uploaded (20)

Plaxis 3d tutorial manual