PDF
Deep Excavation
Introduction
There are two ways to model an excavation in COMSOL Multiphysics, both of which include a parametric sweep. One option involves removing the soil one step at a time by means of a sweep of the geometry. As the soil is removed, the support it supplies is removed as well, subjecting the retaining wall to soil stresses from the nonexcavated side. The other option is to start with the already excavated geometry, and simulate the soil removal by modifying a boundary load. The boundary load applies a force on the nonexcavated side of the retaining wall, equal to the in situ stress on the excavation side, for the part of the wall that is above the virtual excavation depth.
This deep excavation example is inspired by a benchmark exercise specified by a working group of the German Society for Geotechnics (Ref. 1 and Ref. 2). In the example, a 26 meter excavation is modeled by means of a parametric sweep. As the excavation deepens, three struts are activated using a ramp function and boolean expressions. As the excavation reaches their depths, the struts are activated as long as the horizontal wall deflection is greater than what it is allowed to be.
Figure 1: Dimensions and boundary conditions for the deep excavation example.
Model Definition
In this example, a Drucker–Prager criterion is used for studying the soil plasticity, and the retaining wall is made of a linear elastic material. The following material parameters are used:
Soil, Upper layer
•
Young’s modulus E = 20 MPa, Poisson’s ratio ν = 0.3, and density ρ = 1900 kg/m3.
•
Cohesion c = 0 Pa, and angle of internal friction ϕ = 35°.
Soil, Lower layer
•
Young’s modulus E = 60 MPa, Poisson’s ratio ν = 0.3, and density ρ = 1900 kg/m3.
•
Cohesion c = 0 Pa, and angle of internal friction ϕ = 35°.
Struts
•
Young’s modulus E = 200 GPa, length l = 30 m and cross sectional area A = 15 cm2.
Retaining Wall
•
Young’s modulus E = 30 GPa, Poisson’s ratio ν = 0.15, and density ρ = 2400 kg/m3.
Constraints and Loads
•
The bottom soil layer is supported by a rigid and perfectly rough base. Therefore, apply a fixed constraint on the lower horizontal boundary.
•
Due to symmetry, model only the right half of the domain. Use the symmetry boundary condition at the left vertical boundary.
•
Add in situ stress with the External Stress feature. Note that the stress caused by gravity is compressive, which in the convention used in the Structural Mechanics Module means negative sign.
•
The in situ stress accounts for the local stress prior excavating. You can define a different value in the vertical and horizontal directions. The horizontal in situ stress, X_stress, is also used on the boundary load applied to the retaining wall.
•
The boundary load on the retaining wall is gradually added in order to simulate the excavation steps. At the bottom of the excavation it ensures zero initial displacement. This strategy avoids remeshing the excavated volume and thus saves memory.
•
Add struts that can be activated and deactivated according to the excavation depth by means of boolean expressions.
•
The struts are active after a maximum horizontal deflection is reached. Use a ramp function to restrict the allowed wall deflection U_max to 25 mm, and to supply the axial force that the struts apply to the wall.
•
The boundaries between the retaining wall and the soil are modeled with the Interior Contact feature. This feature constrains the normal displacement between the retaining wall and the soil to stay in contact, while the tangential displacement is unconstrained.
•
The axial stiffness of the struts is estimated from their cross sectional area A, the length l, and the material Young’s modulus E as
Results and Discussion
In order to improve convergence on the soil-wall boundary, apply a mapped mesh on the retaining wall domain, as shown in Figure 2.
Figure 2: A mapped mesh on the retaining wall domain gives a better convergence.
Figure 3 shows the soil deformation and the wall deflection after excavating 26 meters. Figure 4 shows that the different properties of the two soil layers have an impact on the plastic deformation.
Figure 3: Deformation of the soil and the retaining wall after excavating 26 meters of soil.
Figure 4: Plastic deformation after excavating 26 meters of soil.
The struts — placed 4.8 m, 9.3 m, and 14.35 m below the initial surface (Ref. 1) — help to increase the overall stiffness of the retaining wall. In Figure 5, a maximum allowed displacement of 2.5 cm constrains the horizontal displacement of the retaining wall.
Figure 5: Wall deflection as a function of depth for different excavation steps (color lines).
As the excavation progresses, it is possible to observe the settlement of the unexcavated region. As expected, the settlement increases as the excavation progresses, and decreases with the distance to the retaining wall, see Figure 6.
.
Figure 6: Surface settlement as a function of the distance from the wall. The different color lines show the settlement for different excavation stages (0 to 26 m).
References
1. H.F. Schweiger, Benchmarking in Geotechnics 1. Technical Report CGG IR006 2002, Institute for Soil Mechanics and Foundation Engineering, Graz University of Technology, Austria.
2. D. Potts and L. Zdravkovic, Finite Element Analysis in Geotechnical Engineering, Thomas Telford Publishing, 2001.
Application Library path: Geomechanics_Module/Soil/deep_excavation
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D.
2
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file deep_excavation_parameters.txt.
In situ stresses are set with negative sign to fit the structural mechanics convention. That convention assumes negative stresses in compression and positive in tension.
Ramp: Strut Force
1
In the Home toolbar, click  Functions and choose Global > Ramp.
2
In the Settings window for Ramp, type Ramp: Strut Force in the Label text field.
3
In the Function name text field, type strut_force.
4
Locate the Parameters section. In the Location text field, type U_max.
5
In the Slope text field, type S_struts.
6
In the Baseline text field, type 0[N].
7
Click to expand the Smoothing section.
8
Select the Size of transition zone at start checkbox. In the associated text field, type 0.1[mm].
Geometry 1
Create the geometry.
To simplify this step, you can insert a prepared geometry sequence. In the Geometry toolbar, click Insert Sequence. Browse to the model’s Application Libraries folder and double-click the file deep_excavation.mph. Click Build All in the Geometry toolbar. Then, continue with the instruction after the geometry plot below.
Otherwise, proceed with the following instructions to create the geometry from scratch:
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 90.
4
In the Height text field, type 60.
5
Locate the Position section. In the y text field, type -60.
6
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (m)
Layer 1
20
7
Clear the Layers on bottom checkbox.
8
Select the Layers on top checkbox.
9
Click  Build Selected.
10
Click  Build Selected.
Rectangle 2 (r2)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 30.
4
In the Height text field, type 30.
5
Locate the Position section. In the y text field, type -30.
6
Click  Build Selected.
Rectangle 3 (r3)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 0.8.
4
In the Height text field, type 30.
5
Locate the Position section. In the x text field, type 30.
6
In the y text field, type -30.
7
Click  Build Selected.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object r1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the objects r2 and r3 only.
6
Select the Keep objects to subtract checkbox.
7
Click  Build Selected.
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Object.
4
Click the  Clear Selection button for Selection.
5
Select the object r2 only.
6
Click  Build Selected.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type 30.
6
Locate the Endpoint section. In the x text field, type 30.
7
Locate the Starting Point section. In the y text field, type Stage_1+1.
8
Locate the Endpoint section. In the y text field, type Stage_1.
9
Click  Build Selected.
Line Segment 2 (ls2)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type 30.
6
Locate the Endpoint section. In the x text field, type 30.
7
Locate the Starting Point section. In the y text field, type Stage_2+1.
8
Locate the Endpoint section. In the y text field, type Stage_2.
9
Click  Build Selected.
Line Segment 3 (ls3)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
From the Specify list, choose Coordinates.
4
Locate the Endpoint section. From the Specify list, choose Coordinates.
5
Locate the Starting Point section. In the x text field, type 30.
6
Locate the Endpoint section. In the x text field, type 30.
7
Locate the Starting Point section. In the y text field, type Stage_3+1.
8
Locate the Endpoint section. In the y text field, type Stage_3.
9
Click  Build Selected.
Form Union (fin)
In the Geometry toolbar, click  Build All.
Definitions
Wall Diaphragm
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Wall Diaphragm in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 13 and 14 only.
Soil Domain
1
In the Definitions toolbar, click  Explicit.
2
Select Domains 1 and 3 only.
3
In the Settings window for Explicit, type Soil Domain in the Label text field.
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
Soil Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Soil Plasticity.
2
In the Settings window for Soil Plasticity, locate the Soil Plasticity Model section.
3
From the Match to Mohr–Coulomb list, choose Inscribe (plane strain).
4
Locate the Domain Selection section. From the Selection list, choose Soil Domain.
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
External Stress 1
1
In the Physics toolbar, click  Attributes and choose External Stress.
2
In the Settings window for External Stress, locate the Domain Selection section.
3
From the Selection list, choose Soil Domain.
4
Locate the External Stress section. From the Stress input list, choose In situ stress.
5
From the list, choose Diagonal.
6
Specify the σins matrix as
X_stress
0
0
0
Y_stress
0
0
0
Z_stress
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundary 1 only.
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundary 2 only.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 17 and 18 only.
Interior Contact 1
1
In the Physics toolbar, click  Boundaries and choose Interior Contact.
2
Select Boundaries 5, 13, and 14 only.
Adhesion 1
1
In the Physics toolbar, click  Attributes and choose Adhesion.
2
In the Settings window for Adhesion, locate the Adhesive Activation section.
3
From the Activation criterion list, choose Always active.
4
Locate the Adhesive Stiffness section. In the nτ text field, type 0.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Wall Diaphragm.
4
Locate the Force section. Specify the fA vector as
X_stress*(y>Depth)
x
0
y
Boundary Load: Strut 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, type Boundary Load: Strut 1 in the Label text field.
3
Select Boundary 10 only.
4
Locate the Force section. From the Load type list, choose Total force.
5
Specify the Ftot vector as
strut_force(abs(u))*(Depth<Stage_1)
x
0
y
Boundary Load: Strut 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, type Boundary Load: Strut 2 in the Label text field.
3
Select Boundary 8 only.
4
Locate the Force section. From the Load type list, choose Total force.
5
Specify the Ftot vector as
strut_force(abs(u))*(Depth<Stage_2)
x
0
y
Boundary Load: Strut 3
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, type Boundary Load: Strut 3 in the Label text field.
3
Select Boundary 6 only.
4
Locate the Force section. From the Load type list, choose Total force.
5
Specify the Ftot vector as
strut_force(abs(u))*(Depth<Stage_3)
x
0
y
Materials
Soil, Upper Layer
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Soil, Upper Layer in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Manual.
4
Click  Clear Selection.
5
Select Domain 3 only.
6
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
20[MPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.3
1
Young’s modulus and Poisson’s ratio
Density
rho
1900
kg/m³
Basic
Initial cohesion
cohesion0
0
Pa
Soil material
Friction angle
phis
35[deg]
rad
Soil material
Soil, Lower Layer
1
Right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Soil, Lower Layer in the Label text field.
3
Select Domain 1 only.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
60[MPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.3
1
Young’s modulus and Poisson’s ratio
Density
rho
1900
kg/m³
Basic
Initial cohesion
cohesion0
0
Pa
Soil material
Friction angle
phis
35[deg]
rad
Soil material
Retaining Wall
1
Right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Retaining Wall in the Label text field.
3
Select Domain 2 only.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
30[GPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.15
1
Young’s modulus and Poisson’s ratio
Density
rho
2400
kg/m³
Basic
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  Free Triangular.
2
In the Settings window for Free Triangular, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Soil Domain.
Distribution 1
1
Right-click Free Triangular 1 and choose Distribution.
2
Select Boundary 13 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 20.
Distribution 2
1
In the Model Builder window, right-click Free Triangular 1 and choose Distribution.
2
Select Boundary 14 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 40.
Distribution 3
1
Right-click Free Triangular 1 and choose Distribution.
2
Select Boundary 5 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 3.
Size
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 click Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Finer.
Mapped 1
1
In the Mesh toolbar, click  Mapped.
Use a mapped mesh inside the wall.
2
In the Settings window for Mapped, click  Build All.
The mesh should look like the one in Figure 2.
Study 1
Step 1: Stationary
Set up an auxiliary continuation sweep for the Depth parameter.
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Auxiliary sweep checkbox.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
Depth (Excavation depth (parameter))
range(0,-2,-26)
m
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Parametric 1.
4
In the Settings window for Parametric, click to expand the Continuation section.
Restrict the step size to 0.5 to better capture the development of the plastic zone.
5
Select the Tuning of step size checkbox.
6
In the Initial step size text field, type 0.5.
7
In the Maximum step size text field, type 0.5.
Solution 1 (sol1)
1
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Displacement Field (comp1.u).
2
In the Settings window for Field, locate the Scaling section.
3
In the Scale text field, type 1e-2.
4
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 click Fully Coupled 1.
5
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
6
From the Nonlinear method list, choose Automatic (Newton).
7
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select General > Displacement (m) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Displacement
m
mm
8
Click  Apply.
Displacement
The default plot shows the von Mises stress for the last value of the continuation parameter. Modify and rename this plot group to display the displacement instead.
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 2D Plot Group, type Displacement in the Label text field.
Surface 1
1
In the Model Builder window, expand the Displacement node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Displacement > solid.disp - Displacement magnitude - m.
3
Locate the Coloring and Style section. From the Color table list, choose SpectrumLight.
4
In the Displacement toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Equivalent Plastic Strain (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Plastic Region
In the Settings window for 2D Plot Group, type Plastic Region in the Label text field.
Surface 1
1
In the Model Builder window, expand the Plastic Region node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type solid.epeGp>0.
4
Locate the Coloring and Style section. In the Number of bands text field, type 2.
5
Click to expand the Quality section. From the Resolution list, choose Custom.
6
In the Plastic Region toolbar, click  Plot.
Wall Deflection
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Wall Deflection in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Wall deflection (mm).
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Horizontal displacement (mm).
7
Select the y-axis label checkbox. In the associated text field, type Depth(m).
8
Locate the Legend section. From the Position list, choose Lower left.
Line Graph 1
1
Right-click Wall Deflection and choose Line Graph.
2
In the Settings window for Line Graph, locate the Selection section.
3
From the Selection list, choose Wall Diaphragm.
4
Locate the y-Axis Data section. In the Expression text field, type y.
5
From the Unit list, choose m.
6
Locate the x-Axis Data section. From the Parameter list, choose Expression.
7
In the Expression text field, type u.
8
Click to expand the Legends section. Select the Show legends checkbox.
9
Find the Prefix and suffix subsection. In the Prefix text field, type Depth=.
10
In the Wall Deflection toolbar, click  Plot.
Surface Settlement
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Surface Settlement in the Label text field.
3
Locate the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Surface settlement.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type Distance from the diaphragm (m).
7
Select the y-axis label checkbox. In the associated text field, type Vertical displacement (mm).
8
Locate the Legend section. From the Position list, choose Lower right.
Line Graph 1
1
Right-click Surface Settlement and choose Line Graph.
2
Select Boundary 16 only.
3
In the Settings window for Line Graph, locate the y-Axis Data section.
4
In the Expression text field, type v.
5
Locate the Legends section. Select the Show legends checkbox.
6
Find the Prefix and suffix subsection. In the Prefix text field, type Depth=.
7
In the Surface Settlement toolbar, click  Plot.
Create an extruded plot of displacement.
Extrusion 2D 1
1
In the Results toolbar, click  More Datasets and choose Extrusion 2D.
2
In the Settings window for Extrusion 2D, locate the Extrusion section.
3
In the z maximum text field, type 80.
Displacement 3D
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement 3D in the Label text field.
Surface 1
1
In the Displacement 3D toolbar, click  Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Color table list, choose SpectrumLight.
Deformation 1
In the Displacement 3D toolbar, click  Deformation.
Displacement 3D
Use the mouse to replicate the view of the following image.
1
In the Model Builder window, under Results click Displacement 3D.